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How to add Custom Information to a SOLIDWORKS Balloon

Article by Ben Crisostomo, CSWP created/updated October 31, 2018

When adding a SOLIDWORKS balloon to a Drawing there is an option to show the quantity of the part. This a great way to give the reader additional information quickly, but what if you want to show other model details in the balloon, for instance the length or material? There is no readily available option, but we can link the desired properties to notes to make it happen!

Why would we want to do this in the first place? Sure, I can just add a note and manually type in the length, but if there were any changes to the model or balloon position, that information would not be captured, so we need a way to link the values to the notes as well.

The Length of the Parts are shown with the balloons

Applying Linked Information to Balloons

In this example, we will be working with the base frame of a shed & the associated weldment cut list. We would like to show the length of the wood pieces in the frame along with the item number.

Create Properties for the Attribute That Will Be Used in the Model

For this step, the wood frame part file will be opened. Here we can check for variable holders and use them to call values in the File Properties list. We want to use values from the Cut List so we will look at the properties to get the syntax for the values.

  1. Go to:   Feature Manager Design Tree > (Right Click) Any CutList Item > Properties.

    Here we can see how the value for each Property is called

    Cut List Item Properties

  2. We can get the variable holder name for the length; e.g. “LENGTH@@@Cut-List-Item1@Wood Frame.SLDPRT” and use that to create the variable we will want to call in the drawing.
  3. As seen in the table below, P1, P2 & P3 will be the variables that will be referenced in the drawing. We can go here by selecting the File Properties button on the top ribbon of the SOLIDWORKS user interface.
Each custom property will be referenced in the drawing

Document Properties: Creating Properties that link to Features

Assigning the variable to the Note

In this step, we will return to the drawing and insert a note.

  1. Select Note from the Annotation Tab and place it in the drawing view where your balloons are populated.
  2. Select the Link to Property button in the Text Format Section to open the dialog box.
  3. Select Model Found Here with the Selected component or other drawing view selected from the drop-down menu.
  4. If you have different assemblies or parts in your drawing, make sure the selection matches the desired view.
  5. Select the corresponding property that we made earlier.
Steps illustrated for linking Document Properties to Notes

Note Pane: Linking Document Properties to Note

Grouping the Notes to the Corresponding Balloon

One more step! Here we will group the notes with the corresponding balloons so that they move together if the balloons are positioned differently.

  1. Align the note with the corresponding balloon to the desired position.
  2. Select the balloon & note pair.
  3. Right click anywhere and select Group from the selection pane.
Grouping Allows the balloon & note to move together

Grouping Note with Balloon

Now we have all the corresponding lengths for the part so we are good to go!

This method of pulling properties to notes and grouping can be used in conjunction with Global Equations/Variables as well as sheet metal properties. A word of caution though. It may become daunting to keep track of variables if there are substantial changes to the part/assembly files, so be weary of the connections between the notes and the File Properties.

With that being said, give it a try and hopefully you find this useful!

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Ben Crisostomo

Ben is a SOLIDWORKS Technical Support Application Expert based in the Javelin Oakville head office

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