This seems like it should be really easy but I can't find a nice way of doing it in Solidworks. All I want to do is add an equation driven value to sketch text so that I can have etched on a part what one of the dimensions is. I thought it would be possible using the 'insert file property' in the add text pane, but all this does is insert the text for the equation name whereas what I want is the actual evaluated value (e.g. '30' degrees as opposed to 'contact_angle...'). I tried changing the type of the file property to number but that didn't seem to work either. Does anyone have any ideas for how to do this? Example variable driven dimension I would like to use

file property linked to the equation value

Adding the linked file property to the text


1 Answer 1

  1. Create a Custom Property, and set the value to be equal to the Dimension you are interested in
  2. When editing the text, us the "link to properties" button, and select the property you created in step 1.

Demo Steps

Demo Video

  • $\begingroup$ Thanks for the reply Jonathan. I should have made it clearer in my question that these are the steps I've followed but I can't get it to behave as yours does (as it is supposed to...), it just pastes the actual text of the dimension (example shown in the image I posted in the question) - is there something I'm missing? $\endgroup$ Sep 7, 2022 at 14:25
  • $\begingroup$ I'll need way more screenshots to diagnose - can you make a screen recording showing you setting this up in a brand new part? $\endgroup$ Sep 7, 2022 at 15:54
  • $\begingroup$ I couldn't figure out how to add a screen recording but I've editted the original question to have pictures of the file properties dialogue and the text box inserting it if that illustrates it? The screen capture is from a new part as well. $\endgroup$ Sep 7, 2022 at 17:31
  • $\begingroup$ I've investigated - it don't understand why, but when the custom property points at a global variable, it doesn't seem to show the evaluated value... The workaround for this, is to point the custom property to a dimension instead - I'm assuming you've used the "length" global variable to drive a dimension somewhere, but if not, you can add a dummy sketch with a single line just for this purpose. $\endgroup$ Sep 12, 2022 at 9:54
  • $\begingroup$ Ah, Solidworks is strange sometimes, this will save me so much time - thank you for investigating! $\endgroup$ Sep 19, 2022 at 10:37

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