NX 8.5 PMI Section "Wire or Acorn Body" error

[JetFueledEngineer]

All,

While creating a cross-section cutting through 90 degrees (one quadrant) of an assembly, NX yields the following error message:

Modeler error: wire or acorn body is unsuitable for this operation

I've created similar cross-sections on other assemblies and have never gotten this error. Any thoughts as to the root cause and fix?

Thanks!

James
NX 8.5

 

[JohnRBaker]

In that case, it's probably part specific and therefore GTAC may be the only people who could help you track this down.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[JetFueledEngineer]

John,

Thanks for the info. I'll see what troubleshooting I can work through and go from there. Thanks!

-James

 

[JohnRBaker]

Yes, you could run Examine Geometry on all of the component parts of the Assembly as that might flag something which could be the culprit and I guess it might be possible to repair and then continue, but try not getting too bogged-down and end up wasting a lot of time.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[JetFueledEngineer]

Thanks! I found it by process of elimination. Evidently the PMI section view command doesn't play well with models that use the "Delete Body" command. After modeling the surface without the command, it works just fine. I'll have to remember the Examine Geometry command for the future.

Thanks!
James

 

[JohnRBaker]

I've tried to reproduce this using NX 8.5.3.3 and was not able to. Could you either provide the minimum assembly in which this error appears, or at least a picture of what you're doing showing the body that you 'deleted'?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[JetFueledEngineer]

Hi John,

I can't provide the file or a picture of it, but here's a description that might clear it up a bit. I made a revolved body and used an extrusion to subtract everything but a small circular area. This operation left two bodies, 180 degrees apart from each other. I used the "delete body" command on one of the bodies, leaving the one I wanted. The PMI section error only showed up after assembling multiple parts into the next higher assembly and trying to make a section at that level. I fixed the error by making the initial revolved body through 180 degrees instead of the full 360. Does that help?

Thanks,
James

 

[JohnRBaker]

OK, I've able to reproduce the problem when creating a model, similar to what you've described, using NX 8.5.3.3.

I also testing NX 9.0 & NX 10.0 and the problem exists there as well, so I'm going to open a PR since this really should work.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[JetFueledEngineer]

Thanks John! Hope it helps everybody out.

-James