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SolidWorks 2014 Essential Training
Illustration by Richard Downs

Using equations to drive a sketch


From:

SolidWorks 2014 Essential Training

with Gabriel Corbett

Video: Using equations to drive a sketch

Equations are awesome, and in SolidWorks 2014, they got even better.
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  1. 1m 51s
    1. Welcome
      1m 7s
    2. Using the exercise files
      44s
  2. 31m 13s
    1. Launching SolidWorks for the first time
      3m 55s
    2. Accessing and customizing the Ribbon
      4m 14s
    3. Touring the shortcut bar and identifying essential keys
      7m 27s
    4. Saving, renaming, and managing files
      10m 28s
    5. Working with the new view cube, or View Selector
      2m 36s
    6. New features in SolidWorks 2013 and 2014
      2m 33s
  3. 14m 11s
    1. Understanding the 3D world
      2m 31s
    2. Creating your first part
      3m 15s
    3. The virtual, parametric prototyping environment
      1m 56s
    4. The FeatureManager and feature-based modeling
      3m 43s
    5. History-based modeling and the rollback bar
      2m 46s
  4. 28m 32s
    1. Starting a new sketch
      6m 50s
    2. The six steps used in almost all modeling features
      52s
    3. The Line and Centerline tools
      3m 25s
    4. Using the Circle tool
      1m 51s
    5. Adding and removing relationships and dimensions
      6m 56s
    6. Understanding relationship types
      3m 58s
    7. System options, units, and templates
      4m 40s
  5. 18m 28s
    1. Drawing rectangles
      5m 31s
    2. Creating arcs in a sketch
      4m 8s
    3. Drawing splines in a sketch
      4m 57s
    4. Sketching polygons
      3m 52s
  6. 36m 5s
    1. Trimming and extending portions of a sketch
      3m 54s
    2. Creating offset geometry
      3m 13s
    3. Moving, copying, rotating, and scaling elements
      3m 13s
    4. Erasing, undoing, and redoing actions
      2m 24s
    5. Using the mirror tools
      2m 24s
    6. Creating repeating patterns in a sketch
      4m 55s
    7. Using construction lines to build robust sketches
      3m 25s
    8. Applying fillets and chamfers to a sketch
      2m 32s
    9. Working with slots
      3m 46s
    10. Adding text to parts
      4m 1s
    11. Using the Convert Entities command
      2m 18s
  7. 9m 33s
    1. Working with planes
      5m 28s
    2. Placing and using axes
      2m 22s
    3. Placing a coordinate system
      1m 43s
  8. 17m 50s
    1. Extruding a sketch into a 3D object
      4m 36s
    2. Using Revolve to create 3D parts
      2m 42s
    3. Using Loft to create complex shapes
      4m 40s
    4. Refining a loft shape with guide curves
      2m 22s
    5. Using the sweep to create wire and pipe shapes
      3m 30s
  9. 20m 23s
    1. Modifying parts using the Extruded Cut tool
      5m 42s
    2. Working with the Revolved Cut tool
      6m 19s
    3. Using the Lofted Cut tool
      3m 32s
    4. Cutting holes and grooves with the Swept Cut tool
      4m 50s
  10. 21m 5s
    1. Using fillets and chamfers to smooth corners
      5m 58s
    2. Creating repeating rectangular patterns
      3m 16s
    3. Creating a circular pattern
      2m 27s
    4. Mirroring objects
      4m 0s
    5. Using the Shell and Draft tools
      3m 52s
    6. Scaling parts
      1m 32s
  11. 9m 39s
    1. Working with reusable sketches and blocks
      2m 47s
    2. Creating blocks
      3m 51s
    3. Designing with blocks
      3m 1s
  12. 29m 45s
    1. Understanding the tools for beginning a new assembly
      4m 46s
    2. The basic steps in creating an assembly
      3m 18s
    3. Mating parts together in an assembly
      6m 43s
    4. Working with subassemblies
      2m 9s
    5. Linear and circular assembly patterns
      4m 56s
    6. Downloading premade parts from the Internet
      3m 32s
    7. Using Toolbox
      4m 21s
  13. 15m 8s
    1. Mating parts with coincident, parallel, and distance mates
      4m 35s
    2. Mating parts with width mates
      5m 53s
    3. Mating parts with path mates
      2m 5s
    4. Mating parts by aligning planes
      2m 35s
  14. 10m 20s
    1. Getting started with the Hole Wizard
      4m 38s
    2. Positioning holes in layout sketches
      5m 42s
  15. 15m 27s
    1. Linking sketches to other parts
      4m 28s
    2. Linking to layout sketches
      6m 48s
    3. Using the Hole Wizard in context
      4m 11s
  16. 17m 15s
    1. Understanding threading concepts
      7m 17s
    2. Using a helix and Swept Path to create a thread
      4m 2s
    3. Understanding internal threads
      5m 56s
  17. 17m 25s
    1. Using equations to drive a sketch
      5m 5s
    2. Working with complex calculations
      2m 6s
    3. Integrating Microsoft Excel to manage design tables
      7m 10s
    4. Building assemblies using part configurations
      3m 4s
  18. 23m 17s
    1. Working with drawing templates
      6m 49s
    2. Setting up drawing options and sheet properties
      3m 43s
    3. Choosing the correct projection angle
      2m 21s
    4. Adding model views to a drawing
      10m 24s
  19. 16m 8s
    1. Creating general dimension notations
      6m 37s
    2. Creating ordinate and running dimensions
      3m 0s
    3. Dimensioning holes and curved features
      3m 8s
    4. Using the autodimension tools
      3m 23s
  20. 14m 38s
    1. Creating holes and callouts
      5m 8s
    2. Adding center marks and centerlines to a drawing
      3m 46s
    3. Adding item notes
      2m 57s
    4. Making drawing revisions
      2m 47s
  21. 11m 42s
    1. Adding assemblies to drawings
      2m 10s
    2. Including a bill of materials
      1m 42s
    3. Adding balloons to specify parts on an assembly drawing
      1m 39s
    4. Adding a title block and sheet properties
      2m 8s
    5. Building an exploded view for an assembly drawing
      4m 3s
  22. 1m 2s
    1. Next steps
      1m 2s

