NX DRAFTING TEXT SYMBOL QUESTION 1

[Alfonz]

Hey everyone,

Has anyone had any luck in modifying the diameter symbol or the number value in a dimension? See my attached picture.
The two dimensions on the left are NX dimensions using the standard symbols. The ones on the left are what we get in IDEAS using a .65 text width ratio.

In NX I can adjust the width ratio for the text, but not the "X" symbol or the diameter symbol. The spacing for the diameter symbol is off as well but I can't see any way to change it.

Anyone got any thoughts on this?

Thanks.

Al

Design Drafter
Alliant Techsystems

 

[Arkance/PhoeNX]

Change the diameter symbol to 'User defined' see image, you can then enter <Y0.75><O><Y> to create the symbol.

The <Y0.75> is to set the aspect ratio, <O> is the dia symbol, <Y> is to turn off the aspect ratio.
See image below for example

If you add the 2X in there, you can get the following.

Otherwise if you add the 2X as appended text, you can change the aspect ratio for appended text in the style dialog.

Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[Arkance/PhoeNX]

FEI, (For Everyone's Information) attached is a snip from the docs about the control codes to format text.


Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[JohnRBaker]

What version of NX are you using?

Note that when I edit the 'Aspect Ratio' of a 'Diametral' dimension's text, it changes the diameter symbol as well as the numbers. As for your example where you've added some appended text, the '2X', you have to edit appended text separate from the dimension text. As for the space between the Diameter symbol and the text, if you use the 'User Defined' symbol you can add extra spaces to get the same effect.

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

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

 

[JohnRBaker]

You know what, I'll bet that no matter what version of NX that you're running, that you're still using the 'old' UG fonts. I you switch over to say Arial, a TrueType font, that life will be better for you.

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

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

 

[Toost]

- I was to be really-really picky, which i'm not,
A diameter sign should by definition be circular and not elliptical because its definition is to denote "circularity"....
In other words it might be better to shrink the symbol rather than squeeze. similar to :
<C0.7><O><C>

and , btw, if you want to continue using traditional UG fonts, try the "Latin_Extended" and skip whatever "Ideas fonts".
( unless you already have.) The "Ideas fonts" does not work that well in NX.

Regards,
Tomas

 

[Alfonz]

Thanks guys, this is exactly what I was looking for! And yes John, what you see in the picture is the IDEAS simplex font. I will look at other fonts.
Anthony thanks for the cheat sheet!

Design Drafter
Alliant Techsystems

 

[Alfonz]

Anthony,

I feel really stupid, but I can't get to the same annotation style screen you have. I'm in NX9 what version are you in?

Thanks

Design Drafter
Alliant Techsystems

 

[Toost]

Anthony's dialogs are Pre-NX9.
The one in my post is NX9


Regards,
Tomas