IntroductionWelcome| 00:03 | Hi, I'm John Helfen, and welcome to
Up and Running with Autodesk Inventor.
| | 00:08 | In this course, I will show you everything a
beginner needs to know to get started creating
| | 00:12 | parts, building assemblies,
and documenting your designs.
| | 00:15 | First, we will explore the interface and how it's
used to interact with the models that we'll be building.
| | 00:20 | Then we'll learn how 2D sketches
can be used to create 3D models.
| | 00:24 | After building several models, we'll look
at how those items can be assembled in order
| | 00:27 | to test how they would
function in the real world.
| | 00:30 | And finally, we'll look at how to document
your designs so that when the time comes,
| | 00:33 | you can have your own parts manufactured.
I'm very excited to be presenting this course.
| | 00:37 | So, welcome to Up and
Running with Autodesk Inventor.
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| Using the exercise files| 00:00 | If you're a Premium Member of the lynda.com
online training library, you have access to
| | 00:04 | the files used throughout this course.
The exercise files are organized by chapter.
| | 00:09 | If you go inside of a chapter, you will
find each separate movie has its own subfolder.
| | 00:14 | Inside that subfolder are
the files used in that movie.
| | 00:17 | So, for example, let's go inside 05_Assemblies,
and then go into the movie 01 folder.
| | 00:24 | In this folder, you will find an assembly
file that shows the completed version of the
| | 00:27 | exercise and all the parts
required to follow along.
| | 00:32 | Also included in the exercise files is a
completed version of the engine assembly for you to
| | 00:36 | explore on your own time.
| | 00:39 | If you don't have access to the exercise files,
many of the exercise files start from a blank screen,
| | 00:44 | so you will still be able to follow along.
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1. Basic ConceptsExploring major workflow steps| 00:00 | When starting a new course on Autodesk Inventor,
I find it very helpful to step back and provide
| | 00:04 | everyone with an overview of what Autodesk Inventor
does and go over a few of the basic workflow steps,
| | 00:11 | so everyone has a good understanding of
why we're here and where we're going.
| | 00:15 | During this course, we will be working with a
small engine that you might find in an RC boat.
| | 00:19 | But to cover the basic workflow concepts,
I like to fall back to the toys that allow
| | 00:23 | me to do the things I do today, the trusty LEGO.
| | 00:26 | The reason for this is nearly everyone on
the planet will recognize what they are and
| | 00:30 | how they work without too much explanation,
and it allows me to easily explain the concepts.
| | 00:35 | I see Legos as one of the most
basic physical prototyping tools around.
| | 00:40 | You have a bucket of standard parts, and you
snap them together in different configurations
| | 00:44 | to build anything you could dream of.
| | 00:46 | Autodesk Inventor is a digital prototyping
tool that allows you to build parts like a
| | 00:51 | single Lego brick, or parts of an engine,
and then put them together and test how they
| | 00:55 | would function before you
actually manufacture any real parts.
| | 00:59 | But an Autodesk Inventor, rather than
starting with a bunch of predefined bricks that you
| | 01:03 | might pull out of a bucket stored in the
closet, you're actually pulling parts that you've
| | 01:06 | built from a folder on your hard drive.
| | 01:09 | The workflow in Inventor can be broken down
into three major steps, building parts, assembling
| | 01:14 | parts, and documenting
your designs with drawings.
| | 01:17 | When building parts, you'll sketch 2D shapes
and use modeling operations to add and remove
| | 01:23 | material to sculpt a part.
| | 01:25 | I've captured a few images to help show how
you might build a simple LEGO brick in Inventor
| | 01:29 | so that you can better understand the process.
| | 01:32 | Once you've built the parts needed for your
design, you can begin pulling them into an
| | 01:35 | assembly file and connecting them, in
this case, to build a simple LEGO house.
| | 01:41 | Once you understand the software, you'll be
able to build much more complex parts and
| | 01:45 | assemble those to build something more advanced.
| | 01:48 | Last but certainly not least, you must be
able to document your designs so that when
| | 01:52 | the time comes, you can
have those parts manufactured.
| | 01:55 | This will be done by creating views of
your parts and assemblies that will be used to
| | 01:59 | completely define how the
part should be manufactured.
| | 02:02 | The beauty of the entire system is that all the
parts, assemblies, and drawings are connected.
| | 02:07 | So if changes are made to any part, the assemblies that
contain the part and the drawings all update instantly,
| | 02:13 | so you can focus on improving your designs, rather
than wasting time redrawing 2D views of your parts.
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| Reviewing different file types| 00:00 | Before we begin digging into the product, I
wanted to take a minute and talk about the
| | 00:03 | file types that can be
created with Autodesk Inventor.
| | 00:07 | Just like Microsoft Office has specific
file types for Word documents, Excel documents,
| | 00:11 | and PowerPoint, Inventor has
similar file types of its own.
| | 00:16 | To see the types of files that can be created
with Autodesk Inventor, you can click the New
| | 00:20 | button, which is found in the
Getting Started tab in the Launch panel.
| | 00:25 | This brings up our New File dialog.
| | 00:28 | On the left you can see a browser that
includes an organization structure for templates that
| | 00:33 | can be used in Inventor.
| | 00:35 | When installing Inventor, a series of
selections during the installation like the standard
| | 00:39 | you're using and the unit you want to
use are reflected partially in this list.
| | 00:44 | The default templates include those settings,
but you'll also have more specific templates,
| | 00:50 | for example, in English and Metric that are
more specific to different types of standards.
| | 00:56 | For example, in the Metric templates we
have both ANSI and DIN as well as some others.
| | 01:03 | While you're learning Inventor, most of the time
the default templates are going to work well for you.
| | 01:08 | If you're using Inventor in a commercial market
or a commercial environment, I highly recommend
| | 01:14 | that you consult your CAD manager before you begin
creating any types of files or parts in Inventor.
| | 01:19 | The reason for this is it's very common for
companies to create their own standards or
| | 01:24 | variations of existing standards that have been agreed
upon with manufacturers and partners that you work with.
| | 01:31 | So again, if using Inventor in a commercial
environment, you should consult your CAD manager
| | 01:35 | before you begin creating files.
| | 01:37 | Now that you know about the templates,
let's talk a little bit about the specific file
| | 01:41 | types that are available.
| | 01:43 | Files fall into four major categories: Part files,
Assembly files, Drawing files, and Presentation files.
| | 01:51 | At the top, you can see the Part files.
| | 01:54 | Within each category there's often slight
variations or multiple variations of a type of file.
| | 02:00 | In the Part environment you can see Standard.ipt,
the .ipt stands for Inventor Part file, and
| | 02:06 | when I select that you can see an image of
what can be created with this type of file.
| | 02:12 | In this case, Part files
represent single items in a design.
| | 02:16 | It could be a Lego brick, it could be
a pen cap, it could be an engine block.
| | 02:20 | The point is that it's a single
file that represents one item.
| | 02:24 | Sheet Metal parts have the same basic concept.
| | 02:27 | The difference is rather than standard
modeling features, Sheet Metal parts include features
| | 02:32 | that are specific to that type of modeling.
| | 02:35 | The ability to create bends
and flat patterns are an example.
| | 02:38 | Next, we have Assembly files.
| | 02:42 | The standard.assembly file is essentially a
container that contains multiple part files.
| | 02:48 | If you need to create a pen or an engine
block, you're going to first create the parts that
| | 02:53 | make up that model and then you're going
to connect them inside of an assembly file.
| | 02:59 | Similar to the Part files, there's
variations of Assembly files as well.
| | 03:02 | Weldments, for example, are very specific
types of assemblies that allow you to show
| | 03:07 | how parts are connected through welding.
Next, we have the Drawing files.
| | 03:12 | Drawing files come in a couple of
variations. The standard one is Standard.idw.
| | 03:18 | This is the default file
format for Inventor Drawings.
| | 03:22 | Drawings are going to be used to document your
parts and assemblies for manufacturing purposes.
| | 03:27 | The other option you have
within Drawings is in DWG file.
| | 03:31 | DWG files work in the exact same way as
an IDW, but they have a different standard.
| | 03:38 | DWG is the standard file format for AutoCAD.
| | 03:42 | Because Autodesk develops AutoCAD as well, we have
the ability to create native drawing files in Inventor.
| | 03:48 | If, for example, your company works with
partners and manufacturers that require DWG files you
| | 03:54 | can simply change settings in Inventor to
always use DWG as your file format, or you
| | 04:00 | can select it on your own
when you're creating a new file.
| | 04:04 | If you create an IDW you can still save a
file as a DWG, and it will create a native
| | 04:10 | DWG file as if it was written out of AutoCAD.
The final file type is a Presentation file.
| | 04:17 | Presentation files are representations of
assemblies, but rather than showing all the
| | 04:22 | parts attached to each other, Presentation
files allow you to disassemble the assembly
| | 04:27 | so people can have a better understanding
of how the parts are connected to each other.
| | 04:31 | In this course we're going to be
focusing on three major components:
| | 04:36 | Part files, Assembly files, and Drawing files.
| | 04:40 | Presentation files are
beyond the scope of this course.
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| Exploring essential settings| 00:00 | Before we get started with the course, I
wanted to go over a couple of settings that I use
| | 00:03 | during my design process that
may be helpful for you as well.
| | 00:07 | These settings are found under the
view tab in the Appearance panel.
| | 00:11 | Here you can find things like shadow, reflections,
and ground planes, and the two I want to focus
| | 00:15 | on are the shadows and orthographic projection.
| | 00:18 | I found that this model on the screen could
be a little clearer, and shadows help do that.
| | 00:25 | Based on the graphics card you have, you could
choose to turn All Shadows, but what I found
| | 00:30 | is in certain cases the most benefit you
get is by leaving just the Ambient Shadows on.
| | 00:36 | It adds a little more depth to the model and lets
you see how things interact a little more clearly.
| | 00:40 | The other option is Orthographic or Perspective view.
I prefer to use Perspective view.
| | 00:45 | Again, it adds another level of depth to the model
that adds a level of realism that helps with design.
| | 00:52 | Whether these are turned on or
not does not affect the design.
| | 00:54 | It's completely a personal preference.
| | 00:56 | I just wanted to make sure everybody understood the
settings that I have turned on and why I use them.
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2. Navigating the InterfaceNavigating using the ViewCube| 00:00 | Up to this point, we've learned about
Autodesk Inventor from a conceptual standpoint, and
| | 00:04 | now we're ready to begin
looking at the user interface.
| | 00:07 | The user interface is made up of a few
different components that you'll interact with while
| | 00:11 | you're building your models
and creating your designs.
| | 00:13 | First, you have the browser on the left, above
that you have the ribbon bar, above the ribbon
| | 00:18 | bar is the Quick Access toolbar, on the right-
hand side of the screen you have your navigation
| | 00:23 | tools, and finally you have your Graphics
window which is the gray window that the model
| | 00:27 | is actually being displayed in.
| | 00:30 | I'm going to go over the navigation tools
first, because I'll use those throughout this
| | 00:33 | section of the course to manipulate the
model and show how the interface changes, based
| | 00:37 | on what type of action is
taking place on the model itself.
| | 00:40 | We'll start with the view cube.
| | 00:43 | The view cube is simply a cube that has labels
that are linked to specific views of the model.
| | 00:49 | As I hover my mouse near the view cube, you'll notice
that it highlights and a Home button becomes available.
| | 00:55 | As I move away, those hide.
| | 00:57 | That's so that the view cube in navigation
tools are not really visible or active while
| | 01:02 | you're working on your design.
It's just to help keep things clean.
| | 01:05 | As I hover over my view cube, you'll notice
different sections of the view cube are highlighted.
| | 01:10 | By clicking on any of those sections, the view cube and
the model will both rotate to represent that orientation.
| | 01:17 | By simply returning to the view cube and clicking
the Home button, I return to a default Isometric view.
| | 01:23 | Now again, as I mentioned, you do have
different sections on the view cube that highlight.
| | 01:29 | By clicking on each of those, you'll very
quickly see how the model is connected to the view
| | 01:33 | cube and moves accordingly when
selecting different views on the view cube.
| | 01:37 | When we select the Front view, for example,
you'll also notice that several other tools pop up.
| | 01:42 | We have a couple different rotation arrows, and we
now have arrows around the view cube on every side.
| | 01:49 | By clicking on the rotation arrows, you can
rotate the model in 90-degree increments.
| | 01:55 | Simply clicking four times, and you'll
actually rotate 360 degrees in 90-degree increments.
| | 02:01 | The same happens with the other
rotation arrow, just in the opposite direction.
| | 02:05 | The arrows that are located around the view
cube work in a similar fashion, but rather
| | 02:09 | than maintaining the current orientation, they
simply rotate to the naked view on the view cube itself.
| | 02:15 | Again, selecting that several times, you'll
actually rotate back to where you started.
| | 02:21 | It works the same for both the top and
bottom and the right and left arrows.
| | 02:27 | Now you might look at this model and say
when you click on the left view this is actually
| | 02:32 | something that represents the front view rather
than the side view, and I would agree with that.
| | 02:37 | It's not very uncommon that you work with
other designers or other companies and receive
| | 02:41 | files that are in an orientation that doesn't quite
make sense for the work that you're going to be doing.
| | 02:46 | To change that, we have a
couple of different options.
| | 02:50 | First, if you view the model from the
orientation that you consider the front view, you can
| | 02:55 | right-click on the view cube to select Set
Current view as, and you have options for Top or Front.
| | 03:03 | In this case, I'm going to select Front, and
you'll notice now my view cube is representing
| | 03:08 | the Front view, and that is the
view that I am viewing on the screen.
| | 03:13 | When I click to my Home button again, you'll
see that I have Top, Front, and Right, rather
| | 03:18 | than Top, Left, and Front.
| | 03:20 | This makes sense to me, and I can change it
at any point during the design as I need to.
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| Navigating using the navigation tools| 00:00 | Next, we'll look at the
navigation tools themselves.
| | 00:03 | Just below the view cube you have a series
of commands that will pan, zoom, and orbit
| | 00:07 | the model that you're working on.
| | 00:09 | The first one in the list
is the Full Navigation Wheel.
| | 00:12 | We'll come back to that in a second after we go
through a couple of these commands, the Pan command.
| | 00:17 | Panning is simply like grabbing the
model and moving it around on the screen.
| | 00:21 | A simple left-click and drag will allow you to
move the model from side to side on the screen.
| | 00:26 | This is typically used in conjunction with
a Zoom function so that you can find exactly
| | 00:30 | the right position for viewing your
model based on the work you're doing.
| | 00:34 | Next, we have the Zoom command.
| | 00:36 | This command on the toolbar
is actually a split button.
| | 00:39 | You'll notice it has a top half with an
icon and the bottom half that has an arrow.
| | 00:44 | Based on where you are in your design
process, that button may be different.
| | 00:48 | If you've never used the button before,
it'll have whatever the default action was.
| | 00:52 | If you've used the command, it
will use your last known command.
| | 00:56 | I'm going to use the dropdown here and
select Zoom and show the basic zoom functionality.
| | 01:01 | With the Zoom command launched, you can
simply left-click on the screen and push away from
| | 01:06 | you to move the model away or pull back towards you
with a mouse to move the model closer to you or zoom in.
| | 01:13 | Now for those people who might be coming
from AutoCAD, this might seem very foreign.
| | 01:18 | In AutoCAD the Zoom functionality is reversed,
and before we move any further I wanted to
| | 01:23 | do a very quickly call out where the option
is to reverse that so that if you choose to
| | 01:27 | have your Zoom work like it has an AutoCAD
you can simply do that and move forward with
| | 01:32 | learning Inventor rather than
having to relearn how to zoom.
| | 01:36 | The Zoom setting can be found under the Application menu
by selecting Options and then selecting the Display tab.
| | 01:44 | In the 3D Navigation section at the bottom,
there's a Zoom Behavior option, and there
| | 01:49 | is a check box to reverse direction.
| | 01:51 | By checking this check box and applying the change,
you can reverse the direction to be more like AutoCAD.
| | 01:57 | In this case, I'm going to cancel because
I want to keep it the way it is, but if you
| | 02:01 | need to you can go ahead and
change that based on your preference.
| | 02:06 | You notice because I used the Zoom button
it is now the last active command, and you
| | 02:10 | can see that icon on the toolbar.
| | 02:13 | The other options are Zoom All,
Zoom Window, and Zoom Selected.
| | 02:16 | I'm going to go with Zoom Window first, and
this allows me to left-click and drag a window
| | 02:23 | on a specific portion of the model
and zoom directly to that location.
| | 02:28 | The Zoom All simply zooms out
so that you can see everything.
| | 02:33 | And finally, we have Zoom Selected. Zoom Selected
allows you to select a specific piece of geometry
| | 02:38 | and actually zoom just on that item.
The next option is Look at.
| | 02:46 | Look at allows you to look
directly at a specific face on the model.
| | 02:50 | At any point you can select Look at, you
can pick a face, and the object will look at a
| | 02:55 | normal view to that face on the model.
| | 03:00 | Now that we've gone through a few of the commands,
I'm going to circle back to the Full Navigation Wheel.
| | 03:04 | The navigation wheel brings all of these
components together into one piece of an interface.
| | 03:09 | You have the Zoom functionality, you have
Orbit, and you have Pan all in one command item.
| | 03:18 | The other item that I wanted to call out here that comes
in handy from time to time is the Rewind functionality.
| | 03:24 | As I've been going through showing these
items, I've been moving and rotating the model.
| | 03:28 | If you click on the Rewind option, you'll
notice that Inventor has saved these views for you
| | 03:33 | so that if you found a specific view that
you like and you need to return to it, you
| | 03:37 | can use the Rewind tool to go back in time
essentially to find that one piece of geometry
| | 03:42 | that you were working with that was important.
| | 03:47 | Having gone through all the navigation tools, I think
it's important to call the fact that I rarely use them.
| | 03:52 | The reason for that is you can do all the
navigation commands from your mouse by itself
| | 03:57 | or in combination with the keyboard.
| | 04:00 | The zoom can be done by simply moving your
wheel mouse in and out, and it corresponds
| | 04:05 | to the same settings that
you have in your options.
| | 04:08 | If, for example, you swapped because you're an
AutoCAD user, that will affect the mouse scrolling as well.
| | 04:13 | The other option is Pan.
| | 04:15 | By clicking my middle mouse button, I
can get the into the Pan operation.
| | 04:19 | Finally, to get a free orbit, I can hold Shift
on my keyboard and do the middle mouse button
| | 04:24 | similar to the way I would
with pan, and I get a free orbit.
| | 04:29 | Between these shortcut keys and the mouse
combinations, you can get all your navigation
| | 04:33 | done through the mouse itself.
| | 04:36 | I do use the navigation toolbar, but I
actually customize it a little bit because there's
| | 04:41 | a couple of commands that come in very handy,
and these are commands I talked about in an
| | 04:44 | earlier video that affect some
of the settings I use frequently.
| | 04:49 | The arrow at the bottom of the navigation
bar brings up a list of tools that you might
| | 04:52 | want to have readily
available on the navigation bar.
| | 04:56 | The ones that I want to call out
are Projection and view Styles.
| | 05:02 | These are two items I called out in the
Settings video that I switch back and forth between
| | 05:07 | on a regular basis during my design process.
| | 05:10 | I can either switch from Orthographic to
Projected view, or I can change the style of the model.
| | 05:16 | Perhaps I want to see this
model shaded with hedges turned on.
| | 05:20 | I might even want to see an artistic
view of this model, maybe in a watercolor.
| | 05:26 | You'll notice that as I change these
visual styles, those are applied to the model, and
| | 05:30 | navigation happens as it normally
would, just with a different view style.
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| Using the browser| 00:00 | The next user interface component
we want to talk about is the browser.
| | 00:04 | The browser is essentially a lens into
what is being shown on this graphic screen.
| | 00:09 | In this case, we are looking at an engine
assembly, and we can tell that from within
| | 00:12 | the browser we have Engine.iam
listed at the top of the tree.
| | 00:17 | Below that, we have things that are
specific to this assembly, things like the parts.
| | 00:21 | This Engine Block, for example, you'll
notice as I highlight it in the browser, it also
| | 00:25 | highlights in the graphics window.
This is a bi-directional link.
| | 00:29 | If I select on something like this Heat Sink, you'll
notice that it highlights down here in the browser.
| | 00:34 | This is a nice way to be able to
find components within the assembly.
| | 00:37 | You notice that not all items are visible,
some are hidden deep within the assembly.
| | 00:42 | For example, the Piston Shaft is actually hidden
inside of the assembly, inside the Engine Block.
| | 00:48 | But as we hover down this list, you
can see certain items highlighting.
| | 00:53 | It's important to understand that the
browser is connected to the graphic screen, because
| | 00:57 | in certain cases, I might need to
interrogate my model a little more closely.
| | 01:01 | For example, let's say we needed to
see how the piston works in this model.
| | 01:10 | We can select things in the graphics window and hide
them so that we can interrogate things inside the model.
| | 01:15 | In this case, we can see that the
piston works, but we have a problem now.
| | 01:19 | On the screen, we don't see those parts.
| | 01:21 | If we want to turn them back on, we actually have to use
the browser in conjunction with the graphics window.
| | 01:27 | Here you can see in the browser the things
we made hidden or not visible have now become
| | 01:31 | grayed out, and we can right-click on them
and select Visibility to bring them back to
| | 01:37 | visibility in the graphics window.
| | 01:39 | So once you've hidden something in the graphics
window, you are going to need to use the browser
| | 01:42 | to actually return that to its original state.
| | 01:49 | Now, as I mentioned, here we are looking at an
assembly, so we've got things like Parts and Assemblies
| | 01:56 | and even if you expand the Engine Block, for
example, you can see the constraints or the
| | 02:00 | rules that tell this model how
they're assembled, or how they're connected.
| | 02:07 | The browser is very context-sensitive to
what is being shown on the screen because it's
| | 02:11 | actually a representation of the same thing.
| | 02:14 | For example, if I actually double-click on
any part in this model, what's happened here
| | 02:20 | is I've begun editing a part.
| | 02:22 | When I did that, the
browser changed significantly.
| | 02:25 | I'm still viewing the Assembly.iam file,
| | 02:28 | but you'll notice that the Engine Block is
now highlighted, and it's got a focus to it.
| | 02:33 | If I expand that, it's as if I've opened
this part on its own, but now I see the Engine
| | 02:39 | Block listed, and instead of other parts, I
actually see features that make this component on.
| | 02:45 | I see Extrusions, I see Work Planes, I see
Lofts, I even see Mirrors, Holes, and Fillets,
| | 02:51 | these are all the modeling operations
that we'll learn about later in this course.
| | 02:55 | But it's important to show that the browser
is a direct link to that which is being shown
| | 02:59 | on the graphic screen.
| | 03:01 | To return to the Assembly, I simply click
the Return button, which is like going up a
| | 03:06 | level back to the Assembly, and now I am
returned to seeing parts in assemblies.
| | 03:11 | So, the system will automatically adjust based
on what types of things and actions you are doing.