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SolidWorks 2014 Essential Training
6h 20m Beginner Dec 09, 2013

Viewers: in countries Watching now:

SolidWorks is the world leader in 3D software for product development and design. Start creating manufacturing-ready parts and assemblies, as well as detailed drawings and bills of materials. In this course, author Gabriel Corbett shows how to create 2D sketches that will become the basis for your 3D models. You'll use the Extrude and Revolve tools to turn 2D sketches into 3D parts, then create more complex geometry with sweep and lofts. Then learn how to use the cut features to remove material and shape parts, and use mirroring, patterning, and scaling to modify parts. Next, you'll combine parts into movable assemblies and subassemblies. Finally, you'll create accurately annotated drawings, complete with itemized bills of materials that relate the final parts and assemblies to a manufacturer.

Topics include:
  • Creating your first part
  • Starting a new sketch
  • Adding and removing relationships and dimensions
  • Sketching polygons
  • Creating offset geometry
  • Moving, copying, and rotating elements
  • Working with planes, axes, and the coordinate system
  • Using Revolve and Loft to create 3D objects
  • Trimming with the Revolve, Loft, and Sweep cuts
  • Creating smooth and angled corners with fillets and chamfers
  • Designing with sketch blocks
  • Working with subassemblies
  • Creating threaded parts
  • Integrating Excel to manage design tables
  • Adding dimension notations to a drawing
  • Rendering an image of a part or assembly
Subjects:
Product Design CAD 3D Drawing
Software:
SolidWorks
Author:
Gabriel Corbett

Using equations to drive a sketch

Equations are awesome, and in SolidWorks 2014, they got even better. Equations allow you to derive an unlimited number of sketch values with one variable. If we later want to change that size, all we need to do is update the one equation, and all the linked values will change. Think about a quarter inch hole that is used across multiple features and sketches. If we wanted to change the hole to a 3/8 inch hole, all we need to do is edit the equation and all those hole will automatically update. Otherwise we would need to open each individual sketch and modify the values independently.

