Six SOLIDWORKS Solutions – BOM and Balloons

When working with SOLIDWORKS support, I receive questions multiple times, and most of the time the answer is the same.

So in this and some of my other blog posts, I will be giving some examples of questions I receive when working in support, as well as offer solutions for them.

In this blog post the focus will be on BOM and Balloons, as that can also prove to be quite a handful on occasions.

All of the solutions offered here can be done by most users

BOM reference

Sometimes it can be useful to have multiple views and BOM in a drawing due to different configurations.

However, if you delete one of the BOMs your Balloon on the referring to view with the deleted Table does not match the remaining BOM.

Reinserting the Balloon does not help.

To solve this you have two options:

  1. Insert a new view.
  2. Make sure the existing view refers to the correct BOM


I will not go over option 1, but instead focus on option 2.

Right click on the view and press “Properties”


Under balloons, set a checkmark on “Link Balloon text to specified table” and select the table you want to link to.


BOM Order

Sometimes it can be useful to have the same assembly in different configurations on the same drawing.

And even if possible, make sure that the BOM numbers match in the view.

Wrong BOM number

It is possible to rearrange the numbers manually, but doing this is a time consuming task and errors can occur.

I recommend rearranging the parts and subassemblies with the suppressed models in the bottom as shown in the below video.

This way the BOM will always update and if a new configuration is inserted, it is automatically sorted in the right order.

You only need to make sure that “Follow assembly order” is checked, and your BOM should match up nicely.

follow assembly order

Bill of material options

When working with subassemblies on BOMs 
you can sometimes experience one the 
 following issues.

1) Your parts does not appear on the BOM, only the subassembly.

BOM options

2) Or the subassembly it self does not appear on the BOM.

In most cases this is due to a setting in the configuration in the affected subassembly. To resolve it, open the assembly and go to configurations, right click on the active configuration and press “Properties.”

Subassembly options

Find “Bill of Materials Options”, and the section “Child component display when used as subassembly.”

Bill of matiarial options

Here you have 3 different options on how to show the assembly when it is used as a subassembly in another assembly AND when the BOM is set as “Indented”;


This shows the entire assembly with both assembly name and parts.



This hides the parts completely in the BOM, and only the Subassembly is visible


When this radio button is marked, only the parts of the assembly is shown and not the assembly itself



All of these have different uses, depending on what you want to show in your BOM.


Size of balloons

In SOLIDWORKS you have many options on how to customize your drawings.

One of these is the size of the balloons.

On the below image you can see an example of to large Balloons.

Balloon size

This is set within the document properties and saved in the template.

Go to Tools->Options->document properties->Annotations->Balloons

Balloon size

You have the option to modify the size and shape of the balloons for both single balloons and stacked balloons.

Once you have found the size and shape you want, press ok and save the template.

However the existing balloons you need to change them manually.

Click on the individual balloon or select multiple balloons and change them in settings.

Manually change balloon size


An Asterisk (*) Instead of a number, 

When placing a placing a balloon on a drawing it can sometimes occur that instead of a number you get an asterisk (*)

Asteriks in Baloon

If you have inserted a BOM Referring to a configuration where the particular part is missing, you can get this error:

BOM configuration

In the below example I have created a configuration with “The train” Missing, the result is an asterisk in the balloon.

Asteriks in balloon

This being a simple assembly it is relatively easy to locate the error.

Another reason for the asterisk, could be if the part (or subassembly) has “Exclude from BOM” option checked.

To find out if this is the issue, go to your assembly, left click on the part or the subassembly and press properties.

part options

Here you have the option to “exclude from the bill of materials”,

Exclude from BOM

If this is checked, you will see an asterisk as well as the part or subassembly will be missing from the Bill of Materials.


Balloons do not snap to the parts

Balloon snap

This is a problem that occurs if you have created your own view in perspective mode and used it in a drawing.


Create a new view where perspective mode is turned off to solve this.

To achieve this easily, select your customized view and make sure that the perspective mode is NOT active.

perspective unselected

Now save the view as a new view, by pressing space and selecting the New view icon.

new view

Now select the new view in the drawing orientation.

select view


And your balloons should snap to the parts just fine.

I started working with CAD systems in 2003, and have since 2012 worked solely with SOLIDWORKS. I am a certified Technical support specialist as well as a SOLIDWORKS Certified Expert. Since 2016 I have helped PLM Group customers to work smarter, not harder. The inspiration for most of my posts comes from the support cases i work on. When writing blogpost I try to focus on the everyday use of SOLIDWORKS.

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