Shrinkwrap oddities

[khauswirth2]

I am using Shrinkwrap on an assembly but getting some strange effects, either surfaces appearing out of nowhere (#1 and inner orange cone) or surfaces that should be included not actually appearing (#2).  Both seem to be based on a C-Face Motor Mount part (light blue in left side assembly).  If I exclude the C-Face both problems disappear.

No matter whether I save the Shrinkwrap as a Single Solid with or without seams, or as a Single Composite, the oddities remain.  If I save the Shrinkwrap maintaining Individual Solids, the surfaces of #2 are shown but the cone in #1 remains.  I have selected to remove all holes and pockets but not remove fillets and chamfers, as well as checked to fill all internal voids and remove internal parts.

I am currently running Inventor 2021.3.1 on Windows 10 Pro, 32 GB RAM.

Any thoughts?  Thanks!

[SharkDesign]

I'd suggest the removing holes, filling voids etc etc is causing it, but it'd be easier to check if you upload your part.

[khauswirth2]

That seems to be it!  If I only select remove holes or only select remove pockets the problems are gone, but choosing both at the same time leads to the strangeness shown.  Thank you!

[SharkDesign]

I don't know for sure, but it probably uses something similar to delete
face to do it and when you do that manually you sometimes get weird stuff
like that.

[johnsonshiue]

Hi! I suspect this is geometry related. Open the assembly and press Ctrl+F7. Is there any bad body reported? If yes, please go through Repair Body workflows to fix the bad geometry.

Please feel free to share the files here. I can take a look and see why the geometry is not properly merged.

Many thanks!

[gcoombridge]

I find this sort of thing happens where you remove fillets on a tapered cone that terminates in a radius. It happens when you remove fillets on a hygienic triclamp ferrule - running the taper back to the intersection of the two faces. You should be able to preserve the feature

[khauswirth2]

Nothing happens when I press Ctrl + F7.  Does this only work if there are bad bodies?

I have attached the C-Face .ipt that seems to be the main cause of issues in this assembly.  It is slightly smaller than the one we actually have but is the closest I could find and extract from online models of similar motor assemblies.  I suppose some of the intricate geometry could be the issue.

Finally, when I use a Shrinkwrapped .ipt with missing surfaces (below left) and export to .stp (below right), the surface issues seem to disappear anyway!

[johnsonshiue]

Hi! Ctrl+F7 should bring up a dialog showing the body statistics regardless of quality. You may need to add C:\Temp\ folder. Or, clean up %temp% in File Explorer.

I took a quick look at the part. It checks clean. The only thing I did was to move it to Repair Environment, Unstitch, and Restitch at very tight tolerance (0.00001mm). Please try it out and see if it works better.

Many thanks!