Hide Balloon Leader Possible - New Post?

[jacob.dillingham]

New post created by moderator, referencing this older post.

Is there any automatic work around for this? I can make the leader line hearts or bullets if I want but I can't make it invisible? I can make the leaders for sketch symbols not visible but not for item bubbles that use the exact same sketch symbol?? Inventors customizability with item bubbles is astonishingly terrible.

[CGBenner]

@jacob.dillingham 

Hi Jacob... what version of Inventor are you trying to do this with?

[jacob.dillingham]

Inventor 2019.

[johnsonshiue]

Hi Jacob,

This is quite easy to do. Edit the Balloon style and edit the associated leader style. Set the leader to None. If this is the style you like to persist, you may want to save it in the drawing template and also save it back to the Styles Library.

Many thanks!

[jacob.dillingham]

I'm not seeing the "None" selection you are talking about.

[johnsonshiue]

Hi Jacob,

I am not talking about the line type. I am talking about the Leader head. It looks like you already have it set to None. But, you want to completely remove the leader line, right? I think I misunderstood it. Sorry!

I guess the only option is to change the leader line color to white or the same as the background. The leaders have to be there and attached to a piece of geometry, so that the balloons can obtain the data from the designated components.

Many thanks!

[gcoombridge]

Can do this with the API... Warning this rule will do it to every balloon in your drawing.

Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet = oDoc.ActiveSheet

Dim oBalloon As Balloon

For Each oBalloon In oSheet.Balloons
	Try
		oBalloon.Leader.AllNodes.Item(1).Delete
	Catch 'Do Nothing
	End Try
Next

[SharkDesign]

You can delete the leader on a text note by right clicking, but not balloons. 

You can hide the leader on a balloon by placing one with a leader and then dragging the balloon on top of the arrow, like this:

But it has to touch the outside line of the part. 

[jacob.dillingham]

yea that's the way we do it currently. The whole point is I'm trying to find a way to keep 10+ engineers from having to do that hundreds of times on hundreds of drawing sets because it's annoying and time consuming. I keep coming back around to item bubble customization in inventor is astonishingly terrible considering the very similar customization that is available for regular sketch symbols. 

@johnsonshiue  can we please look at offering similar functionality between sketch symbols and item bubbles? this is very annoying that item bubbles are the only way, without ilogic, to access BOM level info in a drawing and that the customization for item bubbles is so incredibly lacking. and also you shouldn't need a visible leader in order for item bubbles to work. you should need a leader yes, but it shouldn't have to be a visible leader. sketch symbols have the option to have a leader and be able to toggle it's visibility. you still attach the invisible leader to the part so it can pull info like file name, description, etc from that part but the actual leader itself does not show on the drawing. 

[Curtis_Waguespack]

Hi @jacob.dillingham 

My apologies if I've missed something, but just in case it has been overlooked, I wanted to point out that your users can place the balloon with no leader as they place the balloons.

To do this we start the balloon tool, click the component and then.... rather than clicking on the sheet to place the balloon, just hit the enter button on the keyboard... or right click and choose Continue...

This will place the balloon on the edge of the component where it was selected.

If this is something you're already aware of, or just isn't useful for your workflow, just disregard my reply... but I thought maybe this had been overlooked.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[jacob.dillingham]

Sorry but i need the balloon out in space because we have to place 2 different style item balloons in order to display the needed information in a way that doesn't look like appalling. See the picture below. Even though the line style of the item balloon on the right is barely visible in inventor, when we export the file to AutoCAD for our customer it shows up clear as day and the customer doesn't want 2 leaders going to the same part in the drawing.

[johnsonshiue]

Hi Jacob,

I think I know the requirement. You want to be able to place a balloon by selecting a component and placing on the sheet without a leader. Sketch symbol can do that because it can be just a static text and sketch geometry. If you need to retrieve data from a component, the leader serves as anchor to hook up with the data source.

At the moment, Inventor does not have such paradigm allowing to retrieve component data without attaching a leader. To support it, it will be a big change I have to say.

