Bidirectional Associativity 3

[ben2012]

Hello,

Does anyone know how to break the link between the 3D model and view Drafting (Bidirectional Associativity)?. I'd be very helpful.
I'm using NX8.
Thanks for any help.

Regards,

Ben

 

[PSI-CAD]

Hi,

My laptop with NX is not available at this moment, but I know that is possible to do this:

1°) you need to set a variable on file utilities customer default drafting
==> find the option to set the view non associative

2°) stop and start NX
Open your drafting
Right click on a view then choose style
==> you sould be able to set the view non associative

I hope this help


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[JohnRBaker]

There's actually a couple of Customer Default options which need to be disabled. Go to...

Customer Defaults -> Drafting -> Drawing -> Workflow

...at the bottom of the page, toggle OFF the 'Allow PMI Bidirectional Edits', and on that dialog, select the 'General' tab and then at the bottom of that page, toggle OFF the 'Allow Expressions' options.

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.

 

[ben2012]

Thanks to both of you for trying to help me, but still I am not able to solve my problem.

I made the changes indicated by Mr. Baker, then I restarted NX, I imported 3D model, I went in Drafting, I put the views, and then I do not know what to do to break contact with one 3D model views.

Then I tried to follow the advice of Mr. Psaltopoulos with right click on the view, then choose Style, but I fail to find something that would allow to set the view non associative.

Please, detail your answer if you can.

Thanks a lot.
Regards,
Ben

 

[kapmnit123]

Hi Ben,
I presume you want to have a non-associative view in the drafting.Unluckily i don't have any single shot answer for that but there is a work around if you need.
First of all in the customer defaults/Drafting/General/Miscellaneous/.... turn on the ALLOW NON-ASSOCIATIVE VIEWS.(NX8.5 offers something called SNAPSHOT)
Then after you have imported a view in your drafting sheet ...right click the view STYLE/GENERAL and in the EXTRACTED EDGES option choose non associative.This will take a static snapshot (non-associative edges)of your drafting view .Now even if you delete your model geometry you will notice the drafting view still shows the geometry.
In case you do not wish to delete the model geometry then you need to push the NON-ASSOCIATIVE EXTRACTED EDGES in some other layer and using VISBLE IN VIEW option hide the original model geometry and retain the one containing the NON-ASSOCIATIVE EXTRACTED EDGES.
I hope this will help you a bit.
Best Regards
Kapil Sharma

 

[PSI-CAD]

Hi Ben,

Kapil explain explained exactly what it was in my mind in my first answer (because I had no access to my laptop)

I came back to my office today to check the difference between NX8 and NX8.5

I didn't see that they changed the way to do this in NX8.5. It's more easy because we don't have to change the customer defaults

Have a look at the 2 jpeg files

Let us know if you are happy with our answers


Regards
Didier Psaltopoulos

http://www.psi-cad.com

 

[ben2012]

Hi,

Thanks a lot guys.

Ben

 

[siva46]

but im not getting any options like u said in view style and custome default,.,, kindly look the image i attached and give a solution