Automatically make feature sketches external

[snydeja]

Hello,

I often prefer to have my sketches external and I know I can make my sketches external by clicking on them and making them that way. I know I can also create a sketch, then create the feature after the fact and have an external sketch. My question is if I can create an extrude and have the sketch automatically be external instead of going in after the feature is created and making it so. I looked around in customer defaults but was not able to find anything, maybe I am just looking in the wrong spot.

Let me know if this is possible/you know how to do so.

Thanks,
J

 

[jerry1423]

I don't think you can set the default to make the sketch external, but I could be wrong here. I certainly is a good queestion.

 

[JohnRBaker]

Actually there is an option for that. Simply go to...

Preferences -> Modeling -> General...

...and scroll to the end of the page and you'll find an option titled 'Automatically Make Sketches Internal to Child Features'. Just toggle it OFF and you should be good to go. Note that just like when you optionally make a Sketch 'External', with this option toggled OFF, if you ever wish to make certain Sketches 'Internal' all you have to do is select the feature-of-interest, press MB3 and if the Sketch used to create the feature is able to be made 'Internal' you'll see an option to do so.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[jerry1423]

Oh I see . . .
and in the customer defaults it's under
Modeling -> Miscellaneous

 

[snydeja]

John/Jerry,

I actually found this option before, selected it and closed out of NX/TC and re-opened everything and it did not appear to work. An example of what I would like to do is:

Create a new part
Click on extrude
Click on Sketch Section in the extrude menu
Pick my plane to sketch on
Sketch the curve
Finish sketch
Extrude

At the end of that (I may have missed some minor details) I would like to have my sketch external. When I choose the methods that you both suggested, it does not keep the sketches external (when following the method I mention above).

Again, I realize I can create a sketch, then extrude/revolve/etc. the sketch, generally that is not what I do though.

Thanks,
J

 

[JohnRBaker]

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
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[snydeja]

Thanks John, very detailed. I appreciate it.'

J