IntroductionWelcome| 00:03 | Hi! I am Gabriel Corbett and welcome
to SolidWorks 2012 Essential Training.
| | 00:09 | In this course, we'll look at
the methods and tools for creating
| | 00:13 | manufacturing-ready parts and assemblies along
with detailed drawings and bills of materials.
| | 00:18 | We'll start with the basic sketch
tools to create two-dimensional sketches
| | 00:21 | that will become the foundation for 3D objects.
| | 00:25 | Next, we'll look at modeling 3D features by
extruding or revolving sketches into 3D parts,
| | 00:30 | followed by creating more complex
objects using the Sweep and Loft tools.
| | 00:35 | Then we'll create holes and cuts as well as uniform
standard hole sizes using the automated Hole Wizard.
| | 00:44 | We'll explore the best practice for putting parts
together into assemblies and building robust structures.
| | 00:50 | Finally, we'll see how to create drawings to
relate the final parts and assemblies to a manufacturer
| | 00:54 | complete with an itemized bill
of materials and drawing notes.
| | 00:59 | Now, let's get started with
SolidWorks 2012 Essential Training.
| | Collapse this transcript |
| Using the exercise files| 00:00 | If you're a Premium member of the
lynda.com Online Training Library,
| | 00:04 | or you're watching this tutorial on a DVD-ROM,
| | 00:07 | you have access to the Exercise
Files used throughout the title.
| | 00:11 | After you download the files, I would
recommend saving them to the Desktop here,
| | 00:15 | or to any other location
that might be easily accessible.
| | 00:18 | Double-click on that and you can see we
have all the chapters laid out by chapter
| | 00:22 | and I can go and double-
click on any one of those
| | 00:24 | and you see we got a bunch of
different files in each chapter.
| | 00:27 | They're all labeled by the
Chapter Title plus the Movie Number;
| | 00:30 | so Chapter 14, movie number 1 and
this is made up for this assembly,
| | 00:35 | as well as some different parts
that go up and make that assembly up.
| | 00:37 | We're going to use a -1, -2 type of naming
convention to categorize these types of files.
| | 00:43 | I just want to go back to
Ch 20 (Chapter 20) here.
| | 00:45 | In this chapter, we're actually using
different folders for each chapter and movie,
| | 00:49 | and click in here you can see we've got a bunch of
different files here as well as we have drawings.
| | 00:53 | So SLDDRW is a drawing file.
| | 00:56 | So make sure to pay close
attention to what that extension is.
| | 01:00 | If you're not a premium subscriber to lynda.com,
you don't have access to the Exercise Files,
| | 01:05 | but you can follow along from
scratch with your own assets.
| | 01:08 | So let's get started.
| | Collapse this transcript |
|
|
1. Touring the InterfaceLaunching SolidWorks for the first time| 00:00 | SolidWorks is the world
leader in 3D solid modeling.
| | 00:03 | The software uses a set of
simple building blocks and helpers
| | 00:06 | to assist you in
designing the next great product.
| | 00:09 | Let's go over the opening of the
software and then tour the interface.
| | 00:12 | I'll highlight the main areas of
the interface in the work environment.
| | 00:16 | Let's get started. On the Desktop, I
can see an icon for SolidWorks 2012.
| | 00:21 | We're using the 64-bit version; double-
click that, it opens up the software.
| | 00:25 | It's the first time running it, so we have the
option to activate the product now or we can do it later.
| | 00:29 | So I'll click on the Later tab and Finish.
| | 00:34 | That opens up the environment.
| | 00:35 | On the right-hand side,
we have the Resources tab.
| | 00:38 | We can open new documents, we can
go through some of the Tutorials;
| | 00:42 | the What's New and Introduction to SolidWorks.
| | 00:45 | On the bottom side here, we
can see links to User Groups,
| | 00:49 | some of the technical alerts
and news, what's available,
| | 00:52 | and what's going on in the
world of SolidWorks right now.
| | 00:54 | This is a fly-out tab, so if I
click in the environment, it goes away;
| | 00:58 | if I click back over here, it'll show up.
| | 01:00 | If I'd like to continue to keep this out,
| | 01:02 | I can click on the little
pin which will hold it out.
| | 01:05 | I have tabs here. So the next
tab down is the Design Library.
| | 01:09 | Inside of there, we're going to be
able to store snippets of sketches or
| | 01:14 | parts that are going to be
used later in our design.
| | 01:17 | We have the File Explorer below that and
that's going to be very similar to Windows Explorer,
| | 01:21 | so we can open files on the regular
Desktop or anywhere in the file system.
| | 01:26 | The View palette, we don't really
have any views to open right now,
| | 01:28 | but it's where we would start our drawings from.
| | 01:32 | Following that would be Appearances and Scenes.
| | 01:34 | So if we want to render our part or color the
part in or change the appearances of the material,
| | 01:39 | we can do that and drag these into the
environment, which we'll cover later.
| | 01:44 | The final thing here is the Custom Properties.
| | 01:46 | Inside of there, we're going to have
what would be putting our part number,
| | 01:50 | our revision materials and any documentation
we want to put about our part, it'd go in there.
| | 01:56 | So I'm going to close that little pin.
| | 01:59 | On the upper left-hand corner of the
screen, you notice we have SolidWorks tab
| | 02:02 | and we have this little fly-out window,
if we go over this little icon here.
| | 02:06 | And if we want to keep that
out, I can click on the pin
| | 02:09 | and that will keep that
File > View tab available.
| | 02:11 | To open a new document, we need to
click on either the New icon here
| | 02:15 | or we can go under File and
New or Ctrl+N; click on that.
| | 02:19 | That opens up our New Document window
and we have three available options here
| | 02:24 | which would the Part, Assembly or Drawing.
| | 02:26 | If you don't happen to see this,
you could be on the Advanced tab,
| | 02:28 | which is going to have almost the same thing.
| | 02:30 | Click back on Novice, click on Part, click on
OK and that's going to open up our New window.
| | 02:36 | This is our main drawing environment here.
| | 02:38 | On the left hand side is
going to be our Feature Manager.
| | 02:41 | Feature Manager is going to hold all
the features we create in our part.
| | 02:44 | We start with three fundamental planes;
| | 02:46 | Front Plane, Top Plane, Right Plane and
notice that as I mouse over each one of those,
| | 02:50 | they highlight on the screen.
| | 02:51 | If I'd like to continue to
see that plane, I can click
| | 02:55 | and there is this little icon
that pops up called the Show icon.
| | 02:58 | It looks like a pair of goggles.
Click on that and that continues to show,
| | 03:01 | and notice the icon changes
from black-and-white to color.
| | 03:04 | I can do the same with the
others if I wanted to see those.
| | 03:07 | Turn all three of those on so we can see that.
| | 03:09 | To move the view around, I can always hold down
the middle mouse button and spin that environment.
| | 03:15 | Same thing if I scroll with my
mouse in or out; it'll zoom the view.
| | 03:20 | On the upper portion of the screen,
we have what is called the Ribbon bar
| | 03:24 | and this is similar to many other softwares
out there, and what you'll see is different tabs.
| | 03:29 | So if I click on the corresponding tab,
I get a different ribbon tool palette
| | 03:33 | that will pop up and I have
a variety of like five here,
| | 03:36 | but I can right-click on any one of
them and it will show me the available
| | 03:40 | tool tabs that I can put up here.
So I can quickly add Mold Tools,
| | 03:44 | or same thing, I can take away Sheet
Metal, for instance, to change that around.
| | 03:47 | So the two we're going to be working with most
are going to be the Sketch and Features tabs.
| | 03:53 | Other than that, if we need to
open documents or close documents,
| | 03:56 | we have a quick shortcut
which is on the keyboard.
| | 03:59 | If we hit the R key, it pops up a
little window which is the Recent Documents.
| | 04:03 | So if we wanted to go and open
this part here, for instance,
| | 04:06 | click on that and now I have that part open.
| | 04:09 | We have a couple of documents open now.
| | 04:10 | So if I go up to the Window tab,
I've got a few different choices here
| | 04:14 | as far as how to look at that.
| | 04:15 | One of my favorites is Tile Horizontally
which makes the two documents that are open tile.
| | 04:19 | Now if I had four, it would
put four on the screen and so on.
| | 04:23 | So if I had 20, it would put 20 on
the screen, but they'd become very small,
| | 04:26 | and it's hard to look at; so keep that in mind.
| | 04:28 | Then if you want to open any one of
these documents, just click on the Maximize;
| | 04:31 | it brings us back to full screen.
| | 04:33 | You should now understand where most
of the tools and options are located
| | 04:36 | in the software and how to
navigate the 3D environment.
| | Collapse this transcript |
| Accessing and customizing the Ribbon| 00:00 | The Ribbon bar was introduced to
SolidWorks several versions back.
| | 00:03 | It allows the user to have much
more screen real estate versus
| | 00:07 | having all the required toolbars turned on.
| | 00:09 | It's configurable and dockable.
| | 00:11 | As I covered in the last movie, we can
click on the various tabs below the Ribbon
| | 00:15 | to change what icons are available to us.
| | 00:17 | By default, we have these four here.
| | 00:19 | We can add or remove
different tool tabs to the Ribbon.
| | 00:23 | Click on Weldments, it adds a new tab,
so then if I click on Mold Tools,
| | 00:27 | for instance, it's going to add it there.
| | 00:28 | That Ribbon bar we can move
around the screen if we need to.
| | 00:31 | By clicking anywhere up here, I can drag it out.
| | 00:34 | Notice I drag it out, I could just
place it in the Desktop if I want,
| | 00:36 | I can place it on another window
if I wanted to or I can dock it.
| | 00:40 | So I can dock it back to the
original location at the top.
| | 00:43 | I can come over here and I can dock it to
the right or dock it to the left, your choice.
| | 00:46 | If you do that, it just places it there.
| | 00:50 | You've got the same available tabs.
| | 00:52 | Drag that back out. I prefer to
have it on the top and it docks.
| | 00:57 | We have a lot of other tool tabs that
we can bring out as well, or toolbars.
| | 01:02 | I can right-click here, anywhere in that gray
area and it will bring up these available toolbars.
| | 01:07 | So one that I happen to like and use a lot
is, if you go down here to the Tools tab,
| | 01:12 | it's going to pop out that little toolbar.
| | 01:14 | Now sometimes it will drop it
here in the middle of the screen,
| | 01:16 | sometimes it will dock somewhere.
| | 01:18 | So just kind of look around your screen
to maybe where that originally got dropped.
| | 01:22 | Now I can drag it and dock it over here.
I like to put it on the right hand side.
| | 01:26 | It gives me a little more real estate,
and then I have those tools available
| | 01:30 | and that always stays there.
| | 01:31 | I can also go ahead and add Tools to any one of
these Ribbon bars to customize it to my liking.
| | 01:37 | So if I click on, for instance, the
Sketch tab, if I right-click on it,
| | 01:40 | at the very bottom, I can say
Customize, the CommandManager,
| | 01:44 | and the first screen that comes up is the Toolbar
tab and notice that's exactly what we had before.
| | 01:49 | So if I want to add or remove
toolbars, I can do that here as well.
| | 01:52 | Under the Commands, we have all the commands
that are available in any one of these sketch tabs.
| | 01:59 | So, like for instance, if I go to Sketch,
these are all the sketch tools that are available.
| | 02:04 | Only a subset of those is
available in the actual ribbon.
| | 02:07 | So if I'd like to add something
to that, I can just drag it over.
| | 02:10 | So, one that I like to use a
lot is called Sketch Picture.
| | 02:12 | I'm just going to click on that and drag it.
| | 02:15 | Wherever I drag, it's going to drop a little icon
on the screen for us to use to quickly get to it.
| | 02:20 | You can add as many as you want, and the same
thing is you can click on one of those and remove it.
| | 02:24 | So I don't want it.
| | 02:25 | So I'm going to drop it back there and I can,
same thing, reorganize my icons as needed.
| | 02:31 | Click on that and we're good to go.
| | 02:33 | The Ribbon bar is a very helpful interface for
getting tools quickly and with less clutter on the Desktop.
| | 02:38 | It can be modified with your favorite tools and dock
to one of three locations to suit your layout needs.
| | Collapse this transcript |
| Touring the shortcut bar and identifying essential keys| 00:00 | All the functions and commands to
design in SolidWorks are available
| | 00:04 | in the Ribbon Bar,
various menus, and the toolbars.
| | 00:07 | However there is a group of commands that are used
often that can be assigned to the keys on the keyboard.
| | 00:12 | We should be driving SolidWorks with
two hands, the right hand on the mouse,
| | 00:15 | your left hand on the Escape (Esc) key,
the Shift+Option+Command and Spacebar.
| | 00:19 | Let's go over those.
| | 00:22 | We haven't totally covered the drawing
environment yet, but I am just going to
| | 00:24 | jump into the Line Command and just
throw a couple of lines on the screen.
| | 00:28 | Notice while I'm drawing a line my icon
changes to a little pencil with a line under it.
| | 00:31 | I can drag things around and
then move around in the environment.
| | 00:33 | As I continue to drag out
lines, I stay in that command.
| | 00:36 | If I want to cancel out of that command, hit the
Escape key and I go back to my original pointer.
| | 00:44 | If I click over the Line Command,
notice I have a L showing up in parentheses,
| | 00:48 | that means there is a shortcut for that
command and if I just hit L on the keyboard
| | 00:52 | it jumps into that command.
If I hit L again, it jumps out.
| | 00:55 | So jump in, draw a line,
hit L again, turn it off.
| | 00:58 | It can also add different
commands to the keyboard shortcuts.
| | 01:02 | To do that I can right-click on any one of
these tabs, go down to the Customize Manager again,
| | 01:08 | and I have a tab at the top called
Keyboard, and the one I want to assign is,
| | 01:10 | notice I have just about every
command in SolidWorks available to me.
| | 01:15 | There is quite a few, but the
only one I am looking for is Circle,
| | 01:17 | so I'm just going to search for it here,
which is circle, and my Center Point Circle is
| | 01:22 | the one I'm looking for, and if I just type-in a C,
it's going to give a shortcut to that command.
| | 01:28 | Now if you have something else that is
assigned to that same key it's going to say,
| | 01:32 | hey, do you want to overwrite this?
| | 01:34 | And if you do, that's fine. Click OK.
| | 01:36 | Now if I type C, I jump right in the
Circle Command, draw a circle and it stays
| | 01:41 | in the Circle Command so I
can continue to draw circles.
| | 01:43 | Once I'm done, I can hit C again or the
Escape key to get out of that command.
| | 01:47 | A few other commands here is, if I hit the S
key, that's predefined as the Shortcut Bar,
| | 01:53 | so the same tools I have
available up here, I can actually have
| | 01:57 | have it right there in my screen
wherever my tooltip happens to be.
| | 02:00 | So it's here or here, it just
pops up. It's right next to you.
| | 02:03 | Your tools are available right next to you.
| | 02:04 | Same thing with right-click, anywhere
you are on the screen, I can right-click
| | 02:09 | and get a full listing of
available tools that I can use.
| | 02:13 | Once again this is also customizable.
| | 02:15 | You can do so just at the very
bottom of the screen, Customize Menu.
| | 02:18 | The last thing I'm going to cover
in this movie is the Option and Tab.
| | 02:22 | So if I hold down Option and Tab, I can click to
the different available screens that I have open.
| | 02:28 | So if I need to go back to the
File Manager to grab something,
| | 02:31 | I can jump back into SolidWorks quickly.
| | 02:34 | And we also have the views we can
look at and those are under the Spacebar.
| | 02:40 | If I hit the Spacebar, I get the
Orientation, it pops up, notice I get Front,
| | 02:44 | Back, Side, Isometric, and this
allows me to switch between those views.
| | 02:48 | Before I actually do that, I'm going to
jump into a different window which is available
| | 02:53 | because of the part that I've
already designed, and I can spin around
| | 02:55 | and look at it, but if I want to look at it
for instance in the Front view or the Right view,
| | 02:59 | I can hit the Spacebar and say click
Front. Notice it turns to the Front view.
| | 03:04 | Hit Spacebar to the Back, spins it around. Left.
| | 03:08 | If I click on the Isometric, it gives
it kind of an elevated view from the side
| | 03:13 | and I get a couple of those
Trimetric and Dimetric as well.
| | 03:16 | Just a couple of different views at
different angles and elevations. Okay.
| | 03:21 | And then the last thing here is the R
command which will open up Recent Documents
| | 03:24 | so you can quickly grab any of the
documents that you've been using in the past,
| | 03:28 | I don't know, eight documents yet opened, we'll
just pop up there. You can jump into each one of those.
| | 03:33 | Learning some of these basic keys will dramatically
improve the speed and ease of working with the software.
| | 03:38 | It's the single best way
to do more with less time.
| | Collapse this transcript |
| Saving, renaming, and managing files| 00:00 | Saving your work is essential in all software.
| | 00:02 | However in SolidWorks it's very
important to understand how files interconnect.
| | 00:06 | Let's take a look at this example.
| | 00:08 | This is Assembly 1.4 and
that's made up of 1.4-1, -2 and -3.
| | 00:14 | These three files are
separate files in the file system,
| | 00:16 | which are linked together
in this top-level Assembly.
| | 00:20 | Let's take a look at the File Structure.
| | 00:21 | In the top level here we have a widget.
| | 00:23 | This is a top-level Assembly
in that is made up of two parts,
| | 00:27 | and then another subassembly and a
drawing of that top-level assembly.
| | 00:31 | This subassembly here is made up of two
more parts, another subassembly and a drawing,
| | 00:35 | and then these two drawings down
here represent the drawings for Part3
| | 00:39 | and for Part4, and we have
further structure that goes down here,
| | 00:43 | and this can be as many files as it takes
to make your Assembly. Now look at Part4.
| | 00:48 | If we were to take that part and
change the name without alerting the other
| | 00:52 | members of the file structure that the part
changed, Assembly2 might be looking for Part4.
| | 00:56 | It wouldn't be able to find
it. It can cause a problem.
| | 00:59 | Same thing with Drawing7. Drawing7 is linking up to
that part and looking for that part name or number.
| | 01:05 | So changing that without alerting everybody else
is going to cause a problem for the file structure.
| | 01:09 | The way it works is this.
Files are linked by name.
| | 01:13 | So if you call a part, Part4, it's
always going to be looking for Part4
| | 01:17 | in the associated path or directory.
| | 01:19 | So make sure the path is correct and the
directory you're saving it in is complete.
| | 01:23 | If you, for instance though take a copy of
the entire directory structure in a folder
| | 01:27 | and move it to another machine or another
folder, it won't look further than that.
| | 01:31 | It's going to find the
folders that are closest to it.
| | 01:34 | We have an assembly which then links to
a part, which then links to a drawing.
| | 01:37 | If I were to do Save As in the file
structure, it's going to change that
| | 01:42 | directory linking from assembly to
the new part name back to the drawing.
| | 01:46 | Now the problem is, we have a part that's just
sitting on the file structure not doing anything.
| | 01:50 | It's not linked to anything; it's the same
part as this one here, it's just no longer linked.
| | 01:56 | So that's not really the ideal
way to change names of files.
| | 01:59 | A better way is actually
to use SolidWorks Explorer.
| | 02:02 | So let's jump in there.
| | 02:03 | This is the SolidWorks Explorer and we
have that same Assembly opened up here
| | 02:08 | under just Desktop > Exercise Files >
Ch 1 and we are under the Sample folder.
| | 02:12 | We've got the three files
that make up that Assembly.
| | 02:14 | If I click on each one I can see it,
and here is my top-level Assembly.
| | 02:18 | Now if I wanted to change any one of
these names, I can right-click on it and
| | 02:23 | click on the Rename button.
| | 02:24 | Notice this file is the 1.4-3 and it goes out
and searches the file structure for that Assembly,
| | 02:32 | or any linked files actually, and the only one
it's finding is that Assembly which is the 1.4,
| | 02:37 | and make sure we have a Checkmark
here where it says Update where used.
| | 02:40 | Now if I click here and I change
it to 1.4-4 for instance, click OK.
| | 02:46 | It's going to give me a little error. It's
going to say, hey, there's a problem saving this,
| | 02:49 | and the reason it is, is because we
actually have that part open in the background.
| | 02:52 | So let's go back to SolidWorks and let's just save
these, close them, jump back over here, click OK.
| | 02:59 | Now let's try it one more time.
| | 03:01 | This time, no problem. They changed from -
3 to -4 and everything up based just fine.
| | 03:06 | Now the other way and people will get themselves into
trouble is going just to a regular Windows Explorer.
| | 03:12 | Now under Windows Explorer, I am in the
same folder, I jump in that same file here
| | 03:16 | and I can see those file names.
| | 03:18 | Now I were to say, click on that
and hey, let's just rename it, right?
| | 03:21 | So if I go and change this one to
-5 for instance, and I save that.
| | 03:25 | It'll allow me to do that, no problem.
| | 03:26 | The only problem is, is when I go back into
SolidWorks, it's not going to know which file is what.
| | 03:31 | Now SolidWorks does help out a bit and
they'll say, hey, I can't find this file,
| | 03:35 | can you locate it for me?
| | 03:36 | But that's probably not the
best method for going about that.
| | 03:38 | Okay, let's jump back into
SolidWorks and open that file.
| | 03:41 | So if I click on R on the keyboard,
it brings up my Recent Documents.
| | 03:45 | Here is 1.4. Let's open it up, and notice the
files have now updated to 1.4 and -2 and -4.
| | 03:51 | So there is no longer a -3.
| | 03:52 | It's been replaced by -4 and we don't have any
extra files just floating around in our file system.
| | 03:57 | So that is a nice little update on that,
and it's the best way to change files.
| | 04:02 | We can also do some saving
and backing up in SolidWorks.
| | 04:05 | If I click on the Options tab on the top
of the screen, under the System Options,
| | 04:09 | about three-quarters of the way down,
there is a tab called Backup/Recover.
| | 04:13 | Now I can automatically recover data
for each one of my files if the SolidWorks
| | 04:18 | were to crash for instance and I
can do it in a certain interval.
| | 04:21 | So 10 minutes seems like a long
time, so I'm going to change it to 5
| | 04:24 | and then wherever I'm saving this at,
this is kind of the default and that's fine.
| | 04:29 | If I go down here to Backup, I can
save backup copies of my document.
| | 04:33 | By default 1, I can change this to 3
for instance, and that's going to save,
| | 04:36 | the last three times I save that
document, it's going to put that in a folder.
| | 04:41 | I've got a folder called C:\Backup here.
| | 04:44 | Using that folder, you can
change it to anything you'd like.
| | 04:47 | I'd actually recommend not saving it on
your C drive and saving it to a server
| | 04:51 | or an external backup drive, something
along that lines that can make sure that
| | 04:54 | if this computer were to crash
that you'd still have those files.
| | 04:57 | Just a little housekeeping here is, if
you're saving multiple copies of each file,
| | 05:01 | you can get a lot of files in this one folder.
| | 05:04 | So automatically every 7 days here
this would remove the older backups and
| | 05:08 | make sure you're not adding
too many files to that directory.
| | 05:11 | And the last thing here is just if you
work on a document, you want to have a
| | 05:14 | reminder telling you every certain
amount of minutes to save your work.
| | 05:17 | It's definitely advisable.
| | 05:18 | SolidWorks in general is a very amazing
software and you can do amazing things with it.
| | 05:23 | But along the way, just make
sure you're saving your work.
| | 05:25 | Naming files correctly the first time
is really the best way to make sure that
| | 05:29 | you don't get into trouble with
losing files and having issues like that,
| | 05:33 | and it's going to be a lot less
clutter and a lot better designs.
| | Collapse this transcript |
|
|
2. Introducing the 3D WorkspaceUnderstanding the 3D world| 00:00 | Sketches are the fundamental
building block in all SolidWorks features.
| | 00:04 | But before we can start sketching, let's
learn about the drawing environment and
| | 00:08 | navigating in the 3D workspace.
| | 00:11 | All sketches start on a face or a plane.
| | 00:13 | In the beginning we don't have any faces, so
we're stuck with the three fundamental planes.
| | 00:17 | We have the Front Plane, Top
Plane, and the Right Plane.
| | 00:20 | If I click on any one of these, I can show it
by clicking on the little Goggle icon or Show.
| | 00:26 | Once that's shown, I can also show
the other ones if I need to or want to,
| | 00:31 | and I'm going to spin this user
environment around just by holding on
| | 00:34 | the middle mouse key to spin the environment.
| | 00:36 | I can also zoom in and zoom out
just by scrolling with my mouse.
| | 00:41 | The Origin is what we want to
tie most of our drawings into.
| | 00:45 | Somehow it links to that center of our part.
| | 00:49 | And I can move that environment
around also down here with this tria,
| | 00:51 | which is the lower left-
hand corner of your screen.
| | 00:53 | You can double-click on any
one of those and spin it around.
| | 00:56 | I can see this a little
better if I open a different part.
| | 00:58 | So I'm just going to jump into some
parts that are open here, open this one up,
| | 01:04 | and double-clicking that spins that around.
| | 01:06 | I can see the right side, spin it
around this way, spin it around that way,
| | 01:11 | a bunch of different ways I
can look at that environment.
| | 01:13 | This is very similar to what we
learned earlier with the Spacebar.
| | 01:16 | By clicking the Space, I could get
the Orientation up, I'll go to Front,
| | 01:21 | or Trimetric or Isometric View.
| | 01:23 | It's a nice way to look at the environment.
| | 01:25 | On the top of the screen I have
several commands that I can use.
| | 01:28 | The very first one is Zoom to Fit.
| | 01:30 | Now for instance, I might have
had this drawing over here or
| | 01:33 | somewhere out in the Drawing View that
didn't make a lot of sense over here.
| | 01:36 | If I click on Zoom to Fit, it's going to bring it
right into the center of the screen so you can see it.
| | 01:41 | If there's something I'd
like to look a little closer at,
| | 01:43 | I can use this one here,
which is the Zoom to Area,
| | 01:46 | and then just drag a little box
around the area I'd like to look at.
| | 01:49 | Click OK, it zooms right in.
| | 01:50 | The next one is Zoom Previous View.
| | 01:54 | So if I click on that once,
it takes me to the last View.
| | 01:56 | I can continue to click on it to
all the different views I've been in.
| | 02:00 | The next one is very interesting.
| | 02:00 | It's called the Section View.
| | 02:02 | I can click this part here.
| | 02:03 | Click on Section and it's
going to slice it in half.
| | 02:06 | By default using the Front
Plane to section that part.
| | 02:10 | I can also use for instance, the Top
Plane and drag things around in it,
| | 02:15 | or the direction I want to use.
| | 02:16 | Drag it up here, you can see as you're going
through that part, dividing it up in different features.
| | 02:23 | I can also click on the
Right Plane, there it is.
| | 02:25 | I can also change the angle or
the distance from one of the planes
| | 02:29 | to something else to make it
so it doesn't change things.
| | 02:33 | Once you're happy with what
that does, you can click on OK,
| | 02:36 | and now you've got a nice
Section View of that part.
| | 02:39 | Further along here we've got View Orientation,
which is a lot of what we just looked at.
| | 02:43 | You can look at the top, so just
multiple ways you can look at the same things.
| | 02:47 | Display Style. Right now we're
looking at it in a shaded mode,
[00:02:510.84]
so I'm going to turn that Section View off,
and I'm looking at this thing in shaded.
| | 02:54 | I can go and change it to non-shaded, or
non-edges, just wireframe, see-through...
| | 03:01 | There are a lot of different options here as
far as how you want to look at that environment.
| | 03:05 | Also notice this is in gray. If I want to
change the color, I've got this Edit Appearance.
| | 03:11 | I've got a lot of different
materials over here I can use on the right,
| | 03:14 | so I can assign now a certain material like a
glass one with that, or I can just add a color.
| | 03:19 | So over here if I just say I want this
thing to be red, I can click on the red,
| | 03:22 | click OK and now that material or
that color has been added to that part.
| | 03:26 | You should now understand how to
interact with drawing environments
| | 03:28 | in all the relative planes and the axes.
| | 03:31 | The three fundamental planes are where all
drawings start from, so get started there,
| | 03:35 | select your plane, start your
sketch and build your model.
| | Collapse this transcript |
| The six steps used in almost all modeling features| 00:00 | Modeling in SolidWorks is repetitive.
| | 00:02 | We use the same six steps over and over and over
| | 00:05 | to generate the features
required to build a model.
| | 00:09 | These six steps will help you
to remember the basic workflow.
| | 00:12 | Let's take a look at them:
The Six steps of Modeling.
| | 00:14 | First, select a face or plane;
| | 00:16 | number two, start a sketch
on that face or that plane;
| | 00:21 | draw the geometry you're going to use;
| | 00:23 | next, tie that geometry into the origin;
| | 00:26 | add a relationship to control it;
| | 00:27 | and then create the feature.
| | 00:28 | Let's go ahead and try these out.
| | 00:31 | Starting with a new part, when
you're first into the environment,
| | 00:34 | I have to start a sketch on a Face or a Plane.
| | 00:37 | To do so I have these three
fundamental planes here on the left-hand side:
| | 00:42 | I have the Front, Top or Right.
| | 00:42 | I'm going to choose the Top Plane here and
then go into the Sketch and start a new sketch.
| | 00:48 | Notice as I click on that,
it spins that plane around.
| | 00:51 | So I'm looking straight at it;
that's also considered normal too.
| | 00:54 | Step two, start a sketch, we're done with that.
| | 00:57 | Step three, draw the geometry.
| | 00:59 | I'm going to start with a
rectangle. Just draw it out.
| | 01:03 | The size doesn't matter right now; we're
just putting some geometry on the screen.
| | 01:05 | I'm going to add a couple of holes
as well, so I'm going to go in here
| | 01:08 | and grab the Circle Command and just
place a couple of holes on the screen,
| | 01:12 | location doesn't really matter.
| | 01:14 | Next is, let's tie all of
this geometry into the Origin.
| | 01:17 | Here is the Origin in the center of the screen.
| | 01:19 | We want to tie the two circles in the square
so they're relational to that center point.
| | 01:24 | To do that, I'm going to use a
little bit of construction geometry.
| | 01:26 | There's a thing called a
Centerline, and I can use that to do that.
| | 01:30 | I'm going to grab that upper corner here, drag a
line down to the bottom right-hand corner there,
| | 01:35 | and then I'm going to click on that origin,
| | 01:37 | hold down the Ctrl key and grab that line.
| | 01:40 | Once I select those two, it gives me the
ability to add a midpoint relationship.
| | 01:45 | Do that and notice it snaps to the center point.
| | 01:46 | Now I've got these two circles out
here that I need to do the same thing too.
| | 01:51 | I'm going to start another Centerline.
| | 01:53 | This time, let's start the Centerline off
to the left-hand side of the screen here,
| | 01:57 | and notice as I get in a horizontal-relationship
to the origin, it gives me this little helper line.
| | 02:01 | Click here, drag it across
to the other side and snap.
| | 02:04 | I'm going to select that origin again,
| | 02:07 | and this time I'm going to hold
down Ctrl and select the line.
| | 02:09 | As soon as I let go of Ctrl, it gives me the
option of the Midpoint or Coincident relationship.
| | 02:15 | I'm going to choose
Midpoint which makes that line
| | 02:18 | so it's always on the midpoint of the origin.
| | 02:21 | Now I can grab these circles, drag
them directly over the points and let go.
| | 02:27 | Now we've got a relationship that combines
these two circles and makes them origin-centric.
| | 02:31 | I'm going to add one more
relationship here that just has this circle here,
| | 02:36 | that circle there, and
they're going to be equal.
| | 02:38 | Now we're going to get more into
relationships and how we add them,
| | 02:41 | delete them, and change them in future chapters.
| | 02:43 | I just wanted to give you a quick
walkthrough them so you see how they're used.
| | 02:46 | The last step is creating the Feature.
| | 02:47 | What we're going to do now is
Feature > Extruded Base/Boss. Click OK.
| | 02:51 | As soon as I do that, it turns
it into an Isometric type view,
| | 02:55 | and gives me this little
handle I can drag up or down.
| | 02:58 | Drag that up. It gives me a
representation of what it's going to create.
| | 03:03 | I can also drag the arrows down to
create a feature in another direction as well.
| | 03:08 | As soon as it looks the way you want,
click OK and you have your first feature.
| | 03:13 | By remembering these basic steps, the modeling process
will be easier to understand and more straightforward.
| | 03:18 | Keep in mind the
repetitive nature of all features.
| | 03:21 | The inputs and outputs will be
different, however the steps will be the same.
| | 03:24 | In conclusion, let's step back and take a
look at the Word document with the six steps.
| | 03:30 | I recommend printing this out,
putting it in your cubicle or in your desk
| | 03:33 | to help you remember the six
steps for your next modeling feature.
| | Collapse this transcript |
| Starting a new sketch| 00:00 | Almost all features in
SolidWorks start with a sketch.
| | 00:03 | Sketching correctly and effectively
is the key to be a proficient designer.
| | 00:07 | In the six steps of solid
modeling we covered the basics.
| | 00:11 | However, let's get in a little more depth here.
| | 00:13 | Let's pick either the Front, Top or Right Plane.
| | 00:15 | I'm going to choose the Top Plane.
Select that Plane, make sure you're in the
| | 00:19 | correct sketch tab and then click
the very first icon there under Sketch.
| | 00:22 | As soon as I do that, I'm looking at that plane,
head-on, and I'm in the Sketch environment.
| | 00:27 | I'm just going to throw a
little sketch up on the screen here.
| | 00:29 | I'm just going to use the Rectangle
Command, I'm just going to draw it out here.
| | 00:32 | I'm going to use that
Centerline we covered earlier,
| | 00:37 | and then I'm going to click on that origin,
hold down the Ctrl key and grab that line.
| | 00:41 | Once I select those two, it gives me the
ability to add a Midpoint relationship.
| | 00:44 | So I have that first design here, I can
still move it around a little bit if I need to.
| | 00:49 | Once I have my first sketch,
I have a couple of options.
| | 00:53 | If I want to get out of that sketch and go
to something else, or delete that sketch,
| | 00:56 | I have these two icons on
the upper right-hand corner.
| | 00:58 | The first one is called Exit Sketch.
| | 01:00 | What that's going to do is just
going to draw me out of that sketch,
| | 01:03 | and it's going to drop it over here
on the left-hand side of the screen.
| | 01:05 | The sketch is still there,
but now it's grayed out.
| | 01:07 | So I don't have the ability
to edit the sketch at all.
| | 01:09 | I just have it listed here as Sketch1.
| | 01:12 | If I want to get back into that sketch, I
can just click on it and you'll notice I get
| | 01:15 | this little in-context menu box that pops up,
and the very first thing is Edit Sketch.
| | 01:20 | Next one is Sketch Plane.
| | 01:21 | I can suppress the feature.
| | 01:23 | There's a bunch of things I can
do here: Show Edit, Normal To,
| | 01:26 | but the first one I'm
looking for is called Edit Sketch.
| | 01:28 | Click on that, now I'm back in the
environment that I can modify this sketch around.
| | 01:33 | The second one here is Cancel, and
it's just going to delete you out of that,
| | 01:37 | so most time you want to use the red X
because that's going to not save any of your work.
| | 01:40 | Once you have what you like,
what I'm going to do now is,
| | 01:42 | I'm actually going to turn
this into an Extruded Feature.
| | 01:46 | Now we're going to cover
Extruded Features in future chapters.
| | 01:48 | So I'm just going into the very
basic command of extruding a feature,
| | 01:51 | just to give us the ability
to draw on a few more faces.
| | 01:54 | So I'm just going to drop
that Extrude Feature there.
| | 01:57 | So now we have a block we can
start continuing our model on.
| | 02:01 | I'm going to say Sketch, and this time
instead of choosing one of these three planes here,
| | 02:05 | I'm going to choose the Face.
| | 02:06 | This time I'm going to choose this face
here and I'm going to start a sketch on it.
| | 02:09 | If I click on the Spacebar, I
get the option of Normal To.
| | 02:12 | That way I can spin it
around and look directly on it.
| | 02:14 | So I'm going to use the Circle Command,
| | 02:17 | and I'm just going to put a
circle right there in the center,
| | 02:19 | and because I want to be Origin-
centric, I'm going to use the Centerline.
| | 02:22 | I'm going to tie-in from the origin
to the centerpoint of that circle.
| | 02:28 | Once I have that, I have the ability to go ahead and
extrude it out again if I wanted to and create a feature.
| | 02:33 | The Feature Manager is the main
interface for controlling your model.
| | 02:36 | All features and their sketches
are listed in order of creation.
| | 02:40 | By selecting a feature we're able to access the
sketch and their properties associated with it.
| | 02:45 | Each feature is independent of the others,
| | 02:46 | however many features are built upon
and related to the previous features.
| | 02:50 | Notice the two features here; we have
feature 1, our Boss-Extrude1 and Boss-Extrude2.
| | 02:56 | Under each one of those
features is the sketch that created it.
| | 03:00 | If I want to modify it or
change any of these features,
| | 03:03 | I can either change the sketch that
makes it or the feature that drives it.
| | 03:07 | The sketch itself changes
the size or the shape of it.
| | 03:11 | The feature itself is really the
length of the Extrude or the Cut.
| | 03:16 | There are a few other options that we can
put in here and we'll cover those later.
| | 03:19 | But you think about it as related but
independent. The sketch can be anything you want.
| | 03:24 | So if I go back and I change
that sketch and I make it smaller,
| | 03:27 | the feature doesn't care it's smaller.
| | 03:30 | Now the feature extrudes the exact
same length but the sketch changed.
| | 03:34 | Same thing if I go back to that
same sketch, click on Normal To it,
| | 03:39 | and I add a little bit to it,
put one more circle out here.
| | 03:42 | Get out of that and then guess what happened?
| | 03:47 | It just added one more
circle to that Extrude feature.
| | 03:51 | The Feature Manager over
here looks exactly the same.
| | 03:53 | The only thing that changed was that
underlying sketch, and we just added one thing to it.
| | 03:56 | So we can always go back and
change or modify each one of those.
| | 03:59 | To get into that mode, we click
on the sketch we want to change,
| | 04:02 | click on Edit Sketch or click on the
Feature itself and change that entire Feature.
| | 04:09 | The Feature Manager is user's main
interface for working with a model.
| | 04:13 | Understanding the key aspects of
the interface is an essential skill
| | 04:17 | to being proficient in SolidWorks.
| | 04:19 | However, sketching is the most important aspect
of design and the key to a good SolidWorks feature.
| | 04:25 | Take the time to think through your
sketches and develop simple and effective layouts.
| | 04:30 | Look for symmetry, use
construction geometry, and add relations.
| | Collapse this transcript |
|
|
3. Basic Sketching ToolsSketching lines and center lines| 00:00 | The Line tool is the most common
tool in our arsenal of Sketch tools.
| | 00:04 | It's simple to use and easy to understand.
| | 00:07 | To get started, let's click on the Sketch tab,
make sure we've got a Sketch button up here.
| | 00:11 | Then, we have to choose a face or a plane.
| | 00:13 | Notice we don't have any faces, so
we must choose one of the planes.
| | 00:15 | I'm going to choose the Top
Plane and click on Sketch.
| | 00:18 | Once we're in the Sketch environment,
we're going to jump in and grab the Line tool.
| | 00:22 | The Line tools are what we're going to
use to create most of geometry in our model.
| | 00:27 | So we're going to use the click-
click method to get started with that.
| | 00:30 | So I'm going to click
once where I want to start,
| | 00:32 | and then notice as I move
my mouse around the screen,
| | 00:35 | I get this little length indicator,
telling me how long that line is.
| | 00:39 | As I get close to the horizontal here,
notice it pops up with an angle of 180 degrees
| | 00:44 | and if go up here, I get like 135,
90, and then somewhere over here,
| | 00:51 | we've got a 45, 0 and I've got a length.
| | 00:53 | If I didn't want any of those, I just
figure out where I want to end my line,
| | 00:58 | click one more time, and it stops.
| | 00:59 | As soon as I've created my first line
though, I get these like helper lines,
| | 01:03 | the little yellow lines on the screen
and I can use those to create geometry
| | 01:07 | that it's going to
automatically add a relationship.
| | 01:09 | So notice if I click here, I would
automatically add the relationship of
| | 01:12 | being perpendicular to the first line I created.
| | 01:14 | I don't really want to do that, so
I'm just going to click out here.
| | 01:17 | Once I'm done creating lines with
this command, I want to exit out of it.
| | 01:21 | To do that, I hit Esc. It takes me out
and I'm back to my regular selection cursor.
| | 01:26 | The other thing we might want to use
in SolidWorks is Construction Geometry.
| | 01:30 | Now Construction Geometry is not
actually used for creating models.
| | 01:34 | It's really just for laying
things out, so that we have lines and
| | 01:37 | things that we can use to tie things
to the origin or tie objects together
| | 01:41 | without actually using that geometry
to create that feature or that solid.
| | 01:45 | So, to grab Construction Geometry, we're
going to use what's called a Centerline Command.
| | 01:50 | Now, the Centerline Command and
Construction Geometry really is the same thing,
| | 01:55 | just they're calling it Centerline but
we can use it as Construction Geometry.
| | 01:58 | So I'm going to create a line
from this endpoint by clicking there.
| | 02:02 | Click again on the other side.
| | 02:03 | I've got my first Construction Line.
Hit Esc, and turn off that command.
| | 02:08 | Clicking on that line, notice over here on
the left-hand pane is the Line Properties.
| | 02:13 | One of the things that is turned on is for
construction; I'm using that line for construction.
| | 02:17 | If I were to turn that off, it
would turn it back into a regular line.
| | 02:21 | Same thing as I click on a regular line. I can
go back, and turn that one to the construction.
| | 02:25 | So I have the ability to
switch between one and the other.
| | 02:27 | Keep in mind though, only the real
lines are actually going to be used;
| | 02:31 | construction lines are only
there just as these helper lines
| | 02:33 | to help things lay out in the correct fashion.
| | 02:36 | We have the ability to move these lines around.
| | 02:38 | If I select the center of the line,
I can drag that line in and out
| | 02:42 | to change the shape, but notice
the orientation doesn't change.
| | 02:45 | If I want to change the orientation, I
click on the endpoints of any of the lines.
| | 02:48 | That way, I can drag those points around to
change that shape; so click on the endpoints.
| | 02:53 | Grab the line, I will grab the end point.
| | 02:55 | I'm going to jump back in the Line command right
now and I'm going to start a new line here at the top.
| | 03:01 | So I'm going to click once, and once I drag it out
here, I'm just going to drag it on the horizontal.
| | 03:04 | If I were to drop this line
right here, it's going to create
| | 03:08 | what's called a horizontal
line, an auto-relationship.
| | 03:09 | Let's go ahead and do that.
| | 03:12 | As soon as I do that, it drops this
little green box right below that line.
| | 03:15 | That means it's attached to that line.
| | 03:17 | If I mouse over it, it
highlights the line and it shows
| | 03:20 | this is a horizontal line and now
it has that relationship, saying so.
| | 03:23 | If I didn't want that there, I can click on just the
green box and I can hit the Delete key. It drops it out.
| | 03:28 | If I wanted it again, I can always
go back, and I can add that in again.
| | 03:32 | We're going to cover relationships more
in the future, but just so you know that
| | 03:36 | if you're drawing, that's one of the things
that's going to pop up over and over again.
| | 03:40 | Coming back here, grabbing another line
here, same thing with the helper lines.
| | 03:45 | We've got the same option with the vertical.
| | 03:46 | If I go and create other lines here somewhere,
those helper lines are always going to pop up
| | 03:51 | and allow me to continue
to draw at right angles and
| | 03:54 | it's going to start adding
horizontal or vertical relationships as I go.
| | 03:59 | The Line tool is the basis
for most sketches in SolidWorks.
| | 04:02 | Although, it's simple to use, it's also
one of the most powerful building blocks
| | 04:05 | in the SolidWorks tool library.
| | Collapse this transcript |
| Using the Circle tool| 00:00 | The Circle tool takes us to
the next stage in sketching.
| | 00:03 | From the Circle tool, we
also get the basis for arcs.
| | 00:06 | There are several methods for
creating circles in SolidWorks
| | 00:09 | and the most basic is the Center Point Circle.
| | 00:11 | To get started, click on the Sketch tab,
start a new sketch, and let's pick a plane.
| | 00:15 | I can go up here, and grab the Circle command,
and notice there's a little dropdown next to it.
| | 00:21 | So I have two options; I have the
Perimeter Circle or the Center Point Circle.
| | 00:23 | Let's pick the first one.
| | 00:25 | I'm going to go ahead and click right
on the origin, and then drag this out.
| | 00:29 | Notice a little heads-up
radius button I can see there.
| | 00:32 | It tells us exactly what size
that circle is going to be creating.
| | 00:34 | Now, my second click is
going to drop that on the screen.
| | 00:37 | Notice my cursor is still the Circle command.
| | 00:40 | So anywhere I drag-and-drop a
circle or a two-point click,
| | 00:44 | I'm just going to continue creating circles.
| | 00:45 | To get out of that, go ahead and hit Esc,
and change back to my regular cursor.
| | 00:49 | If I want to move these
circles around the screen.
| | 00:51 | I can click on the center point of
that circle to drag it around the screen,
| | 00:56 | or I can click on the
perimeter of it to change its size.
| | 00:59 | Go over here, I can drag this one
around, change this one's perimeter.
| | 01:04 | The circle in the center though has
got this relationship that was added.
| | 01:07 | So if I try to grab that center point
and drag it around, it won't let me.
| | 01:10 | It says cannot drag.
| | 01:12 | And the reason is, we have this coincident
relationship that's locking us to that origin.
| | 01:16 | If I don't want that, I can
always click on that, hit Delete.
| | 01:20 | Now, I have the ability to
drag that around the screen.
| | 01:22 | If I want to add that back in, I can
click on that center point of the circle.
| | 01:26 | I can hold down Ctrl, select the origin, and I
can re-add that relationship, bring it back there.
| | 01:32 | We're going to get more into
relationship in the next chapter.
| | 01:34 | However, I just want to make you were
understanding what was actually happening there.
| | 01:38 | If I don't like a circle, I can always click
on it, and hit the Delete key. Take it away.
| | 01:43 | If I want to add it back, I can just
grab it up here, drag it out again.
| | 01:46 | Drag one of these circles and I drag
it over on top of the other circle.
| | 01:50 | Notice as I get close to it, it
highlights the circle it's going to drop it on,
| | 01:53 | and it also says, a proposed
relationship it's going to add.
| | 01:57 | So notice if I drop it on here, it's going to
add a coincident relationship to that circle.
| | 02:01 | Let go, notice it adds that
relationship; there it is!
| | 02:04 | What that means is now I'm locked
onto the outside of that circle.
| | 02:07 | I can spin it around, I can drag it out, drag
it in, but it's locked onto the base circle.
| | 02:12 | This circle over here, grab. I can drag it
around. Same thing as I highlight over that.
| | 02:17 | But notice there are these four
little points around that circle.
| | 02:20 | So if I actually snap
this on one of those points,
| | 02:24 | not only does it add a coincident
relationship, but also a horizontal relationship.
| | 02:28 | So now there are two.
| | 02:30 | Now, I cannot spin that one at
all, but I can drag it in and out.
| | 02:33 | So I have a relationship
added to both of those circles.
| | 02:37 | If I don't like any one of
those, I can always click on it,
| | 02:39 | I can right-click on it if I
want to and I can say Delete,
| | 02:41 | or I can just click on the circle
itself, hit Delete, get rid of it.
| | 02:45 | I have the ability to move these things around.
| | 02:48 | The next type of circle is the Perimeter Circle,
and I'm going to go up here and grab that circle.
| | 02:53 | What that's created from
is a series of three points.
| | 02:56 | So I already have some points I can kind of
pull out of the sketch that we already have.
| | 03:00 | So I can click on like the point here, I can
click on a point here, and maybe like the origin;
| | 03:05 | those three points and it creates a
circle through those three points.
| | 03:08 | If I just want to place three points
out here in the Sketch environment,
| | 03:13 | I can also create a circle through those.
| | 03:15 | Grab the Perimeter Circle, click
here, click there, and click there,
| | 03:20 | and it creates a circle through those three.
| | 03:21 | That's a Perimeter Circle and by
changing any one of these points,
[00:03:265.73]
and dragging it around, I can also
affect how that circle looks and shapes.
| | 03:29 | Notice it gives me those three
automatic relationship thing;
| | 03:32 | that circle is linked to those three points.
| | 03:34 | The Circle tool and the Line
command are the two sketch entities needed
| | 03:37 | to build almost all geometry in SolidWorks.
| | 03:40 | Mastery of these tools is essential
to being proficient in SoildWorks.
| | Collapse this transcript |
| Adding and removing relationships| 00:00 | Relations are what take simple
sketch entities to the next level.
| | 00:04 | Relations can control size, location,
and equality between sketch elements.
| | 00:09 | Relations are a core function of SolidWorks
and understanding how they work is essential.
| | 00:14 | Let's take a look at these
four lines on the screen.
| | 00:16 | You think about what creates a
rectangle or what creates a square?
| | 00:19 | Is this a square or a rectangle? Probably not.
| | 00:22 | So let's take a look and see how we can
convert this to being a rectangle or a square.
| | 00:26 | We're going to do so using relationships.
| | 00:30 | If I click on this first
line here, notice it highlights.
| | 00:33 | If I hold down the Ctrl key, I have
the ability to select the adjacent line.
| | 00:37 | As soon as I release the Ctrl key, I get this
little pop-up window here giving me a bunch of options:
| | 00:43 | Horizontal, Vertical, Collinear,
Perpendicular, Parallel, Equal, or Fixed.
| | 00:51 | These are a bunch of relationships that I can add
to these two lines to control how they interact.
| | 00:57 | Notice, I also have those exact same
Relationships over here on the left-hand side.
| | 01:01 | So to create this into a rectangle,
we probably want to add a relationship
| | 01:05 | that has a perpendicularity between those two.
| | 01:08 | Click on this first one and notice what
happens, it changes the way they interact,
| | 01:11 | and it's given us this little
Relationship Indicator showing
| | 01:14 | there's a perpendicular
relationship between these two.
| | 01:16 | Now if I highlight over that little green
box, notice the two related lines highlight.
| | 01:22 | But we still don't quite
have a rectangle, do we?
| | 01:24 | So let's try again on the other side.
| | 01:26 | So let's click on this first line here,
hold down Ctrl, select the next line and
| | 01:31 | add that same Perpendicular Relationship.
| | 01:33 | Well, it's getting closer,
but it's still not quite right.
| | 01:37 | So the third one we're going to add is
going to actually turn this into a rectangle.
| | 01:40 | So I'm going to click here, hold down Ctrl, select
the next line, and go ahead and say Perpendicular.
| | 01:46 | Now we've got a rectangle, we can
drag it out, we can move it around;
| | 01:49 | we can play with this rectangle.
| | 01:51 | But it's not horizontal;
it's not a horizontal rotation.
| | 01:54 | It's kind of rotated out in some angle here.
| | 01:56 | So I can then add one more
relationship here to the top.
| | 01:59 | I can say this line here is Horizontal, and
now I've got a rectangle that's quite controlled.
| | 02:04 | We don't quite have it linked to the
origin yet; that would be the next step,
| | 02:08 | but we can obviously go ahead
and add up one more line here,
| | 02:12 | which would be a construction line, which is not
used for the geometry, just to help us lay it out.
| | 02:16 | I'm going to add another
relationship here as far as this line.
| | 02:19 | I'm going to hold down
the Ctrl, select the origin,
| | 02:21 | and this time I'm going to say, I want
this to be right in the Midpoint of that line.
| | 02:26 | Now as I drag this rectangle around,
it's linked to the origin and all these
| | 02:31 | relationships are constantly active
controlling the shape of the object.
| | 02:37 | If I don't like one of these relationships, I can
always just click on that relationship and hit Delete.
| | 02:42 | Notice if I delete the relationship, the lines
don't move, they stay exactly where they were.
| | 02:47 | However, if I click on this line now, I
have the ability to start wiggling this
| | 02:51 | thing around and it's going to start
violating this being a nice rectangle.
| | 02:55 | So if I want to fix it again, I go back
here, add that relationship one more time,
| | 02:59 | and I'm back to where I was.
| | 03:01 | Sometimes when you're looking at these
drawings, you can see a lot of these relationships.
| | 03:05 | It makes it hard to kind of see what's going
on, or you might be not seeing them at all.
| | 03:09 | To show or hide these, you can go
into the View Command, click on View and
| | 03:13 | go down here to Sketch Relations. Hide them,
and you can back and you can say Show them.
| | 03:19 | Adding and using
relations can be a huge time saver
| | 03:21 | and make your sketches easier to
update and simpler to understand.
| | 03:25 | Relationships are used throughout
SolidWorks and an understanding of how they work
| | 03:29 | is the most important thing in SolidWorks.
| | Collapse this transcript |
| Understanding relationship types| 00:00 | We've covered some of the basic relationships,
now we're going to go a little more in-depth
| | 00:04 | and cover all of the relationships that
we can possibly add to sketch entities.
| | 00:09 | To get started, we're
going to start with Coincident.
| | 00:11 | Coincident is probably your most common of
the sketch relations, and what that means is
| | 00:16 | it's going to have one point just touching
another or one line touching another line.
| | 00:20 | So the origin is here, if I would like to
make a Coincident Relationship between the two,
| | 00:24 | I click on the point, hold down Ctrl, select the
other point that I would like to make that related to.
| | 00:30 | As soon as I let go, it gives me the
three options that would be available,
| | 00:34 | the three relationships that
would make sense in that situation.
| | 00:38 | So the first one would be either
Horizontal, Vertical, or Coincident.
| | 00:42 | So Coincident, and that just moves
down there and locks on to that origin.
| | 00:46 | It gives us this little reminder box in green
showing that the relationship has been added.
| | 00:50 | Now I can move that line around.
| | 00:53 | So one side of it is connected
but the other side is still free.
| | 00:55 | I could connect this point and
this point in the same manner,
| | 01:00 | but instead of holding down
Ctrl and selecting the two points,
| | 01:03 | I can just click on that and just drag it over.
| | 01:05 | As I drag it over, notice
it snaps on to that point,
| | 01:09 | which produces the same type of
relationship and locks those together.
| | 01:13 | So that's a Coincident
Relationship again, but notice it doesn't
| | 01:17 | give us the little green box, because
it's an implied relationship this time,
| | 01:20 | because I was just saying
these two points are not connected.
| | 01:22 | So Connected and Coincident are very similar.
| | 01:25 | This line over here, I can drag around.
| | 01:30 | So we're going to look at a few different of
the other relationships we can add to this.
| | 01:34 | First one would be just Horizontal.
| | 01:36 | So I'm going to actually drag this down
a little bit easier here so you can see.
| | 01:41 | So if I were to just make this
line straight on the Horizontal,
| | 01:46 | it would automatically snap to the Horizontal,
| | 01:49 | but not necessarily give you
that Horizontal Relationship.
| | 01:51 | Notice it gives a white box,
means it's implying a Horizontal,
| | 01:54 | but it's not actually
going to add that relationship.
| | 01:56 | If I do want to add a
relationship to make this Horizontal,
| | 01:59 | just click on the line and say Horizontal.
| | 02:01 | Now it adds a green box
with a Horizontal Relationship
| | 02:05 | and now this line can't do
anything besides be Horizontal.
| | 02:07 | I'm going to draw another line here.
| | 02:09 | Notice, if I draw it correctly in the
Vertical, it adds that Vertical Relationship.
| | 02:16 | If I draw another line kind of off at an
angle here, and I want it to be Vertical,
| | 02:19 | I can select the line and then just
select Vertical; it does the same thing.
| | 02:25 | Notice here, this also added a relationship.
| | 02:28 | Notice the 1 following the
relationship; that mean it's just a pair.
| | 02:33 | So you're just looking for 1 matches 1,
2 matches 2, 3 matches 3 and so on.
| | 02:37 | So if I highlight that
relationship, the two pairs match up.
| | 02:42 | And notice, what it's saying is the endpoint
of this line here is Coincident to this line,
| | 02:47 | even though they're actually not
touching. So let's move it around.
| | 02:50 | The next one we're looking at is
Perpendicular; we covered this a little earlier.
| | 02:54 | But say these two lines here, we
can say select one of the lines,
| | 02:58 | hold down Ctrl, select the other line,
| | 03:00 | now we have a whole bunch of options we can use.
| | 03:02 | So I'm going to pick the Perpendicular one and
that just adds that right angle to that corner.
| | 03:06 | I could still spin it around, but it
continues to maintain that relationship.
| | 03:10 | Parallel is the next one, I'm just
going to add one more line over here.
| | 03:14 | To add Parallel Relationship I'm just
going to select the pair by holding on Ctrl,
| | 03:18 | selecting the two objects,
and clicking on Make Parallel.
| | 03:21 | And no matter what I do, I can move these
things around, those are always going to be parallel.
| | 03:27 | Equal is the next one, so I'm
going to use this pair of lines here,
| | 03:30 | select this line here, hold
down Ctrl, select that line there,
| | 03:33 | add the Equal Relationship;
now they are the same length.
| | 03:35 | If I move these things around, I can
notice these little helper lines will pop up
| | 03:39 | if I want to arrange these in some manner,
if I'm going to create some kind of an object
| | 03:44 | or a sketch to be extruded or
turn it into some kind of geometry.
| | 03:48 | The last one is Fixed, and Fixed is very useful if
you want to kind of constrain a point or a whole line.
| | 03:54 | So if I just want this whole line
here, if I add this little anchor to it
| | 03:57 | that says Make Fixed, it just
means this line can't really move.
| | 04:00 | I can still drag the ends of it,
but the line itself, it can't move.
| | 04:04 | I can't move this line up
and down and I can't drag it.
| | 04:06 | But I can change the length of it still.
| | 04:08 | If I got rid of that one and I just
added that Fixed Relationship to the end,
| | 04:15 | then just that side of the line
won't move, so I can't grab this one.
| | 04:18 | The same thing if I created
another line here, just off in space;
| | 04:23 | actually get rid of that, add a
Fixed Relationship just at the end of it.
| | 04:27 | Now I have something that I can drag
around, but it's going to be fixed at one end.
| | 04:32 | Learn and use relationships in your designs.
| | 04:34 | They make for simpler
sketches with parametric attributes.
| | 04:38 | They are a fundamental part of
SolidWorks and give the designer
| | 04:40 | the added power beyond
basic pen and ink sketching.
| | Collapse this transcript |
| Dimensioning a sketch to define specific size attributes| 00:00 | Now that we've learned the
Line and the Circle Command,
| | 00:03 | let's go ahead and create a part
using those and we'll learn also
| | 00:06 | how to dimension that
part and put it all together.
| | 00:09 | So to get started, let's just start a sketch.
| | 00:11 | I'm going to choose the Top Plane.
| | 00:13 | We're going to make a
little bolt link in this Part,
| | 00:15 | so it's going to start off with a Centerline,
| | 00:17 | so we obviously want to
tie everything to the origin.
| | 00:19 | So I'm just going to start a
line here, snap it across here,
| | 00:22 | and then I just want to make
sure it's centered on the origin,
| | 00:24 | so I'm going to select the origin,
hold down Ctrl, select the line,
| | 00:28 | and I'm going to say I want this to be Midpoint.
| | 00:31 | Then I'm going to grab the Circle command,
which we already learned, center point circle,
| | 00:35 | I'm just going to snap it to the endpoint
here, click once, drag it out, click again.
| | 00:39 | Same thing down here, click on
the point, drag it out, click again.
| | 00:42 | Now these are not the exact same size,
so let's go ahead and add a relationship,
| | 00:46 | which we just learned about, so
let's click on the top circle,
| | 00:49 | hold down Ctrl, select the other
circle and let's say these are Equal.
| | 00:52 | Now we're going to make the outside of the link.
| | 00:55 | So that's going to be made up of
two more circles and two lines.
| | 00:59 | So I'm going to grab that circle again,
click on the endpoint, drag it out,
| | 01:03 | and do the same thing down here,
click on the center point, drag it out.
| | 01:06 | Same thing; let's make these both equal.
| | 01:09 | Now use a couple of lines to
connect these two together.
| | 01:12 | I'm going to snap to that quadrant here,
drag a line down here to the quadrant here,
| | 01:17 | hit Esc; it ends that one segment.
| | 01:19 | Grab that line again, up
here, grab that quadrant,
| | 01:23 | drag down here to the next quadrant and end.
| | 01:25 | Now we can get out of that line command
by either hitting Esc or double-clicking.
| | 01:29 | One thing we haven't covered yet
but we will in the next chapter,
| | 01:32 | I'm going to give you a
preview of, is the Trim command.
| | 01:34 | Now, the Trim command is just
going to allow us to trim out
| | 01:36 | these extra parts of the
circle that we don't want.
| | 01:38 | So I'm going to grab the Trim and I'm
just going to trim out through these,
| | 01:42 | through these, through these, and through
those. So now we have what we call as the link.
| | 01:47 | Notice I can drag this around to
change size, both in and out of here.
| | 01:51 | Notice there is no dimensions though, so now
we're going to learn about dimensioning a Part.
| | 01:54 | My hole to hole center here should be 4 inches.
| | 01:58 | So I'm going to add the dimension.
| | 02:00 | Click on the Smart Dimension tab, come over
here, our cursor turns into a dimensioning icon.
| | 02:04 | Now I can grab that line, drag it out, and click the
end where I want to place that dimension at, click here.
| | 02:11 | Notice it gives me the name of the
dimension automatically and then the length.
| | 02:14 | If I want to change that I can change it here,
Length, and notice now it says the Length@Sketch1.
| | 02:19 | Now I could make that anything I really wanted
to and just keep something that's descriptive.
| | 02:25 | Type in 4.0 here in this box,
click on the green check mark.
| | 02:28 | It says accepting the dimension, and
now it modifies the size and shape of that
| | 02:32 | and gives us that 4-inch dimension.
| | 02:34 | I can drag this around just by clicking it
and dragging it, and let's tie it together now.
