Inventor 2014 Essential Training
Illustration by Richard Downs



Inventor 2014 Essential Training

with John Helfen

Video: Parameters

When we looked at creating dimensions we talked about adding intelligence to a sketch. Parameters are what give dimensions the ability to add that intelligence. And I want to show you how parameters work right now. I'm going to start a new part file by selecting New from the toolbar Selecting Standard.ipt as my template and clicking Create to start a new part file. I'm going to get into a sketch by creating a new 2D sketch. I'm going to select a plane from the origin geometry that's presented.
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  1. 1m 24s
    1. Welcome
    2. Using the exercise files
  2. 6m 20s
    1. Exploring major workflow steps
      2m 19s
    2. Reviewing different file types
      4m 1s
  3. 22m 3s
    1. Navigating using the ViewCube
      4m 56s
    2. Navigating using the navigation tools
      5m 31s
    3. Using the browser
      3m 34s
    4. Using the ribbon bar
      2m 47s
    5. Using the Quick Access Toolbar
    6. Using the Marking menu
      4m 33s
  4. 22m 6s
    1. Basic menu customization
      6m 40s
    2. Custom ribbon bar panels
      6m 22s
    3. Keyboard
      5m 9s
    4. Marking menu customization
      3m 55s
  5. 20m 24s
    1. Project file introduction
      3m 54s
    2. The project file: .ipj
      4m 4s
    3. Setting up the project file for this course
      7m 11s
    4. Frequently used subfolders
      5m 15s
  6. 22m 31s
    1. Introducing sketching
      4m 55s
    2. Working with origin geometry
      4m 46s
    3. Understanding constraints
      7m 39s
    4. Application options
      5m 11s
  7. 50m 43s
    1. Drawing lines
      6m 29s
    2. Creating rectangles and arcs
      9m 26s
    3. Creating splines
      6m 35s
    4. Creating slots
      5m 43s
    5. Construction geometry
      6m 18s
    6. Dimensioning
      9m 34s
    7. Parameters
      6m 38s
  8. 30m 33s
    1. Move, copy, and rotate sketch geometry
      7m 43s
    2. Trim, extend, and split sketch geometry
      6m 20s
    3. Scale, stretch, and offset geometry
      7m 47s
    4. Creating rectangular, circular, and mirrored sketch patterns
      8m 43s
  9. 19m 27s
    1. Understanding work features
      3m 58s
    2. Creating offset work planes
      4m 17s
    3. Creating work planes
      6m 59s
    4. Creating work axes and points
      4m 13s
  10. 16m 50s
    1. Projecting geometry
      7m 7s
    2. Importing AutoCAD data
      9m 43s
  11. 54m 31s
    1. Part feature introduction
      5m 14s
    2. Creating a base extrusion feature
      8m 46s
    3. Keeping extrusions connected with the To next face/body option
      4m 29s
    4. Creating revolves
      7m 42s
    5. Creating complex shapes with the Loft tool
      8m 50s
    6. Adding control to a loft by creating rails
      8m 40s
    7. Creating a sweep feature
      6m 16s
    8. Creating a sweep feature with model edges
      4m 34s
  12. 24m 44s
    1. Adding holes to a part model
      10m 10s
    2. Modifying edges with fillets and chamfers
      4m 18s
    3. Hollowing parts with the shell feature
      10m 16s
  13. 25m 37s
    1. Creating rectangular feature patterns
      9m 23s
    2. Adding intelligence to a rectangular pattern
      5m 45s
    3. Creating rectangular feature patterns along a path
      2m 22s
    4. Creating circular feature patterns
      3m 11s
    5. Mirroring part features
      4m 56s
  14. 31m 30s
    1. Understanding iParts and iFeatures
      3m 19s
    2. Creating an iPart from an existing part
      11m 0s
    3. Changing between versions inside an iPart
      5m 50s
    4. Extracting iFeatures for use in other parts
      5m 11s
    5. Inserting iFeatures into a part
      6m 10s
  15. 26m 23s
    1. Introduction to assemblies
      1m 59s
    2. Placing components
      7m 40s
    3. Creating components in the context of an assembly
      8m 9s
    4. Placing fasteners from the Content Center
      8m 35s
  16. 46m 14s
    1. The Mate/Flush constraint
      9m 42s
    2. The Angle constraint
      5m 34s
    3. The Insert constraint
      3m 55s
    4. Driving constraints
      10m 0s
    5. The Transitional tab
      3m 50s
    6. The Motion tab
      9m 18s
    7. Contact sets
      3m 55s
  17. 18m 38s
    1. Adding materials to parts in an assembly
      4m 3s
    2. Visual styles
      4m 52s
    3. Enhancing the design experience with shadows
      2m 9s
    4. Adding a ground plane, reflections, and perspective to a design
      3m 34s
    5. Changing the lighting style to match a design
      4m 0s
  18. 39m 11s
    1. Exploring initial drawing creation
      5m 6s
    2. Placing base and projected views
      9m 31s
    3. Creating section views
      8m 0s
    4. Creating detail views
      3m 56s
    5. Creating a breakout view
      5m 41s
    6. Creating auxiliary and cropped views
      6m 57s
  19. 25m 57s
    1. Creating general dimensions
      9m 20s
    2. Changing dimension precision
      4m 21s
    3. Creating baseline, ordinate, and chain dimensions
      5m 51s
    4. Creating baseline, ordinate, and chain dimension sets
      6m 25s
  20. 10m 43s
    1. Creating individual balloons
      4m 34s
    2. Creating a group of balloons with automatic ballooning
      3m 40s
    3. Adding a parts list to the drawing
      2m 29s
  21. 30s
    1. Next steps

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Watch the Online Video Course Inventor 2014 Essential Training
8h 36m Beginner Apr 17, 2014 Updated May 19, 2014

Viewers: in countries Watching now:

Already up and running? This course is the next step in building your Autodesk Inventor skillset. Author John Helfen takes you through the interface and key processes of this parametric design system, including sketching, part modeling, assemblies, and drawings. Each process works in conjunction with the rest, allowing you to create parts and assemblies and document them in a way that they can be manufactured. Learn how to set up your project file; create and modify geometry; create extrusions, sweeps, and lofts; build parts with placed features and patterns of features; and create iParts and iFeatures. John also covers assembly visualization techniques, drawing views, and balloons and parts lists.

