How to salvage imported sheet metal data the easy way in SOLIDWORKS

Article by John Lee, CSWE updated August 3, 2020

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What if you receive an imported sheet metal model with weird abnormalities, like jagged edges or crazy surface shapes?

SOLIDWORKS Imported Sheet Metal Service

SOLIDWORKS Imported Sheet Metal

Maybe it’s not even a solid, due to these issues.  I’ve seen a few such models while working in the sheet metal industry, where it was so “not right” that it defies trying to put into pictures, as I’m not even sure how to model such stuff.  Flattening such a model might be impossible unless/until you manage to capture just the intended design while eliminating the weird stuff.  So here is a very efficient way:

  1. Decide which side is closer to the intended design: the inside or the outside.
  2. Right-click that side and choose Select Tangency, assuming that the model has round bends.  The entire model should now be selected, on just the one side.  If the model has sharp bends, then you will need to Ctrl-select all the faces on the chosen side.
  3. Do an Offset Surface of zero distance.  This will copy the entire side of the model as a surface body.
  4. Thicken the new surface body to the correct sheet metal thickness and to the correct direction.  You should now have an exact or almost exact replica of the original design, without the geometric oddities.  I said “almost exact” because before you delete the original solid body, you will want to take note of any geometry that is different between the inside and outside faces, such as countersinks.  You will want to ensure that those get carried across to the new solid body.
  5. Insert Bends to apply sheet metal properties and the flat pattern.
  6. Delete/Keep Body to delete the original body.  This adds a delete feature to the tree to remove the original body from the model, but it will still be accessible for reference if you roll back in the tree.

Note:

  • Solid and Surface bodies are listed in their respective folders at the top of the feature tree.
  • Any commands (features specified in the steps in this article) can be located or launched by doing a Command Search.

How cool is that?  😀

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John Lee, CSWE

John Lee is inherently lazy in that he prefers to work smarter - not harder. A CSWE with fifteen years of experience using SOLIDWORKS and a background in mechanical design, John has used SOLIDWORKS in various industries requiring design for injection molding, sheet metal, weldments and structural steel.