Flattening Imported Sheet Metal Part Files

SOLIDWORKS gives you some great tools to flatten imported sheet metal part files. The tool called “Insert Bends” automates this process. After identifying the fixed face, SOLIDWORKS adds sheet metal information such as Bend Allowance, Auto Relief, as well as Rip Parameters. This works great as long as you have a part with uniform wall thickness. If you find yourself with a part who’s thickness varies (as is the case often in bends), then here is a trick to try out.

• Right click on a face as shown below and pick “Select Tangency.” This should highlight all of the faces on one side of your part. Now use the surfacing tool “Offset Surface,” setting the offset value to zero. This creates a surface that is wrapped on the top or bottom of your part.
• Locate the Folder titled “Solid Bodies” near the top of your Feature Manager. Expand this folder, select the body that is listed and choose “Delete” (from right click or keyboard). Now you are left with only the surface body that you have created.
• Select the surface body and use the “Thicken” (Insert/Boss Base/Thicken) feature to create a solid by thickening the selected surface in the direction and value that you select. This process ensures that you now have a uniform wall thickness.
• Now you are ready to flatten the part as usual with the “Insert Bends.”

This process is one that I use a lot when dealing with problematic sheet metal files. The steps above should help you create geometry that is able to be flattened if the error initially was a result of inconsistent material thickness.