In the next version of NX this will be much easier but for now try this:
Open the piece part file and using the Measure Body function with 'Associative' toggled on, create a measurement feature which will automatically create an expression for the surface area. Now create your drawing (actually you can do this after the drawing is created) and while in the Master Model drawing file, open the Expression dialog and create an interpart expression to the piece part file and linked to the measurement's 'Area' expression. Now while in the Drawing you can go to the Text Editor and using the 'Relationships' function select Expressions and select the area expression and now you've got a note which reflects the value for the area of your piece part.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
thank you John,
is there a way to automize it put the measurement in a table column of my drawing template ? I tried across ug_setattributevalue fighting the problem with measurement - is mm2 in the solid part should be cm2 on the drawing(Nx7.5).Way to get it controlled?
tIa
There's no real way (without writing programs) if make 100% automatic. You could create a dummy expression in your template drawing and link the note in the table to it. Then after you create your drawing using the template, you just edit the expression by creating the interpart link.
In the next version of NX since information like weight and area will automatically be included with each component as attributes there will be no need for interpart expressions and it will much easier to set-up a drawing template where the notes are linked to attributes on the component.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