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| Using the ribbon bar| 00:00 | Now that we have an understanding of the
navigation tools and browser, we can look at the Ribbon bar.
| | 00:05 | For those who have used the Microsoft
Office applications, the Ribbon bar should become
| | 00:09 | immediately familiar to you.
| | 00:11 | You may also recognize it if you've used
AutoCAD or Revit because like the navigation tools,
| | 00:15 | they're part of a common interface.
| | 00:18 | This may help you become more familiar as
you switch between applications as well.
| | 00:22 | Like the browser, the Ribbon
bar is very context-sensitive.
| | 00:25 | Right now, we're looking at an
assembly, therefore we see the Assemble tab.
| | 00:30 | But if we were to switch and view a part file
by double-clicking on an item in the graphics
| | 00:36 | window, you'll notice that the Assemble tab
becomes invisible or is removed from the Ribbon
| | 00:42 | bar, and it's replaced with tools that
are more likely to be used in part modeling.
| | 00:47 | In this case, we've been moved to the 3D
Model tab, and we have things like Extrude and
| | 00:52 | Revolve and features that
we'll cover later in the course.
| | 00:56 | Like the Microsoft Office applications,
there are certain times when the Ribbon bar will
| | 01:01 | present new tabs based on the actions
you're taking in the application itself.
| | 01:06 | For example, in the part modeling environment,
if we were to create a new sketch, you'll
| | 01:13 | notice that a new tab is presented.
| | 01:15 | It's highlighted in green to indicate it that
it is a temporary tab and will only be visible
| | 01:19 | when you're doing a specific
action related to sketching.
| | 01:21 | It will automatically be turned off
by the system when we are finished.
| | 01:25 | If I were to hit Finish Sketch, you'll
notice that the tab is removed and replaced back
| | 01:31 | into the part modeling environment.
| | 01:33 | I am going to use the Undo button on the Quick
Access Toolbar to remove that sketch from the model.
| | 01:38 | We don't really need it in this case, and I am
going to go ahead and return to the Assembly.
| | 01:43 | Within an each of these tabs that you see on
the screen, tools are gathered in an organized
| | 01:48 | fashion within panels on each of the tabs.
| | 01:51 | In the Assemble tab, you have the Component panel,
Position panel, iParts and Assemblies, things like that.
| | 01:58 | Under the Inspection tab, we have Interference
and Measure, things you might use to inspect.
| | 02:03 | So just like the Office applications, the
tools are both gathered by tab and are gathered
| | 02:07 | with similar tools within that panel.
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| Using the Quick Access Toolbar| 00:00 | Now that you have an understanding of the
Ribbon bar, I want to talk a little bit about
| | 00:03 | the Quick Access Toolbar.
| | 00:05 | It's a simple toolbar that can be very
useful as you begin your design process.
| | 00:10 | It's located directly above the
Ribbon bar in the Application Title bar.
| | 00:14 | What used to be blue empty title bar space
now has useful tools in it, and it can be
| | 00:18 | very handy as you become more
proficient with the product.
| | 00:22 | The one unique thing about the Quick
Access Toolbar is it's taking tools that are not
| | 00:26 | specific to a tab, whether it's the
Assemble tab, or the 3D Model tab.
| | 00:30 | Here, we are storing application items like
the Application menu, the File > New button,
| | 00:37 | the Open or Save button, and the Undo and Redo.
| | 00:40 | But we go beyond that and even put the materials
and appearance options on the Quick Access Toolbar.
| | 00:46 | The other nice thing about the Quick Access
Toolbar is as you become more familiar with
| | 00:50 | the features of the product and commands in
the product, you can actually customize that,
| | 00:54 | which we'll cover in another movie.
| | 00:56 | But the nice thing is because the tabs don't
switch, you can easily place commands there,
| | 00:59 | and get to them as needed without
having to switch tabs frequently.
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| Customizing the toolbars| 00:00 | Now that we have an understanding of the
Ribbon bar and Quick Access Toolbar, I want to talk
| | 00:04 | a little bit about how to customize those items.
| | 00:06 | Now, I wouldn't recommend going in and
customizing everything right out of the gate. I think
| | 00:11 | it's important that you understand what the
tools are, where they are located, and use
| | 00:15 | them for a bit before you make a decision
to actually start customizing the interface.
| | 00:20 | The last thing you want to do is, by mistake,
think that you're not going to use a feature,
| | 00:25 | customize the interface, and
forget that, that feature even exists.
| | 00:27 | What I am going to do is begin editing a part,
because I think there's a specific location
| | 00:33 | in the part editing environment that is a
valid place where you might want to make a
| | 00:36 | change to the interface.
| | 00:39 | On the 3D Model tab, you'll notice different panels,
Sketch, Primitives, Create, and Modify, for example.
| | 00:45 | You'll notice that the Create and Modify panels
both have a small dropdown arrow next to the label.
| | 00:51 | This indicates that there are other
commands that are similar to the ones in that panel
| | 00:55 | that are just being hidden from the interface,
and the Create panel is a good example of this.
| | 01:00 | Say, for example, my company--while we do
use Extrude, Revolve, and Loft--perhaps we
| | 01:05 | don't emboss things on our parts.
Instead, we make decals.
| | 01:10 | By default, the Decal command is actually
hidden in the Expanded panel, but it might
| | 01:14 | make more sense in my design
environment to swap those two items around.
| | 01:19 | To do this, we can simply right-click on any
command, and select Move to Expanded panel.
| | 01:26 | And now you can see under the Create panel,
we have Decal and Emboss both located in
| | 01:30 | the Expanded panel.
| | 01:31 | I'm going to right-click on Decal, and
select Move to Main panel, and I have essentially
| | 01:36 | swapped those commands.
| | 01:38 | While it might not seem like a major thing,
if you've never used the Emboss command, you're
| | 01:42 | going to find that it
speeds your design process.
| | 01:45 | Similar to the Ribbon bar, the Quick Access
Toolbar is an excellent place to put commands
| | 01:49 | that you use frequently.
| | 01:51 | For example, when I'm editing parts, I often
want to view the work planes, and work features
| | 01:58 | that have been created for this part.
| | 02:00 | I can get to those from the view tab under the
Visibility panel by selecting Object Visibility,
| | 02:06 | and I can turn on all my work features.
| | 02:08 | And while that might seem scary, that's
part of the reason I am bringing this up.
| | 02:11 | There are certain places where I want to
see these work features and other places where
| | 02:15 | I don't, so I often want to turn
them on and off on a regular basis.
| | 02:21 | Because of this, I actually put my Object
Visibility command on my Quick Access Toolbar
| | 02:26 | by right-clicking on it and
selecting Add to Quick Access Toolbar.
| | 02:30 | Now, you'll notice when I return to the 3D
Model tab, the Object Visibility functionality
| | 02:36 | remains on my Quick Access Toolbar,
and it works in the exact same fashion.
| | 02:40 | Now, when I return to my Assembly environment,
I have a similar issue, the same as I mentioned.
| | 02:47 | I use work features in both my part
modeling and my assembly modeling environment.
| | 02:51 | So I could also make this change in
the Assembly modeling environment as well.
| | 02:55 | I can select Add to Quick Access Toolbar to
place the command on the Quick Access Toolbar
| | 03:00 | in the Assembly environment as well.
| | 03:02 | This makes it a lot easier to access
commands that I use on a regular basis.
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| Using the Marking menu| 00:00 | The last interface component that I want to talk
about is the Graphics Window and the Marking menu.
| | 00:04 | Now you saw a glimpse into the Graphics
Window when we were talking about the browser.
| | 00:08 | It's essentially the gray area of the main
component on the screen where your models
| | 00:11 | and drawings are shown.
| | 00:13 | The Marking menu is essentially a
component of the Graphics Window.
| | 00:17 | By right-clicking anywhere in the Graphics
Window, you can bring up the Marking menu.
| | 00:21 | The Marking menu is essentially just
our right-click menu, but with a twist.
| | 00:26 | Rather than just listing commands like
you'd see in a traditional right-click menu, in
| | 00:30 | Autodesk Inventor, it's very context-sensitive.
| | 00:33 | The most common commands are gathered in a
circular pattern around the top of the right-click menu.
| | 00:39 | It's important to remember that the
Marking menu is very context-sensitive.
| | 00:44 | Very much like the Ribbon bar and browser, it
will change based on the environment you're in.
| | 00:48 | In this case, we are in an Assembly file,
so you see things like Create New Component,
| | 00:52 | Place Component, Constrain, things that you
would use commonly in the Assembly environment.
| | 00:58 | If I double-click and begin adding a part
and right-click again, now you see things
| | 01:03 | like Fillet, Extrude, Revolve modeling actions
that we'll learn more about in a later movie.
| | 01:11 | Again, even further, this continues
on into things like temporary tabs.
| | 01:18 | In our sketch environment which we talked
about in the Ribbon movie, you'll notice that
| | 01:23 | we have a temporary tab and here's
where I use the Marking menu the most.
| | 01:27 | You'll notice, as I move around the Marking
menu at the top, a highlighting action takes place.
| | 01:34 | Once I find an item is highlighted, I can
left-click on it to launch that command, and
| | 01:39 | now I'm able to create rectangles.
| | 01:41 | The important thing about the Marking menu
beyond just where things are located is understanding
| | 01:46 | how you can access this menu.
| | 01:48 | While so far I've right-clicked and simply
selected an item from this list, that doesn't
| | 01:53 | really improve things too
dramatically over a standard right-click menu.
| | 01:58 | Where things become useful is once you
understand where these items are located within this
| | 02:02 | pattern, you can launch the command by
using a right-click drag action without actually
| | 02:08 | having to launch the command.
| | 02:10 | So, if I want to create a line, for example,
which is straight to the top of this pattern,
| | 02:15 | I can right-click and drag my mouse up, and
release my right-mouse button to launch the Line command.
| | 02:22 | If I right-click, and hit Cancel,
I can then launch another command.
| | 02:27 | I know that, in this case, a 2-point
rectangle is up and to the right.
| | 02:32 | I am going to hit Escape to get out of the
Marking menu, and now I can right-click and
| | 02:36 | drag up into the right, and
launch the Rectangle command.
| | 02:39 | So, for those commonly used commands that
you access on a regular basis--once you get
| | 02:45 | the hang of where they are in the Marking
menu--it's going to save you a significant
| | 02:49 | amount of time. Rather than returning
always to the toolbar, you will be able to launch
| | 02:53 | these commands from the right-click menu or
possibly not even bring up the menu in the first place.
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|
|
3. SketchingIntroducing sketching| 00:00 | Now that you have an understanding of the
interface, it's time to begin working on the
| | 00:03 | first step in building a
3D model, that is sketching.
| | 00:07 | Sketching is the foundation
of all modeling in Inventor.
| | 00:10 | At the most basic level, if you can sketch
a rectangle then you can build a 3D part.
| | 00:14 | Perhaps, it won't be the most
interesting part, but it is a part nonetheless.
| | 00:18 | Within a sketch you build intelligence into
the model by adding dimensions, constraints,
| | 00:22 | and formulas to define how
the part can change over time.
| | 00:26 | The best way for you to
understand this is for me to show you.
| | 00:29 | I'm going to create a New Part File and
walk through a few basic steps of taking 2D geometry and
| | 00:35 | creating 3D features or parts out of that.
| | 00:38 | It's not important that you
understand each of these steps.
| | 00:41 | Only that you understand the
connection between sketching and part modeling.
| | 00:44 | We'll get into the details of each of
those as we move forward in the course.
| | 00:48 | I'm going to begin by sketching a
basic rectangle and extruding that.
| | 00:53 | This should give you at least an initial
feel for what 2D shapes turn into when you apply
| | 00:59 | a 3D modeling action to them.
| | 01:01 | In this case, I'm going to go ahead and extrude,
and this rectangle can become a cube.
| | 01:08 | Next what I'm going to do is I'm going to
create a new sketch, and this time I'm going
| | 01:12 | to sketch a simple circle.
| | 01:18 | When I finish my sketch, I can now apply a
modeling action to it to create a 3D shape.
| | 01:25 | When applying the modeling action, I do
have the ability to add material like I'm doing
| | 01:28 | in this case, or I can always go back and
Edit--or choose to do this in the first place--
| | 01:35 | and change things to a Cut to
remove material from this model.
| | 01:41 | So the shape can either be
a positive or a negative.
| | 01:46 | And it's your choice as a designer to
determine which makes most sense in your design.
| | 01:52 | I'm going to go ahead and create another part
to show a little bit more advanced functionality.
| | 01:59 | This time I'm going to combine
the two items that I just created.
| | 02:02 | I'm going to go ahead and create a rectangle,
but I'm also going to combine that with the circle.
| | 02:11 | Now the size doesn't matter right now,
we'll get into those details later.
| | 02:15 | But what's important here is I can combine
multiple sketch profiles in order to create that 3D shape.
| | 02:22 | Here I can select a rectangle and the
circle to get a new more complex 3D shape.
| | 02:29 | Now it's also important to understand that it's
not just extrusions that we're going to be doing.
| | 02:34 | If I undo that extrusion, the same shape that I drew
to extrude, I could apply a revolve action to that.
| | 02:41 | It's a similar function where I select what
profiles are going to be used, but in this
| | 02:45 | case the modeling action
allows me to select an axis.
| | 02:49 | With this axis selected, you can see that I
get a very, very different shape from just
| | 02:54 | adding extrude to that.
| | 02:58 | Based on this, you should have a basic understanding
of the connection between sketching and part modeling.
| | 03:03 | The shapes you sketch become 3D features.
| | 03:06 | That can then add and remove material
to define what your part looks like.
| | 03:11 | Not only can you sketch different shapes,
but you can apply different modeling actions
| | 03:15 | to those shapes to meet your design needs.
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| Working with origin geometry| 00:01 | In this video we're going to
focus on the origin geometry.
| | 00:04 | In the previous video, you watch me create a
few basic features, and you may have noticed
| | 00:08 | the Origin planes being used to start each part.
| | 00:11 | The Origin is essentially the center of
the universe within any part or assembly.
| | 00:16 | And while it's called the Origin, it's
actually made up of three planes and three axes that
| | 00:20 | all intersect at a center point.
| | 00:22 | I'm going to start a blank part file so that
we can better understand the origin geometry.
| | 00:27 | When creating a new part, the very first
feature is always going to be a sketched feature.
| | 00:32 | And in order to create that
sketch you need a flat surface.
| | 00:35 | But in a brand-new part file, there are no
flat surfaces and the origin geometry provides
| | 00:40 | that drawing surface.
| | 00:42 | The Origin can be found in the browser
under the Origin folder, and when you expand it,
| | 00:47 | you can actually see the three planes and three
axes, and the Center Point that make up the Origin.
| | 00:53 | Now by default the origin
geometry is not visible.
| | 00:56 | I'm going to rotate into a home view isometric
and make those visible so that you can better
| | 01:01 | understand where they are and how they work.
| | 01:04 | To turn on the visibility of a plane or an
axis, or any of the origin geometry, simply
| | 01:09 | right-click on it in the
browser and select Visibility.
| | 01:12 | You can also use standard Windows selection
convention, such as selecting an item further
| | 01:17 | down the list to gather a group of items.
| | 01:20 | But once they're selected, you can right-click
and select Visibility to enable them all at once.
| | 01:26 | Now as I rotate, I think you'll get a
better view of how these planes interact.
| | 01:31 | If I hover over one of the planes in the browser,
you'll see it highlight in the graphics window
| | 01:35 | just like you would in any other
part or assembly within Inventor.
| | 01:39 | Again, the browser is linked to
what you see in the graphics window.
| | 01:43 | As I hover down, you can see the XZ Plane
is now highlighted, and here's the XY Plane.
| | 01:48 | The axes are actually the
intersection between two of the Origin planes.
| | 01:52 | The X-axis, for example, is the
intersection of the XY Plane and the XZ Plane.
| | 01:59 | The Y-axis is an intersection
of the XY Plane and the YZ Plane.
| | 02:04 | Now that we know what the origin geometry is,
| | 02:07 | I'm going to go ahead and turn it off--or
make it not visible again--by selecting each of
| | 02:12 | the items and unchecking
Visibility from the right-click menu.
| | 02:16 | The reason I'm doing this is because in
Autodesk Inventor 2013, a new feature was added that
| | 02:22 | makes it less important to turn on and
off the visibility of the origin geometry.
| | 02:27 | When you're creating a sketch, the system now
temporarily makes visible the origin geometry
| | 02:33 | so that you can select your sketching plane,
and it will automatically hide those items--
| | 02:38 | or return them to their hidden state--
after you've made your selection.
| | 02:42 | So here I'm in the Create Sketch command.
| | 02:44 | You'll notice in the browser that these
items are visible, they're highlighted, they have
| | 02:49 | color to them, and I can simply select one of
the planes in the window to create my first sketch.
| | 02:55 | And you'll notice that the origin geometry in
the browser has been returned to its hidden state.
| | 03:00 | Now I'm going to go ahead and create a rectangle and
extrude that to show you how to move forward from here.
| | 03:10 | You'll notice, again, in the browser
the origin geometry is all hidden.
| | 03:14 | I can go ahead and collapse that, because
after I've created my base feature, my first
| | 03:19 | feature of my part, from that point forward
any new sketch will actually use a face on
| | 03:25 | the model to continue the sketching process.
| | 03:28 | Here we'll go ahead and create a circle that's
similar to what we did in the previous video.
| | 03:32 | I'll finish my sketch, and I can extrude that.
| | 03:36 | But for this feature, I've
not used the origin geometry.
| | 03:39 | Instead, I've used a face off of one of the
previous features I've created, and that process
| | 03:44 | will continue as we move
forward with part modeling.
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| Understanding constraints| 00:00 | In this movie we want to
focus on Sketch Constraints.
| | 00:03 | As we move closer to sketching, it's
important to understand what constraints are and how
| | 00:08 | they help build intelligence into your
sketches, and in turn, your parts and assemblies.
| | 00:13 | It's important because Inventor will
automatically apply constraints during the sketching process.
| | 00:17 | And if you don't know what constraints are,
you could easily become confused or frustrated.
| | 00:22 | A constraint by definition is something that
confines or restricts within prescribed bounds.
| | 00:28 | What that means is constraints are
essentially rules that tell sketch geometry how it can
| | 00:33 | and can't move, how big it can be, or how it is
to react in relation to other sketch geometry.
| | 00:40 | In Inventor sketch constraints come in
two flavors, Dimensional and Geometric.
| | 00:45 | Dimensional constraints are just that,
dimensions that tell a piece of geometry exactly how
| | 00:49 | big it needs to be, and we'll
cover dimensions in a later movie.
| | 00:53 | In this movie we'll focus
on Geometric constraints.
| | 00:55 | I've created a simple practice file that
will help you quickly understand how geometric
| | 00:59 | constraints are used to control sketch geometry.
To begin we need to edit the sketch.
| | 01:05 | You can do that in a few different ways, and
I'm going to walk you through each of those,
| | 01:08 | because depending on the scenario you may
need to use one or the other--you'll learn
| | 01:13 | that over time--but at least I want to make
sure you understand each of those options.
| | 01:17 | The first option and the one I use the most,
is selecting sketch geometry on the graphic
| | 01:22 | screen and using the Heads-up
display to edit the sketch.
| | 01:27 | That will rotate you into a normal view to the
sketch, and you can begin the editing process.
| | 01:31 | I'm going to finish this sketch and
show you a couple of other ways to do it.
| | 01:36 | Another way would be finding that sketch in
the browser, right-clicking on it, and selecting
| | 01:41 | Edit Sketch from the right-click menu.
| | 01:44 | That also rotates you into a normal view
and prepares you for editing the sketch.
| | 01:49 | The final way, which is also a very common way,
is to double-click the Sketch icon in the browser.
| | 01:56 | By doing that you activate the sketch
environment, and you're ready to edit the sketch again.
| | 02:01 | Normally I would not say that you have to
look at sketch constraints when you begin
| | 02:06 | editing a sketch, in most cases you're
going to be the one creating the sketch, in that
| | 02:09 | case you already know what
constraints have been applied.
| | 02:12 | In the case where you're getting a file
from somebody else or an exercise file for this
| | 02:16 | course, it's important that you look at what
constraints have already been applied so that
| | 02:21 | you don't try to duplicate that after.
| | 02:24 | To view the constraints that have been applied,
make sure nothing is selected in the graphics
| | 02:28 | window by hitting Escape on your keyboard.
| | 02:31 | This will make sure nothing is selected, that
way when you right-click you have a specific
| | 02:35 | context menu that allows
you to show all constraints.
| | 02:40 | Now when I do that a bunch of stuff happens.
| | 02:42 | Well, in this case it really is just
showing me the constraints that are here, which is
| | 02:46 | what it's supposed to do.
| | 02:47 | But in this case at this point we've only
applied fixed constraints, and these are constraints
| | 02:52 | I applied in order to make this
file work the way it's supposed to.
| | 02:56 | So, because we're not very interested in those lock
constraints we're going to temporarily hide those.
| | 03:01 | I'm going to right-click in the Graphics
window and select Constraint Visibility.
| | 03:06 | This will bring up the list of all the
constraints and allow you to temporarily disable some
| | 03:11 | of the viewing of those items.
| | 03:13 | Now it's important to remember, after you
apply this, that you've turned it off. When you're
| | 03:18 | done, if you think you're going to need
that moving forward, turn it back on.
| | 03:22 | I've seen many cases where people said that
their constraints aren't working come to find
| | 03:26 | out that they have really just turn off the
visibility. So it's important that you remember
| | 03:30 | that Constraint Visibility is available from
the right-click menu in the Sketch environment.
| | 03:36 | The next item I wanted to show, which is very
helpful to those who new to Inventor, is the
| | 03:41 | option for Show All Degrees of Freedom.
| | 03:44 | This shows you what degrees of freedom are
available to any piece of sketch geometry
| | 03:48 | based on the constraints
that have been applied already.
| | 03:52 | In this case, no constraints have been applied.
| | 03:54 | We've hidden the fixed constraint, but
the geometry that's been created doesn't have
| | 03:58 | any constraints at this point.
| | 04:00 | We're going to begin by adding a
horizontal constraint to the first item here.
| | 04:06 | We're going to go to the Sketch tab, under the
Constrain panel, and select the Horizontal constraint.
| | 04:12 | Now when you hover over an item in the
Ribbon bar you will get an option that shows you
| | 04:17 | tool tips. These tool tips are little more advance
than what you might get in a typical application.
| | 04:23 | When I hover over and pause for a moment I
get an initial description of that item, and
| | 04:29 | if I pause a little bit longer I get a full
description and in some cases even video of
| | 04:34 | how to apply these items.
| | 04:38 | Once you've launched the command you can simply
click on a piece of geometry to apply that constraint.
| | 04:44 | You'll notice that the sketch geometry is
now horizontal, and it's also changed color.
| | 04:49 | The color is important here,
because it's providing information.
| | 04:53 | It's telling you that this item is fully
constrained from a geometric standpoint.
| | 04:58 | The arrows that remain are actually telling you that
a dimension is required to provide an overall size.
| | 05:03 | I am going to get out of this command
by right-clicking and selecting Cancel.
| | 05:08 | You could also do this by hitting Escape on
your keyboard, and I'm going to right-click
| | 05:12 | again to add a Dimension.
| | 05:13 | Now we're not going to get into the details
of dimension, but I'm going to apply one simply
| | 05:17 | to show you what happens
when it's fully constrained.
| | 05:20 | In this case, all of the degrees of freedom
are removed, and if I returned to my right-click
| | 05:26 | menu and get out of my Dimension command, I
can then right-click again and select Show
| | 05:30 | All Constraints one more time, and you can see
that the horizontal constraint has been applied.
| | 05:37 | By hovering over that icon you can also see
the geometry highlight which tells you what
| | 05:42 | pieces of geometry are
included with this constraint.
| | 05:46 | To continue, I'm going to go ahead and hide
all my degrees of freedom, and I'm going to
| | 05:52 | Hide all my constraints.
This will help just clean up the interface.
| | 05:57 | We can move forward, and we'll circle back and look
at the constraints once we've applied to each of them.
| | 06:01 | As we continue forward the next
constraint is a Vertical constraint.
| | 06:05 | Again, we're not going to touch all the
constraints, but the key constraints that are most used
| | 06:10 | in design are going to be covered.
| | 06:11 | I am going to select the Vertical constraint
from the Constrain panel and then select the
| | 06:15 | line to apply the vertical constraint.
| | 06:18 | You'll notice again the color changes and at
this point I'm ready to move to my next constraint.
| | 06:23 | I could hit Escape to get out of
this command, but that's not required.
| | 06:27 | Next I can actually move to the Collinear
constraint which is here on the top of the
| | 06:31 | Constrain toolbar, and that will automatically
cancel the Vertical constraint and begin the next command.
| | 06:38 | In this command rather than selecting a single
line, you need to pick two pieces of geometry.
| | 06:43 | One item to start with and a second
item that you want to make collinear.
| | 06:48 | This will put the two pieces of
geometry in line with each other.
| | 06:51 | The next constraint is a Concentric constraint.
| | 06:54 | By selecting each of the circles you have
the ability to lock the center points so that
| | 06:59 | they will always remain connected.
