Feature Tolerance

[NXConsultants]

Fellow NXers,

Is there any best practice advice against me adjusting the feature tolerance (when available) during a session?

For instance: In Trimmed Sheet under settings I can adjust the tolerance, the general modelling distance tolerance is set to 0.01mm at present, this is causing difficulties with trimming foreign (non NX) surfaces. Loosening this slightly to 0.0254mm

I have been using UG/NX for 15 years; I know that it's not the best idea to start adjusting the modelling tolerance whilst modelling, is the same true of the tolerances relating to individual features? I've happily adjusted these over the years with no problems. I’m always diligent with checking surface consistency and fix problems as I find them, am I storing up issues for downstream users of my data – CAM etc?

Thanks, NXConsultants

 

[JohnRBaker]

Adjusting the explicit tolerance associated with a specific feature (the one found on the feature creation dialog) will only effect the creation of that feature and none others. And while under most conditions we generally expect that there should be no need to make any changes, we DID provide you that option for a reason, because sometimes you just need to to make it work. So in this case, feel free, but don't go any larger than you really need to (note that in most cases this tolerance will be saved with the feature and it can be edited later if needed).

Now that being said, whenever you encounter problems with something like a sewing and increasing the tolerance seems to help, it's generally an indication that the original surfaces were created using either very poor techniques or using imprecise data. Now generally speaking, if the sew is successful, even with the larger tolerance, most all downstream applications, such as NC operations, will work fine, but you must understand that the original surfaces have NOT been changed and are still just as inaccurate as they ever were, but as far as NX is concerned, we will try to pretend that the data is OK and we usually get away with that in virtually most places.

So our advice is, do what it takes to get the job done, but if you're going to deal with the people who provided you the original data again in the future it might be in your best interest to let them know about the problems you had and that they may need to reevaluation their procedures and workflows and perhaps even the tools which they are currently using (you could always give their names to you local Siemens PLM rep).

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
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.

 

[hudson888]

Well these days CAM will tessellate your geometry using something akin to a Faceted model for many operations so what you really need to target is the ability for that process to work faultlessly. Some people chase what they call A-Class surface which has to do with smoothness and continuity that is a different question but be aware you're not talking at cross purposes about the subject of tolerances.

In general what you really want to do is to run the examine geometry checks and make certain that your model passes the ones in the middle. That's the "Body Checks" and the "Face Checks". The few at the top under "Object Checks" may warn you of things that you want to take care of and some people with good reason try very hard to avoid tiny objects. Near the bottom tolerances are good if you can achieve them and smoothness if edges depends a lot on the design.

The exception is clearly sheet boundaries, but most people figure out the obvious implications where an external boundary is inherently okay and a hole in the middle may not be.

When running examine geometry on a finished model I usually run all the checks but from time to time I check just one to find a specific problem using the information window and the "highlight results" function to identify the cause.

Now the system modelling tolerances are fine for most purposes. Working with surfaces I may slightly tighten them up. In metric I'll target distance 0.02 and angle 0.5, or in inches 0.001 for distance. However to achieve these I'll go into the general modelling settings and halve the values (distance 0.01 and angle 0.25, or in inches 0.0005).

Using values any smaller or tighter than that can be excessive and just tightening your tolerances doesn't necessarily make your model better. In fact if you force tangency (G1 continuity or better) in surfacing then you can make your surface unduly complex and induce the kind of rapid curvature analogous to a very small radius that your ball nosed cutter can't reach. If you're surfacing for machining learn to use the curvature analysis settings to look at minimum radius values.

If you're surfacing and sewing at all then check the edge conditions as you go. This is one of the main areas where halving your working tolerance will help target better results.

If on a feature by feature basis you need to open up the modelling tolerances in order to make something work (usually getting blends to work), then simply run examine geometry afterwards. Often times nothing bad happens.


Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[NXConsultants]

John & Hudson, thanks for the valuable input guys.

Two of the gurus in this forum have instilled the confidence I needed to argue my corner with confidence – other colleagues have insisted that you never change the tolerance during modelling, that never made sense to me, if the option is available it must be there to be used.

I've been surfacing for years - In my current role (F1) and the last (Moto GP bikes) my colleagues have done their best to stop me pulling all the little stunts NX allows, I'll carry on with confidence now.

Thanks again.