How do I shell a complex part?

[vas123]

Can somebody can help me out? I am trying to shell a solid part but the shell command is not being cooperative. I am working on a 3D art scan of a full scale male mid section. The scan is in IGES format and was initially a geometric shape (comprising of over 400 individual surfaces) before I had it converted into a solid part.

From the shell command dialog box - in the Part design workbench I select the top of the piece as the face to remove and input the required 31mm inside wall thickness.

After I click ok I get the following message: “current offset value leads to a local degeneration in the surface”
“Some faces can’t be offseted. Do you want to remove them?

I click on yes only to get:
“Update error the result cannot be assembled because of a current or permanent restriction.
Deactivate shell and extract offset surfaces?

Once again I click on yes. “Extract.1” and “Offset.1” components are added to the tree menu with an exclamation mark superimposed on the top left corner of the latter - there was no offset or shell created on the part. Could somebody tell me what I am doing wrong here?
Thank you for your time.

 

[Azrael]

Have you analyzed the solid for tangency problems and minimum radius?

 

[DJBenz]

When you try to perform the shell, you should get some annotation showing which surfaces are causing problems. Then you'll need to work on those areas to get them to shell.

Don't expect it to be a quick job, a lot of data translations end up needing quite a lot of resurfacing to get them robust enough for downstream operations.

Alternative approaches:

1. Start with an open surface and apply the thickness command.

2. Start with an open surface and offset in GSD then create the side surfaces between the two. (GSD offset is usually quite good at identifying where your problems lie.)

 

[itsmyjob]

And if you have GSO license you have access to Rough Offset:

Eric N.
indocti discant et ament meminisse periti ​

 

[vas123]

Thank you for your help! I think I will opt for option number 2 as per DJBenz advice.

However before I begin with the offset procedure I have just one more question: The initial art scan comprises of over 400 geometric surfaces.Is there a way I can concentrate these geometric surfaces into one surface and consequntly have a mesh fee open surface? The rough offset command allows me to input each geometric surface one at a time making the offset procedure a real tedium. Secondly I am really sick and tired of seeing the mesh every time I want to work on the part. I figured after having the open surface converted into a solid they would go away - but to no avail.

Thank you for your time

 

[DJBenz]

Use the Join command in GSD. This will join (go figure!) all the patches into one element. You can adjust the accuracy between 0.001mm and 0.1mm (I'd suggest using 0.1mm in your case).

If you're struggling with Join, the alternative is Heal, which does the same job but will also fix minor imperfections in the surface edges.

You'll end up with one element Join.1 or Heal.1 which can then be used in an offset (or rough offset) operation.

I'm not used to working with data from meshes, but isn't it possible to put the mesh into no-show so that it's not in your face while you're working?

 

[solid7]

It's very unlikely that you are going to be able to do what you are trying to do without extensive "touching up" to the surfaces. IGES imports don't tend to go too well with non-ruled surfaces. (and sometimes even have problems with simple surfaces - inversions being the main headache)

Use the Join command, and then the Boundary command to check for openings.

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