The next constraint is the Tangent constraint.
| | 07:05 | By selecting the circle and then the line
you'll add a rule that make sure that line
| | 07:10 | will always remain tangent to that circle.
| | 07:13 | And the final constraint is
the Perpendicular constraint.
| | 07:16 | If we want these two lines to be perfectly
perpendicular--or 90 degrees from each other--
| | 07:21 | I simply select each of these lines while
in the Perpendicular constraint command, and
| | 07:26 | you can see that those two items
are now locked at a 90 degree angle.
| | 07:29 | I am going to hit Escape on my keyboard to
get out of the Constrain command, and we will
| | 07:34 | right-click in the Graphics window and
select Show All Constraints again, and now you can
| | 07:39 | see the constraints that we've
applied to these pieces of geometry.
| | 07:43 | Again, hovering over any of these items
will allow you to see which pieces of geometry
| | 07:48 | are included in the constraint.
| | 07:51 | In this case, in the tangent you see both the
circle and the line highlight, in the collinear
| | 07:55 | constraint both lines highlight.
| | 07:57 | Now the reason that's important is perhaps I
added this collinear constraint by mistake,
| | 08:02 | or it's no longer needed, it's very
simple to remove constraints as well.
| | 08:06 | When I hover over either of these items, it shows
me the geometry that's contained in this constraint.
| | 08:12 | I can left-click to select the constraint--
indicated by the highlighting in red--and then
| | 08:17 | I can right-click and select
Delete from the Marking menu.
| | 08:20 | You'll notice that the colors change to
represent that this item is no longer fully constrained,
| | 08:25 | and I could apply some
other constraint if I chose to.
| | 08:28 | Hopefully at this point you have a solid
understanding of what constraints are and how they work
| | 08:33 | to control geometry in a sketch.
| | 08:36 | We'll cover constraints a little bit more
in each of the following sketch movies, but
| | 08:39 | it's important that you have a
solid understanding from this point.
| | Collapse this transcript |
| Drawing with the Line tool| 00:00 | In this movie, we're going to focus on
drawing with the Line tool. And the time is finally
| | 00:04 | come to begin creating
sketches that will turn into 3D parts.
| | 00:08 | We'll pull together all the things we've learned
up to this point to begin creating our first part.
| | 00:13 | We'll start by creating
the starter mounting plate.
| | 00:15 | I have the assembly of the engine opened
so that we can get a feel for the part we're
| | 00:19 | going to be creating.
| | 00:21 | In this case, it's located right here on
the back of the engine and attached to it is the
| | 00:26 | starter cover, which covers the
mechanism that will be used to start the engine.
| | 00:31 | To get a better look at this part I'm going
to right-click on it and select Open so that
| | 00:35 | it appears in its own window as
if I've opened part file by itself.
| | 00:40 | This should allow us to see a basic overview
of what this part looks like and the components
| | 00:45 | that we're going to begin sketching.
| | 00:48 | Now in this case, the most important part is the base,
the large rectangle that everything attaches to.
| | 00:55 | Whenever I'm creating parts I like to try
to start with the most significant piece of
| | 00:59 | the geometry and build from that.
| | 01:02 | To begin, I'm going to start a new sketch
file, I'm going to go ahead and close these
| | 01:05 | part files and the assembly file,
because we don't need them to move forward.
| | 01:10 | From the Ribbon bar I'll click
New and select Standard part.
| | 01:15 | With an empty file we need somewhere to
sketch from, and you can remember from the origin
| | 01:19 | video that when creating a sketch Inventor
will present the origin geometry and allow
| | 01:24 | you to select a plane to sketch on.
| | 01:26 | In this case, I like sketching my base
features on the X, Y plane, so I'm going to left-click
| | 01:31 | on that and the sketch will become enabled,
and I'm ready to begin sketching my first part.
| | 01:36 | Now reality is this is about the Line tool,
but more than the Line tool we'll be talking
| | 01:41 | about the heads-up display.
| | 01:43 | I mean creating a line is as simple as left-clicking
once and left-clicking again to create a line,
| | 01:50 | that's not so much important.
| | 01:51 | What's important here along with creating the
line is the heads-up display, the constraints
| | 01:56 | that are being applied, and how to
add dimensions on the fly as needed.
| | 02:01 | So to begin I'm going to right-click to bring up
the marking menu, and I'm going to select Create Line.
| | 02:07 | When I do that the heads-up display appears
and shows me the coordinates of where my cursor
| | 02:12 | is located in relation to the center
point which was projected to this sketch.
| | 02:17 | As I move closer to the center point, you'll
notice that my coordinates began to approach zero.
| | 02:23 | When I get to the center point the icon or
cursor will snap to the center point, a green
| | 02:29 | dot will indicate that a coincident
constraint is going to be created, and you'll notice
| | 02:33 | that the coordinates are at 0, 0.
This is a good practice.
| | 02:37 | I'm going to go ahead and left-click to start
this from the center point and locking sketch
| | 02:41 | geometry to this center point
is a good habit to get into.
| | 02:46 | The reason for that is once you've locked
to the center point, the remaining sketch
| | 02:50 | geometry that's created
is much more predictable.
| | 02:53 | As you add dimensions and constraints you
know where things are going to grow from,
| | 02:58 | and that's the center point you lock to.
| | 03:00 | Now that I have selected the starting point,
the heads-up display changes and gives me
| | 03:04 | some good information about what's next.
| | 03:07 | Not only am I selecting the last end point of this
line, but you'll notice the dimensions have appeared.
| | 03:13 | I have a length
dimension and an angle dimension.
| | 03:16 | You'll notice that the length dimension is
highlighted in blue as if it's ready for text input.
| | 03:21 | I know that this part is 1.575 inches square,
so I'm going to type that on my keyboard,
| | 03:27 | and you'll notice those are
input into the dialog box.
| | 03:31 | If I hit tab on my keyboard
a couple of things happen.
| | 03:35 | First I switched to the angle constraint
where I could type in a dimension value for that,
| | 03:39 | but more importantly the 1.575 length
dimension has received a Lock icon next to it.
| | 03:46 | This indicates that I have manually input
some value there. And as I move my cursor,
| | 03:51 | no matter where I move it, you'll notice
that that line is locked to that point.
| | 03:56 | If for some reason I made a mistake you
can always hit tab to return to that, type in
| | 04:01 | a new value, hit tab to accept it, or if I
hit tab to return to it I could hit Spacebar
| | 04:08 | to clear it, and I'm actually back
to not applying an actual dimension.
| | 04:13 | I am going to go ahead and enter it in
this case, because I think it's important that
| | 04:17 | you see how dimensions can be applied while
you're sketching, but also because as we move
| | 04:22 | forward I'm not going to use the dimensions,
and I want to show the difference between the two.
| | 04:28 | Now that I am ready to select my end point as
I hover near Horizontal another thing happens.
| | 04:33 | You'll notice near the end of the cursor
a Horizontal icon indicator has appeared.
| | 04:38 | This lets me know that Inventor is ready to
automatically apply a horizontal constraint,
| | 04:41 | and if I left-click you'll notice that the
line is purple as opposed to green, which
| | 04:47 | if you remember from our previous sketch movie,
indicates that this line is fully constrained,
| | 04:52 | and the reason for that is we have a dimension and
the horizontal constraint locks it into position.
| | 04:58 | I am now ready to
continue with the Line command.
| | 05:00 | You'll notice that the command is still
active and in this case it's using the end point
| | 05:04 | of the previous line to begin this line.
| | 05:06 | So now all I need to do is select an End
point here, and as I hover near Vertical, again, a
| | 05:12 | Constraint icon or Glyph
shows up near the cursor.
| | 05:15 | It also shows up near the original horizontal line,
and in this case it's applying a Perpendicular
| | 05:21 | constraint as opposed to a Vertical constraint.
| | 05:24 | The reason for that is once geometry is
created Inventor prefers to use existing geometry
| | 05:30 | to create constraints as opposed to just
applying a horizontal or vertical constraint.
| | 05:35 | In this case, that works for me, I'm going
to leave this to be perpendicular, but in
| | 05:39 | this case I'm not going to add the dimension, I'm
going to use that length dimension as a reference.
| | 05:44 | I'm going to get it to roughly 1.5, and I'm
going to go ahead and left-click to end that line.
| | 05:50 | The next line I create is going to be the
horizontal line that runs across the top of the square.
| | 05:56 | You'll notice as I hover around the
Graphics window, and I get near where the midpoint
| | 06:01 | of the bottom line is the heads-up
display shows me an Alignment indicator.
| | 06:05 | This isn't going to add a constraint
specifically to lock it to the midpoint, but it's a nice
| | 06:09 | way to let me know exactly where
I am in the sketch environment.
| | 06:13 | In this case, I do want to go ahead and move
all the way over to the end above this center
| | 06:18 | point, and you'll notice that Inventor is
ready to apply a parallel constraint based
| | 06:23 | on the icon shown in the heads-up display.
| | 06:26 | If I don't want that, say for example, I
really want this to be perpendicular to the
| | 06:30 | line here, I can simply hover over that or
scrub over it, and that will become the active
| | 06:37 | piece of geometry that
Inventor uses for reference.
| | 06:40 | In this case, now I'm looking to apply a
perpendicular constraint to the previous line and at any
| | 06:44 | point during the sketch process I can select any
piece of geometry to make that be active reference point.
| | 06:50 | I'm going to go ahead and let it apply the
parallel constraint, I'm going to left-click
| | 06:54 | to end the line and then I'll finish it off by
left-clicking at the center point or where I started.
| | 07:00 | I am going to right-click and hit Cancel to
end the command, you'll notice here one unique
| | 07:06 | item in this sketch, and that's that the
horizontal line at the top is actually green, which means
| | 07:11 | it's unconstrained or under constrained.
| | 07:15 | To review let's go ahead and right-click
and select Show All Degrees of Freedom.
| | 07:19 | Here you can see that the line is allowed
to move up and down, but it is not allowed
| | 07:24 | to move to the right or left.
| | 07:25 | We know that this sketch geometry is still
unconstrained because we did not apply that
| | 07:29 | dimension to the vertical line on the right.
| | 07:33 | We'll get to that in the Dimension movie,
but for now we'll go ahead and hide all the
| | 07:37 | degrees of freedom and
continue on with our sketch.
| | 07:39 | I am going to go ahead and launch the Line
command one more time, and this time we're
| | 07:43 | going to use the existing geometry to
create the overhang that will define part of the
| | 07:47 | starter cover that attaches to this piece.
| | 07:49 | I am going to left-click on the line
to begin our new piece of geometry.
| | 07:55 | I'm going to left-click again to find its
end point and then I'm going to return to
| | 07:59 | that original line again and left-click
just to define the basic shape of our overhang,
| | 08:05 | and in the next movie we'll
look at how to dimension that.
| | Collapse this transcript |
| Dimensioning a part| 00:00 | In the previous movie, we
learned how to draw with the Line tool.
| | 00:03 | During that movie, we created the sketch
that you see on the screen, and we are now ready
| | 00:06 | to add dimensions to define the overall size.
| | 00:09 | To begin, we need to get into the sketch
environment, and we can do that by double-clicking the
| | 00:14 | sketch in the browser to edit that sketch.
| | 00:16 | You will notice that the Sketch tab is
displayed, and we are now in the editing environment,
| | 00:22 | and we are ready to add our dimensions.
Inventor only has a single dimension command.
| | 00:27 | It can be found on the Sketch tab under
the Constrain panel or through right-clicking
| | 00:32 | to bring up the Marking menu, and
selecting the lower-left position.
| | 00:37 | We know that the plate on the
screen needs to be perfectly square.
| | 00:40 | So we need an overall height dimension.
There is a couple of ways to add this.
| | 00:43 | I am going to show you both ways because both
are valid, and depending on the type of sketch
| | 00:47 | geometry you've created, you
may select one over the other.
| | 00:51 | While into the Dimension command, we'll start
by switching the bottom horizontal line followed
| | 00:55 | by the top horizontal line.
| | 00:57 | We can move our cursor off to the left to
where we want our dimension placed, and we
| | 01:01 | can left-click again to place that dimension.
| | 01:04 | After placing the dimension, an Edit
dialog pops up, and allows you to enter an exact
| | 01:08 | value for this piece of geometry.
| | 01:12 | You can now see that the dimension has
been placed, the geometry has changed color to
| | 01:16 | indicate that it's fully constrained or
dimensioned, and we could move forward.
| | 01:19 | I am going to go ahead and undo this using
Ctrl+Z on my keyboard, and show you another way.
| | 01:25 | The first one, I selected two
different pieces of geometry.
| | 01:29 | This time, I'm going to enter the Dimension
command, and select just the single vertical line.
| | 01:35 | Then when I move my cursor to the left, I
get the same dimension I had last time but
| | 01:40 | I had fewer clicks to do it.
| | 01:42 | Placing that dimension again, I can enter
the 1.575 value and hit Enter, and essentially
| | 01:48 | have created an identical dimension.
So, either way is completely valid.
| | 01:51 | The reason you would choose one over the
other would be in a case where you don't have a
| | 01:55 | single vertical line defining the height.
| | 01:57 | For example, if I were to create two different
rectangles here, maybe I am making an L bracket
| | 02:05 | of some sort, and now I
enter the Dimension command.
| | 02:09 | There's no single line or piece of
geometry that defines the overall height.
| | 02:13 | In that case, selecting the bottom horizontal
line and top horizontal line is the only way
| | 02:18 | to create the overall
dimension of this geometry.
| | 02:20 | So, depending on the type of sketch you're
creating, either is completely valid and they
| | 02:25 | create identical sketches.
| | 02:27 | It's just a matter of you selecting
the one that you need for your design.
| | 02:30 | I am going to get out of the Dimension
command by hitting Escape on the keyboard.
| | 02:33 | I am going to delete this
geometry because we don't need it.
| | 02:37 | I just wanted to show you a sample of
where you could use both types of dimension.
| | 02:41 | We are now ready to dimension our overhang.
| | 02:43 | The overhang is found on the right, and you
can see it because it's the only item that's
| | 02:46 | still green, meaning it's still unconstrained.
| | 02:48 | We are going to start by adding a
dimension to locate the top of the overhang.
| | 02:54 | I am going to start by selecting the top horizontal line
because that's what I want the base dimension to start from.
| | 03:00 | Now, rather than selecting the line, I can hover
over and select the vertex where it meets the square.
| | 03:07 | I can then place my dimension just like I
did in the previous dimension, left-click
| | 03:11 | to place that on the screen,
and enter a value of 0.212.
| | 03:16 | Hitting Enter on the keyboard accepts
that value, and we're ready to continue on.
| | 03:20 | We're still in the Dimension command, and I need to
dimension the position of this overhang at the corner.
| | 03:25 | So, I am going to go ahead and select the top
horizontal line again, and this vertex at the corner.
| | 03:31 | Again, I'll place my dimension, and in
this case, I am going to enter 0.404.
| | 03:36 | Now, we are almost
finished dimensioning the sketch.
| | 03:39 | But the next dimension we
need is an angle dimension.
| | 03:42 | As I mentioned, Inventor
only has one Dimension command.
| | 03:46 | I want to dimension the angle
between this line, and this line.
| | 03:49 | To do so, I simply select each of the lines,
and you will notice after I select the first
| | 03:53 | line, if I hover near the second line, an
icon pops up near the cursor, indicating an
| | 03:58 | angle dimension is going to be applied.
| | 04:00 | Simply left-clicking again, and moving my
cursor to where I would want to place the
| | 04:04 | dimension, you will notice that
I've created an angle dimension.
| | 04:07 | Now, before I place this, I am going to
move my cursor to a few different locations.
| | 04:11 | You'll notice that based on where my cursor
is the dimension value will change to indicate
| | 04:16 | the angle of the two lines at that location.
| | 04:20 | Once I find the specific dimension I want
to place, I can move my cursor to where I
| | 04:25 | want to place the dimension and enter a value.
| | 04:30 | The final dimension we need to create is very
similar to the previous few that we've created,
| | 04:34 | we want to measure the overall distance from
the far-left side of the square to the vertex
| | 04:40 | on the corner of the outcrop.
| | 04:41 | I am going to go ahead and place that up near the
top of the screen, and enter 1.88 for that value.
| | 04:48 | At this point, we've
completely dimensioned our sketch.
| | 04:50 | You can tell that because all the geometry
is the darker of the two colors that I have
| | 04:53 | in my color scheme, in this case, purple.
| | 04:56 | And we are now ready to finish
the sketch and begin part modeling.
| | Collapse this transcript |
| Creating parameters| 00:00 | In the previous movie, we
dimensioned this Sketch.
| | 00:03 | While it's completely dimensioned, and we
could move on to part modeling at this point,
| | 00:08 | I wanted to step back for a second and explain
some things that are happening in the background.
| | 00:13 | Because this is an introductory course, I
think it's important that you understand some
| | 00:16 | of that background nuance that's taking
place so that you better understand things as you
| | 00:20 | are learning and moving forward.
| | 00:21 | We are going to go ahead and edit this
sketch by double clicking on it in the browser.
| | 00:26 | What I want to talk about is Parameters.
Inventor is a 3D Parametric Modeling system.
| | 00:31 | What that means is the dimensions that are
created are actually just representations
| | 00:35 | of parameters that the system is
keeping control of in the background.
| | 00:40 | You might've noticed when I was placing
dimensions in the previous movie that each dimension,
| | 00:45 | in the Edit dialog box, has a name.
| | 00:47 | If you double-click any
dimension, you can see this.
| | 00:51 | In this case, we are editing dimension d0.
| | 00:54 | You can see in the title bar here, if I
close this dimension, and I double-click the next
| | 00:59 | dimension, you'll see d1 listed.
| | 01:01 | Now if you've been following along in creating
parts and sketches along with me, your dimension
| | 01:07 | names might be slightly different,
and that makes no difference.
| | 01:10 | You can change the name, and I'm actually going
to show you how to do that as part of this movie.
| | 01:14 | So if you see a different dimension than what
I'm seeing on the screen, or a different dimension
| | 01:18 | name more specifically, that's okay.
You don't need to worry about that.
| | 01:23 | What's important here is because they each
have names, you can do special things with them.
| | 01:28 | For example, d0, d1, d2,
those are not very meaningful.
| | 01:33 | They are really just a way for the system to
keep track of the dimensions that are created.
| | 01:38 | This square would make much more sense if
the dimension name was width and height.
| | 01:42 | So, for example, the very first dimension,
the d0 dimension, if I wanted to give this
| | 01:47 | a name that meant something to me, I can
actually hit the Home button on my keyboard and in
| | 01:53 | front of the dimension, actually place a name.
In this case, I am going to call this width.
| | 01:59 | Now you'll notice as I type everything is
in red which indicates something is wrong,
| | 02:03 | and I purposely stopped here
so that you could see that.
| | 02:06 | Just because you see red, doesn't mean
that you can't make things work correctly.
| | 02:10 | In this case, what it's telling us is it
needs an equal sign, or you could remove that,
| | 02:14 | and it would go back to
normal, it just needs a value.
| | 02:17 | But what I've done here is
I've typed width= and some value.
| | 02:21 | This is a way to name
your dimensions on the fly.
| | 02:24 | Now you won't always do this--and especially
in an introductory course, it's not necessarily
| | 02:28 | needed--but again as your things get more
advanced, and as you start creating more complex
| | 02:34 | designs, naming your
dimensions can be very handy.
| | 02:37 | I am going to go ahead and hit Enter here,
and it looks as if nothing has changed.
| | 02:41 | But if I double-click that dimension again,
you will now see it says Edit Dimension : width
| | 02:46 | and then we're back to seeing
the exact value of that parameter.
| | 02:50 | This is exactly what we want.
| | 02:52 | The reason for that is we can then
use that name in other dimensions.
| | 02:57 | For example, right now the two dimensions
that define the overall size of the square
| | 03:03 | are not related in anyway.
| | 03:05 | If I double-click this dimension and change
it to 2 and hit Enter, my square is no longer
| | 03:10 | square, and that's part of what's powerful
about a Parametric Modeling System is the
| | 03:14 | ability to build rules and intelligence
into the models so that when something changes,
| | 03:19 | it always will, you have to do less
work in going back and changing your model.
| | 03:23 | I am going to go ahead and double-click this
dimension to edit it, but in this case I am
| | 03:27 | going to do two things at the same time.
| | 03:29 | I'm going to name this
dimension and also give it a value.
| | 03:34 | So in this case, this is
the height of the square.
| | 03:35 | I am going to name this height.
I am going to make it equal some value.
| | 03:40 | I could enter some value.
| | 03:43 | In this case, I actually want to enter the
name of the other dimension, which is width.
| | 03:47 | I want the height and
width to always be the same.
| | 03:50 | This will ensure that my plate is always
square, regardless of what value I enter.
| | 03:55 | So in this case, I am going to enter width,
and you'll notice the red goes away because
| | 04:00 | now I have a valid expression,
and I can hit Enter on my keyboard.
| | 04:04 | Now something else
happened here when I hit Enter.
| | 04:07 | The dimension changed a little bit.
| | 04:09 | If I double-click it, you'll notice that it says
Edit Dimension : height and the value for it is width.
| | 04:17 | So what the system is doing is it's taking
the value of this width dimension down here
| | 04:21 | at the bottom, and it's entering that value in.
| | 04:24 | The other thing it did was it indicated
that a formula or an expression was controlling
| | 04:29 | this by entering in fx: in
front of the value in the dimension.
| | 04:33 | But it doesn't change the Dimension value,
it just indicates that something is driving
| | 04:37 | this dimension or controlling this
dimension other than a solid straight value.
| | 04:42 | When you rename things, and you start getting
a little more advanced in your dimensioning,
| | 04:47 | there's going to be times where you want to
see all of the names of things or all of the
| | 04:50 | expressions driving these dimensions.
