NX 10 balloon on different sheets 1

[donrafa7]

How can i add balloons to different sheets of the drawing that are linked to the parts list. I want to balloon a component on sheet 3 with the bom on sheet 1. I believe I used to do this using INSERT > Symbol > ID symbol but in my install of NX 10 there is only insert symbol Custom / Define custom symbol. Using classic interface with role advanced.

 

[Felix K. Holloway]

Hi donrafa7,

If you just want a balloon with a number in it that has a leader terminating at some point on your drawing, in NX 10 you can use the Balloon annotation:

Menu->Insert->Annotation->Balloon

If you want that identifier inside the balloon to be linked to say, a number on your BOM, which will allow you to auto-update all the linked numbers of that same number, you can create an expression for that BOM number and give it the appropriate name.

To link to the expression in the balloon function window, under the Text Rollout, click on the "A" icon to the right of the form box. From here under the Symbols rollout, expand the pull-down menu and click on Relationships. Then directly underneath that click the P1=/P2= icon to the right of "Insert Expression".

From there you can select your pre-made expression.

You can also experiment with the other types of relationships under the relationships Pull-Down list.

I'm not sure if that is exactly what you are looking for, but hopefully if not the answer is somewhere nearby in the Balloon function window settings.


Felix K. Holloway
Design Ninja | NX 9/10

http://www.nxprotips.com

 

[PatelJignesh]

Hello,

After placing part list on sheet 1, Add Balloon from Annotation.
It will Create blank Balloon. After that just update part list from navigator and Empty balloon will show associated part list item number to arrow.

Thanks,
Jignesh Patel
L&T Technology Services

 

[Lars1978]

PatelJignesh,

I've done just wat you told. I placed a emty balloon. When updating the part list the balloon stays emty ?

What can be the reason?

Kind regards




Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[PatelJignesh]

Hello,
There is on variable to update partlist.
please check if variable is set to correct.

UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST = 1

Also are you running with team center or native?

Thanks,
jignesh


Thanks,
Jignesh Patel
(NX9/TC10)
L&T Technology Services

 

[Lars1978]

Patel,

I'm running native.

Where can i check this variable ?

Kind regards,

Lars


Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[PatelJignesh]

GO to Files-Help-Log file and search for variable.

Thanks,
Jignesh Patel
(NX9/TC10)
L&T Technology Services

 

[Lars1978]

Patel,

Thnxs that did the trick

Do you know why I have to set this variable ? I mean why isn't this variable set default to 1 ?

Kind regards,

Lars


Lars
Solid Edge
Inventor
NX10.0.3.5 native

 

[Toost]

No,no,no,
back to the basics.

The foundation of the balloons and partslists in NX, :
A partslist has the option to update a designated shape of id-symbol. Per default this is the circular type but it can be changed to any shape. ( of the NX provided shapes)
When you add a id-symbol ( balloon) you MUST snap the leader to the component. ( You can select a face also but if you load a drawing file only ( not the model/ assembly) this balloon will be "retained". ( dashed lines)
Then select the partslist- "Update" and the balloon will receive it's number.
the formatting of the partslist ( the callout column) then controls what will be written in the corresponding ballon.
The sorting etc of the partslist is controlled by the partslist ( RMB- Sort) - and thereby what position number the component gets.

The variable UGII_UPDATE_ALL_ID_SYMBOLS_WITH_PLIST = 1 is set in the "ugii_env_ug.dat" (by default=1 ) you can find the file in the install directory under \ugii ( note that if you like to change this variable you should write the change in the "ugii_env.dat" and not modify the "ugii_env_ug.dat".)

Regards,
Tomas