Linking SolidWorks Drawing Notes to Model Properties

Often times you will want to have notes in your drawings linked to custom properties in the part/assembly the drawing represents. But did you know there are actually multiple different variables you can use in the notes to link to the model?

If you use the variable $PRPSHEET:”Custom Property” the note will be linked to whatever model is in the view called out in the sheet properties (See image below).


So for a drawing with sheet properties shown above, a note that has $PRPSHEET:”DESCRIPTION” will show the “description” custom property for whatever model is in Drawing View 1. You will notice when using the $PRPSHEET: variable is used the note does not have to be attached to any view. Making it an ideal variable to use for notes located in the Title Block. On the other hand if you would like a note that is directly attached to a view you would use the variable $PRPVIEW:”Custom Property”. $PRPVIEW: pulls in the custom properties of whatever model is in the view. For example, in the image below, there is a note attached to an assembly with the value of $PRPVIEW:”DESCRIPTION”. Notice how the note is not directly connected to any particular part in the assembly but just the assembly as a whole.


Now what if you would like to pull in a custom property of an individual component in the assembly model? Then you would use the $PRPMODEL:”Custom Property” variable. So in the example below the note has the value of $PRPMODEL:”DESCRIPTION” and is directly attached to the component in the assembly.


Next blog post I will cover how EPDM interacts with custom properties and how to link a model data card to a drawing data card.