Ballooning Subassemblies in a SOLIDWORKS Drawing

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Article by Nathan Marsh on Feb 17, 2026

Sometimes, when working within a SOLIDWORKS drawing containing an indented BOM and an assembly with subassemblies, you need to balloon the entire subassembly and not just a component contained within it.

There are a few ways we can balloon the entire subassembly:

Ballooning to the subassembly origin
Ballooning to a sketch entity contained within the subassembly

Ballooning to the Subassembly Origin

For this method, the balloon will simply attach to the origin of the subassembly. First, the origins will need to be set to Show from the Hide/Show menu (View > Hide/Show > Origins). Next, the origin itself within the FeatureManager Design Tree of the drawing will need to be set to “Show”.

Hide / Show Origins in SOLIDWORKS

SOLIDWORKS FeatureManager Design Tree Show Origin

Now you can insert a new balloon and attach it to the origin of the subassembly to show the subassembly Item Number.

Ballooning to the Subassembly Origin in SOLIDWORKS

If you are having issues selecting the origin for the subassembly while placing the balloon, right-click on the origin point and choose Select Other to ensure the origin of the subassembly is what the balloon is attached to.

Select Other Subassembly Balloon in SOLIDWORKS

Once the balloon is inserted, feel free to change the origin visibility back to “Hide” so that the origins are no longer shown in the drawing.

Ballooning to a Sketch Entity Within the Subassembly

The other method of ballooning to the subassembly (and not a component contained within the subassembly) is to open the subassembly and start a new sketch at the assembly level. This method can be used when the subassembly origin is in an undesired location or if you prefer the balloon leader to be attached elsewhere on the subassembly.

Insert a line or a sketch point in an assembly-level sketch.

Insert a line or a sketch point in a SOLIDWORKS assembly-level sketch

Toggle back to the drawing file and set the sketch visibility to “Show” (View > Hide/Show > Sketches). Next, scroll down in the FeatureManager Design Tree to locate the new sketch added in this subassembly, and right-click > Show.

Insert SOLIDWORKS Balloon Point Line

Insert a balloon and attach it to the sketch point/line. It should now show the Item Number of the subassembly and not a component contained within the subassembly.

SOLIDWORKS Ballooning Subassemblies in a Drawing

Lastly, feel free to hide the Sketch or set the Sketch Visibility to OFF from the View > Hide/Show menu.

I hope you found this tutorial for ballooning subassemblies in a SOLIDWORKS drawing helpful. Check out more tutorials below. Additionally, check out the GoEngineer Community, where you can create forum posts, enter design contests, and answer questions from other SOLIDWORKS users.