Look at This Motley Crew: Sheet Metal and Multi-Bodies in Autodesk Inventor

Avatech Tricks Tutorial: With the help of a workaround, you can use multi-body tools in the sheet metal environment.

Editor's note: This tutorial courtesy of Avatech Solutions.

It has always been my opinion that "skeletal modeling" is the most effective method of assembly creation in 3D CAD, so when Autodesk introduced multi-bodies in Inventor 2010, I was energized — a whole new methodology that allows you to build your entire assembly within the context of a single part file! I was devastated, however, when I got a warning dialog box saying I could not use the multi-body tools in the sheet metal environment. Undeterred, I found a workaround I would like to share with you.

What's It Going to Take?

In this example, we are going to build a simple metal picture frame with glass and backing. The driving geometry behind our design intent is the sheet metal frame, so that's where we will start. Using the default template Sheet Metal.ipt, create a new sheet metal part and build it using the typical sheet metal tools.

After we draw the sketch to represent the glass, you will notice the New Solid option in the extrude dialog box is grayed out when you try to extrude it. So you would think that our story ends here, but if you will click Convert to Standard Part under the Environment tab, you will notice that it was the sheet metal environment that disables the multi-body functionality; returning to the standard part environment gets us back to where we want to be.

Now we are ready to model the glass and backing of our picture frame. First, create the sketch for the glass on the back of sheet metal frame and extrude it to the desired thickness, selecting the New Solid option. Repeat these steps to create the backing that will hold the glass in place.

Time for Change

At this point we need to add some flanges on the frame to hold in the glass and backing in place, and this is where we will run into our next problem. When we return to the Environment tab and select Convert to Sheet Metal, we see an error message that reads, "This model cannot be converted to Sheet Metal because it contains features that have created multiple bodies. In order to convert to Sheet Metal these features must first be removed."

Basically, we are warned that in order for us to convert back to the sheet metal environment, the number of Solid Bodies must be "1."

Suppressing the offending features or moving the End of Part above the extrusions will reduce the current number of solid bodies that Inventor identifies, but still does not resolve the issue, so here is the workaround to preserve the workflow (and your sanity). In the browser, revisit each feature and change the solution to Join, thus satisfying Inventor's requirement of having only one solid body for the sheet metal environment.

Once the extrusions are changed to Join, convert the part back to a sheet metal part by going to the Environment tab and selecting Convert to Sheet Metal. After you have finished adding the flanges to the frame with the typical sheet metal tools, convert everything to a "standard" part as before.

Before we can change each extrusion back to the New Solid option, we must drag the last sheet metal feature up in the browser tree.

Remember, we need to do this because the use of multi-bodies can only happen after the sheet metal features. Next, rename all of the solid bodies in the browser to something more descriptive, such as a name or part number (this will be important later on).

On with the Show

Once your model is complete, use the Make Components command under the Manage tab to turn the multi-bodies into part files and place them into a top-level assembly (and yes, the sheet metal frame will flatten when placed into the sheet metal template). Avoid doing this too early in the design; wait until the design is as complete as possible.

If you need to go back and make modifications to the sheet metal frame, follow the same workflow with the "skeleton" part file. Notice, however, that the part names were reset under the Solid Bodies folder in the browser when you turn on the New Solid option; you will need to rename them again as before. When you open the assembly file that is referencing the multi-body skeletal model, all of the parts appear to be gone, but this is really an easy fix. Just open each part, right-click on its node in the browser, select Edit Derived Part, and then reselect the appropriate solid body.

At first, it seems like a lot of work to use sheet metal and multi-bodies methodologies together, but once you know where the difficulties lie and how to avoid them, I think you will find this to be a very powerful addition in your arsenal.