Shell failure

[etfrench]

Shell command is giving the following error for the component,ShellFailure, in http://a360.co/1OSRfC1

  The operation could not create a valid result.
    Try adjusting the values or changing the inputs.

Adjusting the values does not work.  The error message does not contain enough information to correct the problem.

A similar component, FanHopperAndDucts, was successfully shelled.

[Phil.E]

I'll take a look. Might need to respond tomorrow, it's near the end of my day.

[joel.palioca]

Hello,

Looking at the model it looks like there are some locations at the bottom of the shape that are going to be very hard to have shelled an appropriate amount.

One way I used to help determine where some problems may be at was using the surface environment in fusion.  You can delete the bottom face of the body and it will turn into a surface.  From there you can use the thicken command on each of the surfaces that are created and use your hopeful shell value as the thicken value.  This won't be exactly the same as a shell, but should be similar enough to help diagnose where there problem may be at.  By doing this and using very small values I was able to see that the 3 faces shown below seem to not respond very well to being thickened past a specific value.

On another note I do agree that the error message below could be improved.  I will bring this up with the team and see what we can do for the future.

I hope this helps, if you have additional questions please ask.

Cheers,

[PhilProcarioJr]

Joel,

Is it possible for the software to try to shell, and if it fails, color failing face to let us know where the problem is?

[joel.palioca]

We don't have this capability at this moment, but this is a great idea.

I would recommend going to the IdeaStation and submitting this as an idea.  Other users can view your idea and upvote it, I know I would.

http://forums.autodesk.com/t5/ideas/v2/ideaexchangepage/blog-id/125

Cheers,

[etfrench]

The individual components making up the assembly all shell successfully, so I would expect the joined components to shell successfully as well.  I modified the model and was able to get it to shell at .4983mm, but not at the goal of .5mm. I added this to the drawing.


There is also another workaround that was successful:

1. Make a copy of each component.
2. Select one of the components as the master.
3. Outside Shell the other components (not the copies or the master).
4. Combine the Master with the other original components, cutting the Master from the original components. (Save tools in all Combine steps).
5. Shell the Master.
6. Combine the  Master and the outside shell components, cutting the outside shells from the Master.
7. Shell the copies.
8. Combine the Master and copies, joining all to the Master.

[etfrench]

I've added another shape to the original drawing that can't be shelled.  It's a simple loft between two non-parallel planes.  The component name is 'NonParallelPlaneShellFailure'.

[Anonymous]

Wanted to mention when all else fails to get the last little bit of thickness desired one can do a two direction shell, so that can also thicken in outward direction, which is usually a lot more forgiving.  Afterwards, can get close to desired original dimensions via scale, nonuniform scale, press/pull whole sides, etc. 

Jesse

[Phil.E]

Thanks for the new model. While you call it a 'simple loft', which it may be to you or the Loft command solver, it produces a shape that is hard to shell, obviously.

I'll log this against the shell command, to see if they can improve it. FYI: there are limitations to some of these commands, you have found a couple of good examples. The first example sort of begs the question: why are you shelling this? Just curious, but the 'tree' shape you have made cannot be produced on any machine except a 3D printer, unless I'm missing something. So how did you plan to manufacture this, and is the Shell critical to the finished part?

For your second case, I have a workaround, you can try these steps: Offset the loft sketches and loft again as a cut.

Thanks,

[etfrench]

I modified the shapes to try to reduce the number of narrow spaces and was able to shell it at .5mm.  I added this to the original file as 'FinalManifold'.

My 3dprinter is finally working well enough now to print parts for it:)  The tree structure is a print fan manifold.