A Loft, a Shell, and a Boolean walk into a bar...

[william-c-anderson]

After creating a loft and "shelling" it, I wished to use the Boolean combine tool to (first) cut a new body for an interface, and (second) then combine a portion of the cut body into the previous tool body. The second Boolean operation fails. I've attached an example file (part of a project on which I'm working) which demonstrates the error. If you try to use the Combine function to join the two bodies which are left at the end of the timeline, it will fail to even put a combine icon into the timeline.

BTW, I was able to work around this issue by selecting the interfacing faces of the cut object and "pulling" them out by a fraction.

[TrippyLighting]

This is not a surprise. This is a possible near-coincidence problem and your workaround provides a clear interface that the kernel can use to trim surfaces.

I am surprised this even shelled. The loft creates a very complex NURBS surface. If you use the gaussian curvature map on the shelled body and look at the interior surface, this is an indication that there are problems.  

BTW, best thread title ever!

[william-c-anderson]

So, @TrippyLighting, what you are saying is that a Boolean cut has a non-zero-thickness "kerf", and that a Boolean cut is not always invertible with a join. That is, a Boolean cut loses information. Is this correct? This is certainly different from other mechanical CAD programs I've used.

[TrippyLighting]

No, bit I guess I have to be more clear: The input geometry is of questionable quality!

It starts with the terrible curvature of the imported geometry:

And then continues with a loft from a sharp corner blending into a curve. It is even surprising that Fusion 360 shells this.

But that abomination of geometry even shells and creates a fading crease in the inside corner:

 

Which results in rather bad surface curvature :

All along the way right from the start, you force the software to make approximations.

It is no a surprise that this fails at some point in time.

So here is my recomendation.

1. Start with proper input geometry. Use the imported geometry as a visual guideline and re-create the sketch from scratch with FUiosn 360 native geometry.

2. Change your loft strategy. At no point in time should a loft transition from a sharp edge or crease to a curve. Then, this should unlikely be a single lofted surface. 

3. If you shell then make sure that fillets on the outside are large enough so wall thickness of the shell plus radius so the inside surfaces do not collapse on themselves and create possible self-intersections. Again I don't think FUiosn 360 should even shell this, at least not without a proper warning.

[jeff_strater]

"what you are saying is that a Boolean cut has a non-zero-thickness "kerf", and that a Boolean cut is not always invertible with a join. That is, a Boolean cut loses information. Is this correct? This is certainly different from other mechanical CAD programs I've used."

This is a good question.  In general, yes, cut followed by join of the result bodies should be OK. In this case, it could just be a bug in either the cut or the join, or it may just be small numerical inaccuracies introduced by the cut.  Solid modeling is still a computer program, so is limited to the accuracy of the numerical operations.  There could be some approximation introduced by the cut that makes the subsequent join fail.  I will have the modeling kernel folks take a look, but in general, listening to @TrippyLighting is always a good idea.  Better geometry will always produce better results.