move notes and tables to new sheet

[multicaduser]

Back in the old days patterns were used to create title blocks and boarders. Instead of trying to update the pattern every time we have to make a change it would be nice to move everything to a sheet that uses the newer style for these items. The only issues I'm having is how to move notes and tables, i.e. parts list, etc, to the new sheet. An easy work around for notes is to edit them and copy the text then paste them into a new note, clunky but effective. Parts lists cannot be copied while the variable UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST is on. Is there an way to move the parts list to a new sheet without turning this variable off or am I stuck with patterns?

NX9.0.3.4 Windows 7 SP1

 

[jerry1423]

did you try cutting and pasting it?

 

[Arkance/PhoeNX]

If you disable the variable, you can do the copy/paste, save the part, then re-enable the variable.


Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[Toost]

This is how we do it in NX7.5. I tried it in NX9 and it works the same. Don't know if there are better methods or not. In NX7.5 it's the only method i found that keeps the balloons.
in short : Use View Dependent Edit to convert the Partslist from view dependent ( sheet1) to model dependent, then model dependent to view dependent on sheet2.
This will keep the associated ballons associated. The balloons will stay as is on their respective sheets.
( A view dependent object is only visible in a specific view, A model dependent object is visible in all views. The partslist is view dependent on the drawing, which is a special type of view.)

open the sheet with the partslist. RMB on the "Sheet1" in the Part Navigator - View Dependent Edit...- View to Model - Select the Partslist, OK , OK
Open the "Sheet2", RMB on the "Sheet2" in the Part Navigator - View Dependent Edit...- Model to View - Select the Partslist node in the Part Navigator, OK OK.

Regards,
Tomas

 

[multicaduser]

Not sure what is happening but cut/paste works great for notes, however the view-to-model/model-to-view thing isn't working for the parts list. It puts the parts list to the flat xy plane (the sheet with the parts list is a tri view), and it does not show up on the other sheets.

After a quick search through the usual areas (computer->properties->advanced system setting->environment variables, batch files), the UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST is not to be found.

Going to re-create the parts list and call it a day. Thanks for all the replies, this is a great forum.

 

[JohnRBaker]

That environment variable, along with most all of the others used by NX, are found in a file named 'ugii_env_ug.dat' located in the UGII install folder. Now rather then editing this file, you have two choices, either go to "the usual areas (computer->properties->advanced system setting->environment variables, batch files)" and copy & paste this variable there and change it to what what you want as this will override the settings in the above mentioned file. The other option is to copy & paste the variable into another .dat file named 'ugii_env.dat', which will also override the setting in the above named file. Now the reason for having TWO of these .dat files is because when installing an MR or MP update we might have to replace the 'ugii_env_ug.dat' file since it's, as I stated earlier, the repository for virtually all environment variable used by NX. However, the 'ugii_env.dat' is NEVER replaced during an update. Therefore, any entry that's create in that file will be protected and will always be in effect even after several updates.

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.

 

[Arkance/PhoeNX]

@multicaduser, have a look at

http://vimeo.com/106565338

, I explain what the variable does and how to set/unset it (among other things to do with parts lists).


Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[Toost]

"isn't working for the parts list. It puts the parts list to the flat xy plane (the sheet with the parts list is a tri view), and it does not show up on the other sheets."

- Do you have the partslist Inside a TRI View ?!?! - as in the attached image ?
I have never seen that before.

The method described works when the partslist is ON the drawing plane. We use it every week. Our (inhouse-)standard states that the partslist always must be on the last sheet-s, so if somebody needs to insert a new sheet, the partslist must move. ( NX7.5 cannot insert sheets in between, they always add as the "last".)


Regards,
Tomas