NX7.5 with Section View Preference in customer defaults not working?

[lorenolepi]

I got a PR (6477958) in with GTAC but I was wondering if anyone else was having an issue with the section line preference and if there was a work around. In our site customer defaults we have the prefrence under Drafting --> Section line -- Create section line set to "With Section View" and its locked but everytime we go to make a drawing it goes to "Without Section View" and we have to manually reset it = LAME... why would we take a section if we didn't want the view...lol. Any ways GTAC states that its only conrolled through the customer defaults but this is not the case.. if anyone knows another setting that controls this please let me know.

 

[cowski]

Are you starting your drawings from a template file? If so, you will need to open the template and edit the setting there. Future files created from the template will reflect the new setting. Customer defaults will control the settings of a completely new file (a 'blank' file in the new file dialog); a template file is simply a file that has already been created and saved with the settings you want.

 

[MickyV007]

Are you working master/model approach? If not also not so important, same approach.
Open the file, goto file-properties in the attributes tab look for DB_SEED_PART_USED there is a specific name like metric or my-factory-drawing-seed-part or... you get the picture.
Then file open ... fill in the name of the seed part, goto drafting-preferences - section line preferences and change it under settings to With Section view.
SAVE the seed part and for all the new drawings created it should be ok. The seed part is overruling cust def in some cases.

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3

 

[lorenolepi]

Thanks for the input... but I have tried that as well. We are using template parts and that setting was in place at the time of creation... we have tried re-saving all templates with the preference set again and still no luck.

 

[daluigi]

They're actually carrying that issue since NX. Even the templates settings seems to be overwrtten by god knows what while opened.
And that mis-communication between templates and customer defaults input is unfortunatelly not an isolated problem.
Still a long way to go but we're patient guys, isn't it?

 

[JohnRBaker]

I'm running NX 7.5.4.4 (which was released for customer download a week or so ago) and was not able to reproduce your problem. May I suggest that you download this MR and then test this again.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.com/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[lorenolepi]

Thanks but we are running NX 7.5.4.4
I think I semi-figured out what is going on...so all of our templates parts for the File-->New are useing patterns. The second that the pattern gets exploded the setting changes to "With Section View"... Heres the strange part I went into the pattern files figuring I could change the setting there = can't be done. The preference is not available within the pattern files = grayed out. I really want to use the pattens because are template files are similar and if we change that one pattern it will change the background of all of the parts (boarders, logo's etc).
Any clues?

 

[JohnRBaker]

Just one more reason why I've never used 'patterns' for drawing borders ;-) which is probably why I had no problems with this.

BTW, in the next version of NX we will be including a set of tools which will allow you to create your own drawing borders, with smart title blocks, and then convert them into Drawing Templates all using an interactive workflow in Drafting. This new method does not depend on Patterns.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.com/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[lorenolepi]

I realized that the pattern files were all done in modeling mode and didn't contain a drafting sheet and thats why I couldn't change the setting... I tried changing and it still reverts back.
Maybe we will blow away the patterns but that stinks because we have about 30 similar formats and the changing the pattern for the borders/logo's made it a hell of alot easier.. I will keep you posted as I try to work through this madness.

 

[JohnRBaker]

Patterns were developed well before UG V10.0 (1993) where we introduced a separate Modeling versus a Drafting mode.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.com/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[lorenolepi]

So John in all of your infinate wisdom what you suggest instead of patterns? We have about 30 templates with same background that we would like to change at the same time?!?

Also Just as an FYI GTAC states that this is a Windows 7 64 bit/NX 7.5 64 bit problem

 

[ewh]

If you are considering recreating the patterns, wouldn't it be easier to just export the pattern geometry into a new, clean file for each?

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[lorenolepi]

FYI:
The new maintenance pack (7.5.4.4 mp04) that was released on 10/13/11 fixed this problem. The section line preference now works as it should. For those using Teamcenter you will need to update the soa\policies files in order for NX manger to launch. (see the note 4.2 on bottom of the read me file)

 

[cubalibre000]

Hi John,
you wrote :
"BTW, in the next version of NX we will be including a set of tools which will allow you to create your own drawing borders, with smart title blocks, and then convert them into Drawing Templates all using an interactive workflow in Drafting. This new method does not depend on Patterns. "

Can you make a video of this new enhanced in NX8 ?

Thank you...

Using NX 8 and TC8.3

 

[JohnRBaker]

Read the Documentation first. If that doesn't help, try contacting either Siemens or your distributor and see if they're offering training classes in NX 8.0 Drfating.

After all, I don't really have time to create free 'training' material. That's NOT my job.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.