To do this, you can change the Dimension style.
| | 04:57 | With nothing selected on the screen, if you
right-click in the Graphics window, you have
| | 05:02 | an option in your right-click
menu which is Dimension Display.
| | 05:07 | And under this flyout menu, you have a few
different options, you have Value, Name, and Expression.
| | 05:12 | Those are the three I want to focus on.
| | 05:14 | Tolerance and precise value are more advanced,
and we won't be covering those in this movie.
| | 05:18 | Right now, we have Value selected.
| | 05:20 | If I select Name, you'll notice that all
the dimensions change to show the name of the
| | 05:26 | dimension rather than their value.
| | 05:28 | You can see that we have our width dimension
down at the bottom, we have our height dimension
| | 05:31 | here on the side, you can see the name the
system gave to the other dimensions as well.
| | 05:36 | If I go back and right-click again and go back to my
Dimension Display, I have the option for Expression.
| | 05:43 | Expression is a little more valuable in
the sense that it shows you both the name and
| | 05:47 | the value or the formula that's
driving or creating the value.
| | 05:51 | So, for example, here at the
bottom, we have width=1.75.
| | 05:55 | Over on the right, we say height=width, and
we can very easily see the width value right
| | 06:00 | here so that we get a better understanding
of what the system is doing and how this is
| | 06:04 | actually controlling the size of the model.
| | 06:07 | Now to go a little further, I am going to
go ahead and go back to my Dimension Display
| | 06:11 | as Expression by right clicking on the screen,
selecting the Dimension Display and returning
| | 06:16 | to the Value option.
| | 06:18 | The next step in Parameters that really adds
even more power to the system itself is the
| | 06:22 | ability to create formulas.
| | 06:25 | While technically, height = width is a
formula, we can get a little bit more advanced.
| | 06:29 | If, for example, we were to change the overall
size of our square, let's say it's 1.75, you'll
| | 06:37 | notice that our overhang gets squished--I know
not a very technical term--but you see the result.
| | 06:44 | The reason for that is the overall width of
the square is not related to the overall width
| | 06:50 | of our overhang at the same time.
| | 06:52 | So let me go back to set this to 1.575,
and we are back to proper proportions.
| | 06:58 | There is a couple of ways we can handle this,
and this is a really important thing to keep
| | 07:03 | in mind while sketching when you get to a point where
you are going to start using parameters and formulas.
| | 07:08 | Just because you have an overall dimension
that you want to see on a manufactured part,
| | 07:12 | doesn't necessarily mean you need to create
those same dimensions while modeling the part,
| | 07:16 | and I'll show you what I mean.
| | 07:18 | In the case of this 1.88 value, we actually
know that there's going to be some distance
| | 07:25 | from the edge of the out hang to the side
of the square, plus the overall width value.
| | 07:31 | I'm going to edit this value, and I'm going
to enter width +, the difference between the
| | 07:38 | 1.88 and the 1.575, which is actually .305.
| | 07:44 | When I hit Enter, again the overall size
doesn't change, but what's important here is I built
| | 07:49 | into the sketch intelligence that says
always make this value at the top, the total width
| | 07:57 | of this square plus .305.
| | 08:00 | So if, for example, now when I change this
dimension to 1.75, the outcrop moves with
| | 08:07 | the overall size of the square, and
we don't have to change proportions.
| | 08:11 | Now another concern I have is back to what
I mentioned that the dimensions you use in
| | 08:16 | the overall modeling, might not be the exact
same dimensions you use in manufacturing. And
| | 08:21 | the reason for that is I could cancel this
and actually delete this dimension and simply
| | 08:28 | add a dimension to this outcrop to define .305.
| | 08:34 | What I've done here is created the exact
same physical result in two different ways, one
| | 08:38 | using a formula, and one just
selecting a different type of dimension.
| | 08:43 | This is the power of a 3D Parametric
Modeling System, and it shows the importance of the
| | 08:47 | designers sitting behind the computer itself.
| | Collapse this transcript |
| Creating circles and rectangles| 00:00 | In this movie we're going to
focus on circle and rectangles.
| | 00:03 | Now, because this is the last movie in the
sketching chapter, we're also going to bleed
| | 00:07 | a little bit into part modeling as
we create the geometry to sketch on.
| | 00:11 | It's not important that you understand
everything from a part modeling aspect, because we're
| | 00:15 | going to cover that later, but I think you'll
start to see how sketching and part modeling
| | 00:19 | are connected as we move through this video.
| | 00:22 | We're going to begin by extruding this base plate
that we've been creating over the previous movies.
| | 00:27 | We're going to right-click and
from the Marking menu select Extrude.
| | 00:30 | We can then select the two profiles that we
created and give them an overall Height of .125.
| | 00:37 | We can hit Enter on the keyboard to accept that
value and our initial base feature has been created.
| | 00:42 | You can see it here in
the browser as Extrusion1.
| | 00:47 | Before we continue sketching we need one more
item added to this part, and that's a fillet.
| | 00:52 | We're going to fillet each corner.
| | 00:54 | We're going to start by selecting this first
corner and the Heads-Up Display will present
| | 00:57 | a Fillet and Chamfer option.
| | 00:59 | We're going to select Fillet, which is the
rounded corner, and we're going to work our
| | 01:04 | way around the parts,
selecting each corner edge.
| | 01:06 | You can select through the part, so I can
get to this vertical edge in the back simply
| | 01:10 | by selecting through the part.
| | 01:12 | And once I've selected all four corners,
I'll hit the check box to accept those.
| | 01:16 | We've now created our base feature that we're
going to build from, and we can begin looking
| | 01:20 | at circles and rectangles.
| | 01:22 | But before we do that I'm going to switch
back to the faceplate, which is the completed
| | 01:25 | part so you can see where we're headed.
| | 01:28 | In this case, you can see where the base plate
is located here, we're going to go ahead and
| | 01:32 | create circles for these bosses on each corner.
| | 01:36 | We're going to create a
circle for the boss in the center.
| | 01:38 | We're going to create the center hole, and
we're going to create a rectangle that locates
| | 01:42 | these holes around the main boss.
| | 01:45 | We'll switch back to our
part and continue along the way.
| | 01:49 | We're now ready to being sketching circles.
| | 01:51 | We're going to start with the
boss in the center of the part.
| | 01:53 | To do that, we're going to select the top
face and from the Heads-Up Display select
| | 01:58 | Create Sketch on the far right.
| | 02:01 | A couple of things happened, we rotated
so that we're looking normal to the view.
| | 02:04 | We're straight down on the sketch.
| | 02:06 | And you'll notice the yellow lines were
projected from the edges of the part below.
| | 02:10 | We're going to leverage this projected
geometry to create the center boss of our part, and
| | 02:14 | the reason for that is this boss needs to be
perfectly centered in the middle of the base plate.
| | 02:19 | To do this, we're going to start by Creating
a Line--which we learned about in a previous
| | 02:23 | movie--and we're going to start our line at the
center point that was projected from the part.
| | 02:28 | You'll notice as we hover near the center
point a green dot appears, which indicates
| | 02:32 | a coincident constraint is going to be applied.
| | 02:35 | We can then hover the end of the line near the
center point on the opposite corner, left-click
| | 02:39 | to lock that into place.
| | 02:41 | We can hit Escape on our keyboard to get out
of the command, and you'll notice we now have
| | 02:45 | a line that's locked to the center points
and the dark purple color indicates that it's
| | 02:49 | permanently constrained.
| | 02:51 | The next thing I'm going to do, I'm going
to select this line, and because we're using
| | 02:54 | this simply as a construction piece of geometry,
we're using it just to create a midpoint that
| | 02:59 | we can lock to, select that line, right-click,
and the Heads-Up Display has changed to indicate
| | 03:06 | things I can do this line.
| | 03:07 | I could turn it to a Centerline, I could
Delete it, or I could convert it to a piece of
| | 03:11 | Construction geometry.
That's what I'm going to do.
| | 03:15 | And after doing so you'll
notice the display changes a bit.
| | 03:18 | It's now a dashed line, and what that
indicates is that it is construction geometry, and it
| | 03:22 | will be ignored when creating modeling features.
| | 03:25 | All it's there for is so that we can center our
circle or our boss on the midpoint of this line.
| | 03:31 | From the Marking menu
I'm going to select Circle.
| | 03:34 | I can now hover near the midpoint of this line.
| | 03:37 | Again, I get the green dot to lock
the center point to the midpoint.
| | 03:40 | I'm going to left-click to place
and begin to drag my circle out.
| | 03:44 | Now, you'll notice the Heads-Up Display
for a Circle is showing a Diameter dimension.
| | 03:49 | In this case, I know we need a radius dimension.
| | 03:52 | So before placing the circle, while I'm in
the middle of the command, I can right-click,
| | 03:57 | and I do have an option to change to Radius.
| | 04:01 | If at any point you need to switch back,
you can simply right-click while you're in the
| | 04:04 | middle of the command and switch back to a
Diameter, it's just a toggle back and forth.
| | 04:09 | In this case, I'm going to go ahead and right-click
one more time because I do want that Radius
| | 04:13 | value, and I'm going to enter .413 as my value.
| | 04:17 | I'm going to hit tab on my keyboard to accept that,
and then I'm going to left-click to place the circle.
| | 04:22 | I've now completed the sketch, and I can right-click
in the graphics window and select Finish Sketch
| | 04:26 | from the Marking menu, or I can go to the
toolbar and select Finish Sketch at the far
| | 04:31 | right, both do the exact same thing,
and it's a matter of preference.
| | 04:35 | From the Marking menu I'm now ready
to extrude the circle I just created.
| | 04:39 | I can select that circle on the screen and
enter a value of .315 for its Height, hitting
| | 04:45 | Enter on the keyboard will accept
that value, and the boss is created.
| | 04:49 | Now, it's a little hard to
see because of the coloring.
| | 04:52 | I'm going to use my Visual Styles, which we
turned on in the navigation tools video, and
| | 04:56 | I'm going to turn on my
Shaded with edges option.
| | 04:59 | This allows me to see the top of the boss
a little more clearly and will help as we
| | 05:02 | continue along sketching.
| | 05:04 | The next thing we need to do is
add the bosses around each corner.
| | 05:08 | I'm going to sketch on the same face again.
| | 05:10 | It rotates into a Normal view, but this
time you'll notice something happened.
| | 05:15 | If I orbit a little bit, you'll notice that
this sketch actually runs through this part.
| | 05:23 | Now we're ready to create our
circle bosses in each corner.
| | 05:26 | I'm going to use the Marking menu to access
the Circle tool, and in this case I'm going
| | 05:31 | to use the projected geometry to
completely define these bosses.
| | 05:34 | I'm going to hover over the center points
of the fillets to lock my center point of
| | 05:38 | the circle to that, and I'm going to hover up near the
edge of the part to get another coincident constraint.
| | 05:42 | I'm going to left-click, and you'll notice the
circle that's created is automatically purple.
| | 05:47 | The center point is locked to the fillet and
the outer edge is locked to the edge of the part.
| | 05:52 | This completely defines the circle, and I
don't have to add any dimensions. If the fillet
| | 05:56 | underneath changes, the
circles will also update.
| | 05:59 | I'm going to work my way around and repeat
that process for each of the corners, and
| | 06:04 | we'll be ready to extrude our bosses.
| | 06:10 | With those completed, I can hit Escape on
my keyboard to get out of the Circle command,
| | 06:14 | and I can right-click and select
Finish Sketch from the Marking menu.
| | 06:18 | Now we're ready to extrude those bosses.
| | 06:20 | I can right-click on the
Marking menu and select Extrude.
| | 06:23 | I can select each of those bosses that I just created,
and I can give them an overall Height value of .16.
| | 06:32 | Hitting Enter on the keyboard accepts
that value and the bosses are created.
| | 06:35 | Next, I'm going to create the
center hole that goes through this boss.
| | 06:40 | To do so, I'm going to start a new sketch
by selecting that face and from the Heads-Up
| | 06:44 | Display select Create Sketch again.
| | 06:47 | Now that we're in the sketch environment,
the Marking menu has my Sketch Tools again,
| | 06:50 | and I can select Circle.
| | 06:52 | I'm going to lock it to the center of that part,
and I'm going to give it an overall value of .5.
| | 06:59 | I'm going to hit tab on my
keyboard to lock that in.
| | 07:02 | But you'll notice that it remembered
the Radius that we used previously.
| | 07:05 | While I'm in this command, before I place it,
I can right-click and again select Diameter,
| | 07:10 | and you'll notice it maintains the .5 that I
entered, but changes it to a Diameter dimension.
| | 07:15 | Left clicking places that, and
I'm ready to finish the sketch.
| | 07:21 | With that circle created I can right-click
and select Extrude from the Marking menu.
| | 07:25 | I can select the circle that we created, and I'm
going to select a Through All option for this extrusion.
| | 07:30 | I'm going to select the check box in the Heads-Up
Display to accept that, and we now have a
| | 07:35 | hole that goes all the way through the part.
| | 07:39 | The final element we're going to cover
are the holes that surround the boss.
| | 07:42 | Just to refresh, if I switch back to the base
plate, you can see them surrounding the boss
| | 07:46 | here and here, there is four total.
| | 07:50 | We're going to switch back to our part,
and we can being a new sketch on that face.
| | 07:56 | Now here we notice something happens that's
a little different than we've seen before.
| | 08:00 | While we get the projected edges, if I
orbit a little bit, you'll see that this sketch
| | 08:04 | actually cuts through the part a bit.
| | 08:07 | In order to help with visibility while
sketching, you have the ability to right-click in the
| | 08:11 | graphics screen and select Slice Graphics.
You can also hit F7 on your keyboard.
| | 08:16 | What that does is temporarily slices the
graphics away from the part so that you have better
| | 08:21 | visibility of the sketch you're creating.
| | 08:23 | Again, if I hit F7 on the keyboard,
you'll notice it toggles back and forth.
| | 08:28 | It's a simple temporary visibility enhancement that
allows you to see things that you're sketching on.
| | 08:32 | Now, I'm going to rotate back to a Top
view so we're looking normal at this view, and
| | 08:37 | we can begin with our Rectangle command.
| | 08:40 | Because we're in the sketch environment, we
could bring up the Marking menu, but you'll
| | 08:44 | notice that there is a Two
Point Rectangle in our Marking menu.
| | 08:47 | In this case, I don't want the
rectangle that's defined by two corners.
| | 08:51 | I'm going to go up to the Sketch tab, to the
Draw panel, and find the Rectangle command.
| | 08:57 | The Rectangle command has a split button,
and if I select the dropdown option I have
| | 09:01 | different types of rectangles that I can create.
| | 09:04 | In this case, I want a rectangle that's a
Two Point, but one of those point is a center
| | 09:08 | point, because of that I can select the center
of this boss which was projected to our sketch.
| | 09:14 | And as I start to drag you'll notice that
my square or rectangle is locked into the
| | 09:20 | center of that part.
| | 09:22 | I'm going to use the Heads-Up
Display to create dimensions on the fly.
| | 09:25 | In this case, .716 is the Width of the rectangle.
| | 09:28 | I'm going to hit tab on my keyboard to switch to
the other dimension and enter .716 one more time.
| | 09:34 | I'm going to hit Enter on my keyboard to
accept those values, and you'll notice the rectangle
| | 09:38 | is created, it's locked to the center of the
circle, and it's fully constrained, indicated
| | 09:43 | by the purple geometry.
| | 09:44 | I'm going to get out of my Rectangle
command by hitting Escape on my keyboard, and I'm
| | 09:49 | going to make one more change.
| | 09:51 | Because this is construction geometry, I'm
only creating this rectangle to locate the
| | 09:55 | center of holes I'm going to create.
| | 09:56 | I'm going to hold Shift down on my keyboard
and select each of the outer edges of this
| | 10:01 | rectangle, and with them selected right-click
and change to Construction Geometry.
| | 10:06 | I'm going to hit Escape on my keyboard to
make sure nothing is selected now, and I'm
| | 10:10 | ready to finish this sketch.
| | 10:13 | From the Marking menu I'm going to select Finish
2D Sketch, and I'm ready to create my holes now.
| | 10:18 | From the Marking menu I can right-click and
select Hole and in this dialog box you can
| | 10:23 | see that I'm ready to select the center points.
| | 10:26 | I can select the center point of these
circles by clicking on the corners of the rectangle
| | 10:30 | we just created, and I've now
located each of those circles.
| | 10:35 | In this case, the Diameter of the hole is .08,
and I'm going to select the check mark to
| | 10:40 | accept that value, and I've created my holes.
| | 10:43 | Now, because we're going to cover holes and
other things around part modeling in future
| | 10:47 | movies, we're going to stop here.
| | 10:49 | At this point we've seen how to use
circles and rectangles, and we've started to look
| | 10:53 | at a little bit of part
modeling as we prepare for that chapter.
| | Collapse this transcript |
|
|
4. Part ModelingIntroducing part modeling| 00:00 | In this chapter, we are going
to be covering part modeling.
| | 00:03 | Up to this point, we've learned about the
interface, we have learned how to sketch geometry,
| | 00:06 | we have even learned a little bit
about part modeling along the way.
| | 00:10 | Now we are ready to dive into the details.
| | 00:12 | On the screen is the part we are going
to be creating throughout this chapter.
| | 00:15 | I am going to use my Visual
Styles icon to enable part edges.
| | 00:20 | I have selected that from my
Navigation bar which we added earlier.
| | 00:23 | But if you didn't add that, you can access
it from the view tab, under the Appearance
| | 00:28 | panel, the Visual Styles button.
All you do is simply select Shaded with Edges.
| | 00:33 | This simply lets you see the edges a little
more clearly and better understand the part.
| | 00:38 | On the left in the browser, you can see the
features that have been built to create this part.
| | 00:43 | The browser is essentially a view
into what you're seeing on the screen.
| | 00:46 | So, if I hover over Extrusion 1, it will
highlight in the graphics window as well.
| | 00:51 | As you slowly work your way down the list, you can
actually see how the part was built piece by piece.
| | 00:57 | Because Inventor is a history based modeler,
each feature you create is added to the browser,
| | 01:01 | and each subsequent feature is
added below that in the browser.
| | 01:05 | If you look at the bottom of the browser
tree, you'll notice an End of Part icon.
| | 01:08 | This icon can actually be moved to essentially
go back in time, and see how this part was built.
| | 01:14 | I often use this to interrogate models that
others have built in order to learn how they're
| | 01:18 | doing things, perhaps
slightly different than myself.
| | 01:21 | I also use it to double-check my own
work just to remember how a part was built.
| | 01:25 | If you left-click on the End of Part icon
and drag up the browser tree, you have the
| | 01:30 | ability to locate that at any position.
| | 01:32 | By releasing my mouse button, essentially, all
features beyond the End of Part are suppressed--
| | 01:38 | or temporarily turned off--and I can see this
part at its very first base feature or Extrusion 1.
| | 01:44 | I can then take the End of Part icon, and
drag it down below Extrusion 2, and you can
| | 01:49 | see a new feature is
displayed in the graphics window.
| | 01:52 | If you work your way down the model, you can
actually see how this part was built over time.
| | 02:00 | Now, we are going to build this part from scratch,
and we are going to cover each of these items.
| | 02:04 | But in the first movie covering extrusion,
we'll create the first eight excursions.
| | 02:08 | Now, this might seem a bit
repetitive, but part modeling is.
| | 02:12 | It's important to understand how to sketch,
and connect that with modeling features like
| | 02:15 | extrusion to build a complex part.
| | 02:18 | Overall, the process is fairly simple, but in
the end, the part might be much more complex.
| | 02:23 | Hopefully, this helps you understand how part
modeling happens and how the browser is connected
| | 02:27 | to the graphics window.
| | 02:28 | We will be using both throughout this
chapter to learn how to build this part.
| | Collapse this transcript |
| Creating a base extrusion| 00:00 | The first part modeling feature
we're going to focus on is extrusions.
| | 00:04 | On the screen, you'll see the part that
we're going to build throughout this chapter.
| | 00:07 | I'm going to roll the End of Part
icon back to just below Extrusion 8.
| | 00:11 | On screen, you'll see what we should
end up with at the end of our extrusions.
| | 00:14 | We're going to go ahead and create each of
the eight extrusions that make up this part.
| | 00:18 | When I begin part modeling, I like to look
for the biggest or most pronounced feature,
| | 00:22 | or the item that has the most
things attached to it as my base feature.
| | 00:26 | That way, I have something
solid I can build out from.
| | 00:28 | In this case, I see it as being this cube,
and that's where we're going to start.
| | 00:32 | I'm going to start a blank
file to begin this process.
| | 00:35 | From the Application menu, you can select New >
Part to create a blank part file to start from.
| | 00:42 | I'm going to create a new sketch by right-clicking
and selecting New Sketch from the Marking menu.
| | 00:47 | Because this is the base feature, the origin
planes are displayed, and I'm able to select
| | 00:51 | a plane to sketch on.
| | 00:53 | Now, because this part is overall fairly
symmetric, I'm going to draw my initial rectangle in
| | 00:59 | a specific type of way so that we can leverage the
origin planes as we model things throughout this chapter.
| | 01:05 | I'm going to start with the Rectangle command, but
I'm going to select a specific type of rectangle.
| | 01:10 | I'm going to use a Two Point Center Rectangle.
| | 01:13 | By doing this, the first point I select is
considered the very center of the rectangle,
| | 01:18 | and as I drag out, my heads-up
display allows me to add dimensions to this.
| | 01:21 | In this case, this cube is
going to be 0.692 in width.
| | 01:26 | I'm going to hit tab on my keyboard to
move to the next dimension, and enter 0.757.
| | 01:31 | I'm going to hit tab on my keyboard again,
and then Enter to actually create the rectangle.
| | 01:35 | You'll notice by using the heads-up display
and the center point origin that was projected
| | 01:40 | to the sketch, I was able to fully constrain and lock
this rectangle down just using the heads-up display.
| | 01:46 | I'm now ready to create my first extrusion.
| | 01:48 | I'll right-click and select Finish Sketch,
and I return to the modeling environment where
| | 01:53 | I can then right-click and select Extrude.
| | 01:55 | Now, I know this extrusion has a height of 0.518,
and we're going to extrude it to a distance.
| | 02:01 | But before we do that, I wanted to talk a
little bit about the heads-up display, and
| | 02:05 | the other things you see on the screen.
| | 02:07 | You'll notice the heads-up display here
near my cursor, but also on the screen, you'll
| | 02:11 | notice the Extrude dialog box which is hidden.
| | 02:14 | Clicking on the dropdown arrow exposes
the dialog box that actually controls this.
| | 02:19 | It's up to you whether or not you use it.
I prefer to use the heads-up display.
| | 02:22 | But while you're learning, it might be
worthwhile to actually use the Extrude dialog box.
| | 02:26 | When extruding, there's a few different options that you
need to input to determine the geometry that's created.
| | 02:32 | You have to pick a profile,
which we did right when we started.
| | 02:34 | If there's only one profile in a sketch, the
system automatically selects that profile for you.
| | 02:39 | The next option is Output.
| | 02:41 | In this case, we're actually creating a
solid model, the other option is Surface, but we
| | 02:44 | won't be covering that in this course.
| | 02:47 | Because it's the base feature,
we have limited options here.
| | 02:50 | These buttons that are grayed out in the
center are options for Join, Cut, and Intersect.
| | 02:55 | But we'll cover this in later extrusions.
| | 02:57 | By default, the very first base feature is
creating a new solid, and that's checked by default.
| | 03:02 | Under the Extends area, we have the
ability to select different types of termination.
| | 03:07 | We can say extrude to a distance, extrude
to a specific item, or between two items.
| | 03:13 | We have the ability to enter a
distance, and then also a direction.
| | 03:16 | Now that we've seen this, I'm going to go
ahead and collapse this and return to the
| | 03:19 | heads-up display because all the same
information is available in the heads-up display.
| | 03:23 | You have from the dropdown menu a Distance,
the option to select to a specific point or
| | 03:28 | face, or between two faces.
| | 03:32 | We have the ability to select our
profiles which again was already done for us.
| | 03:35 | We have the ability to select
whether we're going to do solid or surface.
| | 03:39 | In this case, we have Join, Cut, and Intersect,
but because it's our base feature, we're going
| | 03:43 | to create a new solid.
