NX8.5 sketch selection scope

[carlharr]

Does anyone know if there is a way to change the NX8.5 default sketch selection scope to "within work part"?

It seems that the default is set to "active sketch only" (which is useless) for each new session.
Changing scope to "work part" will affect all future sketches in a session, but as soon as you close and restart NX8.5 it resets to "active sketch".

I've just got round to testing this, and it looks like the behaviour was the same in NX7.5 (no dialogue memory between sessions), BUT the 7.5 default was "work part" so no one would have noticed. "active sketch" is an annoying noticable difference that our testers have picked up on.

I've recorded an NX8.5 video to explain what I mean (attached)
- create a sketch, and change the scope
- create a second sketch, change is remembered
- close and re-start NX, the scope has been re-set

(note the other NX session in the background is NX7.5, not another 8.5 - I should have minimised it).

So, any way to change the default to "work part"?

http://www.jcb.com

NX 8.5 with TC 8.3

 

[NutAce]

Don't think it is possible.
This is done intentionally by Siemens to make the user aware they will be selecting references outside of the sketch.

Ronald van den Broek
Mechanical Engineer
Cad Environment Coordinator
Wärtsilä, Propulsion Services
NX8.5.3 / TC9.1.2
HPZ420 Intel(R) Xeon(R) CPU E5-1620 0 @ 3.60GHz, 32 Gb Win7 64B
Nvidea Quadro4000 2048MB DDR5
HP EliteBook 8570W Intel(R) Core(TM) I7-3740QM CPU @ 2.70GHz, 16Gb Win7 64B

 

[carlharr]

Wow, really?

That doesn't make any sense, if someone doesn't know what they're picking they're not likely to understand selection scope either.

Why irritate ALL existing users (and competent brand new users), for every new session of NX, just for that.

Wonder if they'd change by ER before I get earache when we go live. Hmmmm

http://www.jcb.com

NX 8.5 with TC 8.3

 

[MickyV007]

Try changing it in your template part...

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit

 

[MickyV007]

... don't forget to save it of course.

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit

 

[carlharr]

I will ask someone if this change can be made when he's back next week.

Just wondering though, how do we set this is it a customer default?

http://www.jcb.com

NX 8.5 with TC 8.3

 

[JOHNLAYKE]

I find this as a real pain as well. Especially when adding dimensions. We're jumping between 7.5 & 8.5 due to customers preference & it's really annoying having to remember to switch this every time. I don't see the logic behind doing this other than to slow progress & waste time. This is almost as painful as adding geometric constraints & having to remember to pick the type of constraint BEFORE you pick your sketch objects.

 

[JohnRBaker]

Trust me, we did NOT make this change so as "to slow progress & waste time." It was done at the request of our customers so as to help them limit the selection of objects to ONLY those aspects of the model that they were interested in.

As for "...adding geometric constraints & having to remember to pick the type of constraint BEFORE you pick your sketch objects", why are you doing that in the first place? If you're working in NX 8.5 all that you have to do is select the sketch curves that you wish to constrain and you'll get a Shortcut Toolbar showing you ONLY the constraints that CAN be applied to the selected set of curves.

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.

 

[carlharr]

Re constraints, the new dialogue in 8.5 is actually a lot quicker and easier than the old 7.5 method once you get used to it, mainly because it controls the selections once you've selected constraint type, so e.g. you can't accidentally select an endpoint if you've chosen tangent constraint.

But it would be difficult switching between the two that's for sure.

Selection scope: I've been told that the default goes back to "within work part only" in later versions, I don't know if that's true but I hope it is. It is a nuisance having to change it every time you try and fail to pick something outside the sketch.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[JohnRBaker]

Yes, starting in NX 9.0, the default when entering the sketch mode is to set the selection scope, once you decide which type of the curve is being added, to 'Within Work Part Only'. However, for the duration of the current session, Dialog Memory will retain the last option that you chose for the Selection Scope on basically a function-by-function basis. For example, if while adding a Line to the sketch you changed the Selection Scope to 'Within Active Sketch Only', then if you selected a Circle next it would remain set to 'Within Active Sketch Only' but most of the other functions would still us 'Within Work Part Only' unless you change them as well. Of course there are an entire class of functions which ONLY work in the context of the Actice sketch, such as Quick Trim, Quick Extend, Fillet, Chamfer, etc, and therefore no other option is even offered. But if after making a Quick Trim or one of these other limited scope operations you were to go back to adding Lines and Arcs and you had last used 'Within Work Part Only' scope it would be reset back to that automatically.

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.

 

[SDETERS]

I am finding this to be very troublsome. We just switched to NX8.5 I make a sketch I go to dimension the sketch curves back to the Csys and I have to switch this scope. I did not have to do this in NX7.5. How would one go about fixing this in your template model? What is the true fix for this. Or do I need to wait for us to go to NX 9.0 to get the behavior like we used to have in NX7.5? Thanks