NX9.0 section view name change problems

[TomLoughlin]

Morning all,

I'm having problems when trying to rename a section view in NX 9.0.0.19. In the part navigator/drafting, I right click the view and in properties, I change the VWLETTER, VWLETTER_DISP and VWMANE from 'A' to 'AB'.
Whilst I'm at it, I also in the general tab, change the name to 'AB'.

All good so far.... But when I save the drawing and open it another time, sometimes it reverts back to 'A'. This seems very hit and miss as to when it works and when it doesn't. However, this morning I have discovered that when I move either the parent, or the section view, it reverts straight back to 'A' - this happens every time without fail.

What am I doing wrong? Is there a more reliable way to change a section view name?

Thanks

Tom

Contract Mechanical Design Engineer.

 

[cowski]

Don't mess with the view attributes or the name of the view on the general tab. Instead, right click the view -> settings -> common -> view label -> change the letter option to what you desire. The new letter will have to be one that is not already in use and it must be on the "allowed letters" list.

www.nxjournaling.com

 

[TomLoughlin]

Thanks Cowski,

I've tried renaming the view from the view label option, but it doesn't seem to let me name it two letters - I want to call a section view 'AB' and for some reason, that is not allowed - can you shed any light on this.

Our company policy for view names is to have details and sections as double letters 'Detail AB' or 'Section AC-AC'

I realise NX is trying to push single view letters which is fine, but what happens when you need more than 26 views on a complex welded assembly?

You could certainly do it in NX6, but they seem to have removed the functionality in NX9.0.

Thanks again

Contract Mechanical Design Engineer.

 

[JohnRBaker]

Try selecting the Section 'Arrow', press MB3, select 'Settings' and change the label there.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[cowski]

You might need to change your drafting preferences to allow more than one letter in the view label.

www.nxjournaling.com

 

[TomLoughlin]

John, tried doing it from the selection arrow menu - same issue.

Cowski, Can't seem to find the menu you show above, have you taken it from NX9? I can't see if within the drafting preferences menu.

Another lad here in the office (with admin privileges) has tried on another drawing, and by changing the common/view label from 'subscript' to 'inline' seems to change it, but this still doesn't work on my box.

Looks like I'm just going to have to put up with this one, as it might be an issue with my profile. The powers that be have locked most of the configuration settings :-(

Contract Mechanical Design Engineer.

 

[cowski]

Yes, NX 9.0.3.4
Customer defaults -> drafting -> general -> standard -> customize standard -> the rest you can see from the screenshot above.

I don't know if you can change this option directly in your current file (I've not found a way to do it). If this is the issue, you will probably have to change the drafting standard in the customer defaults, then import the drafting standard into your current file.

www.nxjournaling.com

 

[TomLoughlin]

I need to get onto the IT bods then, as it's locked down on our system.

Thanks for all your help.

Tom

Contract Mechanical Design Engineer.

 

[JohnRBaker]

Yes, my defaults are set like cowski showed you so everything works fine for me. As for the 'path' you use to get to the 'View Label' option, I suspect that it doesn't really make any difference which one you use, the results are the same.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

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