Drawing opening problem

[sft11]

Hello I'm having following problem when trying to open drawing. Informarion window says "The following circular update was detected:" and in the pop-up window it says "The following files could not be loaded causing this open to fail:" "There is an object which depends on itself"

Most likely the problem is with the interpart expressions used in the drawing but there is not any way to fix those as I am unable to open the drawing in the first place. Is there anyway to force NX to open the drawing?

Any help is appreciated, thanks!

And I'm using NX8.0

 

[looslib]

Try opening the assembly file with load all components turned on.
The interpart relations should be in that file, or lower, and not in the drawing file.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

Start a new session of NX but before you attempt to open your Drawing, go to...

File -> Options -> Assembly Load Options...

...and make sure that the 'Load Interpart Data' option is toggled OFF.

If that doesn't help, with the above setting still toggled OFF, try setting the 'Load' option, in the 'Scope' section of the dialog, to 'Structure Only' and see if that will allow you to open your Drawing. If so, then try to fix or remove those interpart expression links.

If that fails, please contact GTAC as they have some additional tools that they can use to fix your part files.

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.

 

[sft11]

Thanks guys for your prompt replies!

I already tried those load options but those didn't make any difference. We are using NX in teamcenter environment and we are able to load 3 rollback versions of our NX files. But there was the same issue with all of those (maybe I'm too used to not that stable cad systems ). Fortunately I was able to track down from my local drive NX temp folder an older version which I was able to open again. I tracked down the problem to the fact that both drawing and model had exactly the same names, though different item numbers of course. When the drawing was opened and saved without having the model file opened simultaneously, the interpart expressions changed to the drawing itself which caused the issue.

Might be a bit dum question but what GTAC is? I was in contact with the finnish partner of Siemens PLM. They weren't able to open the drawing with NX8.0 either but with NX9 and NX10 they said it was possible.

But lessons learned I should keep my models and drawings named uniquely at least when having interpart expressions!

 

[saumechanica]

@-Sft11

GTAC --> Global Technical Access Center

https://support.industrysoftware.automation.siemens.com/gtac.shtml

 

[Toost]

That's a tricky problem, where these parts created outside Teamcenter and later imported to Teamcenter ?
I-deas conversions ?

Regards,
Tomas

 

[sft11]

Model was made with native NX and then imported to Teamcenter at some point. Drawing was made directly to Teamcenter. Does that make some difference if models are imported?