We have our directions.
| | 03:46 | And in this case, because its symmetric part,
and we used the center rectangle, I'm going
| | 03:50 | to actually use Symmetric.
| | 03:51 | This will allow me to perfectly center
this part so that we can appropriately use the
| | 03:55 | origin planes in future extrusions.
| | 03:58 | And last but not least, we have the option
to cancel this command or accept the inputs.
| | 04:03 | In this case, before I actually accept this
input, I'm going to set the corrected dimension,
| | 04:08 | in this case, 0.518.
| | 04:09 | I'm going to hit Enter on my keyboard to
accept that part, and now we have our first base
| | 04:14 | feature which you can see in the browser.
| | 04:16 | When we hover over it, it
highlights in the graphics window.
| | 04:19 | Now, before we continue, I'm
going to do a couple of other things.
| | 04:22 | I'm going to turn on my
Visual Style to show shaded edges.
| | 04:26 | I'm also going to reorient this model a
little bit from the view Cube standpoint so that
| | 04:30 | it's in the proper orientation for continuing.
| | 04:35 | I like to have my XY plane as the
flat surface and Z pointing straight up.
| | 04:40 | Once I have the orientation set, I can right-click
on my Home button, I can set Set Current view
| | 04:45 | as Home, I'm going to fit it to the view,
and I'm going to select the Right view, and
| | 04:50 | change that to represent the Front view.
| | 04:53 | I can do that by right-clicking on the view cube,
selecting Set Current view As and then Front.
| | 04:59 | When I click my Home view, I now have the
model in the proper orientation to continue.
| | 05:04 | This is really a personal preference, but I
think it's worthwhile for everybody to get
| | 05:08 | used to how to reorient the
model to fit their design preference.
| | Collapse this transcript |
| Creating multiple extrusions| 00:00 | Now that we have our
BaseExtrusion, we're ready to continue on.
| | 00:03 | The process from here on out does
begin to get a little bit repetitive.
| | 00:06 | So I'll make sure to call out all the
actions that I'm taking, and more specifically, call
| | 00:10 | out any new actions that will help you
better understand the Extrusion process.
| | 00:14 | To begin, we need to create a
sketch on the top face of this part.
| | 00:17 | We can select that face and use the
heads-up display to create a new sketch.
| | 00:21 | We know that this boss needs
to be centered on the part.
| | 00:24 | In order to do that, I'm going to create a
line, I'm going to lock it to the midpoint
| | 00:28 | of one of the projected edges, and I'm going to
actually enter its dimension here in the heads-up display.
| | 00:33 | In this case, it's going
to be .319 from the edge.
| | 00:36 | I'm going to hit Escape on my keyboard to
get out of the command, and I'm now ready
| | 00:40 | to create the circle that will create the boss.
| | 00:42 | From the Marking menu, I can select Circle,
and I can lock the center point to the end
| | 00:46 | of the line I just drew by
left-clicking on its endpoint.
| | 00:51 | We know this circle
needs to be .419 in diameter.
| | 00:54 | I'm going to enter that into the heads-up
display and hit Enter on my keyboard to create
| | 00:58 | that dimension and the circle at the same time.
| | 01:01 | We can now finish this sketch, and
we're ready to make our second Extrusion.
| | 01:04 | From the Marking menu, I can
right-click and select Extrude.
| | 01:08 | I can select the circle we just drew, and in
the heads-up display I'm going to enter a value.
| | 01:13 | In this case, this boss needs to be .278 tall.
| | 01:17 | Now in the previous Extrusion, we chose to
make it symmetric, in this case however we
| | 01:21 | can just use Extrusion to a distance,
which is actually the default for the command.
| | 01:25 | With that value entered, we can hit the
check box and our Extrusion is created.
| | 01:29 | You can see it here in the browser.
| | 01:30 | Next, we're going to use that Extrusion that we just
created as a starting point for the third Extrusion.
| | 01:35 | We're going to select the top face, create a
sketch, and this time we're going to create
| | 01:39 | a circle, lock it to the center of the
previous circle, and set its diameter to .462.
| | 01:48 | Hitting Enter on the keyboard
accepts the entry and creates the circle.
| | 01:52 | Now we can finish this sketch,
and we're ready to extrude again.
| | 01:56 | Right click to bring up the Marking menu,
select Extrude, and this time you can select
| | 02:00 | both circles that were created.
| | 02:02 | The first one was from the Projected
Geometry and the second one was the one we created.
| | 02:06 | We want to extrude both of those.
| | 02:08 | Now you'll notice the Extrusion
is facing in the wrong direction.
| | 02:11 | In this case, we want to
make a little lip on this boss.
| | 02:14 | To change the direction from heads-up display,
we can simply select the direction icon and
| | 02:20 | select the opposite arrow
that is being displayed.
| | 02:23 | You'll notice when we do this,
it changes to a cut operation.
| | 02:26 | You can tell this from the red preview which
indicates that material is going to be removed.
| | 02:31 | In this case, we want to actually add material.
| | 02:34 | So from the heads-up display,
we can choose to join material.
| | 02:38 | The next problem we have is that it's remembering
the .278 that we used in the previous Extrusion.
| | 02:43 | In this case, we need to change this to .128.
| | 02:47 | You'll now see that we have a lip, it's
the proper dimension, it's the proper height,
| | 02:51 | and we can now hit the check mark to accept
this, and we have our third Extrusion created.
| | 02:56 | The next several Extrusions are going
actually take place on the bottom of this part.
| | 03:00 | We can use the ViewCube to rotate to
be able to see the model from below.
| | 03:05 | We can right-click and from the Marking menu,
select New Sketch and then select the face
| | 03:09 | on the bottom of the part.
| | 03:11 | It rotates into a normal view so that we can
see the sketch, but this one's going to start
| | 03:15 | a little bit differently.
| | 03:16 | We're going to return to our Home view,
and we're going to project the circle that we
| | 03:21 | created in the second Extrusion to this sketch.
| | 03:24 | The reason for that is we know they're identical, we
know that they're perfectly aligned in the same diameter.
| | 03:29 | So rather than create a completely new sketch,
we're going to add intelligence by telling
| | 03:33 | the system that we want to project an
existing piece of geometry into the sketch, and by
| | 03:38 | clicking on that we can then rotate around
to look back at our sketch, and you can see
| | 03:43 | the new piece of geometry has been created.
| | 03:46 | We can get out of that command,
and that's all we need to do.
| | 03:49 | Because the geometry was projected, it's
actually being controlled by another feature.
| | 03:53 | We can simply finish the sketch, use the Marking menu
to launch the Extrude command, and select that circle.
| | 03:59 | In this case, we know the distance is .404.
| | 04:01 | We'll enter that, and we'll hit Enter
on the keyboard to accept that value.
| | 04:05 | We now have Extrusion 4 listed in the
browser, and we're ready to continue on.
| | 04:10 | The next two extrusions
are an extension of this one.
| | 04:13 | We're going to start a new sketch from the
Marking menu, select the bottom face that
| | 04:17 | we just created, and we can create a new circle
to represent the lip on the bottom of this part.
| | 04:24 | In this case, it's .485 in diameter, I will
enter that on my keyboard and hit Enter, and
| | 04:30 | we're ready to finish this sketch.
| | 04:32 | With the sketch finished, we'll return to our
Marking menu and launch the Extrude command,
| | 04:37 | select both profiles, and in this
case extrude them to a depth of .033.
| | 04:41 | Hitting Enter on the keyboard
accepts, and we have another Extrusion.
| | 04:45 | We have one final Extrusion
on the bottom of this part.
| | 04:47 | The process is identical.
| | 04:49 | We're going to create a new sketch, select
the face we want to sketch on, from the Marking
| | 04:53 | menu, we're going to bring up the Circle
command again, walk to the center point, and this
| | 04:58 | time we're going to create a
circle with a diameter of .390.
| | 05:03 | We can finish the sketch and from the
Marking menu, again launch Extrude and select the
| | 05:09 | circle we just created.
| | 05:10 | This time we're going to
extrude to a distance of .345.
| | 05:14 | Hitting Enter on the keyboard accepts that,
and we can return to our Home view and see
| | 05:18 | where we stand in with this part.
| | 05:20 | The final two extrusions we need to create are
actually going to be created on the backside of the part.
| | 05:24 | I'll use my ViewCube to rotate into a better
view for this, and we can start a new sketch.
| | 05:29 | I'm going to select the face I want to sketch on,
in this case we're going to use some geometry
| | 05:34 | to center this part.
| | 05:35 | We're going to create a line and connect it
from corner to corner on the projected edges.
| | 05:39 | We're going to finish that command,
and we're now ready to add our boss.
| | 05:44 | We're going to right-click and select Circle
from the Marking menu, we'll lock to the midpoint,
| | 05:48 | and we'll set the dimension for this to be .45.
| | 05:51 | Hitting Enter on the
keyboard creates the geometry.
| | 05:54 | We can then finish the sketch, from the
Marking menu, launch the Extrude command and select
| | 06:00 | the circle we just created.
This actually brings up a good point.
| | 06:04 | Now while I was selecting that, because I
didn't turn that line that we were using as
| | 06:08 | construction into construction geometry, the
Extrusion command is finding that, and it's
| | 06:12 | creating closed profiles because of it.
| | 06:15 | So rather than accept this, we're going to
hit Escape, we're going to go back and edit
| | 06:19 | the sketch by selecting a piece of the geometry,
and from the heads-up display, select Edit Sketch.
| | 06:25 | At any point when you're doing extrusions
or any other modeling action, if you find
| | 06:29 | that there is a piece that you need to make
changes to, you can always return and make edits.
| | 06:33 | I'm going to select that line, right-click and
select Construction, and then finish the sketch.
| | 06:41 | This time when we launch the Extrude command,
the command is actually ignoring that line,
| | 06:46 | making it very simple to
select the extrusion that we need.
| | 06:49 | In this case, the extrusion
needs to be to a depth of .09.
| | 06:52 | We'll hit Enter on the keyboard,
and we've created our Extrusion.
| | 06:56 | The final extrusion builds
off of the one we just created.
| | 06:58 | We'll select the face on the model and use
the heads-up display to create a new sketch.
| | 07:03 | Next, we're going to draw another circle,
and we're going to give it a dimension of
| | 07:08 | .548, hit Enter on the keyboard to create
that, and we're going to finish the sketch.
| | 07:14 | For the final extrusion, we need to select
both profiles, flip the direction by selecting
| | 07:20 | the opposite arrow that's being displayed, set the
operation from Cut to Join, and adjust the dimension.
| | 07:26 | In this case, it's going to be .027.
| | 07:29 | Hitting Enter on the keyboard accepts our
entries, and we can return to our Home view
| | 07:33 | to look at our final part.
| | Collapse this transcript |
| Creating a cone by revolving| 00:00 | In this movie we are going to be
focusing on the Revolve feature.
| | 00:03 | To refresh, I have the Carburetor Housing open so
that we can see the features we're going to be creating.
| | 00:08 | In this movie we're going to focus on the
Revolve and the Extrusion that are extending
| | 00:12 | from the right side of the part.
| | 00:15 | This time rather than starting by sketching
on a face in the part we're going to return
| | 00:19 | to the origin geometry, which we
spoke about in an earlier movie.
| | 00:23 | When we created the base extrusion, Extrusion1,
we took special care in how we created that
| | 00:29 | extrusion, we used the center-point rectangle, and we
extruded in a symmetric way in both directions evenly.
| | 00:35 | Because of that our Origin Planes are located
directly in the center of this part, and now
| | 00:39 | we are able to use them to
create the Revolve feature.
| | 00:42 | If you open the Origin folder in the
browser and hover over the planes you can see them
| | 00:46 | highlighting in the Graphics window.
| | 00:48 | We're going to start by
sketching on the XZ Plane.
| | 00:51 | Once we've selected in the browser the heads-up
display allows us to create a sketch on that plane.
| | 00:55 | I'm going to use my view Cube to rotate the
model into a view that I prefer, and we're
| | 01:00 | ready to begin sketching.
| | 01:01 | One of the things you'll notice is
we're sketching in the center of this part.
| | 01:04 | In order to get better visibility of this
sketch we're going to right-click in the Graphics
| | 01:08 | window and select Slice Graphics.
You could also hit F7 on your keyboard.
| | 01:13 | That temporarily removes the top-half of the part
so that we can clearly see what we are sketching on.
| | 01:18 | To begin creating the geometry for the Revolve we're
going to project one of the edges from the existing part.
| | 01:24 | In the Sketch tab you can select the
Project Geometry button, and we'll select the edge
| | 01:28 | on the right side of the part.
| | 01:30 | You'll notice the yellow line is created
because that geometry is now projected into the sketch
| | 01:34 | and available for use.
| | 01:36 | Because it's projected geometry it is
linked to the edge that it was projected from.
| | 01:40 | If this part were to change
this line would change with it.
| | 01:43 | To start creating our geometry we'll use the
marking menu to select the Line command, we'll
| | 01:48 | lock the initial point of the line to the
midpoint of the line we just projected, and
| | 01:52 | we'll draw our basic shape.
| | 01:55 | We'll complete the shape by connecting back
to the projected edge that we just created.
| | 02:00 | Now that the shape is
complete we can begin dimensioning.
| | 02:02 | I'm going to zoom in a bit so that we
can clearly see what we're working on.
| | 02:05 | I'm going to right-click to bring up the
marking menu and enter the Dimension command.
| | 02:09 | I'm going to select the first line we
created and give it a value of 0.322.
| | 02:14 | Hitting Enter creates the
dimension and updates the geometry.
| | 02:17 | You notice the geometry did change a little bit, but
that's okay because the important components remain.
| | 02:22 | What's important here is that the lines
stayed connected to the projected edge so that we
| | 02:26 | can create a close profile for our Revolve.
| | 02:29 | Now we're still in the Dimension command we'll
select the endpoint of the shape and the horizontal
| | 02:34 | line that we originally created,
and give it a value of 0.252.
| | 02:40 | That locates where the end of the shape touches
the projected edge, and we can finish by providing
| | 02:45 | a height to the end line.
In this case, we're going to enter 0.163.
| | 02:49 | We now have all the geometry we need, it's
been fully constrained and fully dimensioned,
| | 02:53 | and we're able to finish the
sketch and start the Revolve command.
| | 02:57 | From the marking menu you can right-click
and select Revolve, and because there was
| | 03:02 | only a single profile, the system
automatically selected that for you.
| | 03:06 | You'll notice in the heads-up
display it's moved to Axis.
| | 03:09 | The system is now looking for you
to select an axis to revolve around.
| | 03:13 | We're going to select the original line we
created as the center-point for this Revolve.
| | 03:17 | The default settings for the
Revolve are very similar to Extrude.
| | 03:21 | If we wanted to we could add material
through Join, we could cut material away with the
| | 03:26 | Cut option, or we could create an intersection
between two solids with the Intersect option.
| | 03:31 | Because the default is Join, and that's
what we want to do, we'll leave it there.
| | 03:34 | Similar to the Extrude command we do
have different termination options.
| | 03:38 | We could choose to select a specific angle,
we could also grab the arrow on the heads-up
| | 03:42 | display and adjust that angle.
| | 03:45 | Simply by dragging on the screen you can
see the angle adjusting in the background.
| | 03:49 | For this specific revolve we actually do want
the full revolve, so we'll go ahead and select
| | 03:53 | the Full option to
completely revolve 360 degrees.
| | 03:58 | Because the preview looks the way we want
it to we can simply click the check mark to
| | 04:01 | accept the settings and create our Revolve.
| | 04:05 | As I mentioned earlier in this movie we
were going to create two features, the first is
| | 04:08 | Revolve and the second is an Extrude.
| | 04:11 | Similar to the way we started the Revolve, in this
case, we're going to use the origin planes again.
| | 04:16 | By hovering over the planes in the browser
we can see in the Graphics window what they
| | 04:20 | look like and select the proper one.
| | 04:22 | In this case, we're going to select the XY
Plane, and we're going to use the heads-up
| | 04:25 | display to create a new sketch.
| | 04:28 | Similar to the one when you were creating
the revolve part of the geometry is in the way.
| | 04:32 | We're going to use F7 on our keyboard to
slice the graphics away to begin this sketch.
| | 04:37 | We're also going to project an edge that
we're going to use as a starting point.
| | 04:41 | From the Sketch tab we're going to select
Project Geometry, and we're going to select
| | 04:45 | the end of the revolve we just created.
| | 04:47 | The extrusion we're about to create needs
to be centered, and we're going to use a line
| | 04:51 | to lock it to the midpoint of the
projected geometry we just created.
| | 04:55 | In this case, we know that the center of
the circle needs to be 0.168 inches away from
| | 05:00 | the projected edge, enter that into the
heads-up display and hit Enter on our keyboard.
| | 05:04 | We can then hit Escape on our keyboard to
get out of the command, and we can use that
| | 05:08 | geometry that we just
created to center our extrusion.
| | 05:11 | We're going to right-click and from the
marking menu select the Circle command.
| | 05:15 | Lock the center of the circle to the endpoint
we just created and enter a diameter of 0.175
| | 05:20 | for the size of our circle.
| | 05:22 | Hitting Enter on the keyboard will accept
that, and you'll notice that all the geometry
| | 05:25 | is fully constrained.
| | 05:26 | We can now finish the sketch
because we're ready to extrude.
| | 05:30 | Now when we finish that command the Slice
Graphics went away because it allows us to
| | 05:35 | select geometry through the part, we can
still launch the Extrude command and hover over
| | 05:39 | where the circle is inside
the part to select that profile.
| | 05:43 | By default, the value entered is one inch,
which is a little too long for our design.
| | 05:47 | In this case, our extrusion actually needs
to be 0.375 inches long, and I'll enter that
| | 05:53 | into the heads-up display,
and we're ready to extrude this.
| | 05:57 | Simply checking the check box will create
the feature, and let's go ahead and use the
| | 06:01 | Visual Styles to enable the edges.
| | 06:04 | So you can see a little more
clearly what our part looks like.
| | 06:06 | We've now completed the Part Extrusions and
the Part Revolves, and we're ready to move
| | 06:10 | on to other features within this model.
| | Collapse this transcript |
| Creating holes| 00:00 | The next feature we're going
to look at is the Hole feature.
| | 00:03 | Inventor has two different types of features.
| | 00:05 | Sketch features, like the Extrude and Revolve,
and Placed features, like the Fillet and Chamfer.
| | 00:11 | The Hole feature actually falls in the middle
because you can use either method to create holes.
| | 00:15 | This part requires four holes to be added.
| | 00:17 | The first one is a flat bottom hole, the next
two run completely through the part, and the
| | 00:22 | final one is a threaded hole.
| | 00:24 | While creating the holes I'll use both the
Placed method and the Sketched method so that
| | 00:28 | you can see how each work.
| | 00:30 | They both create identical geometry so it's up to
you as the designer to determine which you prefer.
| | 00:35 | The first hole we're going to create is on
the back of the part, and it's concentric
| | 00:38 | to one of the earlier extrudes we created.
| | 00:40 | To create the hole we're going to use the
marking menu by right-clicking in the graphics
| | 00:44 | area and selecting the Hole command.
| | 00:47 | Within the Hole dialog box there is a bunch of
different options that let you build intelligence into the hole.
| | 00:52 | In a lot of cases if you were simply going
to create a through hole you could draw a
| | 00:55 | circle and extrude simply cutting material
away, but you'll lose some of the intelligence.
| | 01:01 | This becomes more important as we get to
things like threaded holes, but even on this first
| | 01:05 | hole we have an option that simply
extruding wouldn't allow us to do.
| | 01:09 | We can choose the type of endpoint,
perhaps we're going to use a drill, perhaps we're
| | 01:13 | going to have a flat bottom hole.
| | 01:15 | The Hole dialog actually allows you to determine which
you're going to use and build that into the Hole geometry.
| | 01:22 | Within the dialog box there is a Placement
option, within that dropdown list you have
| | 01:27 | a few different options, From Sketch,
Linear, Concentric, and On Point.
| | 01:32 | In this case, we're going
to create a concentric hole.
| | 01:35 | By selecting the Concentric option some of
the dialog changes because the type of input
| | 01:39 | required for this hole also changes.
| | 01:42 | Inventor tries to walk you
through the dialog box as you go.
| | 01:45 | After we've picked Concentric it automatically
highlighted the Plane option because it wants
| | 01:50 | to know what plane you
want to place the hole on.
| | 01:53 | If we hover over the face on the model and
left-click you can see a preview of the hole
| | 01:58 | is created, but at this
point it's not concentric.
| | 02:00 | In the dialog box you'll notice that Inventor
already moved us to the Concentric Reference.
| | 02:05 | It's now asking what face or what circle
we'd like our hole to be concentric to.
| | 02:09 | By selecting the circular edge on that face
the system aligns the center points, and you
| | 02:15 | can see that this hole is now
perfectly aligned to go through this part.
| | 02:18 | The hole however is not
required to go all the way through.
| | 02:22 | Within the dialog box we have
different types of termination.
| | 02:25 | This hole isn't a Through All
hole, it actually has a distance.
| | 02:29 | Within the Termination dropdown you can
choose Distance, Through All, or to a specific face.
| | 02:34 | Here we're going to select a specific distance, and by
doing so we're enabling other features within the dialog.
| | 02:40 | By selecting a specific distance the
Drill Point options have become enabled.
| | 02:45 | We're going to go ahead and select the Flat
drill point and then we can turn our attention
| | 02:48 | to the depth and to the diameter.
| | 02:51 | This hole is required to be 0.417 in
diameter and only go to a distance of 0.663.
| | 02:58 | As we update the dialog box, you'll notice
the preview on the screen is also being updated.
| | 03:03 | If we orbit you can see that preview, the
red indicates that we're cutting material away.
| | 03:09 | At this point the hole looks correct,
and we are ready to accept these entries.
| | 03:13 | We can either hit OK in the dialog box or
click the OK button in the heads-up display
| | 03:17 | to accept this entry and create our first hole.
| | 03:20 | You can see that the hole has been placed
in the browser at the bottom of the tree.
| | 03:24 | The next hole we'll be creating is on the
top of the part and is a Through All hole.
| | 03:28 | Again, from the marking menu we
can right-click and select Hole.
| | 03:32 | I'm going to go ahead and create
this hole as a concentric hole.
| | 03:36 | So from the Placement menu I'm going to select
Concentric option, and Inventor automatically
| | 03:40 | jumps and asks what plane
I'd like to place my hole on.
| | 03:42 | I'm going to go ahead and
select a face on the top of the part.
| | 03:46 | It now wants to know what edge or what
cylindrical face to become concentric to.
| | 03:51 | I'm going to go ahead and select the cylindrical
face around the top of the boss, and I'm going
| | 03:56 | to set the diameter to 0.375.
| | 03:58 | By doing so the preview shows that the
whole fits within the face that it's been placed
| | 04:03 | on, but you'll also notice that it
remembers the previous settings we had, including a
| | 04:07 | flat bottom drill point and a
termination to a specific distance.
| | 04:11 | As I mentioned this was a Through All hole,
so rather than terminating a specific distance
| | 04:15 | I'm going to select the Through All option.
| | 04:18 | By doing so you can see the preview update
and the hole extends completely through the
| | 04:22 | part, because this appears the way we wanted
to we can simply click OK in the dialog box
| | 04:27 | to accept that entry, and if we orbit, you'll
notice that the hole goes completely through
| | 04:31 | the part, intersecting the
previous hole that we created.
| | 04:34 | This is exactly what we want, so
we're ready to continue to our next hole.
| | 04:38 | As I mentioned earlier in the movie there
are two different ways to place holes, using
| | 04:42 | the Placed method which we've used on the first two
holes and through a sketch which we have not done.
| | 04:48 | Since the last hole was a Through All hole
and the next hole we're creating as a Through
| | 04:51 | All hole, I'll use this opportunity
to use the Sketch method for this hole.
| | 04:55 | To begin we start just like
we were creating an extrusion.
| | 04:58 | We'll right-click and select New Sketch, pick
the face we want to sketch on, and the edges
| | 05:03 | from that face are projected to the sketch.
| | 05:06 | Because it's a cylindrical face, and we know
we want it centered we have a perfect center
| | 05:10 | point to start from.
| | 05:11 | All we need to do now is finish this
sketch and launch the Hole command.
| | 05:15 | From the Marking menu select Hole, and you'll notice
that our Placement option in the dialog box has changed.
| | 05:21 | Because there was an unconsumed sketch at
the bottom of the tree the system automatically
| | 05:25 | defaulted to use that sketch.
| | 05:27 | If we wanted to we could change that option,
say for example, back to Concentric, but
| | 05:32 | in this case we do want to leverage that sketch.
| | 05:34 | The system automatically asks what center
points we want to use, and we can simply click
| | 05:39 | the center point of the
projected circle to create our hole.
| | 05:42 | Last, we need to set the diameter for this.
| | 05:45 | It remembers the previous diameter, but in
this case we wanted to check 0.268 as our
| | 05:50 | size for this hole.
| | 05:52 | It's set to be a Through All hole so we're ready,
and we can click OK to accept these settings.
| | 05:57 | If we rotate around a bit you can see that
this part goes all the way through, punching
| | 06:01 | a hole in the bottom of our flat
bottom hole that we initially created.
| | 06:05 | This is exactly what we expected and what
we need for this design, so we can return
| | 06:09 | to our Home view and
prepare for our final hole.
| | Collapse this transcript |
| Creating a threaded hole| 00:00 | To create the final hole, we'll begin the same
way we did in the previous holes, by right-clicking
| | 00:05 | and selecting Hole from the Marking menu.