I am wondering if you will be better off using AutoCAD to document Inventor components. AutoCAD does support associative drawing view (VIEWBASE). Then you can use AutoCAD's drafting tools to annotate the views more flexibly.

Many thanks!

[jacob.dillingham]

Again I am not talking about not having a leader. I am talking about an invisible leader. Big difference. there would still be an anchor point so that Inventor knows which component to display information on but the leader itself will just not be visible. it would work in the exact same way that a custom sketch symbol created to show the description of the part in which the anchor point is connected to (See "CUSTOM SKETCH SYMBOL.png"). you can then insert that sketch symbol into the drawing. before selecting the sketch symbol you want to insert you can toggle the visibility of the leader in the window (See "SKETCH SYMBOLS WINDOW.png"). see "TWO SKETCH SYMBOLS.png" for one symbol placed with a visible leader and one placed with an invisible leader. the anchor point for both sketch symbol is on the same component and thus pulls the same part level description. I can move the anchor point to any other component in the drawing and it will update automatically to whatever the description is of that part. 

The functionality already exists with sketch symbols. I can't imagine it would be too big of a job to adapt the already existing functionality to item bubbles.

[johnsonshiue]

Hi Jacob,

Many thanks for your explanation! I think I get it. It is indeed doable with custom sketch symbol. But, it is not doable with balloons unfortunately. Here is an idea on Inventor Ideas forum. Please vote for it.

https://forums.autodesk.com/t5/inventor-ideas/delete-balloon-leader/idi-p/6642017

Many thanks!

[gcoombridge]

@jacob.dillingham give that iLogic rule a go - it does exactly what you want and remains associative...

It just needs to be placed in your drawing template or as an external rule. I wouldn't hold your breath on a functionality change in the software

[jacob.dillingham]

I wish I could. But unfortunately I don't need to do this to every item bubble in the drawing. I need it for half of them. Unfortunately this is just another gripe from an ongoing tiff about how the customizability of item bubbles is terrible. for our customers we have to show 3 BOM properties for each component in our assemblies, item number, ref drawing number, and what category the part is (drive, support, guard, tube steel, etc.). So since we can't have all three of these properties shown in one item bubble in a way that looks even remotely good, we have to place 2 custom item bubbles right next to each other in which one of the item bubbles has the leader connected to the part and the other has the leader hidden by pulling the leader underneath the bubble. Thank you for trying to help though.

[gcoombridge]

That's easily solved - this will allow the user to pick the balloons to remove the leader from...

Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet = oDoc.ActiveSheet

Dim oBalloon As Balloon
Dim BalloonCol As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection

While True
	oBalloon = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingBalloonFilter , "Balloons to remove leader from (ESC when done)") 								
	If IsNothing(oBalloon) Then Exit While
		'adding selected curves to a collection
        BalloonCol.Add(oBalloon) 
End While


For Each oBalloon In BalloonCol
	Try
		oBalloon.Leader.AllNodes.Item(1).Delete
	Catch 'Do Nothing
	End Try
Next

[gcoombridge]

Note that if you want to re-attach the balloon you can just add a leader back onto it with the right click menu. 

[jwborra]

Hi there! 

So I had a similair issue. I need big leader texts in my drawings and i need the BOM item number and i want it in a balloon. 

The quickest (dirtiest) trick i am now using since ive spend to much time reading through forms and trying to figure it out is this:

-Make a custom leader style that has no head, is dotted and has an lineweight of 0,01. (Inventor shows a dropdown but you dont have to use that, you can just manualy enter a value) Also make it white so it doesnt show up on your paper.  (added picture is of an A1. Youve got eagle eyes if you can spot it haha)

Hope this helps someone and saves you a lot of time and headaches!

Bye!

Joris

[dan_inv09]

From the pictures of the original problem, it looked like they needed to attach a balloon of a different style. Or they needed a new sketched symbol balloon with the item number in a circle appended to the end of their existing sketched symbol "balloon".

You probably could also accomplish what they wanted by carefully laying the balloon leader for the regular balloon over their special balloon's leader - but that's a real pain, especially if anything has to move.

Now you can use the Item number in a View Label. (Do you want it with the circle?)