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Effects of increasing the Modeling Tolerance in NX

Solution Partner Pioneer Solution Partner Pioneer
Solution Partner Pioneer

I was wondering if anyone has investigated the impact of setting the global modelling tolerance to a very small value like 0.001mm, specifically on model size and general NX performance?

 

Also does anyone have a rule of thumb for setting a sensible CAD modelling tolerance?

 

Many thanks,

 

Mark

Senior Technical Consultant
NX6-NX12
Majenta PLM
5 REPLIES 5

Re: Effects of increasing the Modeling Tolerance in NX

Siemens Phenom Siemens Phenom
Siemens Phenom

Firstly, that tolerance only affects freeform objects, not analytical geometry.

 if you manufacture watches, the internal mechanics will be very small, but most case still analytical. 

But if there are freeform details in that watch which need tight tolerances, you will need a tighter modeling tolerance.

My recommendation is to set the tolerance to 1/10 of what you need to achieve on your ( freeform) products.

 

What will happen when you play with the tolerance , is that when NX creates freeform objects, it can deviate within the given tolerance from your input geometry. NX WILL do that to try create an as simple as possible surface ( as few patches as possible) . If you tighten the tolerance, NX will, depending on the geometry,  need to add more patches to the surface to fit to the tolerance.

 

More patches means more complex data to update, larger files, longer time to open.

 

 

Regards,

 Tomas

Re: Effects of increasing the Modeling Tolerance in NX

Solution Partner Pioneer Solution Partner Pioneer
Solution Partner Pioneer
Tomas,

Thanks for your reply.
To clarify, yes this is an environment where freeform surfaces are used.
Senior Technical Consultant
NX6-NX12
Majenta PLM

Re: Effects of increasing the Modeling Tolerance in NX

Siemens Phenom Siemens Phenom
Siemens Phenom

Note that 'out-of-the-box' the default modeling tolerance in NX 10.0 was set to be smaller than in previous versions of NX.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA

Re: Effects of increasing the Modeling Tolerance in NX

Siemens Phenom Siemens Phenom
Siemens Phenom

Unless you have any specific special reasons I would recommend 0.01 mm as modeling tolerance. Going to finer will only increase the complexity of surfaces. A finer tolerance may not always mean better quality results as you wall start to see small wavy surfaces as it fights to stay within the mathematical target .More complex surface will increase file size and have some effect on update speeds and robustness.

 

Steve V

Re: Effects of increasing the Modeling Tolerance in NX

Valued Contributor
Valued Contributor

If working with freeform, try changing the tolerance for features when needed. For example, if a trim a freeform or match an edge, I may tighten the tolerance. Some operators seem to be more finicky if it is too tight or too loose. I’m comfortable at about .02 or .01 for our plastic automotive products. I may go to .005 for some features. Some have recommended .001 when translating out. See also my Complexity Study

 

 

Complexity Study parametric.JPG

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