Parts List and ID Symbols

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thread561-299247

Please reference the afore mentioned thread. Is it necessary to to select an edge with an ID symbol, or is selecting a surface a viable option, and have the ID symbol update when the parts list is updated? Someone told me that i should be able to select a surface of a component to attach the ID symbol and it should update when the parts list is updated. In our system this does not work, an edge needs to be selected. Is there an option in Customer Defaults or UGII that I am missing?
Craig

 

[ewh]

Choose "face" under the selection filter.

Technically, the glass is always full.

 

[PowderBlazer]

"Face" selection filter does not help. :-/

 

[ewh]

bummer, works for me. Is the appropriate layer selectable? Is "entire assembly" selected for selection scope?

Technically, the glass is always full.

 

[JohnRBaker]

It works for me, using both NX 7.5.5.4 and NX 8.0.1.5. BTW, tyr checking to see if on the Preferences -> Assemblies dialog that the 'Component Member Select' option is toggled ON (not sure that this will help, but I always have this on and I never have any problems with stuff like this).

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.

 

[aszepesi]

John,
Does this work with the autoballoon command, too?
When you use the autoballoon to create the ID symbols first and you change one ID's location to one other part's face then the ID symbol can't update with the Update Part list command. Is my right?

Attila Szepesi
support engineer
graphIT Ltd.

http://www.graphit.hu

 

[JohnRBaker]

I deleted an existing 'Auto-ballooned' ID symbol and then created a replacement, manually selecting the 'face' of a Component before placing the symbol on the Drawing. I then selected the Parts List and forced an update and the proper Callout letter was inserted into the newly created ID symbol. In the case of NX 7.5 the initial symbol was created with some random 'callout' letter which was subsequently changed to the correct one when the Parts List was updated. In NX 8.0, the newly created ID symbol was created without any 'callout' letter which was only added as a result of doing the Parts List update.

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.

 

[PowderBlazer]

All layers are selectable and the entire assembly is in the selection scope. "Component Member Select" was not on. I checked it and there was still no change. We are in 6.0.2.8. I tried on 6.0.5.3 and received the same results. There has to be a setting I am missing somewhere. I believe we have had the same problem since switching to NX back in NX2 or 3.
I also think the "setting" i am missing has to do with us having to add sketches to a dwg reference set, so we can dimension sketches on the drawing. Most of the time we can select edges, but occassionally we need the sketches put on a dwg ref set.

 

[JohnRBaker]

OK, I tested this, using an identical assembly model, with NX 6.0.5.3 and it does NOT work. However, it does work in NX 7.5 so I have to assume that there was a problem with NX 6.0 which has been addressed in NX 7.5 (I also tested this with NX 5.0.6.3 and it failed there as well so perhaps this was actually an enhancement with NX 7.5).

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.

 

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Thanks John and all of you that chimed in!!