I have an imported STEP file which has been converted to a weldment part in SolidWorks. Some of the parts are bent.
How do I convert these bent parts to sheet metal so I can flatten?
Mark (SolidWorks 2019 sp0)
RMB on each cutlist item
run "Insert Into New Part" command
in derived part, run "convert to sheet metal" command
Worked like a charm.
You can run "convert to sheet metal" command inside this file too
Another question on this, how can I get the flattened length in to the cut list, Do I have to manually add it. At the moment the cut list shows the bounding box size which is a lot shorter than the flat pattern size.
What is the name of your property?
It must be "Bounding Box Length" (not 3D-Bounding Box Length of bounding Box feature).
Its showing 3D bounding box, how do I change it?
No way, but you have to look at "Bounding Box Length" instead, it contains the length of flat pattern as you wish (not length of the bended part).
yes I know how to get a flat length bounding box but I wanted this length to show in the cut list, so the only way is to manual edit the cut list properties to show the flattened length.
Upload step file please
Sorry not allowed
Ok, do you have the nearly the same list of properties of cutlist item?
Mark, I think you're still using original bodies which are not sheet metal features.
You should try to convert to sheet-metal inside the part, as Igor suggested in the second place, then the cut list refers to sheet metal bodies.
Sergio / Igor,
Thanks for your suggestions both work.
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