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Inventor 2014 Essential Training
Illustration by Richard Downs
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Creating complex shapes with the Loft tool


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Inventor 2014 Essential Training

with John Helfen

Video: Creating complex shapes with the Loft tool

We're now to a point where we can take all the things we've learned and To work through this, we're going to create a new part file.
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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 complex shapes with the Loft tool

We're now to a point where we can take all the things we've learned and work on one of the more complex sketch features in Inventor, and that's called the loft. On the screen you can see a basic maybe shampoo or salad dressing bottle shape that we're going to create through out this video. A loft is essentially a 3D model that transitions through a series of shapes. And the shapes don't have to be the same. In this case I'm using a couple of ellipses and a circle. But it could be a square, it could be any shape you draw.

The more complex the sketches get, the more time it's going to take to ensure that your loft is being created properly, but in general, you should be able to transition from a bunch of different shapes. To work through this, we're going to create a new part file. I'll select New from the menu. I'll select Standard.ipt as my template and click Create to begin the new part file. To start, we need to create our very first sketch. And to do that, I'll create a 2D sketch, and select the x z plane to sketch on.

Now we're creating the bottom of the bottle here, so what I want to do is use the ellipse tool to create my initial ellipse shape. Now that I have the basic shape, I'm going to dimension. I'm going to set the overall width from center to be, let's do 1.5. I'll hit Enter on my keyboard to enter that value. And then I'll do the overall height or width of the bottle to be, let's say 0.75. That gives me the basic shape I'm going to use as the bottom of this bottle.

I can finish this sketch and I'm ready to continue on. But before I do that, what I want to do is go back to the origin geometry folder, click the plus symbol and find the xz plane and right-click on it and select Visibility. I just want this available because I'm going to use this to create the additional workplanes needed to create the additional two profiles we're going to use. While learning about work planes, we earned about a shortcut where we can create offset work planes from within the 2D sketch command, and we're going to use that right now.

I'm going to create a new 2D sketch, but instead of left-clicking on this plane and sketching on the plane we just used, I'm going to left-click and drag, from that plane, and enter a value of three. When I hit Enter, the work plane is created and the sketch is automatically generated on that work plane. Next I'm going to return to the ellipse tool. I'm going to start from the center point and drag out to the left. And this time I, I'm going to go a little bit further past the outside of this original sketch that I see below.

And, a little bit wider than that as well. I'll right-click and select General Dimension from the marking menu, and I can add some dimensions here. The overall width from center I'm going to set to 1.75 and hit Enter on my keyboard, and then I'll do an additional dimension on the outer edge. At 0.8 inches. I'm now ready to finish this sketch. And you can see that I have two profiles now created for this loft. And I have one left to create.

So, I'm going to create a new 2D sketch one more time. And we will create an offset work plane by left-clicking and dragging from the existing work plane. And I'll enter a value of two inches. The work plane is created, you can see them all here in the browser, and I'm in Sketch3 on that plane now. To finish up, I'm going to right-click in the graphics window and select Center Point Circle. I'll start from the center of the sketch and I'll enter a value of one, and hit Enter on my keyboard. I'm now ready to finish this sketch and I have all the profiles needed for my loft.

The loft tool can be found in the Create panel on the 3D Model tab. When you click on the loft command, you're entered into the loft dialogue box, and just like extrude and revolve, you have a lot of the same options You do have the ability to create a new solid. If this weren't the base feature, you could create joins, cuts and intersects as well. But because this is the base feature, it's always going to be a new solid. I also have the ability to create solids or surfaces, but we're going to stick with a solid model. And we have the ability to begin selecting sections we're going to loft through.

I'm going to click to add a new section, and I'm going to start with the base of the bottle. Since there's only one profile, Inventor automatically selects the entire profile. I can then add an additional option by either clicking add, or I can simply go and click on the next shape and it's automatically added to the sections dialogue. And you can start to see the transition happening. Finally we'll select the final item and you can start to see the overall shape within the preview.

You can see our model bows out a little bit on the side and works its way back to the circle. Same on the outside as well. It's going to bow out. It's going to transition through that point, or through that profile. And up to this circular profile. Now, we could add rails to control this, and we'll do that in the next video. But I wanted to touch on the Conditions tab. The Conditions tab is another way to control the overall shape of this bottle without having to create rails.

And it's not quite as accurate as rails. You'll see in the next video. But it does provide a lot of flexibility to tweak or adjust how the shape of the bottle looks. In general, without having to go through the additional steps of creating rails. In the Conditions tab, we have the ability to change from what is a Free Condition where Inventor naturally just follows its own natural free form through the shapes, to a Direction Condition. By doing that, we enable the Angle in Weight options in this tab.

And if we zoom in, we're looking at section one, which is this bottom section. And if I zoom in, you'll see that we are 90 degrees from this horizontal line, up and to the right. So this sketch starts out 90 degrees from horizontal and it begins to move towards the next section. If we wanted to change that, we could set from 90. We could set it to, let's say 15. And you can see that it works in before it starts to transition to the next profile.

And we can adjust the weight here to two, and you can see it essentially pushes how long this follows that 15 degree angle before it begins transitioning. If we set this to four, you can see that it pushes much, much further toward the center of the model. Let's go ahead and set it back to a weight of two, and let's set this, instead of 15 degrees, let's set it to 120 degrees. With 120 degrees, it's going to start moving outward first before it transitions.

If we zoom out you can see the results of making those changes. The other thing to keep in mind is that it doesn't just happen from one side. It happens from all directions. So, it is bowing it in multiple directions, which is another reason you might want to consider lofting along rails depending on how accurate you need your model to be. You know, how much control you want over the shape of the bottle. If we rotate back to the front-view, and zoom in a little bit on the top of the bottle, you can see the result of changing to a direction condition on the neck.

Here we want it to be 90 degrees coming down from this sketch but I'm going to increase the weight so that you can see how we can add a neck shape to this. As I bump that up from one to two to three, let's even go to five. You can see that I can control how the shape of the bottle looks as it transitions through these items. I'm go ahead and set these back to their default conditions so that we can hit okay, and complete this portion of the course.

Essentially, we've used all that we've learned through work features, through sketching, and through part modeling to create a basic shape of a bottle here.

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