Inventor Sheet Metal: Alternative Applications

I was happy to see Autodesk add a few nice features to Inventor’s Sheet Metal environment this year. However, I find myself still struggling with the software in many ways. Industry-specific applications, such as airframe design, require numerous workarounds to complete daily tasks. I hoped that a walkthrough of some of these might help others get a feel for things that they can try in their own work.

Figure 1: Multi-body sheet metal part

Multi-Body Sheet Metal Design

The introduction of multi-body design in Autodesk Inventor® sheet metal is huge. It allows users to create sheet metal structures within the context of a group, making fit and fasteners a less cumbersome affair.

Writing the parts and assembly out is automated the same way it is for standard solid bodies; just look for the “New Body” button in specific dialog boxes.

Stretched and Curved Flanges

Attached to this bulkhead is a two-part curved seal mount and stiffener, half of which is shown in Figure 1. In most applications this type of flange would be tabbed, braked, and stretched (see Figure 10). This seal mound also acts as a free-standing stiffener and as a result, really needs to be built as depicted. That is, until I find a better plan.

Figure 2: Using Contour Roll to create the curved flange.

In this case, we need to use the Contour Roll function in Inventor. Here I created the flanges’ “L-shaped” sketch profile upon an origin plane and constrained the profile to the existing bulkhead cross section using the Project Cut Edges function.

Using Contour Roll, I selected:

  • Profile – the L-shaped sketch profile
  • Axis – the circular face from the cutout in the bulkhead body
  • Solid – New Body function
  • Rolled Angle – 180°: I need this seal to mate with its opposing counterpart. In most cases, however, we’d need another sketch and parameters to drive this build accurately

Tip: By default, Contour Roll will apply a bend radius wherever it encounters a vertex in the profile geometry. This is awesome and eliminates the need to develop the curves in the sketch. This behavior is controlled by the Bend Radius pull-down in the lower right-hand area of the dialog.

Does this odd structure work in a flat pattern? YES! It works just like braking the flange and running it through a stretcher—just like we’d make it in the shop.

Partial Flanges and the End Tabs

This was painful. Actually if I were being fair and honest I should say really painful. There is no doubt that this functionality is only meant for electrical boxes and further development has not been completed.

Short Flanges and Tabs

The first flange I needed was a bit unorthodox. I wanted to take the fastener away from the inner seal ring area and add a Flange feature on the backside that allows the structure halves to be riveted together.

  • Edges – the short straight edge of the existing flange
  • Width Extents – Width option
  • Minimum Remnant (Bend) – 0”

Inventor really didn’t have much problem with this because it appears similar to a punched-out, bent tab. The trick to developing it in this application is twofold.

Figure 3: The Flange settings; notice the Width Extents options.

Width Extents

First we need to use either the Offset or Width functions hidden in the Width Extents area. This is rolled up by default and can be exposed by picking the chevron at the lower right area of the Flange dialog box.

Figure 4: The tabbed flange.

In this case I used the Width option with a dimension that provided sufficient edge clearance for a rivet, with no offset from the far edge.

Minimum Remnant

This bugger, if left unevaluated, will drive you nuts. Minimum Remnant is the minimum length of material along an edge that is being affected by the flange operation. This amount can be almost anything. However, if left too large, Inventor will not permit the relief slot to execute. It will build the flange with a very unfortunate tear treatment. Somehow this seems like the wrong behavior if you have specified a non-tear Bend Relief Shape.

Tip: using 0” Minimum Remnant will give you the greatest flexibility in workarounds, but will allow Inventor to create some geometries than can’t be built with conventional tools. I caution you to check your work thoroughly.

Full Flanges and Corners

For airframe, in most corners where flanges meet we’d employ a notched relief with a respectable sized radius. (In the field this meant whatever sized twist drill you had on hand, and could get away with.) This would either be cut into the bend, tangent to the far edge, or cut through and beyond the bend, protruding further into the opposite flat, unbent flange.

Figure 5: The existing legacy corner miter delivers far too shallow bend relief for high-vibration applications

Inventor will perform this for single flanges with an offset, as shown in the last example, and give the user the control over how deep to make the notch. But Inventor will not perform this type of operation in a corner. Instead it only delivers the relief-hole radius centered at the intersection of the bend centerlines. Most airframe applications would want the flanges to project tangent from the relief hole. This is impossible without a workaround.

Until the Inventor is able to perform this, we should understand how to control the corner better and discover the workaround options.

Corner Control

If the relief hole is centered at the bend centerline intersection and the relief hole has to extend past the bend, then the CornerReliefSize parameter (which is a diameter) would need to be sufficiently greater than 2X the bend radius:

CornerReliefSize >= BendRadius * 3

If the miter gap cannot be greater than the corner relief size that supports it, then it would need to be sufficiently smaller than the corner relief-hole diameter. More specifically, it needs to be smaller by a factor of the bend radius dimension.

GapSize < CornerReliefSize – BendRadius

This could be rewritten as:

GapSize < BendRadius * 2

When mitering is off, the hole is centered dead on the bend centerlines which makes this calculation straightforward but unnecessary, as the flanges are emitted straight from bend centerline intersection. When mitering is on, the hole is offset by a small factor that is a direct result of the intersecting flange corner angle. Any angle not at 90° will result in some adjustment.

GapSize = BendRadius * 2 ul - 0.002 in

Figure 6: Corner miter settings.

Removing 0.001” to this factor will kill the relief hole feature; no joke.

Figure 7: Flat patterned corner miter. Notice the limits of the miter; up to green is good, but wider values to get to the desired blue tangent will kill the corner treatment.

In Figure 7, note the location of the bend limits and the edge of the mitered flange. Inventor will not permit the edge to pass into the bend (this is the root of the inflexibility). This is the closest to a tangent flange-to-relief-hole condition we can get Inventor to automate (see Figure 5 for the result).

Note: I am using bend compensation for my stretch factor in the bend. These values differ slightly when using a K-factor.

Flange Bend Treatment Overlap

Since the single flange bend treatment will produce a tunable notch, one workaround is to create the notch using the Offset option in the Flange tool’s Width Extents area. Provide precisely the amount of offset needed to set the relief hole, then create the following flange on the remaining edge with no offset.

Figure 8: Step flange operation. It is not perfect, but permits more adjustment.

Tip: to get this workaround to clean up better, adjust the Bend Transition option.

Unfolded Cleanup

The last item I will suggest is the best option. Use an Unfold operation, sketch the clean tangent lines, Extrude-cut the excess out, and Refold. If that seems like a lot of wasted time, you’d be right.

Figure 9: A fully tangent corner miter with additional treatment depth. In the Browser notice the painful Unfold-Extrude-Refold operation that should be automated instead.

This method is the only realistic method of producing predictable and controllable results. It is a serious loss of time and should be an option that is part of the sheet metal automation.

Figure 10: A slightly better result. Notice the tabbed version of the stiffener that would instead be riveted to an intake skin. This variation should also be automated.


Inventor sheet metal is now a more capable tool in Inventor with the addition of multi-body modeling. Unfortunately the legacy corner mitering and inability for Inventor to integrate overlapping flange treatments leaves something to be desired. Hopefully, this information can enlighten Inventor users about the limits for these features, and how to get sheet metal to perform adequately in your design workflow.

More sheet metal solutions like these can be found at Design & Motion.

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