NX12 and boolean features 4

[TomMtz]

Friends

Actually I have the new NX12 version, the problem is with old files created with old version (NX8, NX9, NX10). When I try to apply a boolean in the model, appears the next message:
*cannot add a new feature to the tool body of a supressed Boolen feature*
I made a test deleting all boolean features and applying all of them again without success.
Someone of you can tell me why this mesSage appears?

thanks a lot for your time and comments

Tom

NX11 Windows 10 / Teamcenter 10

 

[PSI-CAD]

Hi,
I know this message. Did you have some features suppressed by expression ?
Regards
Didier

Regards
Didier Psaltopoulos

http://www.psi-cad.fr

 

[Toost]

imagine you have the following feature tree :

feature 1
feature 2
Unite 3 ( Where feature 1 is the target body. )
feature 4

If you suppress the Unite 3, you cannot add a new boolean where feature 1 is either target or tool.
I think this is a "rule" to prevent a "lockup condition", in case later the "unite 3" would be unsuppressed.
I think this was the same in previous versions.

But,
In case the feature tree would look like this :

feature 1
* feature 2 ( Boolean = unite ) Suppressed.
feature 3 ( Boolean = None)

In this case you can add a new , separate boolean as #4


Maybe the "rule" is a very old thing that nobody has thought of removing.

Regards,
Tomas

 

[NutAce]

If all above doesn't bring a solution, please try the "Renew Feature" option.
You can find it in Edit - Feature while in modeling.
It recomputes the feature with the latest version of feature code. (simply said it will bring it up to NX12)

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[TomMtz]

Friends

I checked all your commets and I finally using "Renew Feature" I could Re-design my model in NX12.
Thanks Toost but the software could not work.

Kind regards

Tom

NX12 Windows 10 / Teamcenter 10

 

[cowski]

This happens when you have a boolean feature suppressed and you are trying to modify the tool body used in the boolean. To successfully add a new feature to the tool body, use "make current feature" to roll the model back before the boolean feature where the tool body is used. You can then add new features that affect the tool body then make the last feature in the navigator the 'current' feature.

www.nxjournaling.com

 

[TomMtz]

Cowski

Thanks a lot for your tip, that was a better way to re-design features.

Regards

Tom

NX12 Windows 10 / Teamcenter 10

 

[Xwheelguy]

For those of you that double click on features to Edit, there is a Customer Default that sets the default editing behavior when double clicking on features. If you set it to Edit with Rollback, that may help out a bit. It's also a Modeling Preference for existing part files.

Tim Flater
NX Designer
NX 11.0.2.7 MP11 Rev. A
GM TcE v11.2.3.1
GM GPDL v11-A.3.5.1
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[TomMtz]

Xwheelguy

This method Works only with existing features, but if you make a new sketch then Edit With Rollback does not work.
Probably the link with other NX version has lost when the program is updated.

GTAC have a new homework to resolve for all of us.

Regards

Tom

NX12 Windows 10 / Teamcenter 10

 

[cowski]

In the customer defaults you can set the double click action for features and sketches separately. Personally, I prefer "edit with rollback" for both.

www.nxjournaling.com

 

[Xwheelguy]

@TomMtz,

I didn't mean to imply that Edit With Rollback would cure any Renew Feature ills that need to be addressed first. If the new Sketch is the last feature, there's obviously nothing to roll back. Make sure you're changing your Modeling Preferences for existing parts like I stated - Customer Defaults affect new part files only. If using templates, you'd have to edit the Modeling Preferences then save the template(s) to affect new parts using templates. Changes to Customer Defaults require a restart to take effect, of course.

Edit With Rollback and the default action settings have worked flawless for me since it's introduction and I haven't seen any seasoned users complain about it in newer versions here or on the Siemens forums, so not sure what you're saying doesn't work.

Tim Flater
NX Designer
NX 11.0.2.7 MP11 Rev. A
GM TcE v11.2.3.1
GM GPDL v11-A.3.5.1
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M

 

[cowski]

The "edit with rollback" option is a session setting (as opposed to a part specific setting) and should affect any part that you open on that computer. If you changed the setting in customer defaults, you'll need to restart NX for the change to take effect, of course.

www.nxjournaling.com

 

[Xwheelguy]

Thanks for catching that cowski.

Tim Flater
NX Designer
NX 11.0.2.7 MP11 Rev. A
GM TcE v11.2.3.1
GM GPDL v11-A.3.5.1
Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M