Using a for loop for multiple operations on multiple parts

Lee_Hesketh · September 2016

Hello, I have a script that makes a new sketch on a selected face, draw a rectangle, extrude and finally a Boolean subtraction. Currently it only works for one face at a time. How could I use a for loop to allow the operations to be done on all selected faces? This is for a mortise and tenon script I'm writing and when I tried to use a for loop an error was thrown concerning multiple operations with duplicate id names.
Any ideas?

Thanks
Lee Hesketh

owen_sparks · September 2016

Hi, there's a good explanation in the help files somewhere for this. I'm sure someone will be along with a full explanation soon but the solution is to append i to the feature ID within the loop to make each iteration unique.
Owen S.

cody_armstrong · September 2016

As @owen_sparks mentioned each feature/sketch needs to have a unique Id. An easy way to do this is to add "i" to you feature/sketch Id. Something similar to this...

<br>var sketchId = id + "sketch";
for (var i = 0; i < numberOfThings; i += 1) 
        {
            sketchId = sketchId + i;
            var sketch = newSketchOnPlane(context, sketchId, { "sketchPlane" : sketchPlane });
            //sketch some stuff here
        }

Notice "i" is incremented with each pass of the for loop so the "i + 1" you mentioned is not needed.

Jake_Rosenfeld · November 2017

@Lee_Hesketh

Your skRectange is failing because the second argument is not supposed to be an id, its just a string that uniquely identifies this part of the sketch. This is true in general for all "sk" operations. Sketch code should look something like:

const sketchId = id + "sketch";
var sketch = newSketchOnPlane(context, sketchId, {...});
skRectangle(sketch, "rectangle1", {...});
skRectangle(sketch, "rectangle2", {...});
skLineSegment(sketch, "lineSegment", {...});
skSolve(sketch);

Hope this helps,
Jake

owen_sparks · September 2016

Hi, there's a good explanation in the help files somewhere for this. I'm sure someone will be along with a full explanation soon but the solution is to append i to the feature ID within the loop to make each iteration unique.
Owen S.

Lee_Hesketh · September 2016

@owen_sparks How would I do this? Would it just be a case of say for an opExtrude be opExtrude(context, id + "extrude" + i)?
if I was using two extrudes, would the second one be opExtrude(context, id + "extrude" + i+1)?

Lee_Hesketh · September 2016

Here is the file so you can have a look.
https://cad.onshape.com/documents/57aee7f1e4b083f3982e60a4/w/720337d038a4a9744878f874/e/2059dc0192a94404a962ca5c

cody_armstrong · September 2016

As @owen_sparks mentioned each feature/sketch needs to have a unique Id. An easy way to do this is to add "i" to you feature/sketch Id. Something similar to this...

<br>var sketchId = id + "sketch";
for (var i = 0; i < numberOfThings; i += 1) 
        {
            sketchId = sketchId + i;
            var sketch = newSketchOnPlane(context, sketchId, { "sketchPlane" : sketchPlane });
            //sketch some stuff here
        }

Notice "i" is incremented with each pass of the for loop so the "i + 1" you mentioned is not needed.

Lee_Hesketh · September 2016

@cody_armstrong I tired that but when I was using skRectangle, it threw an error. Could you have a look at the whole script to see if you can see what's happening?

Image: https://us.v-cdn.net/5022071/uploads/editor/i9/smo49hz2ze6r.png

cody_armstrong · September 2016

@LeeH This is a different error than the duplicate Id error mentioned in the original post. The error states "Call skRectangle(Sketch,Id(array), map) does not match skRectangle(..." This error means it does not like something you have entered for the definition of your sketch rectangle.

I copied your Doc and was able to get "Mortise and Tenon Test" feature to work, so I cannot recreate the error. I would debug your inputs for the rectangle and make sure they are correct. My guess is one of your variables should be a string, but is instead an array. Or something similar.

Lee_Hesketh · September 2016

@cody_armstrong Did you edit it in any way because I can't get it to work. Also, I have rewritten the script but now the error is EXTRUDE_NO_SELECT_REGION. Could you have a look at feature studio1 and see if you can see what's going on?

ivan_skachko · November 2017

What if there are nested loops, such as two FOR loops one inside the other with loop counters i and j? How to increment ID in a unique way?

P.S. I found that using hash functions(see e.g. https://math.stackexchange.com/questions/531906/calculate-unique-integer-representing-a-pair-of-integers ), such as Cantor pairing function: id + 0.5*(i+j)*(i+j+1)+j works for low values of i, j, but then it becomes non-monotonic and the error "Parent Id FWDxIioBKfXZcAh_3.6 used at two non-contiguous points in operation history (Cannot have FWDxIioBKfXZcAh_3.10.2 between FWDxIioBKfXZcAh_3.6.1 and FWDxIioBKfXZcAh_3.6.0)" is thrown.

konstantin_shiriazdanov · November 2017

@ivan_skachko
a pair of i, j is unique inside the loop so the id should be something like id + ("sketch" ~ i ~ j). "~" is a string concatenation operator

Jake_Rosenfeld · November 2017

@Lee_Hesketh

Your skRectange is failing because the second argument is not supposed to be an id, its just a string that uniquely identifies this part of the sketch. This is true in general for all "sk" operations. Sketch code should look something like:

const sketchId = id + "sketch";
var sketch = newSketchOnPlane(context, sketchId, {...});
skRectangle(sketch, "rectangle1", {...});
skRectangle(sketch, "rectangle2", {...});
skLineSegment(sketch, "lineSegment", {...});
skSolve(sketch);

Hope this helps,
Jake

Jake_Rosenfeld · November 2017

Didn't realize the original post was from 2016 and there is a new question at hand.

@ivan_skachko @konstantin_shiriazdanov

Note that if there is a large loop with konstantin's solution, you could run into a bad situation where the ids are not unique. For example:

i = 1 j = 12
"sketch112"
i = 11 j = 2
"sketch112"

This can be mitigated with something like:

var sketchId = id + ("sketch." ~ i ~ "." ~ j);

"sketch.1.12"
"sketch.12.1"

or even:

var sketchId = id + unstableIdComponent(i) + unstableComponentId(j) + "sketch"

Note that code like:

for (increasing i)
{
    newSketch(context, id + "sketch" + unstableIdComponent(i), {...});
    opExtrude(context, id + "extrude" +  unstableIdComponent(i), {...});<br>    opDraft(context, id + "draft" + unstableIdComponent(i), {...});<br>}

will fail because of id hierarchy.

From the documentation (https://cad.onshape.com/FsDoc/library.html):

Image: https://us.v-cdn.net/5022071/uploads/editor/72/m8be92pd2qgx.png

konstantin_shiriazdanov · November 2017

Jake_Rosenfeld said:
Note that if there is a large loop with konstantin's solution, you could run into a bad situation where the ids are not unique.

thanks for pointing this, totally missed such situation

Using a for loop for multiple operations on multiple parts

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