Prior to NX 9.0 the default (out-of-the-box) Modeling tolerances were set to:
Distance = 0.0254(mm)/0.0010(inches)
Angle = 0.5000(degrees)
Starting with NX 9.0 the defaults are now set to:
Distance = 0.0100(mm)/0.0004(inches)
Angle = 0.5000(degrees)
As for the 'basis' for these values and the rational for the recent change, when Unigraphics, the precursor to NX, was in its early development stages one of the primary industries that UG was being sold into was Aerospace. After all, from the late 70's until 1991, Unigraphics was developed and sold by McDonnell Douglas Corp, a large aerospace company. At the time we chose to use those first set of values above as they were felt to be appropriate for the majority of our customers.
However, over time our market focus changed as we sold more and more software to automative companies and after some of our more recent successes in the automotive sector, it was decided that we should change our defaults to those that are generally used in the automotive sector, thus the second set of values above. These changes were made with the realization that as we moved from an older aerospace oriented mind-set to an automotive one, that the scale or size of the models being created were becoming smaller and therefore it was appropriate that we use smaller (i.e. tighter) 'Distance' tolerances. After consulting several of our automotive customers we determined that there was a defacto standard being used and those are the values we chose to start using with the release of NX 9.0.
That being said, we've always recommended that our customers look at their specific situations and to choose Modeling tolerances which were appropriate for the type and size of models that they were creating. For example, if you were designing and manufacturing watches or precision instruments then a smaller or tigher tolerance may be best for you, while if you were designing and manufacturing ships I would think that one could get by with a larger or looser tolerance. Keep in mind that the smaller (tighter) the tolerance, the larger and more complex will be the many of the modeling objects created, particularly any that are effected by the modeling tolerance such as any sort of freeform surfaces and curves as well as complex blends and any kind of intersection/projection sort of operation. This can have an impact on the part file size as well as the performance of NX including Model updates and some display/graphics operations.
As for the default feature parameters, those were strictly arbitrary. Years ago the defaults were always set to '1', whether it was Metric or Imperial units, which were totally inappropriate particularly in the case of Metric files. So about 20 years ago we decided to change the defaults to something a bit more reasonable and to set the Metric versus Imperial defaults to something which resulted in approximately the same physical size results. We just thought that 100(mm)/4(inches) was about right for the basic default parameter.
I hope this helps to answer your questions and that you keep in mind that the values of ALL of these defaults, Tolerances and Feature Parameters, are under your total control via Customer Defaults.
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.