| | 02:37 | I can still move the other parts of
this, but I can't change that length.
| | 02:43 | A couple more dimensions we want to add, so
go back up here, grab the Smart Dimension Tool.
| | 02:47 | We can either click on the Radius here or this
distance from here to here, so let's just do that.
| | 02:51 | So I'm going to click on the first
item, notice it gives me the 4.00,
| | 02:54 | and then drag over here and select
the second item we want to dimension to,
| | 02:57 | which now gives a
dimension between those two items.
| | 03:00 | Over here I'm going to say 2.0.
| | 03:03 | That brings that in a little bit and
now these circles need to be adjusted.
| | 03:07 | I can always drag these in and out
to get them close to the right size,
| | 03:11 | and then I'm going to go
ahead and add a dimension there.
| | 03:12 | So I'm just going to click on that
circle, anywhere on the diameter of it,
| | 03:16 | drag out a dimension, just click
wherever I want to place that dimension,
| | 03:19 | and I'm just going to say 0.75.
| | 03:23 | Notice the lines have been changing color.
| | 03:26 | When we first had the lines
drawn, they were all blue,
| | 03:28 | which means they are under-
defined or undefined sketches.
| | 03:31 | As they turn black, that
means they are fully defined.
| | 03:34 | So notice all the lines in
the sketch are now black.
| | 03:37 | That means they are fully defined,
they know exactly what they are,
| | 03:39 | and I can click on any one of these
things and try to drag it around,
| | 03:41 | nothing is going to move,
it's a fully defined sketch.
| | 03:44 | Now if I were to cause a problem, for instance I
went up here and I add an additional dimension,
| | 03:51 | it says, do we want to leave this
driving? So I'm going to say Yes.
| | 03:54 | Notice what it does to our sketch,
it turns it all yellow and says,
| | 03:58 | we have Conflicts, the whole sketch is
conflicting here, because I'm defining it twice.
| | 04:03 | I'm saying down here it's 2 inches across and
then I'm saying up here the Radius is 1 inch.
| | 04:08 | So SolidWorks actually
doesn't know which one to use.
| | 04:11 | So it says, these two conflict, and it
highlights everything in yellow that's causing a problem.
| | 04:16 | Notice the two circles in here are
still black, they're not in violation.
| | 04:19 | So I can either delete this or I can delete
this, either one of them will solve the problem.
| | 04:24 | This is fully defined and it's back.
| | 04:25 | Now if you do something that turns
everything red, which is a major violation,
| | 04:30 | it means that not only is
it a conflicting dimension,
| | 04:32 | but it's also actually causing the sketch to
fail, that's when you're really in trouble.
| | 04:36 | And the same thing happens is, it's
going to highlight all the items in red
| | 04:40 | who might be causing the trouble, so
you need to delete or change those items
| | 04:43 | to get back to a state of having
a fully defined sketch in black.
| | 04:48 | The next step here is to
turn that into a 3D Part,
| | 04:50 | and we're just going to skip ahead and
give a Preview of the Extrude command.
| | 04:53 | I'm going to drag this out a little bit,
we're going to make it a half-inch thick,
| | 04:57 | just type in 0.5 over here, click on OK.
| | 05:00 | This movie combined the Line,
Circle, and Centerline commands.
| | 05:04 | We also learned and used
relationships together to create a usable part.
| | 05:08 | We also got a first look at
the Trim and Extrude commands.
| | 05:12 | Dimensioning is very important in SolidWorks
and make sure to fully define your sketches
| | 05:16 | with no blue lines, no yellow
lines, and definitely no red lines.
| | 05:20 | Now we have a complete Part and this
Part will be used later in the course.
| | Collapse this transcript |
| Setting system options, units, and templates| 00:00 | Understanding how to modify basic system options is
essential to getting the correct results out of the software.
| | 00:06 | Templates are the starting point
for parts, assemblies, and drawings.
| | 00:10 | We're going to create our own
template to use in the rest of the course.
| | 00:13 | Right now I have a new part,
there's nothing in it quite yet,
| | 00:16 | and we want to go in and
change some of the options around.
| | 00:19 | So each part we start with always
has a starting template it uses.
| | 00:24 | On the top of the screen, we've
got a couple of things up here;
| | 00:27 | the very end one is called Options.
| | 00:29 | If I click on that, get
this window that pops up.
| | 00:31 | I have my General options here,
I have Drawing options as far as
| | 00:34 | how I want to look at things, a lot
of things you can go through here;
| | 00:38 | some of the colors of the
background, the sketch, the displays.
| | 00:41 | But this is more system-wide options,
this gives more document property.
| | 00:45 | So click on this other tab here,
that's going to give us Drafting Standards:
| | 00:48 | How we want to look at that? Arrows,
the Fonts, the Leaders, the Dimensions.
| | 00:53 | How we want these to show up when I start
drawing these on screen? How's that going to look?
| | 00:57 | Detailing, What do we want to actually
show on our parts? Do we want to show a grid?
| | 01:02 | Units is one we're going to probably use a lot.
| | 01:04 | Do we want to input our dimensions in millimeters or
in inches or centimeters or meters or miles or however
| | 01:11 | we want to use or input those dimensions and then
how many decimal points do we actually want to use.
| | 01:16 | So I'm right at, you see there is two, I could enter
three or four depending on what I want to change that to.
| | 01:22 | If I change these things, it actually was
based upon a standard, so that's an ANSI standard.
| | 01:28 | Now I'm changing this to an ANSI-MODIFIED standard
because I'm changing the tolerance of those inputs.
| | 01:33 | That's fine depending on what
kind of design you're working with;
| | 01:36 | you might need more or less precision.
| | 01:38 | A couple of other things down here,
we can look at like Image Quality,
| | 01:43 | just how you want to see
those things on the screen.
| | 01:45 | Once you have everything kind of
set up exactly the way you are,
| | 01:47 | you just click OK and that goes away.
| | 01:50 | Now we have Part7, which is an open Part.
| | 01:52 | I want to save out these
changes I made though to this template
| | 01:56 | to be my starting point for every
new part I'm going to get started with.
| | 02:00 | I don't want to have to go up there and
change it for millimeters to inches each time.
| | 02:03 | So to do that, I'm going to go to the File menu
. Under File menu, I'm just going to Save As.
| | 02:08 | When we Save As, by default, it
says Save As type Part which is here.
| | 02:14 | But I don't want to save this as a part, I
actually want to save this as a part template,
| | 02:18 | which is the third one down
Part template. So it's prtdot.
| | 02:20 | Once I've got a Part template I can name it out,
| | 02:25 | I'm going to name my Part template here, lynda2.
| | 02:30 | And then where do we want to
save these Part templates at?
| | 02:31 | Now you can save this anywhere you would like.
| | 02:34 | I have a folder on my C drive which is called
SolidWorks Data and you probably have one similar.
| | 02:39 | I'm going to click in here and I already have
one template, I'm just going to have one more,
| | 02:42 | so one of two, and you can have
as many templates as you want.
| | 02:45 | So you can turn things on and off,
change units, change features,
| | 02:49 | change the look of your start
point and just save those out
| | 02:53 | as a variety pack of different
templates you might be using.
| | 02:54 | So click on Save, that
just saves it as a template.
| | 02:57 | Now there's one more thing we
need to do to kind of hook this up.
| | 02:59 | When we start our files off it actually goes
and finds that template that I want to use.
| | 03:03 | So I'll go back up here to Options, and this
time we're going to be in the System Options tab.
| | 03:08 | We want to go down here to file locations.
| | 03:11 | Click on File locations and document
templates that's what it's asking for,
| | 03:14 | where are these templates stored at right now.
| | 03:17 | We need to add a path to wherever that
folder is we just saved our template at.
| | 03:21 | So click on Add, go ahead to C
drive which is where I saved this at,
| | 03:27 | and I saved it in SolidWorks
data and that's all I need.
| | 03:30 | You notice it adds C:\SolidWorks
Data as a path to our template.
| | 03:33 | Once we're happy with that,
click on OK, it saves that out.
| | 03:38 | Now when I go start a new
Part, I'm going to go to New,
| | 03:42 | and notice we're in what's
called the Novice window here.
| | 03:44 | There's a basic part
that's being used each time.
| | 03:48 | When I click on the Advanced tab, I actually have a few
more options as far as where I want to start my Part from.
| | 03:54 | So here is the basic Templates
here installed with SolidWorks,
| | 03:57 | and then each of these new tabs up
here are the paths that I'm going to add.
| | 04:01 | So notice I added that last
path here; SolidWorks data.
| | 04:03 | Here's lynda1 and lynda2, my two user-
defined templates that I can start from.
| | 04:07 | I'm going to pick lynda2, click
OK and that starts up my new Part.
| | 04:10 | So this has all the changes that we've already
made. I'd just like to go back up here, take a look.
| | 04:15 | So we can change the inches, we
could put three place decimal.
| | 04:18 | Those units or option changes
will automatically propagate through.
| | 04:21 | Creating a template configured with all the
options that you want to use in your design
| | 04:26 | will save you time and
help you focus on the design,
| | 04:28 | versus constantly having to modify
system options on a Part-by-Part basis.
| | 04:32 | Create templates in all
your most common Part types.
| | Collapse this transcript |
|
|
4. Relationships and Sketching ToolsSketching rectangles| 00:01 | The Rectangle command is nothing more than four line
segments and some relationships auto-created by SolidWorks.
| | 00:06 | There are several types of
rectangles preloaded into SolidWorks tools.
| | 00:10 | We can use them or we can create our own.
| | 00:13 | Depending on the tool we use, the
relationships are added differently.
| | 00:16 | The Rectangle is a nonessential command since
it can be created with just four line segments,
| | 00:21 | however it's a huge time saver.
| | 00:23 | Let's jump into SolidWorks
and create some rectangles.
| | 00:26 | I'm going to go into the
Sketch tab, start a new sketch
| | 00:29 | and we're going to select the
Top Plane to start sketching on.
| | 00:34 | So if I click on the Rectangle tab,
there's a bunch of options here.
| | 00:38 | There are five different types of
rectangles on the little dropdown arrow.
| | 00:41 | The very first one is the Corner Rectangle.
| | 00:43 | Let's go ahead and check that one.
| | 00:44 | Corner Rectangle is created by
creating a start point and then an end point.
| | 00:49 | So we're going to start at the origin.
| | 00:50 | Click once, drag it out,
and notice as I'm dragging,
| | 00:53 | I get this little heads-up display
of the X and Y size of that rectangle.
| | 00:58 | Get to the size I want, click again to
place the second part of that rectangle.
| | 01:02 | Notice as I created that rectangle, SolidWorks
automatically adds some relationships for us.
| | 01:08 | We've got a vertical, a vertical, and a
horizontal and a horizontal relationship
| | 01:12 | that have been pre-added by
SolidWorks that defines those lines.
| | 01:16 | Now I can just add a couple of
dimensions to define the shape.
| | 01:20 | So I'm going to type in 12 there and for the dimension
from this line to this line, I'm going to type in 10.
| | 01:27 | Now I have a fully-defined rectangle
that's a two-point Corner Rectangle.
| | 01:30 | Now, if I'm looking in SolidWorks and I'd like to
get rid of whatever I'm drawing on or working with,
| | 01:34 | I can drag a rectangle over a
section, highlight the whole thing,
| | 01:39 | and then hit Delete to get rid of it.
| | 01:40 | The next one is going to be the
Center Point Rectangle. So, click on that.
| | 01:44 | Center Point Rectangle is created much the
same way but this time it's going to start
| | 01:48 | at the origin and when I drag it out
notice it's located now on the center point
| | 01:52 | where I clicked and then I'm
grabbing that upper right-hand corner.
| | 01:56 | Same thing, it's giving me a heads-up
display of exactly the size I'm using.
| | 01:59 | So click there somewhere.
| | 02:00 | Now, we've got a nice rectangle. I
can drag it around to change its size.
| | 02:04 | It's very similar to the
first rectangle we created,
| | 02:08 | in that it's got a vertical, vertical,
horizontal, horizontal, auto-relations,
| | 02:12 | but we've also got these two
center lines that were added and
| | 02:15 | we've got some coincident points saying
that these lines are in the center points
| | 02:20 | or the coincident point to that
origin locking it on there in the center.
| | 02:24 | I can drag this around and I'm going to
go ahead and add a couple more dimensions.
| | 02:29 | Click there, click there and the third click is
going to be where you want to place the dimension.
| | 02:33 | Type in 30 and go over here and click again.
| | 02:36 | This time I'm going to type in 18, click OK.
| | 02:40 | There's our fully-
defined Center Point Rectangle.
| | 02:42 | I'm going to highlight this.
| | 02:43 | One other thing as far as highlighting is if
I highlight from the upper left-hand corner
| | 02:47 | and drag it onto the right-hand corner,
what that does is it's a selective highlight.
| | 02:51 | See nothing is actually highlighted
because I haven't fully gone around that line.
| | 02:55 | As I drag a little further down, still nothing.
| | 02:59 | However, if I come from the bottom right to the upper
left, anything it touches will automatically highlight.
| | 03:04 | So it's a little option there as
far as how you want to highlight.
| | 03:07 | If I select everything it
automatically works. Let's get down.
| | 03:10 | The next one is 3 Points Corner Rectangle.
| | 03:12 | I'm going to start at the origin again, and by
the way, I don't need to start at the origin,
| | 03:16 | I'm just doing that because I always
want my designs to be origin-centric.
| | 03:20 | So I'm going to click at the origin.
This time I'm going to drag out a line.
| | 03:23 | It gives me that dimension and also
the angle that I'm pulling that out at.
| | 03:27 | Click here and then my third click is going
to define the width of the rectangle there.
| | 03:34 | And notice the
relationships that were added here.
| | 03:36 | So I've got a perpendicular.
I've got a parallel relationship.
| | 03:40 | Notice the 4 and 4 mean those are a pair.
| | 03:43 | I've also got another perpendicular down here and then a
coincident meaning that rectangle is locked on to origin.
| | 03:49 | If I didn't want it locked on the origin, I
can just click on that coincident, delete it,
| | 03:53 | and now I have the ability to drag that around
and move it around somewhere else if I wanted to.
| | 03:57 | That's the 3 Point Rectangle. Let's delete that.
| | 04:00 | The next one we're going to grab is the 3
Point Center Rectangle, which is very similar.
| | 04:06 | This time I'm going to click on the
origin again, drag out at the angle,
| | 04:09 | and this time it's very similar to the
Center Rectangle but this time it's at an angle.
| | 04:15 | And notice the relationships
that were added are different now.
| | 04:18 | I've got the ability to now spin
this, which we didn't have before.
| | 04:22 | Now if I want to define the angle this is at, I'm
going to add a construction line from the origin
| | 04:28 | just kind of out here and notice I'm adding
in it as a horizontal line, so it's defined.
| | 04:33 | Notice, it's horizontal.
| | 04:34 | Now I'm going to add a relationship
that says from that horizontal line to
| | 04:39 | some other line on the rectangle,
which I'm using that bottom line.
| | 04:42 | I can define that angle now. I'm
just going to type in 35 degrees.
| | 04:45 | It defines that rotation.
| | 04:47 | Now we're going to go and add a few
more dimensions to define that shape.
| | 04:51 | So I'm going to click on the far side here to
this side here and then place that dimension.
| | 04:55 | This time I'm going to type in 100 as far as
the length and the same thing on the width.
| | 05:01 | Click on this line, click on that
line, third click is me placing it,
| | 05:05 | 45 and there we go, fully
defined rectangle at an angle.
| | 05:09 | Now, if I wanted to change
any one of these dimensions,
| | 05:12 | I would just double-click on it, type in a
new dimension and it automatically updates.
| | 05:16 | Same thing with the length.
| | 05:17 | Change this to 80, click OK and there it is.
| | 05:21 | Select all of that, delete, and we're
going to jump onto our last Parallelogram.
| | 05:26 | I'm going to start at the
origin again, drag out a line.
| | 05:30 | This time, I have the option to change
the angle and the height. Place it here.
| | 05:34 | Now I'm going to define this
angle here between these two lines.
| | 05:38 | So I'm going to click on
the first line, go over here,
| | 05:41 | click on the second line
and place the dimension.
| | 05:44 | I'm going to type in 50 degrees for that one.
| | 05:46 | Now I'm going to define a couple of
dimensions and notice I've got a few options here.
| | 05:51 | I'm going to dimension
either from the top to the bottom,
| | 05:53 | which would be a hard dimension, or I
could dimension from aligned at an angle.
| | 05:59 | As I move that dimension around,
it keeps following me around.
| | 06:03 | So either I have the direct height here or if I go
aligned with this edge, it'll give me that dimension.
| | 06:09 | So depending where you place these dimensions,
it will define the shape a little bit better.
| | 06:13 | And then same thing over here, I've
got still one degree of freedom here.
| | 06:17 | If I click on this bottom line here, I get 77,
but if I didn't want that type of dimension,
| | 06:23 | I could dimension, for instance, from
this point here to that point there.
| | 06:27 | Now, this is an option that if I have it here,
it's going to give me this overall length.
| | 06:31 | However, if I start moving it this way,
now I've got the kind of unaligned dimension,
| | 06:36 | or if I get over here, I'm going to give a
height again and I've got a lot of different options
| | 06:38 | of where I'm going to place that
dimension to define the length of that part.
| | 06:41 | I'm going to type in 100 and click OK.
| | 06:44 | We've got a fully defined part.
| | 06:46 | Rectangles can be
created in many different ways.
| | 06:48 | However, any way you create them, they're
still just four lines and several relationships.
| | 06:53 | Use them to save time and learn
from the way the SolidWorks applies
| | 06:57 | those relationships to
use in your other designs.
| | Collapse this transcript |
| Creating arcs in a sketch| 00:00 | Arcs are a segment of a circle and
can be created in much the same way.
| | 00:04 | Arcs do need more information than a
circle, because you need to define where
| | 00:08 | the beginning and ending points are, in
addition to the center location and the radius.
| | 00:12 | Let's jump into SolidWorks and create some arcs.
| | 00:16 | The Arc command is directly below the
Circle command, and if I click on the
| | 00:19 | arrow next to the Arc icon I
get the three options here;
| | 00:22 | I've got the Centerpoint Arc,
the Tangent Arc, and the 3 Point.
| | 00:25 | So let's just go through those in order.
| | 00:26 | So Centerpoint Arc is very
similar to a Centerpoint Circle.
| | 00:30 | I'm just going to click on
the centerpoint to start off.
| | 00:33 | Define the radius of that
circle or the defining circle,
| | 00:37 | and then wherever I start my click at
is where I'm going to start that arc at.
| | 00:40 | Notice I can drag this
around to define that shape.
| | 00:44 | So as I move around that circle or move
on the other direction, I get that shape,
| | 00:49 | and it has a couple of helper lines that will
pop-up and snap to the horizontal for instance,
| | 00:53 | or something else like that,
depending on how we want to define it.
| | 00:56 | So I'm just going to go
over here and click here.
| | 00:58 | The problem with an arc is it's
just floating out in space, right?
| | 01:01 | I can grab these endpoints, I
can drag it around a little bit.
| | 01:04 | So I don't really have a good way
to define everything about this arc.
| | 01:08 | So if I put a Dimension on here, I
know the radius of it, okay, that's fine.
| | 01:11 | So I can type in a 75, for instance, great.
| | 01:15 | But still the endpoints
are just floating around.
| | 01:17 | We know it's tied to the
centerpoint, which is great.
| | 01:19 | Those are the two pieces of
information that we'd define a circle with.
| | 01:22 | Now we need to go ahead and tie these ends in.
| | 01:24 | So my favorite way to do this
would be to use some centerlines.
| | 01:27 | So I'm going to go from the origin out to one
of those arcs, double-click, and start one more.
| | 01:33 | Now I've get kind of a
definitive attachment to the centerpoint.
| | 01:37 | And now I can put some dimensioning in
here, so I'll dimension from line to line
| | 01:41 | and I can define how many
degrees I want that arc to go through.
| | 01:44 | For instance, I'm going to
type in 130 and there it is.
| | 01:47 | But notice they're still undefined,
or I can still spin this thing around.
| | 01:51 | So I could say something like
this line I want to be Horizontal,
| | 01:54 | so I'm using those
relationships again to define it.
| | 01:57 | Now I look at everything here,
it's a fully-defined sketch,
| | 02:00 | everything has got a
number or dimension or angle.
| | 02:02 | So if we want to change any one of these things,
we can obviously just type in a new number.
| | 02:07 | It's going to change, but it's
fully- defined at this point. Okay.
| | 02:09 | Let's delete that and jump on to
our next arc. This is the Tangent Arc.
| | 02:15 | Now Tangent Arc is a special condition
that needs to start from a straight line.
| | 02:20 | It needs to be tangent to something.
| | 02:21 | So before I actually can get into
this command, I'm going to hit Esc,
| | 02:24 | get out of that, and I'm going to create a line.
| | 02:26 | So I can either use our
regular line or a Centerline,
| | 02:29 | so I'm going to use the Centerline here,
start from the origin, drag it out,
| | 02:32 | and I once have the line defined, now I
can use that Tangent Arc to start from that,
| | 02:37 | and now it's tangent to that
line segment, so I can drag it out,
| | 02:41 | move it around any way I
want, get to the point I like.
| | 02:44 | Notice it gives me some helper lines as far as
the angle and the radius, drop that on there.
| | 02:49 | And notice I stay in that
command, depending on where I go.
| | 02:52 | And I can continue with that
Tangent Arc from another arc.
| | 02:55 | So if I click on the endpoint here, I can
still be tangent to that first arc and continue on,
| | 03:00 | but the thing about Tangent Arcs is that we always need
to start from some other type of item to be tangent to.
| | 03:06 | I can define this a little better by
giving it a dimension, as far as a radius.
| | 03:11 | I'll type in 100 inches here, and now
we're going to need to some more information.
| | 03:16 | We need to have a
dimension here, I'll type in 140.
| | 03:18 | Now we have a fully-defined
arc besides that endpoint, right?
| | 03:21 | So we don't know how far this is
going up here, so we need to define that.
| | 03:26 | And I'm going to use that same method I
used before, just using the centerline,
| | 03:30 | snapping it to that endpoint, now I have
the ability to kind of drag that around.
| | 03:34 | Now, I can define this in
multiple different ways.
| | 03:37 | I can add a Relationship or a Horizontal,
or I can it give it an Angle if I wanted to.
| | 03:42 | So say like 20 degrees from the Horizontal, and
that'll define that arc for us, that's a Tangent Arc.
| | 03:47 | Okay, let's delete that.
| | 03:49 | The last arc here is a 3
Point Arc, quite simple.
| | 03:54 | We're going to pick on the centerpoint again,
| | 03:57 | and my second place is going to be what I
want to snap to, so I'm going to snap up here.
| | 04:01 | Notice it's just giving me a
length at this point in time.
| | 04:04 | Then my third click is defining
how much that's going to arc out,
| | 04:07 | and now I'm getting some more helper
lines as far as the angle that I'm at
| | 04:10 | and the radius that I'm at as far as that shape.
| | 04:12 | So that third placement
is going to drop it here.
| | 04:16 | Now, I can define this a lot of different ways.
| | 04:17 | I can move the arc itself or the endpoint or
either one of the endpoints or the centerpoint.
| | 04:23 | So we have a lot of control with this one.
| | 04:25 | But it's also a lot of degrees of freedom, and I
need to tie down to make this a fully-defined sketch.
| | 04:30 | So to get that point, I
need to get the Centerline.
| | 04:33 | There's a lot of different ways to do
this, I'm just doing one of the ways.
| | 04:36 | I'm just going to click on the origin
and I'm going to snap to the endpoint here.
| | 04:39 | I'm going to throw a dimension on
there, so I'm going to type in say 380.
| | 04:44 | I'm just going to define
the length of that it least.
| | 04:46 | Now, I still have the option to move
this arc around, so I need to add a radius.
| | 04:50 | So I'm going to say 280 on that one.
| | 04:52 | Now, it's got its width across and its radius defined,
but we need to still define as far as maybe an angle.
| | 05:01 | So to do that we can just grab just
another Centerline and just use this as a line,
| | 05:06 | that's a horizontal line here to
place a dimension between the two.
| | 05:10 | Let's give it 25 degrees, for instance.
| | 05:13 | Now that defines the angle that it's at, the
radius and the width between the two points.
| | 05:19 | Now, if I didn't want that one here, I could
have defined this as from this point to this point
| | 05:23 | and a Vertical Relationship as well,
say like 340, and that would work as well.
| | 05:27 | So a lot of different ways to define these shapes, we
just need to make sure we're tying those two edges together.
| | 05:32 | I'm going to do one more last thing
here as far as a way to lay things out.
| | 05:37 | So I can actually use circles.
| | 05:38 | I'm going to start with a circle here
and I'm going to start with a circle here.
| | 05:41 | I'm going to make these circles touch.
| | 05:44 | So I'm going to say this circle and that circle,
| | 05:49 | and I'm going to add a Tangent
Relationship where they touch.
| | 05:52 | So I can actually use these as helpers though.
| | 05:54 | I select both of those, I'm going to
turn these into For construction geometry,
| | 05:58 | and then I can actually
place some arcs on those.
| | 06:02 | I can say from this part of that circle
here to this part of that circle here.
| | 06:06 | I'm using those construction circles as
kind of my guides for creating my arcs
| | 06:12 | and the construction circles will not be used.
| | 06:15 | I'm only going to be using that arc right there.
| | 06:17 | I'll do a couple more just to illustrate it.
| | 06:19 | So I'll click on this point here
and I'll click on that point there,
| | 06:23 | and then I'll snap to that circle diameter,
so that I can use these as a placement
| | 06:28 | or a starting point for the
other creation of geometry.
| | 06:32 | I'll start with that guy, Tangent Arc here,
and then I can snap to this point here
| | 06:35 | and possibly make this arc here, hold down Ctrl to
that arc there, and make that Tangent Arc as well.
| | 06:42 | So now that's going to flow into here.
| | 06:44 | Now let's add one more 3 Point Arc to go and
connect these two together and then snap to that.
| | 06:50 | So now I have a nice guide curve
just dependent upon these two circles.
| | 06:55 | If I go ahead and I define some sizes here
of like 240 for this one, 200 for that one,
| | 07:02 | and we need one more thing that's going to tie
these together as far as where the location is,
| | 07:07 | so I'm going to use my friendly
construction geometry in two more dimensions here.
| | 07:13 | So on this line here 200 and this line here.
| | 07:17 | Uh-oh, this is what we
don't want to have, right?
| | 07:19 | So if we said we have a dimension,
we're saying we're having conflicting sizes,
| | 07:23 | that's actually already been defined, because we gave
it a Horizontal, and so therefore we're fully-defined.
| | 07:29 | We used these two construction circles
to actually lay out a series of arcs.
| | 07:33 | We used 3 Point Arcs and one
Tangent Arc to lay that out.
| | 07:36 | Arcs are helpful for creating smooth
flowing shapes and appealing aesthetics.
| | 07:40 | They are just segments of a circle
and sometimes starting with a circle
| | 07:43 | is a good way to define
location for completing arcs.
| | Collapse this transcript |
| Drawing splines in a sketch| 00:00 | Splines are the ultimate free-form curve tool.
| | 00:03 | Smooth flowing shape and
wild curves are the result.
| | 00:07 | However, be careful. Splines are
very difficult to relay on drawings
| | 00:12 | and manufacturing is more of an issue.
| | 00:13 | Sometimes the best choice is to use a
spline as a layout sketch for traditional arcs
| | 00:18 | to get the best of both worlds.
| | 00:20 | Let's jump into
SolidWorks and create some splines.
| | 00:23 | The Spline Tool here, click on that.
| | 00:24 | Now splines are created
through a series of points.
| | 00:27 | So if I click on the origin, for
instance, my very next point is going to be
| | 00:31 | where my curve is going to bend,
so I'm going to click here.
| | 00:35 | Notice as I now control the
endpoint of that, and if I'm close or far,
| | 00:40 | depending on how far away I am,
that shape is going to change,
| | 00:44 | so it's going to be defined
through a series of points.
| | 00:46 | Generally, my finding is that, if you
put less points, it makes it better.
| | 00:50 | So I'm going to put a point down here, and
notice as I change that, the entire shape changes.
| | 00:56 | As I drag that through, it's
controlling not only the point that I'm dragging,
| | 01:01 | but also the rest of the curve and that shape.
| | 01:04 | And then further away from it, it does a lot
of different motion changes and stuff like that.
| | 01:09 | As I get closer to it, I make
a more sharp curve at the end,
| | 01:12 | and one more click down here.
| | 01:13 | It's going to continue that
way as I click and drag points.
| | 01:17 | As soon as I hit Esc, it stops
that last segment of the line.
| | 01:20 | Now I can click on any one of
these points to define that curve.
| | 01:24 | So I can click on this endpoint
here and drag it around if I wanted to,
| | 01:27 | same thing over here, you can click on that
point and drag that around, drag this one around.
| | 01:32 | Now notice as I'm dragging these around, I get
these couple of arrows that kind of pop-up right here.
| | 01:35 | Now these are control handles, so I
can drag these out a little further,
| | 01:41 | I can push them in, I can twist,
change the shape using these controls,
| | 01:46 | and I can pull them in and
out or go to the other side.
| | 01:48 | Notice I have one of those at
each one of my starting points,
| | 01:53 | so this is a direction vector,
and how much it influences.
| | 01:57 | So the longer that arrow is, the
more influence it has on that curve;
| | 01:59 | the shorter it is, the less, and the same thing
with the angle or the vector that's starting it.
| | 02:04 | So that's the control points.
| | 02:07 | If I select this entire spline,
under the Tools Palette, up here,
| | 02:12 | I can go down and I have a whole bunch of
tools that I can use to control that spline.
| | 02:16 | So I can add Tangency, I can
have Curvature, I can insert Points,
| | 02:21 | I can Simplify, a lot of
times you have too many points.
| | 02:24 | I can actually get rid of some of those
points and make it a little bit smoother curve.
| | 02:27 | I can show the Curves, I
can show a Control Polygon.
| | 02:30 | I'm not going to go through all of these
. A couple of them I am going to show.
| | 02:33 | I'm going to show this Polygon.
| | 02:34 | That's the shape that now I can drag
this around more as like a Polygonal shape
| | 02:38 | that I can grab these control points here and move
these things around to define it inside of those.
| | 02:43 | And the same thing, now these vectors are
kind of attached at the beginning and end
| | 02:48 | along that polygon and through these points,
so each one of those points that we have there.
| | 02:53 | Same thing if I want to go select that
line, and I can go to the Spline Tools,
| | 02:57 | and go in here and I can insert another point.
| | 03:00 | So if I wanted a point right here, for
instance, now I have a little bit more control
| | 03:03 | to drag that part of that spline around.
| | 03:07 | If I take this spline and I try to go manufacture
a part from this or use this out to dimension it,
| | 03:13 | you can think about it, it would be
very difficult to define where this,
| | 03:17 | and I could try to put some dimensions on here.
| | 03:19 | I can dimension maybe from this
point to that point, which would be fine.
| | 03:22 | But how do I define the shape out here,
how do I define this section of that curve?
| | 03:28 | Those are going to be very difficult
to relay on a drawing to anybody else.
| | 03:32 | And same thing, if it goes out to
manufacturing, you're trying to machine this part
| | 03:36 | or bend this part or something like that,
that's going to be very difficult to relay.
| | 03:39 | So the last thing I'm going to show
here is an overlay of regular arcs.
| | 03:43 | I'm going to place this
originally as a construction.
| | 03:47 | It's going to be our Helper Spline.
| | 03:49 | So I'm going to take a 3 Point Arc now.
| | 03:52 | I'm going to start here, and I'm
just going to kind of drag this out.
| | 03:55 | Then I'm going to use my little 3
Point Arc to define that shape a little bit
| | 03:58 | or get close to that shape if I wanted to.
| | 04:01 | If this is not the right shape, which
looks like it's not really right here,
| | 04:04 | I can actually start with a line here, start with a
line, and then we'll use more of like a Tangent Arc.
| | 04:11 | So here's my arc and I'm going
to place that along that line.
| | 04:14 | Then I can continue placing those arcs along
that spline and then use it kind of as a helper.
| | 04:21 | Now, it's not going to be exactly the
same, but we can make a bunch of short arcs
| | 04:26 | that are going to be very,
very similar to that spline shape.
| | 04:30 | As you can see, I've got kind of a
curve here, and then I can go in here
| | 04:34 | and fine-tune those a little bit, and I can drag
them closer to the line or I do like a best fit.
| | 04:39 | So you're not going to get
exactly the same shape as a spline,
| | 04:41 | but depending on how much
time you want to spend on it,
| | 04:43 | and how you want to move those
little curves around to define that shape,
| | 04:46 | you can get a pretty nice shape to define
your spline, and then each one of those arcs
| | 04:51 | can be defined with a radius, a
centerpoint, and a starting and endpoint.
| | 04:56 | Splines have many great features and are
wonderful for smooth curves and complex shapes.
| | 05:00 | However, use them with caution.
| | 05:02 | Dimensioning, defining, and building parts that
were designed with splines can be very complicated.
| | Collapse this transcript |
| Sketching polygons| 00:00 | Polygons are any shape with three or more sides.
| | 00:03 | The Polygon tool allows you to choose the quantity
of sides and the method used to define the shape.
| | 00:09 | Let's jump into SolidWorks
and get the Polygon tool.
| | 00:12 | The Polygon tool is directly below the Arc tool.
| | 00:15 | As soon as I turn at tool on, I get an
option over here on the left-hand side.
| | 00:19 | First off, I can create this just
for construction if I wanted to.
| | 00:22 | How many sides do I want on my
shape, and do I want an inscribed or
| | 00:26 | circumscribed circle to define that
shape, which we'll cover in a second,
| | 00:29 | and then my XY location of the center point,
the diameter of that circle, and the angle.
| | 00:34 | I'm just going to start
right here at the origin.
| | 00:37 | Click once, drag it out.
| | 00:38 | Notice I get the diameter of the inscribed circle
and I get the angle that it's going to be built at.
| | 00:43 | So I'm going to drag it right
over here, I'm going to drop it.
| | 00:47 | Notice, SolidWorks adds a lot of relationship
directly to that shape as soon as I create it,
| | 00:52 | but it doesn't define the angle or the size.
| | 00:54 | If I want to do that, I need to add may be
a centerline here or a construction line,
| | 00:59 | and I'm going to snap that endpoint, we'll
then control to the midpoint of this line,
| | 01:05 | which then defines that shape so it can't spin.
| | 01:07 | Now I can just still make it bigger or smaller.
| | 01:09 | Now I need to define that shape.
| | 01:11 | I can do it two ways; one I can
define the size of the circle,
| | 01:14 | or I can just dimension from
any one of these points or faces.
| | 01:18 | So I'm just going to define from
this side to that side, and type in 8.0.
| | 01:24 | Now I've got a fully-defined octagon that
has all the relationships that are pre-added.
| | 01:29 | Now if I wanted to create that same shape, but
using just line segments, it's quite a bit of work.
| | 01:33 | I need to make them all the same
length, or I have to define the angles,
| | 01:36 | or I have to do some type of a
patterning feature like they've done here.
| | 01:40 | It's going to be a lot of work.
| | 01:41 | So the Polygon feature
does save us a lot of time.
| | 01:43 | Let's go ahead and delete
that and create a couple more.
| | 01:47 | Jump back into Polygon tool. This
time I'm going to try not an eight-sided,
| | 01:50 | but let's do a six-sided and this time,
we're going to do a circumscribed circle
| | 01:55 | and I'm just going to place it out here.
| | 01:56 | As soon as I place it, notice, I still
have the control over here on the left,
| | 02:01 | so I can change its XY
locations, its diameter, its angle.
| | 02:06 | I have the ability to move all these around
while I'm still in that Edit Polygon mode.
| | 02:14 | Notice now we have a circumscribed circle.
| | 02:18 | We have this circle in the
outside that's defining that shape.
| | 02:21 | So if I now place that circle,
I can drag it around outside,
| | 02:24 | and I can also define that
size of that outside circle.
| | 02:29 | Just type in 8.0, change that around,
and I can drag this thing around now.
| | 02:33 | I can spin it around and if I
wanted to place like a relationship,
| | 02:37 | maybe fix that center point, I can spin
that around somewhere I want it to go,
| | 02:40 | or I could make some
dimensions that would define this shape.
| | 02:43 | Just like all things in SolidWorks, we
always want to make it not just floating in space;
| | 02:47 | we want to tie it into something; where is it?
| | 02:50 | So I'm going to use that Centerline.
| | 02:52 | I'm going to come out here and maybe use
some rectangular coordinates to that point.
| | 02:56 | So now I have two dimensions
that I can put in there to define
| | 03:00 | how far it is from the center point
or the origin and how high above it.
| | 03:06 | Type in a couple of those and the last
thing we need to do is define its rotation.
| | 03:11 | So we can do that in multiple ways and one of the
easiest ways, which would be like a bottom edge here,
| | 03:15 | I can say this is horizontal and
notice now everything turns black.
| | 03:19 | It's fully-defined and
notice exactly where it is.
| | 03:21 | I can pull some of these dimensions
around just to make it a little bit more clear
| | 03:24 | where we're at and of course, I can always
change any of these things to move that shape around.
| | 03:30 | Now if I had this shape fully-defined
and I wanted to actually change that shape,
| | 03:35 | I can click on it or actually right-click
and I can come down here to Edit Polygon.
| | 03:39 | As soon as I do that, I could have the
ability to change how many sides are on that shape,
| | 03:44 | change it to a bunch of different
things, maybe a triangle this time.
| | 03:47 | Click OK and now I have a
triangle with all the same dimensions,
| | 03:50 | so I can go back and edit and
modify those things as needed.
| | 03:55 | The Polygon tool is easy to use and saves a lot of
time over creating shapes with just the Line command.
| | 04:01 | It also allows the user to later
edit the polygon without changing
| | 04:05 | and re-adding relationships and/or dimensions.
| | Collapse this transcript |
|
|
5. Sketch-Editing ToolsTrimming and extending portions of a sketch| 00:00 | The Trim and Extend tools allow the creation of complex
shapes in building geometry that combines with other shapes.
| | 00:07 | The Trim tool has various
modes that it can operate it.
| | 00:10 | The most powerful of those
is the Power Trim Command.
| | 00:13 | This should be your Go-To tool
for modifying sketch elements.
| | 00:16 | Let's jump over to SolidWorks and
start up the Trim command. Trim is here.
| | 00:20 | If I click on the dropdown arrow here, I also have
the option to get Extend Entities. Click on Trim.
| | 00:26 | Power Trim is my favorite. But
we're going to come back to that one.
| | 00:29 | So we're going to start here
with Corner Trim. Select that one.
| | 00:32 | Corner Trim is going to keep the two items you
click on, and trim off the other ones in that corner.
| | 00:37 | So this time, I'm going to click,
just a regular left mouse click.
| | 00:40 | Selecting the first item, you then come
over here and select this second item,
| | 00:44 | and notice it's going to trim off
those two legs that were hanging off.
| | 00:49 | Continue down here, do it one more time.
| | 00:50 | Click on the first line, click on
the second line and it's going to
| | 00:53 | trim off entities that are hanging beyond that.
| | 00:56 | Trim Away Inside; I'm going to pick the
two bounds that we're going to trim too.
| | 01:00 | So I'm going to pick this
side here, that side there,
| | 01:04 | and then all you do is just go and
click on the items we want to remove.
| | 01:06 | So I'm going to click here, here and here.
| | 01:08 | Notice as I'm doing that
it's adding those relationships,
| | 01:12 | that's making this point coincident to that one.
| | 01:14 | Trim Away Outside is very similar.
I'm going to pick the two bounds,
| | 01:18 | this one and this one, and now we're
going to start trimming these outside lines,
| | 01:23 | and notice as I trim one, it
trims the other side as well.
| | 01:30 | Then Trim To Closest is going to trim
away legs that kind of extend past something.
| | 01:34 | So I have this line here that's cutting through
that circle and I just want to trim that away.
| | 01:39 | So I just cut that and slice it off.
| | 01:41 | Same thing over here, I might
want to cut off any dangling lines or
| | 01:44 | something like that that might be going
past your part, it's a great way to do that.
| | 01:48 | Then my favorite one is a
Power Trim, click on that.
| | 01:50 | Now Power Trim is a little bit harder to
understand how actually it works, but it's quite powerful.
| | 01:54 | Power Trim starts with the line.
| | 01:55 | So we don't actually want to start on top
of any one of these other lines or entities.
| | 02:00 | We want to kind of start off here in the
space where there is just pure white space.
| | 02:03 | So I'm going to start down here.
| | 02:04 | I'm going to start drawing, and notice as I start drawing,
it creates a kind of little sketch line of where I'm drawing.
| | 02:09 | Anything that little sketch line
actually cuts across, it's going to trim to,
| | 02:14 | so watch I'm going to trim this
little first entity here and trims it away.
| | 02:16 | Come over here, it's going
to trim off the end there.
| | 02:20 | Come up here, go around I can trim
off the top, trim off the bottom.
| | 02:24 | I come through here, I can trim these out.
| | 02:26 | As long as I continue to hold that left
mouse button down, I can continue to trim
| | 02:29 | and you can see the path of where
I've gone through to trim out entities.
| | 02:33 | As soon as I'll let go, it
hides, that trim path I was using,
| | 02:36 | and all those entities have been trimmed.
| | 02:37 | At the Top here I'm going to
go back to Extend Entities.
| | 02:40 | Now Extend takes a line and continues it
on to the next thing that's going to hit.
| | 02:46 | So if there's nothing for it to
hit, it doesn't run the command.
| | 02:48 | Let's click on this line here. As I
go over it gives me a little preview.
| | 02:53 | If I extended that line,
what would it actually do?
| | 02:54 | It would extend it to the next
thing it's going to run into.
| | 02:57 | Same thing over here, it's going to extend that
line out through over here where it would hit.
| | 03:01 | Click on over here, you can extend
that one out, click on anyone of these and
| | 03:03 | you can see what's going to
happen, when I extend it out.
| | 03:06 | It even works on arcs. So we click on
here, it's going to continue that arc down.
| | 03:09 | So we'll just click here,
extend it out, now it touches here.
| | 03:12 | Click on this one, it extends it out over there; click
on this one, it extends it out over here, very similar.
| | 03:16 | Same thing over here, and we can
keep doing this many different ways
| | 03:19 | to connect to these lines
together to build a part.
| | 03:22 | The Trim tool is an essential tool for
building complex shapes in the sketch environment.
| | 03:27 | By leveraging the Trim and Extend commands,
| | 03:39 | we can rapidly modify existing geometry
and take your sketches to the next level.
| | Collapse this transcript |
| Creating offset geometry| 00:00 | By offsetting geometry, we
can save a huge amount of time
| | 00:03 | and have the ability to create slots and
rectangular holes, with a simple line sketch.
| | 00:09 | In SolidWorks, I have a rectangular box on the
screen and if we want to draw another box around that
| | 00:14 | for instance, we could go ahead and use the
Rectangle command and draw it out and dimension it.
| | 00:20 | We actually have a much easier way to do that.
| | 00:22 | I just select anyone of the entities or
the line segments that make up that shape.
| | 00:26 | Click up here and I'm going to use
this thing called the Offset Entities.
| | 00:30 | What that's going to do is, it's going to take that
line segment, and it gives me a couple of previews.
| | 00:34 | This is a two-way, so
I'm going to turn that off.
| | 00:36 | This is just a one-way and you
notice, if I type in that number here,
| | 00:41 | I can adjust how far I
want to offset that geometry.
| | 00:45 | Now I can use one line segments or all the line
segments and that's where you can choose it here; Select Chain.
| | 00:51 | So if I only chose just that one,
I can also change the Direction,
| | 00:54 | so I can move it either
inside or outside of the box.
| | 00:56 | I could select the entire
chain or do the entire box.
| | 00:59 | I can choose Bi-directional to bring it inside
as well, so you've got a lot of options here.
| | 01:03 | So I'm just going to choose the one side,
I'm going to type in 0.4 and click OK.
| | 01:07 | Notice it creates a new box. It made
the base construction if I want it to,
| | 01:11 | that's one of the options that we had there.
| | 01:13 | Then it gives me this dimension here.
| | 01:15 | So if I change that dimension,
it adjusts the entire box.
| | 01:20 | So when I change it to 0.1, it
changes that dimension all the way round.
| | 01:23 | So it's using this base
geometry to create a new box.
| | 01:27 | Now we can do this in a lot of different ways.
| | 01:29 | We can do it with circles as well,
I can create like a base circle.
| | 01:32 | I can go in here to Offset
Geometry, it creates an offset.
| | 01:36 | Type in, do we want a base
construction this time? No.
| | 01:39 | Then I've got the two circles and I can just control
with that one dimension here, it makes it really handy.
| | 01:44 | Now if we wanted to create a slot for
instance, I'm going to delete these two.
| | 01:48 | I'm going to jump just right over
here to that Centerline command.
| | 01:52 | I'm going to drop a
centerline here just by clicking.
| | 01:55 | Then I'm going to add one relation
to it saying the center point of that
| | 01:59 | is that midpoint, there it is.
| | 02:00 | So now as I drag this up
and down, I can control it.
| | 02:04 | Now we're going to actually
remake a part we made it earlier,
| | 02:07 | which is a link part, and
so we're going to do that.
| | 02:09 | Instead of creating a circle on the top or a
circle on the bottom, and connecting the two lines,
| | 02:13 | I can actually use the
Offset command to do that.
| | 02:15 | So I'm going to select that line,
and I'm going to click on Offset.
| | 02:17 | So notice it gives me
just a way offset right now.
| | 02:20 | I can say it's Bi-directional,
now it's going to both ways.
| | 02:22 | Notice I have this Cap
ends thing here checked on.
| | 02:25 | So I can either cap them
with Arcs or Lines, my choice.
| | 02:28 | So I'm going to use the Arcs, and then I'm
going to give it a dimension here of 1.0.
| | 02:33 | So now that gives us that
nice shape that we had before.
| | 02:37 | Instead of creating a circle,
a circle and two line segments,
| | 02:40 | and then trimming them out,
I got everything in one shot.
| | 02:42 | I'm going to add two circles here, one, two.
| | 02:48 | Add a relationship between the two by Holding
down Ctrl, selecting the pair, say they're Equal.
| | 02:53 | Add a couple of dimensions. I think we
had a 0.75 in this one from before, 0.75.
| | 02:58 | Notice they both changed because they're equal.
| | 03:00 | Add a dimension here, which is 4 inches, 4.0.
| | 03:02 | We have fully-defined sketch
with only three dimensions on it,
| | 03:06 | which is exactly the same part we
did before but quite a bit easier.
| | 03:10 | The Offset command is a quick way to use
existing geometry to create secondary sketch entities.
| | 03:15 | This is a perfect choice for quick
slots and basic clearance sketches.
| | Collapse this transcript |
| Moving, copying, and rotating elements| 00:01 | SolidWorks provides nice set of
tools to deal with modifying sketches.
| | 00:04 | We can select the whole sketch so we can move,
copy to a new sketch, or rotate around a point.
| | 00:10 | These tools are very handy, if you're using imported
sketch elements like a block or doing sketch-wide changes.
| | 00:16 | In the SolidWorks window, we've
got a toolbar called Move Entities,
| | 00:21 | that allows me to select the entire object,
get that window, pop it back out here,
| | 00:27 | and then I'm going to say Start
Point, I'm going to start from here,
| | 00:31 | and then it just attached to my Tool tip now
and I can drag this around anywhere I want.
| | 00:35 | So maybe I just want to snap that
on to the origin, and there it goes.
| | 00:38 | Now notice when I do snap onto the origin,
it actually doesn't add a relationship.
| | 00:43 | So we need to go and do that ourselves
if we want that to be locked on here.
| | 00:45 | You might say, well, why would I want to use the Move
Entities versus just dragging this thing around on my own?
| | 00:51 | The reason for that is it
treats it as a one complete object.
| | 00:55 | So if I grab something, it
actually changes the object shape or size.
| | 00:59 | If I just want to move this thing as a whole,
that's where you might want to use Move Entities Command.
| | 01:06 | The next one there is Copy Entities. So
I can just select everything I have here.
| | 01:09 | Start Point must be there and then copy is going
to take exact copy of that and I can drag it around.
| | 01:14 | And once again it's attached to my tool
tip, so wherever my point of my cursor is
| | 01:19 | is where I'm going that one corner of that part.
| | 01:22 | So I can copy those and I can
continue to do that if I wanted to.
| | 01:25 | I can select both of those items for instance.
| | 01:27 | Go up here and do Copy Entities.
| | 01:30 | Take a point from where I want it.
| | 01:31 | Drag it from that, and I'm
copying two at the same time.
| | 01:33 | So you can do that multiple times.
| | 01:35 | I'm going to go ahead and undo that a
couple of times, back to my original one.
| | 01:39 | Now I'm going to go ahead
down here to Rotate Entities.
| | 01:42 | So with Rotate, I'm going to do the same thing.
| | 01:44 | I'll select everything there,
and then a Point of Rotation.
| | 01:47 | So I'm going to pick this upper corner here.
| | 01:50 | And then what I can do is I can drag this
around or I click on the Angles to adjust that.
| | 01:56 | So if I'm happy with that,
I click Ok and there it is.
| | 01:59 | Once again it created all those entities
and treated them all as one whole there.
| | 02:03 | Let's go back and then Scale Entities,
select everything by moving over it.
| | 02:10 | Scale about a point.
| | 02:11 | I'll pick this lower corner here and
then notice it just scales that shape.
| | 02:14 | For now I'm giving it a 0.5 Scale Factor.
| | 02:17 | I can continue to just bump that
up and make it twice the size,
| | 02:19 | or twice as small
depending on what you want to do.
| | 02:21 | You could even copy it. So if I want to
copy it, it's going to keep the original
| | 02:24 | and make a scale copy of
this. So your choice there.
| | 02:27 | Once you're done say OK
and there's your new shape.
| | 02:30 | I'm going to go back again just using Undo
command and the last one here is Stretch Entities.
| | 02:36 | What that allows us to do is take a
portion of the thing, and kind of stretch it out.
| | 02:39 | So by doing that I'm going
select some Entities to stretch.
| | 02:42 | I'm going to pick this one,
that one and that one.
| | 02:45 | Stretch it to about. I'm
going to say this point here.
| | 02:47 | If I hold down that left mouse button,
I can drag this around and kind of
| | 02:52 | change the shape by
stretching it out if I wanted to.
| | 02:55 | As soon as I'm happy with this I will just click
again and let go and it just stretches that out.
| | 02:59 | These tools focus on working with an
existing sketch and making Sketch-wide changes.
| | 03:04 | If modifying individual elements,
it's probably better to just work with
| | 03:08 | constraining relationships to
get the shape you're looking for.
| | Collapse this transcript |
| Erasing, undoing, and redoing actions| 00:00 | The all-powerful Eraser.
| | 00:02 | Sometimes it's better to start with a clean
sketch or to remove selections of the sketch.
| | 00:07 | We already know how to erase a single element,
by selecting the element and pressing Erase,
| | 00:13 | or selecting it from the
Feature Manager and hitting Erase.
| | 00:16 | However, what if we want
to select multiple entities?
| | 00:19 | We've two circles on the screen here.
| | 00:20 | We have couple of ways to do so.
| | 00:23 | I can select any one of these entities just by
clicking on it, hitting Delete and it's gone.
| | 00:27 | I'm going to bring that back by hitting Undo.
| | 00:31 | Or I can also click on that entity and then right-
click and click on Delete. That got rid of it as well.
| | 00:36 | Bring it back. Next what if I want
to select these two entities together?
| | 00:41 | What if I have more than two? What
if I have two hundred or two thousand?
| | 00:45 | I could select each one, hold on the Ctrl and
select the next one, and multiple select that way.
| | 00:50 | But if we have several hundred or more items
to do, that's not going to be very feasible.
| | 00:55 | So we can use the Window select,
and there are two ways to do that.
| | 00:58 | If I go from the upper left-hand
corner to the bottom right-hand corner,
| | 01:01 | everything I'm going to select
in there will be highlighted.
| | 01:05 | Notice the two objects turn to a light
blue color showing you're highlighted.
| | 01:08 | Then over here on the left-hand side, it
says the Select Entities are Arc3 and 4,
| | 01:12 | and we have some relations that we
could add to those if we wanted to.
| | 01:15 | If I wanted to just select one of these items though, I
can mouse over from the left to right over the first one,
| | 01:23 | and that highlights the object,
because it's fully contained by that.
| | 01:25 | However, if wanted to select anything that touches my box, I
can go from the lower right corner to the upper left corner.
| | 01:34 | That would go around
those and it would select it.
| | 01:36 | Notice they both are selected even though I
only caught that bottom corner of the top circle.
| | 01:41 | So that changes the way
the selection property works.
| | 01:44 | We also have a thing called a Selection
Filter and I can turn that tool palette on
| | 01:49 | by clicking anywhere up in the right
-hand corner, if I click on right,
| | 01:52 | go down here, and I'm going to grab a thing
called the Selection Filter, which is right there.
| | 02:01 | Notice that has turned on a toolbar I
have on the bottom of my screen here.
| | 02:05 | So if I have a lot of entities
that I'm looking to select or find,
| | 02:09 | I can Filter them out
using the Selection Filter.
| | 02:12 | So I can say only Vertices, only Lines
or Edges, only Faces, or only surfaces,
| | 02:17 | a lot of these things we don't have in here
quite yet but only axes or planes or points.
| | 02:22 | So you've got a lot of choices here.
| | 02:24 | But one of the thing happens to be Circles, or
Center marks. A lot of things we can select by.
| | 02:29 | So if we had a point here, I'm going to put a
bunch of points on the screen, for instance,
| | 02:36 | and I put the Selection Filter on.
| | 02:38 | I say here I'm just going to select Points,
and then I go ahead and I select things.
| | 02:43 | The Circles are not selected at all,
it's only the points that are selected.
| | 02:46 | So that's Selection Filter for you. Now Undo.
| | 02:49 | We want to undo what we did,
and get rid of those circles here.
| | 02:52 | I have the ability to undo things here.
| | 02:54 | I also can look here and I can go back in
time all the different things that I had.
| | 02:58 | So I can go back here and Undo all four of those points
at one shot by just going back four clicks on my mouse.
| | 03:05 | Also there's a limitation on the undo, so you
can only undo a certain amount of actions back.
| | 03:10 | So you can't take it all
way back to the beginning.
| | 03:13 | You've got a limit of a certain
amount that's feasible at least,
| | 03:15 | and if you exit the sketch it's going to
not allow you to go back into it to change it.
| | 03:20 | Getting back where we were, if I'm going to
turn that Selection Filter Off, to where I was.
| | 03:24 | If I exit that sketch, I also have the ability to work
with that sketch as a whole over here in the Feature Manager.
| | 03:29 | So if I didn't want that entire sketch
I could just click on it and hit Delete.
| | 03:31 | That's going to take off the entire sketch and I could
just operate on it as a whole in that same environment.
| | 03:37 | Sketching is the fundamental
building block in SolidWorks,
| | 03:40 | and removing sketch elements is almost as
useful as creating them in the first place.
| | 03:45 | Simple sketches are best and
multiple sketches across multiple features,
| | 03:49 | oftentimes make for a
design much easier to work with.
| | Collapse this transcript |
| Mirroring part of a sketch| 00:01 | Mirroring in the sketch
environment is very powerful.
| | 00:03 | However, you should try to limit sketch mirroring
to a second resort to mirroring actual features.
| | 00:09 | The Mirror command needs to know two things.
| | 00:12 | Number 1, what do you want to mirror?
| | 00:14 | Number 2, what line do you want
to mirror these entities around?
| | 00:18 | We start by making a centerline.
| | 00:19 | In SolidWorks, you can see I have
three centerlines already created
| | 00:23 | and I have a little triangle
that we're going to mirror around.
| | 00:26 | The Mirror command is
right up here; Mirror Entities.
| | 00:29 | As soon as I click on that,
it asks me two things.
| | 00:31 | Whenever I see a box like
this that's highlighted in blue,
| | 00:34 | it's asking me what are the
entities that I'd like to mirror?
| | 00:37 | I want to go ahead here and
select that entire triangle and
| | 00:40 | notice it says it breaks it
down by lines, so line 2, 3 and 4,
| | 00:44 | and then what do I want a mirror about?
| | 00:46 | You'll notice there's little
check mark here; it's the copy.
| | 00:48 | So I can either copy it
or just completely move it.
| | 00:51 | So Mirror about. I'm going to choose
this item here and notice it gives me
| | 00:56 | a mirrored kind of
representation of what's going to happen.
| | 00:58 | So if I say, ok, that item is now
going to be copied to that side,
| | 01:02 | if I turn this one off, this will no longer
be there, it'll now just be on left-hand side.
| | 01:07 | So let's try that, click
OK, and we have two items.
| | 01:10 | Now these are mirrored copies of each other.
| | 01:13 | So if I move one, the other one moves,
right there. They're mirrors of each other.
| | 01:18 | So anything I do to one, it's going to
always happen to the other one as a pair.
| | 01:22 | Let's make it a little more complicated this
time, let's do mirror again, click on Mirror.
| | 01:25 | What do we want to mirror?
| | 01:25 | I want to mirror these items here,
which is the original triangle we did.
| | 01:31 | I want a mirror about this;
I want to mirror over here.
| | 01:34 | It's going to drop that same triangle down
that here at around this axis versus that axis.
| | 01:40 | Click OK and same thing.
| | 01:43 | Now what's interesting about this is if I change
one they all change, because it's mirrored twice.
| | 01:48 | This item here is mirrored across this
way and this was mirrored again over here.
| | 01:52 | Let's make it really fun,
and let's Mirror one more time.
| | 01:55 | Mirror Entities, and this time I'm
going to choose all these entities here,
| | 02:00 | and this time I'm going to copy those or
mirror those around this centerline here.
| | 02:03 | It's going to drop all
these down here another time.
| | 02:07 | Click OK and now I have a pretty
complicated mirror situation here.
| | 02:11 | As I move one, they're all going to
move around, so you can really get yourself
| | 02:14 | a pretty complicated sketch going
on here using the Mirror command.
| | 02:17 | It's a very powerful command.
| | 02:18 | The problem is I generally try to
keep my sketches extremely simple
| | 02:22 | and do more of the mirroring in the
Feature Manager and the features themselves,
| | 02:27 | than making it very complicated sketch that
is then harder to deal with in the future.
| | 02:31 | But it is a very powerful command;
| | 02:32 | if you need to, it's
definitely available to use.
| | 02:35 | Like I said earlier, try to keep your
sketches simple and use feature mirrors as a first.
| | 02:40 | However, the Mirror command has some nice time
-saving benefits in the creation of sketches.
| | 02:46 |
| | Collapse this transcript |
| Creating repeating patterns in a sketch| 00:00 | Much like the Mirror command,
preference should to be given to using
| | 00:03 | Feature Level Patterning versus
using the Patterning tool in sketches.
| | 00:08 | However, the tools work much in the same way.
| | 00:11 | We have three main questions to answer.
| | 00:13 | Number one is, what do we want to pattern?
| | 00:16 | Number two is, which direction do we
want a pattern in and at what angle?
| | 00:20 | And number three is, if we want a pattern in a
secondary direction, which direction and at what angle?
| | 00:26 | Let's jump over into SolidWorks.
| | 00:29 | We've got a rectangle here and up here
we have a Linear Sketch Pattern tool.
| | 00:33 | We also have to dropdown with the Circular
Pattern, which we'll do in a second here.
| | 00:36 | So let's select Linear Sketch
Pattern, and predefined here,
| | 00:40 | I already have my X and Y
axes selected by SolidWorks.
| | 00:44 | So what I need it to go to is
at the bottom of the screen here,
| | 00:47 | I can click on the Entities to
Pattern link and select those items.
| | 00:50 | I'm going to select those four
sides of that rectangular shape there,
| | 00:55 | and then I'm going to jump
over here to the Spacing.
| | 00:57 | Right now it's only 0.1.
