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Extruding in for loop

josh_crowsonjosh_crowson Member Posts: 7 EDU
edited March 2017 in FeatureScript
I am working on a mortise and tendon joint in feature script.  I know there is already one that exists, but it does not do exactly what I want.  This also pushes me to finally learn FS.  
FeatureScript 543;
import(path : "onshape/std/geometry.fs", version : "543.0");

annotation { "Feature Type Name" : "MortisetAndTennon" }
export const MortisetAndTennon = defineFeature(function(context is Context, id is Id, definition is map)
    precondition
    {
    annotation { "Name" : "tennon faces", "Filter" : EntityType.FACE, "MaxNumberOfPicks" : 100 }
    definition.tennonFaces is Query;
    // annotation { "Name" : "slot faces", "Filter" : EntityType.FACE, "MaxNumberOfPicks" : 100 }
    // definition.slotFaces is Query;
    
    
    }
    {
    var count = 0;
    const facesList = evaluateQuery(context, definition.tennonFaces);
    for (var face in facesList)
    {
        count = count + 1; 
        const plane = evPlane(context, { "face" : face});
        debug(context, plane);
        const sk = newSketchOnPlane(context, id + "sk" + toString(count), {"sketchPlane" : plane});
        skRectangle(sk, "rectangle1", { "firstCorner" : vector(0, 3) * inch, "secondCorner" : vector(1, 5) * inch });
        debug(context, sk);
        skSolve(sk);
        
        opExtrude(context, id + "extrude" + toString(count), {
                "entities" : qSketchRegion(id + "sk" + toString(count), true),
                "direction" : plane.normal,
                "endBound" : BoundingType.BLIND,
                "endDepth" : 1 * inch
        });
    }
    
    });



When I run the feature, Onshape says "Invalid state at the end of execution"  and "@skSolve: Parent Id F41vOgQIuzuAHks_2.sk used at two non-contiguous points in operation history (Cannot have F41vOgQIuzuAHks_2.extrude.1 between F41vOgQIuzuAHks_2.sk.1 and F41vOgQIuzuAHks_2.sk.2)".
It works though when I only select one face or if I comment out the extrude.  

Best Answer

Answers

  • kevin_o_toole_1kevin_o_toole_1 Onshape Employees, Developers, HDM Posts: 552
    edited March 2017
    Welcome!

    For the error, check out the documentation for Ids here. You'll want to set the extrude's id to either id + count + "extrude", or id + ("extrude" ~ count)

    To get the corners of the sketch, you can query for e.g. sketchEntityQuery(id + "sketch1", EntityType.VERTEX, "rectangle1.left.start")
  • josh_crowsonjosh_crowson Member Posts: 7 EDU
    edited March 2017
    Thank you for the quick response.  Your comments helped with the extruding issue.  

  • MacColtelliMacColtelli Member Posts: 2
    Hello @ilya_baran
    I was trying to delete the multiple sketches and extrusions that I created in my for loop. When I used the "extrude" + i format I was able to query all iterations using qCreatedBy( id + "extrude") However, when I used your proposed version the for loop works which is great! but the query I showed fails to return anything. How do you suppose I query the bodies created by the iterations of my for loop?
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 4,508
    @MacColtelli probably best to have a "parent" id then make all sketches and extrudes children of that such as id + "loop" + ("sketch" ~ i) and id + "loop" + ("extrude" ~ i) then you can query id + "loop" to get everything. 
    Director, Technical Services, EMEA
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