You are correct, the options previously commented on, both the Preferences -> Modeling and Customer Default settings are ONLY intended to control the behavior when the Extrude/Revolve/Etc feature is referenceing an EXISTING Sketch. When creating a Sketch
in the context of the modeling feature itself, it is ALWAYS assumed that the Sketch is to be considered PART of the feature and therefore is automatically 'Managed' (this is the term we use internally, meaning hidden yet still available when needed).
Now you may ask WHY do we NOT allow these settings to control ALL Sketch/Feature behavior and the primary reason is that many newer aspects of NX depend very heavily on creating Sketches as part of creating the Feature and that if these sketches were always left visible, the models would soon become so cluttered that it would be very difficult to work with them. The two best examples of this would be when defining the location of Holes and when creating Sheet Metal features.
Note that when we first introduced the concept of automatically 'Managing' the imbedded Sketches this was only supported for Sketches created as part of the Feature since we were trying to duplicate the behavior that virtually every other CAD system which depended on creating profiles as part of a feature behaved. At first, our users fell into two camps, legacy UG users, where the Sketch and the Feature were always two separate items, and the newer users, most of whom were transferring over from these other systems where 'profiles' were considered part of the feature with no questions asked. Over time, many of the 'legacy' users came to appreciate this auto-imbed feature and so we were requested to make the old 'Sketch-first then Feature' behave the same as if the Sketch/Feature were done in a single step. But like most everything that effects legacy behavior we made THAT part of it optional, but felt NO need to change the imbedded Sketch/Feature behavior because in all honesty, no ones really complained about it (and it's been since about NX 2.0 or NX 3.0 that this could have even been seen as an issue). Besides, as I mentioned previously, as we continued to develop new functions where the PREFERRED behavior was to create the Sketch as part of the Feature it was just automatically assumed that these Sketches would ALWAYS be 'managed' yet keeping in mind that users could still opt-out, on a case-by-case basis, by making them 'external' if they really needed to reuse the sketch for some other operation, which BTW, will automatically make the NOW 'external' sketch UNAVAILABLE in the future to be re-imbedded once more. ONLY Sketches which are used to define a SINGLE feature, without any other references being made to it, are able to be imbedded irrespective of whether they were first created as a stand-alone Sketch or as an imbedded Sketch which was later made 'external'.
Anyway, I hope that explains why you're seeing the behavior that you are.
John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
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