How to edit Sketch 1

[BABUGOUDA]

Hello,
It is since long back i worked on Sketches in NX. I feel funny as Now i am unable to recall how to edit the existing sketch...
I have following questions
1. I have created the sketch in Sketch environment and then Finish sketch... Now when i need to edit that sketch i am not able to do...#

2. I have used the Intersect curve option in sketch but i dont want to keep the associate with the body from which i made the intersect ...so how to remove the associativity??

I am using NX8

Thx
BGD

 

[BABUGOUDA]

I am in Modeling
Ctrl+M




BGD

 

[JohnRBaker]

It sounds like you're creating your Sketches in the so-called 'Sketch Task Environment' but when you go to edit the sketch you're ending-up in the 'Direct Sketch' mode. Note that you can still edit your sketch in that mode, but if you would really prefer to always work in the 'Task Environment', which BTW was probably the ONLY option back when you learned to use the NX Sketcher in the first place, just go to...

Preferences -> Modeling -> Edit

...and just set the 'Edit Sketch Action' option to 'Task Environment' and hit OK. Now when you edit the Sketch you will be doing so in the 'Task Environment' which is the same as when you created your sketch.

With that in mind, if you want to create Sketches on the face of a Drawing, the ONLY option will be the 'Direct Sketch' mode. When in Drafting the concept of a special 'Task Environment' when creating a sketch is not practical nor even desirable so only the 'Direct Sketch' method will be available. Note that the 'Direct Sketch' method was first developed for use when working on the face of a Drawing and it was only later that it was made an optional mode while working in Modeling.

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]

Additional to Johns info, RMB > edit with rollback will always send you into the full Task Environment, with a model rollback.

I find Direct Sketch edit ok for quickly changing values in a sketch, but for anything more complex I prefer task environment.

So I stick with the "default" preferences - Edit = Direct Edit, and double-click action = Edit (the item in "bold" in the RMB menu).

If you do click edit you will see that the sketch is active (blue checked pattern) in the part navigator - this means direct edit using the direct sketch toolbar. There's a button on there to send you into task environment aswell.

http://www.jcb.com

NX 7.5 with TC 8.3

 

[JohnRBaker]

As for your second question, it appears that there is no way to do that. You will need to delete the original intersection curve and replace it with a normal Sketch curve. And depending on how you selected the Sketch and/or it's curves when you created any downstream features using this sketch, you may or may not have to reselect the new curve to include it in the profile.

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.

 

[JohnRBaker]

Actually I've set up my system as suggested by carlharr, this way I have control over whether I edit using the 'Task Environment' or the 'Direct Sketch' method by how I choose to edit the sketch. And while it is true that you can use the 'Direct Sketch' mode to sort of gain access to the Sketch dimensions without having to do a Rollback, you can now do that by simply eiting the feature created using the sketch as the driving dimensions will now be automatically displayed and selectable for editing without having to enter either of the Sketch edit modes.

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.

 

[BABUGOUDA]

Hello,
Thanks all ..
John:While designing in Sketch i need to take some sections from other body as a reference to design my model.so once my work done i dont want my intersection curve in sketch to have link with reference body.( Like catia V5).

I worked earlier in mostly plastic automotive interiors with NX. but never used sketch .but now i feel it is good if we use sketch also as and when required to create some complex sections..
or remove the link...

Thx
BGD

 

[cowski]

Outside of the sketcher you can create non-associative intersection curves then add them to the sketch as desired. If/when the components change, you will need to update the curves.

www.nxjournaling.com