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Expressions in Part Navigator

Valued Contributor
Valued Contributor

I have come across a file showing the expression in the Part Navigator. It only contains the ones that are changed most often.

 

I am aware of how to get to expressions (2nd pic), but I can not figure out how they are added to the Part Navigator (1st pic below).

 

expressions.pngexpressions_all.png

Glenn Balon
Production: NX 11.0.1.11 MP6 Primarily CAM
5 REPLIES

Re: Expressions in Part Navigator

Siemens Phenom Siemens Phenom
Siemens Phenom

It's not an option in the Expression editor that you can turn on and off while creating or editing an expression.  Expressions that are manually created in the Expression Editor will appear in the User Expressions folder in the Part Navigator.

 

Per the documentation:

 

The User Expressions folder in the Part Navigator shows user expressions you have defined in your model.

You must create the expressions by choosing "Tools tab > Utilities group > Expressions". The expressions that you created without using this method do not appear in this node.

 

That said, an expression I created in a command "Width=75" (while creating a block) also appeared in the folder, as did typing "len=55" for a dimension value in a Sketch.  You can also enter "p100=len*Width" (where typically a command creates "p" expressions) and it will list it in the folder, because it's a user created expression, verses one created parametrically by a command.

 

Regards, Ben

Re: Expressions in Part Navigator

Valued Contributor
Valued Contributor

As I understand it, only expression variables you define (i.e. A=10, B=20, etc) are shown the Part Navigator. Expressions created as a result of defining dimensions (i.e. p1, p2, p3,...) are not.  So if you want to vary one of the p# expressions from the Part Navigator, define an expression and assign it to that variable (i.e. A=10, p1=A).

Re: Expressions in Part Navigator


pkelecy wrote:

As I understand it, only expression variables you define (i.e. A=10, B=20, etc) are shown the Part Navigator. Expressions created as a result of defining dimensions (i.e. p1, p2, p3,...) are not.  So if you want to vary one of the p# expressions from the Part Navigator, define an expression and assign it to that variable (i.e. A=10, p1=A).


 

If you are certain about the p# expressions and features associated with it. Select the feature in the part navigator and look for the details. There you can change the p# expression values directly.

 

partnavi.PNG

 

 

Ganesh Kadole, QA Analyst (PLM), SQS
Testing: NX 10 | NX 11 | TCIN
TC 11.2 | TC Vis 11.3 | AWC 3.2

Re: Expressions in Part Navigator

Valued Contributor
Valued Contributor
Thank you everyone for the help!
Glenn Balon
Production: NX 11.0.1.11 MP6 Primarily CAM

Re: Expressions in Part Navigator

Experimenter
Experimenter

Is there a way to hide the Expressions in Part Navigator at all?

If I use Product Template Studio, I can set limits on expressions defining geometry (for example defining the list of selectable values). These expressions can still be defined in Part Navigator (or Expressions window) to values violating the limits.

Thanks!