Rather than using the Linear Placement option
| | 00:09 | that has defaulted in the dialog box,
| | 00:11 | we're going to return to our Concentric option.
It automatically jumps forward and asks us
| | 00:15 | what Plane we want to place the hole on,
and I'll select the top of this boss.
| | 00:19 | Now you notice it has picked up the
previous diameter so that when I'm asked to select
| | 00:23 | the Concentric reference I can't select the
top of this hole or the face of this boss.
| | 00:28 | Typically we would just simply change the
diameter to a smaller size so that it fits
| | 00:32 | on that face, but in this
case we're using a threaded hole.
| | 00:36 | So what I am going to do is move to the
bottom of the dialog box where we can define what
| | 00:39 | type of hole is being created.
| | 00:41 | By default, it starts with a Simple Hole,
you also have the option for Clearance Holes,
| | 00:45 | Tapped Holes, or Tapered Tapped Holes.
For this design we need to create a Tapped Hole.
| | 00:51 | By selecting this option an entirely new
section of the dialog box has been enabled.
| | 00:55 | Below you can see Threads, these are the
Threads listed in the engineering handbook so that
| | 01:00 | you don't have to look this up.
| | 01:02 | We know that the size of the hole that we're
creating is going to be drilled with a number
| | 01:06 | eight drill type.
| | 01:07 | By selecting that the Designation for the
Threads automatically changes to 8-32 UNC
| | 01:13 | which is appropriate for our design.
| | 01:15 | We also have other options, but because the
default is what we need, we'll leave it as it is.
| | 01:20 | Now that we've set this option you'll notice that we
have the ability to select that Concentric Reference.
| | 01:25 | But because we had to move to this section,
we do have to tell the dialog box we're ready
| | 01:29 | to make that selection.
| | 01:31 | You'll notice that the plane has already
been selected, and because that's the case the
| | 01:36 | icon has changed to a white.
| | 01:38 | Anything red in the dialog box indicates that
there is input required still, so by clicking
| | 01:43 | on the Concentric Reference icon I am telling
the system I'm ready to make that selection.
| | 01:48 | I can then hover over the cylindrical
face or edge to walk that hole into position.
| | 01:54 | Now we are almost ready to continue.
| | 01:56 | The one remaining component that we
haven't talked about was the type of termination.
| | 02:00 | As I mentioned when we were starting this hole,
this hole does not go all the way through the part.
| | 02:05 | But if we rotate a bit you can see from the
preview that in its current state it's expected
| | 02:11 | to run all the way through the part.
| | 02:13 | The way we can fix this is
through the Termination options.
| | 02:16 | We've used Distance already, we know this
isn't a Through All hole, and we're going
| | 02:20 | to use the To option.
| | 02:22 | What this allows me to do is select a
specific face that I want that hole to terminate on.
| | 02:27 | By selecting that face, you'll notice that
this hole does not continue all the way through
| | 02:31 | the part, and we can click
OK to apply these settings.
| | 02:34 | If we rotate back to a Home view and zoom
in a bit you can actually see this hole has
| | 02:39 | thread representations built-in to
indicate that it is a threaded hole.
| | 02:46 | As we rotate around you can see that the
hole extends through to the first face, but it
| | 02:50 | does not continue through the entire part.
| | 02:53 | At this point you've seen a few different
ways to create holes and should have a solid
| | 02:57 | foundation of how to create them and why the dialog
box adds so much intelligence when creating holes.
| | Collapse this transcript |
| Using placed features| 00:00 | The next set of features we'll be looking at
are the Placed Features Fillet and Chamfer.
| | 00:04 | These are Placed Features because they do
not require a sketch, but instead require
| | 00:08 | a part edge to be created.
| | 00:10 | Fillets and Chamfers at their most basic
level are quite simple, but as parts become more
| | 00:15 | advanced, can add an additional level of
complexity when editing or changing parts.
| | 00:20 | Because of this, it's good practice to save
Fillets and Chamfers to the end of the part
| | 00:24 | modeling process like we've done in this
part unless the design absolutely requires it.
| | 00:30 | Creating Fillets and Chamfers is quite simple,
by selecting any edge on the part the heads-up
| | 00:34 | display provides two different options. One
being the Fillet, the rounded O corner, and
| | 00:39 | the other being chamfer, the one
that's sliced off in a flat surface.
| | 00:42 | We're going to start by
creating several Fillets.
| | 00:45 | Once we select the Fillet option the heads-up
display changes to show a preview of our result.
| | 00:50 | We can then continue selecting edges that
we want to Fillet and the preview updates
| | 00:56 | to show that change.
| | 00:58 | The heads-up display also provides a
simple way to change the radius for the Fillet.
| | 01:03 | By left-clicking and dragging on the arrow,
you'll notice the radius changing on the screen.
| | 01:08 | Releasing the mouse button updates the
preview so that you can see the result.
| | 01:12 | If, for example, you get some type of warning or see
red, it's an indication that the Fillet can't be solved.
| | 01:18 | As long as you release the mouse button and
can still see the preview and then it will
| | 01:22 | be able to solve the Fillet
and place it on your model.
| | 01:24 | In this case, the 0.125 radius that we have
here is perfect, and I'll go ahead and accept
| | 01:29 | these settings by checking the
OK box in the heads-up display.
| | 01:33 | We can rotate around the model a little bit,
and you can see the rounded edges have been
| | 01:36 | applied to the model.
| | 01:40 | The design we're creating actually calls for
Chamfers, so in this case we're going to delete
| | 01:45 | the Fillet from the browser and
return to the state it was at previously.
| | 01:51 | We can now create Chamfers in the exact same
way, I'll walk through the process one more
| | 01:55 | time so you have a better understanding.
| | 01:57 | By selecting any part edge, the heads-up display gives
you the option to creating other Fillets or Chamfers.
| | 02:03 | This time I am going to create a Chamfer, it
looks nearly identical to the Fillet rather
| | 02:07 | than being rounded it's simply sliced off
at an angle, and I can continue selecting
| | 02:12 | edges in the same way I did
when I created the Fillet.
| | 02:15 | Again, I get the same heads-up display
option for clicking and dragging my arrow to see
| | 02:19 | a preview, and in this case the 0.125 is
perfectly fine for the design so I'll go ahead and click
| | 02:25 | the OK check box to apply these settings.
| | 02:28 | Now as we rotate the part, you can see
that the Chamfer has been applied to the model.
| | Collapse this transcript |
| Editing part features| 00:00 | Now that we have a completed part, I wanted
to step back for a minute and talk a little
| | 00:04 | bit about editing those features.
The one constant in design is change.
| | 00:08 | After completing a part like this, it's
common practice to create a prototype or an initial
| | 00:13 | part, maybe do some analysis or testing,
and determine whether or not the design works.
| | 00:18 | More often than not, it turns
out that changes need to be made.
| | 00:21 | The beauty of Autodesk Inventor is that you
can go back and make changes to any of the
| | 00:25 | sketches or any of the modeling
features that you used to create this part.
| | 00:29 | In the browser, you see the list of features we've
created, Extrusions, Revolves, Holes, and Chamfers.
| | 00:35 | The sketched features, which are indicated by
the plus symbol, show both the extrusion
| | 00:40 | or the modeling future that we created,
and the sketch that was used to create that.
| | 00:45 | When you create the modeling feature, the sketch
gets consumed and linked to that modeling feature.
| | 00:50 | Say, for example, our first change was to go back
and make a modification to the original base sketch.
| | 00:56 | If you hover over the extrusion in the browser
and right-click, you have the ability to edit
| | 01:01 | the sketch that's driving
it or the feature itself.
| | 01:04 | We're going to start by editing the sketch.
| | 01:07 | When you do that, Inventor put you back in
the sketch environment, and you can make changes
| | 01:10 | to the sketch as if it were
the first on you are creating it.
| | 01:14 | If we double-click a dimension, we can
change its length to 1 and the geometry updates.
| | 01:20 | If we finish the sketch, the model
geometry updates to reflect that change.
| | 01:25 | We could also go back, and make
changes to the feature itself.
| | 01:28 | If you right-click on the feature in the browser,
rather than selecting Edit Sketch, we can edit the feature.
| | 01:34 | Here, you can see we have the option to reset any of
the settings that were used when creating this feature.
| | 01:39 | Rather than Symmetric, we could
change the direction of this extrusion.
| | 01:43 | Now I am not going to make that change
because I know we specifically picked Symmetric so
| | 01:47 | that we can use the origin geometry
to create other features in this model.
| | 01:51 | However, we could change
the height of this model.
| | 01:54 | We could change it to 1 inch as well.
| | 01:56 | By applying these changes,
the model immediately updates.
| | 01:59 | One of the things we'll notice is that because this part
got bigger, this boss didn't change, but it needed to.
| | 02:05 | If you remember, when we created this boss,
we dimensioned it from this edge of the part,
| | 02:11 | and it's maintained that relationship.
That boss is Extrusion 2 in our browser.
| | 02:16 | If we hover over it and click the plus
symbol, you can hover over the sketch just
| | 02:20 | to quickly review that sketch.
| | 02:21 | In this case, I can see the 0.319 here, and
I know this is something I want to change.
| | 02:26 | Instead of making the change from within the
browser, this time I want to show how to use
| | 02:30 | the heads-up display to make this change.
| | 02:32 | If I select this face in the graphics window, the
heads-up display provides two different options.
| | 02:38 | Just like in the browser, I have the ability
to edit the extrusion, or I have the ability
| | 02:42 | to edit the sketch.
| | 02:44 | By clicking Edit Sketch, I get the same
result as if I would have selected Edit Sketch in
| | 02:48 | the browser, I am returned to the sketch environment,
and I am able to make changes to this geometry.
| | 02:52 | I am going to go ahead and change that 0.319
to 0.6 to accommodate for the change that
| | 02:58 | we made in the base extrusion.
| | 03:01 | By finishing the sketch, you will
notice a couple of things happen.
| | 03:04 | The boss and everything attached to it moved,
but not only that, if we rotate, you'll notice
| | 03:10 | that the boss on the bottom
also moved to reflect that change.
| | 03:14 | If you remember, when we created this bottom
boss, we projected geometry from the top boss,
| | 03:20 | and that intelligence and
relationship has been maintained.
| | 03:23 | If I select this boss down at the bottom
and edit its sketch, you will notice there are
| | 03:27 | no dimensions, but the lines are yellow
indicating that things were projected.
| | 03:32 | Because those two things are linked, the
updates are automatically maintained for you.
| | 03:36 | I am going to go ahead and finish this sketch,
and let's look at this model a little more closely.
| | 03:41 | If we orbit around, there is one item that
I knew was going to happen, and that is when
| | 03:46 | we change that boss, the distance or
depth of this hole has become an issue.
| | 03:53 | Just like a sketched feature, we
can go edit placed features as well.
| | 03:57 | In this case, I am going to select the face
of this hole, and the one option I'm offered
| | 04:01 | is the ability to edit this
feature, or edit this hole.
| | 04:04 | Because it's a placed feature and not driven
by a sketch, the Edit Sketch option is removed.
| | 04:09 | By clicking on that option, we're returned
to the Hole dialog, and we have the ability
| | 04:13 | to make changes to this feature.
| | 04:15 | We could enter a new distance, but rather
than that, I am going to rotate around to
| | 04:19 | the left side and use the heads-up
display to make this change.
| | 04:23 | I know that this hole is required to pass
this boss that we just made a change to.
| | 04:27 | I am going to select the arrow at the end
of the hole, and use the preview to actually
| | 04:30 | see where this hole needs to end.
| | 04:33 | At this point at 0.9755, I can see that it's
passed the boss, and I can accept those changes,
| | 04:39 | and review them in the graphics window.
| | 04:41 | If I orbit around, you now see that the hole
extends past the boss, and the hole that created
| | 04:46 | through it and the model is complete.
| | 04:49 | Now that we've made changes, I think it's
important that you understand that at any
| | 04:52 | point in time during the design process, you
are going to run into times where change happens.
| | 04:58 | That's expected and Inventor
is purposely made for that.
| | 05:01 | At any point in time, feel free to return
to your browser or to your heads-up display
| | 05:05 | to make changes to features to ensure
your parts meet your design requirements.
| | Collapse this transcript |
|
|
5. AssembliesIntroducing assemblies| 00:00 | Up to this point in the course,
we've learned about the interface.
| | 00:02 | We have learned how to sketch and model parts and
the time has come to look at how to assemble the parts.
| | 00:08 | Autodesk Inventor is a tool for digital
prototyping, which means we have the ability to test how
| | 00:12 | or parts fit and function in a digital
format before manufacturing anything.
| | 00:16 | By assembling your parts and testing their
function in the software, you're able to find
| | 00:20 | many mistakes and design errors before
spending any time or money on manufacturing parts.
| | 00:25 | In this chapter we're going to focus on the process
of connecting parts together with assembly constraints.
| | 00:30 | On the screen you can see a portion of the
engine assembly, I've selected a handful of
| | 00:34 | parts so that we can learn how to create and
manage constraints and test some of the moving parts.
| | 00:40 | Here you can see by clicking and dragging
on the crankshaft we can actually see how
| | 00:44 | the piston moves within the engine block.
| | 00:47 | By the time we complete this chapter, you
should have an understanding of how constraints
| | 00:51 | work and be able to begin
assembling your own parts.
| | Collapse this transcript |
| Placing components| 00:00 | In this movie we are going to
begin creating our assembly file.
| | 00:04 | The first step in creating an assembly is
to place components into an assembly file.
| | 00:09 | We can do this by starting a new assembly file.
| | 00:11 | If we go to the Getting Started tab under
the Launch panel, we can click New to bring
| | 00:15 | up the Create New file dialog box.
| | 00:18 | Earlier in the course we talked about file
types, and if you remember we do have the
| | 00:22 | ability to create a couple
different assembly types.
| | 00:25 | We have Weldments, and we
have Standard assemblies.
| | 00:29 | Because we are not creating a Weldment we
are going to select Standard.iam and click
| | 00:32 | Create to begin a new assembly file.
| | 00:35 | On the screen you can now
see our blank assembly file.
| | 00:38 | An assembly file is essentially just a container that
holds the individual parts that are going to be assembled.
| | 00:44 | To begin placing parts into
this assembly, we have two options.
| | 00:47 | We can go to the Assemble tab under the
Component panel and select Place, or we can right-click
| | 00:53 | in the Graphics window and select
Place Components from the marking menu.
| | 00:58 | In the Place Component dialog
box you see our exercise files.
| | 01:01 | We are going to start by
selecting the engine block.
| | 01:04 | The reason for this is the engine block
is the main component of this assembly.
| | 01:08 | Everything attaches to it.
| | 01:10 | So it's the most important component
and makes the most sense to start from.
| | 01:14 | With the engine block selected, we
can click Open to place this file.
| | 01:19 | Now by default Inventor will
automatically place that first component for you.
| | 01:24 | If you notice, as I move my cursor I do
have the ability to add additional versions of
| | 01:28 | this component, but in
this case we don't need that,
| | 01:30 | so I'm going to right-click and
select OK to complete the place process.
| | 01:34 | Now that our component has been placed in
the assembly, you'll notice that we do have
| | 01:37 | the work planes turned on from this part.
| | 01:40 | We don't need that for the assembly, so I
am going to go ahead and go to the view tab
| | 01:43 | and under the Visibility panel select
Object Visibility and uncheck All Workfeatures.
| | 01:49 | This turns them off. I can always return to turn them
back on when needed, but they're out of the way now so
| | 01:54 | we can begin our assembly process.
| | 01:57 | The other thing I am going to do while I'm
on the view tab is turn on my ambient shadows,
| | 02:00 | just so I can see little depth in the model.
| | 02:05 | The other thing you might notice is
the engine block is laying on its side.
| | 02:08 | I am going to quickly reorient the view
cube so that we can have a better visibility of
| | 02:13 | this model and prepare to
place the remaining components.
| | 02:17 | To do this, I am going to orient the
model into an isometric view that I prefer.
| | 02:22 | I am going to right-click on the home
button and from the Set Current view as Home menu
| | 02:30 | select Fit to view.
This resets my default isometric view.
| | 02:34 | Next, I am going to click on the view
that I feel should be the front view.
| | 02:37 | I am going to right-click and from the
Set Current view as menu select Front.
| | 02:43 | Now when I click my Home button, my model is an orientation
that makes sense to continue the assembly process.
| | 02:50 | With the engine block placed into the assembly
you can notice that the browser has been updated
| | 02:54 | to indicate that a part has
been added to this assembly.
| | 02:57 | If I hover over it, you can see a
highlight in the graphics window.
| | 03:01 | The other thing I want to call out here is
the fact that there's a pin icon next to this.
| | 03:05 | The pin icon represents the fact
that this component is grounded.
| | 03:09 | The first component in any assembly
file is going to be a grounded component.
| | 03:13 | We can always change that, and I'll show
you how to do that in a minute, but if I click
| | 03:18 | and drag on this part, you'll notice that I
get the pin icon indicating that this part
| | 03:22 | cannot move because it's grounded.
| | 03:24 | We are now ready to place
another component into this assembly.
| | 03:27 | I will right-click in the Graphics
window and select Place Component.
| | 03:32 | This time from the Place Component dialog
box, we are going to select the crankshaft,
| | 03:35 | we will click Open to place that, and as I
move my cursor the part follows, and I can
| | 03:41 | find a location that makes sense,
left-click, and place that component.
| | 03:46 | Now you will notice I do have the
ability to place the component a second time.
| | 03:49 | I am going to go ahead and do that just so
I can show you what the process is to remove
| | 03:52 | it and explain a little
bit about what that does.
| | 03:56 | Now that I'm finished placing
components, I'll right-click and select OK.
| | 03:59 | In the browser you will notice we'll have two
crankshafts, Crankshaft:1, and Crankshaft:2.
| | 04:05 | These are identical copies
of each other in this model.
| | 04:08 | If I were to change one of these part files,
both would update in the graphics window.
| | 04:13 | Because I don't need the second crankshaft,
I am going to right-click and select Delete,
| | 04:17 | but before we move on, I do want to talk about how
we can place components from the browser itself.
| | 04:22 | Now that we have the crankshaft in the browser,
if for some reason we did need a second one,
| | 04:26 | we could simply click and drag from the
browser into the graphics window, release our mouse
| | 04:32 | button, and place a second version of that item.
Notice we have Crankshaft:1 and Crankshaft:2 again.
| | 04:37 | This is the same as placing the component
twice, but you don't have to use the dialog
| | 04:41 | box to do it the second time.
| | 04:43 | Once you have the parts in the browser, you can
simply drag from the browser to make copies of them.
| | 04:48 | This will save time if you need to do that.
| | 04:50 | Let me go ahead and remove that by right-
clicking on it and selecting Delete so that we only
| | 04:55 | have one crankshaft here.
We are ready to place our next component.
| | 04:59 | I am going to right-click and select Place
Component again from the marking menu, and
| | 05:03 | this time, rather than selecting a single
file, I am going to go ahead and select the crank
| | 05:08 | arm, hold my Ctrl key down on my keyboard,
and select the faceplate, the piston pin,
| | 05:14 | the piston shaft, the piston, and the
pulley shaft, all in one selection set.
| | 05:19 | We left out the crankshaft and engine block
because they're already in the assembly.
| | 05:23 | With those selected I can select Open and
Inventor arranges the parts in an organized
| | 05:28 | fashion and allows me to place them all at once.
| | 05:31 | With those parts placed I can right-
click and select OK to complete the process.
| | 05:35 | You will notice all of the remaining components in
the browser do not have the grounded pin next to them.
| | 05:41 | If from the graphic screen I click and drag on a
part, you'll notice that they're floating in space.
| | 05:47 | If I need to ground one of those components
for any reason, I can right-click on it in
| | 05:51 | the Graphics window and select the
grounded option from the right-click menu.
| | 05:55 | By doing so, you'll notice that the piston
shaft now has a pin next to it, and if I click
| | 06:00 | and drag on it in the graphics
window, I get the pin icon again.
| | 06:04 | At any point I can ground or unground components
as needed, and there will be times while you're
| | 06:10 | assembling simply things that it
makes sense to do that temporarily.
| | 06:12 | I am going to unground that shaft,
because I don't need to have it grounded.
| | 06:17 | I just wanted to show you the process.
By doing so, we can now move it again.
| | 06:23 | With all our parts placed into the assembly, we are
now ready to continue with the assembly process.
| | Collapse this transcript |
| Creating and managing constraints| 00:00 | Now that we've got all our components placed into our
Assembly file, we are ready to begin the assembly process.
| | 00:06 | Before we begin, I wanted to talk a little bit
about the different ways to create constraints.
| | 00:10 | Under the Assemble tab in the Position panel,
there are two different options I want to
| | 00:14 | call out, there is the Constrain
option and the Assemble option.
| | 00:18 | The Constrain option is the default way to
create constraints in Inventor; the Assemble
| | 00:22 | option is a slightly more advanced version
of that, that allows you to create multiple
| | 00:26 | constraints in a single action.
| | 00:28 | I don't recommend this option for those
who are just starting out with Inventor.
| | 00:31 | I think it's important for everybody to
understand what constraints are, how they work, how to
| | 00:35 | edit and manage those constraints, and once
you have that solid foundation, then you can
| | 00:39 | begin exploring the Assemble command.
| | 00:41 | In this movie, we are going to focus on a
couple parts that we'll use to explain how
| | 00:45 | constraints work and how
to edit and manage them.
| | 00:48 | Once we have that foundational understanding, then
we'll move forward with assembling the remaining parts.
| | 00:53 | The parts we're going to be focusing on
are the Piston Shaft and the Engine Block.
| | 00:57 | I am going to zoom in a little bit
on those so we can get a better view.
| | 01:01 | Now I am going to launch the Constrain
dialog box and begin the constraint process.
| | 01:06 | Within the Place Constraint dialog box there is
a few different settings you need to understand.
| | 01:10 | First is the Type Section.
| | 01:11 | There are four major types of constraints
in Inventor: there is a Mate constraint, an
| | 01:15 | Angle constraint, a Tangent
constraint, and an Insert constraint.
| | 01:19 | For this video, we are going
to focus on the Mate constraint.
| | 01:22 | It's the most commonly used constraint, and
once you understand how it works you'll have
| | 01:26 | a solid understanding of how the
other constraints work as well.
| | 01:29 | Next is the Selections area.
| | 01:31 | The whole purpose of constraints in the first place is
to assemble two parts together, or connect those parts.
| | 01:36 | The Selections set area allows you to see
whether or not parts have been selected.
| | 01:40 | A red arrow indicates that nothing has been
selected and Inventor is waiting for an input.
| | 01:45 | A white arrow indicates that a selection has
been made and Inventor is ready to continue.
| | 01:50 | Next we have the Offset section.
| | 01:51 | This allows you to determine the distance
between two faces or two objects that you
| | 01:55 | have connected with a constraint.
We'll go over that in a moment.
| | 01:59 | The Solutions area allows you to select between two
different solutions of the same type of constraint.
| | 02:04 | For example, in the Mate constraint, you
have a Mate option, and you have a Flush option.
| | 02:10 | I'll show those in a minute, because
once you see, it's very easy to understand.
| | 02:13 | To begin, the system is
ready for the first selection.
| | 02:16 | We are going to select the center axis of this
part by hovering over the part and left-clicking.
| | 02:21 | After making that selection, you'll notice
that the Selections set has changed a bit,
| | 02:25 | we now have a white arrow on Selection 1,
indicating that the selection has been made and Inventor
| | 02:29 | is ready to continue at that point.
| | 02:30 | It also move to Selection 2 and
is waiting for us to pick an input.
| | 02:35 | For that item, we are going to select the
center component of the Engine Block, and
| | 02:39 | you'll notice that we receive an audio
indication that the constraint has been made, and we
| | 02:43 | get a preview of the constraint result.
| | 02:45 | At this point we can Apply the constraint
and continue on, or we can select OK to apply
| | 02:50 | that constraint and close the dialog box.
| | 02:52 | That's what we are going to do in this case,
because I want to show you what actually just took place.
| | 02:56 | If we left-click and drag on the Piston Shaft,
you'll notice that as I move my cursor right
| | 03:01 | and left, the component spins, and it can
move up and down, but it remains locked to
| | 03:06 | the center axis of the Engine Block.
