*NEW TO INVENTOR* attaching ballons to sketch elements

[gleclerc]

I have a sketch that I would like to attach a parts list balloon to. Is that possible?

[mcgyvr]

No balloons cannot be attached to a part that is only sketch features..

What specifically are you trying to do? There may be other ways to accomplish your needs..

[gleclerc]

I just want to have a sketch element labeled with an item number that matches my part list. It's something that I don't want to bother to model (heatshrink). Modeling it isn't practical to me as it follows a weird profile and a simple sketch gets the message across clearly on the drawing.

[mdavis22569]

You might be able to use a sketch symbol one .. (not recommended, and won't be part of the BOM/Parts list)

[mcgyvr · Accepted solution]

Well.. In order to balloon to it you will need some "3d feature" applied to something in that part..

It could be a very small extruded circle or something but you will need a 3d feature created of some sort to allow ballooning to.. 

Even an extruded surface of this heatshrink or something.. But you need more than just a sketch to have a fully functioning balloon..

-Workaround possible to not create any 3d features-

I suppose you could balloon another item in the drawing then drag the balloon to those sketch edges on the sketch only part and then override the value of the balloon..

That should work too and not require you to add any 3d features.. 

[gleclerc]

OK so I found a way. Not sure if it's the best way but wil work for me.

1. attach a balloon to an nearby actual component in the parts list

2. grab the arrow head of balloon and attach to sketch element.

3. right mouse click, and select "attach balloon from list".

4. Select the parts list item I want to be attached to

5. now there are 2 balloons attached to leader, Right mouse click on first balloon (unwanted one) and click "remove balloon"

[gleclerc]

@mcgyvr thanks, I was just typing that I did basically that while you were responding (see my response above).

[mcgyvr]

@gleclerc I like how you did the "attach balloon from list"...

That keeps you from potentially making a mistake of not typing in the correct item/part number..

Glad thats gonna work out for you.. 

[jtylerbc · Accepted solution]

@gleclerc, another variation of what you did could be as follows:

1. Add the heatshrink in the assembly as a Virtual Part.  Fill out any properties (Part Number, Description, etc.) that are relevant for your parts list.  You can also override the quantities in the assembly BOM if needed.
2. Start the Balloon command and click a nearby component, just as you did before.
3. Before actually placing the balloon, right click and Select "Custom/Virtual".  Then pick your desired part from the list.
4. Reattach the balloon leader to the sketch geometry, just as you did before.

This cuts out the need to create and delete the extra balloon.  It replaces it with the need to create the Virtual Part, so at that point it's sort of an even trade.  However, the Virtual Part can be copied to other assemblies, so you don't have to type the property data for the heatshrink again every time you use it.

May not be all that helpful for you if this isn't something you do regularly.  But if you use heatshrink (or other not-modeled parts) often, this could be a slightly easier way of doing it.

[gleclerc]

@jtylerbc thank you, this is very helpful