Part Attributes in NX8.5

[OldCADPOPro]

Hello All,

I have a question about NX Part Attributes between models and Drawings. Here is what I am looking to do.

I have a part attribute in the model seed part called DESCRIPTION. I want that same attribute in the drawing file. I tried to use DB_DWG_TEMPLATE_DESCRIPTION to link the attributes between the parts. Then I created an ATTRIBUTE called DESCRIPTION and used expressions to try and link DB_DWG_TEMPLATE_DESCRIPTION to DESCRIPTION. The problem is that the expression value field is blank, which is wierd because I can use the attribute in drawing text and it puts in the text correctly. Does anyone know how I can have the same attribute in both the model and drawing file be the same value drive from the model?


Thanks for your help,


Richard Andrew

 

[JohnRBaker]

If you're using the Master Model approach, the Part Attributes in your modefile will be inherited by the Component in the Master Model Drawing. Simply reference the OBJECT Attribute assigned to the Component when you create your Drafting note.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[OldCADPOPro]

Hello John,

That works great after you added the component to the drawing. I guess that I should have mentioned that I am trying to do this in a template file for drawings. Can you set this up so it is part of a drawing template? This way I will not have to create this everytime I create a new drawing. Let me explain better what I am trying to do:

First, I have a seed part that contains some part attributes like AR_NUMBER (our part number), DESCRIPTION, REV_LTR, and a few more. I want to reference these in the drawing template, so I use the DB_DWG_TEMPATE prefix on each of these. When I setup my drawing template, I can reference the DB_DWG_TEMPLATE part attribute in a note with default text. I am trying to do some things where I link a seperate DESCRIPTION in the drawing seed part to the DB_DWG_TEMPLATE_DESCRIPTION from the model. One way I found was to add DB_DWG_TEMPLATE_DESCRIPTION as an expression and then link DESCRPTION to that expression. Again the issue here is that the DB_DWG_TEMPLATE_DESCRIPTION does not feed that string into the expression. The value for that expression shows up as "" and does not update.

So can I use your method in a drawing template without selecting a component to add the object attribute? or is there something I could be doing wrong when adding the part attribute to the expression?

Thanks,
Richard Andrew

 

[jpetach]

Hello Richard,

The drawing non-master template part that contains the attribute template with the "DB_DWG_TEMPLATE_" prefix will automatically look for the attribute in the master part when the drawing template part is use to make a new drawing or the master part. In the drawing template part containing the attribute template with the prefix, create an annotation (note) and use the attribute template.

PhoenXPLM has a very good video on the topic (attribute template use start about 08:05) [URL unfurl="true"]http://vimeo.com/100179684[/url]

Regards, Joe

 

[OldCADPOPro]

Hello Joe,

Thanks for that input. I am using the DB_DWG_TEMPLATE_ prefix for other attributes in the model file like the part number, cage code, and other attributes. The DB_DWG_TEMPLATE_ prefix works fine for adding the annotation to the drawing. The issue here is when you add that part attribute to an expression, the value field does not report the attribute text. This particular case is unique because the DESCRIPTION text is not used in a drawing note. All I want to do is create a DESCRIPTION attribute that is linked to the DESCRIPTION attribute in the model file. This is so both parts contain the same attribute values when placed in our PLM system. My tact was to add DB_DWG_TEMPLATE_DESCRIPTION as an expression, then link the DESCRIPTION attribute in the drawing to the expression. Seems simple, but the result is not working.

Thanks Again,

Richard Andrew

 

[JohnRBaker]

When you create your Drawing Temaplate file include a 'dummy' Component which contains the same Attributes that you're going to be using in your normal models and link to these Attributes when you set up your template. When the template is used your model-of-interest will replace the 'dummy' place-holder component and your references should resolve themselves.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[OldCADPOPro]

Thanks, John,

I tried this and it works. The only issue is I had to them manually remove the dummy component. It is too bad because I feel that the mechanism is there to do this with attributes and expressions. The only problem is the DB_DWG_TEMPLATE_ does not report a value to the expression or even update the expression later. only 95% there. LOL.

Richard Andrew