NX 12 - Extrude dialog settings stuck on Sheet instead of Solid 1

[BOPdesigner]

For some reason, Extrude/Revolve settings are defaulting to Body Type = Sheet instead of Solid. This happens randomly and I can't figure out where to fix it. Happens to other users also from time to time. Is there something in Customer Defaults? I can't seem to find it. It is a nuisance when modeling, but in other areas it causes real issues, like PCB Exchange, when you import a circuit board and internally it uses the extrude command to generate the PCB and gives you a hollow sheet body instead of a solid board because you don't have an opportunity to change the body type to sheet. Where can I change this setting to Solid and have it stick?

 

[JohnRBaker]

Check your profile. If it's not closed, the system will default to a Sheet.

John R. Baker, P.E. (ret)
Irvine, CA
Siemens PLM:
UG/NX Museum:

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[Arkance/PhoeNX]

The body type option for Solid or Sheet is on the dialog under settings.
It may be hidden from the dialog.
If you use the gear in the top left of the dialog, you can show collapsed groups, then expand the setting section (see image below).

You could also try resetting the dialog using the circle arrow (top right of the dialog).

The other possibility is that dialog memory is remembering what's been set on the dialog. This is usually held in the DialogMemory.dlx file.
Usual path to this file is like below, this may be different on your system.

C:\Users\username\AppData\Local\Siemens\NX120\DialogMemory.dlx

Anthony Galante
Senior Support Engineer


NX9 to NX2008 (11 versions)

 

[cowski]

In addition to the above suggestions, check the modeling preferences -> general -> body type option (it can be set to solid or sheet). This option (part specific) will set the default for the dialog and the dialog memory, mentioned by Anthony, would override this setting.

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