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Inventor 2014 Essential Training
Illustration by Richard Downs

Creating revolves


From:

Inventor 2014 Essential Training

with John Helfen

Video: Creating revolves

Now that we've learned how to create Now that we're in a blank part file, we can begin by creating a new 2D sketch.
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  1. 1m 24s
    1. Welcome
      47s
    2. Using the exercise files
      37s
  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
      42s
    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 NEW
      1m 59s
    2. Placing components NEW
      7m 40s
    3. Creating components in the context of an assembly NEW
      8m 9s
    4. Placing fasteners from the Content Center NEW
      8m 35s
  16. 46m 14s
    1. The Mate/Flush constraint NEW
      9m 42s
    2. The Angle constraint NEW
      5m 34s
    3. The Insert constraint NEW
      3m 55s
    4. Driving constraints NEW
      10m 0s
    5. The Transitional tab NEW
      3m 50s
    6. The Motion tab NEW
      9m 18s
    7. Contact sets NEW
      3m 55s
  17. 18m 38s
    1. Adding materials to parts in an assembly NEW
      4m 3s
    2. Visual styles NEW
      4m 52s
    3. Enhancing the design experience with shadows NEW
      2m 9s
    4. Adding a ground plane, reflections, and perspective to a design NEW
      3m 34s
    5. Changing the lighting style to match a design NEW
      4m 0s
  18. 39m 11s
    1. Exploring initial drawing creation NEW
      5m 6s
    2. Placing base and projected views NEW
      9m 31s
    3. Creating section views NEW
      8m 0s
    4. Creating detail views NEW
      3m 56s
    5. Creating a breakout view NEW
      5m 41s
    6. Creating auxiliary and cropped views NEW
      6m 57s
  19. 25m 57s
    1. Creating general dimensions NEW
      9m 20s
    2. Changing dimension precision NEW
      4m 21s
    3. Creating baseline, ordinate, and chain dimensions NEW
      5m 51s
    4. Creating baseline, ordinate, and chain dimension sets NEW
      6m 25s
  20. 10m 43s
    1. Creating individual balloons NEW
      4m 34s
    2. Creating a group of balloons with automatic ballooning NEW
      3m 40s
    3. Adding a parts list to the drawing NEW
      2m 29s
  21. 30s
    1. Next steps
      30s

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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
Subjects:
Prototyping Product Design CAD 3D Drawing
Software:
Inventor
Author:
John Helfen

Creating revolves

Now that we've learned how to create extrusion, we're ready to move into revolves. The nice thing is, because you've already learned how to create extrusions, a lot of the interface components are going to be exactly the same. Let me create a new part by clicking New on the toolbar, selecting standard.ipt as my template and clicking Create. Now that we're in a blank part file, we can begin by creating a new 2D sketch. We'll click Create 2D Sketch. And select the face to sketch on to enter the sketch environment.

We're now ready to begin creating our shape that we want to revolve. And we're going to do this a couple of times so you can see a few different options. But just like the extrude feature, the base feature or the first feature created in a part is going to have slightly different settings. Than future extrusions or future revolves within each part. I'm going to go ahead and create a rectangle. Starting at the center point of the sketch. And we'll set the overall width to be 0.5. And hit Tab on the keyboard. And we'll hit 1 as our value for the height.

And then we'll hit Enter to create that rectangle. And we also create the dimensions on the fly. Now that we have the shape completed, we can finish the sketch, and enter the Revolve command. We can right click in the graphics window and select Revolve from the Marquee menu. Or you can go to the Create panel and select Revolve there as well. I'll select Revolve from the Marquee menu. And just like the extrusion, because there's only one sketch here, or one profile, Inventor has automatically selected that for me.

It has then put me into the Access Selection mode, which allows me to pick what I want to revolve around. For example, if I select the vertical edge, I'll get a cylinder standing on end. If while still in the Access command, I hold Shift+down on the keyboard I can un-select that axis as well and for example, select a different one. So depending on the axis you select, you're going to get two very very different shapes. They'll both be cylinders, in this case, because we're revolving a rectangle.

