Linked body ID symbol

[JJL79]

Is it possible to create an ID symbol on a linked body in drafting which automatically gets the correct ID according to the parts list? I can only make this by typing the number manually.

 

[JohnRBaker]

When creating the ID symbols make sure that they are actually attached to a component. Not that there is no need to enter anything in the symbol, but rather after the symbols have been created, select the Parts List object on the drawing, press MB3 and select the 'Update Parts List' option. The ID symbols should now contain the proper Item Callout letter/number.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[Arkance/PhoeNX]

Also, you need to have the environment variable UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST set to a value:

If UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST is set to a non-zero value then parts lists will have the pre-NX2 behavior of updating all ID symbols in the part that have rows in the parts list when the parts list updates. Also, creation of multiple parts lists will not be allowed when this variable is set. Set to 0 to allow multiple parts lists.

To set the variable:

Win XP: Windows Control Panel -> System -> Advanced (TAB) -> Environment Variables
or
Win 7: Windows Control Panel -> System -> Advanced System Settings (Upper left) -> Environment Variables

The create a User variable called UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST and set the value to 1. Restart NX and all should be good to do what John has suggested.

Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.0->5.0.6, NX6.0.0->NX6.0.5, NX7.0.0->NX7.0.1 & NX7.5.0.32-> NX7.5.4.4, Beta NX8.0.0.25

 

[JJL79]

I forgot i have to change reference set to Model before i place my ID symbols.