I have a bent piece in parasolids, that I need to make into a cut piece.
Depending on the part, you can convert that into sheet metal. Can you post part or picture of it?
Use convert to sheet metal tool under Sheet Metal and you can easily convert this to sheet metal (assuming the thickness is uniform) and then flatten as required.
Thank you for your info. As I kept playing around, I noticed a body with a flatten choice, which I did and it unbent the whole thing..... Thank you again...
Deepak is correct, but in case you don't follow the instructions:
Thanks Jim, this will be very helpful in the near future....
A little more about sheet metal.. If you get into sheet metal modeling in detail you will want to know the difference between unfold & flatten.
Unfold (circled red below) will add an unfold feature to your feature tree. Flatten (circled green below) will unsuppress the Flat-Pattern feature at the bottom of your feature tree.
If you just need to know the blank size or export the flat pattern to a cut file, either approach should work for a quick answer. If you need to create a print from your file there is a difference. If you take any sheet metal model and make a drawing from it, you will automatically get a flattened configuration in your configuration tree.
This configuration is your part with the Flat-Pattern unsupressed, same as the Flatten tool. Having these configurations is the most direct way to have a view of your flat part on your drawing simultaneously with a formed view. If you make additional configurations with say a pilot hole size or a different flange length, you can toggle the Flatten tool on / off for those configurations as well.
Unfold is best suited when you need to trim your formed part back across a bend. It happens more often than you may first expect. Sometimes you have a part that has a contour going through a bend. It can be better to make a model that's long across the bend, then cut away the extra. You Unfold, make your Cut-Extrude, and Fold it back up.
I typically just use the insert bends sheetmetal feature when working with dumb solids in SolidWorks. I think it is easier and involves less input than converting to sheetmetal does....
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