But they'll be revolved in different directions. Again, if you hold Shift+down, if you're in the axis mode and you hold Shift+down, you can de-select that, and select a new one. Just like the extrusion, I also have the option to create different items. I can select an output of Solid or Surface. I can do Join, Cut, Intersect, or New Solid. Since this is the very first feature, I'm limited to only doing a New Solid. But additional Revolves would enable all of these. And, finally, I would have a direction here.

But since this is a Full Revolve, I don't have those options currently. If for example, I change the angle from Full to 90 degrees or 60 degrees, you can see the model update. And I do have a direction now. I can flip the direction the revolve is going to to take place in. I can make it symmetric, essentially on equal on both sides, or asymmetric, just like we could with the extrusion. I'm going to go ahead and select the default direction. I'll select the termination type.

And you'll, can see I have Angle, Full, and a few other options. Like Between two faces or planes, or between a Fit, or To a selected face or plane. I'm going to go ahead and select Full. Angle and Full are most likely what most people are going to use. And I can select the green check mark to indicate I'm ready to create that feature. Since I created this model directly in the center of the origin, I can use one of the origin planes to create our next revolve. When we rotate into the sketch mode, we can adjust our view so that it's the way we want to view it at.

We can hit F7 on the keyboard which will slice the graphics. So that we can clearly see what we're going to be sketching on. And finally, because this runs through the center of the part, I'm going to use the Project Cut Edges option. To project all of the edges that have been sliced by the workplane running through the center of the part. What this does is allows me to create a new profile that I can revolve. In this case, we're going to go ahead and create a small groove that's cut around this cylinder.

Perhaps for an o-ring to sit in or many other reasons. But I'm going to then right click and select General Dimension from the Marking menu and I can start to define the overall size of this item. I'm going to say that this is 0.125 thick. We're going to say that it is 0.125 deep. And we'll set it to 0.125 off of the top edge. You can now see that I have everything fully dimensioned. But the one thing that I don't have is an axis to revolve around.

I could draw a line in. I'm going to go ahead and do that. From the center of this bottom point to the top of the model. And I'm going to select OK. And when I finish this, you'll see that I get my graphics back and I'm rotated back into a 3D model. I can right click in the graphics windows and select Revolve. Like the extrude, because there is multiple profiles that I could take action on, Inventor's placed me in the profile mode. Where I can select the item I want to specifically take action on.

I'm going to select the rectangle. And then, I can go into the axis selection mode. This allows me to either select the sketch line that we created as an axis. Or, because I know this geometry was created in the center of the origin geometry, I can use the y-axis as well. When I do that I can then continue on selecting different options. For example, just like in the extrude, I could enter a specific distance. But before I do that, I'm going to select the type of revolve I want to do.

In this case rather than Join material, I want to Cut material away. This will allow me to see a preview of what we're going to receive. And we can talk a little bit more about the termination type and the distance. By default, these are the same things that you're going to see in an extrusion or very similar anyway. An angle is just like the distance extrusion and the full is like through all, roughly. If I select an angle, it defaults to 90 degrees and I can enter a specific value. I could say I want this to go 180 degrees and you'll see that it revolves all the way around the back side.

If I select 270 degrees, you can see that it's working its way around the circle. By selecting full, it will complete the full 360 degree cut. By selecting the green check mark. I'm ready to enter all these values and create the feature. You can now see in my browser I have two sketched features, both of them are revolves. And at any point I can go back and double-click on any of the sketches. In this case I'll hit F7, just so I can see a little more clearly. And I can update any of these dimensions.

Perhaps we want to make this groove a little bit deeper. I can enter 0.25 And when I finish this sketch, you can see that the model is updated and the groove is a little bit deeper.

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