These two cut-extrude features look fine in both the part itself and the assembly, but I can not get the rebuild icon to go away. They rebuild in the part but still won't rebuild in the assembly.
I didn't look at the part -
Three things to check...
#1 - Edit the Sketch Plane and see if there is a missing face or plane
#2 - Edit the Sketch and check the Sketch Relations
#3 - Edit the Feature and see if there are missing "Up to Vertex" or "Up to Surface" or "Offset"
It's always one or more of all three..
I am not seeing any, but in my experience, it is typically caused by a circular reference. You might have to look closer at your external references for this part.
Thanks guys. I went back to the sketches and changed some relations. The problem happened after an assembly level hole wizard, so it must have changed an edge or face somehow, even though there were no dangling relations. I really appreciate the advice!
It's something to do with the last 7/16 hole in the assembly. If you click off the "Propagate feature to part" everything rebuilds fine...but you are missing that hole. Don't know why that hole is a problem.
Tom Sidlauskas is correct if you remove the midpoint relationship on that hole in sketch19 it will rebuild. I think this is causing the circular reference that I was describing. Good luck with your part.
I fixed it by going to the sketches on the two cut-extrudes and deleting some coincident relations. I kind of cheated and used the fully define sketch command. Like you said, there was something about that hole that it didn't like. Anyway, it's working nicely now. Thanks Tom and Casey for checking it out for me, and John for the advice. Solidworks forum members are the best!
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