I can't seem to find a way to do this in Creo 2.0, but I need the REF balloon to match my custom balloon.
For reference, my company uses a custom BOM balloon where the part number is displayed in the balloon and the qty is outside the balloon. It looks like this:
I want the REF balloon to look exactly the same but display "REF" instead of the QTY.
Anyone know how to accomplish this?
You need to modify the reference balloon symbol in the symbols>report>bomballoon. I don't think there is a way to place it in another directory and force Creo to recognize it as the default reference balloon.
Try making a copy of your custom balloon (same symbol with a different name). Then do the alt balloon replacement. Then under the Annotate tab go to Symbol -> Symbol Gallery and redefine the alt balloon. Add REF and then Done -> Done -> Regen. See if that gets what you want.
I think you may have the wrong form in the symbol. The form should be the same as what is in your repeat region. If your parts have a parameter part_number the balloon should have the line \asm.mbr.part_number\ or the line \part_number\ and in the Attributes box specify asm.mbr.part_number as the value.
I've never tried to replace the default balloons, but I'd start looking into this folder:
<Creo 2.0 installdir>\Common Files\MXXX\symbols\report\bomballoon
What we do is we modify the standard reference balloon in the folder <Creo 2.0 installdir>\Common Files\MXXX\symbols\report\bomballoon.
It HAS to be the same name as the reference balloon and it HAS to be in the same folder as the standard reference balloon. These are hard coded in to creo.
You can not use alt symbol for reference balloons.
Oh and if I remember correctly, once you've added the standard reference balloon to a drawing, you're stuck with the one you started with. I've never figured out how to get it to re-read the reference balloon once it has been added to a drawing...a source of infinite frustration when we updated build codes and I forget to re-copy my reference balloon over.
I just discovered found the solution to this dilemma. It appears that PTC recently added a hidden dtl option:
Note: its hidden, so you have to manually type in the option name and value.
I have created my custom reference symbol and REPLACED this files in the Creo:
%loadpoint%\PTC\Creo 3.0\%datacode%\Common Files\symbols\report\bomballoon\qty_ref_bln.sym
%loadpoint%\PTC\Creo 3.0\%datacode%\Common Files\symbols\report\bomballoon\smp_ref_bln.sym
Note: default BOM symbol is possible to set in *dtl file >> set configuration option
Best Regards, Vladimir