part visible in drawing but not in modeling

[rdln]

Hello, I have a nx7.5 drawing of an assembly in a teamcenter session that was probably drawn in nx5 (may not be the issue but I am setting this Q up) anyways, components do not show up on the modeling side, its not a layer visibility issue.

Something that is a clue I am sure though is the ANT icons for the components of the problem part have a drawing border behind the part or assembly icon. If I copy and paste the component asm back into the drawing file, the parts show in the modeling side and there is no drawing border in the icons of the pasted part.

I dont want to reassociate drawing items back to new part though.

shot of ANT att.

 

[JohnRBaker]

They may be view-dependent. Or there's a Reference Set which have excluded the Components.

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.

 

[JohnRBaker]

Upon second thought, based on the icons that are shown in your Drawings Assembly Navigator, it would appear that when you created your Drawing and were adding what you thought was the Assembly to your drawing, in reality you used a function intended to add ONLY the views of a part onto the Drawing sheet but without actually loading the Assembly, or it's sub-Components, as Components to the Master Model Drawing. In essences these views contain what looks like Components but they exist ONLY on the face of the Drawing. That's why when you close the Drawing and look at the 'model' there is nothing to see.

Note that I was able to reproduce in very short order the same exact situation you have with all of the same behavior and visual information as seen in your Assembly Navigator.

To avoid this in the future, you need to follow one of two workflows; either open that Part file first, be it an Assembly or a single Piece part model, and then add the Drawing to it. Or if you open the Drawing first, you must then add your Part file using the traditional...

Assemblies -> Components -> Add Component...

...accepting whatever location is offered and THEN go to...

Insert -> View -> Base...

...and place your Drawing views.

And before you ask, I'm not aware of any way to undo this in an existing drawing file short of starting over, either with an actual Assembly of the part model or if the assembly only existed inside the drawing, having to build a new Assembly and then make a Drawing of it.

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.