Inventor 2014 Essential Training
Illustration by Richard Downs

Hollowing parts with the shell feature


Inventor 2014 Essential Training

with John Helfen

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Video: Hollowing parts with the shell feature

We're now ready to begin to looking at the shell feature in Inventor. I'm going to start a new part by clicking New on the toolbar, select standard.ipt, and select Create. With the blank part file, I'm going to start by creating a very simple shape, that we can use to explore the shell feature. I'll start by click create 2D Sketch, selecting one of the origin planes to sketch on, and create a simple rectangle. I'll right-click in the Graphics window and select two point rectangle, and I'll center the first point of the rectangle on the center of the sketch.
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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

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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

Hollowing parts with the shell feature

We're now ready to begin to looking at the shell feature in Inventor. I'm going to start a new part by clicking New on the toolbar, select standard.ipt, and select Create. With the blank part file, I'm going to start by creating a very simple shape, that we can use to explore the shell feature. I'll start by click create 2D Sketch, selecting one of the origin planes to sketch on, and create a simple rectangle. I'll right-click in the Graphics window and select two point rectangle, and I'll center the first point of the rectangle on the center of the sketch.

Using the heads up display I'll enter two inches for the length, hit Tab on my keyboard, and enter one for the other disks. I'll hit Enter on my keyboard to create that shape, and we can finish the sketch. Ill click on my Home button so we can see it a little more clearly. And we're now ready to extrude. If you right-click in the Graphics window, you can select Extrude and then it will select the entire profile, and extrude it by default to one inch. I'm going to select the check mark to accept that, and we have our first basic shape. Before we move on, I'm also going to turn on the Shaded with Edges visual style.

All that does is make the edges of the model stand out slightly. And, if you don't have this button, you can use the triangle at the bottom of this menu to select Visual Styles to enable it. Before we look at the shell feature, I'm going to add one addition feature. I'm going to select the Edge and select Filling. Then I'm going to enter a value of 0.5. Hit Enter on my keyboard, and we now have a part filled in. The other important part with shaded with edges is it will allow you to see these edges created by the filling. And that'll come in handy in a moment when we look at the Shell feature.

So, the Shell feature is essentially going to allow you to hollow out, or remove all the material from the center of a part. And it's going to leave the part hollowed with a uniform wall thickness, or a wall thickness that is the same in every location all the way around the part. The shell feature can be found in the modify panel of the 3D Model tab, here in the toolbar. When you click the Shell feature, what you'll notice is you do get a display that, if you look closely, is essentially cutting out the inside of this model.

In most cases you're not going to want to just shell out a model without opening one of the faces. So by default, Inventor places you in the face Selection mode. So that you can select any face to remove from the shell, because typically, for example, in this case, you're going to want to be able to put things in it. You're going to want to slide another part in, or in the case of this bottle that we're going to look at in a moment, you're going to want an opening to add material like pour a liquid into the bottle, for example. So what you see here is actually the shell with three different faces removed.

This check box here in the heads up display allows you to chain faces. When I selected here to remove this face, I selected the top face and it automatically chained the face for the fill it and the face for the front of this part as well. I'm going to go ahead and select the green check mark to show you what I mean. If I go back and edit the shell by double-clicking on it in the browser, I have the ability to change the faces that I had selected. If you go back to the Faces button, you can hold Shift on your keyboard and select on the face that you had already removed to deselect it.

Now we can look at the results of unchecking the Chained Faces option. Before, with that checked, when we selected this face here, we also got this face and the front face. But in this case, without that option checked, you're only removing the one face that you selected. You can still go add the additional faces. But, that's a couple extra clicks. And if you knew that was what you were going to do in the first place, the chained edges comes in very handy. Here you can see I selected a face by mistake, so I can simply rotate, hold Shift down And deselect that.

