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Adding Reference Balloons manually - NX 11

Adding Reference Balloons manually - NX 11

Adding Reference Balloons manually - NX 11

I use the "Auto Balloon" tool to start documenting my assemblies.

But if I turn on "Reference Symbol Text" under the Parts List settings it gets out of control quickly due to the size of my assemblies.

Is there a way to add singular associative "reference" balloons at my discretion??
It's OK that it would look like the "Reference Symbol Text" balloons but I need to control the "when and where"

The "Main Symbol Text" is set to "Part Name" so the part file and part list call outs always match.
I used to know a way to grab the <W$=@$PART_NAME> attribute using the "Leader" command but have forgotten it somewhere along the way. That would work OK but it would be nice if we had a tool to do this.

I'm hoping there is and I'm just a little out of the loop from relying so much on Auto Balloon.


Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1

RE: Adding Reference Balloons manually - NX 11

You can manually place an empty balloon attached to your individual components at the desired location.
As soon as you place a partslist and update it, the balloons will be filled with the correct callout.

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX11 / TC11

RE: Adding Reference Balloons manually - NX 11

It would be great to be able to place empty balloons on parts and just update the parts list to populate.
But I've played around with your suggestion but haven't had any luck.

What I've rediscovered was the method I mentioned in my initial post.

Using Category: Relationships
"Insert Object Attribute"

Set selection filter: Component

Select the screen component: That already has a balloon

Select: "$PART_NAME" (Under Attribute Group: All Unset)

It works but it's a little painful and you have to make sure your attaching the leader to the right part.
There isn't anything automatic about it but if you change the part name it will update correctly.

Automotive Tooling / Aircraft Tooling / Ground Support Structures

NX9, Win 7 Pro SP1

RE: Adding Reference Balloons manually - NX 11

What Ronald says is correct.
But, there are a few things,
you MUST attach the arrow to an edge of the component. ( point on curve snap type) It will also work if you snap it somewhere on a face ( point on face snaptype.) But, if you later load "drawing file only" , the faces will not be there and that balloon will be in "retained state" in this session. ( will not update since the component isn't there.)
If the arrow isn't attached, the balloon will not update. the position of the "balloon itself" is irrelevant.
You also need to make sure that the type of balloon is the same as what the partslist updates, - you cannot have the partslist / autoballon create and update circular balloons and manually place a different shape.
See image.


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