SolidWorks Sheet Metal Problem

I’ve managed a work-around, but I’m encountering an intermittent SolidWorks sheet metal problem, can anyone help?

Simple sheet metal shape, 1.5mm thick with 3mm bends, right is the desired result, left is the initial shape before converting to sheet metal:


post conversion, the flat configuration which is meant to go to the laser cutter, but it gets these little jagged edges (highlighted red and green):

I can see the jagged edges are caused by cutting a bend on an angle, but the folded configuration should show a distorted edge, the flat version should be dead straight. It’s intermittent though. I found the problem was sometimes solved by changing the fixed face and bend edges:

Anyone have any ideas?

Probably a stupid question, but have you tried drawing the part in sheet metal (Base Flange/Tab as the first process in the tree)? I’ve never drawn parts as solid and then converted as I have been told there can be problems/quirks if you do so.

Start with the flat shape first (as a sheet metal feature, therefore your entire tree should be sheet metal) and then add the bends afterwards, with the middle section being the flat/fixed face. Let us know if that helps; it’s just a suggestion off the top of my head.

I apologize for I am not able to verify this workflow as I have no access to SW this week.

Option 1

  • Create your shape as an extrusion, but do not cut the sides. Leave all edges square.
  • Convert the part to sheet metal and let SW create the bends as normal
  • Extrude a cut from the top to shape the sides. Click the box that forces the cuts to be normal to the sheet metal flat surfaces (the box hould say, “Normal To” next to it) Hopefully this will cut the part and leave perpendicular edges. It might remove more material than desired.
    Normal Cut - 2013 - SOLIDWORKS Help
  • Flatten and check things out.
  • Depending on the outcome, curse my name or praise my name.

Option 2

  • Create your shape as an extrusion, but do not cut the sides. Leave all edges square
  • Convert part to sheet metal and let SW create the bends as normal
  • Flatten the part using unfold
  • Make the cuts on the flattened version. Might be tricky considering you are trying to get the flat pattern rather than specifying.
    Cutting Across Sheet Metal Bends - 2013 - SOLIDWORKS Help
  • Fold it back up and check it out.
  • Depending on the outcome, curse my name or praise my name.

I think the more robust way is to flatten the part as suggested in option 2 above before making the angled cuts. That way you can be sure the flattened part is nice and pretty. Doing cuts with the “normal cut” box checked should work and I do use it when it would be difficult to figure out what the flat looks like, but you’re making SW work harder and sometimes it gets spiteful when you do that (to put it technically).

Also, it’s probably a little more robust and one less step if instead of converting that solid to sheet metal you just start with the base/flange command. All it needs for your shape is three straight lines, then you pick where you want the material to be (like on an extrude thin).

Cheers Sprockets, making the cut post creating the sheet metal part with “Normal Cut” selected has worked. The “Normal Cut” option doesn’t appear unless it’s a sheet metal part, which makes sense.

The result is the cut edge when folded shows distortion, but when flat is dead straight.

Thanks to all the other suggestions, but the part is created in-context in as assembly, and also the strength/ attraction of SolidWorks sheetmetal is to model a part and then press a magic button to convert it to a flat sheet, rather than buggerising around with bend lines.