The course was created and produced by John Helfen. We're honored to host this training in our library.

Topics include:
  • Customizing Inventor's menus
  • Drawing rectangles, arcs, splines, and slots
  • Moving, copying, and rotating geometry
  • Trimming, splitting, scaling, and stretching geometry
  • Creating work planes
  • Projecting and importing geometry
  • Creating extrusions, revolves, sweeps, and lofts
  • Adding holes to a part model
  • Creating rectangular feature patterns
  • Creating iParts and iFeatures
  • Using constraints to position parts
  • Creating drawing views
  • Setting dimensions
John Helfen


When we looked at creating dimensions we talked about adding intelligence to a sketch. Parameters are what give dimensions the ability to add that intelligence. And I want to show you how parameters work right now. I'm going to start a new part file by selecting New from the toolbar Selecting Standard.ipt as my template and clicking Create to start a new part file. I'm going to get into a sketch by creating a new 2D sketch. I'm going to select a plane from the origin geometry that's presented. And I'm now in the sketch environment ready to create geometry.

Now, when we were creating dimensions, what you didn't know is that you were already using parameters. Inventor automatically is creating a parameter for every single dimension that is created in the system. It does it in a very hidden way, but you can access those parameters, because they allow you to do things like create formulas, and make relationships between pieces of geometry very easily. I'm going to start with a very basic shape. I'm going to create a rectangle. And what you're going to see here, I'm going to go ahead and enter a value of one for the width.

And I'm going to hit Tab on my keyboard. And I'm going to enter 0.5 for my value on my height. And I'm going to hit Enter. Now, what I've done here is created two dimensions on a single rectangle. What you didn't see is that in the background, Inventor created two parameters that represent these values. On the Quick Access toolbar you'll see a little function button. Or if you go to the manage tab, you'll see the same button here in the Parameters panel. If I click on that, it'll bring up our Parameters dialog box and you can see d0 and d1, which are 1 inch and 0.5 inches.

Which are actually the value of the dimensions on the model behind us. I'm going to, reduce the size of this so that we can see this a little more clearly. And, what I'll do here, is indicate that this dialog box is, a way to edit, bi-directionally, the dimensions that were just created. If I enter 1.25, instead of one and hit Enter, you'll notice in the background that the dimension changes and the model updates as well. If I go back and return that to 1 and hit Enter, it returns very simply.

Now, I'm going to close this and we'll come back to this dialog box in a little bit. Another thing I wanted to talk about is the naming. In that dialog box you saw d0 and d1. If you double-click on a dimension to edit it, you'll notice the name of that dimension or the name the parameter for the dimension listed at the title bar of the dialog box. In this case, the one inch dimension is tied to parameter d0. Now, d0 is not very descriptive. Inventor's just going to go d0, d1, d2 and select consecutive numbers.

And in most cases that's totally fine. You can even use those dimensions. For example, those names are perfectly acceptable. If I wanted, let me get out of that dimension and go to this 0.5. If I wanted that dimension to always be half the distance of this, with the text highlighted, click on the one inch dimension and you'll see that it enters d0 for me automatically. I can then use the slash symbol, or divide symbol, and enter /2, and hit Enter.

And you'll now see that I have a, a function indicator here. And the value hasn't changed. But what I've done is it connected these two parameters. So that, if this first one changes to, say, 1.5. Then, when I hit Enter, you'll see that the dimension that's driven by our function is automatically updated to be half the size of the dimension we just changed. Now, again, if you go back and double-click on this, you can see d0/2. UL indicates unit list.

It's just a value that allows you to do formulas rather than enter inches or millimeters for this specific formula. I'm going to go ahead and close this. And rather than use d0 or d1, I'm going to go back to this first dimension, double-click it, and instead of 1.5 what I'm going to do is I'm going to name the parameter on the fly. If I hit the Home button, here, I can say, I can type, width, and you'll notice that as I type, everything is red, indicating something's wrong.

At this point, this is an invalid value. It's not going to work. If we hit OK now, we're going to hit an error, and Inventor's going to tell us something's wrong. But as soon as I put an equals sign in here, you'll notice that the color changes to black. This indicates that we've entered a valid expression and Inventor can continue on. If I hit Enter now, it doesn't look like anything has changed. But what you'll find is if I double-click that dimension again, we've changed the oh, the name from d0 to width, and if we go over here to this function, Inventor has automatically updated d0 and swapped out width.

If we close that and return to the Parameter dialog, again you can get to it on the Manage tab, or if for example you're on the Sketch tab, you can always get to it from the quick access toolbar as well. Now here you'll see by naming it on the fly on the graphics window, it's automatically updated in our Parameters dialog box as well. The opposite is true as well. We can select d1 and perhaps enter height. And in this case, when I hit Enter, again nothing's changed, but if I hit Done and go back to this dimension, you'll see that it's height now instead of d1.

So these are the parameters that are most important to add intelligence to the sketch. It's not something you would necessarily use or modify in every case but, being able to center something by do, doing simple math, to ensure that a rule is maintained, for example. I know that no matter how wide this part is, its overall height has to be half that distance. So I can build in a very simple formula to ensure that my design intent is maintained, regardless of how the model changes.

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