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Scale, stretch, and offset geometry


Inventor 2014 Essential Training

with John Helfen

Video: Scale, stretch, and offset geometry

As we continue to learn to how to edit sketch geometry, in this movie we're going to focus on the Scale, Stretch and Offset commands. We're going to begin by creating a new part file. We'll select New on the toolbar. Select Standard.ipt as our template and click Create. To begin, we're going to create a new sketch by clicking Create 2D Sketch, and selecting one of the origin geometry planes. Now that we're in the sketch environment, we can begin with a very basic shape.
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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

Scale, stretch, and offset geometry

As we continue to learn to how to edit sketch geometry, in this movie we're going to focus on the Scale, Stretch and Offset commands. We're going to begin by creating a new part file. We'll select New on the toolbar. Select Standard.ipt as our template and click Create. To begin, we're going to create a new sketch by clicking Create 2D Sketch, and selecting one of the origin geometry planes. Now that we're in the sketch environment, we can begin with a very basic shape. I'm going to right-click and select Rectangle.

I'll hover over the center point of the sketch and left-click. And then I'll move my cursor and define a second location for the other corner of the rectangle. Now that we have this geometry created we can look at scaling, stretching, and offsetting geometry. I ha, I don't use scale or stretch a whole lot, but it can come in handy from time to time. So, just like move, copy, and rotate which we learned about in a previous movie, these functions work in a very similar fashion. I'll start with scale.

In the Modify panel, if you select Scale, you're entered into the dialog box and you're automatically placed in the select mode. This allows you to window geometry or select a group of geometry that you wish to scale. The next item is to select a base point from which to scale. I'm going to go ahead and select the center point, or the center of the sketch, the origin point. And just like in the previous commands we learned about, Inventor is going to warn us if there's constraints added to the geometry that might be preventing it from scaling.

I'm going to go ahead and hit Yes, which will remove the constraints that are causing an issue. And as I move my cursor now, you'll see that my geometry is being scaled uniformly. When I left-click, the geometry is placed and it's in and it is all been scaled proportionally. One of the other things you might notice here, and partially the reason I don't use it that often, is one of the constraints that it removed was this coincident constraint that was locking the geometry to the origin point. If I left-click and drag on this line, you'll see that this line is no longer connected to this point.

Now because this is a rectangle, this is really easy to fix. I can either left-click and drag on that point and hover over the, the center point to snap it back into position and reconstrain it to the origin. Or, I can use the Constrain toolbar, and select Coincident. And select the point at the bottom corner of the rectangle, and the center point to lock those two into position. Now when I do that though it changes the scale of that geometry. So generally, where I use scale is when I'm importing geometry from AutoCAD and perhaps I import it and by mistake.

I import a millimeter into a inch drawing or vice versa. I might use scale to scale a bunch of geometry at once, to have it be the proper size, but I normally try to avoid it when it involves constraints and stuff I drew in Inventor. Because the constraints that are added automatically add intelligence that I typically want to keep in my sketch. But it is very simple to scale geometry using the Scale command. Next we'll look at the Stretch command. And similar to the previous command, it's going to function the same way, and it's going to do the exact same thing when it comes to removing constraints or adding constraints.

I'm going to click on the Stretch command from the Modify panel. I'm in the Select mode, and in this case I'm going to go ahead and just window the geometry here so that I can move this point and stretch it into a different location. Now you, if you remember, when I was drawing this rectangle, certain constraints were added. A horizontal constraint on the bottom, and a perpendicular constraint on this item. If I select my base point, and then pick the bottom right hand corner, I'm going to get the warning that constraints are going to be relaxed.

And when I hit Yes, I now have the ability to reposition this. What it has done, is it's broken the, the perpendicular and horizontal constraints so that these pieces of geometry can be moved. But what you'll also notice, is that the lines are no longer purple. Because of the fact that the horizontal constraint was removed. It has changed the type of geometry. So you may have to add new dimensions, in this case perhaps angle dimensions to control the exact shape of this geometry. I'm going to go ahead and undo by right-clicking and selecting Undo.

I'm going to do that a couple of times until we get back to our rectangle. Now that we're back to our rectangle and you can see that we have our purple lines again, which means we're back to where the constraints still exist, I'm going to look at the offset command. The offset command is something I use quite frequently. For example, if we go to the Modify panel and select Offset, there's a couple of settings that you need to know about that will help you get the most out of this command. First, if we right-click, there's a couple of selection options here that you may toggle on and off depending on what you want to offset.

By default, it's set to select an entire loop and to constrain the offset. And I'll show you what that means. If I go and click to get out of that command, and I hover over my geometry, you can see the effect of the loop select. By hovering over the one line it's chaining all the lines around this rectangle to select the entire loop. If I right-click in the command and uncheck Loop Select, now I'm only getting a single piece of geometry. And there's going to be times where that'll be helpful, so it's important to know about that option.

The other thing to mention is, once you've made this change, it will remain in that state until you turn it back. So it is important to not only know that those options are there, but to know that they remain in the last state. So that you don't forget it and cause confusion later on. So, I, as we go along I'll show you the outcome of, of changing that. I'm going to go ahead and select you, loop select again. And I'm going to go ahead and select that geometry, and I have the ability as I'm moving my cursor to either offset inside or outside of that line, depending on my need.

And in this case I'm going to go inside and I'm going to left-click to locate this geometry. Now I'm going to also right-click and select General Dimension, and add a dimension here. I just want the overall size of the geometry to stay locked at its current size. And the reason for that is, I want to show the constrained loop. Or the constrain option that was mentioned just a moment ago. If I left-click and drag on this corner, you'll notice that the entire loop moves in a uniform fashion.

That is the result of having the constrain option toggled. In the offset command. If, for example, I go back to the Offset command and right-click and select Constrain Offset, what you'll find is when I do my loop now it looks exactly the same up until the point where you want to change the geometry. If I right-click and select OK to get out of the command, and then grab the corner again and drag this one, you'll notice that it's not constraining the geometry beyond its initial offset.

So depending on your needs that might be perfectly okay. It's just a matter of knowing about the command and understanding what the outcome of using it will be so that you can make the proper decisions while you're designing.

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