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How to Link a Property in a Note of a Drawing in SOLIDWORKS

This guide provides step-by-step instructions to link both custom properties and model properties to notes in a SOLIDWORKS drawing.

Linking properties to notes in a SOLIDWORKS drawing is an efficient way to automate the display of part, assembly, or drawing metadata, such as material, part number, description, or revision. This ensures consistency, reduces manual entry errors, and keeps your documentation dynamically updated as properties

 

Creating a Linked Note Through the PropertyManager

  1. Add the properties to your drawing file, or the part/assembly that will be on the drawing, through File > Properties.
  2. In the Drawing, select the Note command on the Annotation tab of the CommandManager and place the note on the drawing.
  3. In the PropertyMangaer, select the Link to Property command, which is the icon that appears like the properties dialog window with a chain link.

  4. Select either Current document or Model found here.
    1. Current document: Pulls from the File Properties of the drawing file.
    2. Model found here: Pulls from the File Properties of the part/assembly file shown on the drawing file.
  5. Click on the Property name dropdown and select from the available properties.

  6. Select OK.

 

TIP: If you do not see any properties in the Property name dropdown, confirm that the properties are already populated in the drawing file or the part/assembly referenced on the drawing sheet.

 

Creating a Linked Note Manually with $PRP and $PRPSHEET

  1. Add the properties to your drawing file, or the part/assembly that will be on the drawing, through File > Properties.
  2. In the Drawing, select the Note command on the Annotation tab of the CommandManager and place the note on the drawing.
  3. Type the note as follows, where custom_property will be exchanged with the value in the Property Name column of the File Properties:
    1. $PRP:"custom_property"
    2. $PRPSHEET:"custom_property"

 

NOTE: $PRP will pull properties from the drawing file and $PRPSHEET will pull properties from the part/assembly model referenced on the drawing sheet.

For example, if I had an assembly with a property called Material, and I wanted that dynamically linked to the drawing for that assembly, I would add a note with the following format:

$PRPSHEET:"Material"