manual dimensions 1

[sasha1]

In NX5 is there any way of overiding the dimensioning to enter size manually?
Many thanks

 

[doc1955]

I don't know if this is the only way but what I do is double click some othe text on the drawing then with the editor open click the dim you wish to override.




Doc

http://www.goodrich.com

 

[MCGNX]

you can go to Edit - Annotation - Text and this will override the dimension. Beware though, once you override it the dim loses associativity permanently

 

[hudson888]

An old drafting convention was to underline manual dimensions, which NX can support. The other way to detect them, was Information>Other>Object-Specific>Dimensions with manual text, it will temporarily highlight the affected dimensions only, but it is not a selection method. It is probably worth passing on ways to ensure that you manage the use of manual dimensions since the overwhelming preference is to try and avoid them where possible.

Best Regards

Hudson

 

[doc1955]

We identify manual dimensions with the () such as (2.450).
That way you can see the manual dimensions at a glance.

Doc

http://www.goodrich.com

 

[JohnRBaker]

Back in my drawing board days (spend 11 years with my nose to the paper) we placed a 'squiggly line' under dimensions that were not-to-scale.

While it's not an automatic function (in that it won't detect which are or which aren't out-of-scale) there is a dimension type in NX to indicate out-of-scale, which is to place a simple line under the dimension (can be edited under 'Style').

Note that dimensions inside of parentheses are generally considered as indicating that they are for 'reference' purposes only.

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/

 

[doc1955]

"Back in my drawing board days (spend 11 years with my nose to the paper) we placed a 'squiggly line' under dimensions that were not-to-scale."

Hey! I remember those days! Pencil in one hand and the power eraser in the other. I do remember the squiggly line.

We try not making a habit of manual dimensions only when absolutely necessary.


Doc

http://www.goodrich.com

 

[hudson888]

Yes John and Doc,

your old school drafting practices agree with what I was taught also. We used the straight line which NX supports, and the brackets for reference.

"Never draw in the morning more that you can rub out in the afternoon." Old drafters adage .

Best Regards

Hudson

 

[ewh]

This is slightly off topic, but isn't there a command in place (NX5) to reassociate manual dimensions to be true? Or is it something in an upcoming version? I know that I read about it, but since we avoid manual dimensions, I haven't had a reason to look into it further.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

Yes, starting in NX 5, just double-click the 'manual' dimension and when the Edit dialog comes up, place the cursor over the now highlighted dimension, press MB3 and at the bottom of the pop-up menu, select 'Convert to Automatic', and the dimension will once again be fully associative showing the proper dimensional value.


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/