Diameter Symbol 1

[Bishbosh]

NX 5.0.2.2

We use Part Attributes (thro File - Properties) to populate the Drawing with text; Drawing Title, Material etc.
How can I add the Diameter Symbol in the Value of an Attribute. The text is Blockfont, but the $r input will not work.

Andy

 

[MCGNX]

I thought Diameter was <o>

 

[JohnRBaker]

Yes, this appears to be a limitation in the Attribute to Drafting Text routine.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[JohnRBaker]

As a workaround, you could create your attribute without the $r text and instead add that in the Annotation editor after adding the link to the attribute. In the Annotation Editor it would look like this:

<W@ATTRIBUTE>$r

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.

 

[man2007]

Suppose you have "DIA" attribute, enter its value as <o>25 for example, in File Properties
In drafting use <W&@DIA> so that you will get Diameter symbol.

 

[JohnRBaker]

OK, that works. If you include the ampersand (&) as in...

<W&@ATTRIBUTE>

...then it works, even using the '$r' special character set.

Even I learn something new once in awhile ;-)

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
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.