Where is the "Edit defining string" ?

[stephlouv]

Hi there,

I jumped from NX2.0 to NX8.0
There was a usefull tools in NX2 called "Edit defining string".
Imagine a sketch with multiple loops which allow me to draw several/optional designs.
I've been using it to edit the strings used by child extrusion/revolved even before exiting the sketch edition.
Doing so i didn't get any error message telling "self intersection" or so on.
And my solid was OK while exiting the skecth tool.

Is there a such tool in NX8.0 ?
Because the "selection intend" is stupid to me.
Even if I set it to "single curve", shift-clic a curve to remove it from the extrusion profil (firstly defined using "feature curves / connected"), it is removing all the curves. :-(
I then must relect my curves one by one ... with the "single curve" filter :-(

Thank you

 

[carlharr]

I've always wondered about curve rule de-selections.

When using single curve to shift > deselect, the entire selection is removed not just a single curve.

Is this because making a de-selection is actually "breaking" the original selection intent?

http://www.jcb.com

NX 7.5 with TC 8.3

 

[stephlouv]

OK, i see it is now called "edit defining section"
But it is very well hidden !
I don't find it anywhere, even the "command finder" can't show it for me !?

 

[carlharr]

Hi Stephlouv, just tested this (and answered my own thought).

If you've selected originally with e.g. feature curves, and picked a sketch, then the selection intent is always all of that sketch. So deselecting one curve breaks that intent.

If you used connected curves for example, then removing one discrete curve e.g. a circle does not break the original intent.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[mmauldin]

Go to you customer defaults and make sure "Deselect All Intent" is unchecked. You may have to restart NX for it to be effective.

See attached:

 

[cowski]

Right click your extrude feature and select "Edit parameters", in the "Section" portion of the extrude dialog, you will be able to select/deselect curves as needed. If you are creating an external sketch to be used as the section, I'd suggest using the selection intent of "feature curves"; this will take all the curves in the sketch. If you later edit the sketch to add and/or remove curves, the selection will automatically be updated to match. As for deselecting single curves from a previous selection, it is possible to deselect individual curves without deselecting everything; see the discussion in this thread:
thread561-349980

www.nxjournaling.com

 

[stephlouv]

OK. I was able to deselect only one curve.
But at the revolved editing, not before exiting my sketch.
You have to fly over the concerned curve (curve rule set on "single curve") and wait for the selection choices.
It will propose the "curve" or the "all of intent"
Hum :-/ time consuming as i knew in advance that my revolve won't update correctly (multiple path possible).
But still better than reselecting the whole profile.

 

[carlharr]

mmaudlin,

Thank you for the info, it's confirmed what I thought.

I can now select feature curves, deselect a single curve, then add a new curve and feature curves (minus the deselected one) is maintained.

That said, it's all too confusing for me now, I'm going back to the old way!

http://www.jcb.com

NX 7.5 with TC 8.3

 

[jerry1423]

You will have issues finding the commands after making such a big jump, be sure to utilize:
Help -> Command Finder
Or make sure it is shown on your Standard toolbar, it is the binoculars icon.

 

[stephlouv]

I found it !

The "Edit defining section" tool is only available in the pure sketch task environment.
So, by initiating a sketch from the revolve or extrude feature.

If you're defining your sketch using the direct sketch toolbar it won't be available until you clic on "Open in The Sketch task environment"

Stephane