SolidWorks Tech Tip: Imported Sheet Metal Parts

You may have to work with imported sheet metal parts that have problems. Here’s a roughly modeled part made to look like sheet metal. There are no bend reliefs and the bends are all made with sharp corners.

SolidWorks is very good at converting parts like these. Using the Insert Bends command almost finishes the job: bends have the correct radius and corner reliefs are added. But notice that the flange on the left is missing. There’s more work to do.

Let’s look at What’s Wrong in the Feature Manager.

SolidWorks sheet metal parts must be a uniform thickness, and the warning is telling us to look at the thickness of the missing flange. In this case, that flange is .06” thick, while the rest of the part is .05” thick. Cutting away material can make the flange a uniform thickness, but there’s a surfacing command that’s faster and perfectly suited to the job. First, roll back the history bar to just below the Imported 1 feature.

Using Insert>Face>Move, select the bottom of the flange and offset it by .01” to match the rest of the part. All the adjacent faces are trimmed to match the moved face and the result is solid body with uniform thickness.

Finally, drag the history bar to the bottom of the Feature Manager to let the part rebuild. The missing flange re-appears because it’s recognized as uniform thickness in Insert Bends.

Here’s another example showing a different problem. This imported part looks good, but it won’t unfold.

Highlight RoundBend 12 and 13: It turns out they really aren’t problems after all. Measuring the inside and outside radii of these bends shows a difference of .06” which is the part thickness.

Looking at other bends shows this one where the inside radius is incorrect for the part thickness. This bend and another at the opposite end of the part are not of uniform thickness and won’t unfold.

It’s possible to do an extruded cut across the part to make a sharp inside corner, and then apply the correct fillet radius. This would have to be repeated for all bends with non-uniform thickness, and could be very time consuming.

There’s another way: using Insert>Surface>Offset, change the offset value to zero and the command becomes Copy Surface. Right click somewhere on the outside surface of the part and accept the Select Tangency option. This will propagate the selected face through all bends. Hide the solid body to see the surface body:

Now use the command Insert>Base/Boss>Thicken with the .06” value for thickness. This offsets every outside face the same amount, and the final result is a part of uniform thickness that unfolds without problems: