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Using Variables in text

mark_morgenmark_morgen Member Posts: 12 ✭
in Community Support
I could not get text to work at all with a #variable.  I tried for over an hour, but nothing worked.  My goal is to emboss a text string that includes a single dimension of the part onto a face, such as "Cube Height is #Height inches".  It only works as a simple text string, but I want to update the text automatically when the dimension is changed in the drawing.
I used Onshape instructions, but they failed me...

Thank you!

Answers

  • Matt_ShieldsMatt_Shields Member, Onshape Employees Posts: 938 PRO
    edited July 2024
    It isn't obvious, but you can right-click in the text box and select "Convert to expression."  But you're not done there.  If you put in #height, Onshape won't like it.  You'll want something like 
    "Cube Height is " ~ toString(#height/in) ~ " inches"

  • mark_morgenmark_morgen Member Posts: 12 ✭
    I got the value to display using toString, but it's not updating the text when the #height variable changes with drawing changes
  • Matt_ShieldsMatt_Shields Member, Onshape Employees Posts: 938 PRO
    make sure the #height variable is above the text sketch in the Features list.
  • _anton_anton Member, Onshape Employees Posts: 525 image
    Working fine for me. Are you committing your text dialog and your sketch? Can you share your document? I'm only aware of one bug in this functionality, which shouldn't be relevant unless you're working with feature patterns.
  • mark_morgenmark_morgen Member Posts: 12 ✭

    I don't know what _anton means by "committing your text dialog and your sketch".

    The text in question is the last variable in the Features List called #TextForSpoolFace, which followed by Plane 2, where the text is defined in Sketch "Face Cutout Shapes".
    When editing the text, and I convert between text and expression, the expression toString(#TextForSpoolFace) is lost as soon as it's converted to text.  Changing the first parameter in the Features List, #SpoolMinBtwnFaces, will change the value for #TextForSpoolFace.  I tried a few workarounds to simplify the expression used in the text editing box, but nothing has worked.

    Thank you for your help with this.  It's been frustrating!

    As long as we're here, where can I find the list of functions like Round, toString, etc.?
  • Matt_ShieldsMatt_Shields Member, Onshape Employees Posts: 938 PRO
    Anton means clicking the green check box. 

    Don't convert it back to text.  Leave it as an expression.  And, since your variable is just a number, 

    toString(#TextForSpoolFace)

    is sufficient.

    I don't know if all of the FeatureScript math functions will work in a text box, but here is a good list of math functions:
    https://cad.onshape.com/FsDoc/library.html#module-math.fs
  • mark_morgenmark_morgen Member Posts: 12 ✭
    if I leave it as an expression (on the expression line, right justified), the text in my sketch shows up as the expression, not the value of the expression.  So the text will display "toString(#TextForSpoolFace)", not "21.5"
  • mark_morgenmark_morgen Member Posts: 12 ✭
    Well, it's working now.  I can't say that I did anything different than before.  The text box now shows the correct value using the toString command... which is what I've been trying all along.
    Thank you for drudging through this with me!
  • Alan_GuthrieAlan_Guthrie Member Posts: 8 ✭

    Had this same issue but it wasn't working for me until I concatenated with an empty text string. Then it started working as intended, even after I deleted the empty text string. ¯\_(ツ)_/¯

    image.png
  • dbaardadbaarda Member Posts: 25 ✭✭

    Explaining why things did/didn't work for particular values of text;

    • If you didn't right-click the text box and convert it into an expression, then it's just a string that doesn't get evaluated.
    • "#height" - doesn't expand the var because you have quotes around it which means "#height" is the string.
    • #height - gives an error because the #height var it uses as the string is not a string, it's a length with a dimension (probably mm).
    • toString(#height)- works because toString() converts the length into a string.
    • roundToPrecision(#Shorten/mm,1)- gives an error because this expression returns a number without a dimension, not a string. It doesn't have a dimension because #Shorten/mm removes the mm dimension.
    • roundToPrecision(#Shorten/mm,1) ~ "" works because the ~ string-concatenation operator converts both sides into strings before joining them if they are not strings.

    The only other thing to be wary of is Sketch Text expressions don't get re-evaluated in feature-patterns with `Reapply features` selected. This is a very old bug that is still not fixed (2026-02-26). This means you cannot use text expressions to dynamicaly generate different text for different feature-pattern-instances by updating var's in the feature-pattern. I think the only workaround is use third-party featurescript extensions.

  • dbaardadbaarda Member Posts: 25 ✭✭

    For the record, I found another workaround for getting text expressions re-evaluated in feature-patterns; instantiate a "derived" sketch with a configuration-variable for the text input. Exact steps are;

    1. Create a new empty part studio.
    2. In the part studio, create a string configuration variable called something like "text".
    3. Create a sketch with nothing in it but the text-block, set the text to "#text" and right-click to convert it to an expression.
    4. In the other part-studio where you want to have varying text in a feature-pattern, add a "Derived" instance, selecting the partstudio and sketch with the text.
    5. For the "text" configuration parameter type in whatever expression you want for the text that needs to be re-evaluated for each feature-pattern instance.
    6. right-click this string to convert it to an expression (you have no idea how long it took me to discover this was also right-click-convertable).
    7. This then gives you a sketch with the text you can extrude/subtract/whatever with.
    8. Create your feature-pattern, selecting everything you want to pattern, including the Derived sketch and extrusions that use it, ticking "reapply features"
    9. viola! you have a pattern with text from an expression that is re-evaluated with each pattern-instance.

    You can also add extra configuration variables for other attributes of the text like size, angle, etc, which can also be set using expressions when you Derive the sketch instance. Note most configuration arguments are expressions by default, and only string config args default to "text" and need to be right-click-converted into expressions.

    One thing that might bite you using this technique; you cannot instantiate multiple instances into the same part studio with the same configuration. This means you will probably get errors if the configuration argument expressions evaluate to the same values for any of your part-pattern-instances.

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