A few expression tips.

lougallo

Over the last couple of months we have received a number of questions on how to make expressions in the Onshape dimension and feature dialogs and I wanted to share a few of them with you all.  You can read about most of them in our help documentation here: Numeric fields

As illustrated in our help you can do most math functions: 

</code>+, -, *, /, ^, ceil, floor, round, exp, sqrt, abs, max, min, log, log10</pre>A few examples:<br><pre class="CodeBlock"><code>ceil(5.667) = 6
floor(5.667) = 5

but we also support a array/lookup table like this: (remember the array starts at 0) . (Array example)

[3,5,6,7][2] = 6
[3,5,6,7][3] = 7

and ternary operators which can yield conditional results.  For example let's say I want the #length of my rectangle to be 7in if the width is > 5in, otherwise make it 4in. (Ternary example)

#width>5?7:4

Note: In the example file I am also making the hole fail if the #width is less than 4in.

I thought this might be useful and I will try to get some examples added to our help as well.  ~Lou

emagdalenaC2i

Great!!! I did'nt know about the conditional

Awesome

john_mcclary

sweet! also didn't know about the inline if statement!

owen_sparks

Very good indeed thanks for making it clear.

Cheers, Owen S.

brian_brady

You can also nest conditionals by placing another complete conditional statement in either the true or false positions. I suggest using parentheses around the second statement (may even be necessary) for readability.

&nbsp;#width<4?1:(#width>4?3:2)

This example sets the value to 1 if width is less than 4, 2 if equal to 4, and 3 if greater than 4

brucebartlett

@jackson_king this could be really handy

brian_brady

brucebartlett said:

@jackson_king this could be really handy

This is how I used it while trying to use Feature Script. I wanted to use variables to drive a simple woodruff key, then figure out how to do the same thing with Feature Script. I haven't taken much time since to learn more though.

https://cad.onshape.com/documents/d84339a898f6048107f919e7/w/6bf19a60af5f77fc35b79e73/e/c14681bd9486c363d1cd88a6

papawo

You said: In the example file I am also making the hole fail if the #width is less than 4in.

Fail means the browser will turn red and will have error msg that it didnt regenerate properly?
Is it okay if we just leave it red?Just a question?

Jake_Rosenfeld

@Nan_Cp , Yes it's fine if you leave a feature in a failing state.  Because it's red, all of its effects have been rolled back, and it has no affect on the final geometry.

Marc_Miller

Red makes me nervous, haha.  :P 

Nested conditional statements are cool!  Thanks @lougallo and @brian_brady for the tips.

papawo

It does make me nervous!    
Thanks Jake.

owen_sparks

Marc_Miller said:

Red makes me nervous, haha.  :P

Maybe we could have purple for "not wrong, but resolves to nothing"...

Owen S.

john_mcclary

Isn't that the same thing?

owen_sparks

john_mcclary said:

Isn't that the same thing?

Noo.  Say we want extra holes in our widget if the length is over a certain value, and we use a pattern feature for the extra holes.  If our widget is under the limit the extra holes value will be zero, as is our intent.  Currently the feature will be red.  In ideal-land we could have a soothing purple to indicate our feature is not producing an output, but is not in error.   #FirstWorldProblems

john_mcclary

Ah i see what you're sayin

john_mcclary

You mean like when solidworks throws a warning where there is nothing wrong?...

owen_sparks

Yes indeed, or when WIN10 states that it can't restart because this (empty) list of applications is preventing it!

Will_Schleter

In one of the examples, a hole_diameter of -1 is used to try and make the hole fail and not be displayed, however, when I copied the file to play with it a hole_diameter variable of -1 used in a dimension on a sketch resulted in a circle of diameter 1 (looks like it used absolute value) The only way I could get it to fail was set the variable to 0.

Alex_Pitt

#variableName*2 (multiplication) works for me but #variableName-2 (subtraction) doesn't work (I get the "enter valid expression" error)


Unless I enter the units...

tim_hess427

@Alex_Pitt - Those examples are working correctly per the way they're designed. Onshape doesn't "assume" it knows what unit to use, but it always checks units to keep the dimensions accurate. 

So, 10mm*2 = 20mm. Using dimensional analysis, onshape knows that the result should have a length unit. 

However, 10mm - 2 does not work because onshape doesn't make assumptions and doesn't know what the units for the result should be. Is it 2 inches? 2 feet? 2mm? 

Alex_Pitt

It's no problem to type in the units. At the time I had incorrectly assumed that when no units were specified, it would use the default document units. (mm in this case). 

tim_hess427

I think it does make that assumption if you're just typing a single value, but once you start getting into more complex expressions things need to be more explicit.

karel_works

https://forum.onshape.com/discussion/comment/31417#Comment_31417

This is magic, thanks