I’ve been using balloons in SOLIDWORKS for years, and so have you, probably.
But I don’t really know a lot about balloons. Which also means I am not using them in the best way possible.
That’s about to change.
Turns out I learned 8 new things while writing this post.
These are some few of the topics I will be discussing:
This is the weldment that we will be experimenting on:
Contrary to my beliefs, you don’t actually need a bill of materials (BOM) or a cut list on your drawing.
SOLIDWORKS will use the same numbering system for the balloons, whether you have a table or not.
When you do have a drawing with a cut list or BOM, it seems like the balloons are linked to the table.
While in reality balloons are only linked automatically when the table is on the same sheet as the view!
The image below shows a view for a single weldment on the second sheet. The table is on the first sheet.
When you change the order of the table, the item number changes but the balloon text stays the same.
The balloon number will only be in sync when you actively link the view (right-click view > Properties) and enable Link balloon text to specified table.
So be very aware of this when changing the sorting order in a table. Especially when working with multiple sheets.
I thought you could only add balloons to a drawing, but then I remembered that you could also add a bill of materials to an assembly. I don’t know why, but hey.
Turns out you can add balloon annotations to assemblies as well. I just couldn’t get the Balloon text source to be linked to the BOM without the balloons disappearing. It seems that every time you add a balloon and it disappears, it stays around but it is hidden.
The balloons also do not show up in the annotation folder in the feature tree:
Stacked balloons are a blessing. They allow you to do group components that belong together, like this bolt, nut and washer:
To turn a single balloon into a stack or add one to an existing stack: right-click the balloon > Add to Stack.
To delete a single balloon from a stack: click the balloon you want to delete, then press delete.
You can even change the direction of the stack:
To sort the stack, right-click one of the balloons and select Sort Stack
Magnetic lines are another great addition to SOLIDWORKS.
Your drawing looks so much prettier when the spacing between balloons is constant.
To add a magnetic line, go to the Annotation toolbar and click the button right under the Auto Balloon button.
Now click to create a start point and an endpoint, all the while picking up as many balloons as you like along the way. To add, remove or reorder a balloon, just drag it onto or away from the magnetic line.
The magnetic lines get hidden automatically when you’re not working with balloons. So if you can’t find them, just click a balloon and all magnetic lines will be visible again. When there are no balloons left but there are magnetic lines, just add a balloon to make the lines visible again.
AutoBalloon tries to add all balloons to a view. Sometimes it’s a great start, sometimes it does more bad than good.
I said tries because there are some limitations. For starters, only components that are visible in that view get a balloon. But in this case, SOLIDWORKS also seems to miss the main vertical and horizontal beams.
As you can see, AutoBalloon seems to have failed to add two balloons.
And then I pressed the Drawing button right next to it:
Turns out I had already added these balloons manually at another sheet, and AutoBalloon figured we didn’t need them twice. Fair point. I’m glad our tool found the error I just made.
I found a trick that might be useful in this video by GoEngineer. It’s at 35 seconds into the video.
The option is that you can change the sorting order in the bill of materials, so the top balloon gets number one, the second gets number two and so forth.
I had trouble finding this option, because:
This one is pretty useful. I don’t add the quantity to every balloon though. I prefer to add the quantity:
You can enable or disable the quantity per balloon, just check the checkbox and you’re off. I use the override value a lot in the situations I mentioned above, even though using override is not very future-proof. When the hole pattern changes and the number of bolts in that subsection changes, the count does not update.
When you remove a component or cut list instance, the balloon breaks and you can end up with a (stacked) balloon with a question mark:
The dirty color means the annotation is now dangling.
To fix the broken link, you need to reattach the balloon. Right-click the broken one > Reattach, then click on the component you want to attach it to.
You can also decide to delete this dangling annotation with Drew:
In this situation, clicking a button will delete only the broken balloon from the stack. The rest of the stack remains intact.
This appears to happen when the drawing view is outdated.
According to this forum post, all you need to do is:
When you have multiple configurations (and remember that exploded views, flat pattern and weldment create additional (derived) configurations) and the bill of materials does not show the quantity for that configuration, the item count will not work.
To fix that, you can add the configurations to the BOM by clicking the column and then the Column Property button. This will add a quantity column for each configuration, but you can hide that column if you want. Just right-click the column letter > Hide > Column.
You can also change the configuration in the feature tree in the properties of the bill of materials.
If the balloons show a different value than the bill of materials, the view and the BOM use a different configuration. You need to make sure they use the same configuration.
You can change the BOM configuration here:
You can change the view configuration here:
If this does not fix your issue. check out Don’t forget to link balloons to a table.
This is an easy one. Just change the style of the bill of materials or the cut list and the balloons will change accordingly.
According to the official help page, balloons can have an asterisk for two reasons:
When SOLIDWORKS is working correctly, a balloon with zero means the component is excluded from the cut list.
SOLIDWORKS creates a cut list for weldment and sheet metal parts. It stores all identical bodies in a folder and you can choose to exclude certain folders.
Other parts get a folder called Solid Bodies, but you cannot exclude bodies from there.
There are two problems with this feature:
SOLIDWORKS adds a single leader/arrow to a balloon by default. But you can add multiple leaders to a balloon:
You can add a second leader by dragging the end of the arrow onto the second component while holding the Control (Ctrl) key.
Don’t get fooled by the preview, the position of the preview is often wrong. Only let go of the mouse when hovering exactly over the second component.
If the component is identical, SOLIDWORKS adds a second leader.
A customer recently told me:
“When you link a balloon to a face and the face moves, the balloon breaks. When you link the balloon to an edge, the link never breaks.”
I had some trouble in the past with broken links, but I just tested a few different scenarios in SOLIDWORKS 2018 and I could not confirm this method. I think his method worked in the past, but SOLIDWORKS has apparently improved the software recently.
When you write a note, just click on a balloon to add it.
If the balloon number changes, the note will update as well.
This feature is pretty neat, I had no idea it existed.
You can change the number in the balloon and the table (BOM or cut list) changes with it:
The drawing template is the file that stores most of your preferences for a drawing. The sheet format is something different, it mainly stores the title block and the frame around the sheet.
So if you would like to change the style of the balloons, change a setting in a new drawing, then save the drawing as a drawing template.
I decided to write this post to learn more about balloons, and to see what would happen. Turns out there are a lot of hidden gems that I didn’t know about yet.
I did not know that changing the item number in a balloon could cause the BOM to update. I also learned how to fix the balloon count when creating an exploded view.
Have you learned something as well? I really hope you did.
If you know a tip that can be added to this post, please let us know in the comments of this post on LinkedIn. I will add all useful tips to this blog post.
Here are some pointers that you might find useful when you want to get started with a macro that works with balloons:
If you need any more help getting your macro to work, or if you would like us to develop a macro or an add-in for your company, get in touch.
You can also use the official SOLIDWORKS forum to ask your question. I’m answering questions there regularly as well.