Save time by linking Notes and Features to Custom Properties in SOLIDWORKS

Article by John Lee, CSWE updated June 30, 2020

Article

Why should you link notes and features to custom properties in SOLIDWORKS? Well have you ever needed to add a stamp to a SOLIDWORKS part to call out the same info that is already in your custom properties?  Ever needed to call that out on the drawing too?

What if you had to keep replicating custom property information into stamps and callouts, hundreds or even thousands of times over the years?  Yuck!  How tedious!  Not only is that duplicating work by entering the same information THREE TIMES per part, but it can grow to be so tiresome that likely many of us would rather eat a few kilograms of raw kale than keep doing that.  Instead, there is a way to enter the information just once, to populate the custom properties, and then leverage that by using library features and library notes for the other two times those properties are used.

How to link a Custom Property to a Note

Fortunately, the function to link those properties into sketches and notes was added, by popular demand, into SOLIDWORKS 2016 (for 2015 and prior year versions, check out this macro solution for some of this functionality).  This article, applicable to SOLIDWORKS 2016 and later versions, should save you considerable time, by showing you how to create a part and annotation as Library Features that you can simply drag onto the part and onto the drawing view to instantly create the stamp and the callout, AND pull from Custom Property values of the part so the note populates with those values.  Here is how:

  1. Set the SOLIDWORKS Custom Properties in the part.

    SOLIDWORKS Custom Properties

    Will this still need to be done every time in future?  Yes!

  2. Create a Cut-Extrude or Split Line feature to make the stamp, linking custom properties to the sketch text.  If assembly performance is a concern due to the graphics triangles needed to model 3D text, then consider using Split Line to model the stamp as 2D text.

    Link PartNo and Revision into the Sketch Text for the stamp

    Link PartNo and Revision into the Sketch Text for the stamp

  3. Add the stamp feature to the Design Library by dragging it from the feature tree on the left into the folder of your choice in the Design Library in the right taskpane.  This will convert the part into a Library Feature Part, so be sure to save your project file beforehand.

    Drag the feature from the tree into the Design Library

    Drag the feature from the tree into the Design Library

  4. The Add to Library manager will launch automatically in the left taskpane.  Complete it to save the new Library Feature.

    Add to Library

    Add to Library

  5. In the drawing, add a callout, linking to the same custom properties.  Select the properties from Model found here >  Current drawing view, or alternately choose component to which the annotation is attached.

    PartNo and Revision are linked into the note

    In this example, PartNo and Revision are linked into the note

  6. Add the note to the Design Library by copying it from drawing view with Ctrl+C and pasting with Ctrl+V into the folder of your choice in the Design Library in the right taskpane.  Once again the Add to Library manager will open in the left taskpane.  Complete it and select OK.
Paste into the Design Library

Copy the note from the view and paste it into the Design Library

To ensure that your custom library feature parts survive various upgrades to newer SOLIDWORKS year versions, consider placing them in a folder that won’t get deleted during the upgrade.  You can then add that file location in the Design Library right taskpane.

That’s it!  Modeling that stamp and typing that callout is now a thing of the past!  It’s so last year!  It’s for the birds!  It’s old hat, as they used to say.

Summary of the New Process

For future parts, simply do this:

  1. In the part, populate the custom properties
  2. In the part, simply drag the stamp feature from the Design Library to the part face, and it should automatically add the stamp feature and populate it with the custom properties.
  3. In the drawing, simply drag the callout note from the Design Library onto the part face, and it should automatically populate the callout note with the custom properties from the model.
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John Lee, CSWE

John Lee is inherently lazy in that he prefers to work smarter - not harder. A CSWE with fifteen years of experience using SOLIDWORKS and a background in mechanical design, John has used SOLIDWORKS in various industries requiring design for injection molding, sheet metal, weldments and structural steel.