Actually if your typical models are small, say less than 2 meters (78 inches) in size, I would change your overall default modeling tolerance to the new 'standard', that is 0.0100 mm (0.0004 inches).
BTW, the reason for our recent change in the default modeling Distance tolerance is because over the years, the size of tha typical piece part modeled by our customers using NX has become smaller. When Unigraphics was first developed back in the mid- to late-70's, many of our customers were in the aerospace sector (after all, for years Unigraphics was developed and sold by McDonnell Douglas). However, over the last 20 years or so, our 'sweet spot' in the industry has moved toward automotive, where the typical piece part size is much smaller. Therefore, starting with NX 10.0 we've switched our default Distance tolerance to the standard that was adopted by the majority of the automotive OEM's and their suppliers, that is 0.0100 mm (0.0004 inches). But as always, these default tolerances can be changed and they should be reviewed when purchasing CAD and selecting something appropriate for your particular product line.
As for your question about is it OK to set the tolerance for a single operation, the answer is YES. After all, why do you think we include an option to set the tolerance inside of specific modeling functions. But note that changing the tolerance values while in a feature dialog will ONLY effect the tolerance used for that particular operation and will have no impact on the default (AKA pre-set) modeling tolerance that was saved with the part file. However, changing the tolerance in Preferences -> Modeling and saving the part will change it for any subsequent modeling operations but it will have no impact on features already created. Also note that not all modeling operations are affected by the tolerance settings. Generally speaking, those features or operations where tolerance is a factor, those are the ones where you'll find a tolerance option in the settings section of the dialog. Also note that for most of these features, the tolerance itself will be become part of the parametric values of that particular feature, often even showing-up as its own expression. And before you ask, there is no way, at least not as part of an interactive operation, to change the tolerance of all of the features of a model. Please note that while there are some CAD systems which does allow you to do that, Pro-E comes to mind, it is generally NOT something that you should be doing as it can be problematic and so we decided years ago to not provide a way to do that. If you feel that you need to tighten or loosen the tolerance on your models, for whatever reason, it should be done on a feature by feature basis so as to know exactly how this will impact the results and the reliability of updating.
Anyway, I thought that you should know how all this works and why.
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.