Difficulty with Shell Operation

[RogerInHawaii]

I'm having trouble with the Shell operation. It succeeds when I select a very small value for the Inside Thickness (0.01 inches) but fails for anything larger, even 0.013 inches. My actual intent is for an Inside Thickness of 1.71 mm (which is basically three layers when 3D printing the object) but I can't get it to work for any value anywhere near that., although it works for really small Inside Thickness values.

I just have no clue what it is that it doesn't like, why it can Shell it for a really small Thickness value but fails for even slightly larger values.

It would REALLY HELP if, when it's doing the Shell process and encounters a problem, it would HIGHLIGHT the problem area in the model so that at least I could TRY to change something to  its liking. 

Also, just a side observation: I can save the model as an stl file and bring it up in the PRUSA Slicer, select zero infill and any number of vertical shells and it, PRUSA Slicer, is able to accomplish basically the same thing that the Fusion 360 Shell command is supposedly able to do. But whatever programming approach Fusion 360 takes doesn't seem to be able to handle it. And, no, doing an effective Shell in the Slicer doesn't solve my problem because there's other operations I need to do to the model after it gets Shelled.

My f3d file is attached in case anyone wants to give it a try or try to figure out what it doesn't like.

[wersy]

For printing, you do not need a wall thickness for the stl file. A solid is OK.
Just print with perimeter (lines) without infill.

[laughingcreek]

agreed. fusion falls short on providing this kind of feed back.

the body that's visible when I open the file looks different from the body you have pictured. which body are you trying this with?

I would give up hope on the one that is visible in the attached file. the surface quality for it is among the worst I've seen. would need to be completely remodeled to do anything significant with it in a nurbs/brep modeler.

comparing offsetting/shelling of a mesh file (the .stl in Pursa) to offsetting a nurbs/brep surface (as in fusion) is comparing apples to oranges. Not the same beast.

[laughingcreek]

there is a "divide and conquer" technique that can be used with surfaces to help find the offending geometry. run the surface offset command, in-check the chain select box, and start adding 1 surface at a time to the selection set. the command will fail when the 2 adjacent surfaces that are preventing a shell , etc are selected. of course, you may have more than one problem area...

[RogerInHawaii]

You are missing the point. The issue is with the Shell command. I mentioned that the Slicer can do it (basically to indicate that it CAN be done, just not by Fusion 360), and I noted that my model needs additional operations on it AFTER a successful Shelling, so doing an effective Shell (zero infill) in the Slicer is not an option for what I need to do.

[wersy]

Sorry, you're right, I didn't read through everything.

[RogerInHawaii]

"the surface quality for it is among the worst I've seen"

Insults aren't helpful.

Perhaps, "The model has some surface quality issues, which are likely contributing to the Shell operation failing", and maybe pointing out how to fix them, would be helpful.

The point is that the Shell is working at a thickness of 0.013 and failing for anything thicker. How does poor surface quality allow thin values but fail at larger values?

[RogerInHawaii]

Thank you. I'll try that.

I HAD been able to isolate a prior, similar, issue by slicing the model into a small upper section, doing the Shell and seeing if it fails. If it didn't fail I sliced it for a bigger section. Kept doing that until , very near the bottom, it failed, and isolated the issue to one of the "bolt holes" near the bottom. Doing an operation that "smoothed over" that area and re-creating the bolt hole eliminated that issue and the Shell succeeded. But still only for the 0.013 inch thickness. 

With YOUR approach, what do I do once I determine which two surfaces are preventing the Shell from succeeding? Is there a "heal" operation or something to easily smooth over adjacent surfaces?

[etfrench]

Start by fixing this:

Create a section analysis, then zoom in on the boundaries.

p.s. Basically, anywhere you see a line in the model has this issue.

[TrippyLighting]

---

@RogerInHawaii wrote:

... the Slicer can do it (basically to indicate that it CAN be done, just not by Fusion 360)

---

That is a completely incorrect conclusion!

The slicer will shell using a mesh based approach.

Fusion 360 attempts to create s shell using precisely offset NURBS surfaces/BRep. 

[jeff_strater]

While I agree that Fusion could be better at highlighting problem areas, I would like to point out that it does exactly what you request.  At .1 in, this face is highlighted:

now, this is not exhaustive, and I have seen cases where fixing one problem just leads to other problems.  And, the highlighting does not always show up, I'm not sure why.  I do think that your "dimples" might be contributing to the problem.  Here is one hear the top of the model:

near the upper left there is this one:

These are clearly going to cause problems.  

These sliver faces are also part of the problem, I suspect:

Remember:  Shell is not magic.  Shell has to:

• offset every face of the body by the shell thickness (except those removed)
• add in new faces where the removed faces were to bridge the original surfaces and the offset
• stitch those offsets together
• subtract that from the original

so, it will fail on some geometries.  They better input it has, the better chance of success.

[TheCADWhisperer]

@RogerInHawaii 

Does Ctrl b (CMD b on Mac) return any warnings? (other than for the Shell of course?)

Why is this "dimple" on the left modeled differently than the one on the right?

I would expect to see Symmetry in the Design Intent.

[TrippyLighting]

Even with the timeline rolled almost all the way back (I also deleted the holes) this cannot be shelled.

I was able to see some curve inconsistencies with the bare eye and then inspected some of the edges using the curvature combs tool. 

The center edge can be selected as a whole and looks fine. The right and left upper edges also lok fine but that edge cannot be selected as a whole. THe lower edge as a visible kink in it.

Using the curvature comb inspection tool on it confirms bad curvature:

This is almost always the result of improper modeling technique.

[wersy]

Hi@RogerInHawaii 

It is always very annoying when you find out that you cannot shell a part that you have already invested a lot of work in.
That's why I have made it a rule to check regularly at an early stage whether it can still be shell.
This way you can also recognise problematic areas and change them.

[wersy]

I have erased all the recesses but even this simple body cannot be shelled.
Error message: The selected body appears to have already been shelled.

[laughingcreek]

@wersy - you missed some internal geometry when you were defeaturing-