I'm going to change it to 2.0.
| | 01:00 | As soon as I do that it spaces this out, and then
I'm also going to give it a few more of these patterns.
| | 01:04 | So I'm going to do five this way.
| | 01:06 | I also have the ability to change the angle these are
patterning at, so I can keep changing this up and down.
| | 01:12 | Notice the Orientation of the boxes don't
change; just the patterning direction does.
| | 01:18 | If I want to go in another direction, notice
this is all grayed out at this point in time.
| | 01:22 | The only thing that is
not is it has a 1 in there.
| | 01:24 | As soon as I change that to a 2,
these all become real entry boxes here,
| | 01:29 | so I can go and change the
spacing between the two of those.
| | 01:31 | I can add a few more if wanted to.
| | 01:34 | And then I can also change the
angle to control how that pattern works.
| | 01:40 | I'm going to space them out, just a little bit
more and click Ok and now we've got that pattern.
| | 01:45 | Now these are all patterned
off this original seed part here.
| | 01:48 | So if I were to change this
part, they all change together.
| | 01:52 | It's kind of like the Mirror command,
if I change one, they all change.
| | 01:54 | It's a pattern of this original seed.
| | 01:57 | Now I'm going to just undo this
whole pattern and go back to original
| | 01:59 | and then we're going to do the Circular Pattern.
| | 02:01 | So the Circular Pattern is, we have a
couple of questions to answer as well.
| | 02:05 | What do we want to pattern? That
is going to be this rectangular box.
| | 02:07 | Where do we want a circle or, rotate it
around? That is going to be this point here,
| | 02:12 | so jump down here, pick on Circular Pattern.
| | 02:16 | The first question is what is our
center of rotation? Click right there.
| | 02:21 | Point 21 is where we're going to rotate around.
| | 02:22 | I'm going to jump down here
to the Entities to Pattern,
| | 02:25 | and I'm going to pick
these four parts of that box.
| | 02:30 | You could see a little preview
of what it's going to be doing.
| | 02:32 | Now I have other questions to answer over
here. Where is the center point of this?
| | 02:36 | What are the XY coordinates?
| | 02:37 | How many degrees do you want to
circularly rotate this thing around?
| | 02:40 | By default, it's giving a
360 with an equal spacing.
| | 02:43 | I could change that to 180
and only go halfway around.
| | 02:46 | So I've got four of these and
half of a circle patterned around.
| | 02:51 | I could change that to 90 if
I wanted to and you can see
| | 02:54 | how that is changing around there and
I can continue to add more and more.
| | 02:59 | So I can continue to kind a put a lot of pieces in
there or just a few, depending on what I want to do.
| | 03:04 | Same thing with Equal Spacing. I could change
that. I can change the spacing between them.
| | 03:08 | I can put a radius in there.
| | 03:09 | I can change the diameter that
I'm spacing these thing out on.
| | 03:13 | I can start pushing this thing out a little further
if I needed to, or the angle I'm going to go through.
| | 03:17 | So a lot of options here for a circular pattern.
| | 03:19 | Once you're done and have enough items that you want
in there, click OK and there's your circular pattern.
| | 03:25 | Following along with the simple sketch
methodology, we don't really want to overuse this tool.
| | 03:31 | However, in certain situations,
it does come in very handy.
| | 03:33 | The steps to follow are simple as
selecting the objects, choosing the directions,
| | 03:38 | or the center point of rotation.
| | Collapse this transcript |
| Using construction lines to place features with precision| 00:00 | Effective use of construction
lines and construction geometry
| | 00:03 | is the key to being an
effective and efficient designer.
| | 00:07 | Many times sketches can be fully-
defined without even a single dimension.
| | 00:12 | By tying your sketch geometry into existing
geometry, we build powerful sketches that are dynamic.
| | 00:18 | Let's consider the case of two holes that need to
be equally distanced from the centerline of a part.
| | 00:24 | Let's take a look.
| | 00:25 | This part here we want to add a hole
on either side of the existing part.
| | 00:28 | So what I'm going to do is I'm
going to click on the top face here,
| | 00:31 | I'm going to click on Sketch, I'm
going to start a brand new sketch,
| | 00:33 | and then I'm going to hit the Spacebar so I'm going
to get the Orientation window and click on Normal To.
| | 00:37 | Now I'm looking directly down on that part.
| | 00:39 | Now I want a hole here and I want a hole here.
| | 00:42 | Before I do that, I'm going to draw a few lines.
| | 00:44 | Now we have not covered
the Extruding command yet,
| | 00:49 | but we'll be just giving a brief
demo of how that's going to work.
| | 00:52 | So to start off, I want to click on
the origin, I'm going to drag a line up,
| | 00:55 | make sure it's got a vertical
orientation, click here, double-click,
| | 00:58 | and then I'm going to create
one more line right above it.
| | 01:00 | Make sure that one has got the horizontal
relationship. Now I'm going to click on this line,
| | 01:06 | hold down Ctrl, select that endpoint, and
then I'm going to say I make this mid point.
| | 01:11 | So now I have a line that's
connected and on the center.
| | 01:15 | Now I can go ahead and I want these holes to
be kind of in the center of these ears here.
| | 01:21 | To do that, what I can do is add another
construction line from the upper corner here in the upper right
| | 01:27 | to this little point here and then I can drag
this line here to the midpoint of that line.
| | 01:33 | Now notice these lines are now fully
defined, I can't drag this one or anything else.
| | 01:37 | They're all tied together
with purely construction lines.
| | 01:40 | Now let's go ahead and put the circles in there.
| | 01:42 | So I'm going to go click on here, click
on the midpoint of that, draw the circle.
| | 01:47 | Click on this point here, draw out
a circle, and let's just go ahead
| | 01:50 | and add an equal relationship
between the two, so they're the same size.
| | 01:53 | The last thing we need to do is add a
dimension just to define the size of the circle,
| | 01:58 | I'm going to go to 0.75, and
there's our two circles fully-defined,
| | 02:03 | and they're defining context of the other
parts and the other geometry around them.
| | 02:06 | Now what makes the sketch geometry so
powerful is that if this base part changes,
| | 02:11 | these holes will automatically adjusted
the correct locations. Let's take a look.
| | 02:14 | I'm going to go ahead and show you a little bit
of a head here and do an extruded cut for a hole.
| | 02:20 | So this is very similar to an extrude, but
extrude cut which we'll be doing in a few chapters.
| | 02:24 | I'm going to go ahead and click line, I'm going
to say Through All, so it cuts the entire part.
| | 02:29 | I'll OK and there is my two
holes, it goes through the part.
| | 02:32 | Now what we want to do is we actually
want to go and change this base part.
| | 02:36 | So you notice, we have
two features, here and here.
| | 02:39 | I might look at the sketch
underlying the Boss feature which is Sketch1.
| | 02:42 | Click on that, and let's say Edit Sketch.
| | 02:45 | Now looking at this, it's undefined;
| | 02:47 | all the sketches are blue, we
don't have any dimensions at all.
| | 02:49 | So let's go ahead and add some dimensions to it.
| | 02:51 | I'm going to click and click from here to
here, add a dimension of 12 from the top,
| | 02:56 | add a dimension from here this
bottom line, add dimension of 4, click OK
| | 03:03 | and I add another dimension here of 4,
click OK, and then the last thing we need to do
| | 03:07 | is from the bottom of that to the bottom
of here and we're going to say 4 as well.
| | 03:11 | So now we have a fully-
defined sketch that's changed.
| | 03:15 | So as soon as I exit out of this, guess what?
| | 03:19 | The holes are in the perfect location,
we didn't change any of the dimensions.
| | 03:22 | If I go back and I look at the sketch to define
where they were, it's because those centerlines,
| | 03:27 | or those construction geometry,
automatically scale and move to the right size,
| | 03:31 | because they're tied in to the
sketch that was based below it.
| | 03:34 | Building good construction geometry is
the single best way to make better sketches
| | 03:39 | and to leverage the power of the
dynamic capabilities of SolidWorks.
| | 03:43 | Always try to think through how your sketch
will behave and try to minimize excess dimensions.
| | 03:49 |
| | Collapse this transcript |
|
|
6. Reference GeometryWorking with planes| 00:00 | When a new SolidWorks Part is opened, we have
three predefined planes to start building our model.
| | 00:05 | To start a sketch we need
to choose a face or a plane.
| | 00:09 | So what happens when we need a plane other
than the ones that are located at the origin?
| | 00:13 | Lucky for us, SolidWorks has given us
the ability to create planes where we want.
| | 00:18 | Planes are infinite and in all directions,
so there are no perimeter boundaries.
| | 00:23 | In order to create a plane we need a
series of three points, or a line and a point,
| | 00:27 | or an existing plane and a distance.
| | 00:30 | I have this Top Plane highlighted here
. I can highlight it by just clicking
| | 00:34 | on the goggles and toggle that on and off.
| | 00:36 | So that's the first plane and we're going
to create a plane directly above this plane.
| | 00:40 | New planes are created under
the Reference Geometry tab here.
| | 00:43 | If I click on the Down Arrow, I've got
options of Plane, Axis, Coordinate System,
| | 00:46 | and we're just going to
pick that first one, Plane.
| | 00:49 | As soon as I start a plane, notice
over here I've got a bunch of options;
| | 00:54 | I have a First Reference,
Second, and Third Reference.
| | 00:56 | If I pick another plane like this existing
plane here, I don't need any other references;
| | 01:01 | all I need is that plane and
then a distance away from it.
| | 01:04 | These planes extend infinite
directions; there are no boundaries at all.
| | 01:08 | What I see here is this little
box, it's just representation.
| | 01:11 | I can actually drag the planes
to make them bigger or smaller.
| | 01:14 | So if I select this first plane here to create,
| | 01:17 | notice if I spin the world around a
little bit here in my environment,
| | 01:20 | I can see that here is my beginning
plane and then here is my existing plane.
| | 01:24 | I can change the
distance by just typing this in.
| | 01:28 | So above that Top Plane
I'm creating a new plane.
| | 01:31 | That looks kind of like a sheet
of plywood or a big rectangle here.
| | 01:34 | As far as bringing up above the
height, I'm saying 2 inches above,
| | 01:37 | and I can also just flip that to
the bottom side if I wanted to.
| | 01:40 | And I can ask how many planes I want.
| | 01:42 | I can add multiple planes if I wanted;
they're all spaced off at 2 inches at a time.
| | 01:46 | I'm just going to create the first
one, choose Mid Plane and flip it.
| | 01:50 | Flip it a different direction. I
can do a lot of different things.
| | 01:52 | I could play around with that.
But we just want the distance.
| | 01:57 | Notice Second and Third
References are not included in this one.
| | 02:00 | As soon as I click OK, it
gives me this new Plane here.
| | 02:03 | If I click on that Plane, notice I've got these little
handles all around the outside, little balls around the corners.
| | 02:09 | I can grab any one of these things and
just drag it around to make the plane bigger.
| | 02:12 | This really means nothing; it's just
there for us to see the plane easier.
| | 02:17 | This plane really does extend in
all directions and into infinity.
| | 02:20 | So we can have the plane as big
as we want or as small as we want,
| | 02:23 | it doesn't really matter, just we can drag it
around or move it around in our environment,
| | 02:26 | just to make it some more
visually appealing and easy to work with,
| | 02:30 | to find where that plane is,
that's all those guys are.
| | 02:33 | So that is the first type of plane, which
is an offset plane from an existing plane.
| | 02:37 | I'm going to flip over here to my second
example, which is pretty much the same thing.
| | 02:41 | I've got the Top Plane turned on, and this time
I've actually got a sketch here, so I've got Sketch1.
| | 02:47 | Inside that sketch I have just this
one line, so I will open up that sketch,
| | 02:51 | take a look, it's just a sketch, it's an
undefined line, with a dimension from the origin.
| | 02:57 | And then on my second sketch here,
I've got another construction line.
| | 03:02 | So those are two things I have,
just to kind of lay things out.
| | 03:04 | Now, I don't necessarily need to use these.
| | 03:07 | I could be making a plane from other
geometry that might be having my model,
| | 03:11 | but since I don't have any, I've just
created those two to define this plane,
| | 03:15 | so I'm going to click on Plane.
| | 03:16 | For my First Reference this time, I'm
going to choose that line, there it is.
| | 03:19 | Notice as soon as I pick that line, look what
I get, I get this plane kind of coming up here,
| | 03:24 | at a little bit of an angle, it
doesn't actually know where it is.
| | 03:27 | So to find this thing I've got to kind of
spin it around so it touches another point,
| | 03:31 | and here is a point I'm going to use
that's at the very top of this thing.
| | 03:34 | So I pick that, now that plane is defined
through that line and through that point,
| | 03:39 | so that's all I actually
need to define that plane here.
| | 03:42 | And I don't need the Third Reference,
because I'm actually picking up three points,
| | 03:45 | because I'm getting two
from that one existing line.
| | 03:48 | As soon as I choose that,
click OK and we're good to go.
| | 03:51 | Next we're going to add a
plane through three points.
| | 03:54 | So the points we're going to use are going to
be slightly different than what we had before.
| | 03:58 | So I'm going to click here and create
another plane on top of this existing plane.
| | 04:02 | So I'm going to say Reference Geometry > Plane.
| | 04:05 | This time instead of picking Lines or
Planes, I'm actually going to pick just Points.
| | 04:09 | So I'm going to pick a point here,
I'll pick a point here, pick a point here,
| | 04:12 | and now I have a new plane off at an
angle created off of that existing Plane.
| | 04:19 | Now I could have just chosen that
entire line if I wanted to, or a point,
| | 04:22 | but sometimes you just have like
vertices you might be using to pick points,
| | 04:25 | so now I'm using all three of those
References and they are all coincident to that point.
| | 04:30 | Click OK, and I've got a next reference there.
| | 04:32 | Those are the three
different ways to create Planes.
| | 04:34 | So then here's an example of how we can use
planes and we're going to be doing a lot more
| | 04:38 | with planes later, but this is a quick
example of just showing how they can be used.
| | 04:42 | This part here has got a couple of holes that
we've added to it at angles that are nonstandard,
| | 04:47 | and we've created three different
planes here to go ahead and to create that.
| | 04:51 | The very first plane is actually just
a Top Plane and I'm showing that there.
| | 04:55 | So what I'm going to do is I'm going to use
the History Bar and I'm going roll this way back
| | 04:58 | to the very beginning, and I'm
going to see just the Top Plane.
| | 05:01 | On that Top Plane I went ahead
and created this Boss-Extrude.
| | 05:04 | Now obviously we're going to cover
Extrude in more depth in the future,
| | 05:08 | however, the underlying
sketch is just a simple rectangle.
| | 05:12 | Then, I create a sketch down here;
| | 05:14 | I can highlight it showing just
a line on that same Top Plane.
| | 05:19 | Then I create one more
sketch with a vertical line here.
| | 05:24 | What I want to do here is I want to create a
plane through that line and through that point.
| | 05:28 | Now we saw that a little bit earlier
as far as how to create that plane.
| | 05:31 | So what that's going to do is going to
create that plane there, off at this angle.
| | 05:35 | And that's defined if I were to
change the height of this line here,
| | 05:39 | it would obviously change the angle of
that plane and how it intersects to the block.
| | 05:44 | You can see it's also cutting
through that block a little bit too.
| | 05:47 | My first cut is just going to
be a sketch cut at an angle here.
| | 05:50 | So what that's created by is
creating a circle on that plane.
| | 05:54 | If I hit the Spacebar, I
can look at Normal To it.
| | 05:56 | So I'm looking straight down that
block; it's a perfect Circle here.
| | 06:01 | It's being cut into that part through it.
| | 06:05 | And it's undefined right now, so it's
just going to be cutting through there.
| | 06:08 | I can always go ahead and define
that later with some dimensions.
| | 06:13 | And then next we're going to do
another plane and then do another cut here.
| | 06:15 | So I'm going roll forward again
. I'm creating a plane this time
| | 06:19 | off of this corner of the
base block and this line here.
| | 06:24 | So we've got a plane that aligns
between those two, as you can see.
| | 06:27 | And then on that plane I create
a sketch and a cut at an angle,
| | 06:31 | so that sketch is just another
circle, cutting across that part,
| | 06:35 | right in that kind of the middle of that block.
| | 06:37 | And what we're doing is a cut there and
I'm using a special part of the Cut feature,
| | 06:42 | which is called the Mid Plane Cut, and I'm just
extruding it to make sure it cuts through everything,
| | 06:49 | just a little bit past the ends
there, so it's a Mid Plane Cut,
| | 06:52 | which we're going to be covering in Chapter 7.
| | 06:54 | Clearly a lot of these
tools we have not covered yet,
| | 06:56 | I just want to give you the value
of planes and give you a glimpse of
| | 06:59 | some of the new tools I'm going to be
covering, like the Boss-Extrude, Extrude Cut,
| | 07:03 | and some of the other plane
features you might be using in the future.
| | 07:05 | Planes are the foundation for sketches,
and in order to build complex features
| | 07:10 | or higher-level features like lofts and sweeps,
| | 07:12 | we need to understand the
basics for creating new planes.
| | 07:15 | There are up to three reference
values used for creating planes;
| | 07:18 | however, you can use as little as one,
depending if you're choosing Points, Lines or Planes.
| | 07:23 | For instance, a line already has two
endpoints, so that counts as two references.
| | Collapse this transcript |
| Placing and using axes| 00:00 | Anytime we're building revolved or
rotated geometry, we need an axis of rotation.
| | 00:05 | We can create an axis by selecting
intersecting planes, lines or points.
| | 00:10 | Axes are also very useful
for building assemblies.
| | 00:13 | The first one I'd like to create is
actually between these two planes.
| | 00:16 | So I'm going to click on the Axis command,
and the one I'm going to choose is Two Planes.
| | 00:21 | Pick that one and notice I see already a
dashed line here where the two planes intersect
| | 00:26 | and that's exactly where
that axis is going to go.
| | 00:29 | So I'm going to pick Front
Plane and the Right Plane
| | 00:32 | and right there it generates a
preview, click OK and we've got axes;
| | 00:36 | the first axis there which
I'm calling axis number 6.
| | 00:41 | Okay, the next axis we're going to
go ahead and create is going to be
| | 00:43 | between these two points here, and
I've already laid those out as a sketch.
| | 00:47 | So if I take a look at that sketch
here, it's just on the right plane,
| | 00:52 | and I really just put two points on that plane.
| | 00:55 | So we'll go back up here to Axis.
| | 00:56 | This time I'm going to pick two
points, pick that point, pick that point,
| | 01:02 | and pretty easily we've got
another axis. There it is.
| | 01:04 | This one's called Axis7.
| | 01:08 | Okay, continuing on, we've
got it one more time here;
| | 01:12 | on line or edge. I've got
these rectangular blocks over here
| | 01:16 | and I'm just going to pick any one
of these edges to create another axis.
| | 01:18 | So I'm just going to pick this one here, and
it just drops that axis just along that edge.
| | 01:23 | Click OK, there it is.
| | 01:27 | Okay, one more time,
we're going to grab one more;
| | 01:30 | Cylindrical or Conical Face, click on that.
| | 01:32 | This has already got a
nice cylinder on the outside.
| | 01:35 | So, if I just click on that, it just will
automatically drop an axis in the center of it.
| | 01:39 | But actually, before I do
that, I'm going to cancel that.
| | 01:40 | Anytime you have a
revolved or even a round feature,
| | 01:44 | SolidWorks actually adds an
axis in the center there for you.
| | 01:47 | So if I go up here to View,
and say Temporary Axes,
| | 01:50 | I can actually see there's already an
axis in there, and those would be very useful
| | 01:54 | especially if you have holes or
something like that in your trial line.
| | 01:56 | But if I didn't use that, or didn't
want to use that, I can hide that and
| | 02:00 | use that Reference Geometry > Axis >
Cylindrical Face, click on the outside face,
| | 02:04 | and there is my axis. There it is.
| | 02:07 | And the very last one would
be Point with a Face or a Plane
| | 02:12 | and I'm going to go ahead and
turn on one of these planes first.
| | 02:16 | So the Top Plane, I'm
going to show, so I can see it.
| | 02:19 | Now I'm going to use that plane and this
point here just to create another axis.
| | 02:23 | So I'm going to come up here to
Axis, select on Point and Face/Plane
| | 02:27 | and the plane I'm going to choose is this one,
| | 02:30 | and the point I'm going to choose is
this one right here, and there it is.
| | 02:32 | So it's just making a vertical axis
that's normal to this plane through that point.
| | 02:37 | So those are all the different
types of axes that we can create.
| | 02:41 | The ability to create axes allows us to
define the center line of rotated features
| | 02:45 | and aids in constructing assemblies.
| | 02:48 | Leverage axes to define the center of your
design and to help build complex revolved geometry.
| | 02:53 | We'll be seeing more of axes in
Chapter 7 when we do Revolves,
| | 02:57 | as well as in Chapter 11 when
we start building assemblies.
| | Collapse this transcript |
| Working with the coordinate system and individual points| 00:00 | Sometimes we need to work with our model using
a different coordinate system that was defined.
| | 00:05 | It is very useful for measuring the center
of mass or for other physical properties.
| | 00:10 | Coordinate systems can also be
very useful for assembling parts.
| | 00:12 | We're also going to learn about applying
points to models, and how to define them.
| | 00:17 | Looking at this part, we've actually
looked at this part in previous movies,
| | 00:21 | and I'm going to use this to define
some points in our new coordinate system.
| | 00:23 | First off, let's click on Reference
Geometry, let's click on Coordinate System.
| | 00:26 | Now, by default, our coordinate
system is based right at the origin.
| | 00:31 | But, if I want to place a new coordinate
system, I can just click on Point to define that.
| | 00:35 | Notice I've got an X, Y, and a Z, and I
can align any one of these axes to that.
| | 00:39 | So with X axis, I'm going to
just place it along a line.
| | 00:41 | So you can use any line that happens to
be close to where you're drawing from.
| | 00:45 | So I'm going to use the X axis. Now
that's pointing in that direction.
| | 00:47 | I can also flop and rotate
it to the side if I needed to.
| | 00:51 | And for the Y axis, that same thing, I can go
in and say, I want the Y going in this direction,
| | 00:55 | or I can change the direction there.
| | 00:56 | Then Z is going to kind of always be the third.
| | 00:59 | We don't really need to define it, but if we
wanted to, we could add that in there as well.
| | 01:03 | Once I have that defined, it shows up there.
| | 01:06 | I've got the axes there, and then I can go over,
| | 01:08 | and under the Tools palette, which if you
don't have it, you can just click up here,
| | 01:12 | right-click anywhere and show
the Tools palette just down here.
| | 01:15 | Tools, I already have it showing,
so I don't need to turn that on.
| | 01:18 | Here is the Tool, and the first one here is like
a little balance, and that's the Mass Properties.
| | 01:22 | So I click on that, and this little window here is
going to show me some of the mass properties of this.
| | 01:27 | Now over here I don't have any material defined,
so that's probably what we would need to do first.
| | 01:30 | So I'm going to cancel that.
| | 01:32 | I'm going to go over here and I'm
going to define our material real quick,
| | 01:33 | and you can do that just by clicking
on it, with your right-click actually,
| | 01:37 | and let's just change
this to Plain Carbon Steel.
| | 01:40 | Select that, and that's
going to change this material,
| | 01:43 | and the look and feel of
this part to being a steel part.
| | 01:47 | It changes the visual appearance as
well as all the physical properties.
| | 01:50 | And then I come over here to Mass Properties, and
this is all based upon the real density of steel,
| | 01:56 | the mass, and I also get the center of mass
based upon this part with a bunch of things here.
| | 02:02 | Now I can go up here to default and I can
change which coordinate system I'm working with.
| | 02:06 | So if I click to Coordinate System3,
I get a center of mass here and here.
| | 02:10 | If I click on the default, notice
this goes back to like x = 0, z = 0
| | 02:16 | because it's right there at the origin.
| | 02:17 | So I'm allowing myself to calculate the center of
mass, the moments of inertia from a different point.
| | 02:24 | Okay, let's spin it around. I'm
actually going to change this from Carbon Steel
| | 02:30 | to maybe ABS, or we can
change it to Brass for instance.
| | 02:35 | So you can see how you change that around and it also
changes a lot of the physical and visual properties.
| | 02:40 | I'm also going to delete this Coordinate System
right now, because we're not going to be using it.
| | 02:43 | Now we're going to go ahead
and put some points on this.
| | 02:47 | So under Reference Geometry, I can select Point.
There are a couple of different ways to do this.
| | 02:50 | So the first one is called Center of
the Arc, so I'm going to select that.
| | 02:54 | Now I have a couple of arcs to use.
| | 02:55 | I'm going to say I like this one right here.
| | 02:57 | If I select that, it just drops a
point right there in the center.
| | 03:00 | Pretty handy, so there's a new point.
| | 03:02 | One more, I'm going to go up here
to Reference Geometry, click Point,
| | 03:06 | and this is going to be Center of Face.
| | 03:08 | Pick that one, grab a face, for
instance this face over here, pick that face,
| | 03:12 | it drops it right in the center of
that face and now we've got Point17.
| | 03:15 | Pretty nice. Add a few more, this
time with the Point > Intersection.
| | 03:20 | Now you need two curves to use this one.
| | 03:22 | So I drew two little lines up here at the top,
and notice I have a curve one, and I have curve two.
| | 03:27 | As soon as I do that, click, it
drops a point right at the intersection.
| | 03:31 | And a little further, do Point > Projection.
| | 03:34 | This means we're going to project from an
existing point down to a face or a plain.
| | 03:39 | I'm going to pick maybe this point
here, and I'll pick like this face here.
| | 03:43 | That's going to project that
point all the way down here.
| | 03:46 | It's actually inside of
that cylinder a little bit,
| | 03:49 | but you might have some occasion, you
might need a point in there, and there it is.
| | 03:53 | Okay, and then the very last one here is under
Reference Geometry > Point, and it's a series of points.
| | 04:01 | So you can lay out a bunch
of points along one edge.
| | 04:03 | So for instance, I'm
going to use this edge here.
| | 04:06 | Actually I'm going to get rid of this,
and I'm going to pick this edge here.
| | 04:11 | Notice I've got a bunch of points now
evenly distributed across that edge,
| | 04:17 | where I can put them at a certain
distance that it's going to be going through,
| | 04:20 | like we'll make that distance longer or shorter.
| | 04:22 | I can adjust that. I can change
the distribution or the percentage.
| | 04:25 | There's a lot of different things I can do
here to lay out those points and how I want them.
| | 04:29 | So I want them evenly distributed and I
can change how many I'm putting on there;
| | 04:33 | click OK and those are my new points.
| | 04:35 | SolidWorks provides a nice feature to redefine
the local coordinate system used in our model.
| | 04:42 | In fact, you can assign multiple coordinate systems
based upon your needs and switch between them at will.
| | 04:47 | The Points are very handy little helpers. They'll
allow you to define sketches as well as build assemblies.
| | Collapse this transcript |
|
|
7. Building 3D GeometryExtruding a sketch into a 3D object| 00:00 | Let's get into the solid aspects of SolidWorks.
| | 00:03 | Until now we've learned how to create
sketches and to work with sketch geometry.
| | 00:08 | Now it's time to take those
sketches and turn them into a 3D solid.
| | 00:11 | The first of these
commands is the Extrude command.
| | 00:14 | The requirements are a close sketch region on a
Face or Plane and then selecting the Extrude Feature.
| | 00:20 | In SolidWorks I have a rectangular
shape and a circle just drawn out here.
| | 00:25 | Notice there are no
dimensions on them quite yet.
| | 00:27 | But we're just going to use them
to demonstrate the Extrude command.
| | 00:30 | So, so far with this Sketch I'm
going to jump up here to Features tab,
| | 00:34 | Click on Extrude Boss/Base.
| | 00:35 | As soon as I do that, I get this
little arrow that pops up here,
| | 00:40 | and I can drag this up or
down actually to find that shape.
| | 00:44 | I get this little ruler there
showing me exactly how long that is.
| | 00:48 | It's kind of a rough estimation.
| | 00:49 | It's better to actually type in over here on
the left-hand side the exact length we want.
| | 00:54 | We have a few options as far as
how we want to extrude this shape.
| | 00:58 | The first one here is
where do we want to start from?
| | 01:01 | By default it's going to pick right
where you drew that sketch at on that plane.
| | 01:04 | Alright, we have a plane
shown here under the Top Plane,
| | 01:07 | I'll just highlight it there, so
it's showing us right where we drew it.
| | 01:10 | But I can also start from a Surface
or from a Vertex or from an Offset.
| | 01:15 | So we don't have any surfaces or vertexes
right now, but we'll click on the Offset.
| | 01:19 | As soon as I do that I can
just type in a number here,
| | 01:22 | and notice how that block
kind of moves up a little bit.
| | 01:24 | I can also flip the direction of offsetting.
| | 01:28 | So I can flip it between the two and
change that number around a little bit.
| | 01:33 | So that's Offset, but I'm going to
change it back to the regular Sketch Plane.
| | 01:36 | For Direction, by default it's Blind,
so that whatever number we type in here,
| | 01:39 | as far as 8 inches, it's just
going to go those 8 inches up.
| | 01:43 | I also have a few options here.
| | 01:45 | Up To Vertex, if I had a point
somewhere, if I wanted to just extrude it
| | 01:48 | up to that point, that's
the option I would choose.
| | 01:51 | Same thing, if I had a surface that
I wanted to extrude this thing up to,
| | 01:54 | it would continue to go
until it hit that surface.
| | 01:56 | Offset From Surface is the same thing.
| | 01:58 | So if wanted to be up to the surface, but a
certain distance away, that's what I would choose.
| | 02:03 | Up To Body, if there was another body
in my model, we could actually do that
| | 02:08 | and we're going to do a few
of these in a few minutes here,
| | 02:09 | and then Mid Plane, Mid Plane actually would put
that Sketch Plane right in the center of my block,
| | 02:16 | and then as I change that,
it expands in both directions.
| | 02:18 | We have the option to add draft to our features.
| | 02:21 | So notice if I click on a Draft here, it
drafts it in both directions from the Sketch Plane.
| | 02:27 | If I had only Blind going in one direction,
it would just draft it in that direction.
| | 02:31 | Then I can change the Draft angle, I can
draft it outwards if I wanted to or inwards,
| | 02:36 | a bunch of things I can do there.
| | 02:37 | Direction 2, if I click on that, just allows me
to expand that block in the secondary direction.
| | 02:44 | I can draft just that one side if I
wanted to, draft both sides if I wanted to.
| | 02:48 | I could change different angles if I
wanted to, a bunch of things there.
| | 02:51 | I'm going to turn Direction 2 off.
| | 02:53 | Thin Feature turns this into
more like a Sheet Metal part.
| | 02:56 | So instead of actually filling it in, it
actually uses to create two different shapes here,
| | 03:01 | and I can change the thickness
of how much I want to do that.
| | 03:05 | So now I have kind of like just the profiles,
and I even have the option to cap the ends of it
| | 03:10 | to create like a block, and I can fill this in now,
so I've got this kind of a solid filled block.
| | 03:18 | The Select Contours is
the last option down here.
| | 03:21 | Now if I didn't want to extrude all
this stuff, I just wanted a portion of it,
| | 03:25 | you know I wanted maybe just one half of this
block, I could select that and it would just extrude
| | 03:30 | that one-half with a little half circle
cutout of it, that's a real handy feature.
| | 03:35 | And also if you didn't have a fully-enclosed
sketch and there were some extra lines in there
| | 03:40 | and SolidWorks didn't actually
understand what you wanted to extrude,
| | 03:44 | it would automatically go into the Selected Contours Mode and
say what of these things do we actually want to extrude out?
| | 03:50 | For right now, we're just
going to turn off the Thin Feature
| | 03:52 | and we're just going to turn this
into a regular block, then we click OK,
| | 03:55 | and there is our first official 3D solid.
| | 03:59 | The 3D solid is made up of two things
; one is the Extrude Feature itself.
| | 04:03 | So if I want to go back and change
how much we extruded or add draft or
| | 04:06 | something like that, I would go and
click here under the Edit Feature.
| | 04:10 | There it is, so I can go back and change it,
so instead of 9 inches, maybe I want 8 inches.
| | 04:14 | Click OK, it's going to drop it down
a little bit and there we are, okay.
| | 04:16 | But if I actually wanted to change the
shape, I'd actually have to click on this
| | 04:20 | little Plus (+) sign here and that is
going to open up the underlying sketch.
| | 04:24 | Now the sketch geometry is
where the shape is defined.
| | 04:27 | Click on that and then in the in-
context window here, I click on Edit Sketch.
| | 04:30 | I'm going to hit the Spacebar and click
on Normal To so I'm looking straight at it.
| | 04:35 | I can move these things around, so if I drag this around,
I change the shape a little bit, make a long rectangle.
| | 04:40 | As soon as I exit out of the Sketch, the shape
changes, but the Extrude is exactly the same.
| | 04:46 | It just took whatever shape I
had and extrudes it 8 inches.
| | 04:50 | Let's go back to the Sketch again, this
time let's play with it a little bit and
| | 04:56 | actually take this rectangular block here and
let's take this circle and pull it to the outside.
| | 05:00 | Alright, let's see what happens. A
completely different shape, look at that, because the
| | 05:06 | circle is now the exterior boundary and the
square rectangle is now the interior boundary.
| | 05:11 | So it just changed it around.
| | 05:12 | Now I can also go back to this sketch and
start adding some things if I wanted to.
| | 05:16 | I'm going to happen to add just
four circles around the perimeter here,
| | 05:21 | and I'm just throwing them in
there just to illustrate this.
| | 05:23 | Of course if we were making this for real,
we would like to fully-define those sketches
| | 05:28 | to not have any blue and
all fully-defined sketches.
| | 05:32 | From there we're going to click
OK, and notice what happens here.
| | 05:37 | It automatically just adds
those four holes to our design.
| | 05:40 | We're going to continue on with this block here.
| | 05:43 | I'm going to click on this inside face here.
| | 05:45 | I'm going to create a new extrude.
| | 05:46 | So I'm going to click on the
Sketch, draw a little sketch.
| | 05:50 | We're going to pull this circle
over here in the corner, there he is.
| | 05:53 | Then I'm going to click on the Features > Extrude
tab and it's going to extrude it out a little bit.
| | 05:58 | So by default, we can extrude a certain
amount of inches, so we've got 9 inches in here.
| | 06:02 | Let's go through a few of
these other options here.
| | 06:04 | Through All, click on that and notice it goes
all the way up to the end of the part, there it is,
| | 06:09 | but it's sticking through a little bit and
it's aligned with the end of that feature.
| | 06:13 | If I go to Up To Next, it's going
to go the very next thing it finds,
| | 06:18 | so it finds the inside of this
rectangular shape, so it's going to go up to that.
| | 06:22 | Now if I were to change that
size of that rectangular hole,
| | 06:24 | it would automatically update
and go to the next face it found.
| | 06:29 | Up To Vertex, if I have any point or
line or intersection, I can select,
| | 06:34 | I can pick like a corner from here or here.
| | 06:36 | I can even go in and turn on other sketches.
| | 06:40 | If I want to click over here and show that sketch,
so here is the underlying sketch we had before,
| | 06:45 | and maybe I'll go up to like the center
point, see that with center point there,
| | 06:49 | snap to that and now I've got a shape
that's going to go up to the center point,
| | 06:53 | that's the vertex I'm choosing.
| | 06:55 | I'm going to go Up To Surface. This
one's kind of cool. Pick that surface.
| | 07:03 | So now it's extruding up to that surface.
| | 07:05 | Now it wouldn't make a lot of sense here
because we already have that filled in,
| | 07:09 | but the next one here is Offset From
Surface and now I can actually pick that surface
| | 07:15 | and pick how much I want to offset from it and I'm
just going to type in like 0.1 for instance there,
| | 07:23 | and let's flip the direction, and now I
can just expand that out a little bit.
| | 07:28 | And now notice it follows that
same shape of the outside of this part
| | 07:31 | and I'm extruding a little bit past there and you
can just do that a little bit with your Reverse Offset
| | 07:36 | and then how much you want to offset,
so it just keeps that same shape.
| | 07:39 | And then the next one here is Up To Body.
| | 07:42 | We don't have any other bodies
because it's a single body part right now,
| | 07:45 | so we can't do that, but it will do
exactly the same thing as Up To Next,
| | 07:49 | so we just go up there and find it.
| | 07:50 | Then Mid Plane we've already done; we're just
going to go kind of in both directions there.
| | 07:54 | Let's go back to Blind, Through
All, a couple of different options.
| | 08:02 | Of the four main solid Features,
Extrude is the most common and easiest to use.
| | 08:07 | The Feature itself is very simple; however, it
builds on the complexity of the underlying sketch.
| | 08:12 | There are a variety of end constraints that you can
assign to the features that affect how it builds its shape.
| | 08:17 | The Extrude command is the building block
that is the most used for model creation.
| | Collapse this transcript |
| Using Revolve to create 3D parts around a circular axis| 00:00 | Much like the Extrude command, the
Revolve Feature creates geometry from a sketch.
| | 00:05 | However the Revolve requires one
more ingredient, the axis of rotation.
| | 00:09 | Once you have a sketch, the next element is a
centerline, an axis or an internal line of the sketch.
| | 00:14 | This is the feature we're going
to create; it's a revolved bottle,
| | 00:19 | and to create that shape we need a sketch
and a centerline and then the Revolve Feature.
| | 00:23 | So I'm going to jump over here
to another sketch I have open.
| | 00:26 | This is kind of a sketch
of the profile of bottle.
| | 00:29 | Notice it's one enclosed perimeter
and the way I created that was just
| | 00:34 | a series of lines and arcs with some
tangency relationships added to them.
| | 00:38 | So I'm just going to show you
how to create that real quick.
| | 00:40 | Jump over here, create a line,
come up here to the tangent arc.
| | 00:47 | Click up here to line. Now I could
easily use the Shortcut Bar if I wanted to,
| | 00:53 | but I'm just showing you by
going up to the simple mouse icons,
| | 01:01 | and I'm just going to continue these.
| | 01:02 | Notice as I am creating the shapes,
it's automatically adding some tangency.
| | 01:07 | Notice that it didn't add it
here though, that's a problem.
| | 01:09 | So it's still like not
working the way I want it to.
| | 01:11 | So I just click on the pairs, and hold down
Ctrl, select the two items, and say Tangent.
| | 01:17 | So now if I move this
around that tangency stays.
| | 01:21 | I can move any of these things around to get
that shape that I want, I can move it in and out.
| | 01:25 | So as long as I have that tangency,
then I have a nice fluid motion that
| | 01:29 | I can move these lines around and
contour that shape to however I want.
| | 01:33 | So that's how you'd kind of go ahead and
create that shape and just continue around,
| | 01:36 | with just a bunch of series of lines and
arcs and we could probably come in here
| | 01:40 | and start defining that with
dimensions or some construction geometry.
| | 01:43 | I'll delete that for right now.
| | 01:45 | So here is our shape and we're
just going to revolve that around.
| | 01:50 | Notice I have a little centerline down
here which it's going to revolve around
| | 01:53 | or I can actually use just
the centerline of the part.
| | 01:55 | So I'm going to click on Features and
Revolve, and the very first question,
| | 02:01 | notice it gives this little arrow, it says,
what do I want to revolve this thing around?
| | 02:05 | And there is my centerline of the part
or I can use this little Revolve axis,
| | 02:09 | click on that, and notice it
just spins it right around for us
| | 02:13 | and we go down here to Direction1 and it says,
how do we want to spin this thing around?
| | 02:17 | By default it's giving you just a blind, so blindly
it's going to spin this thing around in 360 degrees.
| | 02:21 | I could change that if I
wanted to, say like, 45 degrees,
| | 02:25 | and then my profile just
shows it only revolving it for 45.
| | 02:28 | There are some other options in here.
| | 02:30 | If I had a Vertex Up To, I could spin
this around until it actually hit that point,
| | 02:33 | same thing if I had a surface, I
could spin it around until it actually
| | 02:37 | encountered that surface, or
even offset from that surface.
| | 02:40 | Mid Plane is the last one here and that will just
put the sketch right in the center of that extrude.
| | 02:45 | As I expand that out, it
expands it equally in both directions.
| | 02:48 | I'm going to go back to Blind for a second here.
| | 02:51 | I also have a Direction2.
| | 02:52 | If I click on that, now it's also going to
go in the other direction in the same way.
| | 02:56 | So I've got 60 both ways, but
if I wanted to change the angle,
| | 02:59 | it went through on one side more than the
other side, I have that ability to do that.
| | 03:03 | And same thing I can change one way to go
Blind and the other one to maybe go up to a Vertex
| | 03:07 | or a Surface or something like that, so a
lot of different options here I can use.
| | 03:12 | The Thin Feature, if I wanted
to make this like a hollow shape,
| | 03:14 | I could go ahead and turn Thin Feature on
and go through some of the options in here
| | 03:19 | and pick up the thickness I wanted to use.
| | 03:21 | You might have a little bit of an issue with a
part like this, especially when you have small curves,
| | 03:24 | if you try to turn out Thin Feature on, you
have to make sure that the thinness of your feature
| | 03:27 | is actually smaller than the
curve you're going to be using.
| | 03:30 | And then the last thing here is Selected Contours
. So right now we only have one enclosed shape.
| | 03:38 | So if we wanted to break this into
sections or maybe just do like the top section
| | 03:43 | or the lower section, I have to go back to that
sketch and modify that, so let's go try that out.
| | 03:47 | So I'm just going to cancel this for right now.
| | 03:50 | Click on Spacebar, click on Normal
To, so I'm looking straight at it.
| | 03:53 | I'm just going to go back to the Sketch tab
here and I'm just going to say, add a couple lines.
| | 03:56 | So I'm going to section this off
here and one more line up here.
| | 04:04 | So now I have three independent close
boundaries, that one, that one and that one.
| | 04:09 | Now I go back to the Revolve command.
| | 04:12 | Notice as soon as I get into Revolve command, it
doesn't actually know which boundary I want to use,
| | 04:16 | so it goes ahead and
turns the Selection Filter on.
| | 04:19 | Notice my icon has that little
Selection Filter icon next to it.
| | 04:22 | So as I move over each one of these, it
highlights the area that's the enclosed boundary.
| | 04:27 | So I can choose any of these or
all of these or any combination.
| | 04:31 | So I'm just going to pick the very
top one here and I'm going to go pick
| | 04:35 | that axis of rotation that's right here
and click OK and then I'm just going to
| | 04:39 | give that very top piece a
little Hershey's kiss look and shape
| | 04:44 | and you can always go back and edit
this feature again and continue adding on.
| | 04:47 | So you might say, I'd like to add the next
section of it and there is a little bit taller one,
| | 04:53 | or you can go back here and continue and add the
whole shape just by selecting any one of these things
| | 04:59 | or I can just remove one of these just by
selecting it here and hitting Delete and getting rid of it.
| | 05:03 | There is my whole shape, defined out as a
Revolve Feature with the Selected Contour Option.
| | 05:10 | The Rotate command is one of my favorites,
and more than likely will be one of yours.
| | 05:14 | With a simple sketch and an axis of rotation, we can
build elaborate shapes with just a few clicks of the mouse.
| | Collapse this transcript |
| Using Loft to create a complex shape| 00:00 | The Loft command again builds on all the
other features then it needs the sketch.
| | 00:04 | However, the Loft command actually needs at
least two sketches and can have many more.
| | 00:08 | All the heavy-lifting in creating lofts is
spent setting up the correct planes and sketches.
| | 00:13 | If that was not enough, we can even add
guide curves that are independent sketches.
| | 00:17 | The Loft command is one of the most
powerful modeling tools in SolidWorks.
| | 00:21 | If you need to create complex shapes in one
feature, this would be the command of choice.
| | 00:26 | In this video we're going to
cover the basics of this command.
| | 00:29 | However, if you're working with complex shapes,
this command might require a little further study.
| | 00:33 | In SolidWorks I have a rectangle here with
rounded out corners and it's created on the Top Plane.
| | 00:39 | So you should be fairly
comfortable with creating that.
| | 00:41 | Now what I want to do is I want
to add another plane up above this.
| | 00:45 | So I'm going to click on the
Reference Geometry, click on Plane.
| | 00:47 | Now my first reference is just
going to be this Top Plane here.
| | 00:50 | So I'm going to click on that and
it's going to give me a distance
| | 00:54 | and I'm going to just type
in a distance here of 3.0.
| | 00:55 | It's going to move that plane up here,
I'm going to move it around so you can see
| | 00:59 | it's just placing another plane up
above, click OK and there is my Plane.
| | 01:04 | Now I want to create a sketch on this new plane.
| | 01:06 | That's why we put it there.
| | 01:08 | Click on that Plane, click
on Sketch, start a new sketch.
| | 01:11 | Instead of doing that, I'm actually going to
just draw a little circle right there on the top.
| | 01:14 | I can always click on the Spacebar to go to
Normal To that if I wanted to, drag it out.
| | 01:19 | I can add some dimensions if I wanted to, but
I'm just going to leave it as is for right now.
| | 01:23 | I'm going to exit out of that sketch now,
so now I have two independent sketches:
| | 01:26 | Sketch1, Sketch3, and then I have
this Plane that I created that sketch on.
| | 01:31 | Now if I wanted to move this sketch up or
down, I actually move that plane up or down,
| | 01:36 | and that would affect where it lies.
| | 01:38 | To create the loft, what we're going to do is
just go over here to Features and go to Loft.
| | 01:43 | So we've got a couple of choices here in the beginning,
so profiles are the two shapes we're going to use.
| | 01:47 | So we've got this rectangle and this circle.
| | 01:50 | So instead of choosing them from the actual window here,
it's better to actually choose the sketches as a whole.
| | 01:57 | I have the top level expansion bar here.
| | 01:59 | So I can click on this little
Plus (+) and it expands out my tree.
| | 02:03 | So I'm going to pick my first Sketch1 to be the
bottom, and then Sketch3 is going to be the top,
| | 02:08 | and notice as soon as I do that, it actually
creates the Loft Feature for me between the two.
| | 02:12 | Pretty nice, click OK and there's my first loft.
| | 02:15 | Now I'm going to hide that sketch here,
so it just makes a little cleaner looking.
| | 02:20 | Here is my shape.
| | 02:23 | Now I have the ability to kind of go
back and change this around a little bit,
| | 02:26 | so let's go back into that Loft and notice that the
two sketches now are underneath that Loft Feature.
| | 02:33 | So I can change either one of those or I
can go back and change the Loft itself.
| | 02:36 | Okay, so below this is the Start/End
Constraints, so I can click on that
| | 02:41 | and when I start my loft off, which
we start on the bottom piece here,
| | 02:45 | I'm going to click on and I can either do
a Direction Vector or a Normal To Profile.
| | 02:48 | So Normal To Profile actually will make this so
it's facing straight up when it comes off that sketch
| | 02:54 | and then it starts curving
in to hit the other sketcher.
| | 02:57 | So if I click OK, I get a nice kind of
more organic shape, it flows nicely there,
| | 03:03 | and if I do it again, I go back in here and I add
the Normal Constraint to the End Constraint here.
| | 03:11 | So I go back to Normal To Profile,
then I get a shape like this.
| | 03:15 | I also have the option to use a
Direction Vector and I would have to go ahead
| | 03:20 | and put which direction I'd
like to actually move this in,
| | 03:24 | so I'm going to just use the Normal To
Profile, but if I did need to contour
| | 03:27 | that shape a little further, I could do that.
| | 03:29 | So that's Start/End Constraint, I'll
click OK, so you can see how my shape is
| | 03:33 | kind of evolving here as I want to change it
around, I can go back to that one more time.
| | 03:37 | We have got a few different
things down here as far as options,
| | 03:42 | as far as showing the preview, merging the
resulting if I was working with adding a loft
| | 03:46 | to another part of this right there,
I can choose either merge together
| | 03:49 | or just keep it as separate features and
separate bodies and closing out the Loft,
| | 03:53 | Show preview and then Merge tangent faces,
| | 03:56 | these are all just kinds of things
you can turn on and off to define that.
| | 03:59 | The next big thing here is going to be guide
curves and it's how we can actually contour that shape.
| | 04:04 | Right now the shape is defined
just by these Direction Vectors.
| | 04:07 | But if we wanted to kind of
smooth this to a different direction
| | 04:10 | or work with something else,
we could use the guide curves.
| | 04:13 | Now we're going to be going through guide
curves in the next movie, so stay tuned for that.
| | 04:18 | Click on OK. We're going to end
out that feature and there it is.
| | 04:21 | The Loft command is definitely one of
the most powerful commands in SolidWorks
| | 04:25 | and the creation process can be time-consuming.
| | 04:27 | However, the concept is fairly
straightforward and the complexity really lies in
| | 04:32 | building the appropriate
sketches and trying out the shape.
| | 04:35 | Lofts can be very simple to extremely complex.
| | 04:39 | Make sure to review the sketching and plane movies
to really feel comfortable with the Loft command.
| | Collapse this transcript |
| Refining a loft shape with guide curves| 00:00 | Now that we have learned the basics
of creating Loft commands features,
| | 00:04 | we're going to go ahead and take
these things to the next level.
| | 00:07 | We're going to use this starting
sketch here as our layout for creating
| | 00:11 | a mouse-like shape or about
half of a mouse-looking profile.
| | 00:15 | And we have got a few
things to lay this out with.
| | 00:18 | We've got a basic layout on the bottom which is
a sketch, that's just created on the Top Plane,
| | 00:24 | had to show that so I just drew that
out, and I go inside of that sketch.
| | 00:27 | I can see that we did a couple, both lines
here and overall, and it's not fully-defined yet,
| | 00:36 | cause we're still working with that
curve and that shape, but we're just kind of
| | 00:39 | laying out some of these spaces and
putting in some of these construction lines.
| | 00:42 | Okay, once I have that shape, I'm going to go
ahead and build a couple of planes at the two ends.
| | 00:49 | So to do that, I just start a plane,
an Offset Plane from the Front Plane,
| | 00:54 | and I just snapped it to this point here,
and the same thing on the other side,
| | 00:57 | I just snapped it to the point
here to create these two planes.
| | 01:00 | The STARTING_POINT of this
thing is just a single point.
| | 01:03 | If I open that sketch, it
really is just one point.
| | 01:05 | I've just gone up here to point,
dropped it right there and that was it.
| | 01:11 | Get out of that sketch.
| | 01:12 | The END_POINT, same-same,
it's just a single point.
| | 01:15 | The PROFILE is a sketch that's
just created on the Front Plane
| | 01:20 | and that just controls the shape of the mouse.
| | 01:24 | I can move things around if I wanted to,
but notice it just starts at the origin,
| | 01:27 | comes out here and it
snaps to that layout sketch
| | 01:30 | and then it comes up with whatever
shape we want up to the top here.
| | 01:33 | So that's the PROFILE, the END_POINT;
| | 01:38 | now the LOWER_GUIDE is just a straight
line that's going to control the shape,
| | 01:42 | so it just flows along the bottom edge,
| | 01:45 | and then the UPPER_GUIDE is the shape
of mouse over we're going to contour.
| | 01:48 | And the last Guide Curve we're going to
use is actually the original layout here
| | 01:52 | and that's going to be controlling
the bottom profile on the outside edge.
| | 01:56 | So let's go ahead and see if we can't
- and by the way the LOWER_GUIDE here
| | 02:03 | as well as the UPPER_GUIDE were both
created on the Right Plane, so if I show that,
| | 02:07 | you can just see how I started on the Right
Plane and did both of those sketches on that.
| | 02:10 | So I'm just going to hide that for right now.
| | 02:12 | Okay, so let's jump into the
Loft command in our Profiles.
| | 02:18 | So we're going to start on this side
and we're going to progress this way,
| | 02:23 | and so my very first sketch I'm going
to use is actually starting right here
| | 02:26 | and instead of picking it from the
Graphics window, I'm going to go ahead
| | 02:29 | and expand out the tree and I'm going
to use this one called STARTING_POINT.
| | 02:34 | Now I renamed my sketches and
you can just click on sketches
| | 02:37 | and rename them to anything
you want; same thing with planes.
| | 02:39 | So we just made it a little easier to look at.
| | 02:41 | So STARTING_POINT is my very first,
followed by PROFILE and notice as soon as I
| | 02:46 | pick those two, there they are, it shows me
a preview of what I' ll actually get here.
| | 02:50 | So I'm just going to start with a
small point and then go to that PROFILE.
| | 02:56 | Now I have an END_POINT, coming at
the back to the end and notice as I
| | 03:00 | add an END_POINT, now that shape changed
a little bit more, a little more curvy.
| | 03:03 | It's not quite what we're looking for, right?
| | 03:05 | We kind of want this to be more
smoothed down and flowing better.
| | 03:10 | So that's where we want
to use those Guide Curves.
| | 03:12 | Now I just want to point this out as well
is if you have a profile in the wrong order,
| | 03:15 | that's why you have these little arrows
here, so you could change the END_POINT
| | 03:18 | to move it up or down depending if
you got these in the wrong order.
| | 03:22 | In the Guide Curves, we're going to start with
LOWER_GUIDE, that's just going to constrain that,
| | 03:27 | so that, it pulls that
shape along that bottom edge,
| | 03:31 | make sure it's a nice sharp edge and
then our UPPER_GUIDE is just going to change
| | 03:36 | the shape so it flows along that upper shape,
so we're going to take a look at that there.
| | 03:40 | As soon as I click on that UPPER_GUIDE it
drags the shape out to flow along that Guide Curve.
| | 03:45 | And then the last curve is just going to
be one here where we're going to drag the
| | 03:48 | bottom edge of that out to that outside guide,
and that one is the original layout sketch we use.
| | 03:53 | As soon as we do that, it brings it out
and we've got a nice shape that kind of
| | 03:59 | flows very nicely and
ends these two little points.
| | 04:03 | Once we have that, we have pretty much
a complete shape, looking pretty good.
| | 04:07 | Click on OK and there it is. Pretty nice!
| | 04:12 | Now I was going to show a couple of
things that will help us to analyze our shapes,
| | 04:18 | And we click up here under View, we can
click into the Display and we get these things
| | 04:24 | called Curvature, Zebra Stripes, and we can
use either one of these things to actually
| | 04:28 | look at what that shape looks like and see how
much curvature is actually being applied here.
| | 04:33 | As the color changes, you can see it's a
little Sharper Curve or a Smoother Curve.
| | 04:37 | I can turn either one of those
one or both on at the same time,
| | 04:41 | turn the Curvature off. I'm going to turn
on Display and Zebra Stripes, same thing.
| | 04:46 | So if you had something that was a
sharp line or a cut or something like that,
| | 04:50 | the stripes wouldn't be as smooth, so you
can kind of just analyze what kind of shape
| | 04:54 | you've created and how much curvature,
things like that you have applied to it.
| | 04:59 | So there's just couple of things
that you can to analyze your shape
| | 05:02 | and just to smooth it out a little
bit, make sure it's looking well.
| | 05:06 | Okay, now that I have the shape complete,
I'm just going to continue this off.
| | 05:10 | I'm going to jump ahead a little bit.
| | 05:11 | I'm going to teach you guys just
a little about the Mirror command.
| | 05:14 | So I'm going choose the Mirror.
| | 05:15 | It's just going to be a solid mirror,
and I'm going to pick the Mirror Face
| | 05:17 | which is going to be this face here and
I'm going to mirror that entire feature over.
| | 05:21 | Click OK and that finishes out
that shape so we get it complete now.
| | 05:25 | As you can see this is kind of
the start of a computer mouse
| | 05:32 | and we might want to maybe
add a few more curves in there,
| | 05:34 | something like that to change that shape a
little more to get a little bit smoother,
| | 05:37 | but overall it's looking like a good start.
| | 05:40 | As you can see lofts can be very complicated
and can be made from many planes and sketches.
| | 05:45 | Each Guide Curve and Shape
must be on its own sketch.
| | 05:48 | So laying them out is what takes all the time.
| | 05:51 | However, once you have it complete, you have
the opportunity to build something amazing.
| | Collapse this transcript |
| Using Sweep to create wire and pipe shapes| 00:00 | Sweeps allow for the creation of
tubes, hoses, wires or any other object
| | 00:05 | that has a constant profile formed into a shape.
| | 00:08 | Think of a wire hanger.
| | 00:10 | The wire size stays the same, however
we can form it into any desired shape.
| | 00:14 | The requirements are a profile and a path.
| | 00:18 | The profile is a shape that is constant.
| | 00:20 | For a hanger, the profile
is just a simple circle.
| | 00:23 | The path is the final
shape that we want to build.
| | 00:26 | This requires two separate sketches
defining both the profile and the path.
| | 00:29 | In SolidWorks I have a finished hanger
here, that's already defined as one Sweep.
| | 00:35 | To build that, it starts from two sketches.
| | 00:37 | So let's jump over here,
here is the beginning sketch.
| | 00:40 | So here is our Sketch1 just created on
the Front Plane and we define out the shape
| | 00:44 | of what that is, and we should know
how to use most of these commands here.
| | 00:48 | We're just using arcs, lines, arc, lines,
and just lay it out with construction geometry.
| | 00:54 | From there we want to create a profile.
| | 00:56 | Now the profile, we need to have it
aligned to the endpoints of one of these,
| | 01:01 | this endpoint here or this endpoint here. So I can
create a plane at the end of one of these points.
| | 01:07 | I'm going to choose this one here.
| | 01:08 | By using the Reference Geometry, create a plane, and
my reference here is just going to be that endpoint.
| | 01:14 | I want the plane touching that point, and then my
second reference is actually just going to be that line.
| | 01:18 | So pick that line and now I have a
plane that's perpendicular to that endpoint
| | 01:26 | and perfectly aligned with it, a
nice way to create a little plane.
| | 01:30 | Click OK and there it is.
| | 01:32 | Click on Sketch, start new Sketch, and we're
going to choose that plane to draw our sketch on.
| | 01:36 | And we just want a simple
circle right here at the end of that.
| | 01:39 | There is our circle, just draw
it out and we can add a dimension.
| | 01:44 | So I'm going to pick like .25,
like one of those plastic hangers.
| | 01:50 | Click OK and exit out of that sketch.
| | 01:52 | I'm going to hide this plane
just to make it easy to see.
| | 01:55 | So now we have two separate sketches
; Sketch1 is actually the path and
| | 01:59 | Sketch2 is the profile. There it is.
| | 02:02 | That's everything we need to create a Sweep.
| | 02:05 | So let's go in here under
Features and click Swept Base/Boss.
| | 02:10 | The first question, notice the
available icons here and it shows the profile
| | 02:14 | which it just basically shows a
little circle which just makes it handy
| | 02:17 | that we happen to have one, there it is.
| | 02:19 | So we're going to pick that out of the tree.
| | 02:20 | It's always better to pick things from the
tree than from the actual Sketch environment.
| | 02:26 | And secondly, is going to be the path,
and that's going to that Sketch1.
| | 02:29 | As soon as I click on
those two it gives me a preview
| | 02:32 | of what it's going to generate
and how we want to go though there.
| | 02:35 | We've got some other options that we
can click on down here too if we wanted to
| | 02:37 | as far following the path
or twisting along the path,
| | 02:40 | a bunch of things that we can do
to make this a little more wild.
| | 02:43 | We can also use Guide Curves similar
to Lofts to actually change that shape
| | 02:46 | if we wanted to not keep it going exactly
the same profile as I went through that shape.
| | 02:51 | You can get quite complicated doing
that, but it's done much the same way.
| | 02:54 | Start/End Tangency, same thing, so
right now we're starting with None,
| | 02:58 | but we can make it follow the
path or tangent to the path,
| | 03:00 | if we wanted to, just change the shape
a little bit as far as how it's actually
| | 03:05 | going to be dragging that
one profile along that path.
| | 03:08 | And then the last thing here is, we
could turn that into a Thin Feature,
| | 03:10 | but we've got to make
sure we get fairly thin wall,
| | 03:15 | and that would make it a very thin tube here.
| | 03:18 | So if we wanted to create like a thin
tube to or a hose or something like that,
| | 03:22 | we could use the Thin Feature to
create that, very simple way to do that.
| | 03:25 | Right now we're not going to do that.
| | 03:26 | I'm just going to click on OK, and there we go.
| | 03:31 | Wire hanger, quickly create it with the Sweep.
| | 03:34 | Now Sweeps can be used to create wires, like
these hoses, this is just obviously a 2D shape,
| | 03:40 | but we could actually jump into 3D
and create a 3D sketch if we needed to,
| | 03:44 | to have a wire or a tube going in all
kinds of different directions if we needed to,
| | 03:48 | or spinning around in a helix if we needed to,
| | 03:51 | and we'll learn how to make a
helix in the next few chapters.
| | 03:54 | Swept shapes are easy to create as long as
you have the correctly defined profile and path.
| | 03:59 | The complexity of this feature is based
upon laying out the sketches correctly.
| | 04:04 | Spend the time to think through
how you want the shape to be created
| | 04:08 | and the best way to build planes
and their corresponding sketches.
| | Collapse this transcript |
|
|
8. Removing MaterialUsing Extruded Cut to trim parts of a 3D object| 00:00 | Extrude Cut command is basically
the same as the Extrude command,
| | 00:04 | except now, we're cutting with the feature.
| | 00:07 | The requirements are a closed sketch region on
a Face or Plane, and something to cut through.
| | 00:12 | Let's start by selecting a
face and drawing a simple sketch.
| | 00:15 | In SolidWorks here I've got a simple
block that we're using kind of as our layout,
| | 00:19 | and demonstrating to cut through, and
I've created a sketch on that plane here.
| | 00:24 | So I'll pick the end of
the part, click on Sketch,
| | 00:27 | and I just have a real
simple circle that I drew.
| | 00:31 | Now, we could draw a lot of
other things on here if we wanted to,
| | 00:33 | but there is our sketch on that face, click OK.
| | 00:35 | Once I've got that sketch drawn out,
I'm going to use this sketch here,
| | 00:39 | so Sketch2 is what we're going
to use to cut through things.
| | 00:42 | Extruded Cut icon is right here; click on that.
| | 00:46 | Much like the Extrude Command, the first
thing is where do I want to start cutting from?
| | 00:50 | So Sketch Plane, wherever I drew that
shape originally is where my default;
| | 00:55 | I can also push it off to another surface,
I can pick a vertex, or we can offset it.
| | 00:59 | So if I wanted to, I'm going to start cutting
somewhere inside of the part here or something like that.
| | 01:06 | So I didn't actually start here, I
kind of started in the middle here.
| | 01:08 | That would make a nice little offset.
| | 01:10 | But, we don't quite want that right now.
| | 01:12 | So let's go back to the Sketch Plane.
| | 01:14 | So by default, we just start with
Blind, so it's just blindly cut.
| | 01:17 | So it's going to put 3.9 inches.
| | 01:19 | That's how far we're going to cut.
| | 01:20 | So click OK, and there it is.
| | 01:22 | There is our cut feature; it just starts at the
circle, just cuts it through and it cuts 3.9 inches.
| | 01:27 | If I want to go in here and measure that,
I can say measure from this face here
| | 01:31 | to that face there, and there
it is, normal distance is 3.9.
| | 01:33 | So that's my cut distance I cut.
| | 01:36 | I can obviously just section this in
two, to show you how it would look.
| | 01:39 | I'm going to go in and look at that part.
| | 01:41 | Let's go back to that feature.
| | 01:44 | Instead of Blind, we can say, Through All.
| | 01:47 | So if we want a hole, it just
automatically cuts through everything there
| | 01:49 | that's in front of it, click on that.
| | 01:50 | That's going to give us that
nice hole through everything.
| | 01:53 | Okay, go back again; instead
of Through All, Up To Next.
| | 01:59 | Now Up To Next is just going to
find the next face that completely
| | 02:02 | cuts off that sketch region and end there.
| | 02:05 | So no matter how thick the section was here,
it's always going to cut all the way through it.
| | 02:08 | Click OK, and we've got a nice little hole.
