how to edit Arc length in drafting enviorment 2

[Gokulkrishna]

Hi,

In drafting enviornment, once a line is drawn and dimensioned its length can be changed by double clicking and then entering the required length. But the same is not happening while drawing a arc.

THanx

 

[Toost]

1) What version of NX are we talking about ?
2) Do you want to set the length of the arc ???
- In NX8.5, use the command Finder under Help, then search for "Curve Length". Then RMB for options if this is something you do frequently.

Regards,
Tomas

 

[JohnRBaker]

I assume that you're creating these curves on your Drawing as Sketch curves, correct? And that you're then adding dimensions, correct?

Well the dimensions, since this is a 'sketch', are driving dimensions (AKA dimensional constraints), at least the linear and radial ones are. However, the 'Arc Length' dimension is NOT driving-dimension and therefore it's not a constraint (at least not at the moment). However, you can assign a 'Parimeter Dimension' which, while it will NOT actually create a 'dimension' on your Drawing, it will create an expression which you can then edit to change the 'arc length' of the arc. And if you had added an 'Arc Length' non-driving dimension to your drawing, it will update to read the same as the edited value of the 'Perimeter Length' of the arc.

Anyway, give that a shot and see if this will meeting your requirements.

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

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

 

[Gokulkrishna]

Hi,

I'm using NX8.5 and both the ways are working fine.

John : After using the perimeter dimension, when I go to tools the expressions option is greyed out. So I had to right click on the curve and select Remove all Constrains. Is this the correct way?

Thank you!!

 

[JohnRBaker]

In order for the Expression editor to be accessible while in Drafting, you need to go to...

Customer Defaults -> Drafting -> Drawing -> General

...and toggle ON the last item on the page, 'Allow Expressions'. Now hit OK and restart NX and you'll now be able to use the workflow I described.

And NO, that NOT how it's supposed to work (removing constraints).

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

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