Inventor

Set Divergence Points When Modeling Products in Inventor

31 Jan, 2014 By: Jeff Stueck

IMAGINiT Tricks Tutorial: You may be familiar with top-down and bottom-up design methods, but the outside-in approach can save you time and rework.


Editor's note: This tutorial courtesy of IMAGINiT Technologies.

Whether we realize it or not, by modeling in 3D we’re already utilizing some combination of top-down and bottom-up methodology. The bottom-up approach means we’re constraining a bunch of saved components together inside an assembly. Or, if we’re modeling multiple bodies inside a single part file, then we’re using the top-down approach. Regardless of how we get it done, is there a logical way to start modeling a product in Autodesk Inventor before we know all the nitty-gritty details?

Enter the Outside-In Method

The outside-in method is just a variation of top-down design, but approaching our designs in this manner can help us move forward with concepts before we have all the details. Of course, by approaching our designs strategically, we can set up parameters along the way to facilitate basic changes that we might anticipate. However, the outside-in method also helps us set up divergence points so we can backpedal when we discover we’re headed down the wrong road (or if we just want to explore multiple roads at the same time).

Video gamers might compare this concept to their ability to save a reference point in their game so they can go back and replay a certain chapter. The bad news is that to improve their standing, they will need to replay that chapter from the reference point. The good news? They don’t have to start over from the beginning.

Where to Start?

In the figure below we see an airplane design being modeled as a multibodied part. In the browser, we find that all the main components (wing, tail booms, etc.) were modeled as individual bodies. By projecting geometry from one sketch to the next, each body dynamically adjusts in size and position relative to the others.



Now that our concept is taking shape, we can start thinking about how to construct the wing. Will it be built from solid foam? Or will it be framed with wood, then covered with plastic?

The outside-in approach allows us to develop our design without knowing the exact answer to those questions, so we can explore both options without losing the progress we have made so far. Let’s call this our divergence point, analogous to the “save point” in our video game where we can return and replay the chapter if necessary.

Avoid the Save-As Command

In order to explore the two possible construction methods for our wing, some designers may be tempted to use the Save-As command to create new versions of their model to work on independently. However, using this command will create multiple files, which must all be updated manually if anything changes in the original design concept file. (That never happens, though, right?)

A much more elegant and powerful alternative to the Save-As command is Inventor’s ability to derive bodies from one part file to another. In other words, rather than exploring our various wing construction methods in separate, unlinked files, Inventor allows us to derive the original wing into multiple (actually limitless) part files which are all linked back to the original. That means when the original wing changes size or position, all of the derived versions update as well.

To demonstrate the process, we will create two new part files (one for each wing concept), then use the Derive command (whose location is highlighted below) to bring in the wing from our original concept file.

 

Once executed, the Derive command will prompt us to select the file from which we want to use the original wing. Inventor refers to the original part as the “base component.” Inventor allows for some specific options in the Derived Part dialog box, but we will just focus on the Solid Bodies folder for now. In the figure below, we see that everything except the solid body named “Wing” is deselected.



Once we accept these options, we see that a reference part appears in our browser and the wing appears in our modeling window. We won’t go into the details here, but by right-clicking on this browser node at any time, we can adjust the criteria from the previous window or open the base component itself for editing.



Model Both Options without Affecting the Original

Now that we have the wing inside our new part, we can perform modeling features such as split, mirror, extrude, etc. without affecting the base component.

The image below shows the progress as we add features to the “framed” version of our wing.



Here we see our “foam” version as it evolves. Who knows — at some point we may even add a third version of the wing wrapped in carbon fiber.



The Payoff

The point is, now that we have a base component driving the size and position of our model, we can take advantage of that by branching off in limitless directions. Then, when changes are made to the base component, every instance of that derived component will update as well.

Now that you understand the concept, try approaching your models from the outside-in and see where you can find places to “save your game” along the way so you don’t have to start over.

Next Time

In a future tutorial, I’ll demonstrate the Make Components command, which creates new part files for individual solid bodies and places them into a target assembly of our choice (or lets us create a new target assembly on the fly). This process paves the way to generate parts lists, subassemblies, and exploded views.


About the Author: Jeff Stueck


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