That's exactly what the constraints do.
| | 03:10 | They're rules that tell parts how they connect
and how they can interact with each other.
| | 03:14 | The problem we have here is the part is
upside-down, and that happens from time to time and
| | 03:19 | is perfectly acceptable and expected.
| | 03:21 | We are going to go a head and use the Marking
menu by right-clicking and select the Constraint
| | 03:25 | option to bring up the Constraint dialog box.
| | 03:27 | We are now ready to create
a second constraint here.
| | 03:31 | This time rather than selecting the axis,
I'm going to select the bottom face of the
| | 03:35 | Piston Shaft and the top face of the Engine
Block, because I want those two parts connected.
| | 03:40 | Now you'll notice from the preview the part
has remained in the Engine Block but now it's
| | 03:44 | been flipped over and positioned properly.
| | 03:48 | If I zoom in a bit and orbit just a hair, you can
see that these two faces are touching each other now.
| | 03:54 | This is a point I want to show you
the two different Solution options.
| | 03:57 | Right now we have the two
faces touching each other.
| | 04:00 | The Flush option allows me to just flip that
option over, and if I zoom in a bit you can
| | 04:05 | see the two faces are
perfectly flushed with each other.
| | 04:08 | Again, you can toggle back and
forth between these to see the result.
| | 04:11 | I do want to go ahead and continue with the Mate
constraint, so I'll go ahead and leave that as it is.
| | 04:16 | The next item I want to mention
before we continue on is the Offset.
| | 04:21 | The Offset in the dialog box allows you to
determine how far apart the two faces are.
| | 04:26 | For example, if I enter .25, you'll notice
that the preview updates to show that result,
| | 04:32 | if I make it .5, that moves up even further.
| | 04:36 | In this case, I do want to go ahead and
leave it at zero, so I'll return that, and now I
| | 04:40 | am going to click OK to accept
that constraint and close the dialog.
| | 04:44 | Now that we have the part constrained, I am
going to rotate it around and show you one
| | 04:48 | more time what just took place.
| | 04:50 | If we left-click and drag on the part, it
now will rotate, but it won't move up and
| | 04:55 | down because the bottom of the Piston Shaft
and the top of the Engine Block are connected,
| | 05:00 | and the axis of the Piston Shaft and the
axis of the Engine Block are locked together.
| | 05:05 | Now you'll notice as I move this around we
do have an Exhaust port down here, and this
| | 05:09 | is important, because if we rotate around
to the other side, you'll notice that there
| | 05:13 | is corresponding Exhaust port
on the side of the Engine Block.
| | 05:17 | In the Piston Shaft component, you'll also
notice that there's a little notch here.
| | 05:23 | As we drag the component around, you'll notice
a little notch on the top of the Engine Block.
| | 05:28 | The purpose for that is to align the two
components so that the Exhaust Ports match up.
| | 05:33 | So the final constraint we need on this component is
an axis-axis constraint between these two components.
| | 05:38 | I am going to right-click and select Constraint
from the Marking menu, and this time I'm going
| | 05:43 | to select the axis on the Piston Shaft and
the axis on the Engine Block, and those two
| | 05:48 | components align, and now I can
select OK, and that constraint is created.
| | 05:54 | This time if I go to click and drag that part
I get a no-go symbol, essentially it's telling
| | 05:59 | me that there is enough constraints on this,
that it's permanently positioned, and the
| | 06:02 | only way I can move it at this point would
be to remove a constraint or edit an Offset.
| | 06:09 | Now that we've created a few constraints, let's
look at the browser to see what's actually happened.
| | 06:13 | If we expand the Engine Block,
you'll see a couple of things.
| | 06:16 | You see some hidden work planes and then you see the
constraints that have been applied to the Engine Block.
| | 06:22 | Let's zoom back in on the Engine Block
so we can see this in the Graphics Window.
| | 06:26 | If you hover over the first Mate, you'll
see that it highlights in the graphic screen.
| | 06:30 | This is the Mate between the axis of the
Piston Shaft and the axis of the Engine Block.
| | 06:35 | Because there are two components involved
in this constraint, sometimes you might want
| | 06:39 | to find the other half of that constraint or what
part is contained in that other half of the constraint.
| | 06:44 | To do that, you can right-click on the constraint
in the browser and select other half, and
| | 06:49 | you notice the browser expands the Piston Shaft part
and highlights the other half of the Mate constraint.
| | 06:55 | This is just a nice way to find out how
components are interacting with each other, and it comes
| | 06:59 | in handy if you ever run into a problem and you
need to interrogate the model a little bit closer.
| | 07:03 | The next item we have is this Mate here.
| | 07:06 | This is the Mate between the top of the Engine
Block and the face on the bottom of the Piston Shaft.
| | 07:11 | Finally, we have the last Mate we just created,
the axis between the pin and the corresponding
| | 07:15 | notch on the Piston Shaft.
| | 07:17 | At any point we can go back and right-click
on any constraint and make some edits to it.
| | 07:22 | For example, if we wanted to update the offset, we
could go back and hit Edit and change that after the fact.
| | 07:28 | Here we have a .05 offset, we can set that to
.25, and you see the preview updating as well.
| | 07:34 | In this case, we don't want to make that
change so we'll leave it at zero, but you can always
| | 07:38 | go back and make changes.
| | 07:41 | Now that we have a solid understanding of
what constraints are, what they do, how we
| | 07:46 | can edit and manage them, we're ready
to move on and continue assembling parts.
| | Collapse this transcript |
| Assembling parts| 00:00 | Now that we have a solid understanding of what
Constraints are, how they work, and how to manage them,
| | 00:05 | we can continue assembling parts. Before we
get started, in the previous movie we heard
| | 00:09 | an audio indicator, and we saw a
preview when a constraint was applied.
| | 00:13 | A lot of times people find the audio indication
a little disruptive during the design process,
| | 00:18 | so I am going to show you how
to turn that off for this movie.
| | 00:21 | If you go the Application menu and select
Options you can make sure this Assembly tab
| | 00:27 | is selected, and there's a check box that
says Constrain audio notification we are going
| | 00:32 | to unchecked that so that we
can disable that notification.
| | 00:35 | We still get the preview so we can see the constraint,
but the noise won't distract us during the process.
| | 00:41 | Now we are ready to begin constraining parts.
| | 00:43 | I am going to right-click and bring up my
Constraint dialog box from the Marking menu,
| | 00:47 | and I am going to constrain the
Crankshaft to the Engine Block.
| | 00:50 | I am going to that by selecting the center
axes of the Crankshaft and a center axis that
| | 00:56 | runs to the center of the Engine Block.
| | 00:58 | I am going to select OK to apply that
constraint and close the dialog box, and we can now see
| | 01:05 | the Crankshaft slides through the center of
the Engine Block, and it rotates, but it's
| | 01:10 | always locked in position.
| | 01:13 | Next we are going to look at assembling
the Crank Arm and the Crankshaft together.
| | 01:17 | Again, from the Marking menu will select the
Constraint option and here we will zoom in
| | 01:21 | and select the inner axis for the end of the
Crank Arm and pan over and select the Cylindrical
| | 01:27 | Face on the Crankshaft. Now you can notice
we get the preview, but no audio indicator,
| | 01:33 | and we can continue on.
| | 01:35 | I'm going to go ahead and apply this constraint,
and we are ready to move to our next constraint.
| | 01:40 | Before we do that, I'm going to go
ahead and cancel this dialog box.
| | 01:43 | From time to time, it's always a good idea
to get out of the Constraint dialog and just
| | 01:47 | double check some of the motions.
| | 01:49 | You can see here that my parts are starting to
work right together, but they are not quite there.
| | 01:54 | The next company to take is to constrain
the two faces between these two parts.
| | 01:59 | From the Marking menu, I'll select the Constraint option,
and this time I am going to select the face
| | 02:03 | of the Crankshaft and rotate around and zoom
in a bit and select the face on the Crank Arm.
| | 02:09 | The two faces are now touching each other.
If I zoom in from the right, you can see that
| | 02:14 | there is 0 Offset between the two.
| | 02:16 | Before I apply that constraint, because in
the real world these parts are not going to
| | 02:20 | be rubbing up against each other perfectly, I am
going to add a very small gap between the two pieces.
| | 02:25 | I am going to enter .005, and you can see it
update on the screen, and that looks perfect.
| | 02:31 | So we are going to a go ahead and hit OK to
apply the constraint, and now we can now zoom
| | 02:36 | out and begin assembling our next components.
| | 02:38 | In this step we are going to go ahead and
connect the Piston Pin to the Piston Head.
| | 02:42 | So I'll right-click to bring up my Marking
menu and select the Constraint option, this
| | 02:47 | time I am going to select the Cylindrical
Axis through pin, and I'm going to zoom in
| | 02:51 | and select the Axis to hold that pin belongs in.
You can see the preview, and that looks right.
| | 02:56 | I am going to go ahead and click Apply to
accept that, and if you notice, the end of
| | 03:01 | the pin is curved. This is because it's
going to be pressed into the Piston head, and we
| | 03:05 | need to make sure it's properly aligned.
| | 03:07 | So we are going to select the axis on that
curved edge and then the axis on the Piston
| | 03:12 | Head, and the two Parts become connected.
If I click OK, we can see the result.
| | 03:18 | If I click and drag on the Piston Head, these
two components move as one now because they
| | 03:22 | are properly constrained together.
| | 03:24 | If I were to click and drag
the pin, the same action occurs.
| | 03:30 | Now we are ready to a symbol
the Piston Head to the Crank Arm.
| | 03:33 | Let's zoom back out and rotate into a view where it
will give us our best ability to do the constraining.
| | 03:39 | And I'm going to drag the part so that these
two components are near each other, just to
| | 03:43 | make the selection process easier.
| | 03:45 | I am going to right-click to bring up my
Marking menu and select Constrain again, and this
| | 03:50 | time I'm going to select the center axis for
the Crank Arm, and I am going to select the
| | 03:54 | center axis of the pin.
| | 03:57 | I'm going to hit OK to apply those
two constraints and test motion again.
| | 04:02 | If I click and drag the piston head you
can see that it rotates around the Crankshaft,
| | 04:06 | which is what we want it to do.
| | 04:08 | But it is able to float along the axis of the
Crank Arm, and this is exactly what we want.
| | 04:13 | The actual piston position is going to be
defined by the center of the Piston Shaft.
| | 04:17 | We can go ahead and apply that
constraint now so you see what I mean.
| | 04:20 | I am going to right-click and bring up my
Marking menu and select the Constraint option,
| | 04:24 | this time we will select the axis through the
Piston Head and the axis to the Piston Shaft.
| | 04:29 | You'll notice that the two are perfectly
aligned now, but it's slid away from the Crank Arm,
| | 04:34 | and that's okay at this point.
Let me show you what I mean.
| | 04:37 | If I hit click OK to apply that constraint
and close the dialog box I can left-click
| | 04:42 | and drag on the Crankshaft, and as that
component moves you can see the Piston moving up and
| | 04:46 | down in the Piston Shaft.
| | 04:48 | So we are almost there, but we still
have a couple more constraints to finish.
| | 04:54 | Now we are ready to add the Pulley Shaft to
the Crank Arm. I am going to drag this component
| | 04:58 | down so it's a little bit closer to where
we need it to be, and we'll rotate around
| | 05:01 | so that we can see from the other side.
| | 05:03 | I like positioning the components a little bit
closer just to make selections easier from time to time.
| | 05:11 | Now we have the components rotated in the
proper position, and we can right-click to
| | 05:15 | bring up our Marking menu and
select the Constraint dialog.
| | 05:18 | We can now pick the face of the Crank Arm,
rotate around and get the Front Face of the
| | 05:24 | pulley arm, and you can see them
snap into place with each other.
| | 05:27 | I am going to apply that constraint, and
now I have got the faces touching, but I don't
| | 05:33 | have the parts aligned properly.
| | 05:34 | I am going to select the center axis of the
Pulley Arm and the center axis of the Crankshaft
| | 05:39 | to properly position the two components.
| | 05:42 | I can hit Apply and cancel this
dialog box to double check my work.
| | 05:49 | If we zoom in a bit, we notice
there is one thing I forgot.
| | 05:53 | I forgot to add the gap between
the two faces. That's okay, though.
| | 05:58 | I can always go back and edit that constraint.
| | 06:01 | One of the nice features of the Assembly
environment is the ability to right-click on a part and
| | 06:05 | select Find in Browser. This isn't so
important when you only have a few parts,
| | 06:10 | but once you get 100 parts into a browser,
it makes it very easy to find things very quickly.
| | 06:15 | Now that I found the part in the browser, I
can expand it and look for the mate we just
| | 06:19 | created, here it is Mate 11.
| | 06:21 | I am going to right-click on it and select
Edit, and we can now enter our Offset.
| | 06:27 | From the preview, you can see that now we're
matching on both sides, and this is appropriate, so
| | 06:31 | I am going to hit OK and continue on.
| | 06:35 | The last component we need to assemble is the Face
Plate we created during the Part Modeling chapter.
| | 06:40 | We'll go ahead and bring up our Constraint
dialog box from the Marking menu, we'll select
| | 06:45 | the top Face of the boss, and we can rotate
around to select the backside of the Pulley Shaft.
| | 06:52 | In doing so, you can see the preview puts
these two faces together, and that's the way it's
| | 06:56 | supposed to be so we are good there.
| | 06:58 | We're going to go ahead and click OK to accept
that and close the dialog box. At this point, we
| | 07:03 | are nearly complete with our Assembly.
| | 07:08 | The last item we need to do is Align the Face
Plate with the Engine Block, but we are going
| | 07:12 | to do that with an Insert
Constraint in the next movie.
| | Collapse this transcript |
| Understanding the Insert constraint| 00:00 | At this point, we've nearly completed our Assembly.
| | 00:02 | The last step in the process is to align
the faceplate to the engine block properly.
| | 00:07 | We're going to do that
with the Insert constraint.
| | 00:09 | If we right-click in the Graphics window, we can
bring up the Constraint dialog box from the marking menu.
| | 00:13 | Now up to this point we've used the Make
constraint, and in the Type section of the dialog box
| | 00:17 | we want to switch to an Insert constraint.
| | 00:20 | Now an Insert constraint is essentially a
shortcut to creating two Make constraints.
| | 00:24 | Let me show you what I mean.
| | 00:26 | We're going to make our
first selection on the faceplate.
| | 00:29 | We want to align this hole
with the hole on the engine block.
| | 00:32 | What you'll notice is if I hover over this
hole, two items are highlighting, the edge
| | 00:37 | of the hole, and the access through the hole.
| | 00:39 | I am going to go ahead and make this
selection by left-clicking, and we'll rotate to find
| | 00:43 | the corresponding hole on the engine block.
| | 00:46 | The hole we selected on the faceplate
should align with this hole on the engine block.
| | 00:51 | By selecting that edge of that hole, you can see
from the preview that the holes are now aligned.
| | 00:56 | Not only are the holes are aligned,
but the two faces are also touching.
| | 01:00 | If I click OK to accept this, the dialog box
closes, and we can test our function by left-clicking
| | 01:07 | and dragging the faceplate.
| | 01:09 | You'll notice we're rotating around the
axis of the hole, and if we rotate a little bit
| | 01:13 | further up you can see that the
faces are actually touching as well.
| | 01:17 | So essentially we've created two Make
constraints in one action by using the Insert constraint.
| | 01:24 | The final stuff here is to add one more
constraint to align one more hole on the faceplate to
| | 01:29 | one more hole on the engine block.
| | 01:31 | We're going to do that by right-clicking in the
Graphics window and bringing up our Constraint
| | 01:35 | dialog box from the marking menu.
| | 01:37 | This time, rather than using the Insert
constraint, we're going to use one more Make constraint.
| | 01:41 | We're going to select the access through the
hole on the engine block and the access through
| | 01:45 | the hole on the faceplate.
| | 01:46 | By doing so, you can see that the preview is
showing that the parts are properly aligned,
| | 01:51 | and we can click OK to accept
this and close our dialog box.
| | 01:55 | We're going to click on the Home button to
return to our default Isometric view, and
| | 01:59 | now we can begin to test
the motion of this part.
| | 02:01 | If I left-click and drag on the crankshaft,
you'll notice that the piston is moving up
| | 02:05 | and down in the piston shaft.
| | 02:08 | The problem is that you can't
actually see that very well.
| | 02:10 | One of the nice things about the Assembly
environment is the ability to turn the visibility
| | 02:14 | of parts off, but also to enable and disable parts,
and they provide slightly different functionalities.
| | 02:21 | Turning off the Visibility simply removes the
part from the Graphics window, but disabling
| | 02:25 | the part offers something else.
| | 02:27 | If we right-click on a part in the graphics
window and uncheck Enabled, you'll see that
| | 02:32 | the part has become clearer or ghosted, and
in the browser the icon has changed to a green
| | 02:37 | color to indicate that
the part has been disabled.
| | 02:40 | What this means is that I can't select the
part in the Graphics window, but we can still
| | 02:45 | see a ghosted image of it so that we can
understand the context of the assembly.
| | 02:49 | We're going to also do this with the piston shaft by
right-clicking on the part and un-checking Enabled.
| | 02:54 | And we now have a pretty clear view of the
parts inside the model, but we also have a
| | 02:58 | view of the context in which those parts exist.
| | 03:02 | If we left-click and drag on a crankshaft
now you can actually see the motion of the
| | 03:06 | piston in the piston shaft
even inside the engine block.
| | 03:10 | The beauty of this is we're actually able to test the
function of our parts before we actually manufacture anything.
| | 03:16 | This allows us to find design mistakes before we spend
any time or money manufacturing any of these parts.
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|
|
6. DrawingsExploring initial drawing creation| 00:00 | Now that we know how to create parts and assemblies,
it's time to talk about how to document your designs.
| | 00:05 | In order to get a part or an assembly manufactured,
you're almost always going to be required
| | 00:10 | to create a drawing for manufacturing.
| | 00:12 | To create a drawing, we're going to start by
hitting the New button found in the Getting
| | 00:16 | Started tab under the Launch panel.
| | 00:19 | Because IDWs are the default drawing
format in Inventor, we'll select the standard.idw
| | 00:24 | file type, and Inventor will
configure our initial drawing for us.
| | 00:28 | Here on the screen you can
see our initial drawing sheet.
| | 00:31 | This represents the piece of paper that
your views are going to be printed on.
| | 00:34 | On that sheet you can see a border has been
added, and also a title block, and just like
| | 00:40 | parts and assemblies, the browser
represents what you are seeing on the screen.
| | 00:44 | On the left you can see that Sheet 1 has been
created for us, we have a default border that
| | 00:49 | has been added, and a default title block.
| | 00:52 | Above that in the browser you have
a folder called Drawing Resources.
| | 00:56 | This is where Inventor stores all of the
things that you can add to the sheet and also some
| | 01:00 | preconfigured sheet formats that could
help speed the drawing creation process.
| | 01:06 | Sheet formats are
preconfigured layouts for drawings.
| | 01:09 | For example, if you're going to create parts
that are very similar all the time and that
| | 01:14 | require the same types of views, you can lay out
all your drawing views, select the sheet size,
| | 01:19 | lay out the title block and border information,
and save that configuration to the sheet format.
| | 01:25 | That way the next time you go to create a
drawing you can use a sheet format to automatically
| | 01:30 | pre-configure all that information.
Next we have Borders.
| | 01:35 | As I mentioned, when you create a new drawing,
Inventor is going to configure a border for
| | 01:39 | you based on the sheet size.
| | 01:41 | If you don't like the default border that
is being used, you can create your own, or
| | 01:45 | in this case I'm going to just delete the one we
have, and it's removed from the Graphics window.
| | 01:50 | If I simply want to replace the drawing
border and have Inventor preconfigured for me, I
| | 01:55 | can double-click the
default border in the browser.
| | 01:58 | It preconfigures everything
and replaces that drawing.
| | 02:01 | I'm going to go ahead and remove that border one
more time and show you another way to insert a border.
| | 02:07 | Rather than just double-clicking, you can right-
click on the default border and insert a drawing border.
| | 02:13 | This allows you to configure the zones that are
laid out in your border to meet your design needs.
| | 02:18 | I'm going to go ahead and leave the
default settings, and hit OK, but I want to point
| | 02:22 | out where the zones are.
| | 02:24 | For example, if I'm working on a complex drawing,
and I wanted to have somebody review a specific
| | 02:29 | piece of information on the drawing sheet, I
can help them locate the piece of information
| | 02:33 | I'm looking for by telling them
to look in zone D4, for example.
| | 02:38 | You can see here D represents the
rows, and 4 represents the columns.
| | 02:43 | If I tell somebody to look in zone D4,
they're going to look in this area of the drawing
| | 02:47 | for the information we're discussing.
| | 02:52 | If the default borders don't work for you,
you can right-click on the folder and select
| | 02:56 | to define a new border.
| | 02:58 | In most cases you're not going to do that,
and if you do, I would highly recommend speaking
| | 03:03 | with your CAD Manager because often
companies have predefined borders, predefined title
| | 03:08 | blocks, and predefined sheet layouts that
are used on a regular basis in the company.
| | 03:13 | Next, we have Title Blocks.
| | 03:15 | By default, Inventor creates a couple of
different title blocks for you based on the standard
| | 03:19 | you select during install.
| | 03:20 | In this case, we selected ANSI and two
default title blocks were created for us.
| | 03:25 | I'm going to circle back to title blocks in
just one minute. Before I do that, I'm going
| | 03:29 | to talk about how to edit the sheet.
| | 03:32 | One of the things you might need to change
with the sheet is the sheet size, and this
| | 03:36 | is where the title blocks
and sheets are connected.
| | 03:39 | If I hover over the sheet in a browser and
right-click, I have the option to edit this sheet.
| | 03:44 | I can change the name of the sheet, perhaps
I want to name it to reflect the information
| | 03:48 | that's on the sheet, or I
could change the sheet size.
| | 03:51 | Say, for example, I wanted to print this on
an 8.5 by 11 sheet of paper, which is represented
| | 03:57 | by the A sheet size.
| | 03:59 | I could select A from the list and hit OK
and my sheet size changes and my title block
| | 04:05 | is updated to indicate the new sheet size.
| | 04:08 | The one thing that didn't change was the physical size
of the title block in the drawing sheet space itself.
| | 04:14 | We have the ANSI-Large title block listed, and
it's physically a little bit larger for larger sheets.
| | 04:20 | I'm going to go ahead and remove that from
the drawing, and I can return to the Title
| | 04:24 | Blocks folder and double-click my ANSI A to
insert the smaller title block, and you can
| | 04:30 | see that it now takes up
less space on the sheet.
| | 04:33 | Again, just like Borders, Title Blocks can
be configured as well, but I highly recommend
| | 04:38 | talking to your CAD Manager to make sure that you
are following common standards for your company.
| | Collapse this transcript |
| Placing views| 00:00 | On the screen you see our completed
Carburetor Housing, and we're going to use this part
| | 00:04 | as we look at how to work
through the process of placing views.
| | 00:07 | To begin, we need to create a new drawing file.
| | 00:10 | To do that we can select the Application menu,
and then click on New to bring up the Create
| | 00:15 | New File dialog box.
| | 00:17 | We're going to go ahead and
create a Standard.idw file.
| | 00:21 | We'll select that in the
dialog box and click Create.
| | 00:25 | By doing this, Inventor creates our
first sheet in our drawing for us.
| | 00:29 | You can see that it's preconfigured a drawing
border and a title bar on a C size sheet of paper.
| | 00:35 | There are a couple of ways to
begin creating drawing views.
| | 00:38 | The initial view is called the Base view.
| | 00:40 | You can find the Base view under the
Place Views tab in the Create panel.
| | 00:44 | But instead of doing that, I'm
going to use the Marking menu.
| | 00:47 | You can also right-click and select Base
view there to initiate your Base view creation.
| | 00:53 | By doing so, the Drawing view dialog box is
presented, and there's a few things in here
| | 00:57 | that we want to talk about so that we better
understand the process and how to move forward.
| | 01:01 | First, you'll notice a File dropdown list.
| | 01:04 | This lists all the files that are
currently open in the background.
| | 01:07 | In this case, it's just our Carburetor Housing.
| | 01:10 | If you didn't have a file open, you could
select the Open an existing file and select
| | 01:14 | a specific file from your hard drive.
