Pattern not loaded

[cubalibre000]

Hi,
we work under Teamcenter.
We have exported a project locally to send to our supplier to complete the project.
We have exported also the pattern locally in the same folder where project files reside, but when we open a drawing with the master model approach, the title block (pattern) is not visible, sure not loaded.
Exist a procedure to reload the pattern automatically, manually o via macro ?

Thank you...

Using NX 8 and TC9.1

 

[looslib]

There is a varaible, pattern_dir, that will point to the location of the pattern file. If it is blank, I'm not sure where it will look for the pattern that your drawing part file references.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

While I can't say for sure in this case, generally speaking when not directed otherwise, NX looks in the folder where NX was installed.

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.

 

[cubalibre000]

Hi looslib,
I tried to follow your suggestion, but we work under TC and when we export the project, the drawing look for a pattern called like %PAT VYPtKe2nHhbWqD.

Thank you...

Using NX 8 and TC9.1

 

[looslib]

That happens when you store your patterns in TC. I have never used TC, but have lots of experience with another package.

We were told to load the formats (patterns) outside of the PDM and reference them from the external location. We also have to have a copy of the format in the PDM for when a file is retrieved after initially being created with the external format. TC may work differently, but our files are looking for the actual name of the format, not the PDM encrypted filename that your exported files seem to be looking for.

If you tried the pat_dir folder with your pattern, retry it with a renamed pattern file matching the TC internal filename.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[cubalibre000]

Hi Ben,
you have wrote :retry it with a renamed pattern file matching the TC internal filename.

Yes, after your primary suggestion, I tried this.
The problem is that NX store in the file each pattern you have used.
For example, I start to create a A4 format drawing, but after some saves and modification I need to switch to A3 because I've added some more views.
So NX save in this file like some type of info 'pattern A4' and 'pattern A3'.
When I export this file outside TC, in native, using Format->Pattern->List pattern errors, NX lists %PAT VYPtKe2nHhbWqD and %PAT VYtKKf45HhfIhF.
So, if I rename pattern A3 and pattern A4 whit this name, NX drawing show each pattern.

For this we have decided to change from old format (pattern) to the new title block.
The new title block are ready, but as other thread, I'm not able to delete old pattern and load the new title block.
GTAC doesn't have experience on this new title block, so I need to ask here and try myself.

Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

Just remember, the new Drawing Border/Title Block functionality is not a direct replacement for 'Patterns' as they are not 'referenced' items but rather are intended to be used as a template which is copied and then becomes the Drawing file itself.

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.

 

[cubalibre000]

John,
now it's more clear.
So if I want to dismiss 'Patterns', for new files, I use the new templates that contain the new title block. Right ?
If the drawing exist with the old 'Patterns', for example I make a new revision, how can use the new title block ? Only via some type of automation ?


Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

If you're updating older drawings, you will need to explicitly delete the 'pattern' object and then add the Drawing Border/Title Block. Now the Drawing Borders will need to be added manually, using the new (NX 8.0) Drawing Border function, to each sheet of each Drawing. However, Title Blocks and Parts List and other additional sysmbols and notation, such as sheet numbers, 1st/3rd Angle symbols, etc, they can all be 'Copy & Pasted' from a master template in each sheet of each Drawing.

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.

 

[cubalibre000]

Hi John,
always more clear.
So, if I want that this procedure must be transparent to the users, I will need some type of macro.
The last question, in this topic

http://www.eng-tips.com/viewthread.cfm?qid=221010,

you talk about yours title block used for demos.
Yours title blocks are symbols.
Can I import my 'pattern' in a drawing, convert to lines and texts and create a symbol title block for each format, inside each template ?
Which are the benefit to use NX8 Drawing Border/ general table converted in Title Block, respect to lines and texts converted in symbols under 256 layer ?
I thought symbol, because can be related to the master symbol, so if I change the master symbol, all old drawings will have the new modified title block without extra works to the NX users when drawings are open.

Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

I no longer use Symbol-based Borders and Title Blocks. I've converted my demo parts to the new NX 8.0 style Drawing Border/Title Block Drawing templates.

As for the automation, I'll have to leave that to someone else.

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.