When flattened, It appears this part is deleting all that is not on the same plane as the flat face. Anyone see this before? I have but it has been years. Any ideas would be greatly appreciated.
Roll back to just before your last cut and put in an unfold feature. Roll forward to just after the cut and put in a fold feature. Your part should now flatten properly.
that got it, works with drawing flat pattern as well.
I would like to be able to do a flange extrusion but as was said, didn't work for features. Also, the extrude to surface is needed for design intent.
Thanks Jeff and Deepak for your help!
Oh Solidworks, so tricky. Open the files today and even with the fold/unfold before/after the last cut, same result as tuesday. flattens with only a portion of the part left. Have attempted redoing the fold/unfold but with the same results.
This is the first part in an assembly with all other inplaces either on it or based off of secondary parts. If I have to, I will hide and create new part over it but would like to find a solution.
Any further ideas besides taking it back to formula?
Nothing changed but it reverted to its previous behavior? I wonder if it wouldn't be better to create it from scratch, but with all sheet metal features.
Report to your VAR plus replace base extrude features with sheet metal tabs.
Not sure if this is a bug or expected behavior but I feel the boss extrude features are the reasons for the issue you're seeing. Use base/tab flange feature from sheet metal and it should take care of that.
I've added the updated part for reference.
It's actually his last cut that's causing the issue, Deepak. I initially had the same thought as you, but found that you couldn't recreate the boss extrude with the base/tab feature. SolidWorks didn't like it.
Actually just found out that the issue is missing face in the first feature which is causing the issue. If you change the Base-Flange1 option to blind instead of up to surface, then it takes care of the issue.
That is does. I assumed that the up to surface feature had to do with the external reference and was part of the design intent.
Yes. But if you keep that feature at it is and delete all other boss and cut features then also the flatten doesn't work properly.
This is interesting to say the least Al. It doesn't seem to matter when you put an unfold/fold in (as long as it is after the base flange) but that seems to tell SW that this is indeed a bend (you do have to force that). Notice that in your file there is no "Flatten Base Bend1 in the expanded Flat Pattern. After doing an unfold and fold there is one. You don't have to have another operation in between.
I also tried adding a .375 fillet to your base sketch (without any other changes) and that worked also.
I suspect that the in (or out of) context relations has something to do with this. I also suspect that you didn't really want that last cut. Figured you put that in there hoping it would resolve the problem.
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