What to do when loft prevents shelling?

3vi1

Greetings! I'm a complete Onshape/CAD newb, but have been trying to teach myself over the last couple of weeks as I recreate the curves of real-world pieces.

Unfortunately, the lofting that's required for one of the components in my current project seems to completely break shelling ("Shell did not regenerate properly: Could not shell part with selections"), and I don't have the experience to know why. I've searched the forums here and found users that have run into similar issues, but their particular solutions don't seem to apply in my case.

In the picture below, you can see I'm trying to shell with the bottom piece. The lighter yellow piece is where I have my cursor highlighting one of the four matching lofts in question. I'm sure the problem is generated by the loft, as I did not have any issue shelling the part when I was instead using a simple extrude and fillet (which couldn't give me the correct transition to match the actual object… hence my move to lofts).

If I reverse the direction of the shell, it highlights the lofts.

Please forgive the numerous suppressed steps. I've been down a lot of blind allies as I experiment.

The public document is here: https://cad.onshape.com/documents/e99c355693eee9eb36d8f22a/v/c6542a36c989e548bb4c5f37/e/38181df396fd552e0d804c2a. Any pointers are greatly appreciated.

MDesign

Self interaction is usually a culprit for shell features. Try a really tiny thickness to see if it clears it up. Then bump it up bigger incrementally. To experiment. The red highlighted surfaces point you in a direction of the issue.

S1mon

There are a few issues which are making this challenging.

1. There are some weird (likely unintentional) voids that are created by loft 1 and loft 2
2. Loft 1 and 2 are both creating really bad surfaces because they are fighting against what surfaces want to do
3. You are creating things two or four times (all your lofts) where you could make 1/2 or 1/4 and mirror the results
4. Many of your sketches are un- or underconstrained
5. Your shell thickness has been toggled to add to the outside instead of creating a wall on the inside - is that intentional?
6. Your hump profile curves are not very clean and don't join with even tangency in the center
   

I didn't clean up all the above, but by adding some fillets to cover up some issues and selecting the voids (#1), and flipping the shell (#5) I was able to at least get a 1mm shell to happen.

https://cad.onshape.com/documents/fb84b8b9e2b1f456e74fd801/w/321dbb67a45ba64217cb4a57/e/ffd5d384a4c68162cde7a92c

glen_dewsbury

Ditto what S1mon said.

Unfortunately the aspect ratio on images is out of whack as well. To get consistency between them you'll need a different to tool than OS that can adjust image in 2 directions instead of one, along with some actual overall dimensions to make them directly traceable. It's been a while and I don't remember the names of the tools I got to work. It was a trial program that has long since expired. The differences have to do with how a camera takes pictures.

3vi1

https://forum.onshape.com/discussion/comment/111522#Comment_111522

I neglected to mention that while I was looking up similar topics, I tried setting the shell to 0.01mm (the smallest possible) yet it still failed. Thank you for the suggestion though.

3vi1

Thanks for the tips!

The voids created by lofting were the root problem, once I saw how S1mon had selected them I was able to do the same and create a reasonable facsimile of the original part with my original 1.25mm shell size.