| | 02:10 | Okay come back here, Up To Vertex.
| | 02:16 | Now I can pick any point
or vertex to stop the cut.
| | 02:22 | So I'm going to pick like this point here,
| | 02:24 | and notice that point is aligned
with the end of the sketch, click OK.
| | 02:27 | That's actually only going to cut
a little half-moon section up here,
| | 02:30 | because it only goes up to this
point here when it does that cut.
| | 02:32 | I'm going to go back to it, Up To
Vertex; next one will be Up To Surface.
| | 02:39 | Up To Surface, I could say I want to cut up
to this surface here, or this surface here.
| | 02:43 | It's going to cut all the way up to
there, and not through the next one.
| | 02:47 | Alright. So it's a nice way to cut up to there.
| | 02:52 | Over here, we're going to
go to Offset From Surface.
| | 02:54 | This is kind of a neat one, so I can
pick, I can face like this as my surface,
| | 02:58 | and put in something like a 0.25.
| | 03:03 | What that's going to do is
going to bring from this surface
| | 03:05 | we're going to move a quarter-inch back from it.
| | 03:08 | But it's continued to cut
using that surface. So click on OK.
| | 03:11 | If we look down in that hole,
you can see it's at an angle.
| | 03:14 | I'm going to section it just so
we can see it a little easier.
| | 03:16 | So you can see it actually followed the
contour of that original face here or the surface,
| | 03:21 | and then just brought it back a
quarter-of-an-inch; really handy.
| | 03:27 | Up to Body; we don't have any other bodies.
| | 03:29 | We only have the one body we're
cutting through at this point in time.
| | 03:32 | But if we had another body, we could
actually have it cutting through this body up
| | 03:34 | until it encountered the next body,
and then Mid Plane is the last one here,
| | 03:38 | and you can see as it cuts both directions,
| | 03:41 | now we have nothing over here to cut, so it
doesn't really make a lot of sense in this application.
| | 03:45 | But you can see we can cut in both directions
and it's just fine, we have got a hole at the end.
| | 03:49 | So that is the Extrude command.
| | 03:52 | Now, we have a couple of other options here.
| | 03:55 | I'm just going to go back to Blind.
| | 03:56 | We can go in obviously two directions if we
wanted to if we had something else over here,
| | 04:00 | and we also have Selected Contours.
| | 04:03 | So right now, we only have that one shape,
but just like we did in the past is if we wanted
| | 04:06 | to cut something else, we could totally do
that, and I'll just give you an example of that.
| | 04:10 | If I cut this away and I say Through All, it ends up with
just those sections inside of there, kind of a cool thing.
| | 04:18 | So it's cutting where
everything else besides the sketch we had
| | 04:22 | and it's actually cutting and creating three separate
pieces and now we've kept all three of those bodies.
| | 04:25 | I'm going to go back, so we don't have that, and
then the other thing here was we can add draft.
| | 04:31 | So if I put Blind, I can add some Draft
to it and as we go through these parts
| | 04:36 | or select Through All, you can see how
that draft is creating a drafted hole,
| | 04:42 | that starts big and get smaller as it goes.
| | 04:45 | Much like the Extrude command, the
Extruded Cut is straightforward and easy to use.
| | 04:50 | It is one of the most used commands,
and there is a variety pack of options
| | 04:53 | that make this a very handy feature.
| | Collapse this transcript |
| Trimming with the revolve cut| 00:00 | Creating a revolved cut is exactly
the same as creating a basic revolve.
| | 00:05 | However, this time we need something to cut
and the features act a little differently.
| | 00:09 | This command also builds on
plane creation and sketching skills.
| | 00:13 | So make sure you're up to speed.
| | 00:14 | In SolidWorks here we've got a piece of
hexagonal stock that we created already
| | 00:18 | and we're going to take this
profile here and we're going to
| | 00:22 | spin and rotate this around and
cut the end section of this off.
| | 00:26 | This would be very similar to
something we would do in a like a lathe or
| | 00:30 | turning operation in a machine shop to
actually prepare this maybe for threading.
| | 00:35 | So let's take a look at
the features it go in here.
| | 00:38 | The original piece of hex stock
I'm going to hide just for a second,
| | 00:41 | so we can just look directly at that sketch.
| | 00:43 | So here is the sketch profile,
it's really just a bunch of lines,
| | 00:47 | and we've tied to the outside of
that hex stock, came in here with a 45,
| | 00:50 | straight section, a little
thread relief and come back out here.
| | 00:55 | We have a centerline
we're going to rotate around.
| | 00:56 | Go back and I'm going to show this hex stock
again and let's go take a look at that Sketch2.
| | 01:02 | So here's our sketch, and I'm going to hide
that block one more time, so we don't see it.
| | 01:06 | So there're the inputs we've
put in there to define that shape.
| | 01:10 | Now this could be anything; it's just basic
straight lines that just create this shape,
| | 01:13 | but we have added a bunch of angles and
distances to define where they're all going to go to
| | 01:18 | and you can see we have some
Perpendicular Relationships here and some Coincidents,
| | 01:21 | so we're kind of snapping onto the
outside of that hex stock on this upper corner.
| | 01:26 | We're snapping again to that
outside of that hex stock over here.
| | 01:29 | And then we're using what's
called double dimensions up here.
| | 01:33 | Double dimensions are
created by going over a centerline.
| | 01:35 | So I'm going to delete this dimension
here and I'm going to create one for you.
| | 01:39 | So I'm going to select this line here
and I'm going to click on the centerline.
| | 01:44 | And as soon as I do that watch what happens.
| | 01:46 | As long as I'm on this side of
it, it stays a single dimension.
| | 01:50 | But as soon as I go over that centerline,
it doubles and turns into a double dimension.
| | 01:55 | See that? As I go over that centerline
; it has to have a centerline to work.
| | 01:59 | So a line to a line won't work; it always has
to go to a centerline or a construction line.
| | 02:03 | So as long as I put that in there
that just allows us to input values
| | 02:08 | as a diameter versus putting them as a radius.
| | 02:11 | Once I have my sketch looking good, click OK.
| | 02:13 | Now I've got that sketch,
which I want to revolve around.
| | 02:16 | I go up here to Revolved Cut, click on that.
| | 02:18 | The first question it's going to say
which axis of rotation we'd like to go around
| | 02:24 | and we're going to pick that centerline.
| | 02:25 | Notice as I spin that around it's going to
do a cut, click OK and there's my new shape.
| | 02:30 | I'm going to Hide that sketch and there it is.
| | 02:34 | So we've taken kind of the end of this piece
of hex stock and created it in a revolve shape.
| | 02:39 | And the next stage here we might do a threading
portion, something like that, to finish that end.
| | 02:45 | Let's go back to the Revolve Cut.
| | 02:49 | We have a few other options that we can look at.
| | 02:51 | By default we're just doing Blind, which is
going to give us full rotation of 360 degrees.
| | 02:56 | I can always just do like half of that for
instance and I'll get half of it revolved away.
| | 03:00 | That's kind of showing you how that looks.
| | 03:04 | And then also, go back in there,
| | 03:06 | I've got the options that we saw on
the original revolve as Up To Vertex,
| | 03:10 | so if we had a point that we
wanted to revolve Up To a Surface,
| | 03:13 | Offset From a Surface or Mid Plane,
so we can just do a Mid Plane cut
| | 03:17 | from that original sketch both directions,
however many degrees you wanted to cut something from.
| | 03:22 | Make sure we have a few points
here, so we can say Up To Vertex,
| | 03:27 | I can select a point and it would
go around there to cut that vertex.
| | 03:31 | So it makes a lot of sense,
you'd be able to do things like that.
| | 03:33 | Same thing with Direction 2, if I wanted to
cut in one direction and the other direction,
| | 03:38 | I can setup a certain amount of degrees that
I would like to come from one or the other,
| | 03:43 | and you can see how that preview is changing.
| | 03:45 | And then the same thing with Selected
Contours, if I had more than one shape there,
| | 03:49 | there where it's divided up, I could
choose which part of it I wanted to use to cut.
| | 03:52 | And that's exactly the same as we've
done in some of the previous features.
| | 03:56 | Once you have that, we go back to Blind.
| | 03:58 | We're just going to go on to one direction
and we'll going to change it back to 360.
| | 04:05 | And there's our feature. Revolve features
can do a lot with only a very simple input.
| | 04:09 | The basics are choose or build a
sketch and choose an axis of rotation.
| | 04:14 | Then select the degrees
of rotation and select OK.
| | Collapse this transcript |
| Trimming with the loft cut| 00:00 | The Lofted Cut command is
very similar to Standard Loft.
| | 00:04 | It can be fairly easy to extremely complex.
| | 00:07 | In SolidWorks here, I have a
base block that's been created
| | 00:10 | and I've created a sketch on the
front and back faces of this block;
| | 00:14 | my front sketch here and my back sketch
here on the backside here, and there it is.
| | 00:19 | To create a lofted cut, I'll just jump
up here to Lofted Cut, click on that.
| | 00:26 | And for my Profiles, as we've been doing
in the past, instead of choosing it from
| | 00:30 | the actual graphics window here, let's
use the tree and select the first sketch.
| | 00:34 | So Sketch2 would be my first sketch
and my second sketch would be Sketch3.
| | 00:39 | As soon as I do that, it gives me a nice little preview
of what it's going to do as far as creating that loft.
| | 00:45 | If I click on OK, as simple as that, I've
created a lofted cut through that block.
| | 00:50 | As you can see it looks pretty good, spin it
around, select Cut, and now we'll slice it in half.
| | 00:57 | So we can take a look and
see what that shape looks like.
| | 01:01 | From there, let's go back
to that Lofted Cut feature.
| | 01:06 | And notice as I create the loft, both of
those sketches are now underlying that.
| | 01:10 | So if I were to change either one of
those, so let's say I went here and
| | 01:14 | I changed this from 1.875 to 0.5, click on
OK, it updates and the loft updates as well.
| | 01:20 | If I want to change the loft itself,
I've got a bunch of different options here.
| | 01:27 | Just like with the original loft, we can
change the way that the constraints start and end.
| | 01:32 | So I can put a constraint here as far as Normal
To Profile, which will then start coming out here,
| | 01:38 | click on OK and see how that
changed the profile a little bit,
| | 01:43 | more of like a funnel going down there
and then same thing with the End Constraint.
| | 01:49 | So I can say Normal To Profile and now it changes it
to be more like a horn or an hourglass type of shape.
| | 01:57 | So I'll slice that in half,
showing me how that profile looks,
| | 02:03 | just by changing the start and end constraints.
| | 02:06 | Let's go back to that.
| | 02:09 | We also have the option for Guide Curves.
| | 02:11 | So just like we did in the original loft, we
can lay out some curves here to modify that shape,
| | 02:17 | and how we want that profile to
change as we go from one to the next.
| | 02:20 | We can have it bulge out here a
little bit or something like that,
| | 02:24 | by adding some Guide Curves, and all that
would be doing is just maybe starting on
| | 02:27 | like the right plane here and drawing
a curve or you can use the Top Plane to
| | 02:31 | draw some curves or you can add some
other planes in there to draw those out
| | 02:34 | as we came along here as far as
guiding that curve from one to the next.
| | 02:38 | A couple of other options here as far
as closing it off, showing the preview;
| | 02:41 | so I'm going to turn that one off and see what
it's going to look like when we get it completed.
| | 02:45 | We can also base things off of our centerline,
if we want it to get a little more complex,
| | 02:49 | we have that option as well.
| | 02:51 | The Lofted Cut shares most of the
same options as the original loft.
| | 02:55 | Keep in mind; you'll need a
minimum of two separate sketches.
| | 03:00 | Plan out the shape and think through
the process before you get started.
| | Collapse this transcript |
| Trimming with the sweep cut| 00:00 | A Swept Cut allows for a tool or a
profile to be used to cut along a path.
| | 00:05 | The creation process is almost
the same as with a regular sweep,
| | 00:09 | with the addition of
needing something to cut through.
| | 00:12 | On the screen, we can see we have a
rectangular block with rounded corners and
| | 00:17 | I've got two sketches here.
| | 00:18 | The first sketch is the profile of
what I want to cut, and the second one is
| | 00:22 | just the path of that edge
around the top of that shape.
| | 00:24 | I want to take this cut.
| | 00:26 | This would be very similar to
using like a router bit to cut a top of
| | 00:30 | a piece of wood or metal or something like
that to come up with some certain profile.
| | 00:34 | We can also use sweeps for
creating holes or things like that where
| | 00:38 | it would be cut through channels in a part
; a lot of different options there. Okay.
| | 00:41 | So let's go and take a look at
a couple of these things here.
| | 00:44 | The first sketch here, I'm going to edit that
sketch and I'm going to go over and look at it.
| | 00:49 | I'm going to just zoom in here, and I'm going to
turn it to wireframe, so we can see it a little easier.
| | 00:52 | So basically, I've just
got some dimensions here.
| | 00:54 | You should be very comfortable with all
these things here, those basic lines and arcs,
| | 00:59 | go ahead and create this and some
addition of some relationships showing where
| | 01:04 | and how we created these things here.
| | 01:06 | So we're snapping to the edge of the
part here with a Coincident relationship.
| | 01:10 | We've got a vertical, a horizontal. We've
got a tangency relationship on this arc here.
| | 01:15 | We've got radius, a vertical,
horizontal vertical, a tangency and
| | 01:19 | they're snapping to the top of that
part there with a couple of dimensions.
| | 01:23 | So this profile could be really anything we wanted
to, that's just where we're starting with, click OK.
| | 01:30 | Then up here, we just basically pick the
top surface, choose back to Shaded Mode.
| | 01:37 | I'm just picking the top
surface there, and starting a sketch.
| | 01:40 | So there's my Sketch here and on the top
there, I basically create the lines that
| | 01:46 | are going to go all the way round
that arc, click in the wireframe.
| | 01:49 | What I'm using here is actually if I pick that
top face, I use this one called Convert Entities,
| | 01:55 | and that brings those and just copies those edges
and we're going to cover that in a future chapter.
| | 01:59 | But we could also just lay out
using lines and arcs to go around that,
| | 02:03 | so they just snap off the outside edges.
| | 02:07 | So there is our profile, there is our path.
| | 02:09 | Let's go ahead and create that shape.
| | 02:11 | We're going to do a Swept Cut and our
Profile Sweep, we're going to pick for our profile,
| | 02:19 | it's going to be that first sketch right
here, and for our path, it's that one there.
| | 02:24 | You can see it gives us a nice
example of what it's going to look like.
| | 02:29 | Everything looks okay,
click OK, and there we go.
| | 02:32 | You can see how that part looks,
you get that nice rounded corner here,
| | 02:39 | a couple of other things,
a nice decorative part.
| | 02:40 | This might be like a nice piece to
start as a metal part for the base of
| | 02:45 | some machinery or some thing you
might be creating. Looks pretty nice.
| | 02:48 | Underneath the Swept Cut, let's take
a look;, we've got a few options here.
| | 02:53 | We've got Follow Path, as far
as how you want to use that.
| | 02:55 | We've got a bunch of other options here.
| | 02:57 | We can have other curves, and
Guide Curves and stuff that we want
| | 03:01 | to twist things along the path if we needed to.
| | 03:03 | So some more complex things we can look at.
| | 03:06 | Same thing with Twisting, direction
vectors; we can change things along here.
| | 03:10 | The Guide Curves also, we can
add-in more curves if we want to,
| | 03:14 | to control how that shape might change
as it goes through the different paths.
| | 03:18 | And same thing with Start and End Tangency;
this is how we're going to start from that part.
| | 03:23 | Now we're starting on a flat surface,
or starting like on that front plane.
| | 03:26 | So that's not going to have much effect on
this one, but we could adjust the tangency here
| | 03:31 | if we needed to, just turn it
off and on, or Path Tangent.
| | 03:35 | But those are two options here, but
it's not really going to change anything.
| | 03:37 | Other than that, that's
pretty much the Sweep command.
| | 03:41 | The Swept Cut command can be very useful
and is great for creating special features.
| | 03:46 | To create a swept cut, we
need a profile and a path.
| | 03:50 | These two sketches cannot be on the same plane,
| | 03:52 | and have to have an orientation
that allows the shape to be built.
| | Collapse this transcript |
|
|
9. Refining GeometryUsing fillets and chamfers to create smooth or angled corners| 00:00 | Rounding or beveling of sharp corners
is used extensively in product design and
| | 00:05 | SolidWorks has provided an easy-to-
use interface for applying either one.
| | 00:09 | Rounding is called adding a fillet
and beveling is called adding a chamfer.
| | 00:14 | The most basic type of fillet
is called the Edge Fillet and
| | 00:17 | is created by selecting one or more
edges and choosing the desired radius.
| | 00:21 | In SolidWorks here we have a part we're going to
add a bunch of different fillets and chamfers too.
| | 00:27 | So I'm going to jump up here to Fillet and
notice there is a dropdown that adds a chamfer.
| | 00:30 | Fillets and Chamfers are
added almost exactly the same way.
| | 00:32 | So on a Fillet, I'm going to
start with Constant radius.
| | 00:36 | My very first fillet I'm going to
add is just right here at this edge.
| | 00:38 | So I'm going to select that edge, and
I can put in whatever radius I want.
| | 00:43 | I'm going to leave it at 0.375, and click on OK.
| | 00:46 | I'm going to say Full Preview, showing me
exactly what that's going to actually do for us.
| | 00:51 | Click on OK, and that's my
first fillet. Pretty simple.
| | 00:54 | I'm going to try that again.
| | 00:57 | This time I'm going to change it to 0.25
radius, and continue to use the Constant radius,
| | 01:02 | and so I'm going to use an inside of a hole,
| | 01:06 | and there's a nice little fillet of that hole.
| | 01:08 | So you can see how that works.
| | 01:11 | Going back to Fillet, I'm going to click on
the Variable radius one, which is the next one.
| | 01:16 | And on the bottom of the part here,
I've got this edge I'm going to fillet,
| | 01:19 | and the Variable radius allows me to start at
one side of the fillet edge with a bigger radius,
| | 01:25 | and I can change it to a
smaller radius on the other side.
| | 01:26 | So I'm going to click in this box
here; I'm going to type in 0.375.
| | 01:32 | I'm going to click in this box here to 0
.05, so I'll make it a little smaller.
| | 01:36 | As soon as I click out of that, it should
give me a preview of what I'm going to see.
| | 01:40 | Click OK, and there's that Fillet.
| | 01:41 | I also have the option of going
back to that one and changing,
| | 01:45 | do I either want a Smooth transition
or do I want a Straight transition?
| | 01:48 | Clicking on that gives me a nice little
straight conversion from big to small.
| | 01:55 | On the Fillets here, we're going
to continue on with a Face Fillet.
| | 01:58 | I'm going to spin that part around
and take a look at the other side here.
| | 02:00 | There it is, and I want a
nice fillet in this edge here.
| | 02:04 | So I'm going to pick a series of faces.
| | 02:06 | So the face that I'm going to use is this
face here and that face there and that one.
| | 02:10 | And then for the bottom face I'm
going to pick this one. Click OK.
| | 02:13 | That's a nice little fillet in
that corner for us. Looks pretty good.
| | 02:17 | Jump into Fillets some more, and this
is going to be the Full round fillet.
| | 02:21 | That's a combination of three faces.
| | 02:23 | So I'm going to use this edge of
the part here for creating that.
| | 02:25 | I'm going to pick this as my
first face, jump into the next box,
| | 02:29 | this box, and the bottom one,
I'm going to pick the bottom face.
| | 02:32 | It gives me a preview of what's going to happen,
Click OK, and that's the Full round fillet.
| | 02:37 | Now, instead of creating
fillets in the solid form,
| | 02:42 | we can also go back and
add fillets into the sketch.
| | 02:44 | I have a sketch kind of laid out here.
| | 02:46 | I'm going to open up that
sketch and click on Normal To.
| | 02:51 | So I also have a fillet
command I could add to this sketch.
| | 02:54 | I'm going to jump into the
sketch window and grab Fillet.
| | 02:57 | I'm just going to put in 0.25 and then just
pick the corners, or you can pick a pair of faces.
| | 03:02 | I'm going to pick the corner first,
and then I'll pick the pair over here.
| | 03:05 | So either way, it allows you
to fillet out those corners.
| | 03:08 | As soon as you're happy with
what it looks like click on OK,
| | 03:10 | and then I have filleted corners here,
so when I go ahead and extrude that,
| | 03:18 | you can see that though the edges
were already filleted before that,
| | 03:21 | we could add them before in the
sketch or during the sort portion of it.
| | 03:25 | I'm going to switch over
to the Chamfer Mode now.
| | 03:28 | So I'm going to click on Chamfer,
and Chamfer is almost exactly the same.
| | 03:31 | It just allows you to use an angle or distance.
| | 03:34 | 45 is kind of the default here.
| | 03:36 | So I can either pick an edge itself to Chamfer,
or I can pick something like a whole face.
| | 03:41 | That's a Chamfer of the entire face; all
the outside edges of something like that.
| | 03:47 | And it works the same
thing with the Fillet command.
| | 03:49 | So if I wanted to Fillet or Chamfer something,
| | 03:52 | I can either pick an edge or a whole face.
| | 03:53 | So if I go up here to
Chamfer and I pick this Face,
| | 03:57 | it will chamfer all these inside
edges as well as the outside edges.
| | 04:02 | So all edges of that outside
face will be chamfered or filleted,
| | 04:05 | depending on how we pick
up and use those options.
| | 04:09 | As you can see, that's pretty much what
we've got as far as our options under the Fillet.
| | 04:13 | And jump out of that, and same thing with the
Chamfer, we've covered most of the things here.
| | 04:18 | The only thing we might want to look at
now is if I wanted to change the angle here.
| | 04:22 | So if I change that to like a 30
degree angle, for instance, 30 degrees,
| | 04:27 | makes something like this, like the top
of that part, and it changes the angle,
| | 04:30 | so it's a little bit
steeper going around that part.
| | 04:33 | We can also always go back and change any one
of these features to make it a little bit bigger.
| | 04:41 | Fillets are used extensively in many designs
| | 04:44 | and many times make up the majority
of the features in the design tree.
| | 04:48 | This is especially true
with molded plastic parts.
| | 04:51 | Fillets are easy to apply.
| | 04:52 | However, keep track of how you apply the
Fillets to get the optimal design, look and feel.
| | Collapse this transcript |
| Creating repeating rectangular patterns| 00:00 | Patterning is one of the most
efficient and powerful commands in SolidWorks.
| | 00:05 | Features, Bodies or Surfaces can be patterned
and there's no limit on the number of instances.
| | 00:11 | To get started, we need to select the features
and/or set of features we would like to pattern.
| | 00:16 | Next we need to select the First Direction and the
Number of Instances of that pattern, then the spacing.
| | 00:22 | If we want a pattern in one
direction we're ready to go.
| | 00:25 | However, if we'd like a Grid pattern,
like a set of holes or a vent for instance,
| | 00:29 | we need to select a second direction.
| | 00:33 | Directions are chosen by selecting any edge or line
that goes in the direction that we'd like to pattern in.
| | 00:38 | On the screen here I've got a
plate, with a Boss-Extrude and
| | 00:42 | I've got one Cut feature in there and that Cut
feature is what we want to pattern along here.
| | 00:47 | So I'm going to go up here to Linear Pattern,
| | 00:49 | click on OK and my first
direction I want to pattern in is,
| | 00:53 | you know I can pick any edge that's
going to be going in that direction,
| | 00:56 | so like this edge up here or that
edge or this edge or any of those edges,
| | 01:00 | I could use or can actually draw a line here,
if there's some other direction I wanted to go.
| | 01:05 | But I'm just going to go along this edge here.
| | 01:06 | So I'm going to click on that edge and
there it is, so that's Direction 1 and
| | 01:11 | it's giving me a Spacing of 0.
10 which is probably too small.
| | 01:14 | So I'll give it like a, 1 inch Spacing, so
1.0 (1.00in) and then how many do I want?
| | 01:18 | So I want to go, make sure that we're
going the right way and I'm going to make sure
| | 01:26 | we turned the Preview On of what
we're actually going to see here, okay.
| | 01:32 | The next thing we need to do is
actually select what thing we want to pattern.
| | 01:35 | So the feature that we
want to pattern is that hole.
| | 01:37 | So go up here, click in the
Features to Pattern and grab that hole.
| | 01:40 | Now you can see I've got three of those,
make sure that I pattern one direction,
| | 01:46 | I can change the Spacing,
I can change the Quantity.
| | 01:49 | Click on OK and there's our first pattern.
| | 01:51 | Now if we wanted to go in another
direction, I can go back to that Pattern
| | 01:55 | and Edit it and I can go into Direction 2 now.
| | 01:59 | Direction 2, I just pick any other Vector
or a Line, so these two lines might be good,
| | 02:03 | either one I could choose.
| | 02:05 | Pick that and then I want to make
sure we're in the right box here.
| | 02:10 | So pick that line and as our direction vector.
| | 02:13 | And how many Instances we'd like?
| | 02:14 | We want two, and then notice as I
change that, it keeps moving out,
| | 02:19 | so I get a nice little pattern of parts here.
| | 02:23 | I can continue to add more of
those Instances across there.
| | 02:29 | Click on OK and there it is,
just that simple, a linear pattern.
| | 02:33 | Now if I wanted to add something to this, I
could go ahead and like click on the top of this.
| | 02:36 | Double-click and I'm going to go add,
just a simple sketch of like a hole.
| | 02:42 | I'll put a hole just right next to this one.
| | 02:45 | There's our hole, it's a little
bit hard to see but there it is and
| | 02:50 | I could define it if I want to, but I'm just
going to exit out of that sketch right now.
| | 02:53 | So there's my little hole pattern and
I'm going to go ahead and make a cut.
| | 02:57 | So I'm going to cut through that,
Extruded Cut and we'll say Through All. Click OK.
| | 03:02 | So now I have a hole next to my other hole
and if I wanted to add that to the Pattern,
| | 03:06 | it's just as simple as going to this pattern.
| | 03:09 | The problem that we have here is the
pattern's first and then there's the hole.
| | 03:12 | Alright so, we actually have the
ability to reorder these items,
| | 03:15 | just by grabbing that and
dragging up a little bit above it.
| | 03:18 | So now the hole is before the pattern and
that's called a Parent-Child Relationship.
| | 03:23 | So this hole needs to be before
what's going to be using it in that tree.
| | 03:27 | So we have the ability to
reorder these items here.
| | 03:29 | Now I'm going to go to the
Pattern here and I'll say Add and
| | 03:32 | go down to the Features
and just click on that hole.
| | 03:35 | We're going to add that hole to it and
notice just like that we added something
| | 03:39 | to the pattern and it
patterns it all the way across.
| | 03:42 | Patterning can be a huge timesaver and
the Pattern Features can be easily adjusted.
| | 03:46 | Patterning can be done in the Sketch-mode;
| | 03:49 | however that creates large complicated
sketch, that's much harder to work with.
| | 03:54 | I always recommend keeping your
sketches as simple as possible and patterning
| | 03:58 | and mirroring on the bodies and
features rather than sketches.
| | 04:01 | The results will be the
same and there are no rules.
| | 04:04 | However, Feature Level
Patterns are much easier to work with.
| | Collapse this transcript |
| Creating repeating circular patterns| 00:00 | The Circular Pattern is much
like the Rectangular Pattern.
| | 00:03 | However, we need an axis
rotation versus a direction.
| | 00:07 | We can choose features or bodies, the
number of instances and the angle between them.
| | 00:12 | On the screen here, you see we've
got a pipe with a piece of flange
| | 00:16 | maybe welded on there; we want to
add some bolt holes to that flange.
| | 00:20 | So I've already created a
sketch here to lay out my first hole.
| | 00:23 | I'm going to jump into that
sketch and show you how it's created.
| | 00:26 | I'm just using a 8.25
diameter for this layout circle.
| | 00:31 | I've got it tied into the origin so that was
directly vertical above the origin and I've got a size.
| | 00:37 | From there, I'm going to go ahead and
extrude cut that out through that flange
| | 00:42 | and I'm going to say Up To Next.
| | 00:43 | Let's make sure it goes all
the way through and there it is.
| | 00:46 | Now we want to take this feature we just did
and cut and we'll revolve it around that face.
| | 00:51 | So to do so, I need an axis
of rotation and that feature.
| | 00:55 | So let's go under Linear Pattern,
there's a Circular Pattern, click on that.
| | 00:59 | Okay and Circular Pattern, I need
to choose something to spin around.
| | 01:03 | I can actually click up here under
View and say show Temporary Axes and
| | 01:08 | notice I get an axis in the center, and I
also get a little one in the center of that hole.
| | 01:11 | So my rotation axis is going to be this.
| | 01:14 | As soon as I click on that, notice it
gives me a pattern going around there.
| | 01:17 | Now this is going through 360
degrees and there are eight of them.
| | 01:20 | Now I could change that if I wanted to.
| | 01:22 | I could say like 180 and that way it
will only pattern half way around it or
| | 01:26 | I could do 60 degrees if I wanted to,
change that around as much as I wanted and
| | 01:31 | change how many of them there are.
| | 01:34 | We do want 360 for this example,
and I do want 8. There's my 8.
| | 01:39 | And the other thing I have is Equal Spacing.
| | 01:41 | So if I didn't have Equal Spacing, I
could change the degree between each one
| | 01:45 | and however many I wanted.
| | 01:46 | So if I change the degrees, I
keep going around and around here.
| | 01:49 | But for this one, we're
going to use Equal Spacing.
| | 01:52 | Here's the features to pattern, so inside of
there we already have that feature selected but
| | 01:56 | if we had multiple features that we wanted to
continue to pattern around here, we can choose those there.
| | 02:00 | We also have the option to Pattern Faces or even
Bodies, but we're not going to that in this example.
| | 02:06 | Instances to Skip, if I
wanted to remove one of these,
| | 02:10 | I could just click on one of these little
purple dots to remove those from the pattern
| | 02:15 | and notice they show up here as far as 2 or 3.
| | 02:17 | We want to bring it back to
select it here and hit Delete,
| | 02:20 | which will take it out of that
box and bring it back to the screen.
| | 02:23 | Okay, it gives a nice
example of what we want to do.
| | 02:27 | Click up here, close that up and
click OK and there's our pattern.
| | 02:31 | Now the pattern is quite easy to change as well.
| | 02:34 | I can just click back on it.
| | 02:36 | I can add more holes, remove
holes, or whatever I need to do.
| | 02:40 | So it's very easy to go back and change and
also I can go back and change that original sketch.
| | 02:45 | If I change that size from 1 inch
to .875, make it a little smaller.
| | 02:47 | It doesn't matter, the pattern continues to use
whatever that original feature was to pattern it around.
| | 02:58 | The Circular Pattern, by far, is
my favorite feature in SolidWorks.
| | 03:00 | It is simple to use and the results are awesome.
| | 03:04 | Play around with the various
combinations of instances, angles,
| | 03:08 | or either simple bolt holes
or wild creative patterns.
| | Collapse this transcript |
| Mirroring objects| 00:00 | Mirroring is the best way to
double or quadruple your efficiency.
| | 00:04 | Look for part symmetry; if the right-
hand and the left-hand side look the same,
| | 00:08 | let's mirror it, save yourself
some time and make better parts.
| | 00:13 | In this example, we're going
to take a look at this block.
| | 00:15 | It's got four holes in the
corners; it's pretty straight-forward.
| | 00:18 | We've got a Boss feature,
created from one Sketch.
| | 00:20 | Let's jump in there and take a look.
| | 00:22 | Now there's nothing technically wrong with
this; everything is fully-defined and black,
| | 00:28 | there's dimensions, and it looks pretty good.
| | 00:30 | However, we can be a lot more efficient in
our design if we think through a few of these.
| | 00:35 | Look at these dimensions here,
three-quarter of an inch (0.75),
| | 00:37 | three-quarter of an inch over here, and here.
| | 00:39 | We're using that same dimension four times.
| | 00:41 | Any time you're seeing a dimension more
than once in your drawing it's too many.
| | 00:45 | Let's go ahead and delete those,
delete, and delete, and delete.
| | 00:49 | Let's go ahead and add an equal relationship
so this one dimension here controls all four.
| | 00:58 | Select Ctrl, select all four of those,
by holding down Ctrl and say Equal.
| | 01:01 | Now all four of those are
controlled by this one dimension here.
| | 01:06 | Same thing over here, 1 inch,
1 inch, 1 inch, and 1 inch.
| | 01:09 | We're using that to space this off
the corner of the part. Why do it?
| | 01:12 | Let's delete this, delete
that, and delete that one.
| | 01:15 | I'm going to now add a Centerline,
just from this edge of the part or that
| | 01:23 | little spacing to there and then add a
relationship that says this center point here,
| | 01:27 | hold down Ctrl and select
that line, is at the midpoint.
| | 01:30 | Now that controls that and the
last thing we do want to do is,
| | 01:34 | we still have some leeway
this way, so we want to make sure
| | 01:37 | that the spacing here is
the same as it is up here.
| | 01:39 | I can do that by adding more centerlines.
| | 01:41 | Let me make a centerline out to the
edge, and then one more up to the top.
| | 01:46 | I'm just going to make
those two centerlines equal.
| | 01:52 | Now by just one dimension
here I can control the spacing
| | 01:55 | from the edge of the part to
the centerline of the holes.
| | 01:58 | I can control the diameter of the hole
by this three-quarter inch in the size.
| | 02:02 | But if you look at this part, the left-hand
side here is the same as the right-hand side,
| | 02:07 | the upper portion is the
same as the lower portion.
| | 02:09 | So we're doing a lot more work than
we need to; we're drawing four holes.
| | 02:12 | We can really just draw one-quarter of
this thing, this one hole and the shape here.
| | 02:16 | So let's go take a look at another example.
| | 02:18 | So this is almost exact same
part, but just one-quarter of it.
| | 02:24 | If I look at the Sketch
underlying here, it's a simple hole and
| | 02:32 | we've just got a couple of
these little centerlines here with
| | 02:34 | an equal relationship and a
three-quarter of diameter here.
| | 02:37 | So it's very easy to change, very simple,
very straight-forward, very easy to create.
| | 02:41 | All I did was create a rectangle,
one hole and two centerlines;
| | 02:45 | very straightforward, very easy.
| | 02:46 | Once I have that part there, I'm going
to use the Mirror Command to compound it.
| | 02:51 | Hit the Mirror.
| | 02:51 | The first question it's going to ask is,
which Mirror Plane do I want to mirror over?
| | 02:56 | Now I can either choose a Face or
a Plane, let's use this face here,
| | 03:01 | and then it's going to ask me, do I
want a Feature Mirror, a Face Mirror,
| | 03:05 | or a Body Mirror? There's
three different options here.
| | 03:07 | A Feature Mirror, which is the default, is
the most common type of mirror, which would be
| | 03:11 | like if you had a hole here and you wanted
to mirror it to another section of your part.
| | 03:15 | However, we want the entire part,
we don't want just that hole.
| | 03:19 | We want the whole body, so I'm
going to jump down here to Body Mirrors,
| | 03:22 | and the Body Mirror could be
made up from one feature or
| | 03:25 | it could be made up from hundreds of
features that went into to create that body,
| | 03:27 | and I can mirror all those over in
one shot just by selecting that body.
| | 03:30 | As soon as I do that it gives
me a nice preview, click OK,
| | 03:34 | and I've doubled the part
and it's exactly the same.
| | 03:37 | Now click on Mirror one more time, this
time I'm going to mirror this face here
| | 03:40 | so I'm going to select that
face, and as far as the body,
| | 03:43 | I'm just going to pick this entire body here.
| | 03:44 | Click on it, and there it is.
| | 03:47 | The same part, whether we look
at original part or this part,
| | 03:52 | at the end of the day, they're the same.
| | 03:53 | However, they're really not, right?
| | 03:55 | Because this part is much simpler to make,
and if I want to make a change to this,
| | 03:59 | all I have to do is change that one section
or that one quadrant to easily make an update.
| | 04:04 | So let's go ahead and try that out.
| | 04:05 | Click on Sketch and edit that.
| | 04:09 | Say we wanted to add one additional
hole or maybe a square hole, so this time
| | 04:12 | we're just going to click on a 2 Point
Rectangle, I'm going to add a square hole here.
| | 04:18 | Now if I was going to do this in the
other part, I would have to add four
| | 04:21 | rectangles and I'd have to
add dimensions four times.
| | 04:24 | So I'm going to say, 1.0 inches here,
let's add a couple of dimensions to the edges
| | 04:29 | if I wanted to or I could even use
some centerlines as well if I wanted there
| | 04:33 | and then just a couple more
just to define that shape.
| | 04:35 | So I'm doing it one time versus having to do
these things four times. Lay out that part.
| | 04:45 | There is my hole, there
are the controlling arms.
| | 04:47 | Now I could even get rid of
this one here like I said,
| | 04:49 | if I just want to make a couple of
constructions going back to the edge.
| | 04:52 | Now here is the magic.
| | 04:53 | As soon as I delete or
get out of this sketch here,
| | 04:58 | that square hole has now
propagated across all four,
| | 05:00 | because I used that Body Mirror feature, so
this entire original body was copied over.
| | 05:06 | There's my original body, I mirrored over once,
| | 05:08 | it takes everything that was
originally there and the same thing over here,
| | 05:11 | everything I had originally on
this side is now on this side.
| | 05:13 | So it's a very powerful feature,
especially if you want to add or modify.
| | 05:16 | Mirroring is a great time-saver and it makes
modifying and updating parts quick and efficient.
| | Collapse this transcript |
| Creating hollow objects with Shell and Draft| 00:00 | The Shell command takes a solid
and turns into a thin-walled feature.
| | 00:04 | This is used a lot in molded parts.
| | 00:06 | This feature can do amazing
things with just a few clicks.
| | 00:09 | Before we shell this part I
want to add some draft to it.
| | 00:13 | Draft is when we add some angularity to
the outside faces or inside faces of a part.
| | 00:18 | So if it's molded, we can
easily release from the mould.
| | 00:22 | We generally assign this as an
angle of maybe three to five degrees,
| | 00:26 | and sometimes as low as maybe a half degree,
depending on the circumstances of the molded part.
| | 00:30 | So to add the draft angle
let's go ahead and click on Draft.
| | 00:34 | We're just going to use the basic
type, which is the Neutral Plan Draft
| | 00:39 | and the Draft Angle is specified here.
| | 00:42 | This is going to be how much the
part is actually going to angle in,
| | 00:45 | from the top side to the bottom side,
as it progresses through the draft.
| | 00:50 | The Neutral Plane is going to be the
face where we start that draft from.
| | 00:53 | I'm going to click there.
| | 00:54 | And then I'm going to pick on the Faces Draft.
| | 00:56 | I'm going to pick this
face, that face, that face,
| | 00:58 | spin the part around and
grab this back face here.
| | 01:01 | As I click on OK notice what happens.
| | 01:05 | The top of the part, if we
look at the side of the part here,
| | 01:08 | the top is skinnier and now it
gets wider as it gets to the bottom.
| | 01:11 | That's exactly the opposite of what we wanted.
| | 01:13 | We want it to be skinnier at
the bottom and wider at the top.
| | 01:15 | So let's go back to Draft and
click on this Reverse Direction.
| | 01:21 | And notice that's going to now make
the bottom of the part slightly skinnier.
| | 01:25 | That'll make it easy to pull that part out of the
mold and makes that little bit easier to work with.
| | 01:30 | Now we're ready to turn this part and
do a shelled part, but before we do that
| | 01:34 | we just need to add one more
little Fillet on the top corner here.
| | 01:37 | So let's just go ahead and grab a 0.25 Fillet
and grab any of these edges and select that chain.
| | 01:43 | Fillet out top of that part
and now we're ready to shell.
| | 01:46 | Inside the Shell command, it's going
to ask us for how Thick we would like to
| | 01:51 | make those walls and number two,
what faces we would like to remove.
| | 01:56 | So right now I'm just going
to remove just that top face.
| | 02:00 | Click OK and there it is.
| | 02:02 | We've got our first shelled part including the
Draft Angle we added to
the outside of that part.
| | 02:06 | I'm going to section that part in half.
| | 02:10 | Take a look here; we've got a nice
uniform wall thickness throughout the part.
| | 02:14 | Let's go back and play with
the shell command a little bit.
| | 02:20 | This time I'm going to go and add
some more of these faces to be removed.
| | 02:24 | This time I'm going to select in here
and I'm going to and add this face now.
| | 02:29 | Click OK and that's going to remove
that and take it right down to the base.
| | 02:31 | So any face I select it's going to
remove it from that shell feature.
| | 02:36 | Go back one more time.
| | 02:37 | This time I'll remove this Edge
over here, this Face over here.
| | 02:42 | And now I remove that as well and we've
got a nice uniform wall thickness part,
| | 02:45 | which I can remove any faces I'd like to
make a part that'll be very easy part to mold.
| | 02:51 | Shelling a part gives us the ability to
quickly create a part with uniform wall thickness
| | 02:55 | and is an amazing tool
for building complex parts.
| | Collapse this transcript |
|
|
10. BlocksWorking with reusable sketches using blocks| 00:01 | Imagine that you spent all day
working on designing the cutouts for a
| | 00:04 | motherboard on a new computer case.
| | 00:07 | If you'll be using that same
motherboard in other designs, why not create a
| | 00:10 | block to be able to easily
reuse that sketch geometry?
| | 00:14 | Blocks are independent, non-solving
sketches that can be used in a variety
| | 00:19 | of ways in SolidWorks.
| | 00:21 | The most common would be to copy a
sketch to be used elsewhere in your design.
| | 00:26 | By creating a block, all of the
entities in the block become frozen and can be
| | 00:30 | manipulated as a whole.
| | 00:32 | We can save blocks for later use, as well
as open blocks in the SolidWorks format
| | 00:36 | or any AutoCAD format
such as a DWG or a DXF file.
| | 00:41 | To insert an existing block, we first
need to locate it on our file system.
| | 00:44 | In SolidWorks, the first thing what we like
to do is actually add in the Blocks toolbar.
| | 00:49 | To do that, go up here in the
right-hand side in the gray area and right-click
| | 00:53 | and come down here to the Blocks toolbar.
| | 00:55 | Just turn that one on.
| | 00:56 | Notice it drops it here. I want to
place it right up here in this upper corner.
| | 01:00 | The first one would be to make a block,
which we'll do in the next movie, and then
| | 01:03 | the second one here would be to
insert a block, so I'll click on that.
| | 01:07 | As soon as we click on that, we get the
option to go ahead and browse to that
| | 01:11 | block. And in my file system, I have
it here, under Exercise Files, and we're in
| | 01:17 | Chapter 10, and then we have Blocks.
| | 01:20 | So I have a bunch of different
blocks here we can play around with.
| | 01:22 | And then what we're going to use is
this last one here called VGA-Cutout.
| | 01:24 | So go ahead and click on that.
| | 01:27 | Notice as soon as I open that block, it
actually attaches to my cursor and then
| | 01:32 | where I drag my cursor around,
| | 01:33 | I have the ability to place that block.
| | 01:34 | Now I'm just going to place it one time
and then once we place it one time,
| | 01:38 | it continues to stay attached to the cursor.
| | 01:40 | I can place it again and
again throughout my design.
| | 01:45 | Also, while I'm working with it, I have
the ability to increase its size or scale
| | 01:50 | factor, so I can scale the block.
| | 01:52 | I can also rotate this
block by typing the stuff in.
| | 01:55 | So I can place another
instance of that same block.
| | 01:58 | It's the same block; it's just
this one has a rotation and a scale
| | 02:02 | factor applied to it.
| | 02:03 | As soon as I'm done with that, I
click on OK, and there are my blocks.
| | 02:06 | Now you could see underneath that
sketch, I've got a bunch of different ones
| | 02:10 | here that are placed.
| | 02:12 | Now if I go in and edit one of these
blocks, so if I click on the block itself,
| | 02:16 | I can add relationships to them, like
Horizontal or Vertical to orient it.
| | 02:20 | We can then also place
dimensions to place it in our sketch.
| | 02:24 | I can also click on Edit.
| | 02:25 | So if I edit this block, notice all the
sketch entities now become active and I
| | 02:31 | can go ahead and maybe add a dimension.
| | 02:34 | So right here it says 0.152.
I'm going to change it to 0.25.
| | 02:37 | As soon as I do that, look what happens.
| | 02:40 | Not only does this one change,
but so do all the other ones.
| | 02:44 | Now even though these are smaller,
they're not scaled. This is 0.25, and
| | 02:48 | that's scaled 2.3 times.
| | 02:51 | So anything I change in this one is
going to change all the other blocks and so,
| | 02:54 | the same thing if I change
any one of the other ones.
| | 02:56 | They will all be changed exactly the same way.
| | 02:59 | So if I edit that, notice that
0.25 now is part of that block.
| | 03:03 | So we've edited the block as a whole and
then we've copied it throughout the design.
| | 03:07 | We can also go back and add other blocks
if we want to, by just clicking here and
| | 03:12 | selecting more blocks to bring them in.
| | 03:14 | Just go to the same Exercise Files,
grab those blocks, and here's a bunch of
| | 03:18 | different things that we can take a look at.
| | 03:19 | So we can snap things on to bring
in like an AngleSlot or a Drill.
| | 03:24 | Now here's another block I can
just place anywhere I want.
| | 03:27 | So you can have as many blocks as you
want. And then each one these blocks can be
| | 03:31 | operated on over here.
| | 03:32 | If I right-click on it, I can edit
the block. I can save the block out.
| | 03:36 | If I change that block at all, I could
then save it as a different name, back to
| | 03:39 | the file system, which can
be then used somewhere else.
| | 03:42 | I can even explode a block.
| | 03:43 | So if I click on, say, this one here, if I
didn't want this to be a block anymore,
| | 03:48 | I can just right-click on
it and I can say Explode.
| | 03:51 | Now that turns that back
into regular geometry.
| | 03:55 | Notice this dimension change as well,
because it applied that scale factor.
| | 03:59 | Now anything I do here to change this
around, it's no longer a block, so it's
| | 04:02 | not going to affect the other items here.
| | 04:04 | If I wanted to turn it
back into a block, I could, and
| | 04:06 | save it back to the system. And we'll
learn how to create blocks in the next movie.
| | 04:10 | Blocks allow the designer to reuse sketches.
| | 04:13 | If you have designed the perfect connector
cutout, why sketch it out every single time?
| | 04:17 | Save yourself some time and create
a block and then reuse that asset
| | 04:20 | throughout your design.
| | 04:21 | SolidWorks can leverage AutoCAD files,
if you're working with other systems, and
| | 04:26 | turn them into usable geometry as well.
| | Collapse this transcript |
| Creating blocks| 00:00 | Reuse of sketches is one of the best ways to
save time and be more efficient in SolidWorks.
| | 00:06 | Creating blocks is as easy as
selecting the elements and choosing Make Block.
| | 00:10 | We can then use that block in other sketches.
| | 00:13 | On the screen I've got some cutouts for
a motherboard, and we've got like a DVI
| | 00:19 | and HDMI and some USB ports, Ethernet
ports, some audio jacks that have all kind
| | 00:23 | of been laid out here.
| | 00:25 | Now I can take this and turn it into a
block and we can easily reuse this data in
| | 00:29 | another sketch or another feature.
| | 00:32 | To do so, let's make sure we got the
block toolbar turned on. If we don't, just
| | 00:35 | right-click in the gray area and
make sure the Blocks is turned on.
| | 00:39 | And then the first thing
here is called Make Block.
| | 00:41 | Click on that. It allows us to go here
and select which items I want to include.
| | 00:45 | So I'm just going to window around all
these, select OK, and notice it gives
| | 00:50 | us all the entities that are going to be there.
| | 00:51 | The next thing is Insertion Point.
| | 00:54 | So click here and it's a little manipulator.
| | 00:56 | I can just drag this around. I am just
going to snap that to my origin right now.
| | 01:00 | That's going to be cut on the
tool tip when I import that block.
| | 01:02 | Once you are happy with what you have
selected, click on OK, and there it is.
| | 01:07 | We have got now Block1-1, and we can now
manipulate this and move this around our
| | 01:12 | sketch if we wanted to, or we can go
out and save it out for file system. So
| | 01:16 | let's right-click on that, Block1, and
say Save Block. And I have a folder called
| | 01:25 | Chapter 10 in Blocks, but you can
really save this in just about anywhere you
| | 01:28 | want on your file system.
| | 01:30 | In fact, sometimes I would recommend, if
you're using blocks in an organization,
| | 01:33 | and you have a certain cutouts or
different features you might want to share
| | 01:36 | throughout your organization, put it on
file server, call it blocks, and then you
| | 01:40 | can use it any way you like.
| | 01:42 | So I will just go ahead and just say
New and save it out, and there it is.
| | 01:48 | So now I have a new block that's saved
out to the file system, and I'm going to
| | 01:51 | now go open up this file here, which is
10.2. And this is just a sheet of material
| | 01:59 | that we are going to add
that block to it to make a cutout.
| | 02:01 | So let me click on that Top Face, click on
Normal To, and I am going to start with Sketch.
| | 02:06 | As soon as I am in the sketch, I am going to
go over here and say Insert the Block.
| | 02:11 | And I'm going to Browse for block
and it happens to be on the Desktop, under
| | 02:15 | Exercise Files, Chapter 10, and inside
Blocks and there it is, the new file we
| | 02:20 | just saved. Click on OK.
| | 02:22 | Then as soon as I do that,
it attaches to my cursor.
| | 02:26 | I can drop it anywhere I want.
| | 02:27 | I am just going to put it in the center
here. And I could add more if I wanted to,
| | 02:31 | or just hit Escape to turn it off.
| | 02:32 | Now I can add some dimensions, so I
am going to dimension from this edge to
| | 02:36 | that circle. And I want to dimension
one more from there to the bottom to place
| | 02:42 | that, and notice as I'm doing these,
that the whole block is moving as I am
| | 02:47 | changing those dimensions.
| | 02:48 | It's operating on it as a whole.
| | 02:50 | As soon as I am happy with my
dimensions, everything looks good,
| | 02:52 | I am just going to go ahead and go to
Features > Extruded Cut, spin it around and
| | 02:57 | can see what's going to happen there. And I
am going to say Through All and click on OK.
| | 03:01 | We have just added that connector cutout
quickly to another sheet, and there it is.
| | 03:06 | By creating blocks we can save a lot of time.
| | 03:09 | Blocks can be saved to a central
file server and used throughout your
| | 03:12 | organization, or saved to your
local library for easy access.
| | 03:16 | Additionally, if you are working
with imported data, like AutoCAD files or
| | 03:20 | exported files from graphics programs,
blocks can make it easy to get those files
| | 03:24 | into SolidWorks, and easy to work with.
| | Collapse this transcript |
| Designing with blocks| 00:00 | Blocks can be used to lay out mechanisms.
Then the sketch serves as a skeleton
| | 00:04 | to build the parts.
| | 00:06 | Take a look at this example.
| | 00:08 | What we have a sketch here with the
mechanism for like a forklift-lifting device;
| | 00:13 | it's more of a four-bar mechanism here.
| | 00:15 | And so what I can do is I can turn each
one of these elements into a block, and
| | 00:20 | we can see how they operate
together. Let's try it out.
| | 00:22 | So this first section here would be
like the lifting mechanism. Let's go ahead
| | 00:26 | and select all those items there,
and we're going to say Make Block.
| | 00:30 | As soon as I do that, just click OK.
Now we have a block there at that front
| | 00:33 | section. It turns gray. I have Block14-1.
| | 00:37 | These two mechanisms are the two
lines here. Click there, click there, select
| | 00:41 | those, and say Make Block.
| | 00:43 | Now we need to make an independent block of
each section of our design.
| | 00:49 | So this one and this one are
going to be in another section.
| | 00:51 | I am going to say Make Block, click on
OK. This little wheel here, we're
| | 00:58 | going to turn that into a block itself,
click OK and then the line here and just
| | 01:03 | say Make Block, so they
are all independent blocks.
| | 01:06 | Then we need to tie a few things down. So
the points we don't want to move we want
| | 01:10 | to add a relationship, like an anchor,
so just fix that end point and we'll fix that
| | 01:14 | end point there, and let's also fix the
centre of that one so it doesn't move.
| | 01:18 | Let's see what happens.
| | 01:19 | Notice as I move this thing around,
this block actually move the entire
| | 01:25 | mechanism. Let's treat it as a whole, so
you can actually layout and see how this
| | 01:29 | things comes down here, how these
mechanisms are going to start moving around.
| | 01:33 | Now I can go back and edit this blocks
to change the way the linkages are,
| | 01:37 | where there endpoints are fixed at,
to change and modify that shape.
| | 01:42 | We can add on things like, say we add
like a line here, maybe it would be like a
| | 01:46 | rack and pinion drive
| | 01:47 | for instance. And I'll say this is going
to be a vertical line, and then let's go
| | 01:52 | ahead and make that a block.
| | 01:53 | And we can add maybe a traction
relationship, so I'll click on there, hold down
| | 01:57 | Ctrl, grab this, I'll say Traction,
which is kind of cool mate property.
| | 02:03 | I need one more thing here. We have got to
continue and make sure that's at Vertical.
| | 02:06 | As this thing moves around,
notice that it goes up and down as a
| | 02:10 | traction mechanism. It's pretty cool.
| | 02:13 | Once you've worked on your design a
little bit and you have it kind of laid
| | 02:16 | out exactly the way you want, we can use this
layout as a skeleton for actually the real parts.
| | 02:21 | So I'm going to say exist that sketch right now.
| | 02:24 | All those blocks, by the way, are under
Sketch1. And we were on the Front Plane, so
| | 02:28 | I'm going to back to the Front Plane.
I'm going to start another sketch this time.
| | 02:32 | Part of my sketch now is I'm going to
use these two elements from that to create
| | 02:37 | a part. So I'm going to click on this one,
hold down Ctrl, click on that one, and
| | 02:41 | I'm going to use this thing called Convert Entities.
| | 02:43 | Now we haven't seen Convert Entities
yet, but what that does is it inputs
| | 02:47 | geometry from behind into our current
sketch. So I will just click on Convert
| | 02:52 | Entities and it just brings
those two lines into my current sketch.
| | 02:54 | As soon as I have that, I'm going to
also use this Offset Entities command and
| | 02:59 | select those two, and let's say Offset.
| | 03:02 | And we did this a little bit before with
creating a slot, and I'm going to just
| | 03:05 | take this lines and use the Cap ends
with the Arcs and offset it a little
| | 03:09 | distance here, click on OK.
| | 03:11 | Then I'm going to go ahead and turn
that to a Feature. Click OK and you can see,
| | 03:17 | that would be the first
item, part of our mechanism.
| | 03:21 | We can use these different items here
that we're going to be creating, or these
| | 03:24 | different sections, to go and actually
create the mechanism to build an assembly.
| | 03:28 | But as I move these things around, it
will automatically be the skeleton that
| | 03:31 | will derive that shape.
| | 03:33 | So I'll go ahead and again create
another boss down here if I wanted to and
| | 03:37 | continue on with this. It's a great way
to layout mechanisms and kind of see how
| | 03:41 | things are going to work to help you visualize.
| | 03:44 | Using blocks to lay out mechanisms is a
great way to think through design and
| | 03:48 | rapidly modify the mechanism.
| | 03:50 | Just remember that each section must be
its own block and to relationships.
| | Collapse this transcript |
|
|
11. Assembly: Putting it All TogetherUnderstanding the tools for beginning a new assembly| 00:00 | Now that we can build parts, the next
step in the design process is to assemble
| | 00:04 | the parts together to create your product.
| | 00:07 | You can think of parts like LEGOs and
the assemblies as connecting the parts
| | 00:10 | together to build your creation.
| | 00:13 | Parts are the building blocks;
| | 00:14 | assemblies are the combination of parts.
And we can combine other assemblies
| | 00:18 | together to create sub-
assemblies into a top-level assembly.
| | 00:22 | Parts, assemblies, and sub-
assemblies can all have drawings.
| | 00:26 | The Assembly environment is very
similar to the Part environment, with its own
| | 00:29 | specialized set of tools.
| | 00:32 | To get started with assemblies, we
need to get into the Assembly environment.
| | 00:35 | There are several ways to start
assemblies, and the easiest is to open the part
| | 00:39 | we would like to be at the base of our assembly.
| | 00:41 | Choose this part wisely, since this
part will be fixed and the other parts
| | 00:45 | will be added to it.
| | 00:46 | For example, if you're building an
engine, it would be wise to start with the
| | 00:50 | engine block and then attach other
parts to it, like the pistons and valves.
| | 00:55 | Starting with the piston would
still work, however the assembly process
| | 00:58 | would be a bit odd.
| | 01:00 | To get started with assemblies, let's
click on the New dialog box up here or
| | 01:04 | click under File > New, and we get the
New Document window pops up. And we've
| | 01:08 | been using the part and now
we're going to use the assembly.
| | 01:10 | So just make sure that assembly is
highlighted there and then click on OK.
| | 01:14 | As we go into this, it's going to bring
up the dialog box on the left that says,
| | 01:18 | Begin Assembly, and if we had
open documents, they'd be here.
| | 01:21 | Unfortunately, nothing else is open, so
let's go back and open something up, or
| | 01:25 | we can browse for it here.
| | 01:26 | But before I do that, I am just going to
cancel that and I am going to hit R key
| | 01:29 | on my keyboard to bring
up some recent documents.
| | 01:31 | So here is the part we want to begin
an assembly with, and then jump over to
| | 01:36 | that window. And again, let's go back to
that same Insert Component window right
| | 01:40 | here, and now notice there are documents listed.
| | 01:42 | So if I click on OK, that imports
that block into my new assembly, and
| | 01:48 | notice the part here, and if I click on the
plus, it opens up the entire tree of that part.
| | 01:55 | Assemblies and parts both have planes.
| | 01:57 | Inside of here, I've got the three planes.
I am going to go up here and say View >
| | 02:01 | Planes and make sure I see them.
| | 02:03 | And then I've got the planes in the
assembly, I am going to show those as
| | 02:06 | well. Show, Show, Show.
| | 02:09 | And notice those planes are kind of
laying right on top of each other.
| | 02:12 | And this block is centered right at the origin.
| | 02:14 | Now, if I wanted this block to be able
to move around, notice this little F in
| | 02:18 | the front of its name.
| | 02:19 | That means it's fixed.
| | 02:21 | If I right-click on it, I come down
here to Float, that's no longer there.
| | 02:24 | But there is a little minus sign.
