NX6 - EXPRESSION MANAGEMENT IN DRAFTING 1

[CAD2015]

Hi,
Most of the time, the "EXPRESSION" in Drafting environment turn to pasive(neutral); I can not modify the dimensions in the views in which I used FEATURE PARAMETERS for adding sketch dimension.
Is there any way to correct that?

Thanks

 

[JohnRBaker]

In order for the Expression dialog being available while working in a Drawing you need to set the following environment variable:

UGII_DRAFT_EXPRESSIONS_OK=1

Note that starting with NX 7.5, this is now controlled by an option set in Customer Defaults at...

Customer Defaults -> Drafting -> General -> Drawing

...and at the bottom of the page you will find the 'Allow Expressions' option that when toggled ON, the Expression dialog will be active while working in the context of a Drawing.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[CAD2015]

Thanks, John, but how to get to "UGII_DRAFT_EXPRESSIONS"? I am not so good in IT stuff.......

 

[JohnRBaker]

Go to the UGII folder where NX is installed and open the file named 'ugii_env.dat'. Search for the string 'expressions' and your first hit should be this variable. Just set it equal to 1 and un-comment the item (remove the '#' sign), save the file and restart NX.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[Toost]

Does this work in "the master model concept" or is it "all types of objects ( Drawing + model) in one file" ?

Regards,
Tomas

 

[JohnRBaker]

If the need is to access expression values found in the master model part (the piece part) file, while in the Master Model Drawing, what you do is when creating your note(s) and you select the 'Insert Expression' option in the Note editor when the Expression dialog comes up, there will be a large button in the middle of the dialog labeled 'Link to Part'. When you select that it will give you a list of all the component parts accessible from within your Master Model Drawing. Select the desired part and you will get a list of the all of the expressions available in that part. Now just select the expression needed and hit OK and a link to that expression will now be inserted into the note that you were creating/editing in the Master Model Drawing.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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