Myself, and a coworker have both recently had a shell operation fail, when updating a part. When the shell fails, it doesn't show an *, or other indication of where the issue lies. In my case, the edits I was making were very localized, but not so much with my coworker.
We have tried Examine Geometry, looking for a tiny face, etc. Loosening the model tolerance from .0004 to .017 will get it to shell, but it doesn't look correct. User has tried to thicken the outer faces inboard, selecitng a face at a time, to see when/if that fails, hoping to narrow down the problem area, but hasn't had any luck yet.
Are there any other tools to narrow down where the shell is having issues?
My usual method is to extract a copy of the body then use the offset face command (body face selection rule) with the offset size equal to the shell offset. This will usually highlight the edge or face that is causing the issue.
Shell and offset errors are usually caused by an area of a face that has a smaller curvature value than the desired shell thickness (which would result in a self-intersecting face or consistency error). You might be able to use one of the analysis tools that checks face radius values to find this condition.
Make an offset datum plane from one side of the body and cut away the large portion of the body by trim body.
Test the shell command in the small portion left.
If it failed it means the problem area lies in the small portion. If it succeeded offset your plane a few milimiters ahead and repeat the procedure.