That means it's undefined as far, as its location.
| | 02:28 | So now if I move this thing around, you
can see that these are the planes of the
| | 02:32 | assembly itself, and then these are
the planes that are inside of the block.
| | 02:35 | So those are owned by that part itself.
| | 02:38 | And as we add other parts to this
assembly, we are going to have the same thing.
| | 02:41 | Each part is going to have its own
series of planes, and then the assembly itself
| | 02:45 | has got its own set.
| | 02:46 | Now let's take a look up
here at the Assembly toolbar.
| | 02:50 | If we have a component selected, I
can go back and edit that component.
| | 02:53 | So I can either edit the part in its own
environment or in the context of the assembly.
| | 02:57 | If I would like to add other components
to my assembly, I can insert it here.
| | 03:01 | Or I can just go into window and I can
just drag and drop components in, which
| | 03:05 | we will cover in the next movie.
| | 03:07 | Mate is how we connect two components
together with a series of commands we can
| | 03:11 | go through, and I will cover
that in the next few movies.
| | 03:13 | We have options for doing linear or
circular patterns, mirroring components, a
| | 03:18 | lot of different ways we can start
adding components on the next level here.
| | 03:22 | We can have smart fasteners like bolts
and nuts like that we'll auto-create.
| | 03:26 | We can move components
around just by clicking on them.
| | 03:28 | Or if we are not in that command, I
can just grab that component, and with my
| | 03:33 | left mouse key, just hold it down.
| | 03:35 | If I want to spin this component around,
I can click on it with my right mouse
| | 03:38 | key and I can spin it around, just
holding down your right mouse button.
| | 03:44 | Most of the other world environments,
they are the same; if you hold down the
| | 03:47 | middle mouse button, you can spin the world
around, and you can zoom in and zoom out as well.
| | 03:53 | And then of course these
buttons up here still work the same.
| | 03:55 | So Zoom to Fit, Zoom to Area, Previous
View, and Section View all still work the
| | 03:59 | same as they did in the Part environment.
| | 04:02 | We can add features that are only
available in the assembly, like if you had two
| | 04:07 | parts would be welded together, then
you might add a hole through them, that
| | 04:10 | would be an Assembly-level feature.
| | 04:12 | We can add reference geometry here,
just like we could in parts, as far as
| | 04:15 | planes and axes and things like that
| | 04:16 | that might help us to lay things out.
| | 04:19 | Once we start assembling things
together, they can move, so we can do some
| | 04:22 | studying of how they are going
to move or create some animations.
| | 04:26 | We can add bills of materials and we
can explode things out, so that we can
| | 04:30 | see how they would be assembled together, and
then that can be brought into a drawing later on.
| | 04:34 | Once you start to assemble parts together,
you really start to realize the power
| | 04:39 | of designing in a 3D modeling environment.
| | 04:41 | Your computer becomes a
virtual prototype environment.
| | 04:45 | By assembling the parts together, we
can see most of what we would in real
| | 04:48 | life and save ourselves a lot of time
and see things we may have overlooked
| | 04:52 | while building the parts.
| | 04:54 | This ability will save countless hours
and dramatically reduce the amount of
| | 04:58 | prototyping that is necessary.
| | Collapse this transcript |
| Identifying steps in creating an assembly| 00:00 | In this video we're going to cover
the steps to assemble parts together.
| | 00:04 | The first step is to make sure we
have the required parts in the assembly.
| | 00:08 | You don't need to bring all the
components in at once; however, sometimes it
| | 00:11 | speeds the workflow to have
the major components available.
| | 00:15 | Secondly, aligning the parts close
to their desired location will help to
| | 00:18 | connect the parts together.
| | 00:20 | In this assembly, I have a block and
I am showing the planes of both the
| | 00:23 | assembly and the part.
| | 00:25 | Now, most of the time when you bring
in a new part, your beginning part you
| | 00:28 | are going to start with, they are going to be
automatically aligned together on the origins.
| | 00:33 | In this case, we don't have that.
| | 00:34 | So what I am going to do is I am
going to mate the two together, and we are
| | 00:36 | going to cover the Mate
command in the next few movies.
| | 00:40 | Click on Mate, and I am going to click
on the origin of this one and the origin
| | 00:42 | of that one, and they are just going to
slide together. And it says Coincident
| | 00:46 | and it says Align axes, and that's what we want.
| | 00:49 | Click on OK, and now those two parts
are mated together exactly on those.
| | 00:52 | So if I click on the part and try to
drag it out, it's not going to move,
| | 00:56 | because it's now locked to the origin.
| | 00:58 | I am going to now hide those planes so
that I don't have to see them, and I am
| | 01:03 | also going to hide the origins.
| | 01:04 | We can always turn those on or off
depending on how many mating parts you have,
| | 01:08 | if they are going to come in handy or not. Okay.
| | 01:10 | So now we have one part in our assembly,
but it's going to be a fairly boring
| | 01:13 | assembly if we only have one part in it.
| | 01:15 | So let's go get some more parts.
| | 01:17 | Two ways to do this.
| | 01:18 | Number one is insert components.
| | 01:20 | If you look here, we've got three
components that are currently open.
| | 01:24 | If there are more components, they
will all be listed here, or I can actually
| | 01:27 | go out to the file system here and
click and browse to find a component that's
| | 01:30 | not currently open. And then once we
have something we like, we can click on
| | 01:34 | it and just click OK.
| | 01:35 | The problem with this is a lot of times
it adds it right to the origin, if I were
| | 01:38 | just to click, but notice it's now
stuck to my tooltip, so I can also drag it
| | 01:42 | and drop it anywhere on
the screen if I'd like to.
| | 01:45 | But if I click on just OK, it
will just put it right at the origin.
| | 01:47 | Sometimes that part will actually
be hidden inside the other part.
| | 01:51 | So instead of doing this, I am
going to go ahead and cancel that.
| | 01:53 | The way I prefer would be to click on
the window and I am going to say Tile
| | 01:58 | Horizontally or Tile Vertically.
| | 02:00 | So that's going to open up all the
windows that are currently open, and if I
| | 02:03 | wanted to add more windows, I just click
File > Open and go grab a part that's not
| | 02:07 | currently open, click on OK, and then
once again, Tile Horizontally. Now I have
| | 02:11 | all those parts open.
| | 02:13 | These are the parts I want to
put into this assembly here.
| | 02:15 | So I can just click on this part, hold down
my left mouse button, and just drag it right in.
| | 02:20 | Same thing with this part
here: just drag it right in.
| | 02:23 | This is the part we
originally had in our assembly.
| | 02:26 | I am just going to click on that
and just drag one more of those in.
| | 02:29 | I don't really want this one yet,
so I am not going to add that one in.
| | 02:32 | Once you're happy with what you have in
there, click on the Expand button. And I
| | 02:35 | am going to take a look at my assembly.
| | 02:38 | I can move these parts around
| | 02:39 | if I hold down my left mouse button,
click on the part and drag it around.
| | 02:44 | If I hold down my right mouse button, I
can spin it around to change its orientation.
| | 02:49 | I also have the ability to spin the
world environment around exactly how I did
| | 02:53 | with the parts, by holding down the
middle mouse button to spin things around.
| | 02:56 | And then I can also zoom in and zoom
out just by using the scroll on the mouse.
| | 03:02 | Up here I also have Move components, so
if I click on Move component, I can just
| | 03:06 | click on a component, drag it around.
| | 03:07 | Or I click on Rotate component
to spin that component around.
| | 03:12 | I really don't use those commands
because they're both available just by
| | 03:16 | clicking on a component, with your
left mouse button to move it, or your
| | 03:19 | right-mouse button to rotate the
component around. And I can do that with all
| | 03:24 | the components here to moving them around.
| | 03:25 | Now, if I wanted another one of these
components, I can hold down Ctrl and I can
| | 03:30 | drag another component out.
| | 03:31 | The neat thing about that is it
actually copies it in the exact orientation
| | 03:35 | that it starts from.
| | 03:36 | So like this component here, I am
going to rotate it around a little bit, and
| | 03:38 | then I am going to Ctrl+Drag to show that.
| | 03:42 | So see it's coming out in the exact
orientation as the one it copied from.
| | 03:45 | So it's really handy if you are just
adding a bunch of more parts or hardware or
| | 03:48 | screws or something like that.
| | 03:50 | You want to add a bunch of them to your
design without having to drag and drop them.
| | 03:53 | It's a real nice way just to copy those parts.
| | 03:56 | We want to mate these things together here.
| | 03:58 | In our next movie we're going to learn
how to do the mates, but right now let's
| | 04:01 | just get them into the orientation.
| | 04:02 | So I am going to hold down my right
mouse button and spin this part around, and
| | 04:05 | then I am just going to kind of put it
right up above here so we know that that
| | 04:08 | part is going to go down in that hole.
| | 04:10 | In one of these, we're going to spin
that around like this, and I am going to
| | 04:14 | spin my world around by holding down
my middle mouse button and just drag it
| | 04:18 | over here. So it's going to be close by.
| | 04:20 | We are going to put this on top of there,
so those are going to mate together.
| | 04:24 | And if I spin it around, I can move
these things a little bit more, so get them
| | 04:27 | close to where they are going to be.
| | 04:29 | Having it perfect is not essential here;
| | 04:31 | we're just getting them close to what
we're going to be working with when we
| | 04:34 | start mating these parts together.
| | 04:36 | The steps led out in this video will be
repeated in every single part in every assembly.
| | 04:40 | Getting the parts laid out well will
help to get your model assembled quickly
| | 04:44 | and with less errors.
| | Collapse this transcript |
| Mating parts together in an assembly| 00:00 | Mating parts together is the
fundamental skill of working with assemblies.
| | 00:05 | Mates are very similar to sketch relations.
| | 00:07 | We choose two or more faces, planes,
lines, or points and then choose how
| | 00:12 | they will be connected.
| | 00:13 | The most basic is a coincident mate.
| | 00:15 | This is basically just saying the two
items are touching. Let's take a look.
| | 00:19 | In a window here we see we've got a
block, which is at the origin, which is
| | 00:24 | our first part there, and then we've got two
more parts that we've added into this assembly.
| | 00:29 | And so we're going to jump
into the very most basic mates.
| | 00:32 | To get started, let's click on Mate.
| | 00:33 | As soon as I open that up, notice the
first window here is the Entities to Mate.
| | 00:39 | So anything I'm going to select in here is going to
automatically start mating things together.
| | 00:43 | We also have these standard
mates here like Coincident, Parallel,
| | 00:46 | Perpendicular, Tangent, Concentri,c and some
distances and angles, so we can put in there as well.
| | 00:52 | By default, SolidWorks is actually
going to find out which mate is going to be
| | 00:56 | the most appropriate when we select our pair.
| | 00:59 | So we always have to pick a pair, a
minimum of two things to create a mate.
| | 01:03 | So for example, I'm going to come down here and
I'm going to pick the outside of this boss here.
| | 01:08 | Now you can pick an edge, you can pick
a point, you can pick a face, you can
| | 01:12 | do a lot of different things, but it's
always better to pick faces versus edges
| | 01:17 | or edges over points.
| | 01:19 | The bigger they are the
harder they are to break.
| | 01:21 | So I'm going to go ahead and select
that face there--notice it highlights--and
| | 01:25 | then the face that I want
to be going around that.
| | 01:27 | And we are going to have a concentric mate,
so these two faces are going to be concentric.
| | 01:32 | So if I click on this face
here notice what happens.
| | 01:35 | That moves into position and now by
default that selects hey, this is probably
| | 01:40 | what you're looking for is Concentric
Mate, because I've picked two concentric
| | 01:43 | circles or two concentric faces.
| | 01:45 | Once I click OK, that mate is now established.
| | 01:49 | So if I click OK, it'll turn it
off, or it continues to stay active.
| | 01:53 | The Mate window stays open, so I can continue
just to pick pairs of faces to mate together.
| | 01:58 | If I pick this face here and I pick
this face here, it creates another mate, and
| | 02:04 | this time it chooses Coincident
because it's saying you're picking two faces
| | 02:07 | that can be easily coincident. It makes sense.
| | 02:10 | We could also change that to Parallel
or distance if we wanted to as well,
| | 02:14 | but SolidWorks just assumes one, and
you can always change it to something
| | 02:18 | else if you'd like to.
| | 02:19 | Once you're happy with that, you click on OK,
and then I'm going to close that Mate window.
| | 02:23 | Now notice this part here. It's got
a little spacing up there because we
| | 02:27 | mated the front of this face, put
that face there. And I can spin this part
| | 02:31 | around right now, still because we
notice this little negative or minus sign
| | 02:35 | in front of that part.
| | 02:36 | That means the part is not fully defined yet.
| | 02:38 | Now I'm going to click on that part
here and I'm going to show its right plane,
| | 02:43 | and then I make sure to turn
on Planes so we can see them.
| | 02:45 | Then I am going to go ahead and hide
these other planes here, so we don't see
| | 02:48 | those while we are mating things together.
| | 02:50 | So I mean you can always turn planes
on and off just like that, to easily see
| | 02:56 | where they are, and planes are a really
great way to mate and we're going to go
| | 02:59 | and cover those in a future chapter here.
| | 03:00 | So now while I move this part
around, you can see that that plane's
| | 03:03 | spinning around, right?
| | 03:04 | There are no degrees of freedom
if we were to lock that plane down.
| | 03:08 | So for instance, I'll say like that
plane there and I'll mate it to like the
| | 03:12 | outside of this and I'll say these
are actually going to need to be parallel.
| | 03:15 | As soon as I do that, let's look at this part.
| | 03:20 | Notice it used to have a minus sign
in front of it and now it doesn't.
| | 03:23 | That means it's fully defined. So most
items we're going to need a minimum of
| | 03:26 | three mates to fully define their location.
| | 03:29 | Now you don't have to have
fully defined parts; that's fine.
| | 03:32 | We might want this thing to be able
to spin around here and that's fine.
| | 03:35 | But just keep that in mind. If you see
a little negative sign there, that means the
| | 03:38 | parts are not fully
defined, but now it is, right.
| | 03:40 | So we've locked the plane, so the
orientation, we've got the face, and we know the
| | 03:44 | location, where it is.
| | 03:45 | Let's try a couple of more here.
| | 03:48 | This time this is kind of like a
small screw or a representation of a screw
| | 03:51 | without the threading and
things like that in there.
| | 03:54 | Make sure we want to put that in to the hole.
| | 03:55 | We also have this angle or the
chamfer that we're going to mate to this
| | 03:58 | other chamfer here.
| | 03:59 | So we have a bunch of different Mate options.
| | 04:01 | So first let's get into the Mate window,
let's click on the outside face, and
| | 04:06 | click on that, and then we're going to
spin around, and this is the other face.
| | 04:09 | So the best way to think
about mates is to say it out loud.
| | 04:12 | You say, I want the outside of this
screw and the inside of that hole and
| | 04:16 | that's you mate pair. As soon as you pick
that pair then move into position and now that's mated.
| | 04:21 | Once you have a mate now
these things can move around.
| | 04:23 | So I can drag this up and down, but the
mates are always going to be established here.
| | 04:30 | And if you look at the mates over
here at the very bottom of our Feature
| | 04:33 | Manager, I can expand that box out
by clicking on the plus and then I've
| | 04:38 | got all the different mates, and I
can click on them to highlight them and
| | 04:41 | they'll show the pair
that's being mated together.
| | 04:44 | That last mate we did, which is Concentric Mate,
| | 04:46 | if you didn't want that one, you can
just hit Delete and delete that mate.
| | 04:50 | Now I can move this thing
around anywhere I wanted to.
| | 04:53 | To put it back, just go Mate, select
that pair, select that, and there we go.
| | 04:59 | We have a couple of more
mates we're going to add to this.
| | 05:01 | So this time I'm going to pick this face here.
| | 05:03 | Pick that face there, come up here and I pick
that face there, and I'm going to say Coincident.
| | 05:08 | All right that brings that down into the hole.
| | 05:11 | So we've got a nice mate here.
| | 05:13 | And in fact, if we think about those
mates making, those two coincident, we
| | 05:17 | actually don't need the mate before that.
| | 05:20 | This one here, it's redundant.
| | 05:21 | All right, because by making these two
faces here coincident it actually just
| | 05:25 | establishes both the location and
depth that's going to be in there and the
| | 05:29 | concentricity, all in one shot.
| | 05:30 | So if I got rid of this one here, I
can just click on it and hit Delete,
| | 05:33 | it's not going to hurt anything to
have it there, but I can now only spin this
| | 05:38 | part; I can't move it up and down
or I can't move it right or left.
| | 05:40 | All right, so it's fully defined.
| | 05:43 | And notice I'm using faces; I'm
choosing faces to mate things together.
| | 05:46 | So, the priority of mating is number one,
most powerful thing would be choosing
| | 05:52 | the fundamental planes, right because
the planes are always going to be there.
| | 05:55 | They start there when you start your part.
| | 05:56 | So if you mate a plane to another plane, it's
going to be the most solid mate you can choose.
| | 06:01 | Secondly would be faces.
| | 06:03 | If I pick entire face to mate to something
else, that's probably going to stick around.
| | 06:07 | Whereas if I pick an edge to mate
something else, if I were to chamfer that edge
| | 06:11 | or radius it or just something else of
that, as soon as that edge is no longer
| | 06:15 | there, that mate's going to fail.
| | 06:16 | And so let's try a couple of failed mates.
| | 06:18 | Now notice this part here.
| | 06:21 | We've got the back of this part.
| | 06:23 | Right there I can select that part,
by grabbing the back of the part.
| | 06:26 | Now I am going to say that back of that part,
let's mate that together with this face here.
| | 06:30 | As soon as I do this, it's going to
say hey, both of these are already fully
| | 06:34 | defined, but I'm going to say it
doesn't matter. I'm not going to put it on
| | 06:36 | there. I'm going to say okay.
| | 06:38 | But it's going to warn you hey, we
can't do that. It's going to cause errors.
| | 06:43 | But if were to change something in
these parts to make one of these mate faces
| | 06:48 | go away, it would change the
way this is mated together.
| | 06:51 | So I'm going to open that part here, and
I'm going to go and I'm going to select
| | 06:55 | that top face, and I'm just going to
draw a rectangle over it, and I'm just going
| | 07:03 | to cut a little bit away.
| | 07:04 | I'm just going to trim off just a
little bit of that, make it a little thinner.
| | 07:06 | So now I have changed that part.
| | 07:08 | When I go back to that assembly, it
says update the thing, and then I say OK.
| | 07:14 | And now look what happens. It says we
got all these red errors. It's just saying
| | 07:18 | hey, this Coincident Mate can no longer
do because that face is no longer there.
| | 07:22 | All right, it's moved in.
We chopped off that face.
| | 07:26 | It's highlighting the two faces or the two
parts that actually made up that mate pair.
| | 07:30 | So we've got this part here, and it's
showing that mate again is in there, and
| | 07:34 | each part itself has the
mates that are assigned to that.
| | 07:38 | So the mates that are inside the part
are the exact same mates that are down
| | 07:40 | here; they're just listed twice.
| | 07:42 | This is all the mates in entire
assembly, and these are the mates that only
| | 07:46 | apply just to that part.
| | 07:47 | All right, so if I go ahead and I delete that
mate here, click OK, it fixes all the mates.
| | 07:52 | But now the problem is is that's free-floating.
| | 07:55 | Move it in now. So I need if we go back
and re-mate that to fix it, and there it is.
| | 08:04 | These basic Mate tools will
help you build your models.
| | 08:07 | When building mates, try to choose
items that are stronger versus weaker or
| | 08:10 | easier to break. For instance parts
start with three fundamental planes and
| | 08:14 | we cannot remove them.
| | 08:15 | So if you mate two planes together,
there's no way to break that mate.
| | 08:20 | However, if you mate a corner point of
your part to something else, anything
| | 08:23 | that changes that point will break that mate.
| | 08:26 | Try to think about the easiest
and most robust way to mate parts.
| | Collapse this transcript |
| Matching part sizes accurately in the parametric prototyping environment| 00:00 | The most powerful benefit of using solid
modeling is to virtually create objects
| | 00:05 | and assemble them together in the computer.
| | 00:08 | This allows us an opportunity to foresee
potential problems way before the first
| | 00:12 | prototypes are made.
| | 00:14 | An added benefit is we can directly
generate the files needed to produce rapid
| | 00:17 | prototypes like SLAs, FDM, or 3D printed parts.
| | 00:22 | On the screen here, we've got a block
and we've got this little washer-looking
| | 00:26 | part, and we're going to assemble them together.
| | 00:28 | So number one, we've got a mate already
established here, and I am just going to
| | 00:31 | delete that mate, so we can re-
add it and that mate is right here.
| | 00:35 | I am just going to find it in the
tree just by highlighting over each pair.
| | 00:38 | Then I want to get rid of that one
there. I am just going to go back and
| | 00:41 | re-create that to review.
| | 00:43 | So right now, these parts are free-floating.
| | 00:45 | I can move it around a little bit.
And I am going to click on this outside face
| | 00:49 | here, select mate, and take that inside
face there, and it's going to give us a
| | 00:54 | coincident mate. Highlight it up,
and click OK, and there we go.
| | 00:58 | Now I can bring this
part in and out, drag it in.
| | 01:01 | So I've got that degree of freedom.
| | 01:02 | So a couple of things I see.
So I bring this closer together here.
| | 01:05 | So if I start mating it up, I might
overlook this, but I think I wanted these to
| | 01:08 | be a slip fit, but not quite that loose, right.
| | 01:11 | We want it to slide over that,
but not to be so sloppy like that.
| | 01:15 | And secondly, I want to mate this back
face here to the back of that washer.
| | 01:19 | I am going to click there and
I am going to pick that mate.
| | 01:22 | You can always pick the pair first, so
you can save that face, hold on Ctrl,
| | 01:26 | select the other face, like that.
| | 01:29 | Then select mate, and then it just
automatically puts that pair together, and it
| | 01:32 | pre-highlights them both.
| | 01:33 | It makes it an easy way to select things.
| | 01:35 | Once you have it look good, click
OK, and now let's mate it together.
| | 01:40 | So now this part is stuck on there.
| | 01:42 | Two things we want to go back and edit.
Number is is this hole is too big
| | 01:46 | for this shaft. And number two, we
want to thicken this up so it's the same
| | 01:51 | length as this boss here.
| | 01:52 | So we're going to do that two different ways.
| | 01:54 | Number one is I am just going to click
on the part. I am going to go Open part.
| | 01:57 | We get this in-context dialog when it
pops up anytime that we just click on a part.
| | 02:01 | And so just click on with a left-click.
It's going to pop up an open part.
| | 02:05 | We can open it, we can edit it in
context, we can hide it, we can change
| | 02:09 | transparency, we can suppress it--
a lot of things we can do here.
| | 02:12 | We're just going to do the
very first one called Open part.
| | 02:13 | That's going to open up that part
there. Delete this little sketch here, and
| | 02:19 | we're going to go and click on that
sketch, and we're going to edit it, just like
| | 02:24 | we did when we changed the parts around.
| | 02:25 | And now I have got a 2.25 and that shaft
we had in the other part, let's go find
| | 02:30 | out how big that shaft is.
| | 02:31 | So before I go and change this, let's
go back to the assembly and take a look.
| | 02:35 | We're editing the part, so
it's hidden for right now.
| | 02:39 | But, I am going to go ahead and I am
going to show the Tools palette down here
| | 02:43 | and the tools right here, and
they show up on the side.
| | 02:47 | Now, I am going to go back and actually
get out of that sketch here. That part
| | 02:52 | is going to come back.
| | 02:53 | So before we do that, let's go back to
the assembly and update the part,
| | 02:56 | and I am going to use the Measure command.
| | 02:58 | That's part of the Tools palette.
| | 03:00 | So I click on the Measure and then I
am just going to click on that face.
| | 03:03 | It says okay, here is an Area, here is
a Diameter, here is a Perimeter, and the
| | 03:06 | Diameter is what we're looking for. So it's 2.0.
| | 03:08 | We can do a little inspection
to figure out what's going on.
| | 03:11 | So now, we have a 2-inch diameter.
| | 03:13 | So I am going to go back to that part
now, go back and edit that sketch, and I
| | 03:18 | want a slipfit, so I am going
to change this to like 2.005.
| | 03:20 | So we're going to make it a 5000th of an
inch larger than a 2 inch, so it's going
| | 03:25 | to give us a 5000 slip fit.
Click OK, modify that.
| | 03:29 | The way I have it designed here is the 1
inch over, so it's going to change that
| | 03:32 | outside diameter too.
| | 03:33 | So I am going to click OK.
| | 03:34 | We go back to that assembly, and notice
that part automatically updates, and now
| | 03:39 | it just slides over that shaft.
| | 03:42 | The next thing we want to do is we want to
change the thickness of this washer, so
| | 03:45 | it's the same length.
| | 03:47 | To do that, this time I am going to
use an in-context editing technique.
| | 03:50 | So I am going to click on the part,
and I am just going to say Edit part.
| | 03:53 | Now, I am editing in context to the assembly.
| | 03:56 | So I am going to go back to that part,
and notice over here in the tree, it
| | 04:00 | highlights it in blue.
| | 04:01 | I can go back in here, and now I can
actually change any of the features that
| | 04:04 | when we created that part.
| | 04:05 | So I am going to click on that and say Edit
Feature, and right now it's using a Blind Extrude.
| | 04:10 | So instead of Blind, I am
going to say Up To Surface.
| | 04:12 | And the surface I am going to choose is
actually part of the block, not the part
| | 04:17 | itself, so it's a different piece.
And as soon as I click on that, it changes it
| | 04:21 | so it's actually related now
to the base block that it's on.
| | 04:26 | Click on OK and then when I want to get
back into editing the assembly, I click
| | 04:30 | on that, and notice the washer has now
changed. It's in context of this and it
| | 04:35 | just allows us to quickly and rapidly
adjust parts so they fit together well,
| | 04:39 | all in the computer.
| | 04:41 | Prototyping in a computer is
fast, economical, and easy.
| | 04:45 | Leverage the power of SolidWorks and
the variety of tools that are available to
| | 04:48 | build, compare, and analyze your designs.
| | Collapse this transcript |
| Working with subassemblies| 00:00 | Just like we can combine other parts,
we can also assemble other assemblies.
| | 00:05 | The tools are the same.
| | 00:06 | All we need to do is drag a few
subassemblies into a new assembly.
| | 00:11 | To get started, I've got four parts here.
| | 00:13 | And what I want to do is I want to
combine this part, this part, and this part
| | 00:17 | into a subassembly, and then we are
going to add that subassembly to this tray.
| | 00:21 | And we can actually add multiples of that.
| | 00:23 | If you think about it, if I didn't
create the subassembly, I would have to
| | 00:26 | add this part, then add that part, and
then the third part, and each time we
| | 00:31 | want to add it to a new little slot here, a little hole,
we are going to put that in container. Let's get started.
| | 00:36 | I'm going to open up this part here,
and I'm going to say, one easy way to
| | 00:40 | actually start an assembly is
actually start right from the part.
| | 00:43 | Let's say File > Make assembly from part.
| | 00:48 | What that does is it just drops that
part right into the assembly, selects
| | 00:52 | it over here, and just click OK, and there it
is. Just quick way to get into a new assembly.
| | 00:58 | To assemble that together, let's go back
here and tile our windows jorizontally
| | 01:00 | so we can see them all.
| | 01:01 | Now I want this part here, so I'm going
to drag in, and then I want the cover and
| | 01:06 | I'm going to drag that in too.
| | 01:09 | So that's my subassembly.
| | 01:09 | We are going to use a couple of
techniques here to mat these together.
| | 01:12 | One of the ways I'm going to do that
is I'm going to turn on the Temporary
| | 01:16 | Axes, so each one of these has an axis
in the center of it, because they are
| | 01:19 | all revolved parts.
| | 01:20 | Okay then we will click on Mate, and
I'm going to mate together this axis here
| | 01:25 | with this one here.
| | 01:26 | That just puts that cone inside of our
container here, so we can move it up and down.
| | 01:32 | Then I will use one of those Coincident Mates,
so I'm going to say the bottom of that container.
| | 01:36 | Then I'm going to spin it around and pick the
bottom of this part. It puts that right in the
| | 01:40 | container. And let's put the cover on.
| | 01:42 | So I will select that axis there and
select the axis here. That brings the cover
| | 01:47 | directly over the part.
| | 01:48 | I can still move up or down. And then
I'm going to pick like this little edge here, spin
| | 01:52 | that around, and grab the bottom
of that and mate those together.
| | 01:56 | All right, so we have done a
little more mating practice here.
| | 01:59 | Now that we have mate all these
together, we have assembly9,
| | 02:02 | so I'm going to go out and save that.
| | 02:04 | You got to make sure you save here
subassembly before you can import it
| | 02:07 | into another assembly.
| | 02:08 | So I am just going to call
that 11.5. Save that out.
| | 02:13 | So now we have an assembly. We are
going to now put into another part.
| | 02:16 | So let's go back and take a look
at all the things we have opened.
| | 02:19 | So this part here is the 11.5-1.
I'm going to open that up.
| | 02:24 | It's just a part, right, so we want
to put that into an assembly itself.
| | 02:27 | So I am going to go File > Make assembly
from part, and I'm going to start with
| | 02:32 | that part there. There it is.
| | 02:33 | Okay, now I am going to start
dragging in other parts or other assemblies.
| | 02:37 | So I'm going to Tile Horizontally again.
| | 02:40 | Now I could drag individual parts on if I
wanted to, but I can grab this entire assembly.
| | 02:45 | And instead of grabbing it from the
actual graphics window here, I'm going to
| | 02:48 | grab the icon over here in the tree,
drag it all the way up here, and then you
| | 02:52 | can see the assembly comes into the
other assembly. This is assembly10.
| | 02:55 | So now I have a subassembly inside of
another assembly, so it allows us to
| | 03:02 | bring that. And then inside of that
subassembly, I can see I that's made up
| | 03:04 | of these three parts.
| | 03:05 | And then I can continue to do that.
| | 03:09 | Here is that part, or that subassembly, and
I can just drag it up to this new assembly.
| | 03:13 | Keep dragging them in as I need them.
| | 03:15 | So I can drag as many as I want to.
| | 03:17 | That's definitely going to be a huge timesaver
versus having to bring each one of these
| | 03:21 | parts in and then assemble all three of
those together for each single item and
| | 03:25 | then put it and assemble it together.
| | 03:28 | Now that we have some items in here,
we can start mating them together.
| | 03:31 | So we know that this little inside face
here and the outside of that part are
| | 03:37 | going to be mate it together, and probably
the inside bottom there and bottom of
| | 03:42 | that container are going to get mated together.
| | 03:44 | And so that's my first mate,
placing it right there on the tray.
| | 03:49 | So I can have those mates that
apply on an assembly level as well.
| | 03:53 | So you can see, here are my
different assemblies, and there is the icons
| | 03:55 | little bit different here.
| | 03:56 | This is a part icon and the
subassembly has a little green corner to it
| | 04:01 | showing that it's actually an assembly and
then that's made up of these individual
| | 04:04 | parts that go back in there.
| | 04:06 | And then the mates themselves can
apply right there, and those are applying
| | 04:10 | on the assembly level.
| | 04:11 | So we are affecting these directly.
And also if you open up that assembly, you
| | 04:15 | can see the mates in each one of those there.
| | 04:17 | They go up and make that part up.
And as soon as you add mates to like a part of
| | 04:23 | this, you get another little
folder called Mates in assembly10.
| | 04:25 | It's going to show you the mates that
you have added to control that assembly.
| | 04:30 | Let's go ahead and just do a couple of more
here, just to get the rest of them in there.
| | 04:34 | I will click on there, click on
there. It's going to bring those together.
| | 04:36 | Click on the bottom there, spin it
around, click on there. These are just
| | 04:41 | rapidly adding Coincident mates or Concentric
mates, and let's do the same thing over here.
| | 04:45 | Click over here, click over here,
and then it just brings them together.
| | 04:49 | You can do it in different orders too.
| | 04:50 | So I can go select this one
here and put that one there.
| | 04:54 | The next thing I'm going to show is
what's called a Multi-Mate. And we have a
| | 04:57 | bunch of items that have
already mated to the same face,
| | 05:00 | we can use this. And notice this little
like lightening bolt on the corner of
| | 05:04 | that thing. Anytime you see a
lightening bolt what that just means, it's going
| | 05:06 | to make things rapid and faster.
| | 05:08 | Once I click on that, the Mate Selection, so
this is the item that's going to be in common,
| | 05:14 | so the common one is going to be this
one here, so that face and then the items
| | 05:18 | we want to mate to there.
| | 05:19 | So I want both the bottoms of these.
I'll just click there and click there.
| | 05:23 | And then in one shot it does both of
those mates at the same time, pretty handy.
| | 05:27 | By assembling one assembly into another,
it automatically becomes a subassembly.
| | 05:32 | We can continue to nest
assemblies into other assemblies.
| | 05:35 | The tree structure can be
assembled in any way you want, with as much
| | 05:38 | complexity as needed.
| | 05:40 | However, best practice would be to
assemble the parts in the same way you
| | 05:44 | would in real life.
| | 05:45 | Look for a series of parts that
would be repeated, and then combine them
| | 05:50 | together into a subassembly to be
put into the top-level assembly.
| | Collapse this transcript |
| Patterning in assemblies| 00:00 | In this movie, we are going to cover patterning.
| | 00:02 | We are going to do linear
patterning as well circular patterning.
| | 00:05 | Now, patterns can be made from
individual parts or subassemblies or even
| | 00:09 | top-level assemblies.
| | 00:11 | You can pattern just about anything you like.
| | 00:13 | If we look at this example here, this
is one we finished in a previous movie,
| | 00:17 | and we kept adding individual
subassemblies to this, and adding relationships.
| | 00:22 | And you can look down here, we have
got a lot of relationships we added to
| | 00:25 | locate each one of these little jars.
| | 00:28 | And instead of doing all that work of
adding a new one in, mating it up to all
| | 00:33 | the different references, we've got a
bunch of holes here that could take quite
| | 00:36 | a while. But think about if we had
hundreds of holes that we needed to put jars
| | 00:40 | in. That would really take a long time.
| | 00:42 | So instead of doing that, why don't
we go ahead and use a pattern instead?
| | 00:45 | So what I am going to do is I am
going to click and hold down Ctrl and just
| | 00:48 | select those three right there,
and I am going to get rid of those.
| | 00:50 | I am just going to hit Delete and Yes to All.
| | 00:53 | Now I am going to select that one.
| | 00:55 | Keep in mind, this is a subassembly, so
there's actually three parts inside of here.
| | 00:58 | I can either pick one of the parts
individually or I can pick the whole
| | 01:02 | subassembly, no problem.
| | 01:04 | Click on the Subassembly and then
click up here under Linear Pattern.
| | 01:08 | So Linear Pattern works almost
identical to patterning in the part level.
| | 01:13 | First thing is which direction do we
want to pattern in? And I am going to
| | 01:16 | select any edge going in that direction.
I am going to pick that edge there.
| | 01:21 | And then it's asking you the spacing
between the parts, and I believe it's 4
| | 01:25 | inches here. And we're going to
say how many we want. There it is.
| | 01:30 | So as soon as I click on 2, there
we've got our next pattern there.
| | 01:34 | You can see we've got all three parts
in there. And it's easy as just going 1,
| | 01:38 | 2, 3, 4. More patterns, so
we've got 5 across that way.
| | 01:42 | And then same thing with direction 2,
pick that top edge, and like I said, you
| | 01:45 | can pick any edge going in that direction.
| | 01:47 | I can pick this edge back here if I
wanted to, or you could even draw a sketch
| | 01:51 | if you wanted a pattern
going in a different direction.
| | 01:53 | I am just going to pick this edge here and put
the same spacing of 4.0 and then take a look.
| | 01:59 | Notice we're going in the wrong
direction. I can just flip that with the arrow
| | 02:03 | here, and there we go.
| | 02:05 | So we've got 3 going that way, 5 going that way,
| | 02:07 | and just that quickly
we've established our pattern.
| | 02:11 | Now, if we wanted to remove an
instance from there, first off, in here, we've
| | 02:16 | got the components we're Patterning,
which is that of subassembly, and then
| | 02:18 | down here in Instances, if we click in this box,
it gives me this little purple dot on each one.
| | 02:23 | If I want to get rid of any one of those,
I could just randomly remove some of
| | 02:27 | the items if I wanted to, and they show
up here as far as a matrix level,
| | 02:31 | third row second column, fourth
row second column, kind of thing.
| | 02:35 | So if you want to bring them back,
just delete them out of this box here, and
| | 02:39 | then they'll pop back in.
| | 02:40 | Click on OK, and there it is. Just that
quickly we've got a nice linear pattern,
| | 02:45 | laying up all these parts.
| | 02:46 | And we've got a very simple tree here.
| | 02:49 | We've got the original base and
then we've got that subassembly.
| | 02:52 | And then below Mate, notice that in
the Mate we only have two mates in
| | 02:54 | this whole assembly. Pretty cool!
| | 02:56 | And then the linear pattern here
and all those new parts under there.
| | 03:01 | And if I wanted to, I could actually
suppress that entire thing to hide them
| | 03:05 | all. If I wanted to I can bring them all
back, and I can also go in here and edit that.
| | 03:10 | I can change the spacing if I wanted to
or remove certain items out of that group.
| | 03:14 | A lot of power in one simple command.
| | 03:17 | Click OK, and there we are. Okay.
| | 03:19 | Now I am going to jump over to the
Circular Pattern, and I have a file open here
| | 03:24 | called 11.6-2. And this is just a plate.
| | 03:28 | Now, what we want to do is we want to
Circular Pattern this one around, so
| | 03:31 | I've got one quarter of an enclosure
kind of laid out. I just want to take that,
| | 03:36 | instead of having to make it four
different times, and then assemble it
| | 03:38 | altogether, it makes it real easy just
to go ahead and pattern that around.
| | 03:42 | For circular patterns what
we need is a axis of rotation.
| | 03:46 | So before we can pattern things
around, I need to add that axis in.
| | 03:49 | It's the same way we've been doing it before.
| | 03:51 | I am going to go up here to Reference
Geometry and I'm going to say we need an Axis.
| | 03:56 | And the Two Planes method is
probably going to work out best for us.
| | 04:00 | And I am going to pick the--let's see what
we've got here. We've got the Top Plane and
| | 04:04 | the Right Plane. Those are the ones
that are intersecting here for us.
| | 04:08 | So that's going to be right
in the center of that shape.
| | 04:11 | And you have to pick these planes
dependent upon how you drew your original sketch.
| | 04:14 | So this one was drawn on the Front Plane
so that's why we have to pick that pair.
| | 04:18 | So just take a look at it in the
Drawing view to make the correct selection.
| | 04:22 | Click on OK, and now we've got an axis
to view around, and I am going to make
| | 04:25 | sure we're viewing our axes.
| | 04:27 | There it is, and there is our
part we want to move around.
| | 04:30 | So, same thing, under Linear Pattern,
there is a thing called Circular Pattern.
| | 04:34 | And let's just simply jump into this.
| | 04:35 | The first question it's going to
ask me is, what axes? There it is.
| | 04:40 | And then second one is, what's the component we
want to pattern? I am going to select it here.
| | 04:44 | I always try to select things from
the tree versus from the Drawing window.
| | 04:48 | So I am going to pick that
pattern there, and notice you can see a
| | 04:50 | little representation.
| | 04:51 | Right now it's giving us a
15 degree and there's two of them.
| | 04:52 | We probably prefer to have equal
spacing, so it's going to put on the other
| | 04:56 | side, and we actually want 4.
| | 04:58 | So as you see, as we add those up, it just
adds one more, adds one more, spin around.
| | 05:03 | And same thing, we can always remove an
item if we wanted to take one of those
| | 05:07 | out of the grouping, but we don't in
this case. Click on OK, and it's as simple as
| | 05:12 | that. We've generated a
circular pattern of these parts,
| | 05:15 | and we can do that with
as many parts as we want.
| | 05:17 | And we can also go back, just like we
did with the linear pattern, and then
| | 05:21 | here are the parts. We can suppress
these if we didn't want to see them for a
| | 05:25 | second, bring them back.
| | 05:26 | We can edit this pattern here, just
by clicking on the Edit feature, and we
| | 05:31 | can change things around a lot of
different ways here if we wanted to change
| | 05:34 | it through different angle or a certain
amount of instances we wanted to put in there.
| | 05:38 | So a lot of power, again, in
a very simple-to-use command.
| | 05:42 | So there you have it for the
linear pattern and the circular pattern.
| | 05:46 | Patterning can save a lot of time and
provides an easy way to modify the spacing
| | 05:51 | and quantities of parts or subassemblies.
| | 05:54 | If you find yourself adding more than a
few of the same item to your assembly,
| | 05:58 | maybe a pattern can help out.
| | Collapse this transcript |
| Downloading pre-made parts from the Internet| 00:00 | One of the best ways to build
assemblies is to not build the parts at all.
| | 00:04 | Standardized parts can be downloaded
from a variety of web sites for your use
| | 00:08 | in your assemblies. Let's take a look.
| | 00:11 | The first web site I was going to show
is 3D Content Central, and this is owned
| | 00:14 | by SolidWorks. And you can upload
brackets and cylinders, hardware and bunch of
| | 00:19 | companies who do a lot of
these type of products too.
| | 00:22 | And you can look at some of these
companies, who they are, and you can browse
| | 00:26 | and search for items you might be looking for,
download them into your model very quickly.
| | 00:30 | Next thing I'm going to show you is
MiSUMi, and this is a configurable website,
| | 00:35 | so you can download all types of the
products for mold designs and automation
| | 00:39 | components, press die components.
| | 00:41 | You can take a look at some of these.
| | 00:43 | We have like automation like
linear motion, like shaft, bearings.
| | 00:46 | Go on the web site, configure the
product exactly the way you want, and then
| | 00:50 | download it, maybe into custom
machine and things like that based upon the
| | 00:54 | input data you give them.
| | 00:56 | Up here, another one called GrabCAD.
There is all types of really neat models
| | 01:00 | that have been uploaded here.
| | 01:01 | They use SolidWorks models as well as
models from other different companies in
| | 01:05 | 3D formats like STEP and
IGES that are uploaded here as well.
| | 01:08 | And then if you have some neat models
you've developed, you can upload them,
| | 01:10 | share them with the community as well.
| | 01:12 | PEM Engineering, so they make PEM
hardware like the captive fasteners, this
| | 01:16 | is very common in sheet metal type parts,
but it can be used in machine parts as well.
| | 01:20 | You can search for a part number here,
download the cad model, bring it right
| | 01:24 | directly into SolidWorks.
| | 01:25 | And the last one I am going
to show you is McMaster-Carr.
| | 01:28 | And this is a great resource.
| | 01:29 | It's kind of like the world's best
hardware store online, and you can download
| | 01:33 | the parts quickly here.
| | 01:34 | And if you order the parts, they
normally show up in less than a day a lot of
| | 01:37 | times. It's a really great resource,
and there is also some really good
| | 01:40 | information as far as technical data about
the hardware and the materials that go into it.
| | 01:44 | So I am just going to download
one socket and cap screw here.
| | 01:46 | So, notice how I can select which one I want.
| | 01:48 | I am going to pick that style right there.
| | 01:50 | Not all of their components have a
download, but a lot of them do, so I'm going
| | 01:54 | to go over here and pick this socket
head and go down to a size I am looking
| | 01:59 | for. I am looking for, say, 1/2"-13 and
once I find the type of hardware, it gives
| | 02:05 | me a couple of options as far as what
type. I am going to use Stainless Steel
| | 02:09 | and I got a choice of 316 or
18-8 and I can pick the length.
| | 02:13 | So say like this one here, it's a 1"1,
so if I click on that item right there,
| | 02:16 | notice I get a few options here.
| | 02:18 | I get a CAD download, I get the
catalog page or I can bookmark it.
| | 02:21 | Click on CAD and I get a picture of
the drawing--it's pretty nice--and then I
| | 02:26 | can download it on all types of
formats: IGES, PDF, SolidWorks,
| | 02:30 | STEP files. And then I can also get the
technical drawings as an AutoCAD drawing or a PDF.
| | 02:34 | So I lot of times would download both
the 3D SolidWorks file as well as like
| | 02:38 | maybe a 2D-PDF or 2D-DXF drawing,
just so I can keep that as a reference in
| | 02:42 | maybe a reference folder I might design.
| | 02:44 | Pick the 3D SolidWorks, click on Save,
and it says, open the file up, click OK,
| | 02:49 | and it's going to say Read-Only.
That's great, and there it is, just that quickly.
| | 02:53 | I downloaded a file off the
Internet and now I can take it, this little
| | 02:55 | component here, and save it out to my
local directory and use it in my assemblies.
| | 03:01 | Downloading CAD models can save a lot of time,
| | 03:03 | and many times you will
get an even better model.
| | 03:06 | If you're working with standardized
components like hardware or off-the-shelf
| | 03:09 | items, make sure to check on the Internet.
| | 03:11 | You will be surprised at what you find.
| | Collapse this transcript |
| Working with pre-made parts bundled with SolidWorks Professional and SolidWorks Premium| 00:00 | If you have SolidWorks Professional or
Premium, you have the option of using the Toolbox.
| | 00:05 | The Toolbox provides millions of hardware items that
can be quickly added to your assembly. Let's take a look.
| | 00:11 | Here is a part that we've got four
holes in, and these could easily be created
| | 00:15 | with a Revolved Cut, or we could use
the Hole Wizard, which we'll be learning
| | 00:19 | about in Chapter 13.
| | 00:21 | And what we want to do is we want to
add some hardware to this assembly.
| | 00:23 | To do so, over here in the Library
we've got the Design Library, and notice
| | 00:28 | we've got the different blocks and then
you have this thing called the Toolbox.
| | 00:31 | And notice it says it's not quite added in yet,
| | 00:33 | so we want to either click on this
link here to add it in, or come up here to
| | 00:36 | the top and say Tools, and at the
very bottom of that, say Add-Ins.
| | 00:40 | This also gives us a way to add in a
lot of different features in SolidWorks.
| | 00:45 | We've got FeatureWorks, we've got
the 3D rendering package, which is
| | 00:48 | PhotoView 360, we can use the Motion,
the Routing, Simulation. And then down
| | 00:52 | here we've got Toolbox--we want to turn
that one on--as well as Toolbox Browser.
| | 00:57 | And then if you want those items to
show up automatically during startup, just
| | 01:01 | click and turn them on over here.
| | 01:02 | And once you are happy with that,
click OK and that adds that in.
| | 01:05 | And then over here back in the Library,
now we've got the Toolbox. And notice
| | 01:09 | it gives us this little window that says
Toolbox is currently installed on this computer.
| | 01:12 | If you want to use it just for one
user, that's fine; however, if you are
| | 01:16 | working with a group of people, it's
best to have Toolbox installed on a server
| | 01:20 | or a community machine that
everybody can access the same Toolbox files.
| | 01:24 | So I am going to click down here and look
at some of the items that are available.
| | 01:27 | Click on the Inch Folder, and you can
see there is Bearings, there is Bolts,
| | 01:30 | there is Screws, there is Bushings, O-Rings.
You've got a lot of neat things you can add in.
| | 01:34 | So let's just take a look at
Bolts and Screws for right now.
| | 01:36 | And what type of Screws, there are
Countersunk Head if we want. And maybe we
| | 01:41 | want a Countersunk Bolt. And once we
grab that, we're just going to pull it out
| | 01:45 | to the window and let go.
| | 01:47 | As soon as we do that, it's going to
ask us, how do we want to configure
| | 01:50 | that bolt or that screw?
| | 01:52 | So first is what Size we want.
We've got all kinds of different sizes here, and
| | 01:55 | I am going to start with a quarter 20 (1/4-20).
| | 01:58 | And what type of Drive we want,
so it's a Slotted, that's fine.
| | 02:02 | And how long do we want to have it?
So I am going to pick like three quarters of
| | 02:04 | an inch (0.75) and notice
it changes on the fly for us.
| | 02:07 | And come down a little bit further, and
how do we want it to display? Do we want
| | 02:10 | Cosmetic Threads and make it look a
little fancier, or Schematic to actually
| | 02:15 | put the threads on?
| | 02:16 | This might look nice to have that in there.
| | 02:18 | However, it's going to add a lot more
data to your model, so a lot of the times
| | 02:22 | you don't want to add all that extra
weight to your models, so just maybe
| | 02:24 | Simplified is the easiest way to go.
| | 02:26 | And then click on OK, and
that's going to build that model.
| | 02:30 | Notice it attaches to your Tooltip.
| | 02:32 | So now if I want to go place this, I
can just click anywhere I want to place
| | 02:35 | one, or I can actually
automatically mate these together.
| | 02:38 | And if I hold down Tab, it will actually
flip it upside down so I can change the
| | 02:42 | mating orientation, and I can
just drop it right in the hole.
| | 02:45 | Same thing over here. Go over the hole.
It just automatically will find a mate for you.
| | 02:49 | Hold down Tab, it's going to
lock into the hole, and click OK.
| | 02:52 | So it's an easy-to-place hardware,
and we can literally add millions of
| | 02:56 | different styles and configurations of
hardware to our model just that quickly.
| | 03:00 | When you are done, hit Esc, and that
turns that off, and now you've got these
| | 03:03 | holes in there, and you can
see they've mounted in there.
| | 03:06 | And then if we want to go and work
with this part here, we can just use our
| | 03:09 | standard mate techniques we've already used,
use the right mouse button, spin it around.
| | 03:12 | We can click on Mate, grab the outside
of that, grab the inside of this hole,
| | 03:16 | mate those together,
| | 03:18 | and then maybe bring that top of
the screw here to the top of the part.
| | 03:22 | Something like that, it's
a really easy way to Mate.
| | 03:25 | So you can do it both ways.
| | 03:27 | If we are using a lot of hardware in
our design and we are sharing it on the
| | 03:30 | server, that's great, but what if we
want to send our design to somebody else,
| | 03:33 | maybe a manufacturer, to build those parts?
| | 03:35 | We want to make sure that that hardware
is included with that assembly, because
| | 03:39 | right now it's stored in a different location.
| | 03:40 | So I am going to go up here to File >
Pack and Go. If I click on Pack and Go, it's
| | 03:46 | going to go out and find all the
items that are part of this assembly.
| | 03:49 | This is a brand-new assembly so I
haven't saved it yet, so we probably want to
| | 03:51 | save it first. But it's called
Assembly Two and then it's made up of
| | 03:54 | 11.8-1, and then this new
countersunk bolt that we just found.
| | 03:58 | And you can see where it is in the
folder, its name, and then where it's being
| | 04:02 | saved to, and then a lot of other
information here. In this folder, you can
| | 04:07 | go see where it's located at.
| | 04:08 | So first off, this one hasn't been found
because we haven't saved it out yet, so
| | 04:12 | let's go ahead and do that
before we go any further.
| | 04:14 | So let's cancel this, let's go File >
Save As, and we are going to save it right
| | 04:19 | here. We are just going to call this
one 11.8, and click on Save, and that's
| | 04:24 | going to save that. Now we have 11.8 assembly.
| | 04:26 | Now, let's go back to the Pack and Go.
| | 04:28 | Now you can see it's saved out correctly.
| | 04:31 | And then in the folder, we can see where
it is, so it's in Ch 11. That's great.
| | 04:35 | And then this one here,
notice it's in a different folder.
| | 04:37 | So we want to make sure we have a
folder that has all the items in one.
| | 04:40 | So we can click here and find out which
path we might be using for that, and you
| | 04:44 | generally don't want to save it
into the same folder you're already in.
| | 04:46 | Choose a different folder to save it to,
and it's going to copy all those items
| | 04:49 | and put it in that folder, so
you have a second copy of it.
| | 04:52 | The other great thing you can
do is click on Zip the file out.
| | 04:55 | So if I want to just take all those
files and put it in a new folder and zip it
| | 04:58 | up, this is the way to go.
| | 05:00 | And by the way, that's also a great way
just make a copy of your design at any
| | 05:03 | one stage you are at. You can just
make a zip copy, have everything in there,
| | 05:07 | and then any time you want to come back
to an older version of your files, they
| | 05:10 | are all in that zip file, which also
makes it really easy to email out or put on
| | 05:13 | a FTP server if you need to send a lot of files.
| | 05:15 | A couple of other things on the top here.
If we have drawings, which we haven't
| | 05:19 | covered yet, we can also include those.
| | 05:21 | We can include simulation results, as
well as a few other things in that package.
| | 05:25 | So it's really a great way to add
everything up and make sure that there's
| | 05:28 | nothing missed from that design.
| | 05:29 | Once you are happy with it,
click on Save and we are good to go.
| | 05:35 | Toolbox is a great way to
quickly add hardware to an assembly.
| | 05:38 | If you are working with others or
sending the files to a manufacturer, make sure
| | 05:41 | to use the Pack and Go Wizard to pack
those files up so they are in a nice ZIP
| | 05:46 | file and all the files are included.
| | Collapse this transcript |
|
|
12. Advanced MatesMating parts with coincident, parallel, and distance mates| 00:00 | Mates are very similar to sketch relations.
| | 00:02 | We need a minimum of two parts and
an idea of how to connect the parts.
| | 00:07 | Much like relations, we have all the
basic ways of aligning parts, for example,
| | 00:11 | Coincident, Parallel, Collinear,
Distance, and a whole bunch more.
| | 00:15 | Coincident is the most common of these
mates, and attaches two items together by
| | 00:19 | touching the selections.
| | 00:21 | In general, most parts will
acquire three mates to fully define their
| | 00:24 | location and orientation.
| | 00:26 | So we have got an assembly here with
just one part in it, and I am going to go
| | 00:29 | ahead and just tile horizontally and
just drag a couple of additional parts
| | 00:33 | into that assembly. Okay, there it is.
| | 00:35 | I can move these parts around, get
them oriented kind of the way we are going
| | 00:41 | to start assembling.
So we will start with this part here.
| | 00:44 | We will click on the mate, and my
selections here, I am going to choose this face here.
| | 00:49 | So I want to mate this block down to that face.
| | 00:52 | Now, first I am going to show you
what not to do, or what's going to maybe
| | 00:55 | cause some problems.
| | 00:56 | If I just pick like this point, this
corner of this block, click OK, it's going
| | 00:59 | to move that and make it touch.
| | 01:01 | Here is the problem though: as I move
this thing around, it's touching, but if
| | 01:06 | we look at the part itself, only that
one point is touchin. So I can have the
| | 01:10 | block that's inside of there, I can
spin this thing around, there's a lot of
| | 01:13 | things that can happen.
| | 01:15 | But that part is really not very
constraint, just really just that point that's
| | 01:19 | touching and everything
else is just wiggling around.
| | 01:22 | So let's go ahead and
delete that mate.
| | 01:24 | Hit Delete. The next Mate is going to be a line point.
| | 01:29 | So I am going to hit Mate, and I am
going to choose this line here on the
| | 01:32 | edge and that face.
| | 01:34 | So now it's going to
bring that edge down to touch.
| | 01:37 | And now what we are going to have is
kind of like more of a hinge type of mate.
| | 01:40 | So it's going to rotate around that
point, but it's really not locking it down.
| | 01:43 | So those aren't quite as powerful
mates as if we picked the whole face.
| | 01:47 | So I am going to go back and
undo that and cancel that.
| | 01:50 | So take a look at the mate, so there is
no mates now, we are free to move around.
| | 01:53 | Let's go back and mate that face here
to actually the entire face, and now that
| | 01:58 | brings that all the way down and
constrains it in, in at least two dimensions.
| | 02:01 | Now, this block moves around or I
can drag it around the screen if I needed
| | 02:05 | to. Let me start adding
some additional mates here.
| | 02:07 | Let's take a look, go down to
Mates. Let's go down to Parallel.
| | 02:11 | So Parallel is going to mate
just two faces that are parallel.
| | 02:14 | Now, we can use lines as well, but like
I said, lines are just not as powerful
| | 02:18 | as the full faces are, or surfaces.
| | 02:20 | So let's pick a whole surface versus a line.
| | 02:22 | Pick that surface there, and there is a
face here, and those are going to be parallel.
| | 02:28 | So now in Parallel, we still move
this thing around; it just blocks the
| | 02:32 | orientation so they are aligned at
least, so you can move it in and out.
| | 02:35 | Now that we have a parallel
relationship. I can move this around, and if we add
| | 02:40 | another mate, this time
we can go to Perpendicular.
| | 02:43 | Now, Perpendicular would
actually add almost the same thing.
| | 02:46 | So Parallel and Perpendicular, but I
pick a different pair, so I pick this face
| | 02:49 | here and that there.
| | 02:51 | So I will pick this and--hold on,
we have got too many things chosen.
| | 02:55 | If I select too many things, I can always go
in this box and hit Delete to take them out.
| | 02:59 | Pick there, pick there, and say
Perpendicular, and that's going to be fine.
| | 03:05 | Now, we have two mates that are
actually doing the same thing:
| | 03:06 | we have a Parallel and a Perpendicular.
| | 03:09 | And the reason I added those--
you can see Parallel here and the
| | 03:12 | Perpendicular there--as long as they
don't violate each other, there is not
| | 03:15 | going to be any problems.
| | 03:17 | But really, these are redundant.
They are doing almost exactly the same thing.
| | 03:20 | So we can get rid of either one of
those and it won't cause any problems.
| | 03:23 | The blocks still lock down.
| | 03:26 | Go back to the Mate, and this time
I am going to put in a Distance.
| | 03:30 | So down here, as far as Distance, I can
type in a number, and I can choose a pair.
| | 03:34 | So I say this face here, that face
there, and we give it a number. Or I can
| | 03:38 | change that number, say like 2.0.
| | 03:40 | I am just going to span that out.
| | 03:43 | It's not going to give you a hard
number of distance, it's going to place that
| | 03:45 | block at a certain place,
right up along that other edge now.
| | 03:50 | Those are our basic mates.
| | 03:51 | Let's spin this thing around over here on the
other side, and let's take a look at this pair.
| | 03:55 | So I am going to do a Mate here, let's
just say this face here, click on Mate.
| | 03:59 | And by the way, I can pre-select these
two faces, so I can pick that one, hold
| | 04:02 | down Ctrl, spin it around.
| | 04:04 | Let's select that other face first and
then notice I get this in-context pop-up
| | 04:09 | window and I can click on Mate
right there and it mates those together.
| | 04:12 | Now, we want this to kind of be in here
first. And right now it's kind of at a
| | 04:17 | different angle, so let's play
with a few of the other ones.
| | 04:20 | So one of the mates we can do is an Angle Mate.
| | 04:22 | So I can say like this face here and
that face there, and I can choose an angle, so 30 degrees.
| | 04:29 | And if I change that, notice
that block, it starts moving around.
| | 04:32 | I can change that angle, adjust to that
face, and I can zoom in, zoom out, so I can
| | 04:37 | adjust that to an angle if I wanted to.
| | 04:39 | And I can also flip the direction, the
other side if I needed to, and you can
| | 04:43 | change the alignment by flopping it to the
other side if you wanted to as well. Click on OK.
| | 04:47 | But that's not the orientation we're
going to need to get that in there, so to
| | 04:50 | fully define this thing,
let's go back, cancel out of that.
| | 04:53 | Let's go to Mates, let's delete that angle.
| | 04:55 | If you ever want to change or modify
or delete a relationship or a mate, we
| | 05:00 | can go down here and just click on it
and then say Edit that feature, and we
| | 05:04 | can go back and change it.
| | 05:05 | We don't necessarily have to delete it
and then reapply it; we can just go ahead
| | 05:08 | and go back in and edit that
feature or that mate. Click there.
| | 05:13 | But in this case, I actually do want to
get rid of this, so I am going to hit
| | 05:16 | Delete and there it goes.
| | 05:17 | So to bring this in here, first I have
got to save this into to this block here
| | 05:21 | and mate it together with the end of that.
| | 05:23 | And then we have got our relationship.
| | 05:25 | We can slide this up and down, and we
are probably just going to go ahead and
| | 05:29 | use another coincident mate here
to just lock these two together.
| | 05:32 | All right, there it is.
| | 05:36 | These mates will handle
most parts with flat sides.
| | 05:39 | As you get used to the Mate tools, you
will see the SolidWorks generally chooses
| | 05:43 | a mate based upon the selections you make.
| | 05:45 | You still have the option to
change the mate; however, it gives you a
| | 05:48 | good starting point.
| | Collapse this transcript |
| Mating parts with tangent and width mates| 00:00 | In this movie, we're going to cover
the Tangent mate and also the Width mate.
| | 00:04 | The Width mate is a great tool
to center one part within another.
| | 00:08 | Many times, when there is not a plane
to work with, or some other easy, center-
| | 00:11 | aligning feature, the Width mate
can solve the center alignment.
| | 00:14 | You can even handle the case
with uneven sides or angles.
| | 00:18 | But first, let's take a look
at the Tangent relationship.
| | 00:21 | So we will click on Mate,
and I've got this part here.
| | 00:24 | We are going to make that so it actually rolls
or slides around the outside of this part here.
| | 00:28 | That's where we are going to
jump into this Tangent relationship.
| | 00:31 | So first, I am going to select the pair.
| | 00:32 | If I click over here on this face and
click on this face here, by default,
| | 00:37 | SolidWorks thinks what we want is a
Concentric mate, and that would be fine for
| | 00:41 | some circumstances and I would add that.
| | 00:43 | But if we didn't, we can
actually go right next to it, and it's a
| | 00:46 | Tangent relationship. Click on that one.
| | 00:48 | Notice it pushes it out and just
makes the two faces tangent to each other.
| | 00:52 | Click on OK, and then we
have the degree of freedom.
| | 00:54 | I can actually roll over
this part right around there.
| | 00:57 | These two faces we are going to be touching.
| | 00:59 | I have two circles here, but if we had,
like, a wheel and you wanted to roll down
| | 01:03 | the road or something like that, we
could attach the wheel to a tangent
| | 01:06 | relationship along the track and I
could easily move it forward or backwards. Or
| | 01:09 | we can have things that roll around
and things like that with tangent.
| | 01:12 | So it makes it really nice.
| | 01:13 | The second case we are going
to look at is the Width mate.
| | 01:17 | Now, I've got this part
here that's locked in there.
| | 01:19 | I am going to click on that part,
and we are going to expand it out.
| | 01:22 | Now you look in here, we've got
the mates, and this thing's got three
| | 01:25 | mates attached to it.
| | 01:26 | It's got that side there,
and it's got this one here.
| | 01:29 | So I am going to delete these two here,
that one, and that one, just by hitting
| | 01:34 | the Delete key on my
keyboard by selecting the mates.
| | 01:36 | Now we should be able to move around.
| | 01:38 | Now these happened to be the exact same
size, if you look at them, but what if we
| | 01:43 | went back and change that part?
| | 01:45 | So let me go back and open this part
here, and let's go back and edit that
| | 01:49 | sketch. And as you can see, we've
got a part that's a little bit bigger.
| | 01:52 | So I am going to change this one to
1.25, and we'll change this one to 3.25.
| | 01:59 | Now this wedge is a little bit smaller.
| | 02:02 | I am going to go back into that
assembly, and you can see there is a
| | 02:06 | little space there.
| | 02:08 | If we were to go and make a mate
between like this edge and that one or that face
| | 02:14 | and that face, now the parts are here.
| | 02:16 | But if we wanted to--for instance, you
can use a Coincident mate, so we will
| | 02:20 | hit this face here.
| | 02:22 | Now the problem is, is well, we've got
this gap here at the top, right, and
| | 02:26 | that's not really what we want.
| | 02:27 | We want things more symmetrical if
they are going to fit inside there.
| | 02:30 | Obviously, that's not going to
work out as far, as that mate there.
| | 02:33 | So Coincident, let's get rid of that one.
| | 02:34 | What we do have is a thing called a Width mate.
| | 02:37 | It takes care of this situation for us.
| | 02:39 | I am actually going to delete this
other coincident relationship right now too.
| | 02:43 | So I can still move this out here.
| | 02:45 | So a Width mate looks for a pair.
| | 02:46 | So I am going to Mate, and that's
actually under, not our Standard Mate palette,
| | 02:51 | but if you look under here, we
have a thing called Advanced Mates.
| | 02:53 | So Advanced Mates has got a bunch of
different mates we are going to look
| | 02:56 | at. And keep in mind, there's also a
thing called Mechanical Mates down here,
| | 03:00 | and we've got things like Cams, Hinges,
Gears, Rack Pinion, Screws, Universal Joints.
| | 03:05 | These are more advanced mates that we
are really not going to cover in this
| | 03:08 | course, but I just want to let you
know they are there if you need to take a
| | 03:10 | look and try to play around with those.
| | 03:11 | Let's go back to Advanced Mates, and we
are going to cover several of these, but
| | 03:16 | right now we are just working on the Width mate.
| | 03:18 | When I select Width mate,
it gives me two choices.
| | 03:20 | It says one, the first thing I want
to know what are the Width selections?
| | 03:24 | I am going to spin this thing around.
| | 03:25 | I want to pick this face
here and this face there.
| | 03:29 | So basically, we want two pairs, so
basically what's going to fit between those
| | 03:34 | two faces, and then my Tab selections is
going to be the tab on this side and I
| | 03:39 | am picking on this side as well.
| | 03:40 | And let's say it's going to make the
distance between these two faces and these
| | 03:45 | two faces exactly the same.
| | 03:46 | I am going to click on OK
and that mate the lines.
| | 03:49 | Now notice, as I move that in there,
it's the same distance between the spacing here
| | 03:54 | and that spacing there.
| | 03:55 | Click on OK. Then I can go ahead and maybe add
that relationship back at the end here,
| | 03:59 | just so you can see it a little better.
| | 04:02 | So it handles the case of always
fitting that perfectly between the two faces.
| | 04:06 | Now what's even cooler about this
feature is if I go back and I change this
| | 04:10 | part, right now those outside edges are aligned.
| | 04:13 | If I were to change this to
like 2.0 and click on OK, the part
| | 04:18 | drastically changes.
| | 04:19 | If I go back over here to the
assembly, it updates. Guess what?
| | 04:23 | The Width mate has no problem with it.