Next we have the Representation section.
| | 01:18 | Now, we didn't create any view representations
for this model, but I wanted to explain very
| | 01:23 | briefly how that would work.
| | 01:25 | If in our engine assembly we wanted to show
a representation of the piston at its fully
| | 01:29 | extended position and a view with it in its
fully retracted position, we could do so and
| | 01:34 | they would be listed here.
| | 01:35 | We can then select one of
those to create a Drawing view.
| | 01:38 | Next we have the Orientation section.
| | 01:41 | The Orientation section lists
several different positions of our model.
| | 01:45 | If I hover over the graphics window, you'll see
a preview of that model in its Front Orientation.
| | 01:50 | We can go back and select a different Orientation
if we need to start from a different position.
| | 01:55 | In this case, I want to start with the front, that
works for me, so I'm going to leave that as it was.
| | 02:00 | The next thing you might notice is the preview
is a little small for the sheet size we have.
| | 02:04 | To change that, we can go to the Scale section
at the bottom of the dialog box, and we can
| | 02:09 | select a different Scale for our drawing.
| | 02:11 | In this case, I'm going to select 2:1, and you'll
notice that the preview updates to reflect that change.
| | 02:17 | The other item I'll mention
is the Style section.
| | 02:20 | We're not going to change this right now, but I want
to call it out because we will later in the movie.
| | 02:25 | The default style is to show Hidden Lines.
| | 02:27 | You also have the ability to show with
Hidden Lines Removed and Shaded views.
| | 02:32 | We're now ready to place our view.
| | 02:34 | I wanted to remind everybody that
we are in our Base view command.
| | 02:37 | I'm going to go ahead and zoom out a bit and
position our sheet so that we can place our Drawing Views.
| | 02:43 | As I move the cursor, the view follows around.
| | 02:46 | I simply need to find the location that works best
for this Drawing view and left-click to place it.
| | 02:51 | In doing so, the dialog box is removed,
and we're moved into the Projected mode.
| | 02:56 | You can see on the Ribbon bar that the
Projected command is highlighted and active currently.
| | 03:01 | I'm going to go ahead and zoom in a bit, or
reposition my view a bit, and as I move my
| | 03:07 | cursor, you'll notice because we're now in
Projected, the cursor is showing previews
| | 03:12 | of what a Projected view would look like.
| | 03:14 | Inventor does this on its own, because the
most logical step after a Base view is to
| | 03:18 | create several Projected Views of that model.
| | 03:21 | All you need to do is simply move your
cursor to the position you wish to place the view,
| | 03:26 | left-click, and a temporary version of
that view is placed on the drawing sheet.
| | 03:30 | As I move my cursor up a little bit
further, I get a preview of an Isometric view.
| | 03:35 | I can left-click to temporarily place that,
and then I can position my cursor above the
| | 03:39 | Base view for a Top view, and I can left-click one
last time to create a temporary version of that view.
| | 03:45 | Now that I have all my views placed, I want
to go ahead and create them and have Inventor
| | 03:49 | actually create the views on the drawing sheet.
| | 03:52 | To do that, you simply
right-click and select Create.
| | 03:55 | If I zoom in a bit, you can see what happened.
| | 03:58 | Inventor created my Drawing Views, and because
the style was Hidden Line, I can see my object
| | 04:04 | lines, I can also see the hidden lines
representing the holes being cut through this part.
| | 04:09 | Now that we have the views placed on the screen, I
want to show a little bit about how they're connected.
| | 04:13 | As I mentioned, we created
a Base view at this point.
| | 04:16 | If I hovered over that, you can see that it
highlights in red, it's also highlighted in
| | 04:19 | the browser as well.
| | 04:21 | It's important to remember that just like
parts and assemblies, the browser in the drawing
| | 04:25 | represents the things are
being shown on the screen as well.
| | 04:28 | If I were to hover over this Drawing view
and left-click and drag, you'll notice the
| | 04:33 | connection between the Base and Projected Views.
| | 04:36 | As I reposition my Base view, the alignment
with the Projected Views remains connected.
| | 04:42 | If you need to change that, in most
cases that's going to be perfectly fine.
| | 04:46 | In certain scenarios you may need to break the
link between the Projected view and its parent view.
| | 04:51 | If you hover over one of the Projected Views
and right-click, in the right-click menu you
| | 04:55 | have an Alignment option, and you can choose to
Break that alignment so that you can reposition
| | 04:59 | it in a location that is not
in alignment with the Base view.
| | 05:03 | In this case, I do want to maintain that
alignment, so I'm going to skip that for now.
| | 05:07 | Before we move on to our next movie,
I wanted to add one more item here.
| | 05:11 | The Isometric view, while not connected to
the Base view, is really there to give better
| | 05:16 | visualization to the other three views.
| | 05:19 | By having an Isometric view, people can more
quickly understand the details that are involved
| | 05:23 | in those other views.
| | 05:25 | Earlier in the movie we talked a little bit
about the Style section of the Create dialog box.
| | 05:30 | If I hover over my Isometric view, right-click
and select Edit view, that dialog box returns,
| | 05:37 | and we can make changes to
some of the initial settings.
| | 05:40 | If I wanted to I could adjust the Scale for
the Isometric view, but in this case I actually
| | 05:44 | want to change the Style.
| | 05:46 | I would prefer to have this view Shaded to
better improve the visibility and understanding
| | 05:52 | of what this design entails.
| | 05:55 | If you zoom in a little bit, you can see
that this with it shaded actually very closely
| | 05:59 | represents the model that we saw
on the screen in the modeling view.
| | 06:05 | At this point, we've created our initial Drawing Views,
and we can move forward with documenting our design.
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| Creating section and detail views| 00:00 | Now that we have our initial views placed, I
want to focus on Section and Detail Views.
| | 00:05 | These are slightly more specialized views,
and there are not used just frequently as
| | 00:09 | Base and Projected Views, but they are used frequently
enough that I want to show you how to create them.
| | 00:15 | Section Views allow you to slice through part
so that you can properly document the inside
| | 00:19 | components of a part.
| | 00:21 | We're going to zoom in and
create a section of this view.
| | 00:24 | There's a couple ways to begin.
| | 00:26 | From the Place Views tab under the Create
panel, we could select Section, and you'll
| | 00:30 | notice in the bottom left-hand corner the Status
bar is telling us to select a view or view sketch.
| | 00:37 | If I hover over the view and left-click,
it tells the system that this is the view we
| | 00:40 | want to create the section from, and we
can continue on creating our section line.
| | 00:46 | I'm going to hit Escape on the
keyboard to cancel this command.
| | 00:49 | The other way to do this is to
actually use the Marking menu.
| | 00:53 | If I hover over the specific view I want to
create a section of, right-click, I can select
| | 00:58 | section from the Marking menu itself.
| | 01:00 | This does two things, it launches the command,
and it selects the view we want to create
| | 01:04 | the section from all in one action.
| | 01:07 | Now that we're in this Section view command, we
need to essentially draw a line that represents
| | 01:12 | where we want the cut to take place.
| | 01:14 | I want is part to be sectioned
right down the middle of this hole.
| | 01:18 | So I'm going to hover over the midpoint of
this top line, and I'm going to use the Alignment
| | 01:22 | Indicator to position my
start point for the line.
| | 01:25 | I'm going to left-click, and as I drag my
cursor down below the part, you'll notice
| | 01:30 | I get a perpendicular
indicator at that location.
| | 01:34 | This is telling me that this section line is
going to remain perpendicular to the initial
| | 01:38 | line that we hovered over to get our midpoint.
| | 01:41 | I'm going to left-click to
place the endpoint of the line.
| | 01:44 | If I wanted to continue on making more sections
and maybe a more advanced part, I could do so,
| | 01:49 | but I'm ready actually to
create this section line now.
| | 01:52 | I'm going to right-click on
the screen and select Continue.
| | 01:55 | When I do that, the Section view dialog box
comes up, and Inventor creates a preview of the view.
| | 02:01 | If I drag the view back and forth across
the part, you'll notice that the section line
| | 02:05 | automatically changes based
on the location of my cursor.
| | 02:10 | I'm going to go ahead and position this off to
the left and talk a little bit about the dialog box.
| | 02:14 | Within the dialog box, we have the
ability to make some basic changes.
| | 02:18 | We can change the Label Identifier, we
could change the Scale, and even the Style.
| | 02:23 | In case of this section we can also change
from a Full section to a specific Depth or
| | 02:28 | Distance, but in this case I'm
going to go ahead and leave the Full.
| | 02:31 | So the default settings work perfectly for me.
| | 02:34 | I'm going to go ahead and
left-click to place this view.
| | 02:38 | After doing so, Inventor
renders it as a Section view.
| | 02:41 | It also applies the hatch automatically
based on the material type, it's also created a
| | 02:47 | label for us, it's provided our scale, and
it's labeled the section line so that we can
| | 02:51 | quickly identify where the
section was created from.
| | 02:54 | Next, I want a little bit about the Detail view.
| | 02:58 | Detail Views are created in a very
similar fashion to the Section Views,
| | 03:01 | so this makes perfect sense to combine the two.
| | 03:03 | Say, for example, we want to get a little
more detail of this lip here up from the section.
| | 03:08 | To do so, we can use the marking menu just
like we did with the Section view, right-click
| | 03:13 | on the view, and select Detail view.
| | 03:16 | Just like the Section view the Detail view
dialog box is presented, and we have the ability
| | 03:21 | to change the Identifier, the Scale,
the Style, and a few other options.
| | 03:26 | At the most basic level, the default
settings are going to work most of the time.
| | 03:29 | So I'm going to go ahead and
begin creating my detail view.
| | 03:33 | To actually create the detail view, you need
to left-click in the center of where you want
| | 03:37 | your detail view to begin.
| | 03:38 | In this case, I left-clicked right in the
middle of that lip that I want to detail.
| | 03:43 | Now as I drag my cursor, I can adjust the size of the
detail and the position of the label for this detail.
| | 03:51 | Right about here looks about the right size.
| | 03:53 | I'm going to go ahead and left-click to
create the view, and Inventor creates a preview.
| | 03:58 | I can now zoom out, find a position on my
drawing sheet where I want to place this view,
| | 04:03 | and left-click to create the view.
| | 04:05 | Just like the section view it provides a
detailed label, it provides a scale label, and it labels
| | 04:12 | the initial detail view so that you can
quickly determine where this detail is coming from.
| | 04:17 | One last thing about the Detail view:
| | 04:19 | Sometimes you're going to find that maybe
the detail changes or the part changes, and
| | 04:23 | you need to reposition this detail.
| | 04:25 | You can do so by simply hovering over the
detail indicator, clicking and dragging the
| | 04:30 | position of that circle.
| | 04:32 | By doing so, the Drawing view updates
automatically to show the new position of the Detail view.
| | 04:38 | This comes in handy when the part changes or if
for some reason you made an improper selection.
| | 04:44 | You don't have to start from the beginning.
You can just reposition this Detail view.
| | 04:51 | Now that I've zoomed out a bit, you can
still see that my Section view is little
| | 04:54 | off from a position standpoint, and I'm
going to simply drag that over so it's a little
| | 04:58 | further away and my views
are a little bit more aligned.
| | 05:01 | I'll even adjust my
position of my Detail view a bit.
| | 05:05 | Now I've got a nice, clean position for my Drawing
Views, and I can continue on documenting my design.
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| Setting basic dimensions| 00:00 | Now that we have our initial views placed,
we're ready to begin annotating our design.
| | 00:05 | To start the process, we're going to
select the Annotate tab in the Ribbon bar.
| | 00:09 | Within the Annotation tab, you have all the
tools you are going to need to document your
| | 00:12 | design for manufacturing, things like
dimensions and hole notes, center marks, and even symbols
| | 00:18 | for welding operations and surface finishes.
| | 00:20 | Now to be honest, documenting a design for
manufacture takes a lot of work, a lot of
| | 00:24 | time, and a lot of practice.
| | 00:26 | The purpose of this movie is to provide a
basic foundation of the general tools you
| | 00:30 | can use to get started with the process.
| | 00:32 | We're going to start with
the general Dimension tool.
| | 00:35 | I'm going to zoom in on my
Detail view to begin this process.
| | 00:39 | The general Dimension tool can be found on
the Annotate tab in the Dimension panel, and
| | 00:44 | it works in a very similar fashion to
the dimensioning command in sketches.
| | 00:48 | There are some slight
differences that I want to call out, though.
| | 00:51 | We're going to start by
dimensioning the overall height of this lip.
| | 00:54 | I'll click on the lip to select it, and as
I drag my dimension out to the left, you'll
| | 00:58 | notice that it changes
styles at specific increments.
| | 01:01 | This is an organization tool.
| | 01:03 | It allows you to organize your dimensions so
that while manufacturing, there is no confusion.
| | 01:08 | I still left-click to place the
dimension just like I did before.
| | 01:11 | But you will notice the dimensions are
actually disconnected from the endpoints a bit.
| | 01:16 | This is standard drawing practice as you
know why your dimension lines to interfere with
| | 01:19 | the actual part edges.
| | 01:21 | The next dimension we're going to add is to
dimension the horizontal line at the bottom of the lip.
| | 01:24 | I'm going to drag down to the bottom here
and place my dimension, and you'll notice
| | 01:30 | that we're running into a
couple of different problems.
| | 01:32 | First, the Detail label is
interfering with our dimension.
| | 01:35 | I'm going to right-click and select OK to
get out of the Dimension command, and I can
| | 01:39 | simply left-click and drag my
Detail label out of the way a bit.
| | 01:44 | If the part changes, you can
move that detail label at any point.
| | 01:47 | The other problem we have, if we select this
dimension is you will notice because we selected
| | 01:51 | the horizontal line like we might when we
are sketching, it locked the dimension to
| | 01:55 | the endpoints of that line.
| | 01:57 | The problem is is it's hard to tell the
difference between the part edge and the dimension.
| | 02:02 | To fix this, we can simply grab the green
dot at the endpoint, left-click and drag, and
| | 02:08 | lock it to the endpoint of our drawing view.
| | 02:10 | The still creates the exact same dimension, but,
as you can see, there's now a break between
| | 02:14 | the part edge and the dimension.
| | 02:18 | We're going to get back into
the Dimension command again.
| | 02:20 | This time, I'm going to show you how to create that
dimension without having to fix the dimension after the fact.
| | 02:25 | Rather than selecting the horizontal line
here at the top, I'm going to select its endpoint,
| | 02:30 | and then I'm going to select
the endpoint of the part edge.
| | 02:33 | Now, when I place the dimension, you'll see
that I don't have to go back and correct that.
| | 02:38 | Based on where I selected, I've already
solved the problem before it actually happened.
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| Changing dimension precision| 00:00 | On the screen you can see
the dimensions that we created.
| | 00:03 | One of the things you might notice is that the
dimensions are only to two decimal points of precision.
| | 00:08 | Now typically I wouldn't recommend jumping in
and changing a lot of settings in the drawing,
| | 00:12 | especially without talking to a CAD manager,
because a lot of these standards are set.
| | 00:16 | But I know that the precision is something that
people might want to change right out of the gate.
| | 00:20 | I'm going to take a minute to show you how
to do this so that you can ensure that your
| | 00:23 | designs are documented
properly for manufacturing.
| | 00:27 | To make this change, we're going to go
to the Manage tab on the Ribbon bar.
| | 00:31 | Under the Styles and Standards panel
we're going to select Style Editor.
| | 00:35 | Now there's a lot of settings here, and we're
not going to through all of them, we're most
| | 00:39 | specifically looking at Dimensions.
| | 00:41 | Even more specifically than that, we're
looking for the default ANSI Dimensions.
| | 00:46 | Depending on the type of standard you've
installed on your system, these may be slightly different
| | 00:50 | but you're going to look
for the defaults anyway.
| | 00:53 | Here in the Linear section we have the
Precision called out as two decimal points.
| | 00:58 | We're going to simply select the dropdown
list and pick 3.123, which indicates a three
| | 01:04 | decimal precision, and
we're going to select Done.
| | 01:07 | Inventors is going to ask us to save our Edits,
and when we do that you can see that the change
| | 01:11 | has been reflected in our drawings.
| | 01:13 | Again, I wouldn't recommend changing these
settings in a commercial environment without
| | 01:17 | talking to your CAD manager, but hopefully
this will allow you to begin documenting your
| | 01:21 | designs properly for manufacturing.
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| Creating baseline dimensions| 00:00 | In a previous movie we learned how to create general
dimensions and adjust the precision of those dimensions.
| | 00:06 | In this movie we want to focus on how to accelerate
the annotation process by using baseline dimensions.
| | 00:12 | To start this process we're going to go to
the Annotation tab, and in the Dimension panel
| | 00:17 | you can see along with our general dimension
we have Baseline, Ordinate, and Chain dimensions.
| | 00:22 | Now all three of these types of dimensions
work in very similar fashion, that's why I'm
| | 00:26 | going to focus simply on baseline here.
| | 00:28 | I'm going to launch the Baseline command,
and I'm going to zoom in on the view in the
| | 00:32 | bottom corner of the drawing.
| | 00:35 | Within the Baseline command, Inventor is
now ready for us to select specific pieces of
| | 00:39 | geometry we want to dimension in this view.
| | 00:41 | I'm going to start by selecting the bottom
of the part, and I'm going to work my way
| | 00:45 | up through the view, selecting specific
items I want to create dimensions for.
| | 00:50 | Once I've selected all those items, I can
simply right-click, select Continue, and Inventor
| | 00:56 | will create all of the dimensions in one action.
| | 00:58 | Now while placing the dimensions, it does
work with the general dimensions. I do have the
| | 01:02 | ability to snap to my increments for
organization purposes, and here I'm going to find a location
| | 01:08 | that I like, I'm going to left-click to place
those dimensions, and then I'm going to right-click
| | 01:13 | to actually create those permanently.
| | 01:16 | You can see that with just a few clicks
Inventor has created a number of dimensions in one
| | 01:20 | action, which should help
speed the design process.
| | 01:24 | The one thing you might notice if we zoom out
a bit is because we added all these dimensions
| | 01:28 | in one action, they extend a little
too close to the view to the right.
| | 01:32 | If we were to add dimensions
to this, they might overlap.
| | 01:35 | To fix this, we can simply hover over the
view, left-click and drag to reposition the
| | 01:40 | view and the dimensions all move because
they're linked to that view specifically.
| | 01:46 | As you can see, the Baseline dimensioning is
a great way to speed the Annotation process.
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| Creating center lines, center marks, and hole notes| 00:00 | In this chapter we've learned how to place
views, we've learned a few ways to create
| | 00:04 | dimensions, we've even learned how to
control the precision of those dimensions.
| | 00:08 | In this movie I want to turn our focus to
Centerline, Center Marks, and Hole Notes.
| | 00:13 | To create those, we're going to go to the
Annotation tab, and under the Symbols panel you can see
| | 00:18 | a few different options for
creating Centerline and Center Marks.
| | 00:21 | I'm going to zoom in on our front view and
start with creating up general Centerline.
| | 00:29 | This command allows you to simply select points
in the view that you can create Centerlines from.
| | 00:34 | For example, if I hover over the midpoint
on this side of the part, simply drag to the
| | 00:38 | other side of the part and connect to the
midpoint there, I can then right-click and
| | 00:42 | select Create, and I've
manually created a Centerline.
| | 00:46 | This can be done with any view
and any geometry within that view.
| | 00:50 | The other way to create a Centerline
would be to use the Centerline Bisector tool.
| | 00:56 | This tool allows you to select two lines
and have Inventor create a Centerline between
| | 01:01 | them automatically.
| | 01:03 | After creating the Centerline we can get
out of the command, and we can manually extend
| | 01:08 | that throughout the part.
The next item I wanted to cover is Center Marks.
| | 01:15 | Center Marks are also very simple to create
and are required in many drawing documents.
| | 01:20 | The Center Mark tool is also
located in the Symbols panel.
| | 01:24 | After launching the command, you can create a Center Mark
by simply selecting any circular geometry in a view.
| | 01:29 | Inventor will automatically scale the Center Mark
to meet the size of that specific piece of geometry.
| | 01:35 | Now that we've created a few Centerlines and Center
Marks, I wanted to turn our attention to Hole Notes.
| | 01:41 | Hole Notes can be found on the
Annotation tab under the Feature Notes panel.
| | 01:45 | The Hole Notes command is also very simple
to use, and I wanted to call out some of the
| | 01:50 | benefits of using it.
| | 01:51 | While we were in the part modeling chapter
we created holes using the Hole command and
| | 01:55 | during that process I mentioned that we were building
a lot of intelligence into the model through that command.
| | 02:01 | Here's where we get to see the benefit of that.
| | 02:03 | When we were creating the holes, the one hole
that extended off of the revolve feature was
| | 02:08 | actually a threaded hole.
| | 02:10 | And if I select that hole in our drawing view,
you can see that the Hole Note command has
| | 02:15 | pulled the information directly from the
model and updated that into our drawing.
| | 02:20 | In this case, it's an 8-32 threaded hole.
| | 02:23 | Because it's connected to the model, if the
model changes the drawing will automatically
| | 02:27 | update to reflect that change.
| | 02:29 | I want to turn our attention to
another hole in the Section view.
| | 02:32 | While still in the Hole Note command, we can
select part of the circle that makes up the
| | 02:36 | hole in the Section view.
| | 02:39 | Here you can see the Hole Note has created
a couple of pieces of information for this.
| | 02:43 | It's pulled the diameter from the model,
but it's also pulled the depth as well.
| | 02:48 | Again, using the hole feature in the part
modeling environment greatly affects the outcome of
| | 02:53 | drawings that you're annotating.
| | 02:55 | Rather than having to manually input this
information if you had used an Extrude, the
| | 02:59 | information was built into the model and is
actually pulled on the fly into the drawing,
| | 03:04 | and it's connected so that any updates
will be reflected without any intervention.
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|
|
ConclusionNext steps| 00:00 | At this point you should have a solid
understanding of the major components needed to get started
| | 00:04 | building your own models.
| | 00:06 | From here I would recommend
exploring a few different web resources.
| | 00:10 | The first would be my YouTube channel which
can be found at www.youtube.com/johnhelfen.
| | 00:16 | On this channel I have videos that further
explore things like part modeling, and there
| | 00:20 | are also videos that discuss more advanced topics like
finite element analysis and dynamic simulation in Inventor.
| | 00:26 | There are also videos of other products that
are commonly used in conjunction with Inventor
| | 00:31 | like Inventor Publisher and Autodesk Showcase.
| | 00:34 | Another web resource worth exploring is Autodesk
WikiHelp, which can be found at wikihelp.autodesk.com.
| | 00:41 | The WikiHelp is an open community where
people using Inventor everyday are compiling their
| | 00:45 | collective knowledge on the product.
| | 00:48 | And finally, I would recommend you
check out autodesk.com Digital STEAM.
| | 00:53 | This is a free educational site that
contains everything from basic information on design
| | 00:57 | principles like color, scale, proportion, and balance,
to projects that range from 90 minutes to several days.
| | 01:05 | As we wrap up, I want to remind everyone that
Autodesk Inventor is an exciting product to
| | 01:09 | learn because it allows you to
explore your ideas without bounds.
| | 01:13 | Not everyone has the ability to manufacture
parts, but with Autodesk Inventor everyone
| | 01:17 | can explore and share
their ideas in a digital world.
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