Applying Linked Properties to Drawing Sheet Formats

Automation of your SOLIDWORKS drawings is one of the biggest time savers in the software. Manually entering values for model properties, such as Weight, is not only time consuming but prone to human error. This information already exists within your part file so why not have SOLIDWORKS fill it in for you?

drawing sheet

SOLIDWORKS allows to you to link properties into the drawing border so all of these fields will automatically populate. In this example, we will look at adding a property of ‘Weight’ from the part shown in the drawing.

You can do this by:

  • Creating a dummy part file
  • Setting up the ‘Weight’ property field at part level
  • Creating a new drawing with the dummy part
  • Adding a note to the drawing that links to the new ‘Weight’ property
  • Saving the edited sheet format

Step 1) Create a new part.  You need to have the property ‘Weight’ set up at the part level. To do this go to ‘File > Properties’ and click on the ‘Custom’ tab. From here, use the drop down list and select the ‘Weight’ property.  Next drop down ‘Value / Text Expression’ and link this to the mass of the part:


Here you can add other properties to the part file, e.g. Material. Once complete you will need to save the part template to keep these properties in all new parts created. ‘File > Save As’ then change the ‘Save as type’ to ‘Part template’. The default file location for templates is C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2016\templates.

Step 2) Create a dummy part in this new template (for example a rectangular block) and save.

Step 3) Create a new drawing of this dummy part (insert at least one view of the part). Edit the sheet format ‘Edit > Sheet format’ and add a new note where you want the weight to display ‘Insert > Annotations > Note’

Step 4) In the Note property manager on the left hand side of the screen, click the icon that shows the property symbol with a chain link ‘Link to Property’:


Step 5) In the Link to Property dialog, change the option to ‘Model found here’ so that it will look at the part model properties rather than the drawing file properties. Use the drop down ‘Property name’ to select the ‘Weight’ property that we added to the part earlier:



You should now see the weight of the dummy part display in the note you have just added.

Step 6) Exit the sheet format using the icon in the top right of the screen:


Step 7)  Save the edited sheet format, ‘File > Save sheet format’ to save these changes.

Once saved, test the template by creating a new drawing, and adding a part with a weight property assigned.


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