It says, "No problem. I can handle that. I
| | 04:27 | can figure that out for you."
| | 04:28 | So even though these faces are not
parallel at all, it still finds the best fit
| | 04:33 | and puts it directly in
the center between the two.
| | 04:35 | The Width mate command is very handy.
| | 04:37 | It can solve mate problems that would
otherwise lead to lower-quality mates.
| | 04:41 | This is an advanced mate and it
does take more system resources,
| | 04:44 | so only choose this option
when simpler mates will not work.
| | Collapse this transcript |
| Mating parts along a path| 00:00 | The Path mate is very handy when you
want a part to move along a specific path,
| | 00:05 | specified by a sketch.
| | 00:07 | And to saw how it works I've got a
plate here, and on the plate I've created a
| | 00:11 | sketch on the top plane to define my path.
Then I've added in this little cone here,
| | 00:17 | and in the bottom of my cone I've added a point.
| | 00:19 | Now you could also use the Origin, but
in case you didn't have the origin right
| | 00:22 | at the bottom of the part, you can always add
a point or some type of a sketch to tie into.
| | 00:26 | So I want to make sure I go and View > Points.
| | 00:31 | So my first mate, so I'm just going to
say, at the top of this plate here, and
| | 00:34 | then I'm just going to spin around.
I'm going to grab just the bottom of that
| | 00:37 | part there, and let's do
a typical coincident mate.
| | 00:41 | Now I've got that plate there with
the cone on top of it, and this can
| | 00:47 | slide around now.
| | 00:48 | So now what we want to do is we
want to lock this cone onto that path.
| | 00:52 | To do so, I am just going to click on
Mate and then come into not the Standard
| | 00:57 | Mates but beloe that, the Advanced
Mates. We have one called Path Mate.
| | 01:02 | A Path mate is pretty simple to set up.
| | 01:05 | The first question it's going to
ask is I need a vertex on my point.
| | 01:08 | So I am going to use that point right
there, and then in my Path Selection right
| | 01:12 | there, I'm just going to choose that path.
| | 01:13 | As soon as I do that, it's just kind of
brings that point over and lays it right
| | 01:17 | on top of that path. And just to point
something out is this point has to be
| | 01:22 | right on the bottom of that part.
| | 01:23 | If it was in the middle of that part
for instance, it would violate that mate
| | 01:27 | because you've already made a
Coincident Mate with the bottom touching the
| | 01:29 | top of that plate here.
| | 01:31 | That definitely needs to be on the
bottom or on edge or something like that.
| | 01:34 | Click on OK, and now we've got that mate
set up. And as I grab this part here, we
| | 01:40 | should be able to drag it along that path.
| | 01:44 | It just smoothly slides along that path.
You can go anywhere you would like to take it.
| | 01:50 | The Path Mate provides a nice way to
move parts along a fixed length and path.
| | 01:55 | With a little preparation, the Path
mate can provide some very handy advanced
| | 01:59 | motion for your assemblies.
| | Collapse this transcript |
| Mating parts by aligning planes| 00:00 | When we start a new part, we have three
planes and an origin as a starting point
| | 00:04 | to construct a new part.
| | 00:06 | None of these can be deleted or modified;
therefore, if I use this to mate parts
| | 00:10 | together, they are unbreakable mates
that are easy for the computer to solve and
| | 00:14 | provide for automatic centering.
| | 00:17 | As long as we design origin-centric,
this type of mate will be perfect.
| | 00:21 | There are a few things to make
creating mates like this easier.
| | 00:25 | We're going to start by viewing the planes
that are going to be used as the mate pair.
| | 00:29 | So I have this block here, and I am
going to click on the Plus to open up
| | 00:33 | this dropdown. And I want to see
the Front Plane, and notice it shows up
| | 00:38 | here in the Right Plane.
| | 00:39 | So those show up. And then I'm going to
do the same thing for the cone, click
| | 00:44 | down here to the Front Plane, and show
that one, and then go down to the Right
| | 00:47 | Plane, and show that one.
| | 00:48 | Now if for some reason you are not seeing
these, you can always go to View and make
| | 00:52 | sure we have Planes turned on; if
I turned that off, they just hide.
| | 00:55 | Go back to View > Planes and it show up.
| | 00:57 | So you don't need to turn on all the
planes, just the ones that you are really
| | 00:59 | going to be using your mate pair.
| | 01:01 | So our first mate, we're just going to
use a Coincident Mate, just to put the
| | 01:05 | cone on top of this block.
| | 01:07 | Select the top of that block, select
the bottom of the cone, and that just makes the
| | 01:12 | first mate pair there.
| | 01:13 | So now we have a cone who is
sliding around on the block.
| | 01:17 | I am going to place it right here for now.
| | 01:21 | My next mate is going to be just
picking this pair, and we're just going to use
| | 01:24 | the Standard Coincident Mate
like we've already learned.
| | 01:26 | So I'm just going to select that plane
here and that plane there, and they come
| | 01:32 | together. And then same thing now we
have got another degree of freedom
| | 01:34 | back and forth this way.
| | 01:36 | So just go ahead and pick that pair,
so the Right Plane there, and the Right
| | 01:40 | Plane there, and notice those come
together. Pretty simple to do, as long as you
| | 01:44 | can see those planes.
| | 01:46 | Now these planes being made together
makes for a very, very powerful mate because
| | 01:50 | these planes are there from the very
beginning when we created these parts.
| | 01:53 | So if I completely change these
parts, those plane mates won't fail.
| | 01:57 | There is nothing to fail about them
because they are the fundamental building
| | 02:00 | blocks for that model.
| | 02:01 | They are also quite easy for the
computer to solve, and it gives you automatic
| | 02:05 | symmetry. It puts it right
in the center of that part.
| | 02:08 | Keep in mind, when you're designing
though, make sure we are origin-centric; we
| | 02:10 | have got the origin in the center
of our part. That way everything will
| | 02:13 | automatically align. It makes
for building assemblies very easy.
| | 02:17 | Plane mates are the strongest type of
mates, and by using them, you can build
| | 02:20 | almost unbreakable assemblies.
| | 02:23 | In small assemblies this might not
seem like a big problem; however, as your
| | 02:26 | model grows, having failing mates can
cause a cascade effect that can really
| | 02:31 | make for a bad day.
| | Collapse this transcript |
|
|
13. Hole WizardGetting started with the Hole Wizard| 00:00 | The Hole Wizard provides a quick way
to generate a variety of standard size
| | 00:04 | holes for screws, tapped holes,
counterbores, and the ability to easily change
| | 00:08 | from one style or size to another.
| | 00:11 | Let's have a block open up here and
we are going to add some holes to that.
| | 00:14 | So the best way to use a Hole Wizard
and the Hole Wizard is located here under
| | 00:18 | the Features and Hole Wizard.
| | 00:19 | And before actually opening the Hole
Wizard, select the face first and then jump
| | 00:23 | into the Hole Wizard.
| | 00:24 | Okay, you have got a bunch of choices here.
| | 00:27 | So starting at the top here, we
have got what type of holes; we've got
| | 00:30 | counterbored holes, we have countersunk
holes, we just have simple holes here.
| | 00:33 | We have tapped holes, pipe tapped
holes, and then you can actually make a
| | 00:37 | customized or a legacy-style hole by
changing and putting the values yourself.
| | 00:41 | Below that, we've got our Standard,
which we are going to cover in the next
| | 00:45 | movie, but you have got a bunch of
different types of fasteners and holes that
| | 00:49 | we can select from to choose those
type of fasteners, but, your most standard
| | 00:53 | probably would be ANSI Inch or
Metric, let's choose that one.
| | 00:57 | And then from there we have got a
variety pack of types of screws.
| | 01:00 | So we've got all these different
things we can put in there as far as
| | 01:03 | counterbored holes for these types of
screws, so binding head screws,
| | 01:08 | heavy hex bolts, pan heads, you get
all these little choices down here,
| | 01:12 | socket head screws.
| | 01:13 | So I'm going to pick like a
socket head cap screw for instance.
| | 01:15 | Don't want to get down here to Hole
Specifications as it is going to ask me
| | 01:18 | the size and the fit.
| | 01:20 | So with the size I'm going to go down to
pick like a standard size, let's pick a
| | 01:24 | big one to just make it easy to see.
| | 01:26 | So say like 1 inch and then a normal
fit, or you can choose close or loose,
| | 01:30 | depending on how tight you want to make
those fit tolerances, and if you click on
| | 01:34 | Show custom sizing, it's going to
tell you what the actual values are.
| | 01:37 | This comes in really handy because most
people don't know off the top of their
| | 01:40 | head, exactly the size hole I should
be putting in my block, for a clearance
| | 01:44 | hole for that screw, or the size of the
head of the screw or the thickness of the
| | 01:47 | head of that screw to make a nice
counterbore, so most people are not going to
| | 01:50 | have that information off the top of their head.
| | 01:52 | So SolidWorks has a nice, table lookup to
pull these values, and these are your standard
| | 01:56 | values, and if I change the values here,
you'll notice that a couple of these
| | 01:59 | numbers will change depending on if we
want a loose fit or a tight fit, as far as
| | 02:03 | the through hole there.
| | 02:04 | End Condition, come down here a little
further, we've got Through All, we have
| | 02:08 | Blind, Up To Next, these are the
same as kind of our extrude cut choices.
| | 02:12 | All right, so if I only want a hole
a certain amount of inches deep I can
| | 02:15 | choose Blind, I can say Through All to
make sure it continues to go through the
| | 02:18 | part no matter how thick it is, Up To
Next, Up To Vertex, Up To Surface, so
| | 02:21 | a lot of that kind of repeats there.
| | 02:23 | So I'm just going to choose Through
All for this one, and then you get an
| | 02:26 | option of Head clearance.
| | 02:27 | If you want it to be a little bit of
more space above, countersink this screw a
| | 02:30 | little bit deeper than it
would really need to be.
| | 02:32 | You can also add some countersinks to
either the front side or the backside
| | 02:36 | or under the head countersink or far
side countersink, just by clicking these
| | 02:40 | little tabs, these little checkmark boxes
on, and we can adjust the way that this is.
| | 02:44 | Now keep in mind, anything that we fill
out in here, these values are going to
| | 02:48 | propagate through to your drawings.
| | 02:50 | So make sure you fill it out
correctly here -- it's a common error is the
| | 02:53 | End Condition, right?
| | 02:54 | Instead of Through All they say Blind
and give it 20 inches, well that shows up
| | 02:59 | in your drawing as this hole is 20 inches
deep, or your part only might be a half
| | 03:03 | inch deep, and it clearly goes through it,
but you don't really need a drill
| | 03:06 | hole 20 inches deep.
| | 03:07 | So sometimes there is a
little area for confusion.
| | 03:09 | So if you do want to go all the way through
the part, it's best to check here Through All.
| | 03:13 | Once you've gone through and picked
all these different choices out, then we
| | 03:17 | click on this tab here at
the top which is Positions.
| | 03:19 | Now the way that the Hole Wizard will
work is it just relies upon the Point
| | 03:23 | command, here is a Point command up here.
| | 03:24 | And so anywhere I place a point,
it's going to put that hole.
| | 03:27 | I will click here on that face and
notice it gives you a visual representation
| | 03:31 | of where it's going to be placed, and
any where else I place a point, there it is,
| | 03:34 | it's just going to keep dropping those holes.
| | 03:36 | If I hit Escape, it will turn
that off or I can go up here back to the
| | 03:39 | Point command and just unselect it.
| | 03:41 | Now if I've got a point on here and I
want it, I can just make sure I turn the
| | 03:44 | Point command off first and then go
and select that point and hit Delete and
| | 03:47 | just remove that point there.
| | 03:49 | I can also -- while I am in this mode, I
can hit the Spacebar and look straight
| | 03:53 | down on these parts, I can
move these things around.
| | 03:55 | I can use dimensions to dimension them out to
the edge, to define where they are. All right,
| | 04:03 | as soon as I do that, notice the point
turns black, the other ones are still
| | 04:05 | blue, so these are still moving around.
| | 04:07 | I can snap them to something like the
origin, and then it's fully-defined with a
| | 04:11 | little relationship so we
can add relationships to them.
| | 04:13 | Then we can also use construction
geometry to draw in the Hole Wizard.
| | 04:19 | All right, and I will make a
little rectangular box here.
| | 04:24 | Then I can drag those points and
snap them over here to the corners.
| | 04:27 | Now if I want to add a few more, you just go
back to the Point command, drop a couple on there.
| | 04:32 | Now here is one thing that doesn't work.
| | 04:33 | If you actually have a point already
and you try to click on top of it, you
| | 04:37 | can add that point.
| | 04:38 | But it doesn't necessarily
always link together with that point.
| | 04:41 | So it's sometimes easier actually just
to drag an existing point over another
| | 04:45 | point so it snaps on there, so
kind of create that geometry first.
| | 04:48 | I've got one extra one almost
deleted there, and there we go.
| | 04:51 | So we can move things around and then
we can use this construction geometry to
| | 04:54 | layout that part, so I will put 2.0
there and 2.0 there, just so we have a nice
| | 05:03 | fully defined sketch, all the
lines are black and we are doing good.
| | 05:06 | So now you can see, there's all the
holes, there are multiple different ways we
| | 05:11 | define where their locations are, and as
soon as we are happy with that, we just
| | 05:14 | click on the OK checkmark and there they are.
| | 05:17 | So there's our holes placed on the part.
| | 05:19 | We can see on the back side they go
through there and it's all fully-defined in
| | 05:23 | just the standards we chose to create
this part, and notice there's a little
| | 05:26 | cheer from the top edge.
| | 05:28 | We can easily go back and modify this.
| | 05:30 | Notice it just tells us,
counterbore for 1 inch Socket Head Cap Screw.
| | 05:33 | You can always go back to this feature,
jump back in here and I can easily
| | 05:37 | change, okay, I didn't want a 1 inch,
I only wanted a half-inch.
| | 05:40 | Click on that and they all update
just that quickly, so it's easier change
| | 05:43 | from one to the next.
| | 05:45 | The Hole Wizard is based on points,
because a location of a hole is
| | 05:48 | defined by a point, to add another hole, all we
need to do is add another point to our sketch.
| | 05:53 | To change holes, we can just select
a different style and all the holes
| | 05:56 | automatically change.
| | Collapse this transcript |
| Understanding hole types and standards| 00:00 | The Hole Wizard can create
everything from tapped holes, to countersunk,
| | 00:04 | to counterbored holes.
| | 00:05 | There are a lot of options and
it's best just to go from the top, go
| | 00:08 | through them one at a time.
| | 00:10 | To get started, let's choose a face and
then select the Hole Wizard, so I am just
| | 00:13 | going to choose the top here, and
jump right into the Hole Wizard.
| | 00:16 | Now we've already covered the first one,
which is counterbore, we also have countersink.
| | 00:20 | If I click on Countersink, we've
got a few things that change here.
| | 00:22 | We get at what degree we want to use,
so we have 100 degree screws or 82
| | 00:27 | degree screws, and Oval Head or Socket Head
Countersunk Screws, we've got a lot of choices here.
| | 00:32 | And notice if I change over here to
like Metric, for instance, a different
| | 00:36 | standard, then I get a subset and type of
spec that those are going to
| | 00:41 | be built to, so for instance Metric screws are
normally 90 degrees versus the 82 or 100 degrees.
| | 00:46 | So choosing a different standard
definitely will modify the options that
| | 00:49 | are available to you.
| | 00:50 | Same thing for Metric, I get M2 through
all of my different metric sizes in here.
| | 00:54 | If I go back to inch, I get 100 degrees
or 82 degree screws, and then I get all
| | 01:01 | my standard screw sizes that I can go
ahead and put something in for us, so
| | 01:04 | I'm going to put like a half-inch screw.
| | 01:06 | This is countersunk screw, and End
Condition I've got Through All, the same
| | 01:10 | choice that we had before, and then
we can also do head clearance.
| | 01:13 | So depending on which type of hole we are
adding these options are going to change.
| | 01:18 | Simple hole, if I could click on that
one instead, I've got a bunch of options
| | 01:21 | here as far as which standard I want to use.
| | 01:23 | The Type, which would be All Drill
sizes, Fractional Drill sizes, Helicoil
| | 01:28 | sizes, Letter Drills, Number Drills,
Pipe Tap Drills, and this is really popular
| | 01:33 | one here, Screw Clearances.
| | 01:34 | So if you are just going to add some
holes to one part they are going to
| | 01:37 | obviously screw down to another part
with some tapped holes, you can use Screw
| | 01:40 | Clearances which will then provide
the right spacing around that fastener.
| | 01:44 | So if I pick like a quarter-inch screw,
the normal fit is going to be a little
| | 01:48 | bit bigger than a quarter-inch to give
it a little bit of clearance, and just
| | 01:51 | gives you the recommended size for that.
Same thing with the condition and I can
| | 01:55 | also countersink the near side of that
hole if I would like to, there's a bunch
| | 01:58 | of different options there.
| | 02:00 | Tapped holes is another one that's
really important here, and so we've got the
| | 02:03 | Type Tap, which is the Bottoming Tap
or a Straight or a Through Hole, exactly
| | 02:07 | the thread size I am trying to tap
to, so I can pick like a half 13.
| | 02:11 | I can put the custom sizing if I needed to,
or the degrees of how I want to drill the hole.
| | 02:16 | Here's the End Condition and it asks you,
if you take a look at this picture really
| | 02:19 | quick, it's actually not the very tip
of the drill, it's actually to the full
| | 02:24 | diameter of that drill, so it's
right before it tapers down to the point;
| | 02:27 | so keep that in mind when you are choosing that.
| | 02:30 | You have this little link here which
automatically figures out the correct
| | 02:33 | distance, so if I say I want a one-inch
thread depth, the hole that needs a
| | 02:37 | drill is going to have to be deeper
than that, and the method they are are
| | 02:40 | using is you go Blind Hole.
| | 02:42 | So if I change this to like 2.0, when I
go back up here, this will automatically
| | 02:46 | link together to specify
the right size and depth hole.
| | 02:50 | Now you can obviously change this and
if you wanted to put something in custom
| | 02:53 | in here, you might want to unlink those
so that it doesn't automatically change,
| | 02:56 | but you want to make sure you're at
least drilling a little bit deeper than your
| | 03:00 | tapped hole, and obviously the deeper
the better to make it easier to put that
| | 03:03 | tapped hole in there.
| | 03:04 | You can always go back and reset the values.
| | 03:07 | And there are options here, this is
how we want to show this on our part,
| | 03:11 | because it's actually not going to cut
those threads for us, it's just going to
| | 03:14 | give us a representation using a
dashed line with this method here.
| | 03:18 | We can also just pick just a hole, so it's
just going to put a hole in, which is the
| | 03:21 | correct size for the drill that you
would use to then tap the hole afterwards.
| | 03:25 | This is showing the correct size hole
with a cosmetic thread and this is showing
| | 03:28 | it with the thread section completely removed.
| | 03:31 | So I generally would not recommend this
one, it's either going to be this one or
| | 03:34 | this one, would probably the best bet,
and my favorite spot is to keep the
| | 03:37 | cosmetic thread showing where that is.
| | 03:39 | And you can give it a thread callout,
and these are some of the things that are
| | 03:42 | going to show up on your drawing as well.
| | 03:43 | So I think with a thread class you can
pick a 1B, 2B or 3B thread to designate
| | 03:49 | that on your drawing and
you've got a few options here.
| | 03:52 | And then the last major thing here is
going to be your Pipe Tap, so same thing,
| | 03:57 | what type of Pipe Tap do you have,
the size of the Pipe Tap hole, and your
| | 04:00 | different input values here.
| | 04:02 | So that's how you go ahead and
add a hole to a different part.
| | 04:06 | I am just going to put a Straight Pipe
Tap, let me go to Tapped hole, I am going
| | 04:11 | to make it half 20, and then I am just
going to click on here and just put a one
| | 04:14 | tapped hole, so we could see it and if
we go in here and look, you can see the
| | 04:18 | bottom of the hole there and
you get a little cosmetic thread.
| | 04:19 | Now the other thing I was going to
touch on here is go up to Options, click on
| | 04:23 | Options, it's under System Options,
Hole Wizard/Toolbox, and you can see
| | 04:28 | where we are pulling this data from.
| | 04:30 | So different organizations if you have
a lot of people using the Hole Wizard or
| | 04:34 | the Toolbox we can set up custom
features or holes or hardware in there, and so
| | 04:39 | it's going to be pulling
it from a certain location.
| | 04:41 | Right here we are just going the C Drive, so if
I want to go configure that, I click on that.
| | 04:45 | And these are my Toolbox Standards and I
also have the Hole Wizard standards, so
| | 04:50 | I will click on the first page there
which is Hole Wizard, and these are all the
| | 04:53 | standards that I can display.
| | 04:55 | So if I am not in Japan for instance,
I am not using that type of hardware, I
| | 04:59 | can turn that off and so
it won't show up in my book.
| | 05:02 | But you've got a lot of different
countries here and then specific companies
| | 05:06 | like Helicoil and some other companies
that are making specialty hardware that
| | 05:10 | you might be using to put into your design.
| | 05:12 | So if you do want to use those or if you
are trying to use the standard that you
| | 05:15 | don't see there, it might have been
turned off, you can go ahead and just turn
| | 05:18 | that back on then and they will show up.
| | 05:19 | Let's make sure you click up here and
you save what you have done, and then that
| | 05:23 | will show up over here in your Hole Wizard.
| | 05:25 | If you are done with that click on OK,
cancel that out and we're back to where we were.
| | 05:30 | The Hole Wizard provides a lot of
functionality and many options and types of holes.
| | 05:35 | Make sure to review all the options
in the interface, since these would be
| | 05:38 | shown on the drawing.
| | Collapse this transcript |
| Positioning holes in layout sketches| 00:00 | We can create sketches to drive the
Hole Wizard in the wizard interface or we
| | 00:04 | can predefine a sketch to place the holes.
| | 00:07 | We can also use the 3D Hole option
to place holes on different faces and
| | 00:11 | at different angles.
| | 00:12 | We've got a part here and we defined
two layout sketches on it, so here's our
| | 00:16 | original Boss, and we've got a sketch
here, which is on the top plane, so it's
| | 00:23 | kind of in the middle of that part.
| | 00:24 | And then Sketch3 here is another
little sketch on that top face.
| | 00:28 | So we're going to use those to place our holes.
| | 00:30 | We're going to go into Hole Wizard, click on OK.
| | 00:32 | Now in the past, I said to pre-select a
face right before we start the Hole Wizard.
| | 00:37 | It makes it easy just jump right in.
| | 00:39 | But in this case, when we want 3D
holes, we don't want to do that.
| | 00:42 | So we're going to go here and select a
counterbored hole, three-quarter
| | 00:47 | inch looks good, normal sizing, and instead
of going Through All, let's just say
| | 00:50 | Blind, and 3 inches is fine.
| | 00:53 | Near side countersink, that all looks great.
| | 00:56 | Click on the Positions,
| | 00:57 | now as soon as we click on the Positions, I
get this option for 3D Sketch, right?
| | 01:00 | And that's what we want. All right, and
| | 01:01 | if we just make some holes on one face,
we wouldn't choose that option, but
| | 01:04 | since I want to place these holes
all the way around the outside and on
| | 01:07 | different faces, I do want the 3D Sketch.
| | 01:09 | So click over there.
| | 01:10 | Now notice my cursor gives me which
plane I'm operating in, so the XY plane,
| | 01:15 | and it gives me the option to go start placing
some points and notice the Point command is active.
| | 01:20 | Now there's one thing interesting
about SolidWorks is, if you actually try to
| | 01:23 | click on an existing point,
it gives you a little error.
| | 01:27 | So just place the holes right
next to the points you want to be on.
| | 01:31 | And then same thing as I go over a face
like this, I can click there and click there.
| | 01:36 | Notice those are angling themselves
to be perpendicular to that face or
| | 01:40 | normal to that face.
| | 01:41 | Same thing over here, I am going to just
place these holes right next to where I
| | 01:46 | want them and same thing in the end,
place the holes, and then on this top
| | 01:51 | face, I can actually snap right to those points.
| | 01:54 | Okay, so then I hit Escape and
now I'm out of the Point command and now I
| | 02:02 | have the option, I can just drag these
points around, and I'm just going to snap
| | 02:05 | those points right to
those endpoints of these lines.
| | 02:09 | And you can see how that's coming together,
snap to there, snap to there. All right!
| | 02:16 | So we're really just building
points on multiple faces of this part.
| | 02:21 | So with one feature we
can add all of these holes.
| | 02:24 | It's pretty powerful.
| | 02:25 | I'm just going to drag them over
right to those points and notice as I'm
| | 02:31 | dragging them over, they are becoming
black which means they are going to be
| | 02:35 | fully-defined, I know exactly where they are.
| | 02:38 | And that one I didn't get, so snap it
again, there we go, and one more time.
| | 02:43 | And notice I've got relationships
turned off, so I'll go to View > Sketch
| | 02:47 | Relations, so they show up for a
second there, but they hide right away.
| | 02:51 | So once I have all those points defined
where they are, I can just click on OK,
| | 02:55 | and there it is, it places all
those holes in one feature. All right!
| | 02:59 | On multiple faces, on curved faces,
notice we're pointing towards the
| | 03:03 | outside face of that, we get some type
of a normal relationship, and same thing
| | 03:07 | over here on the sides.
| | 03:08 | So this is very powerful, especially if
you've got a lot of points to place on a
| | 03:12 | part, but the best way to do this is
actually to do these layout sketches.
| | 03:16 | Now if I went and changed one of
these sketches, these are just kind of
| | 03:19 | undefined sketches right now.
| | 03:20 | So I can just drag these things around.
| | 03:22 | If I wanted to, I can drag these out or
closer to the faces and move this stuff around.
| | 03:27 | Soon as I go back and get out of that
sketch, notice the holes, their locations
| | 03:32 | are defined by the endpoints of these
lines and that's how I am defining that,
| | 03:35 | same thing with this other sketch here.
| | 03:37 | Even though all the holes are created
with just that one feature, I'm using two
| | 03:41 | separate sketches to define
where their locations are.
| | 03:44 | Click on that and notice those will
automatically move out based upon those sketches.
| | 03:49 | So it's very powerful and a nice
way to add a lot of holes to one part
| | 03:53 | just using one feature.
| | 03:55 | And if I needed to, I can always click
back in here and easily change this, say
| | 03:59 | like to a 1-inch hole, they all
automatically update and just that quick to go
| | 04:03 | from one type of hole to the next.
| | 04:05 | I can even go to say we have a
different size hole, I could change this to a
| | 04:08 | tapped hole for instance.
| | 04:10 | Click OK and there it is.
| | 04:11 | Just easily changed from tapped hole
to counterbore or countersink hole, any
| | 04:15 | options I want, I can
easily change between the two.
| | 04:18 | By using a separate sketch to drive
the Hole Wizard, we can have a dynamic
| | 04:22 | feature that will adapt to the driving sketch.
| | 04:24 | We also have the ability to create
holes on multiple faces all in one feature.
| | Collapse this transcript |
|
|
14. In-Context ModelingLinking sketches to other parts| 00:00 | The real power of SolidWorks starts to
shine when you link one part to another.
| | 00:05 | If we think about assemblies as a whole,
instead of individual parts, we can use
| | 00:09 | one part to drive the other.
| | 00:11 | Think about a jar and a lid.
| | 00:12 | Wouldn't it be nice if we made
the jar bigger that the lid would
| | 00:15 | automatically change size to fit?
| | 00:17 | We can, and we could do so much more.
| | 00:19 | Now we've seen this part before, we're
going to go ahead and modify this assembly.
| | 00:23 | If you've got two parts in an assembly
here and what we're going to do is we are
| | 00:27 | going to modify the base of this part.
| | 00:28 | So right now, if we open up one of
these parts, File > Open, take a look at it,
| | 00:34 | let's look at the sketch real quick, and
inside there you can see, we've got all hard
| | 00:37 | numbers, we've got a three-inch
diameter here, which is a double-dimension
| | 00:40 | because it's going to
across this centerline here.
| | 00:42 | We will go back to the other part, same
thing as I have got all hard dimensions
| | 00:47 | here showing exactly the size of that
part, so this is the dimension we are
| | 00:51 | going to change here, it's the 3-inch dimension.
| | 00:51 | So if I change this dimension here
to 4 inches, it should get bigger.
| | 00:57 | If I go back to my assembly,
notice we've got a problem.
| | 01:01 | The lid didn't change size, so I'd
have to go back and physically change the
| | 01:05 | size of that lid to match so, change
this to 4.0 and then everything should
| | 01:11 | be fine, in that situation go back
to the Assembly, and there it is, so
| | 01:15 | everything looks fine.
| | 01:16 | But wouldn't it be a lot better if we could
actually just link this lid to the size
| | 01:20 | of the base, so if I change the base
size that lid would automatically change.
| | 01:23 | So instead of having to go back to
the individual parts to do that, we can
| | 01:26 | actually do that right here in the assembly.
| | 01:28 | So I am going to click on the lid part
here, and notice, the first option is
| | 01:32 | Open Part, but the second
one here is called Edit Part.
| | 01:34 | So we are going to be editing this
part now in context to this sssembly, and
| | 01:38 | notice it changes to a blue color and
I can expand it out, and I have all the
| | 01:42 | same features and sketches
I do in the individual part.
| | 01:45 | So the sketch here for that Revolve1 is
the one that actually controls the size,
| | 01:50 | so that's the one I need to edit.
| | 01:51 | When I click on that I'm going to say Edit Sketch,
hit the Spacebar and click on Normal To.
| | 01:55 | Then I can see this four-inch
diameter here, and you can see it kind of in
| | 01:59 | context to the other part
too which makes it really handy.
| | 02:01 | So what we want to do is
delete this four-inch dimension.
| | 02:05 | By doing that, now I have the ability
to kind of drag the size of this lid out
| | 02:09 | and move it around, and that's what we want.
| | 02:11 | We want to give it a degree of freedom that
we want to control by linking to another part.
| | 02:15 | Now notice up here in the
upper left-hand corner, there is a thing
| | 02:18 | called No External References.
| | 02:20 | Make sure that's not turned on,
because if that's turned on it will not let
| | 02:23 | us link to another part, and sometimes
you don't want to be able to link your
| | 02:26 | part together, you just want to be
able to change it without adding links,
| | 02:28 | but in this case we do want to add a link or
reference to another part which is the base here.
| | 02:32 | So to do that, I can either drag this
point here and have it snap on to this
| | 02:37 | corner, but that's probably not going
to be the best method for doing that
| | 02:41 | because what if I want to be able to
move the lid up and down, that wouldn't
| | 02:43 | allow me to do that.
| | 02:44 | So instead of doing that, I am just
going to make a relationship here that says,
| | 02:47 | hold down Ctrl, select the two, I am
going to say Colinear, outside of the base
| | 02:52 | and the outside of the cover will be colinear.
| | 02:54 | So now notice they both become all
black and fully-defined, so it knows
| | 02:59 | exactly what size it is.
| | 03:00 | Now I am going to exit out of that
sketch and then exit back into the assembly.
| | 03:04 | Now you are thinking nothing changed.
| | 03:06 | Well they didn't, but how about if we
go back and change the base part now?
| | 03:11 | So here is our part, I am going to physically
change this part by changing this to a 6 inch.
| | 03:15 | So now that part changes, and when I go
back to the assembly, we are hoping that
| | 03:19 | the lid changes size too.
| | 03:20 | So here we go, there is the lid, it
didn't change quite yet, but it says
| | 03:23 | Models have changed.
Would you like to rebuild?
| | 03:25 | Yes, and there it is, pretty nice.
| | 03:28 | So now anytime we change the size of the
base, the lid is automatically going to
| | 03:31 | resize and change shape.
| | 03:33 | Now we've only added one link to another part.
| | 03:35 | There can be hundreds of links to other parts.
| | 03:37 | You can make a very, very complicated
assembly that has parts that are changing
| | 03:41 | size and related to all types
of different parts.
| | 03:44 | Keep in mind though, it's best practice to
choose one part which is going to be your
| | 03:47 | driving part and then have most of
the other parts linking to that part.
| | 03:50 | So you just have to change one
part and the other parts will change.
| | 03:53 | You can get yourself into a little
bit of a problem if you have a circular
| | 03:56 | reference when you have one part
referencing another one, and then that one
| | 03:59 | comes back and references the
beginning part so try to avoid the circular
| | 04:02 | reference and try to stay with one
part as your driving part and other parts
| | 04:06 | linking to it to control their size.
| | 04:08 | External references can generate highly
-automated assemblies that really show
| | 04:12 | the power of SolidWorks.
| | 04:14 | Best practice is to have one main
driving part and the others reference it.
| | 04:18 | It is possible to create a circular
reference so make sure you think through how
| | 04:21 | your design is laid out.
| | Collapse this transcript |
| Linking to layout sketches| 00:00 | Much like linking to other parts, we can have
a layout sketch that drives a series of parts.
| | 00:06 | SolidWorks has a built-in layout
function, and we can also use standard
| | 00:09 | sketches to layout designs.
| | 00:11 | To start using a layout we need to create a
layout in the Assembly Mode of SolidWorks.
| | 00:16 | In this example I've got a layout
made for this part here and I have got a
| | 00:20 | sketch for the next part that
we're going to be putting in there.
| | 00:23 | Now you can tell we are in the Layout
Mode, because if you look at the very top
| | 00:26 | of the tree you can see this little
wooden four-bar mechanism, that means we
| | 00:29 | are using a layout.
| | 00:30 | So if I right-click on that I can go
down to Layout and I can take a look
| | 00:34 | at that layout sketch.
| | 00:36 | So it's a pretty simple sketch here, but
basically i've just kind of octagonal shape
| | 00:39 | here of one-quarter of an octagon,
and then I've got a couple of the lines
| | 00:43 | here laid out for a little rib we
are going to add to this to design.
| | 00:46 | I've got to mention here that's
driving the outside of that part.
| | 00:49 | So if I go back and exit out of that
layout, now by the way to get into the
| | 00:54 | original layout when I start a new file,
under Assembly click on OK, it gives me
| | 00:59 | the option right when I start a new
assembly, do I want to create a layout?
| | 01:02 | If I did click on that, it would just
drop me directly into that on a Sketch
| | 01:05 | Mode in the layout portion of SolidWorks to
start just sketching out what our layout is.
| | 01:10 | Now the nice thing about layouts, you
don't need to worry about overlapping
| | 01:13 | lines, or have a complete sketch, it
doesn't really matter because none of these
| | 01:17 | entities are actually going to be
directly used for creating geometry, or an
| | 01:21 | extrude or something like that.
| | 01:22 | It's just the layout for that and then
we are going to convert those entities or
| | 01:26 | link to them in our other sketches.
| | 01:28 | So I am going to go back to the part I
have open, which is here, and we're
| | 01:32 | going to go ahead and add-in this new part.
| | 01:34 | So adding a new part, we can do it in
several different ways, one of them is we
| | 01:37 | can just go start new part and then drag and
drop it into the assembly, and then mate it up.
| | 01:41 | We always want to have our parts fully
mated before we start working with them
| | 01:45 | in context to these other parts, that
way they are not going to move around and
| | 01:48 | the sketches won't be skewed.
| | 01:49 | So the second way would be to actually
go to Insert Components, and under there,
| | 01:53 | is a thing called New Part.
| | 01:54 | So if we click on New Part it's going to
allow me to actually put a part, it's a
| | 01:58 | virtual part inside of this assembly.
| | 02:00 | Before we do that we want to make sure
though that we save out our assembly.
| | 02:04 | So under File, do a Save As or
Save, to make sure you've got a nice
| | 02:08 | filename saved to that, because
that new part is going to be saved
| | 02:10 | underneath that filename.
| | 02:12 | So I go to Insert Components > New Part,
you'll notice it dropped a new part here
| | 02:16 | and I just click on OK, and this is a
virtual part, it's just in this assembly,
| | 02:19 | it's not saved anywhere on the
file system right now at all.
| | 02:21 | If I want to edit that part I can just
click on it and go to Edit Part, and what
| | 02:26 | we want to do is, create this little
rib here, and to do that I am going to go
| | 02:29 | down here to find the
corresponding plane that would match up.
| | 02:33 | So probably the Front Plane in this situation
would work, that way it's on the bottom of
| | 02:37 | this part and we're going to go under
Sketch, and start a new sketch there.
| | 02:41 | Hit the Spacebar, which is then going to
make it, I am looking down on the part.
| | 02:44 | So I've got these entities that are
from the layout sketch, and I am going to
| | 02:48 | use those to layout my design.
| | 02:50 | Now these two down here I can just
convert those directly over, so I am going
| | 02:53 | to click on Convert Entities, just by selecting
the two, hold down Ctrl and say Convert Entities.
| | 02:58 | Those just bring those from the
layout sketch directly into this sketch.
| | 03:01 | Then we've got the line command and I am
just going to start from that end point
| | 03:05 | and drag it up here.
| | 03:06 | I don't want to go all at the end, I
just want to come to the inside, and I am
| | 03:09 | going to snap to that intersection, I
am going to come over here and snap to
| | 03:12 | that intersection and then the last one,
all the way down here and snap there.
| | 03:15 | So I am just snapping to that
underlying sketch and leveraging some of
| | 03:19 | that layout geometry.
| | 03:20 | Once I have the shape I want, I can say,
okay, I want to go down to a feature
| | 03:24 | and notice we're in the Assembly Mode
so some of the tool palettes are in a
| | 03:27 | different order here, Boss Extrude is
over here now, and we're going to type in
| | 03:31 | half of an inch, 0.5 and click OK.
| | 03:34 | So now we've just added this part to
this assembly and notice we are still in
| | 03:38 | the Editing Mode, so I want to go back
to assembly, I click here, now I am back
| | 03:42 | into the Assemble Mode and I
have got a couple of parts here.
| | 03:45 | Now this part here is a virtual part,
if I want to save that out to the file
| | 03:48 | system I can right-click on it and I
can say Save Part (in External File),
| | 03:53 | here it is, and that will actually save
it out to the file system, but I don't
| | 03:56 | need that quite yet.
| | 03:57 | Now what I am going to do is, I am
going to go back to that layout sketch and I
| | 04:00 | am going to change the layout, and
hopefully these parts are going to
| | 04:02 | automatically adjust, so let's go try that out.
| | 04:04 | Go down here to Layout, and
instead of 24 I am going to click on 36.
| | 04:09 | Click on OK, you can see that sketch
automatically adjusts, go back and the part
| | 04:14 | should rebuild, and notice both of those
two parts have now adjusted to that new
| | 04:18 | layout sketch, so that sketch
is driving both of those parts.
| | 04:21 | Now I've created a circular pattern
already with the Circular Pattern command,
| | 04:26 | and I've got the parts rolled back a
little bit here, so I am just going to roll
| | 04:29 | it forward, and I am going to
go, we'll take a look at that.
| | 04:32 | So now I have the outside in the pattern,
but I don't have this new part, so I
| | 04:36 | am going to go and add that in,
and select Components to Pattern, I tap
| | 04:40 | the first one, I am going to add
that second one in, there it is.
| | 04:42 | Now I have all four
sides of that thing complete.
| | 04:44 | And I am just going to back one more
time and see if we can change that layout.
| | 04:50 | We're going to go, look at the part
straight on and I am going to drag this up a
| | 04:55 | little bit and change that to 48.
| | 04:57 | And so you can see the layout sketch
expands out, so as you go back, all those
| | 05:03 | parts are automatically driven,
and you can see the circular pattern
| | 05:07 | automatically updates as well.
| | 05:08 | Layouts can be very helpful to give the
ability to drive a large amount of parts
| | 05:12 | from the same layout.
| | 05:13 | It also creates a clear order,
what's driving what, just by changing one
| | 05:17 | single sketch.
| | Collapse this transcript |
| Using the Hole Wizard in context| 00:00 | We have already learned
the power of the Hole Wizard.
| | 00:03 | Now let's take it to the next level by
linking the location of the holes to another part.
| | 00:07 | In order to do this, we need to
edit a part within the assembly.
| | 00:10 | Then we simply open the Hole Wizard and
choose a reference point in another part.
| | 00:14 | Let's give it a shot.
| | 00:15 | I've got base plate here, and notice
there's no holes in it, and then I've got a
| | 00:19 | plate that has four counter board
holes and then over here I've got a little
| | 00:24 | socket head cap screw that we'd like to install.
| | 00:26 | Problem is before we can install it we
need to add some tapped holes in this plate
| | 00:30 | and we want to add those in context.
| | 00:32 | We don't have to memorize what whole
spacing was here, we just want to place
| | 00:35 | them directly underneath where these holes are.
| | 00:37 | And this thing by the way
is still floating around.
| | 00:39 | We haven't locked this down at all either.
| | 00:41 | So let's go ahead and edit
this part in the assembly.
| | 00:44 | To do that let's click on the part
and over here it shows up highlighted.
| | 00:47 | And if I left mouse click it, I can
say File Open Part or Edit Part and Edit
| | 00:52 | Part is what I'm looking for, click OK.
| | 00:54 | And notice everything turns blue
meaning that we're editing within context of
| | 00:58 | the assembly and I'm going to pick this
top face to use the Hole Wizard on and
| | 01:03 | I'm going to click on Hole Wizard and
then come down here to a tapped hole and we
| | 01:08 | want a tapped hole through and half 13 is
the size we're looking for, and I want to
| | 01:12 | just say Through All.
| | 01:13 | And I am going to make sure we got all
the correct things filled out here as far
| | 01:18 | as thread class 2B and we'll add a
little nice near side countersink.
| | 01:21 | I am going to jump over here to
Positions and notice as soon as I do that I get
| | 01:25 | a little point on my cursor and because
I have Point command turned on, that's the
| | 01:28 | default for being inside of the Hole Wizard.
| | 01:30 | Now I'm going to hit the Spacebar, click
so I'm looking directly down through here.
| | 01:34 | Now I can snap to any
points here in context.
| | 01:37 | So I'm going to right in the center of
this hole and notice as I go over the
| | 01:40 | edge of these holes it gives me four
little quadrants and the center point.
| | 01:43 | So I'm going to snap right there,
pretty easy to put these in context.
| | 01:46 | I just go over here, snap and notice it
doesn't show me that center point till I
| | 01:50 | actually mouse over the
edge and then it pops up.
| | 01:53 | Okay and last one here.
| | 01:55 | Now those holes have now been added in context.
| | 01:58 | As soon as I'm done adding holes, hit Escape.
| | 02:00 | Turn that Point command off.
| | 02:02 | I got four holes in context and the Hole Wizard, I
click OK and then click OK again and go back.
| | 02:08 | Now notice just that quickly I've added
those holes to the assembly, they
| | 02:11 | show up below here and I'm going to go ahead
and add a relation here or mate this together.
| | 02:17 | I am going to say that external there
with this here, and then I think the inside
| | 02:22 | of this, the bottom of that
with the bottom of the fastener.
| | 02:26 | All right, now what I have is a plate and I
just have one of the socket head cap screws installed.
| | 02:32 | You can se there it is in the bottom, I've
the tapped holes and here's the power of that.
| | 02:35 | So whereever I want to place this
plate now I can drag it over here and watch,
| | 02:39 | as soon as I click on rebuild, the holes
automatically will follow that plate to
| | 02:44 | wherever it's going to be.
| | 02:45 | So you need to move things around
and click on the rebuild which is that
| | 02:48 | red light green light.
| | 02:49 | And then it just rebuilds the assembly,
brings the part over to where it's new location is.
| | 02:53 | And so wherever I put these parts,
the holes are automatically going to
| | 02:57 | follow as well as any other mate
references I have like a fastener or
| | 02:59 | something like that.
| | 03:00 | So that's using the Hole Wizard in context.
| | 03:02 | Using the Hole Wizard in context is a
great time saver, and using this technique
| | 03:06 | can be a nice design improvement.
| | 03:08 | To create a mating hole pattern we
don't even need locations or spacing.
| | 03:12 | All that info is received from the attach part.
| | 03:14 | If the attach part changes, the
corresponding holes update and life is good.
| | 03:19 | Changes are inevitable.
| | 03:20 | And the more self-solving you can make
your model in the beginning, the more
| | 03:24 | your model will pay dividends in the end.
| | Collapse this transcript |
|
|
15. Creating Threaded PartsCalculating values for creating a threaded part| 00:00 | SolidWorks has several ways to
represent threads including the Hole Wizard
| | 00:05 | and cosmetic threads.
| | 00:06 | However, if you really need to create
threads, we need to use a swept cut to
| | 00:10 | actually cut those threads.
| | 00:12 | This can be time-consuming and
adds a complex feature to your model.
| | 00:15 | As with all sweeps, we
need a profile and a path.
| | 00:18 | The profile is just a 60 degree
triangle and the path is a helix.
| | 00:22 | Now for the hard part.
| | 00:24 | We need to input the correct values into
the helix and the profile sketch to get
| | 00:28 | the correct thread when finished.
| | 00:30 | Let's look up the thread data from
the Machinery's Handbook or any other
| | 00:33 | threading reference.
| | 00:34 | The size thread we're
going to use is a 1-inch 16.
| | 00:38 | Before we go and look that up though,
I'd like to cover how we got to this stage
| | 00:41 | in this bolt creation process.
| | 00:43 | So I am going to roll back using the
history bar at the beginning and I just
| | 00:46 | have a piece of hex stock just created
with a simple hex sketch, extruded that out.
| | 00:50 | And then the next one here is going to
be the revolved cut and we did something
| | 00:54 | very similar to this in an earlier movie.
| | 00:56 | Click on the sketch and I am
going to take a look at how it looks.
| | 01:00 | Now from here, I am going to go around here,
we've got a little lead-in to the thread.
| | 01:03 | This is a section that's going to be
threaded, we have a little thread really for
| | 01:05 | the backside and then just finish
it off as far as the outside shape.
| | 01:08 | Now these values here, this value here
in particular, this is going to be our
| | 01:12 | major diameter for our thread and
this is what we're going to look up this
| | 01:15 | value to input into the sketch.
| | 01:17 | So then we just do a revolved cut on
that and we're back to the stage we're here.
| | 01:20 | Then what we're going to do here is
just we're going to do a revolved cut to
| | 01:23 | just trim off the top of the bolt, make
it look right, and then we're going to
| | 01:27 | create this sketch here to
actually cut those threads.
| | 01:30 | Okay, so let's jump over
to the Machinery Handbook.
| | 01:33 | So this is a Machinery's Handbook and
it's a very common reference, and if you
| | 01:37 | don't happen to have one, you can
always buy one from Amazon or Barnes & Noble
| | 01:42 | or any major bookseller out there.
| | 01:43 | And this is the digital copy version
so I have a PDF of it and I can look
| | 01:47 | things up quite easily, or if you
might have the paper copy, that's just the
| | 01:50 | same to look things up.
| | 01:51 | So we're going to first
look at the thread profile.
| | 01:53 | So here's a standard unified thread
profile and it's a 60 degree profile.
| | 01:58 | If you notice, everything is based
upon the P, and the P is the pitch.
| | 02:02 | And so pitch means 1 divided by
the threads per inch and we're going
| | 02:07 | to calculate that out.
| | 02:08 | And what that means is what a pitch is,
if I turn the thread or the bolt one
| | 02:13 | turn, how far does that progress.
| | 02:15 | That's what the pitch is.
| | 02:16 | Okay, you can see most of the
values here are based upon the pitch.
| | 02:19 | The pitch line is a 0.5P and the basic
pitch diameter is what we're going to be
| | 02:24 | looking up from the table, and you
can see that everything here is laid out
| | 02:28 | based upon the P. So thread pitch is 1
divided by the threads per inch or TPI.
| | 02:33 | In this case, we have 16 threads per
inch and so that's going to be 1 divided by
| | 02:37 | 16 which equals to 0.0625.
| | 02:41 | Now let's go over and take a look at the table.
| | 02:43 | So here's the table and we're going to
look at the 1-inch 16 thread, and we're
| | 02:48 | going to look at the 2A variety of that.
| | 02:50 | As you can see, external threads have a major
or a max and min diameter kind of laid within.
| | 02:56 | So in this case, we have a max diameter
of 0.9985 and a min diameter of 0.9891.
| | 03:03 | So if I average those, I get .9938.
| | 03:05 | The next column there
would be the pitch diameter.
| | 03:08 | In this case, we have a max
of 0.9579 and a min of 0.9529.
| | 03:14 | Average those and I get 0.9554.
| | 03:17 | Those are the values we're going to
be using to put into our sketches.
| | 03:21 | Back in our sketch, let's just review
inside of the sketch here we used for
| | 03:25 | revolve, this value here, this 994,
that's our first value we calculated.
| | 03:30 | If I double-click on that you can see it's
exactly the number I told you. It's 0.9938.
| | 03:34 | It's a four-place decimal, so when I
click OK, it's actually rounded down to a
| | 03:38 | three-place decimal.
| | 03:39 | Okay, that's my first input value,
that's going to give the major overall.
| | 03:42 | Even though it's a 1-inch thread, most
of the time those are slightly undersized
| | 03:46 | for the actual nominal value it's
calling out for like the 1 inch.
| | 03:49 | Okay, and next is going to be this
profile sketch and I am going to open that up
| | 03:55 | and let's take a look what's inside here.
| | 03:57 | This 0.955, if I double-click on that,
that's the same value we came up with
| | 04:01 | for the pitch diameter.
| | 04:03 | So that's 0.9554 and that's what
we're going to input into the equation.
| | 04:07 | It's a triangle here with a 60 degree
triangle and here is the pitch line that
| | 04:12 | we defined and we're going to input that value.
| | 04:14 | Before I do that, I am actually just going
to show how to create this just real quick.
| | 04:17 | So I am going to delete all that
and we'll start from the beginning.
| | 04:20 | I am going to start with construction
line, I am then going to snap it right to
| | 04:23 | the end of that bolt.
| | 04:24 | Here it is, bring it out, and then I am
going to continue on with just a regular line.
| | 04:29 | I am going to draw a triangle.
| | 04:33 | One more construction line in the
center there and let's start at that point, I
| | 04:36 | am just going to drag it out and I am
actually going to cut it short there and
| | 04:40 | then I am going to add a relationship.
| | 04:42 | So I am going to say that point, hold
down Ctrl, select that line, and I am
| | 04:45 | going to say Make Midpoint.
| | 04:46 | Now I am going to add some
relationships and some dimensions, so I am going to
| | 04:51 | say this is a 60 degree triangle,
which we know from thread profile chart.
| | 04:56 | And I don't want this sticking out too
much further than the outside of my bolt,
| | 04:59 | so I am actually just going to make
another little construction line and then I
| | 05:02 | am going to merge these two points together.
| | 05:04 | And the next line we need is a little
center line and this is just between
| | 05:10 | the two outside edges, and make sure you
don't snap that to the midpoint or anything.
| | 05:13 | We just want this to be able to move in and
out, so it's a construction line we can move.
| | 05:17 | Now this is the pitch line, it's
actually half the pitch line, so what I want to
| | 05:21 | do is input that value.
| | 05:22 | So I am going to click on
that line and come out here.
| | 05:24 | Now I can use this input bar here to
actually calculate things out for me.
| | 05:28 | So as I remember from that table, the
pitch is 1 divided by the threads per inch.
| | 05:33 | I'll type in 1 divided by
16 or 16 threads per inch.
| | 05:37 | And then from the profile sketch we saw
earlier, it's actually divided by 2, so
| | 05:41 | I am going to divide it by 2.
| | 05:42 | And I can do all that in one
calculation right here in just the input bar.
| | 05:45 | Click on OK and that solves
it out for us giving 0.031.
| | 05:49 | The last piece of information we
need here is the pitch diameter.
| | 05:53 | Now we calculated it as 0.9554,
so let's go input that value now.
| | 05:57 | I am going to click on this center line here.
| | 05:58 | From this center line, I am going to
click on this little point here and notice
| | 06:01 | if I go across that center line,
it turns into a double dimension.
| | 06:05 | So I can actually input
exactly the value I calculated.
| | 06:07 | That's what I want to do.
| | 06:08 | I am going to type in 0.9554, click on OK.
| | 06:13 | Notice my sketch is now fully defined.
| | 06:15 | I've got all of the lines are
black and so I am pretty good.
| | 06:18 | Now in the next movie we're going to
create the helix and then finish out the
| | 06:22 | cut by doing that revolved
sweep to cut out that profile.
| | 06:25 | It takes a bit of work to create real
cut threads, so I would not recommend this
| | 06:29 | option for all situations.
| | 06:30 | However, if you're going to rapid-
prototype your parts or just want real threads
| | 06:35 | to look visually correct, this is the option.
| | Collapse this transcript |
| Using a helix sweep path to create a thread| 00:00 | The next step in the thread creation
process is generating a helix that will
| | 00:05 | guide the Cut tool.
| | 00:06 | To do this, we need to draw a circle
that will be the size of the helix.
| | 00:09 | Let's get into the Helix tool and get started.
| | 00:11 | Before we do that, you can see on the screen
this is exactly where we left off in the last movie.
| | 00:16 | We have a profile of the shape of a 60
degree triangle, which we're going to use
| | 00:20 | a helix to drive around
this part to cut the threads.
| | 00:24 | So now we need to create the helix.
| | 00:25 | So I'm going to exit out of the sketch,
and you can see that sketch was there
| | 00:28 | and now we're going to go --
| | 00:29 | I'm going to make sure we are viewing sketches,
| | 00:32 | so we can see where that sketch is, and now
we're going to go ahead and create a helix.
| | 00:35 | To do so, I need to say
Insert > Curve > Helix.
| | 00:39 | Once I do that, the first part of
creating a helix is I need to select a face for
| | 00:42 | playing, I need to draw a circle
that's going to be the size of that helix.
| | 00:46 | So I'm just going to
pick the very front of this bolt.
| | 00:48 | So I am going to click on that, I am
going to click on the Spacebar, Normal To
| | 00:52 | it, I am going to use
just this outside edge here.
| | 00:54 | I could either draw a circle myself or
just click on that outside edge and covert it.
| | 00:59 | So bring that entity into the current sketch.
| | 01:01 | Notice if I do that, it
just brings that sketch here.
| | 01:03 | As soon as I exit out of this, it's
going to go directly into the Helix tool,
| | 01:06 | and sometimes it's a little hard to
figure out exactly where you are because
| | 01:08 | there is no little window that
tells you do this or do that.
| | 01:11 | So it's going to make you draw a circle
and as soon as you exit out, it's going
| | 01:14 | to go into the Helix Tool. Okay,
| | 01:16 | so we have a couple of
different ways to define a helix.
| | 01:19 | First one is Pitch and Revolution, but
we can also do Height and Revolution,
| | 01:22 | Height and Pitch, Spiral,
a lot of things we can do.
| | 01:24 | But we're just going to
leave default one there.
| | 01:26 | Now the constant pitch is what we
want and here's the pitch, right?
| | 01:29 | So I got to that number by just using
the Input Bar to do the calculation, I say
| | 01:34 | 1 divided by 16 threads per inch,
and that's what the pitch is.
| | 01:38 | And we are spinning the correct direction, if
we are going the wrong way, we go this way.
| | 01:43 | So if we can always flip that one way
or another and then I can figure how many
| | 01:46 | revolutions it's going to take me to get
down to the base of this thread. Okay,
| | 01:49 | now the other thing that is very
important is notice this start angle here.
| | 01:53 | We want to make sure we're
starting our helix right at that sketch.
| | 01:57 | So if I zoom in here, notice this little start
arrow is right at the same level of that sketch.
| | 02:03 | It's a little bit hard to see on
the screen, but that's going to be
| | 02:06 | starting right there.
| | 02:07 | So I could adjust this angle to make
sure that that start point is right at the
| | 02:11 | same plane as where I drew
that sketch, so make sure you do that.
| | 02:14 | If it's over here, some like that,
it's going to give you an error, and then
| | 02:17 | make sure we're going either clockwise
or counterclockwise to make sure we're
| | 02:20 | doing the right type of thread, either
right-hand thread or left-hand thread.
| | 02:23 | Once all that looks okay, click on the
check mark, there it is, and we can verify
| | 02:27 | our thread, just by zooming in making
sure that it looks way it's supposed to, I
| | 02:32 | am going to spin it around.
| | 02:33 | Okay, so now we have a profile, and we have
a path, and we are ready to do the swept cut.
| | 02:38 | I'm just going to click on Swept Cut,
and for the profile, I'm just going to
| | 02:42 | zoom out a little bit here, and I'm going
to pick that first sketch.
| | 02:45 | That's going to be our profile sketch, and
then our second one is going to be our path.
| | 02:50 | We're using that Helix as our path.
| | 02:52 | As soon as I click on that, it gives me
a little preview of what it's going to
| | 02:55 | look like, as far as cutting down the
line there, and all the other options we
| | 02:58 | just leave them as their defaults.
| | 02:59 | Click on OK and there it is.
| | 03:02 | We've cut those threads and you can
see how they look, they're pretty nice.
| | 03:06 | So that's a real cut thread on a part,
and this is part of the standard, part of
| | 03:11 | the Machinery Handbook, as far as
those input values and we can use the same
| | 03:14 | exact method for any size thread.
| | 03:16 | It's a 60 degree thread or if you needed
to create an ACME screw thread or some
| | 03:20 | other shape thread profile, it's
really just a matter of changing that 60
| | 03:23 | degree triangle to whatever thread
profile you might be using, and just make
| | 03:27 | sure you got the correct pitch
diameter and that overall outside diameter of
| | 03:30 | your thread correct.
| | 03:32 | The Sweep tool can be used to make a
variety of shapes and a thread profile
| | 03:36 | is just one of them.
| | 03:37 | The key point to remember in
creating threads is that the process will be
| | 03:40 | the same each time.
| | 03:41 | So make sure to use good
thread values from a table.
| | 03:44 | Also, make sure to specify the
correct thread in class on your drawing.
| | Collapse this transcript |
| Understanding internal and external threads| 00:00 | The process to create internal threads
is the same as with external threads.
| | 00:05 | However, there are a few subtle
differences that we will review.
| | 00:07 | First off, let's open up 15.3-1.
| | 00:11 | This is a simple part with a
hole that we want to thread.
| | 00:13 | Take a look at the screen here, I can
see that I am actually sectioning this in
| | 00:17 | half so I can easily see the
part we're going to be working with.
| | 00:19 | And if I go back and turn that off
see the hole, and I created this hole
| | 00:23 | just with a revolved cut, and we did
that right here in the Front Plane, and my
| | 00:27 | sketch just looks like this.
| | 00:29 | Okay I've got just a rectangle with a
little chamfer added to the upper corner
| | 00:34 | there with 45 degrees, and giving it 100,000
chamfer, and then this value here is
| | 00:40 | the 0.939 is the value that we looked up
from the Machinery Handbook, and if you
| | 00:45 | didn't catch the movie at the
beginning of this chapter where we did that, we
| | 00:48 | are going to do it again in this
movie to look that internal diameter up.
| | 00:50 | So we are going to go
ahead and do that right now.
| | 00:54 | Okay, and the thread size we are
creating is a 1-16.
| | 00:57 | And we are using an internal thread this
time so we are going to go look up these values.
| | 01:02 | As you can see, the diameter has a max
and min value, and we want to kind of
| | 01:06 | shoot right for the middle of those,
that would make sure that it's not too big,
| | 01:09 | too small, we are right in the middle
so we have a little leeway either way.
| | 01:11 | As you can see the max diameter is 0.946
and the min diameter is 0.932, and so
| | 01:18 | if we average those out, we get 0.939.
| | 01:20 | And on the pitch, which is the next
column over, we get a minimum of 0.9594 and
| | 01:27 | a max of 0.9659, if we
average those we get 0.963.
| | 01:33 | So those are the two values we are going
to use as our input values in our sketches.
| | 01:36 | Back here at the sketch, you can see
that diameter value, there it is, that
| | 01:40 | 0.939, that's where that gets input.
| | 01:42 | I am going to exit out of that, and
now you can see that we've got a start of
| | 01:46 | another sketch here, and I am going to
put the Section View back on so we can
| | 01:50 | see easily in there.
| | 01:52 | So let's go back in the sketch
here, take a look what we have got.
| | 01:55 | Now, very similar to the external thread
sketch, we have got a little 60 degree
| | 01:59 | triangle here, and we have got it
snapped on to the inside of that hole, and we
| | 02:03 | have got this pitch line here,
and this is the pitch divided by 2.
| | 02:07 | And I got to that number just by saying
1/16/2, and if you don't remember where
| | 02:13 | this value came from, but in the
beginning of this chapter we covered how to get
| | 02:17 | those values and how to look those values up
from the Machinery Handbook. I'll click there,
| | 02:22 | and the other piece of information we
need is this pitch diameter, and that's a
| | 02:25 | value we just looked up in the table,
so it's 0.963, just type that in, attach
| | 02:30 | that to the little construction geometry
there, and that's all we really need to
| | 02:34 | create that profile.
| | 02:36 | Click on Exit Sketch, accept
that, and now we need is a helix.
| | 02:39 | I am going to go up here to
Insert > Curve > Helix/Spiral.
| | 02:45 | And the first question it says is,
please select a face or plane to draw a
| | 02:48 | circle, and I am going to pick just
that top face, and I am going to hit the
| | 02:51 | Spacebar to look straight down on it.
