Link a Note to a Feature Dimension in SOLIDWORKS!

Link a Note to a Feature Dimension in SOLIDWORKS!
Posted in: Mechanical Design
September 21, 2016
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A question that often gets asked in Support is how a designer is able to link a note to a dimension of a feature, and that’s what we’ll take a look at today! As a designer, changes are constantly being made to the part and ECO’s (Engineering Change Orders) issued. By being able to link a note to a part feature dimension, it’s one less thing for designer to have to remember to change!

To start it off, we’re going to create a block that has a Length of 6 inches, Width of 7 inches, and Height of 8 inches. We can reference other dimensions with respect to another, which allows for the update process to be even faster. For example, if we wanted the width of my cube (7 inches) to be controlling the height (8 inches) and length (6 inches), we can double click on the ‘Height’ dimension to open the ‘Modify’ dialog box, click “=”, click on the ‘7.000’ inch dimension to represent the width, and then type “+1”. This will yield me an equation that says the ‘Height = Width + 1’. Creating an equation is not required to link a note to a dimension, but just for this example, I wanted to show it since it follows a similar workflow as we’ll see later on! We can repeat the process for the length, where I have it always equal to the “width (7 inches) – 1” to give me 6 inches.

Once we have the part squared away, we can create a drawing with all front and top views, and insert the dimensions using ‘Model Items’. To create a note with the Length, Width, and Height dimensions, we’ll create a note that reads ‘Length x Width x Height’, type “=”, and click the “6.000” inch dimension for the Length, “7.000” inch for the Width, and the “8.000” inch dimension for the Height. That’s it!

To verify this was done correctly, we’ll want to hover over the note itself to reveal the syntax. Your syntax won’t be the exact same as below because it’s dependent on the features and name of the part; regardless, it should display something along the lines of “Length x Width x Height = “D1@NameOfFeature@NameOfPart@DrawingViewName...” Here’s an example of the syntax for the cube we’ve been working with:

Once it’s completed, we want to make sure to test it out! We can double click on the ‘7.000’ inch dimension in the Front Drawing view to “8.000” inches, and we should see the ‘Length’ and ‘Height’ adjust both in the drawings views as well as the note!

This opens up a whole world of notes that have intelligence to them; not only can you include dimensions, but custom properties like Material or Configuration Names can be added too. In conclusion, the benefit lies in the fact that when dimensions change (sometimes more often than we’d like them to!) we don’t have to worry about the note that references it and instead, trust it gets updated, thanks to SOLIDWORKS!

September 21, 2016
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Evan Jensen
May 13, 2022
Is it possible to insert an equation into the referential note. For example, I'd like the note to automatically calculate and display the volume of the above shape. Thanks in advance!

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