using Variable

papawo

is it possible to make a text variable if a dimension of a part becomes diff?
ex. text1 = if the hole is 1" dia; 
      text2=if the hole is 2" dia

konstantin_shiriazdanov

there exist conditional expression syntax like condition?value_if_true:value_if_false
but now we have configurations so seems like defining several rows of config table for two parameters is a better approach

mahir

If you want to use the conditional route, then it would look something like this.

First, the hole diameter needs to be controlled or at least linked to a variable (#Hole_Dia).

Then, your #Hole_Text would be set to the following:
#Hole_Dia<10mm?"Small Hole":"Big Hole"

So if the hole is less than 10mm, the text would read "Small Hole". If it's equal to or larger than 10mm, the text will be "Large Hole".

papawo

can I put formula in configuration? 

konstantin_shiriazdanov

if i'm not mistaken currently there is no way to make something useful with text expressions, there are no features that can process it correctly and text fields of feature table beahve the same way so if you assign a result of text expression to variable and feed that variable to the feature like Surface text it wouldn't print the value of variable but just its name

mahir

But you could input the actual expression into an "Any" field of of a feature or FS, no?

konstantin_shiriazdanov

mahir said:

But you could input the actual expression into an "Any" field of of a feature or FS, no?

the problem is that field of "any" type only exists in variable defenition builtin feature, so you can't pass text expression to the geometry level of feature studio. several days ago i made a request to Dave Cowden for optional support of isAnything() predicate in his Surface text FS, and somewhere on the forum Ilya Baran posted a link to the rewrapped Surface text feature with support of isAnything

mahir

I don't pretend to know what goes on under the hood, but OS recently made some changes to isAnything that made my Parametric Curve FS work pretty well without workarounds. I thought expression parsing was standard now?

konstantin_shiriazdanov

mahir said:

I thought expression parsing was standard now?

it works good but currently there are no features that support text expression input. they all have input fields of string type, except one by Ilya

mahir

Ah, gotcha.

papawo

I am trying to control the part naming according to the variation of parts. i dont want to just name it . i want to have a check or formula that will name the part. anyone can tell me if its possible?

konstantin_shiriazdanov

found those feature by @ilya_baran it can take text expression as input
https://cad.onshape.com/documents/370197508187d5d8b361a414/w/64f8595ca2deaa8d5338db1a/e/fe4c2d2550f7c2d63b2704f9

papawo

not exactly what i want.

Jake_Rosenfeld

@Nan_Cp

You cannot currently change the name of the part in FeatureScript, but this is coming soon.  Stay tuned to the update announcements.

matthew_stacy

@ilya_baran thanks so much for that ST Surface Text (Expression-based) feature-script!  I was looking for something exactly like that, to allow users to configure a label on a part (shared document).  And thanks to @konstantin_shiriazdanov for providing the link (Jan. 2018).

The user community is a fantastic aspect of the Onshape platform. Seeing so many intelligent people generously sharing ideas restores my faith in humanity.

matthew_stacy

So the ST Surface Text (Expression-based) feature script works great for creating surface text from text variables.  Is there a way to do this with numeric variables?

This url is for a part with configuration variables for a text string and two dimensions (numeric).  I would like to generate surface text from the text string (√ done) AND generate more surface text to label the part with its dimensions (x & y).

https://cad.onshape.com/documents/b3dcf2a6219b73357ebe90aa/w/cf35b879f6907604941b3789/e/e61633325143361396de41b4

If there is a way to create surface text from numeric variables, it is then possible to concatenate a string from characters and numeric data (e.g. create the string "(100mm x 40mm)" based on the values of x & y?

Ideas?

ilya_baran

@matthew_stacy
It's doable, but it's a slightly tricky expression.  The string concatenation operator in FeatureScript is ~.  You also want to use the roundToPrecision function to avoid too many significant figures.  For the string you asked for, with 3 significant figures, you end up with something like this:
"(" ~ roundToPrecision(#x / mm, 3) ~ "mm x " ~ roundToPrecision(#y / mm, 3) ~ "mm)"

You can also debug intermediate subexpressions by assigning them to "any" type variables -- in other words, you can create a variable xString of type "any" with the expression
roundToPrecision(#x / mm, 3) ~ "mm"
and then use #xString and similarly #yString in the text field

Hope this helps.

matthew_stacy

Thanks for the syntax lesson @ilya_baran.  Greatly appreciated.

david_santopietro

@papawo, did you find a solution?

I reached out to Onshape support about same issue and they lead me to this: 

https://cad.onshape.com/documents/3a320c371e27789f9e7681bc/w/b639c9809964f0ef281ad6cf/e/ae295a8e774ff3beff1948e2

This kind of resolves the problem. Happy to discuss in more depth.