| | 02:53 | Now, it doesn't actually tell us this, and
right now there is no other dialog boxes
| | 02:57 | open and it makes it slightly
confusing, but all it's really looking for is
| | 03:00 | a circle and then as soon as we exit
out of the sketch, it's going to jump
| | 03:03 | into the Helix command.
| | 03:04 | I am going to grab the Circle command
here and I am going to snap my circle out
| | 03:09 | and make it so it's attached to this,
and if it didn't automatically add that, I
| | 03:13 | can just go ahead and add a
relationship here, and let's say, Make Coradial.
| | 03:16 | It's the exact same size,
it fully defined as black.
| | 03:20 | And since we are done with that, we
will click on OK, and as soon as we do that
| | 03:23 | it will jump right into the Helix command.
| | 03:25 | So we have got a bunch of
ways we can create helix.
| | 03:28 | First one will be Pitch and Revolution,
we have got Height and Revolution, few
| | 03:31 | different options, I am just
going to use the first one.
| | 03:33 | Now, we are using a Constant Pitch, and
then the pitch here is the same thing.
| | 03:37 | So 1/16 or 16 threads per inch,
that's where you can put that value.
| | 03:41 | And then if our threading was going in
the wrong direction, I could just reverse
| | 03:44 | it, so depending on how you have it drawn out.
| | 03:46 | And then the same thing with
Revolution, if I want to go little bit
| | 03:49 | further, it's fine.
| | 03:50 | As long as we go past the part,
everything will work just fine.
| | 03:52 | And then this is the start angle, and
that's very important, we have got to make
| | 03:55 | sure that we start our
helix right on our sketch.
| | 03:59 | And if I change that value a little bit,
see how that start point is moving around.
| | 04:02 | We want to make sure those both start
exactly at the same location, otherwise
| | 04:06 | you will have errors.
| | 04:07 | Once you have that, click
on OK, there is our helix.
| | 04:10 | So now we have a profile and we have a
path and we are ready to create the Swept Cut.
| | 04:15 | Our profile is going to be Sketch4,
and notice I am selecting from the tree
| | 04:19 | here, I can always get to that tree by
hitting this little plus, open it up
| | 04:22 | and see what's in that tree.
| | 04:24 | So I am going to pick Sketch4 for my
profile, and then for my path I am going
| | 04:27 | to pick just that helix.
| | 04:28 | Soon as I do that, it gives me a nice
preview of what's going to happen, and I
| | 04:31 | click on OK, and there's our threaded cut.
| | 04:35 | You can see it does a pretty nice job,
and you can always turn the Section View
| | 04:39 | off to see the full part.
| | 04:40 | See down there, bend it around, perfect!
| | 04:43 | Whether you are creating a 1 inch thread or
a small thread, a 4/40, something
| | 04:47 | like that, the process is going to be
exactly the same, just the values are
| | 04:50 | going to be slightly different.
| | 04:52 | Threading is used extensively in
product design and development.
| | 04:55 | Having these basic skills is essential.
| | 04:57 | The threads we created
were standard 60 degree threads,
| | 05:00 | however the same technique can be used
to create Acme, Ball Screw, or really any
| | 05:05 | other type of threads.
| | Collapse this transcript |
|
|
16. Equations and Design TablesUsing equations in refining sketching| 00:00 | Equations are awesome and in
SolidWorks 2012 they got even better.
| | 00:05 | Equations allow you to drive an unlimited
number of sketch values from one variable.
| | 00:10 | If we later want to change the size
all we need to do is to update that one
| | 00:13 | value and all the linked values change.
| | 00:16 | Think about a quarter inch hole that was
used across multiple features and sketches.
| | 00:20 | If we wanted to change that hole to a
three eighths of an inch hole all we need
| | 00:23 | to do is edit the equation
and all the holes update.
| | 00:26 | Otherwise, we would need to open
each individual sketch and modify those
| | 00:30 | values independently.
| | 00:31 | In the Graphics view here we have
one quarter of a part that looks very
| | 00:34 | similar to some things we've done in the past,
and I am going to drive this using equations.
| | 00:38 | So I am going to go up here to Smart
Dimension and I typically would have just
| | 00:42 | clicked over here and clicked on maybe
this centerline dimension, and input a
| | 00:45 | double dimension here.
| | 00:46 | And if I do input this, notice I just
type in the number and it's the value I get.
| | 00:51 | It is a little pop up that says,
"Start with = to create an equation."
| | 00:54 | So if I do that, let's try it out, =
now I can link to various different like
| | 00:59 | equations, like sin(), cos(), and
tan(), or I can even link to file
| | 01:03 | properties, like the Mass, the Density,
the Volume, Surface Area, I mean all
| | 01:07 | kind of things you can do here.
| | 01:08 | Or we can just start typing a
variable name out here, so as soon as I start
| | 01:12 | typing something like length, L-E-N-G-T-H.
| | 01:16 | Then I get this little pop-up saying,
it's going to create a global variable.
| | 01:19 | As soon as I click on OK, all right it says
create a new variable, call this and I say Yes.
| | 01:24 | And now it gives me a chance to
input what that value is supposed to be.
| | 01:27 | So I am going to type in 12 and then click OK.
| | 01:30 | So now, not only I have created a
variable called Length, I have also assigned a
| | 01:35 | value of 12 to it and you can tell I
have a little sigma in front of here that looks
| | 01:39 | like kind of like an E, that means
that it's linked to an equation.
| | 01:43 | And the Equation Editor
is in the Toolbars palette.
| | 01:46 | So if I don't have this toolbar opener
here which is the Tool palette, I can
| | 01:49 | right-click here and make sure that
I go down and grab the Tools palette
| | 01:53 | which is right here.
| | 01:54 | I happen to have it already on, so I
am not going to turn it on, but that's
| | 01:57 | where you get the Equation editor.
| | 01:59 | They are also show up over here,
under Equations and then you got values
| | 02:02 | they are linked to.
| | 02:03 | Okay, so let's go on and add some more.
| | 02:06 | Now we can continue to add things in
the input bar or we can go back to the
| | 02:10 | Equation Editor itself and open these values up.
| | 02:12 | Now I've got a bunch of values I can
put in here, so I can say something
| | 02:17 | like Width and then give it a value and
type in 8 and then it equates out to something.
| | 02:24 | You can even give it some notes, type it
over here and we can then just continue
| | 02:28 | on this way and we'll try a Height and
let's give it 2, so we can just start
| | 02:34 | inputting values like this that we are
going to use in our design and we can use
| | 02:38 | things like Hole, and you can
write anything you want here.
| | 02:41 | You can fill this whole space with a
paragraph if you wanted to describe your
| | 02:44 | variable but you probably want to use
something that's short and sweet
| | 02:47 | that's easy to remember and just to
type in, and let's go give it like a .75, and
| | 02:54 | we can continue here to as many
values as we want and then notice down here
| | 02:57 | also we have these equations that are
set up so we are saying D1@Sketch1 is
| | 03:01 | equal to that Length value.
| | 03:03 | So we can add more like that as well.
| | 03:04 | So I click on OK, now we got a bunch
of values that are in there, so now we
| | 03:08 | just got to go link them to it.
| | 03:10 | So click on this sketch dimension and
then click here, across that centerline
| | 03:14 | value and this time if I want to link
that to something, hit the equals again
| | 03:19 | and now I got these global variables,
they are already assigned, I can just go
| | 03:22 | grab one of those, right.
| | 03:23 | I want the width this time and say Width
and click OK, and just inputs that values.
| | 03:26 | Okay, I have got a few more that I can
input here, I can say this value here, we
| | 03:32 | want a dimension on that and I can say
equals again and just go grab that
| | 03:37 | hole size, click on OK, there's that hole.
| | 03:42 | We don't have a value for these lines here
quite yet, so I can just input it on the bars.
| | 03:47 | So I can say, this is going
to be equal to space maybe.
| | 03:51 | Okay and click OK, it's going to create
a new global variable and then we are
| | 03:55 | going to change the value here to 1,
click OK and now that links those values
| | 04:00 | and adds that global variable.
| | 04:02 | Now once we have got all these values
here, everything is equation driven.
| | 04:05 | I don't actually need to ever come
back to this sketch, right, everything here
| | 04:08 | is all linked value.
| | 04:10 | So I am going to go and now create this
feature and extruded it, and I am going
| | 04:14 | to type in like 1 inch, now there is my
Extruded Base/Boss and there is my part.
| | 04:19 | Now, notice I put in a value there.
| | 04:20 | If I want to, I can also double-click
on this and you can see all these values
| | 04:25 | that are input that are there.
| | 04:26 | Now even that one inch value
there, if I want to double-click on that,
| | 04:29 | I can link that as well, I can say = global
variables, and this time I change the Height.
| | 04:33 | So I can link all of those, okay and
click on OK, and hit rebuild and there it is.
| | 04:41 | Now if I want to change this part
around I can go right here to the Equation
| | 04:45 | Editor, here is all the values and I can just
go ahead and change any of these that I want to.
| | 04:50 | I am going to change this one to 8
inches and I am going to this one to 4
| | 04:55 | inches, and I am going to change this
one to 1 inch and let's change those holes
| | 05:00 | to .5 inches and the spacing
we'll leave the same.
| | 05:04 | Click on OK, and you can see that
the part changes automatically.
| | 05:10 | Everything is just updates and if
didn't update you can just hit rebuild
| | 05:13 | to refresh that part.
| | 05:14 | But everything automatically changes quickly.
| | 05:16 | If I go back to that sketch you can see
those values are now input from those equations.
| | 05:21 | It's a really easy way to
go and leverage those values.
| | 05:24 | Now I'm using this as just one sketch,
but I could be creating sketches on all
| | 05:28 | types of different faces and
creating a very complex part.
| | 05:30 | If I was using a half-inch hole for
instance, I could link to that half-inch
| | 05:34 | variable over and over and over again through
multiple sketches through multiple features.
| | 05:37 | If I change one thing, they would all update.
| | 05:39 | So it's a very, very
powerfully way to go about that.
| | 05:41 | When I go back to the Equator Editor
here, I have a few other things I can do.
| | 05:45 | Notice I've got some values that are kind of
linked here and I can display where they are.
| | 05:48 | I can also import and export these values.
| | 05:51 | So if I am using these type of things
over and over again, I can export all
| | 05:55 | these values to an equation in just a text file.
| | 05:58 | So equation.txt, I have a Chapter 16,
I am just going to drop in there,
| | 06:01 | and these are all the values that I
am exporting out of there and I can hit
| | 06:06 | Export and there they go.
| | 06:08 | And then notice down here, I have got a
file that's linking to this external file
| | 06:11 | that's driving these equations.
| | 06:13 | So if I go back into the File System,
inside of that folder, notice I have got
| | 06:17 | this equation.txt file.
| | 06:20 | If I click on it I can see a Preview of
it, I can actually right-click on it, I
| | 06:23 | can say Open with and
something like Notepad would be good.
| | 06:26 | And you can see it's just a simple text
file that says Length is equal to 8, and
| | 06:30 | there are all these other values that
are linking to what they are, so I can
| | 06:33 | continue as long as I keep that same
format, I can start adding values here or I
| | 06:37 | can take this and I import it to
another file that I might be using length, and
| | 06:41 | width, and height and hole diameters
already and then I just can update those
| | 06:44 | values to what they need to be.
| | 06:45 | So that links those values out to the
system and makes it really handy and you
| | 06:49 | can see that value there, import that same
file or a different file, if I wanted to use
| | 06:53 | different equations in my design.
| | 06:55 | Design reusability is a great
timesaver and using equations in your
| | 06:59 | designs makes it easier to make
changes and allows others to easily
| | 07:02 | understand your input values.
| | 07:04 | In SolidWorks 2012 they made it very
easy to create equation values in the input
| | 07:09 | bar, so integrating them into
your design is easy and efficient.
| | Collapse this transcript |
| Working with complex calculations| 00:00 | The Equation Editor gives us the
ability to create equations based on
| | 00:03 | variables and input values.
| | 00:05 | Equations can use the results from
other equations as their input values and
| | 00:09 | some very complicated
dynamic values can be calculated.
| | 00:12 | These values can then easily
be linked to sketch dimensions.
| | 00:16 | In this part here we've got just a simple
layout and we're going to add some dimensions.
| | 00:20 | So I'm going to add dimension from
this right-hand side across the centerline
| | 00:24 | to create a double dimension, and I am
going to create a global variable here, so
| | 00:27 | I am going to say equals, I should
call this one L, and I click OK, and I am
| | 00:32 | going to create a global, say Yes,
and then it gives us the opportunity to
| | 00:35 | type in that value, so I'm going to click on
in that box here and type in 12 and click OK.
| | 00:42 | So now we got a value, global value
called L, which is now equal to 12. Okay,
| | 00:45 | so another dimension over here, this
time I'm going to make another equation,
| | 00:50 | I'm going to say equals.
| | 00:51 | Now what I'm going to do is, I'm going
to grab this value down here and I can
| | 00:53 | add anything into this bar just by
clicking on it, into any value that's
| | 00:57 | available, so click on that, and notice that
it gives the name of that value and where it is.
| | 01:01 | If you mouse over it, it'll tell you the
length of it, which is 12, and then
| | 01:04 | I can do something else to that, so I
can start doing some math functions, so
| | 01:07 | I'm going to divide it by 4, and that's
going to give you what you are inputting
| | 01:10 | there and click OK, and click OK, so
then there is your value of 3, and I'm
| | 01:15 | going to define some of these lines here and
dimension right there, so this is 1 inch right now.
| | 01:21 | So I'm going to take this value here.
| | 01:23 | So I'm going to say equals that value
there, and divide it by 3 to get the 1
| | 01:28 | inch and then make it slightly small,
so I'm going to subtract 0.125. Okay,
| | 01:32 | click OK, and there is that value and
then the last one is going to be this hole
| | 01:36 | here and we can do some interesting
things here to say, I like this value here,
| | 01:40 | and say times, we can use some functions
in there if you wanted to, like the sin
| | 01:43 | of 30, for instance, plus 0.125
maybe, and we can continue on here, make a
| | 01:50 | very complicated equation.
| | 01:51 | And anything else we wanted to add in
here, if we needed to, we can just click on
| | 01:55 | a plus or minus sign, and just go grab
that value, it's going to automatically
| | 01:57 | add that in, so I can say like minus and
click on this value here, it's going to add it in.
| | 02:02 | If all of a sudden that's not what you want,
you can just backspace out of that and
| | 02:06 | remove it out of there, click OK
and that's my value and there it is.
| | 02:10 | So now all these values are linked
together and then if I want to go ahead and
| | 02:15 | if I need to change any of these
things or modify how they operate I can go
| | 02:18 | into the Equation Editor and I can take
a look and see some of the values here,
| | 02:22 | here's the equations that are
linked to this, they're cascading.
| | 02:26 | So if I change L, all these other
values are all cascading down from that.
| | 02:30 | So if I change L which is 12, notice
this is D1, so D1@Sketch1 divided by 4
| | 02:36 | is the second value here.
| | 02:38 | So obviously if L changes, this value
is going to change, and then this value
| | 02:41 | below it is going to change based
on that value, so you can get a quite
| | 02:45 | complicated cascading effect in equations.
| | 02:48 | And you can also just add complicated
equations here, so say like something
| | 02:51 | like G, I can grab values from in
here, so I can say like there or I can
| | 02:56 | type in values that I have already
created list global variables are linked to
| | 02:59 | them, so I already got a global variable
called L I can link to here, or I can
| | 03:02 | just type it out, I can plus another L
if I wanted to, there's my other L and
| | 03:07 | click OK and there it is.
| | 03:09 | So once I've got everything put in
there I can give some comments to what we're
| | 03:12 | doing and you really can create some
pretty amazing equation-driven parts, and
| | 03:17 | let's just go try to change a part here, let's
just make a Extrude, I am going to drag it
| | 03:22 | up 2 inches for instance, and I
got that part equationed out now.
| | 03:29 | So I'm just going to go back to that
equation and this time instead of 12, I'm
| | 03:32 | going to change this to 24, click on
OK and then everything automatically
| | 03:39 | updates, the hole updates, everything
changes in that part if I go back and take a look.
| | 03:42 | Here all the values are, and they have
all been calculated and updated based
| | 03:48 | upon those equations we used.
| | 03:51 | Creating dynamic equation-driven
models in SolidWorks is easy, and it's a
| | 03:55 | great tool to figure out complex shapes that
would otherwise be very difficult to
| | 03:58 | calculate or draw.
| | Collapse this transcript |
| Integrating Microsoft Excel to manage design tables| 00:00 | Within SolidWorks we can use all the
power of Microsoft Excel to drive our parts
| | 00:05 | and to create various
configurations of the same part.
| | 00:08 | To get started we need a base
part that we're going to drive.
| | 00:11 | Let's get started with 16.3-1, this is
just a block with a hole in the center.
| | 00:16 | We are then going to link the values
to drive the size with a design table.
| | 00:20 | Let's take a look at the underlying sketch
here, and take a look at some of the values.
| | 00:25 | Pretty simple sketch here, it's
outlining a few things, and notice if I
| | 00:29 | double-click on any one of
these dimensions, here is the value.
| | 00:32 | So I can actually overwrite
this value or the name of this.
| | 00:35 | So I am going to type in here
just capital W for the width.
| | 00:38 | Over here I am going to double-click
and say, this one is going to be the
| | 00:42 | height, so just H. This one here I
can make it hole, so I can change it to
| | 00:48 | anything I really like.
| | 00:49 | Then over here I am going to change
this one to radius, and there it is.
| | 00:55 | If I double-click back on that, notice
now its Radius@Sketch1, so those are the
| | 00:59 | values we are going to input
into our table to drive this part.
| | 01:02 | Click OK, and those
values have now been updated.
| | 01:05 | And go back to the extrude and then you
can see here the extrude is, I am just
| | 01:11 | extruding it one inch, so
that makes it pretty simple to understand,
| | 01:14 | and it's saying D1, so that's
dimension one in that extrude. Click OK.
| | 01:20 | Now, we haven't really played with many
of these other tabs here at the top of
| | 01:23 | the screen yet, so the first one is
the Feature Manager, the next one is the
| | 01:26 | Property Manager, and then followed
by that is the Configuration Manager.
| | 01:29 | Now, if we have a part and we want to
make some small modification to it, I can
| | 01:33 | always go here and I can right-click and
I can say Add Derived Configuration, or
| | 01:37 | if I click on the top one I can say
create a new configuration, or Add a
| | 01:41 | Configuration to that part, so then I
could go in and maybe change the size of
| | 01:44 | the hole to be a smaller hole.
| | 01:45 | And you have two configurations
of the same exact part.
| | 01:48 | Now, we could do that directly or we
can use Microsoft Excel to drive a table
| | 01:53 | and create the configurations for us.
| | 01:55 | So to do that, let's go up here
to say Insert > Tables > Design Table.
| | 02:00 | The Auto-create is just fine, we are going
to use that as the default, and click on OK.
| | 02:06 | And as soon as I do that, it actually
opens Excel in the background and then it
| | 02:09 | asks us which values we want to
import into Excel to be driven.
| | 02:13 | Now, if we just wanted to change the
length of the extrusion, we could use this
| | 02:17 | one here, which is just that D1 we
looked at, and right now that's one inch,
| | 02:20 | so if we wanted to have a
bunch of different lengths of this piece
| | 02:23 | with a bunch of different
values, we could just drive that.
| | 02:25 | If we want to drive all the
values, we need to select all these.
| | 02:27 | Hold down Ctrl, select
all those and click on OK.
| | 02:30 | What that does, it makes a little
window of Excel inside of SolidWorks.
| | 02:35 | You notice it's the default configuration,
and here's those values that we input before.
| | 02:40 | So if I want to add another configuration,
all I need to do here is just name
| | 02:43 | it, so I'll say like C2 for
configuration 2, and type in some values, so I am
| | 02:48 | going to say, type .5, type in 10, 5,
2, and I will extrude it 2 inches.
| | 02:56 | Those are those values, and I can keep going
if I want to and type in some more values, C3.
| | 03:00 | And if I only want to change one or a
couple of these values instead of having
| | 03:03 | to type them all in, I can use the
Excel command, which is just Fill Down, and
| | 03:07 | select over all those windows, and
hit Ctrl+D for Fill Down, and that just
| | 03:12 | copies those values down, then I can
just change the ones I want to change.
| | 03:15 | So I could say this is maybe 12
inches and I want to extrude it 8.
| | 03:19 | And if I want to I can
name this anything I want.
| | 03:21 | I can add a configuration
named Bob, for instance.
| | 03:23 | It doesn't really matter, you can name
your configurations anything you want.
| | 03:27 | And use that same technique of Fill
Down, so Ctrl+D. And do a couple more
| | 03:33 | things here, we'll change this to
8 and we'll change this one to 12.
| | 03:37 | So if you do add another configuration,
we have got to make sure that we
| | 03:39 | fill in all the values,
otherwise it's going to give us an error.
| | 03:42 | So as soon as we've got all the
values filled out the way we want, we click
| | 03:45 | anywhere in here in the graphics window,
outside of Excel, click there, and it's
| | 03:50 | going to say, it created these configurations
for us. That's great! Click on OK.
| | 03:53 | If I go over here to the Configuration
Manager, you can see these are the new
| | 03:58 | configurations that have been created.
| | 03:59 | So we are still on the default, but
if I want to go and look at my new
| | 04:01 | configurations, I just double-click
on them, double-click on that and, wow,
| | 04:05 | we've got a much bigger part now.
| | 04:07 | You can see how that rapidly
changes that part's shape and size.
| | 04:11 | Double-click on this one, makes a
small part, and bunch of different options
| | 04:16 | here we can take a look at.
| | 04:17 | So it's pretty neat what you can
do with just changing those values.
| | 04:21 | The part really is the same type of
part, just the input values have changed.
| | 04:24 | Now, if I want to go back and edit
the table or change things around, under
| | 04:28 | the Tables tab here, and keep in mind
we are under the Configurations tab, not
| | 04:31 | the Property Manager.
| | 04:32 | Configurations Tab > Tables, and
then here's that Design Table.
| | 04:36 | So if I want to change that table, I
can right-click on it and I can say Edit
| | 04:39 | Table, which will bring
up that same little window.
| | 04:41 | Or I can say Edit the Table in a New
Window, which actually opens up the full
| | 04:45 | version of Excel, click
on that, and there it is.
| | 04:48 | It's going to ask us, these are some
configurations, click on OK, and I am
| | 04:53 | going to jump over here to Excel, open it up,
and expand out these windows so we can see it.
| | 04:58 | And under the View Tab, I just
want to make it a little bit bigger.
| | 05:01 | So you can see the same table is
now open in Excel and we can add more
| | 05:07 | configurations if we wanted to.
| | 05:08 | We can also use the power of Excel
here to figure things out for us.
| | 05:11 | So I can say this row here and I can
Fill Down, Ctrl+D, and I am going to
| | 05:16 | change this one to Gabe.
| | 05:19 | Now, if I want to drive some of these
values dynamically, for instance, if I
| | 05:22 | want to say this value here, maybe this hole,
I want to make it half the size of the width.
| | 05:27 | So I can actually just say equals
and the input bar here is just exactly as
| | 05:32 | Excel would work, and say this value
here divided by 2, and click OK, and
| | 05:36 | that's completely fine.
| | 05:38 | We can use all the power of Excel.
| | 05:40 | In fact, if we skip either a column or a row;
| | 05:42 | we can go out here and
calculate some values out.
| | 05:45 | I could say this cell is equal to that
cell, plus that cell, minus that cell,
| | 05:52 | and divided by this cell, whatever you want to
put in here, and just create some crazy values.
| | 05:57 | So we don't probably want to put a
negative number, but whatever you calculate
| | 06:00 | out, you can go ahead and use any
values you want in Excel to go calculate
| | 06:05 | these values and fill them out, so
you can really come up with some very
| | 06:07 | powerful equations.
| | 06:09 | And we can go up into Excel and use
their Equation Editor and all the lookup
| | 06:12 | tables and values, concatenate, a lot
of real powerful things inside of Excel
| | 06:16 | that we can use to fill out our design table.
| | 06:19 | Once we've got these things looking
good, we can go in and easily create new
| | 06:22 | configurations, but keep in mind, when
we do create configurations, make sure
| | 06:26 | that we are making values that make sense.
| | 06:27 | Like here the width of the part is 10,
the height is 12, and then here's that hole.
| | 06:31 | Well, what happens if I make this hole
like 24, for instance, and I make this
| | 06:35 | thing four inches tall? Let's try it out.
| | 06:38 | Soon as I am done with this, I am
going to click on Save and close that down,
| | 06:43 | and then it says in SolidWorks we've
now got a new configuration, click on
| | 06:47 | OK, jump over here back to SolidWorks, and
there is our new configuration called Gabe.
| | 06:50 | And watch what happened, I made that hole
bigger than the part, double-click on it.
| | 06:56 | Now, we've got a completely different
looking part, even though the values
| | 07:00 | really just changed, it's the same
part with different values, but now this
| | 07:03 | circle is on the outside of this
rectangle, so we've got a completely
| | 07:05 | different looking part.
| | 07:06 | So keep in mind that some of those
values, by changing them you might end up
| | 07:09 | with different parts.
| | 07:10 | And also, if you made, for instance,
like a radius here bigger than this length
| | 07:14 | if this line here or something like
that, that would give you an error saying
| | 07:17 | this configuration couldn't be built.
| | 07:19 | But still we have all the other
configurations still there, just
| | 07:21 | by double-clicking on them.
| | 07:23 | And if we wanted to build an
assembly from one of these, I can drag them
| | 07:27 | directly from this Configuration window
into a new assembly, and each one of the
| | 07:31 | configurations will be
operated as a separate part.
| | 07:33 | Using Excel and design tables allows you
to create a collection of similar parts.
| | 07:38 | This comes in very handy if you're
working with something like a bolt.
| | 07:42 | They look about the same,
| | 07:43 | however, they are different
sizes and different lengths.
| | 07:45 | The features are created the
same with different input values.
| | 07:49 | If you have a design that looks
similar to the bolt example, design tables
| | 07:52 | would be a good choice.
| | Collapse this transcript |
| Making assemblies using part configurations| 00:00 | We can create assemblies
from configurations of a part.
| | 00:04 | We're right here where we left off at 16.3-1,
and we have several configurations of
| | 00:09 | this part that have been defined with a
design table here, and we can go modify
| | 00:13 | those values in the design table and
Excel if we want to, you can double-click
| | 00:17 | on any one of these to get different
input into that shape, and you can rebuild
| | 00:23 | it to get different sizes. Okay,
| | 00:25 | so I can go ahead and
build an assembly using these.
| | 00:28 | So I'm going to say, let's start with
this configuration here, which is Gabe,
| | 00:32 | which is my name, and I'm going to
say, make an assembly from that, so Make
| | 00:36 | Assembly from Part, and notice I
got that one there and then put it in.
| | 00:41 | Now what might seem funny is I'm
going to go ahead and create an assembly
| | 00:44 | of all the same part yet they are going to be
different, so let's click on Tile Horizontally.
| | 00:49 | Notice down here we have those display states,
if I double-click on one my part will change.
| | 00:55 | I can grab it from the Excel
window here or from here and drag it in.
| | 00:59 | Notice, there are the same part, it's
just different configurations of that same
| | 01:03 | part, let's double-click on one of these
other ones, drag it in up here as well.
| | 01:07 | So I can actually take every single
configuration of this part and put it into
| | 01:14 | this assembly, so there is
all bunch of difference ones.
| | 01:17 | All the same part, notice they're
all exactly the same file name and the
| | 01:21 | different values, but they are
different configurations of that part, so notice
| | 01:24 | it's Gabe, Bob, C2, C3, and the
default configuration that are all in there.
| | 01:28 | So there's different configurations
of the same part, and I can create
| | 01:30 | assemblies as I would anyway else,
I can also add other components to this
| | 01:33 | assembly, it doesn't really matter,
so you can actually have a complete
| | 01:36 | assembly using just one part.
| | 01:39 | Makes a lot of sense if you're going to
create like a railing or something like
| | 01:41 | that, you have pieces of rectangular
tubing, they are in different sizes, but
| | 01:45 | really the shape is the same or very similar.
| | 01:47 | So you can have a big tube at the top,
a big tube on the bottom, and then
| | 01:50 | smaller tubes from maybe with the
pickets or the other parts, I can move these
| | 01:54 | components around and adjust them.
| | 01:56 | If I click on a component here this
little in-context window pops up giving
| | 02:00 | a bunch of options.
| | 02:01 | If I go to the very end of this there
is Component Properties, click on that,
| | 02:05 | take a look inside here.
| | 02:06 | It gives me those configurations of
that part and notice the C3 is highlighted.
| | 02:11 | If I were to change this to C2, it
would just change that part, so I can easily
| | 02:16 | change from one part, or one configuration
to the next, inside of this Assembly
| | 02:20 | window just by clicking on a part,
selecting the Component Properties and
| | 02:23 | choosing which configuration I want solved.
| | 02:26 | So right now it's the Bob one, I can
go down here to C3 or Gabe, change that
| | 02:30 | around just by clicking those, hitting
update and it changes that part to something
| | 02:34 | else, so it's very powerful what you can do.
| | 02:36 | So Microsoft Excel inside of
SolidWorks there are these real great powerful
| | 02:39 | features for creating configurations,
and then those configurations again can be
| | 02:44 | used in assembly or in other parts to
create very complex parts, and you can
| | 02:47 | also use all the power of those
equations to solve very complicated and
| | 02:51 | cascading part calculations to
really build some amazing things.
| | Collapse this transcript |
|
|
17. Part DrawingsWorking with drawing templates| 00:00 | A sheet template is the
border and size of a drawing.
| | 00:03 | Making or choosing a template is
important to relay the correct information
| | 00:07 | about your part as well as your company.
| | 00:09 | A sheet template will have a block
tolerance, the projection type, the units,
| | 00:14 | and the scale of the drawing.
| | 00:16 | This is a part we're
going to make a drawing for.
| | 00:17 | I have a couple of different ways to do that.
| | 00:19 | I'll just start a new document here,
I'll click on New, and notice from the
| | 00:23 | Novice tab here, I've get my
standard Part, Assembly, and Drawing.
| | 00:27 | If I click on this drawing here, it's
going to use my default template, or I can
| | 00:30 | click over the Advanced tab to get more
drawings and templates that I might have
| | 00:34 | already established, but I
don't have one of those yet.
| | 00:36 | So let's click on just Drawing
under the Novice tab and click OK.
| | 00:40 | So when I do that, it gives me a
listing of the sizes of standard drawings that
| | 00:43 | are preloaded with SolidWorks.
| | 00:44 | If I click through the different ones here,
you can see the drawing size changes, the
| | 00:48 | width and height change, and I get
a bunch of different options here.
| | 00:52 | I can go through different standards and see
your ISO or a whole bunch of different ones;
| | 00:57 | I can click on here that will change.
| | 01:00 | I'm going to use the ANSI C-size drawing.
| | 01:04 | So that gives us a lot a real estate to
draw out our parts, as well as smaller
| | 01:08 | block down here, so it doesn't take up half
the page like some of the AMB sized drawings.
| | 01:12 | The nice thing about the C-sized
drawing is it's the same ratio as a regular
| | 01:17 | 8.5x11 sheet of paper.
| | 01:19 | So when you print it out, it fits perfectly
on a regular sheet of paper and it looks nice.
| | 01:23 | Now, also down here, this is the
Templates menus and make sure we're seeing that
| | 01:28 | sheet format and click OK.
| | 01:30 | This just opens up a very basic sheet
template, and right off the bat it brings
| | 01:34 | up over here, which file do we
want to incorporate into a drawing.
| | 01:38 | Any documents I have open right
now, which show up right here.
| | 01:41 | So I think they'll be listed here.
| | 01:42 | If I don't have one, I can just click
on Browse to go find the document I want
| | 01:45 | to make a drawing from.
| | 01:47 | Once you have the drawing you like, click
on Next and we get an option for some views.
| | 01:51 | Notice if I bring my mouse over here
into the window, it gives me whatever
| | 01:54 | view I have selected.
| | 01:55 | If I change that view, I can pick
which view I want to start my drawing with.
| | 01:59 | I can also create multiple views if I
wanted to, but this time, I'm just going
| | 02:02 | to pick this top view and just
drop it on the screen. There it is.
| | 02:08 | Again, so I right click, and then as
soon as I've placed the first view, it
| | 02:11 | automatically puts a projection style
on, so I can project out to look at the
| | 02:15 | right hand part of this drawing or
the top view of this drawing or even
| | 02:19 | isometric view if I go to an angle.
| | 02:20 | Notice if I move around that part, all
these different views are available, so I
| | 02:24 | can just keep adding views
until I'm happy with what I got.
| | 02:28 | And as soon as I am done with views,
I just hit Escape and it turns that off.
| | 02:31 | If I have like an isometric view or
something like this, I can drag it around.
| | 02:35 | These views here are linked with that
little line, so I can move them in and
| | 02:38 | out, but I can't them move
them up and down. All right, and
| | 02:40 | same thing over here.
| | 02:41 | I can move it up and down, I can't move it
right or left, and then this view here
| | 02:44 | controls both of those.
| | 02:45 | So they're all kind of linked together.
| | 02:46 | Now, I can start putting dimensions and
annotations on here if I wanted to, but
| | 02:51 | also, let's go and take a look at the block
down here and take a look at what we have.
| | 02:54 | And if you read through some of
this and it says, this is the sole property of
| | 02:58 | insert company name here.
| | 03:00 | So this is really just a starting
point for you to go and create your own
| | 03:03 | customized template that has your
company name, your tolerances you want to use
| | 03:07 | in your parts, and notice these are all
blank right now, the material to finish,
| | 03:11 | all those information is
blank for you to fill out.
| | 03:14 | Now, some of these things you want to
incorporate into your template yourself
| | 03:17 | and some of them you wouldn't. You don't
want to necessarily make the material
| | 03:20 | part of your template unless you're making all
of your parts out of exactly the same material.
| | 03:24 | Same thing with finish and things like that.
| | 03:26 | And things like the drawing number or
the revision, we want to make those so
| | 03:29 | they can link back to the part itself
and gets either the drawing number, the
| | 03:34 | part number or whatever number we want
to show on the drawings here, and we can
| | 03:38 | make these links that go back and it
grabs the part name or the revision.
| | 03:42 | So, before we go ahead and make
changes to the drawing template, let's go and
| | 03:46 | find out where they're
located at and how to access them.
| | 03:49 | So I've created a drawing
template in the Chapter 17 folder.
| | 03:54 | So I'm going to tab over to that
folder here and open this one up.
| | 03:59 | So now you can see over here, I got the C-
drive and under there, I've got a folder
| | 04:02 | called SolidWorks Data.
| | 04:03 | Now, SolidWorks more than likely
installed this folder for you when they
| | 04:07 | installed SolidWorks, and inside of
this folder is your information as far as
| | 04:12 | your toolbox or your browser for the
different styles of Hole Wizard and things like
| | 04:16 | that, and you can also place
things like drawing templates in here.
| | 04:19 | You can make a folder called
drawing templates if you wanted to.
| | 04:21 | You can organize this folder however you want.
| | 04:23 | But it's right on the C-drive, it's easy to
get to, and you can put a lot of data here.
| | 04:27 | So that's where I recommend
putting your sheet templates.
| | 04:30 | Now, over here, I've got a Chapter 17 folder
that came with your exercise files, and
| | 04:35 | I'm going to go and select these four documents.
| | 04:38 | The first one is a drawing template.
| | 04:40 | I've got a picture of the Olive Oil
company logo, I also have a DWG of the same
| | 04:45 | logo and then I have just the sheet format.
| | 04:47 | So you need both a drawing template and
a sheet format, and I'm going to copy
| | 04:51 | those over to that folder there.
| | 04:53 | Now, in SolidWorks, I need to go
and link to where that folder is.
| | 04:58 | So go back to SolidWorks here and
we're going to go back to this drawing, and
| | 05:02 | go up to System Options here, and when I
get to System Options, I go down here a
| | 05:06 | little bit, and I get File Locations.
And in File Locations I've got a bunch of
| | 05:10 | different options as far as where all
these files are located and things like that.
| | 05:13 | But right now, it's already on
Document Templates, and this is where it's
| | 05:17 | looking for those default templates, or
those document templates that we're going
| | 05:20 | to start from and inside of these
places would be part templates, assembly
| | 05:25 | templates or drawing templates.
| | 05:26 | So we want to go, add a new link
to that C:\SolidWorks Data folder.
| | 05:29 | So, I'm just clicking on Add and I'm
going to go in here to the Computer > C drive
| | 05:36 | and scroll down to SolidWorks
Data and that's what I want.
| | 05:39 | So Click OK, it just adds a C:\
SolidWorks Data, and that should be good to go.
| | 05:45 | And then also just before we get out of
this, I want to point out that up here
| | 05:48 | under Default Templates, it also lists
which template is going to be used when
| | 05:52 | you just click on that Novice tab
as far as part, assembly, or drawing.
| | 05:56 | These are the templates that are
going to be automatically pulled in.
| | 05:58 | So I can go change those paths to
whatever my latest and greatest newest
| | 06:02 | template is for each one of those.
| | 06:04 | And I can and save out a new
template anytime I want.
| | 06:06 | Save it to your favorite location like
C:\SolidWorks Data, and then change this
| | 06:11 | path to it so you can just grab that
every time you start a new file, you don't
| | 06:13 | have to go and change it each time.
| | 06:15 | So once I'm happy with that, I'm going
to add the C:\SolidWorks Data to my path,
| | 06:19 | click on OK, and there it is.
| | 06:21 | So, let's go ahead and try
a new drawing out this time.
| | 06:24 | But I'm going to go back
and actually go to the part.
| | 06:25 | So here's the part, and before we
actually do this part here, I'm going to back
| | 06:31 | to this drawing here and just
cancel that one so it doesn't interfere.
| | 06:35 | So don't save that one.
| | 06:36 | Now from this part here, I'm going to
go up to File > Make Drawing from Part.
| | 06:41 | That pulls a lot of that data and it
already knows which part we're using and
| | 06:44 | everything else like that.
| | 06:45 | Click on Make Drawing from Part, and as
soon as I pull this up, it gives me this
| | 06:48 | option here of the different sheet
formats as well that I could import in.
| | 06:53 | Or if I hit Escape out of this and cancel
that, I can go to the New tab here and
| | 06:58 | under the Advanced tab, I've
got this new template I just made.
| | 07:02 | So if click on that one,
| | 07:04 | notice I get that new template I
made, and this is a quite a bit nicer
| | 07:07 | template than the original default and I've
customized it to this company that we're using.
| | 07:12 | So you can see on the left-hand side here,
we got the Model View that has a file
| | 07:16 | we have opened, and I click OK, and the
same questions I can just place that
| | 07:20 | directly on my drawing and now I have
what I need to do and I can place a couple
| | 07:24 | of other views here real quickly and
then I can go, click Escape, and then I can
| | 07:29 | move those around to make them,
so they look nice in the drawing.
| | 07:32 | Now, I've got this sheet format that's
pretty established as far as I've got a
| | 07:36 | picture in here, I've got some company
information, and I've got some tolerance
| | 07:41 | information placed in here as well. A
lot of information that might be good to
| | 07:45 | relay to the customer.
| | 07:46 | I also have a revision block
that I've pre-added in here.
| | 07:49 | Down here, I've got a time and date stamp,
which you may or may not want, and outside
| | 07:54 | of the drawing, I've actually
placed the path to where that file is.
| | 07:58 | It doesn't actually print on the
drawing because it's directly outside of the
| | 08:01 | border of it, but what happens is
sometimes you're looking for where this file
| | 08:04 | is, and it gives you a nice little
link to where to go find these files and
| | 08:08 | that's the file location of where this
part itself is, and it's going to change
| | 08:12 | depending on, obviously, where
you have stored on the file system.
| | 08:15 | So if we want to go and make some
changes now to the template itself, I can go
| | 08:19 | here and I can right-click and say
Edit Sheet Format, and we're going to be
| | 08:25 | right-clicking anywhere that is
not a part, so Edit Sheet Format.
| | 08:28 | As soon as I do that, now I
get blue lines on my drawing.
| | 08:31 | So these are standard sketch lines,
so I can add circles and squares and
| | 08:36 | rectangles and lines as much
as I want to change this around.
| | 08:38 | I can click on lines and move them up and down.
| | 08:42 | I can adjust things if I wanted to.
| | 08:44 | I can click into a text box like this, double-click
it and I have the ability to type or
| | 08:50 | change the font or change the size, change
the formatting how I want to align these things.
| | 08:55 | So each one of these is just a text
box that has some information in it and a
| | 08:59 | font and a size, and same thing down
here, I can just keep going round and
| | 09:03 | round changing things as we want;
| | 09:04 | a bunch of different ways
we can go ahead and do that.
| | 09:08 | You might want to incorporate
a picture into your template.
| | 09:11 | The best way to do it is go under the Sketch tab
and I've got this Sketch Picture, and by
| | 09:16 | default Sketch Picture doesn't show up
in SolidWorks and we did add this in an
| | 09:19 | earlier movie, but I'm going to go
ahead and show you how to do that again.
| | 09:21 | Customize CommandManager, and go up here to
Commands, and we're going to go down to the
| | 09:27 | Sketch toolbar, and then here's all the
available Sketch tools that we can put
| | 09:32 | into this folder over here.
| | 09:33 | So if I wanted to add a sketch to it, I'd
just click on Sketch, drag and drop it in here.
| | 09:37 | But I already have one so I
don't really need to that.
| | 09:39 | And the same thing with any
other tools you ever wanted to add.
| | 09:41 | You can always drag and drop them in. If
you don't want in there or you just drag
| | 09:44 | it back out and put it back in
the palette here. Click on OK.
| | 09:47 | So, once I have that, I can click on
it and it's going to ask me to go look
| | 09:50 | for a file. And here's the file that I put in
there, which is that logo and we'll click on OK.
| | 09:54 | As soon as I do that, it's
going to place it in the drawing.
| | 09:58 | It's kind of big so I've got
to zoom out to go see it.
| | 10:00 | So right now it says Transparency none,
I want to actually say, From file which
| | 10:03 | then says it's a clear background.
| | 10:06 | And I can define the size of that file so I
can just drag it up and down, and I can
| | 10:10 | move it anywhere I want.
| | 10:11 | Once I'm happy with where it is, I'll
click on OK and it just places that file.
| | 10:15 | So, I'll say, I've moved it down here.
| | 10:17 | That's how you'll place an
image in your sheet format.
| | 10:19 | Any other changes you want to make here as well.
| | 10:22 | We can go ahead and add notes as well
just by using the annotations and we're
| | 10:26 | going to be covering
that in the next few movies.
| | 10:29 | Once you have all these changes made,
go back out of the sheet format and then
| | 10:33 | we might want to make these updates. And notice
this is obviously going over the top of my part.
| | 10:36 | So this probably -- we don't want to place that
| | 10:38 | there, we'd probably have it down here.
| | 10:39 | I just want to give you an illustration of how
we can easily place an image in the drawing.
| | 10:43 | But once we have one that we
really like, we can go up here and say
| | 10:46 | File > Save Sheet Format, and we already
have one called TWOTREES, and I don't
| | 10:52 | want to replace it right now, but if
you did, this is what you'd call it, or you can
| | 10:55 | also name it something else as
SheetFormat2 or TWOTREES2 would be another sheet
| | 11:01 | format, so you can actually choose one
or the other depending on what type of
| | 11:04 | drawing you're making, and a lot of
times, you'd make one that would be like a
| | 11:07 | metric one and one would be an
English unit one, so we could have the block
| | 11:11 | tolerances changed depending on what
type of part you're making and other
| | 11:14 | standard sheet format templates, or art
templates, or drawing templates we'd use
| | 11:18 | would be something like changing the units.
| | 11:20 | So, if you're making drawings in
metric, you'd have a metric template and it
| | 11:24 | have one in English units as well,
and then the block tolerance would
| | 11:28 | automatically match that same thing.
| | 11:29 | So you can have as many templates
as you want to define your drawings.
| | 11:33 | I've already got that saved,
| | 11:35 | so I'm going to say Cancel and there it is.
| | 11:37 | SolidWorks has some built-in
templates that can be easily customized.
| | 11:41 | Spending a few minutes and setting
up your default templates will put a
| | 11:45 | professional polish on your drawings
and make sure you're relaying the correct
| | 11:48 | information about your parts.
| | Collapse this transcript |
| Setting up drawing options and sheet properties| 00:00 | There are many different standards and
drawing options that can be modified.
| | 00:04 | Once these options have been set, we
can save the drawing templates so these
| | 00:07 | options will be the defaults.
| | 00:09 | To get started, let's open
17.2-1 and make a drawing.
| | 00:13 | I am going to go under the File menu and
since I already have a part open, I can
| | 00:16 | use this Make Drawing from Part.
| | 00:18 | And notice I get the template that we
just created in the last movie, and also
| | 00:22 | you see the tabs here at the top or just
the other templates that are available.
| | 00:25 | So I am going to pick that TT template
for the Olive Oil Company and click on OK,
| | 00:30 | and that's going to open that
template in the background here.
| | 00:32 | It also brings up this pretty
handy little window on this side.
| | 00:34 | It gives me some views
that I can just drag and drop in.
| | 00:37 | So I am going to grab that Top
view and just bring it right in.
| | 00:40 | Okay, there's our view, and then
automatically as soon as I create that view, it
| | 00:44 | turns on the projection views, and
I can just go ahead and make cool
| | 00:47 | projections of that same part.
| | 00:48 | When I am done, hit Escape, turns that
off and I can just move some of these
| | 00:52 | around to lay them out on my
sheet a little better, they look nice.
| | 00:55 | Let's go ahead and add a few dimensions
now, just so when we do change some of
| | 00:59 | the options, we can see how those
dimensions are going to change when we make
| | 01:04 | those option changes. I am going
throw one up here, and then one over here.
| | 01:11 | Okay, so there's a few different
views here and maybe I will do one on the
| | 01:15 | thickness of the block over here.
| | 01:17 | Okay, let's go up now and change some options.
| | 01:20 | So under the Options tab here, click on
that and under Documents Properties, we
| | 01:25 | have got all these different choices here.
| | 01:27 | The very first one is the Drafting
Standard, and we looked at that before and
| | 01:31 | right now we are on ISO-MODIFIED
environment, we can change to ANSI or anything else.
| | 01:35 | If I change this, it's going to
change all the styles and fonts and methods
| | 01:40 | for laying things out.
| | 01:41 | So if I change to ISO for instance, go
back here, and I click on OK, notice all
| | 01:46 | these views changed, all the annotations,
now they are aligned with the leader
| | 01:51 | in a vertical orientation
here instead of horizontal.
| | 01:53 | And this way doesn't look quite as nice
in my opinion, but you can modify this
| | 01:58 | to however you want to have your
drawings look, and same thing if probably
| | 02:01 | the fonts a little bit small.
| | 02:02 | So I might want to go back and modify some
of the stuff to go and change that around.
| | 02:05 | So go back to Options, go back to
Document Properties and I am going to change
| | 02:10 | this one back to ANSI, and then
let's go through some of these options.
| | 02:14 | So first one there is a little plus
mark, I can click on the Annotations.
| | 02:18 | So any kind of notes we are going to be
placing in our drawing is going to be defined here.
| | 02:22 | The font, the size, the style and
everything else is defined here.
| | 02:27 | So right now we are using 12 point, I'd
maybe change that to Points 18,
| | 02:32 | click OK, and now notice it says, I have
deviated from this standard, that ANSI
| | 02:38 | standard, now we are in ANSI-MODIFIED standard.
| | 02:41 | Okay, that's fine with me.
| | 02:44 | And we have got a couple
of different type of arrows.
| | 02:46 | We can do a lot of things here.
| | 02:48 | Then we jump down to Balloons. When we
start making assemblies how do we want
| | 02:51 | our balloons to look?
| | 02:52 | Same thing with Datums, we can
change everything, the Leader style, the font
| | 02:56 | width, the line width, I
mean a lot of stuff here.
| | 02:59 | Geometric Tolerancing, same thing, go
into Notes, we can change the font again,
| | 03:04 | the style, the Services Finishes, Weld Symbols.
| | 03:07 | We go down to Dimension, we got another
plus mark, we can click on here, we
| | 03:11 | can change the Font directly for those
as well, so maybe I will makes these 22.
| | 03:17 | You can make whatever fits your drawing
best, and then a lot of different things
| | 03:20 | for Dual dimensioning, your
Primary precisions, your Dual precisions,
| | 03:24 | Fractionals, if you are going to be
using those, how do you want your arrows to
| | 03:27 | look, you know if you want like
a bigger arrow or a longer arrow.
| | 03:29 | I can adjust all the size of the arrows
and change them to my preference, and
| | 03:34 | different zeros, we have standards.
| | 03:35 | So then come down to our Angles.
| | 03:37 | How do we want our Angles to show up?
| | 03:39 | How do we want the Text position? Do we want to
kind of be on the circle there, aligned
| | 03:43 | horizontally, a bunch of choices.
| | 03:45 | Arc Length same thing, Text positions, big
one, how do we want the font to be laid out?
| | 03:51 | Chamfer, so we can really control
almost everything about how our drawing is
| | 03:55 | going to look by going through some
of these different options here. With
| | 03:59 | something like the Diameter or Radiuses,
we can establish here, how do we want
| | 04:03 | the Text position to be?
| | 04:05 | Same thing with Hole Callouts. We've got
Linear dimensions, how do I want them to look?
| | 04:09 | And these are the ones that I change a lot.
| | 04:11 | This is my favorite one here in the
middle, it's just horizontal text, that way
| | 04:14 | you have to turn your head sideways to
go and read all the different values.
| | 04:17 | Ordinate values here, Radius,
Centerlines, how do we want these marks to look?
| | 04:22 | If I go down here to a couple of
Tables, View Labels, Virtual Sharps.
| | 04:29 | Virtual Sharps is something like if
you have two lines intersecting, how do
| | 04:32 | you want that to look?
| | 04:34 | So they do that a lot in sheet metal
when you have a bend and you want to have
| | 04:37 | a Virtual Sharp showing where
those two edges might come together.
| | 04:40 | As far as Detailing, this
is a pretty handy one here.
| | 04:43 | So first of all we are showing what do
we want to show by default, and then over
| | 04:47 | here we have this auto
insert which is really nice.
| | 04:50 | So by default, it can automatically add
center marks for holes and that can save
| | 04:55 | you a lot of time if you are using that.
Same thing with automatic centerlines,
| | 04:58 | or automatic balloons if
you are working with assemblies.
| | 05:02 | Dimensions marked for the drawings, so
a lot of things that we can just
| | 05:05 | bring in automatically.
| | 05:06 | And then yes, sometimes you might want
to have different templates for different
| | 05:09 | types of options, so for instance, if you
are working with sheet metal and you have a
| | 05:12 | grid pattern with a lot of holes in it,
bringing in center marks may not be the
| | 05:15 | best choice because sometimes they can
make your drawing look very cluttered and
| | 05:18 | then you have maybe a few
hundred center marks to go get rid of.
| | 05:21 | So depending on which type of part you
are working with, you might or might not
| | 05:25 | want these things turned on.
| | 05:27 | You can have a Grid to lay things out if
you want, you can set the spacing here.
| | 05:30 | Units is probably going to be
the one we're going to use the most.
| | 05:32 | We are going to go and say what
unit system do we want to use?
| | 05:36 | The most common will be millimeter or
inch, pound, second, and then what are our
| | 05:40 | decimals points that we want?
| | 05:41 | Do we want a two point, a three
point, a four point, and so on.
| | 05:44 | So we can define all those right
there and then same thing if we have dual
| | 05:47 | dimension, if we have different angles
things like that, we can change these
| | 05:51 | around, so you know two or three place
decimals will probably be the most common
| | 05:55 | ones you are going to see.
| | 05:57 | And we'll go down a little further here,
you've got different types of
| | 06:00 | lines you have in your drawings, we
can go through those, the different
| | 06:03 | styles, we can have Dashed lines, we
can have a bunch of different things we
| | 06:06 | can establish here and we can actually load
new ones if we wanted to or save custom ones.
| | 06:10 | Same thing with Line Thicknesses, these
are our standards, and Image Quality, this is
| | 06:14 | another one that's important.
| | 06:15 | If you have a big drawing and it looks
kind of more like an octagon than a
| | 06:20 | circle, at that point of time, so if
we have a low resolution, and it starts
| | 06:23 | turning into more like a multi-sided
shape versus actually like a circle.
| | 06:27 | But the higher you go here, also the
more system resources you are using.
| | 06:30 | So you want it somewhere in the mid
range here would probably be fine unless you
| | 06:34 | really want to show something very
accurately and you have a little more time to
| | 06:37 | wait, you can do that, and same thing
you got a little slider you can do for
| | 06:41 | Wireframe as well. And then the very
last one here, Sheet Metal, and if you are
| | 06:45 | making drawings for that which we haven't
really covered sheet metal yet, but it allows
| | 06:47 | you to insert bend line
information and things of that nature.
| | 06:51 | So anyways, those are all the system options.
| | 06:53 | You can see there is quite a bit of
stuff that you can go ahead and change to
| | 06:56 | modify your drawing.
| | 06:57 | So once you have gone through here and
made a bunch of modifications and got
| | 07:01 | your drawing so it's really looking
good, you want to go, get back to your
| | 07:04 | drawing and make sure then once we have
made all those changes, go back here and
| | 07:09 | make sure you go to File > Save Sheet Format.
| | 07:12 | And save that sheet format or overwrite
your existing format, that way the next
| | 07:16 | time you open that drawing, it's going
to be using that new sheet format and
| | 07:20 | same thing with property.
| | 07:21 | So that's the sheet format which is
going to be the location of all the
| | 07:24 | note changes, and then the other one
we need to make sure we change is the
| | 07:28 | part template, and most of those system
options are actually located in the part template.
| | 07:32 | So there is two files, there is a sheet
format and there is also the part template.
| | 07:37 | So we need to save both of those
and just go save that part template.
| | 07:40 | We go to File > Save As, and as far as
the Drawing, we need to go down here to
| | 07:47 | Drawing Templates and you can see we
have a template here and we can go up to
| | 07:52 | the C folder, go down to SolidWorks
Data and there is that TT.Drawing template,
| | 07:58 | that's where all that data stored in.
| | 08:00 | So if I overwrote that file
that would save that file out.
| | 08:03 | But keep in mind, we don't want to have
any views like this in our drawing when
| | 08:08 | we save that drawing template out
because then those views will automatically
| | 08:11 | show up the next time we make a drawing.
| | 08:13 | So when we do work with a drawing template
and go out and save those options out, we
| | 08:17 | want to go back and just open up a
blank drawing and make the changes to the
| | 08:21 | template, make the changes to the
sheet format, save those out and that way
| | 08:24 | when we open it again, everything is
looking perfect, and we can just get
| | 08:28 | straight to drawing.
| | 08:29 | Saving your options as the defaults
in a drawing is the single best time
| | 08:33 | saver in SolidWorks.
| | 08:34 | More than half of the new users that I
encounter don't know this and don't make
| | 08:38 | these changes and have to go back and
modify their sheet format or drawing
| | 08:41 | options every single time
they are making a drawing.
| | 08:43 | This could be very time-
consuming and it's really not necessary.
| | 08:47 | Save that sheet format, make those
options changes and you will be on your way
| | 08:50 | to being a better designer.
| | Collapse this transcript |
| Choosing the correct projection angle: first angle vs. third angle| 00:00 | In this movie we're going to cover the
differences between a first angle and a
| | 00:04 | third angle projection.
| | 00:05 | In the United States, the most
common projection is called third angle.
| | 00:09 | In Europe, and most of the rest of
the world, first angle is the norm.
| | 00:12 | To change from one to the other
it's really just an option click away.
| | 00:15 | However it's important to understand
what the differences are, and how the
| | 00:19 | projections look different.
| | 00:21 | This part here is the same part we've
been working with, but I've added a little
| | 00:24 | polygon on the side and a triangle, so
we can see which side we're working with.
| | 00:29 | I'm going to go make a drawing from this,
| | 00:30 | I can say Make Drawing from Part, and
use that same template we've been using.
| | 00:34 | Click on OK and it pops up over here
and I'm going to click on that top view to
| | 00:38 | bring it out, and I am going to make a
projection on the right and one on the left,
| | 00:42 | one at the top and one on the bottom of this.
| | 00:44 | So as you can see we've got the front
view here and then on this right hand
| | 00:49 | view I've got the little polygon here, the
hexagon, and on the top I've get the triangle.
| | 00:53 | Now if I want to change
different styles of projections, I can
| | 00:56 | right-click anywhere in the
Drawing view, so if I right-click here and then
| | 01:00 | come down to Properties.
| | 01:01 | Inside of Properties I get
a bunch of information here,
| | 01:04 | the name of that sheet, the scale of
that sheet that I'm using, here's the sheet
| | 01:08 | format that I'm using for that, and then
up here is the projection style, first
| | 01:12 | angle or third angle.
| | 01:13 | So right now I'm using a third angle
projection because we set this drawing sheet up.
| | 01:16 | Now if I change over to first angle
and click OK watch what happens to that
| | 01:20 | drawing, I'm just going to move
it over here, so that you can see.
| | 01:22 | Click OK and now the hexagon here
moved to the other side and the triangle
| | 01:27 | moved down to the bottom.
| | 01:28 | Now did the part change?
| | 01:30 | No, the part is exactly the same part as it
was before, but the projection style changes.
| | 01:35 | So, keep in mind if you change from
one to the other, your parts are going to
| | 01:38 | look completely different.
| | 01:39 | So if somebody is expecting a part to
have the right view on the right side of
| | 01:44 | your part and it's actually on the
left, you might get the wrong part
| | 01:47 | manufactured when you send your drawings out.
| | 01:50 | So make sure that if you in the U.S.
you're using third angle projections.
| | 01:53 | If you're using first angle projections,
hopefully you're in Europe or Japan or
| | 01:57 | somewhere like that whose using
that as their kind of standard type.
| | 02:00 | And a lot of times in your block down
here, you'll write in first angle or
| | 02:05 | third angle projection.
| | 02:06 | So it's very clear to whoever is making
a part or working with your drawing, the
| | 02:10 | style of projection that you're using.
| | 02:12 | It can be a big stumbling point especially,
when you are first setting up your template.
| | 02:16 | If you overlook that, you're drawings
might look quite a bit different from the
| | 02:19 | parts you're going to be getting, if
they're expecting a third angle and you're
| | 02:22 | producing a first angle drawing.
| | 02:24 | Even though it might not seem that
important, one of the most common errors on
| | 02:27 | new SolidWorks drawings is using the
wrong projection type and confusing vendors.
| | 02:32 | It's a quick thing to check and it
makes sure that you're getting the right
| | 02:35 | projections and the right parts.
| | Collapse this transcript |
| Adding model views to a drawing| 00:00 | In this movie, we're going to learn to
add different sheets to our drawings as
| | 00:03 | well as adding additional
sheets to continue on our drawings.
| | 00:06 | This is the same part we've been
working with and I am going to click on
| | 00:09 | File > Make Drawing from Part,
| | 00:11 | and use that basic template
we've been working with, and I am just
| | 00:14 | going to add that top view here.
| | 00:16 | Okay, there's our top view and we
can add a couple of projections if we want.
| | 00:19 | We've got some options when we do add these.
| | 00:21 | So if I click on any one of these, I
can actually change those options and
| | 00:25 | notice, it's the view that I am using here,
which I can always change if I wanted to.
| | 00:28 | Go down here, I can see
how I want to display that.
| | 00:32 | You can do Wireframe, you can do it with
the hidden lines removed, and notice if I
| | 00:36 | click on one of these
things, all those views change.
| | 00:39 | Now you can do them individually, but I
am changing the base view so these other
| | 00:42 | views are automatically updating as well.
| | 00:44 | I can change it to a Standard one here,
I can do the Shaded Mode with edges, I
| | 00:47 | can do it with without edges.
| | 00:49 | Now sometimes these type
of views look really nice.
| | 00:51 | I mean, you can see a view and you can
do some projections of it and it looks
| | 00:55 | all shaded and nice, like
you used to in SolidWorks.
| | 00:57 | I am going to caution you
against these a little bit.
| | 01:00 | When you work with views like this, a
lot of times drawings are around for a
| | 01:03 | long time and they're photocopied,
they're faxed, there's a lot of things that
| | 01:07 | happen with drawings.
| | 01:08 | And a view like this just turns into a
big black blob here in the upper corner
| | 01:12 | when you start copying that file.
| | 01:14 | So I would caution you against
trying to use those types of views.
| | 01:17 | The Hidden Lines Removed is probably
the best, best bet for that or
| | 01:20 | showing where those files are
as hidden lines are visible.
| | 01:22 | So either one of those will
work just great for your views.
| | 01:25 | We also have the sheet scale
or the scale of the drawing.
| | 01:29 | So notice this part here.
| | 01:30 | Sometimes you're working on a drawing and
running out of space, you can take that
| | 01:33 | isometric projection and you
can make it smaller. All right,
| | 01:35 | so you use a custom scale
and scale that down smaller.
| | 01:38 | And if I do, I probably want to
put a little annotation down here that's
| | 01:41 | noting what the scale is because I
have a scale down here in the drawing
| | 01:44 | telling me what size it is.
| | 01:45 | So if I am making something that's a
different scale, make sure we're noting that.
| | 01:49 | And then once you're happy with what
you've got there, you can click OK and
| | 01:52 | there's your different views.
| | 01:54 | Now if we're working with maybe an
outside vendor and you want to have a part
| | 01:57 | like this, maybe if it's laser cut
first, and then maybe some secondary
| | 02:01 | machining or something done on it, you might
want to send a file to them for laser cutting.
| | 02:04 | So I am going to show you how you create
another view for that, so I can add a sheet.
| | 02:07 | If I add another sheet here, I can just
add more views if I needed to, and you
| | 02:11 | need to have a model in your view.
| | 02:12 | So to do that, I am also just going to
go, select that same model that we were
| | 02:16 | using before and throw it out here.