To get started let's go ahead and take a look at sketch one of 16.1 dash 1 and you can see here I have a pretty simple sketch. And I want to derive this with an equation value. So first things first let's jump over to the sketch tab and click on Smart dimension. And what I want to do here is I want to make a dimension from this far edge here and I'm gona click on this center line. And if I use the center line value, what I can use is what's called a double dimension. So from this side it's a single dimension. As soon as I pass over the center line, it doubles, it's a double dimension. It's a nice way to input full values versus half the value.

In this case here, I'm going to type in 10. But I don't really want to use a regular ten. What I want to do is actually define a global variable here. So instead of just typing a ten directly. Lets go ahead and hit equals. And as soon as I do so, it gives an option to choose a function or a file property or I can define a global variable here by giving it a name. In this case I'm just going to make it l. As soon as I do that I get this little icon here that says it's going to create a global variable. And if I click OK, or Enter it says, hey do you want to create this global variable named L? Let's say sure, let's do it.

And now it's asking me what the variable wants to be. So I'm going to type in 10.0, click OK, and click OK, again. So notice I got this little sigma in front of here showing me that I'm using an equation to drive that length and the value happens to be 10 at this point in time. Now that's great. And I can also, I can create more values the same way or if I'm happy with that, click on OK, and jump over here to the Equation Editor and right-click on Equations and say Manage equation. And on side of the equation editor here you can see I've already created this global variable named L with a value equal to ten.

Now I can add more global variables. Right inside here. So I'm going to type in W, and I'm going to say this is equal to five and thus equates to five. And down here you see I've got equations so I'm actually linking D1 at sketch one to that L variable. And I can do more of those down here if I wanted to as well, or I can do it from within the sketch environment. I also wanted to point out instead of just Ls and Ws, you can type out a full variable name here, doesn't really matter as long as it's one easy to understand block. But I wouldn't get too crazy with a long name because you're going to have to type that in every time.

Or select it from the Variable cell. You want to make it something that's easy to figure out, like length or width would be a fine word, but you don't want to get too extensive. Once you're happy with it, go ahead and click, OK. Now I want to grab that Smart Dimension tool. I'm going to dimension from the top and back again to that center line, and notice it's a single dimension turning into a double dimension, as soon as you go past the Center line. As soon as you click, again, if you hit equals, now you have the option to choose from one of those global variables, or create a function or a file property. So I'm going to back to global variables, in this time I'm just going to say hey I'd like to link to the width.

Click OK, and there's your value. Let's just do a couple more. Up here I'm going to go ahead and define the size of this hole. And I want it to be 1 inch, but instead of just typing one directly, I'm going to type in equals, and I'm going to give it the variable called whole. Okay? Click, Ok. Create a new global variable called whole. Look's good. And for my value, 1.0. Okay? I can also then use that same value over here. So we go ahead and push equals. We'll then get to the global variable, and I'll use Whole.

Click OK, and I have the size of the holes determining not only the size of the whole, but also the spacing from the edge. When everything's fully defined, it looks good. It's time to go ahead and extrude the feature, so go over here to Features, go to Boss Extrude, and I could type in my value here. But, you can also say, equals, and go ahead and choose one of those global variables, or create one, again, from there, click on Hole, and make it equal to one, click OK, and it created a part completely equation driven. Now, if I want to go back and make some modifications to my part, it's very easy.

Go ahead, go back to Equations > Manage my Equations. Notice my variables here are listed. Just go ahead and change those, I can say, instead of ten, I want five. On my next little item down here I'm going to click on 2.5. And for my hole, I'm going to make it half of an inch so 0.5. Those variables update. As soon as I click OK, the part automatically shrinks in size to its new variables. And in fact, if I open up the part, open up that sketch, you can see the new variables are used to define the shape of this part. Go ahead and exit out. And you can see also the thickness changed as well because we're defining that.

By linking it to the whole variable. Design re-usability is a great time saver, and using equations in your designs makes it easier to change and allow others to easily understand your input values. In SolidWorks 2014 they made it very easy to create equation values and integrate them into designs to make them easy and efficient.

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