We can now explore some of the other options in this menu. Here on the menu you see the 0.1 thickness. This is actually the wall thickness. If I enter 0.05, you'll notice the preview shows thinner walls. The drop down to the left of that is telling Inventor which side of the model it's going to create the wall from. The default is inside which is what you're going to want in most cases. And what that means is that, when we created this model, this edge on the bottom here was 2 inches long and this edge was 1 inch long.

And, if we go to the inside, those distances will be maintained. If we know that the inside of our shell needs to be set to those distances, we can select Outside. And what it means now is that this face here is one inch on the inside of the shell, and the wall thickness of 0.05 is added to the outside of the model. The alternative is both options. What that does is essentially splits the difference. If you zoom in here, you can see it's shelling on the inside, and shelling on the outside of what was the original model.

I'm going to go ahead and set it back to inside, because that's really the default that most people are going to use. And I really briefly mention the other options here. These options generally only get you in more complex models. And they give you options to select whether or not Inventor can relax the wall thickness setting, based on the fact that certain complex models would not allow you to shell at a consistent thickness all the way around. If you run into any errors where shell can't be completed, I would consider looking at some of these options, but for an essentials course, we're not going to get into all the details now.

If I select the green check mark and look at the model now, you can see we have a fairly basic shape. And what's important to consider about the Shell feature is if we were going to create this model some people might look here and say you could have accomplished this without the shell feature. And that's true. We could have created the original extrusion, filled in the edge and then drawn or sketched on the end of the model to cut a hollow part out here. So in this prismatic part, while you could do it without the shell; the shell does make it easier.

Where the shell becomes most important is with more complex models. If we go to Exercise files and open up the bottle file, you'll see a shape that's a little more complex. This is a model that we created in an earlier movie. And what we can do here is use the Shell feature to hollow this bottle out. Now, you could also create the shell by using an additional loft, but it would take significantly more work to re-create the profiles, and re-set up the loft for the inside of the model.

So, by using the Shell feature and simply selecting the top face to remove, we're able to create a hollowed out bottle very easily. If we rotate the model a little bit and zoom in, you'll be able to see the bottom corner inside the bottle. You can see this edge, right here. Now, this brings up another point I want to call out about the shelf feature. One of the things you'll notice here is that if we look at this from the front view, this bottle has a flat and hard corner on the bottom of the bottle and that's not something you see in most cases.

Most bottles, you'll find, don't have a hard edge around the bottom. They're rounded or filleted a little bit. What I'm going to do is go ahead and return to my Home view, select this bottom edge, use the heads up display to add a fill it and I'm going to enter a value of 0.5. If I click the green check mark, you can walk from the front view and see that this model is now rounded on the bottom and that's probably more like what you would expect in a bottle like this. The problem that you have with this is that if we go to the Visual Styles menu, and select Wire Frame with Hidden Edges.

We can zoom in on the bottom corner of this bottle and you'll notice that while we rounded the outside, the inside remained a hard corner. And that's not really as intended either. Because we did the shell first, this inside edge remained hard, or, a sharp corner, while the outside filleted. And the result of that means, the distance between this outside edge of the bottle and this inside edge is very, very thin, which might be a point of weakness in the design, so you probably want to change that.

And the, it's very easy to do in Inventor. We have a couple of options. We can simply delete the shell, and we keep the rounded edge, and then we can re-add the shell to ensure that the rounded edge is maintained on the inside of the bottle. Another option would be, if we undo that and bring that shell back, in Inventor, we do have the ability to drag and drop features, which essentially, is like moving features back in time. What you were seeing me do previously was deleting the shell, which would move the fillet up to where the loft is, or right below the loft.

And then we could add the shell after the fillet. A quicker option would be to simply select the fillet, left-click and drag it, and drop it right before the shell. By doing that, what Inventor has done is gone back in time for you, added the fillet feature, and then created the shell for you. And you'll notice now, that we have the outside edge and the inside edge that maintain that point one wall thickness. So, it is important to keep in mind the order in which you're adding these fillets and these shelves in combination just so that you get the results you expect.

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