If your SOLIDWORKS part file seems to be unusable for some reason, but you can still access the feature tree, don’t count the part out just yet. Here is a creative way to salvage your work by transplanting the feature tree into a new part file! This hopefully spares you the time and effort of remodeling from scratch. Note: it will replace the ID’s of the face, edge, and model, requiring re-detailing of the drawing and repair of assembly mates, but at least you won’t have to re-model from scratch. When opening any containing assemblies or drawings, you will likely see a message about a mismatch between the internal ID of the new part versus the original.
- Close all currently open SOLIDWORKS files
- File > New > Part > OK
- From the new part, Insert > Part > navigate to, and single click, the part that has the problem > Open …do not complete the Insert Part command yet.
- In the Insert Part Property Manager, scroll down and check the box to “Break link to original part” > OK ….this causes all items under “Transfer” to transfer in to the new part.
Check these boxes to bring along as much as possible from original part
- Click the green check mark, which automatically sets the origin of the inserted part onto that of the new part, unless the box was checked for Locate Part with Move/Copy feature, in which case the Locate Part Manager will appear, in which case make selections to continue.
- In the Feature Tree, select the newly-added folder (with the same name as the original part) and delete it. Whatever was in the original feature tree should now appear in the new part.
Thanks to the Technical Support team at SOLIDWORKS for passing along this useful tidbit, and a special thank you to the original discoverer.
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