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Linked Mirror Part (NX)


Does anyone know of a way to break the link of a Linked Mirror Part?

The part that this came from no longer exists and the part that is so called linked is constantly shown as out of date.

There is an attibute in the model, but I can't seem to find a way to remove it. I thought I remembered somewhere by deleting the attribute the link can be removed completely to make the model as a stand alone NX part.


This was originally created with the WAVE function:

  • In the Assembly Navigator , right-click the component node for the part you want to mirror, and choose WAVE Create Linked Mirror Part .




Re: Linked Mirror Part (NX)

Siemens Phenom Siemens Phenom
Siemens Phenom

'MirrorPartType' attribute can be deleted from the properties. You have to make changes to the attribute in the Attributes Templates.




File > Utilities > Attribute Templates. Select the attribute 'MirrorPartType' and uncheck the option 'Enforce Constraints'.




Under the properties of part, select attribute 'MirrorPartType' > RMB > Delete. It will remove the value of the attribute. Note the change in icon in 'Info' column of ASN. It will change from 'Part is a Linked Mirror Part' to 'Part is a Linked Part'




In 'Attribute Templates' select the attribute template 'MirrorPartType' > RMB > Delete. It should get delete. Check under the properties of part, attribute 'MirrorPartType' will not be listed anymore.


Also break the interpart links by using 'Interpart Link Browser'.




Hope this will solve your problem!


Ganesh Kadole
#IngenuityIsNX | NX - What's New

Re: Linked Mirror Part (NX)


Worked just as you described.

Thank you so much for the detailed instructions and video!

Much appreciated!