| | 02:19 | Now we already have that view but if we
want some other different views, we can
| | 02:22 | throw this in here as well,
something like an auxiliary view.
| | 02:24 | So if I had maybe a cut at a certain
angle or a hole at some funny angle and I
| | 02:28 | needed a view to look at, you
would ask me for an auxiliary view.
| | 02:31 | I need to go pick an edge.
| | 02:32 | So there's no specialty edges on this part here,
| | 02:35 | it's just a rectangular part with a hole in it.
| | 02:37 | So I don't really have an edge to
pick from this, but I just want to show
| | 02:39 | you that's available.
| | 02:41 | Same thing with up here; Standard Views.
| | 02:42 | Those with 3 Standard
Views it would automatically add.
| | 02:45 | The Model View is just going to
tell me it's going to add a part.
| | 02:47 | Projected Views, we've already done,
we'll just pick the base view and then it's
| | 02:50 | going to give you those projections.
| | 02:51 | Okay, the Section Views, if you want
to slice this in half, I can slice it
| | 02:56 | wherever I want to place it
and then place that new view.
| | 02:58 | It's going to give you a section view of
that and those are aligned together as well.
| | 03:01 | So it shows you what it's going to look like.
| | 03:03 | A Detail View, it's going to allow me
to zoom in on a certain section and make
| | 03:08 | it bigger so I can detail
that a little bit easier.
| | 03:10 | I'll break out a section if I want to
slice halfway through something to go get
| | 03:14 | a little more detail, as far as
what's inside of a part, I can use that.
| | 03:18 | If I have a long part, I can break it and pull
together so it's a lot smaller on the drawing.
| | 03:23 | I can crop a view so I am closely
at it and then I can also use this
| | 03:26 | Alternate Position View.
| | 03:27 | So if you have something like a pair
of pliers, you can show it in the closed
| | 03:30 | position as well as the open position.
| | 03:32 | So a lot of things you can
add as far as the drawings.
| | 03:34 | Okay, now what we're going to do is go
ahead and add another sheet and we're
| | 03:38 | going to place a Model View on there
so we can go ahead and use that to send
| | 03:42 | to maybe a laser cutting company or a water
jet company who could cut these parts out for us.
| | 03:47 | So I am going to click on New Sheet and
notice I get that sheet here, and we'll click
| | 03:50 | on the Model View and I am going to
grab just that top view. And there it is.
| | 03:54 | So that's exactly what I want to cut.
| | 03:56 | However, I don't want to have the rest
of this border and everything on there.
| | 03:59 | I want to go and get rid of that.
| | 04:01 | So I am going to right-click here and
say Properties, and I am just going to say
| | 04:04 | Display sheet format and just turn that off.
| | 04:06 | Now notice this little image
you have on your sheet format.
| | 04:09 | It might not have disappeared.
| | 04:11 | Sometimes that's an issue in SolidWorks
that it's not disappearing when you
| | 04:14 | are hiding the sheet format.
| | 04:14 | So to get rid of that, let's just say
Edit Sheet Format, click on it and, hit
| | 04:18 | Delete and it takes it
out. Go back. All right,
| | 04:21 | so now we have pretty much
exactly what we want.
| | 04:23 | We've got the shape that we want, just
purely the lines, nothing else on the
| | 04:26 | sheet format and we can go save this out.
| | 04:28 | But before we do that, let's double-
check that we're using the sheet scale.
| | 04:31 | So make sure we've got sheet scale
selected and then go back to Properties by
| | 04:34 | right-clicking anywhere, select
Properties, and make sure up here we've got a
| | 04:37 | 1:1 scale, and third angle
projection or first angle.
| | 04:40 | It doesn't actually matter here
because we're just looking at the top view.
| | 04:43 | But make sure that's scaled to 1:1, otherwise
you are going to get a part that's either 2
| | 04:46 | times too big, or too
small or something like that.
| | 04:48 | So make sure you're 1:1, and then when
you go to save this out, we're going to
| | 04:51 | go to File > Save As, and I am
going to select either DWG or DXF.
| | 04:56 | If I do that, I get a couple of options here.
| | 04:58 | Just click on that and inside the
Options window here, you've got a bunch of
| | 05:01 | different versions you can save it out to.
| | 05:04 | I find sometimes saving out to these
older versions, like R13, sometimes works
| | 05:08 | better especially with legacy systems.
| | 05:10 | And then also export the active sheet only.
| | 05:13 | Otherwise it's going to export all
of the sheets of your drawing to that.
| | 05:16 | And once you've got all these selected
out, click on OK, and now I can say Save,
| | 05:21 | and I already have one there, I
am just going to overwrite it,
| | 05:23 | replace that file, and now I have
that version I can go ahead and send out to
| | 05:28 | any type of manufacturing.
| | 05:29 | So machine shops, laser cutting,
water jet cutting, all of those types of
| | 05:33 | companies can use this type
of a 2D file to cut things out.
| | 05:37 | Also, I just want to point out while
we're in here, if we go back to that part
| | 05:41 | itself, if you wanted to send this as
a solid file out to somebody, you could
| | 05:45 | send the native SolidWorks files, but
a lot of times they're looking for maybe like a
| | 05:48 | STEP file or an IGES file.
| | 05:49 | We can do the same thing there, we can
go File > Save As, and click OK, and then go
| | 05:54 | down here, we've got a bunch of
options on how we can export that data.
| | 05:57 | Parasolid is a really popular one, IGES
files, STEP files, but you can see
| | 06:02 | there's just a ton of things you can work
with other types of software to export files.
| | 06:06 | So I'd probably recommend STEP files,
as it's kind of the most common file
| | 06:08 | format you'd probably use.
| | 06:09 | And then same thing, you've got
some options you can change there.
| | 06:12 | I just want to point
out that that was available.
| | 06:14 | Let's go back here, here's our drawing, so
we've got couple a different sheets that we're
| | 06:17 | drawing, see how it lays out.
| | 06:19 | SolidWorks makes it easy to add views to
your drawings by selecting the starting
| | 06:22 | view and the various projections.
| | 06:24 | You can see we can do quite a bit with
the different projection views and the
| | 06:27 | different sheet formats.
| | 06:28 | We can export files and work with a
lot of different softwares and vendors.
| | 06:32 | From here, we're going to move into the
next movies where we're going to learn
| | 06:34 | about adding dimensions and annotations.
| | Collapse this transcript |
|
|
18. Adding Dimension Notations to a DrawingCreating general dimension notations| 00:00 | In SolidWorks, all the sizes and
features are defined in the model.
| | 00:04 | Therefore, to add dimensions, we just
need to define what values we want to show.
| | 00:10 | SolidWorks can also do a lot of this
for us, using the Auto Dimension command.
| | 00:14 | The tools are straightforward.
| | 00:15 | However, what's not straightforward is,
understanding how to correctly place
| | 00:19 | dimensions and tolerances.
| | 00:20 | There is a lot that goes into
this and we will cover the basics.
| | 00:24 | Over here in SolidWorks, we have a part
defined here and we have one view of it,
| | 00:28 | and this is part of the Olive Oil
Company's manufacturing process, it goes into
| | 00:32 | their machines, and we're going to go
and add some dimensions to this now. Okay,
| | 00:37 | to get to the Dimension Toolbar, we
have a Smart Dimension up here, at the
| | 00:40 | top, and most of the dimensioning we're going to
be doing is going to be based in this one tool.
| | 00:45 | First, let's click right on that tool,
and we're going to just do some basic
| | 00:49 | Dimension Expert dimensioning, and by
default, we're in just a basic baseline
| | 00:54 | type dimensioning tool.
| | 00:56 | So if I want to dimension the overall
part here, I'll click from this edge here
| | 01:00 | to this edge here, and then place the dimension.
| | 01:03 | So I'll do that right now.
| | 01:04 | I'll click here, and notice that if I
click there, it actually gives you the
| | 01:07 | dimension of that line there, but
it's really not the dimension I want.
| | 01:10 | So I want the dimension from that
line over here to this other line.
| | 01:14 | So notice if I highlight that, and
click it, now it changes where the
| | 01:17 | dimension is, and then my third click
is going to be where I would like to
| | 01:20 | place that dimension.
| | 01:21 | So I placed it right here.
| | 01:22 | So those are the three
steps to start a dimension;
| | 01:24 | pick from where, to where, and
then the third is going to be where you
| | 01:28 | want to actually have that dimension show up.
| | 01:30 | Now, if I just want to dimension this
side over here, I can just do a one-click
| | 01:32 | pick, and place that dimension. And
that's just fine, but sometimes when you
| | 01:37 | have like a radius on the corner or
something like that, it's not actually
| | 01:40 | going to pick up that full dimension,
it's only going to pick up the length of
| | 01:42 | that one line segment.
| | 01:44 | So instead of placing a dimension like
that, you might want to use a two-click
| | 01:47 | method, and pick on the bottom-edge
here, and the top-edge there and then
| | 01:50 | place the dimension.
| | 01:51 | That way, if there's a chamfer or
some other type of radius, or something on
| | 01:55 | the corner, it's not going to be
affected, and you're not going to get the
| | 01:58 | wrong dimension here.
| | 01:59 | Okay, so that's a couple of
different ways to go ahead and place just
| | 02:02 | standardized dimensions.
| | 02:04 | Now, I can move these things around
if I need to, just by picking them and
| | 02:07 | highlighting and moving them around.
| | 02:08 | And the method I might use to, like for
instance, dimension some of these holes,
| | 02:12 | is I can start -- you kind of want to
pick a corner that's going to be your origin of
| | 02:16 | your dimension, so that your baselines --
this is the two baselines we're using.
| | 02:20 | So I'm going to pick from that
bottom of the part, to any one of these
| | 02:24 | circles to give a dimension here,
and I can continue doing that just by
| | 02:28 | clicking and placing dimensions.
| | 02:30 | Now, this is what we're going to
call it is baseline dimensioning.
| | 02:33 | So we're starting from the base and
we're just placing dimensions across there,
| | 02:37 | and then you can arrange
them in a nice orderly fashion.
| | 02:42 | You can see that they look very nice,
and the nice thing about baseline
| | 02:45 | dimensions is they're easy to move
around, there's a clear defined number
| | 02:49 | between the different parts, and
we're starting from this one line here.
| | 02:52 | I can do the same thing in the other direction.
| | 02:54 | I'll pick this as my baseline, and
then I can go ahead and place like a
| | 02:59 | dimension here, keep going across just
by clicking on the pairs of items that
| | 03:03 | I'd like to include.
| | 03:05 | And you can see as if we start
dimensioning more and more items, we start using
| | 03:08 | a lot of space using the
baseline dimensioning schemes.
| | 03:11 | We have to really space these out correctly.
| | 03:13 | And so if we do have a problem with
minimizing our space here, we have a
| | 03:17 | couple of other options which we're
going to cover in the next movie as far as
| | 03:20 | using chain dimensions and/or
ordinate dimensions to put a little more
| | 03:24 | information on a drawing.
| | 03:26 | Those are your basic baseline type of
dimensions, and also, before we get out of
| | 03:30 | this movie, I'm also going to cover --
if you click on these, you have a lot of
| | 03:33 | options over here too.
| | 03:34 | So there's a Precision and
Tolerance, so I can pick a style.
| | 03:38 | For instance, no tolerance here, so if
there's no tolerance, it uses the number
| | 03:42 | of characters after the decimal place.
| | 03:44 | So this is a three place decimal, is what we
call that, so it's a point and then there's
| | 03:47 | three places after it.
| | 03:48 | So that would go down to our block
tolerance here, and we've got a three
| | 03:52 | place decimal as .005.
| | 03:54 | So the tolerance there is five-thousandths
of an inch, plus or minus. All right,
| | 03:58 | if it's a two place decimal, it changes the
tolerance to only being a plus or minus,
| | 04:02 | ten-thousandths of an inch.
| | 04:04 | Keep in mind how many decimal places I'm
showing is defining the tolerance of that dimension.
| | 04:09 | So if I didn't really need that type
of dimension here and there to there, I
| | 04:12 | could change that instead of a three
place decimal to a two place decimal, and
| | 04:17 | now it's going to be using the block tolerance
here of ten-thousandths or, plus or minus 10.
| | 04:19 | So that's the most basic way
to add tolerancing to a drawing.
| | 04:25 | Now, if I wanted a custom
tolerance, I could use something here.
| | 04:29 | So I could say, I'd either want like a Basic,
Bilateral, Limit, Symmetric, a lot of
| | 04:32 | different things we can do here.
| | 04:34 | So if I do like a Bilateral tolerance, that's
going to give me a plus and minus, that
| | 04:38 | this feature can be bigger or smaller.
| | 04:40 | So I'm going to say this is going to
be twenty-thousandths larger, and it can
| | 04:45 | only be ten-thousandths smaller.
| | 04:49 | So now I've assigned a specialty
tolerance to that one dimension here.
| | 04:54 | So it's going to be interpreted differently
when we go ahead and work on the drawing.
| | 04:58 | We are going to cover that
some more in future movies.
| | 05:01 | Dimensioning and tolerancing is
a class in itself.
| | 05:04 | We touched on the basics in this movie.
| | 05:06 | However, this is definitely an area
that will require a bit more study to
| | 05:09 | be great.
| | Collapse this transcript |
| Creating chain and ordinate dimensions| 00:01 | In this movie, we're going to continue
on with dimensioning, by adding the chain
| | 00:04 | and ordinate styles of dimensioning.
| | 00:06 | The whole purpose for dimensioning
our drawings, and even drawings in the
| | 00:09 | beginning, is to relay information
about building our parts to a manufacturer.
| | 00:13 | Now, in the real world, things aren't
quite as perfect as they are in the computer.
| | 00:16 | For instance, if we have a hole and a
peg or a pin, and it's a 2 inch hole,
| | 00:21 | and a 2 inch peg, and if we try to put those
together, it's going to be a pretty tight fit.
| | 00:25 | So we need to make sure we're relaying
information that's going to allow those
| | 00:28 | two items to fit together correctly.
| | 00:30 | So for the hole, we might want to make
the hole slightly bigger and give it a
| | 00:33 | tolerance that's on the plus side.
| | 00:34 | So it says, it can be maybe 2.05, and
maybe ten-thousandths bigger, so it gives
| | 00:39 | a little bit of play.
| | 00:40 | Then, the peg has to be a little bit smaller.
| | 00:42 | So then, when we put them together,
we're guaranteed that within that tolerance
| | 00:45 | block they're going to fit
together and not have any problems.
| | 00:48 | So we want to continue to relay that
information when we're working with
| | 00:51 | drawings, and think about the peg and
the hole methodology as far as how we want
| | 00:55 | to lay these items out, and
how we want to tolerance them.
| | 00:58 | So first, we're going to start with
the chain style dimension, and actually a
| | 01:02 | chain dimension is no different
than a regular dimension here.
| | 01:04 | And in fact, before I start the
chain, I'm just going to start with a
| | 01:06 | regular baseline dimension.
| | 01:07 | I start here, dimension here,
just like we did in the last movie.
| | 01:11 | Now, instead of starting from the
baseline and going to the next item, I'm
| | 01:14 | actually going to start from the last
item, and dimension up here to this next
| | 01:18 | item here, and I can
continue this way, up the part.
| | 01:23 | So this is what you'd call
a Chain Style Dimension.
| | 01:26 | This way, you're holding from hole to hole,
within plus or minus five-thousandths of an
| | 01:31 | inch, to a three place decimal.
| | 01:32 | And if that's a situation you need,
you've got to make sure that these are very
| | 01:35 | accurately represented
between 0.6 between the two.
| | 01:38 | Then, that would be the way to go.
| | 01:40 | So it really depends upon how you're designing
and what the requirements are for your design.
| | 01:44 | You could also combine baseline with
chain dimensioning by getting rid of
| | 01:48 | these and doing a chain from here,
and then continue to do like a baseline
| | 01:53 | from that first hole.
| | 01:55 | So then, you're specifying a tolerance
from the first hole to the other holes,
| | 02:00 | so you're holding now a different
tolerance block to each one of these.
| | 02:04 | So from the first hole to the last hole,
they're not going to be more different
| | 02:08 | than plus or minus five-thousandths of an inch.
| | 02:09 | Now, I know that because I'm
looking at the block down here.
| | 02:12 | For a three place decimal, I've got .005.
| | 02:14 | So I've got plus or minus five-thousandths.
| | 02:17 | And maybe to the edge of the holes,
we're not quite as concerned with the
| | 02:20 | distance, so I could go change this now
to like a two place decimal to give it
| | 02:25 | a little bit more leeway as far as it's
tolerance block, if that was okay in your design.
| | 02:29 | Generally, the larger the tolerance range
you give, the easier it is to make the parts.
| | 02:33 | The tighter you make that tolerance,
the more costly your parts to be made, and
| | 02:37 | the better machinery or more
accurate machinery is going to be needed.
| | 02:40 | So in general, try to open them up if
you can, and that's going to make things a
| | 02:43 | lot easier for manufacturing.
| | 02:44 | Okay, so now we want to look at
the ordinate type dimensioning.
| | 02:47 | So if we have a lot of items across a
part that we need to dimension, using
| | 02:51 | the baseline or chain dimension, you can
sometimes get a lot of dimensions that are crowded.
| | 02:55 | So to use ordinate, all we're going
to do is go up here under the drop-down
| | 02:58 | arrow and I'm going to go down to
Horizontal Ordinate, and same thing if I
| | 03:01 | wanted a vertical one, I
could choose that as well.
| | 03:03 | Pick on Horizontal, and I'm going to
go and pick where I want to start that
| | 03:07 | Ordinate Dimension from, and I'm going
to start from right here, which is going
| | 03:10 | to be the baseline for it.
| | 03:11 | Then I just drag it out
with a click and place that 0.
| | 03:14 | Any item I click on now is going to be added
in a horizontal fashion across from this part.
| | 03:20 | So I'm going to click on this outside
edge here, I'm going to click on this hole
| | 03:23 | here, maybe this line here, that one
there, that one there, that one there, and
| | 03:29 | the hole there, and that hole.
| | 03:30 | So you can see I can quickly add a
bunch of dimensions really quick across a
| | 03:33 | part, and they're fairly compact,
they don't take up a lot of space.
| | 03:36 | I can just click on there, so I get
quite a bit of information with it really
| | 03:39 | quick, ordinate dimension.
| | 03:40 | And the same thing if I wanted to use
a Vertical Ordinate, I could choose a
| | 03:44 | baseline over here, which is really the
same baseline, so I could choose this as
| | 03:46 | my baseline and place my 0 here, and I
can come in, and start dimensioning items
| | 03:51 | like that across the part.
| | 03:52 | So I can add a dimension in, same thing.
| | 03:56 | Now, you can intermix them.
| | 03:57 | Sometimes it's better if you're going
to be in ordinate, just have all ordinate
| | 04:00 | dimensions across your part, because
you can relay a lot of information.
| | 04:02 | But really, your choice and it depends on
really how your specifications are being met.
| | 04:06 | The last thing in this movie, if you do
have a special dimension here, you can
| | 04:09 | always click on that dimension.
| | 04:11 | And we can go in here and change its
tolerance as well, so I can add like a
| | 04:15 | Basic Tolerance or a Bilateral Tolerance to
any individual one of these, if we needed to.
| | 04:19 | And we can change the precision
of each one, by the way, as well.
| | 04:22 | So I can go like a two place decimal
here, and that would be just fine, keep it
| | 04:25 | like a twenty-thousandths or
something like that.
| | 04:28 | The other thing is if we miss
something, say we missed that one dimension
| | 04:31 | there, we can always just click back
on the ordinate, right-click on it, and
| | 04:34 | say Add To Ordinate.
| | 04:36 | Also, if you have the items that are
mixed up a little bit or they're not
| | 04:39 | looking perfect, you can always go here,
and go to Display Options, and re-jog
| | 04:43 | the ordinate or just jog the ordinate,
and move things around a little bit.
| | 04:47 | So you get a bunch of different options.
| | 04:47 | So I'm going to go to Add To Ordinate,
and just add one more item to that
| | 04:51 | and then we're good.
| | 04:52 | There are various tools to dimension
parts, and depending on the conditions and
| | 04:56 | the amount of dimensions, we'll
determine the best dimensioning scheme.
| | 04:59 | There are no hard and fast
rules about the best way.
| | 05:01 | However, best practice would be to try
to relate the information in the easiest
| | 05:05 | and most direct way.
| | Collapse this transcript |
| Dimensioning holes and curved features| 00:01 | There are some special tools and
techniques used for using the Dimensioning tool
| | 00:04 | with holes and curves.
| | 00:06 | By default, the hole dimensions
relate to the center of the hole.
| | 00:09 | So let's go ahead and
apply some dimensions here.
| | 00:11 | So we've got quite a few
different holes on this part.
| | 00:13 | So if I dimension from an edge to a
hole, notice as I go over the hole, I can
| | 00:17 | pick either the center of the hole
and the outside of the hole for the
| | 00:20 | countersink, and either one, so it's going
to really write to the center of the hole.
| | 00:23 | All right, so notice it just drops a
dimension here kind of just hanging.
| | 00:27 | So sometimes it's nice when you're
working with holes, is to add a center
| | 00:30 | line or a center point.
| | 00:32 | And so we can go grab this Center Mark
here and it just allows us to do that and
| | 00:36 | some options over here on the left.
| | 00:39 | If I just place it here, it goes
out pretty big, I can change that to
| | 00:44 | outside the default if I wanted to.
| | 00:46 | I can get rid of the
extension lines if I wanted to.
| | 00:48 | Once I'm in that command, I can continue
to just go here and add center marks
| | 00:51 | to all the different
holes showing where they are.
| | 00:54 | Also when you go back to your sheet
templates or sheet formats, you can actually
| | 00:57 | have it automatically add in
these center marks, if we wanted to.
| | 01:01 | Oh I need one more here.
| | 01:03 | I'm going to center mark the center of
this feature here and I'm going to make
| | 01:07 | it a little smaller. So there it is.
| | 01:10 | All right, so that makes a little easier
to kind of say, hey, this dimension
| | 01:12 | actually is really going
to the center of that hole.
| | 01:15 | Same thing with like hole to hole
dimensions, I can click on hole to hole
| | 01:17 | like this and easily place
that same dimension. Here it is.
| | 01:22 | Now when I have something like this, it's not
actually a full hole, it's just a radius.
| | 01:25 | So then first off, we need to tell the
manufacturer where the center of that radius is.
| | 01:29 | So that's one thing we've got to make
sure we're giving a dimension from here to
| | 01:33 | the center of that radius.
| | 01:34 | So now it knows if we're going to go
create that part where to get that from.
| | 01:38 | All right, so couple of
dimensions here to lay that out.
| | 01:41 | Then we need to go in and
add the radiuses in, right.
| | 01:44 | So we've got a radius here, that's going
to go up to the part and
| | 01:47 | notice it gives you an R value here
that's saying it's a radius, so it changes
| | 01:51 | the way it looks a little bit and then
same thing up here, we need to give a
| | 01:53 | radius of that value there.
| | 01:55 | So a couple of different options and
notice they're having this little leader
| | 01:58 | that drops back to that center point.
| | 02:00 | We can always click on these as well.
| | 02:02 | We can just change the
dimensions if we need to.
| | 02:05 | And then we can add some specialty text
here if we have some special information
| | 02:08 | we needed to add and we can also change
the way it's defined or we can add some
| | 02:11 | special characters like
diameter or degrees or plus or minus.
| | 02:15 | So if you do make a customized
little text, you can add some of that into
| | 02:19 | changing those dimensions around.
| | 02:22 | Now sometimes we just have round
features like curved features like this one or
| | 02:25 | like this one over here, and we
need a dimension to them.
| | 02:28 | So if I go to dimension something like
from the edge of this part here, right
| | 02:31 | to this curved feature, it's going to give
me the edge or the center point of that.
| | 02:35 | All right, so we've king of got this arbitrary
point out there and it's going to be in
| | 02:38 | the middle of that part.
| | 02:39 | So that's sometimes not really what we want.
| | 02:41 | So sometimes you want to make a
dimension from like the outside of a curved
| | 02:44 | feature to another outside of a curved feature.
| | 02:47 | You can do that by holding down Shift.
| | 02:48 | If you hold own Shift while you're
selecting, if I pick the outside edge here
| | 02:52 | and then I pick the outside edge here,
notice it gives me a dimension from the outsides.
| | 02:56 | All right and I can place that dimension
from the outside of a hole to an outside
| | 03:00 | of a hole, or the outside of a curved feature.
| | 03:02 | Maybe you just care about what the distance is
from the base here to the top of this feature.
| | 03:07 | By default if I click on it, it's
going to give me to the center point.
| | 03:09 | But if I hold down Shift and select
that, then it will allow me to pick that one
| | 03:14 | curved feature and give a
dimension there of what that is.
| | 03:17 | So a couple of different ways
to work with curved features.
| | 03:20 | And then the same thing is true if I
want to use the same command here and use
| | 03:24 | the Shift command and pick the inside
of the hole, it's really dependent upon
| | 03:27 | where you pick on the hole and I get
the inside dimensions, so pretty handy for
| | 03:30 | working with those types of features.
| | 03:31 | And then same thing over here, if we
have like a radius in the corner we can
| | 03:37 | just easily drop that out there.
| | 03:39 | And sometimes I'll put the
leader on the inside.
| | 03:41 | If I click on this little dot right here,
it'll push it out to the outside so we
| | 03:44 | can adjust how that looks a little bit
by moving things around and we can always
| | 03:47 | just click on any dimensions and drag
them around so they look the right way.
| | 03:51 | Okay, so that's going to be hole
dimensioning and using curved features.
| | 03:56 | The commands are the
same for working with holes.
| | 03:58 | However there's a few simple
modifiers that are not overly apparent.
| | 04:01 | This movie should give you a good
overview of the tools and the techniques.
| | Collapse this transcript |
| Applying auto dimensions| 00:00 | In this movie we are going to
continue on with our dimensioning techniques.
| | 00:03 | So first off, I want to make sure
that everyone understands that this part
| | 00:07 | itself is related to this
part that we designed.
| | 00:10 | So that's the actual
baseline part that's in the drawing.
| | 00:13 | So if I go to this drawing here, and I
add a dimension across this part, it's
| | 00:18 | a dimension of 6.5.
| | 00:19 | Notice, I can't change that dimension.
| | 00:22 | It just related back to that part which
where that dimension is actually defined.
| | 00:26 | So if I go back to that part now and I
open up that base sketch that created
| | 00:30 | that part, notice that dimension is
that dimension right here, the 6.5.
| | 00:35 | So if I were to change that to 7.0,
it's going to make that part longer, the
| | 00:39 | part updates automatically and then if I go
back to that drawing, it's now seven inches.
| | 00:44 | So that just really just relates
back to that drawing.
| | 00:46 | So keep that in mind while working with designs.
| | 00:48 | Okay so this part, I'll delete that for
right now and we've only got the front view here.
| | 00:51 | So if I wanted to add some more views
to this part, I can go up here to View
| | 00:55 | Layout and do things like a Projected View,
| | 00:57 | I could do the Bottom View here,
I could do a view over here.
| | 01:01 | We could use some of those
| | 01:02 | Auxiliary Views this time by clicking
on a line to project a view out at an
| | 01:07 | angle here, so I can see like that top
hole maybe to mention that out.
| | 01:11 | So there's a lot of things you can do with
your views -- I'm going get rid of that one
| | 01:14 | for right now, just showing you that
right now is a place that you can place a
| | 01:16 | lot of these dimension on different
views, make your own views, there are
| | 01:19 | different ways we want to look at things.
| | 01:21 | But I am going to get rid of that for
right now, I just want to show you could
| | 01:22 | do that and that's just going
to be pulling those views out.
| | 01:25 | Then what we are going to look at
is our dimensioning.
| | 01:27 | So because all those values are
actually stored in the model, SolidWorks
| | 01:31 | actually knows how to go get all those
values and place them in your drawing.
| | 01:34 | Now sometimes it does a pretty good job
and sometimes it's not quite as good of
| | 01:38 | a job, so let's see what it does.
| | 01:39 | So go under Annotations and click on
Drawing Dimensions, and notice this tab up
| | 01:43 | here called Autodimension.
| | 01:44 | Now this is going to reuse a lot
of the skills we just learned about.
| | 01:48 | So it's going to say, what type of
scheme would you like to use dimension in
| | 01:51 | your part, do you want to use a
Chain Dimension, do you want to use a
| | 01:53 | Baseline Dimension, do you want to use
an Ordinate Dimension, how do you want
| | 01:56 | to apply that.
| | 01:58 | And then you can select which edge you want.
| | 02:00 | So notice, this little pink
it's highlighting that edge.
| | 02:03 | So that's the edge it's going to use
for horizontal dimension, it's going to go
| | 02:06 | across the part to there.
| | 02:07 | So if I go to use like a Baseline
dimension, it's going to continually use that.
| | 02:10 | And then same thing over here with
the vertical dimension, if I choose a
| | 02:13 | Baseline dimension here, it's
using this purple edge here.
| | 02:15 | I could use this edge here if I
wanted to, or a different edge;
| | 02:18 | whichever edge you wanted to
use, you could change it to.
| | 02:21 | But right now, by default
it's using this edge right here.
| | 02:23 | There's a lot of different
options you can change here.
| | 02:25 | And then do we want it on
the left or on the right?
| | 02:28 | All right, it's going to either put
the dimensions over here or over here.
| | 02:29 | So I am going to put it over on the
right and once we say OK, it's going to go
| | 02:35 | ahead and do it, and
let's see what happens. Wow!
| | 02:37 | Look at all of these dimensions.
| | 02:40 | So like I said, it does a pretty good
job but it's really not very aesthetically
| | 02:44 | pleasing to have all of these
lines and dimensions and everything.
| | 02:47 | But one thing good about computers
is they remember everything you want.
| | 02:50 | So every dimension here is placed, and
we've learned about a lot of dimensions.
| | 02:54 | Now it's up to you to kind of massage these
into something that looks a little bit better.
| | 02:59 | And some of them you might want to
get rid of and put them here
| | 03:02 | to line up a little bit better.
| | 03:03 | So you can use the Autodimension
technique and sometimes it works out great and
| | 03:06 | sometimes it just really clutters your
drawing and makes it very hard to read
| | 03:11 | and probably take more work to actually
go ahead and figure out how to move all
| | 03:16 | these dimensions to a place that's going
to make sense than just putting them in
| | 03:19 | there in the first place.
| | 03:20 | But a nice thing about it is it makes
sure that all of these items do have
| | 03:25 | dimensions wherever we place them, and
so we got things that are overlapping.
| | 03:28 | We got a lot of things to kind of work
with on this drawing to make sure that
| | 03:32 | this will start looking nice.
| | 03:33 | We are going to be working on that for a
while and trying to make sure that stuff.
| | 03:36 | You can see there is a lot of
dimensions to define this part.
| | 03:39 | And we are seeing some of the hole
dimensions already, we've got a bunch of
| | 03:42 | stuff here that's been laid out and we are
going to be learning about a few of these later on.
| | 03:45 | And same thing if we add another view of this;
| | 03:49 | we have a Projected View, I can
continue to use those same techniques if
| | 03:54 | I wanted to, I can say, Annotation.
| | 03:55 | Go down here to Autodimension
and I can dimension that again.
| | 03:58 | So it's going to add some dimensions here.
| | 04:00 | There's not quite as many dimensions over here.
| | 04:02 | So this time it does a pretty good job.
| | 04:03 | You just have to move them around a
little bit, and these look pretty good as
| | 04:08 | far as dimensioning techniques go, and
just move things around a little bit and
| | 04:12 | move these in properly.
| | 04:14 | We've got a nice way to dimension things.
| | 04:15 | And notice we have these little
helper lines help lines things up and start
| | 04:18 | moving things around with.
| | 04:19 | I just wanted to show this is the
Autodimensioning command, it definitely is very powerful.
| | 04:22 | But sometimes, you want to use it
sometimes you might not depending on how you
| | 04:25 | want to lay out your drawing.
| | 04:26 | And sometimes if you have just too many
dimensions on one area, you might want
| | 04:29 | to make anther view of that part or a
backside view and maybe dimension the
| | 04:32 | holes from the front side and the
other shape from the back side or something
| | 04:35 | like that, just to make it a
little clear to the end user.
| | 04:38 | So that's Autodimensioning.
| | Collapse this transcript |
|
|
19. Adding General AnnotationsCreating hole callouts| 00:00 | Specifying holes is very common in SolidWorks.
| | 00:03 | If you use the Hole Wizard to create
your holes, then you're in luck, and the
| | 00:06 | software will help you
callout the holes as well.
| | 00:09 | If not, you can still specify
holes with simple note changes.
| | 00:12 | So over here in SolidWorks, we're
going to go and take a look at some of the
| | 00:14 | different holes that we have
established here on our part.
| | 00:18 | So I am going to go up here to the
Annotations and use the regular Dimension tool.
| | 00:23 | So if our dimension just a hole itself, it
just gives me the outside dimension and
| | 00:26 | it just gives me a diameter symbol in
front of it, it gives me the size.
| | 00:29 | That's just standard dimension tool.
| | 00:31 | We also have a thing called the Hole Callout.
| | 00:33 | So we use the Hole Callout -- actually it's
going to go ahead and pull all the data
| | 00:37 | from the Hole Wizard that
went and created that part.
| | 00:40 | If I click here, it's going to bring
all that data out, and notice that gives me a
| | 00:42 | three times, it gives me the diameter
of the hole through there, it gives me a
| | 00:46 | counter sync symbol and then the size
and then the degree of the counter sync.
| | 00:49 | So all that data is coming from there.
| | 00:51 | If we look at the part behind the
scenes here, that all came from this feature
| | 00:56 | here, that created that Hole Specification.
| | 00:58 | So all that, the angle, the size, the Through All
condition, all that data is being pulled in.
| | 01:02 | So when you do make and use the Hole
Wizard, make sure you fill this out
| | 01:05 | correctly because that's what's going
to propagate through to your drawing when
| | 01:08 | you go ahead and create it.
| | 01:08 | So let me go back to the
drawing, that's already there.
| | 01:11 | Now, if you didn't use the Hole Wizard
to create a hole, I can still go ahead
| | 01:15 | and add a dimension or something like
that to a hole and then notice, I've got
| | 01:18 | like four holes here.
| | 01:19 | So I can just go down to the text box
where the dimension is and notice, it's
| | 01:23 | giving a little bit of cryptic
information here like MOD-DIAM-DIM.
| | 01:27 | So, don't change that part, but we
can type it in front of that like 4x and
| | 01:30 | that's totally fine.
| | 01:32 | So that's what's pulling that
information back from SolidWorks.
| | 01:34 | So those are the information, and then
we can also add like if we need to add
| | 01:38 | like a diameter symbol or degrees or
plus or minus or something like that, we
| | 01:41 | can add special features in here as well.
Or if we wanted like a counter board or
| | 01:45 | something like that.
| | 01:46 | We can add that symbol and then give it a
depth or something like that, the Depth command.
| | 01:50 | You can just add those to
your callout here as you go.
| | 01:52 | If you don't want them, you can just delete them out
of that box there too, and we're back to where we were.
| | 01:56 | Now in some situations, this whole
callout or diameter callout or something like
| | 02:01 | this is not going to work.
| | 02:03 | So these holes here are actually kind
of special and since it's a little bit
| | 02:06 | hard to see those holes, so what I'm going
to do is actually illustrate them on a drawing.
| | 02:10 | I'm going to use a line here and
I'm going to use like a centerline.
| | 02:13 | I'm just going to kind of snap up
here to above this part here, and I'm just
| | 02:18 | going to go right through all those holes
and I want to make basically a section cut.
| | 02:22 | So that's what I'm going to use to
section this part up in half and go up
| | 02:25 | here to Section View,
which is under View Layout.
| | 02:28 | Click on Section View, and it's saying
it's not going to cut away through because
| | 02:31 | it doesn't extend up here pass that,
that's just fine, and there you have it.
| | 02:35 | I can cut a little section view
of my model and place it over here.
| | 02:39 | I can place it on the right or left wherever
I want to of how I want to look at that cut.
| | 02:44 | Typically, we'd probably put this on the right
hand side here or we can click and flip the
| | 02:48 | direction that it cuts in, and so now we
have it going in this direction, we can
| | 02:52 | see those holes, and it's
giving you the Section B-B.
| | 02:54 | Okay, so now you can see, these holes
are actually quite complicated and they're
| | 02:58 | intersecting another hole from the edge here.
| | 03:00 | So this is where you might want to go
and use a detailed view, or something like
| | 03:03 | that, and annotate this out a little further.
| | 03:05 | I can start specifying
the angle of the cuts here;
| | 03:08 | I can start specifying the size of
the through hole, the depth, the angles, a
| | 03:13 | lot of that kind of stuff as well.
| | 03:14 | So that's a nice way to kind of
specify some of the stuff that might not be
| | 03:17 | overly apparent just from the top view,
so we can cut into there and take a look
| | 03:22 | and see some information.
| | 03:23 | And notice you've got a hole
here too that's coming down.
| | 03:25 | So I can go and move this view
around a little bit. All right, and
| | 03:29 | I can make another projected view of
this part here and put it up here and
| | 03:33 | that's that hole there.
| | 03:33 | We can see it again, I can go back to
the Annotations and I can use that hole
| | 03:37 | callout, and then I can go and specify that
hole there and see what it's going to say.
| | 03:43 | So it's going to give you an NPT tapped
hole with a near side counter sync,
| | 03:46 | there's a lot of data that it's
going to pull from there.
| | 03:47 | So that's going to be that through hole
there, it's going to intersect
| | 03:49 | these other holes, so you have kind of like a
little port, probably some olive oil is going
| | 03:53 | to be flowing through that part and out
through some NPT port here to something else.
| | 03:58 | So, a lot of things we can do with
the Hole Callouts and bunch of powerful
| | 04:01 | tools that we can use.
| | 04:02 | As with many things in SolidWorks,
there's a handy tool to callout holes.
| | 04:05 | The tool does most of the work for you.
| | 04:07 | However, make sure to double check
your callout values make sense.
| | 04:11 | After all, it's just writing the
input values from your part file if you're
| | 04:14 | using the Hole Wizard.
| | Collapse this transcript |
| Adding center marks and centerlines to a drawing| 00:01 | Center marks add a nice reference
to a hole center or arc location.
| | 00:05 | SolidWorks has a tool for inserting
these, we can also set up our template to
| | 00:08 | auto insert the center marks for us.
| | 00:10 | Centerlines can be helpful for drawing and
indicating the alignment of various features.
| | 00:14 | I got a part here with a series of holes
and we are going to make a drawing for that.
| | 00:17 | So let me go ahead and go up here to
Make Drawing from Part and let's select
| | 00:22 | that TT one and drop it in, and I'm just
going to bring the top view in, there it is.
| | 00:29 | So we have a top view of that part and we
want to establish some of the holes.
| | 00:34 | First off, I am going to
change a few things around.
| | 00:35 | I am going to go back to this Properties
and we are going to change the scale.
| | 00:38 | So probably try 1:1, see how that looks.
| | 00:42 | It's a little bigger, that looks good.
| | 00:44 | So we can see things a little clearer.
| | 00:46 | And if we're going to go dimension all
these things out then we might want to go
| | 00:48 | and add center marks.
| | 00:50 | So if I go up to Center Marks command
here, which is under Annotations, or I
| | 00:54 | can click on each one of these holes and
start adding the center marks, and if we
| | 00:58 | click on that little button there, you
see that it just actually added a grid
| | 01:02 | for us, pretty handy.
| | 01:04 | That's something that's
fairly new in SolidWorks.
| | 01:06 | So let's go back and see if
we can see that one more time.
| | 01:08 | So if I go and I put a center mark in,
notice here's the Center Mark, it
| | 01:13 | recognizes a pattern.
| | 01:14 | As soon as I place that first mark, it gives
us this little Propagate icon here, so
| | 01:18 | it's saying that once I placed one, I
am going to propagate it through all
| | 01:21 | these other things.
| | 01:22 | And notice, not only does it give us
center marks, it also gives us centerlines
| | 01:26 | between all of those.
| | 01:27 | What that does is it
establishes this as a grid pattern.
| | 01:30 | So we can see that these are all
related, they will have the same spacing.
| | 01:33 | So over here, we do the same thing.
| | 01:36 | I can click on a hole, but this time
it's not really a grid pattern. And the
| | 01:39 | reason it gave me the grid pattern
is because I used the linear pattern
| | 01:43 | technique for creating this one.
| | 01:44 | This one I just laid it out.
| | 01:46 | So if I want to go ahead and establish the
center marks, I have to go in
| | 01:48 | and add a center mark to each one of these
items, and then go ahead and use some centerlines.
| | 01:53 | Now we have all the Sketch tools
available in the drawing functions of
| | 01:57 | SolidWorks as we do when we're
creating parts.
| | 01:59 | So we can go ahead and just draw a box
out here if we wanted to, draw a rectangle,
| | 02:03 | and we can define the box with
dimensions if we wanted to.
| | 02:05 | There is a lot of things we can do.
| | 02:07 | We can just create drawings
from the beginning in SolidWorks.
| | 02:09 | There is nothing saying that we can't
do that, and sometimes people do just
| | 02:12 | design things in a drawing view and
just lay it out. If you have something
| | 02:16 | simple, and you need to turn it into
solid, you have all that ability.
| | 02:19 | Speaking of those same tools just to lay
things out inside the drawing too, if I
| | 02:23 | want to just dimensions or just put a
centerline from here to here, there to
| | 02:26 | there, there to there, there to there,
it's just saying, these four holes are
| | 02:31 | all related together and
saying they're aligned up as well.
| | 02:34 | Then I can give a dimension from
an edge to this line here and I have
| | 02:39 | dimensioned only this first hole, but
it's also saying this hole is inline with
| | 02:41 | the first hole, and same thing here.
| | 02:43 | If I am going to give other dimension
here from that hole to that hole and place
| | 02:46 | it and place from here to here
and then from there to there.
| | 02:50 | That way we find the spacing, everything
looks clean, and then it really kind
| | 02:54 | of continues that dimension line across
to the next part so we can really see that
| | 02:58 | they are all part of the same team here.
| | 03:00 | One other thing I was going to show is
I am actually going to get rid of this
| | 03:03 | hole view now, delete that out,
delete the view and I am going to go
| | 03:07 | and try to add it in.
| | 03:07 | But this time, instead of putting all that
work into it at the beginning, let's go up to
| | 03:11 | some of our options and under Document
Properties, we can come down here to
| | 03:16 | Detailing, and in Detailing it
says, Auto insert on view creation.
| | 03:20 | So we can say center marks for holes,
center marks for filets, slots, center
| | 03:25 | marks for holes and assemblies, centerlines.
| | 03:28 | Look at a lot of these things,
we can automatically add in.
| | 03:30 | Okay, so I am going to click OK,
turn those on.
| | 03:34 | Now let's go and grab a Model View,
that same one we have right there, and
| | 03:39 | let's take a look at that top of that
part and drop it in there and take a
| | 03:43 | look at what it did.
| | 03:44 | It created a whole grid pattern
for us and add all the center marks.
| | 03:47 | It didn't add the centerlines between
there here, because they weren't created
| | 03:50 | as a grid pattern but a lot of that
work we just did is all automatically
| | 03:54 | created just by turning those two options on.
| | 03:57 | We have a lot more options in
the software option to do that.
| | 04:01 | Sometimes it works good, but sometimes
if you do have too many centerlines, and
| | 04:03 | too many center points, your
drawing will start looking a little messy.
| | 04:06 | So you have the ability to turn that on
automatically but you've got to make sure you
| | 04:09 | have that option turned on before you
insert that view into your Model view.
| | 04:13 | Center points and centerlines are great
for showing feature's locations without
| | 04:17 | the need for excess dimensions.
| | 04:18 | Use these tools to link together
related features and make your drawings easier
| | 04:22 | to understand and clear.
| | Collapse this transcript |
| Adding item notes| 00:01 | Almost all drawings have some sort of
notes calling out information that cannot
| | 00:04 | be relayed in the views.
| | 00:06 | Common information is materials, finishes,
extra processes, special features or packaging.
| | 00:13 | SolidWorks has a Note tool that allows
us to type out notes and even has some
| | 00:16 | auto-indent and numbering functionality.
| | 00:18 | Additionally, these notes can be saved
in the Design Library for future use.
| | 00:22 | I'm going to click on the Note command
here and go up in the upper left hand
| | 00:25 | corner and just place a note.
| | 00:26 | I'm just going to start typing it out,
and I type a 1 and I can give it a finish
| | 00:33 | or something like this that I want to finish.
| | 00:36 | As soon as I click on OK, I'm going
to have the 2.0 and notice it adds the
| | 00:41 | numbering for me and auto-indents it
for us and then wherever I place that
| | 00:45 | note now is going to be on my tool tip, so I
can just place it somewhere else in the drawing.
| | 00:48 | If I hit Escape I can get out of
that and just delete those notes and I
| | 00:52 | happen to have a note already saved
from a text file, I'm going to just paste
| | 00:55 | in here, and you can paste things
from any text file or a Word document
| | 01:00 | directly into Notes, pretty easy.
| | 01:01 | Then if I want to go save this note to
the Design Library, I'm going to click
| | 01:05 | over here under Design Library and
notice I've got some folders called
| | 01:09 | annotations, assemblies, features and
this is where we have a lot of other
| | 01:13 | blocks and surface callouts and
that's where I'm going to save my note.
| | 01:16 | So I'm going to say Add to Library,
first I'm going to select it and then I am
| | 01:20 | going to say Add to Library.
| | 01:21 | It's going be Note<1> that's being saved,
and I'm going to call this one N1 for
| | 01:26 | Note 1, okay and I'm just going to Save it
in annotations and click OK and there it is.
| | 01:31 | So N1 is now in that library.
| | 01:33 | If anytime I want a new note I can just
delete this one now and I can go
| | 01:36 | and grab a note and just drag and drop
it in and place it on the screen, quick
| | 01:40 | and easy, very nice.
| | 01:42 | Also under the Note command is the
ability to add some little boxes or triangles
| | 01:48 | and that's under this thing called Border.
| | 01:48 | So I'm going to click on Border and
then click on Box and I'm going to make it
| | 01:53 | just like a 1 Character box, and notice
where I place that box and I can fill out
| | 01:57 | like a number, like 1.
| | 01:58 | Okay so then have 1, and notice once I
have this box here I can add a Leader to it.
| | 02:04 | So I can go to back to Leaders and I
can add a Leader here, then I can then
| | 02:08 | relate this or link this back to a
drawing and move it around and grab the
| | 02:12 | tip of it and attach it to like a hole or
something that and then we can have a note.
| | 02:16 | So this would relate from Note Leader
1 to the first Note in your drawing.
| | 02:20 | Now let's take a look down here in the
bottom right hand corner of our screen.
| | 02:24 | We have the block and we have some
information that we can fill out like the
| | 02:29 | title of the drawing, number
| | 02:30 | and the revision, material, finish.
| | 02:32 | So we could just go up here and grab this
Note box and start typing if we wanted to.
| | 02:36 | However, a lot of that information is
actually in the part behind the scenes here.
| | 02:40 | So instead of filling this out directly,
let's go back to that part and open it up.
| | 02:45 | So inside of this part here the
first thing we're going to look at is the
| | 02:48 | material, and up here in the left-hand
corner we have this little material box
| | 02:51 | and right now we've got
AISI 304 stainless steel.
| | 02:54 | If I right-click on that, I've got a
whole listing of different materials that I
| | 02:57 | can select from to quickly change that.
| | 02:59 | If I do change something, it changes
the material, color, and all of the
| | 03:03 | material properties.
| | 03:04 | In fact if I go over here to the
right, I click on Mass Properties;
| | 03:07 | I can go find out what those properties
are, the density, the mass, the volume,
| | 03:10 | a lot of information.
| | 03:11 | Okay, so if I do want to go and change
the material I can also go over here and
| | 03:14 | say Edit Material to get the full listing.
| | 03:17 | You can see we've got a lot of different types
of steels, irons, aluminums, and if I pick
| | 03:21 | one of those like a steel, and I go to
304 stainless I get the mechanical
| | 03:25 | properties, I got the appearances, hatching;
a lot of information and if I don't have
| | 03:29 | that in my list of Favorites I can
always just click and add it, but I do have it
| | 03:32 | here at the bottom, so I don't need to add it.
| | 03:34 | Now that I have the material I've got
it selected, I'm going to go up here and
| | 03:38 | add some custom properties.
| | 03:39 | So click on File Properties.
| | 03:41 | The first tab here is called Summary
and I can type in the author, keywords
| | 03:45 | or comments, and some information down here
about when the last time I saved this file was.
| | 03:49 | Under Custom Properties is actually
where we're going to start filling out that
| | 03:52 | information we want on the drawing.
| | 03:53 | I'm going to click on Description and
I'm going to call this one PLATE and then
| | 03:57 | I am going to go down here to part
number and I'm just going to name it
| | 04:01 | the same as the file name, which is the
19.1-1, and then maybe Revision we'll fill
| | 04:08 | out, revision A, and then we
can also link to properties.
| | 04:14 | So I come down here to like material,
instead of typing it out I can actually
| | 04:18 | click on this little drop-down
arrow here and link to a property value.
| | 04:21 | Notice we got a lot of different things in here.
| | 04:23 | I'm going to select the material which
is the top one and notice it gives us
| | 04:27 | this Malleable Cast Iron
exactly what we selected over here.
| | 04:31 | And then we're going to go down to
Weight and select weight, and we'll click it
| | 04:34 | to Mass, so now we got the
mass of that property as well.
| | 04:37 | So we are linking these values
from the solid to the drawing.
| | 04:41 | So click OK when we got all that done and
now let's jump back over to our drawing.
| | 04:46 | And notice this information is now
filled out, so the description, the revision,
| | 04:50 | the drawing number, the
material, a lot of stuff is filled out.
| | 04:53 | Some things aren't filled out though, like
finish and drawn by or the date, so
| | 04:57 | there's actually values hidden behind there
that we haven't filled out yet or dealt with.
| | 05:02 | I can look at those by clicking on
View > Link > Annotation Link Errors.
| | 05:07 | And if I right-click and say Edit Sheet
Format, I can actually go in here and
| | 05:11 | hold my mouse over one of those, and it
will tell me which of those I'm actually
| | 05:14 | linking back to and that's kind of a
cryptic notation that it uses is at dollar
| | 05:18 | prompt $PRP, which means the
part and then the company name.
| | 05:21 | And I get the same thing if I go
over any one of these other ones here.
| | 05:24 | So you can go see where
these things link back to.
| | 05:26 | You might be saying, well it'll be really neat
if I could actually make my own, and you can.
| | 05:30 | So I'm clicking on Note, I
just drop a note up here.
| | 05:34 | I actually have the option to make a
hyperlink here first, or I can click on this
| | 05:37 | one here Link to Property.
| | 05:38 | If I click on that, I got a couple of choices
here as far as how do I want to link them.
| | 05:42 | I want to use a second one here,
which is the model in view.
| | 05:45 | I'm going to click on that.
| | 05:46 | I've got all these different values, and I'm
going to link to Author, but I can link
| | 05:49 | to anything I want, click OK, and it
shows me what I'm actually linking to.
| | 05:55 | And once I'm happy with that I might
say hey, why is it not there?
| | 05:59 | Well, we have to make sure we fill
these values out back in that part or
| | 06:02 | they won't show up.
| | 06:03 | So I'm going to go back to the part
now and I'm going to look at this part.
| | 06:06 | Go back to the File Properties and I'm
going to fill out my name under Author.
| | 06:13 | Click OK and then go back to the drawing.
| | 06:16 | Here is the drawing, and notice there
it is, my name popped up and for some
| | 06:20 | reason if it did not show up we can always go
up here to Rebuild to make it pop-up here.
| | 06:25 | And notice we also have these errors showing up.
| | 06:27 | So if I don't want to view those, I
can always go to click on View >
| | 06:32 | Annotation Link Errors, and make sure
those aren't showing right now.
| | 06:35 | All good drawings should always
have some sort of drawing notes.
| | 06:38 | Use the notes to further explain
complex operations or to callout specs for
| | 06:42 | post-finishing operation.
| | Collapse this transcript |
| Drawing revisions| 00:01 | Revisions are best handled at the
part level, and we link our drawings
| | 00:04 | to that part revision.
| | 00:06 | The custom properties of the part will
generally have some revision property
| | 00:10 | that we can fill out.
| | 00:11 | From there we need to make sure our
drawing template is linking to that property.
| | 00:15 | Once we have a revision, we might also
want to add a revision table that says,
| | 00:19 | what has been changed and at what stage.
| | 00:21 | We have a part here that doesn't
have any revision data in it at all.
| | 00:24 | So we are going to do a little review
and add a revision to it. And we'll go back
| | 00:28 | here to the part and click on the File
Properties at the top, and click here and
| | 00:33 | we want to go to the Revision.
| | 00:33 | That's all we are going to add to this
one and we are going to add Revision A.
| | 00:37 | Click on OK, and now we have added that,
let's go back to the drawing and we
| | 00:41 | should show up with Revision A.
| | 00:43 | Now we want to go up here
and add a Revision table.
| | 00:46 | So anytime we are making a drawing
change, we are going to put those
| | 00:49 | changes into the table.
| | 00:50 | Now most of the time when you start with a
drawing table, we are just going to have --
| | 00:53 | especially Revision A, it is just going to
say this is the initial release of the drawing.
| | 00:56 | So to do that, I am going to say
Insert > Table > Revision Table.
| | 01:01 | These are some of the options we can use, but
most of these are just the defaults, so just
| | 01:05 | click OK and it's just going to drop
that table, and now I can move this table
| | 01:09 | around a little bit and we can resize
it by just dragging things out and make
| | 01:13 | sure we got enough space here.
| | 01:15 | Once you have got your table looking the
right way, you probably want to add it
| | 01:18 | to your sheet format.
| | 01:19 | So every time you open up a new drawing,
that revision table is already going to
| | 01:23 | be there. It's already going to
be formatted in the right way.
| | 01:24 | So we will go here and just snap up
to the upper corner and let's bring it
| | 01:29 | in just a little bit.
| | 01:31 | There we go, it looks nice.
| | 01:33 | Okay, now we're going to add a revision. To
do so, we are going to right-click and say
| | 01:36 | Revision > Add Revision.
| | 01:39 | And it goes ahead and adds that, and
notice my tool tip is a little marker.
| | 01:43 | I can go and add something that the
revision pertains to, but generally in our
| | 01:46 | first revision there is not going to be
anything that changed because it's the first
| | 01:49 | time you are releasing the drawing.
| | 01:50 | So hit Escape to just turn that off.
| | 01:52 | Then I can go in here and edit this row.
| | 01:55 | Just because I want to make the
fonts a little bit bigger and I do so by
| | 01:58 | clicking on this document font thing,
and I am going to go up here to maybe 16
| | 02:02 | point, or 14 point is probably a little
better, makes it a little bigger, easier to see.
| | 02:06 | Now imagine we make a change to
this drawing, actually this part.
| | 02:10 | To make a change to the part, we want to
sure we go and roll the revision forward.
| | 02:13 | So to do so, I am going to go back to
the part, there is some part that got
| | 02:17 | changed, and I will go back up to the
File Properties and make sure I am changing
| | 02:20 | this to Revision B now.
| | 02:22 | So I am going to click on that, now
we have a revised part, go back to the
| | 02:25 | drawing and now we have
a Revision B drawing.
| | 02:28 | So we want to make sure we
reflect any changes in the table.
| | 02:31 | Let's go back up here, right-click on
it again, say Revisions > Add Revision, and
| | 02:35 | it's going to give us Revision B,
and notice we have that tool tip.
| | 02:37 | So now if I have something maybe like
this hole down here, it has changed, I can
| | 02:41 | click and place a revision symbol.
| | 02:44 | Now I also have a zone, so I have -- if you
look at these numbers here, 26 and 7 and I
| | 02:49 | have a zone b over here, or
| | 02:50 | AB so I can give it like a B7 zone.
| | 02:54 | So somewhere in this zone here that
change happens and I can actually write
| | 02:58 | that number right in here if I wanted
to and then I can describe what I am
| | 03:02 | changing. If I changed maybe the hole
size to this from this size to that size.
| | 03:05 | We don't have to search around the
drawing to figure out what's got modified.
| | 03:10 | Revisions are very important in design
and even more important in manufacturing.
| | 03:14 | Each time a part is changed, the
revision should be updated in the
| | 03:17 | corresponding drawing.
| | 03:18 | Failure to roll the revision of parts is
a leading cause of manufacturing errors,
| | 03:22 | mostly from not being inspected
or made to the latest changes.
| | Collapse this transcript |
|
|
20. Assembly DrawingsAdding assemblies to drawings| 00:00 | Drawings can be made from assemblies,
just like we make drawings of parts.
| | 00:04 | However, most of the time, in an
assembly drawing, our focus is different.
| | 00:08 | On the part side, we show the
dimensions and the finishes.
| | 00:12 | On the assembly side, we're more
concerned with what parts are in the assembly
| | 00:15 | and how they're connected together.
| | 00:17 | Some of the tools specific to assemblies are
balloons, builds and materials, and weld callouts.
| | 00:23 | We'll be covering it in the next few movies.
| | 00:26 | In this movie, let's get the
assembly drawing started and add some views.
| | 00:29 | I've got an engine that we've designed
and it's got a lot of components here,
| | 00:33 | I just want to show first before as
we're making the drawings for it.
| | 00:37 | Over here in the tree, you can see
we've got a lot of different items, and in
| | 00:40 | fact, we even have folders in here
with even more items as far as the hardware.
| | 00:43 | We've a lot of things here.
| | 00:45 | So we're not going to get started with
entire assembly drawing, and we can even
| | 00:49 | see that we've got other subassemblies built
inside of here, so quite a complicated model.
| | 00:54 | Now let's look at the view here and I'm
going to take this part here and click
| | 00:57 | and say Change Transparency.
| | 00:59 | I can see inside there and I can just
show you that if we zoom in a
| | 01:03 | little bit, spin it around, I can
move this engine around and all of the
| | 01:07 | components move around;
| | 01:08 | the engine, the pistons, the crankshaft,
the valves, everything moves just like
| | 01:12 | it was a real engine and in fact,
this is a scale model of an engine.
| | 01:16 | So if you hooked it up, it actually works.
| | 01:19 | Spin it around a little more, you can see
all the detail here and all the different
| | 01:22 | fasteners and different
features we've added together.
| | 01:25 | So, the part we are going to make an
assembly drawing for of this is just a
| | 01:29 | space here, and I have that opened up,
and here it is and there is the base.
| | 01:33 | You can see, here is all the
parts to make that up and a bunch of
| | 01:36 | different hardware.
| | 01:37 | A couple of these are the same parts,
so we got two of these, two of these, and
| | 01:42 | you got a top and then you get the hardware.
| | 01:43 | So let's go ahead and make
a drawing of this assembly.
| | 01:46 | So let me go to File > Make Drawing from
Assembly, and it's going to open up the
| | 01:51 | same template we've been using. Click OK.
| | 01:54 | Now over here on the right, I've got a
couple of different views that we can use,
| | 01:57 | and I'm just going to choose the right
hand view and just drag that into the
| | 02:00 | screen, and as soon as I do that,
obviously, I'm in the Projection mode and I'm
| | 02:04 | going to just going to drop
a couple more projections.
| | 02:06 | Now that I have the projections on the
screen, I'm going to move things around a
| | 02:09 | little bit and lay it out.
| | 02:12 | Our focus generally when we're working in
assemblies is not to add a lot of dimensions
| | 02:16 | to our parts into our assemblies.
| | 02:18 | We're really more concerned about
which parts are here and how they're
| | 02:21 | connected together. So we might be
detailing out the hardware, giving up building
| | 02:25 | material as far as where things are,
ballooning out the different items, so we
| | 02:29 | know where each item is in our assembly.
| | 02:32 | The same tools are available for
both parts and assembly drawings.
| | 02:36 | However, when we're making an assembly,
the documentation should focus on what
| | 02:40 | parts are in the assembly
and how they are attached.
| | 02:43 | Hardware generally plays a big part
in assemblies and good descriptions
| | 02:47 | can really help out.
| | Collapse this transcript |
| Including a bill of materials| 00:00 | A bill of materials is a shopping list
for the items that make up an assembly.
| | 00:04 | Many times this list is made up of
parts that you or members of your team
| | 00:08 | design, parts from outside
vendors, downloads and/or hardware.
| | 00:13 | Keeping track of all these parts
and part numbers can be a big job.
| | 00:16 | Different companies have various
standards, some add internal part numbers,
| | 00:20 | some just use vendor part numbers.
| | 00:21 | Hardware can be called out in many ways
and it's all about the user preference.
| | 00:26 | There's no correct answer,
it's just a matter of preferences.
| | 00:29 | So first off let's go ahead and add
a bill of materials to our drawing.
| | 00:33 | Now we have this same assembly
we we're using in the last movie
| | 00:36 | open and I'm going to go up here
to Insert > Tables > Bill of Materials.
| | 00:40 | When I first click that, I get this
little window on the side over here that
| | 00:45 | gives me a bunch of different options.
| | 00:46 | First one is do I want top-level only
parts, do I want parts, or do I want them
| | 00:50 | indented with the top-level and the parts.
| | 00:52 | So I'm going to just use top-level,
it's fine, and then I can go down here and
| | 00:56 | have a few other options as far as
how I want to display these items, I can
| | 01:01 | change the way I want to number the different
items of the bill of materials as well.
| | 01:04 | But I am going to just use the basic one,
click on OK, and notice it gives me a
| | 01:08 | little table that I can
drop anywhere on my screen.
| | 01:10 | I want to drop it just over here.
| | 01:12 | So then I can modify that a little bit,
I am just going to move these things
| | 01:15 | around so we get a little bit more space.
| | 01:18 | And I can grab this lower corner and
drag the table out a little bit, and notice it
| | 01 |
|
|
