FS generated sketch to be accessible in Asseblies

MakotoNinja
MakotoNinja Member Posts: 6 EDU
in FeatureScript
Aloha All,

I am trying to write a FS that generates a sketch that is accessible from within Assemblies. What I am seeing is that a feature is generated with the sketch I have devised but this "sketch" isn't available to insert into an Assembly. Is there a way to create a sketch in FS that shows up as an actual sketch instead of a feature?
The first feature in the following image shows the sketch as generated by FS and the second feature in the list is a vanilla sketch created with the sketch button. Only the latter is available to insert into an Assembly.

I am new to FS but not new at programming. My code is as follows:
FeatureScript 1993;
import(path : "onshape/std/common.fs", version : "1993.0");

const BOUNDS = {(unitless) : [10, 100, 1e5]} as IntegerBoundSpec;

annotation { "Feature Type Name" : "Axes" }
export const axes = defineFeature(function(context is Context, id is Id, definition is map)
precondition
{
    // Define the parameters of the feature type
    annotation
    {
        "Name" : "Sketch Plane",
        "Filter" : EntityType.FACE,
        "MaxNumberOfPicks" : 1
    }
    definition.sketchPlane is Query;
    
    annotation
    {
        "Name" : "Diameter",
        "UIHint" : [UIHint.SHOW_LABEL, UIHint.REMEMBER_PREVIOUS_VALUE],
        "Description" : "Set the diameter of the circle"
    }
    // isLength(definition.radius, LENGTH_BOUNDS);
    isInteger(definition.diameter, BOUNDS);
}
{
    var diameter = definition.diameter;
    var splane = definition.sketchPlane;
    
    // Define the function's action
    var sketch1 = newSketch(context, id + "sketch1", {
        "sketchPlane" : splane
    });
    skCircle(sketch1, "circle1", {
        "center" : vector(0, 0) * millimeter,
        "radius" : (diameter / 2) * millimeter,
        "construction" : true
    });
    skLineSegment(sketch1, "line1", {
        "start" : vector(-diameter / 2, 0) * millimeter,
        "end" : vector(diameter / 2, 0) * millimeter,
        "construction" : true
    });
    skLineSegment(sketch1, "line2", {
        "start" : vector(0, diameter / 2) * millimeter,
        "end" : vector(0, -diameter / 2) * millimeter,
        "construction" : true
    });
    skSolve(sketch1);
});

Tagged:

Comments

  • TillysInteriors
    TillysInteriors Member Posts: 12 PRO

    I'd like this too. Is there an improvement request?

  • Scott_Boeberitz
    Scott_Boeberitz Member Posts: 14 PRO
    edited October 20

    I just checked to confirm that FS generated sketch edges can be included in composite parts. So I threw an extra few lines onto your script to wrap the sketch into a new composite part. This part can be put into an assembly.

    image.png image.png

    EDIT: forgot to add the changed code:

    FeatureScript 1993;
import(path : "onshape/std/common.fs", version : "1993.0");

const BOUNDS = {(unitless) : [10, 100, 1e5]} as IntegerBoundSpec;

annotation { "Feature Type Name" : "Axes" }
export const axes = defineFeature(function(context is Context, id is Id, definition is map)
    precondition
    {
        // Define the parameters of the feature type
        annotation
        {
            "Name" : "Sketch Plane",
            "Filter" : EntityType.FACE,
            "MaxNumberOfPicks" : 1
        }
        definition.sketchPlane is Query;

        annotation
        {
            "Name" : "Diameter",
            "UIHint" : [UIHint.SHOW_LABEL, UIHint.REMEMBER_PREVIOUS_VALUE],
            "Description" : "Set the diameter of the circle"
        }
        // isLength(definition.radius, LENGTH_BOUNDS);
        isInteger(definition.diameter, BOUNDS);
    }
    {
        var diameter = definition.diameter;
        var splane = definition.sketchPlane;

        // Define the function's action
        var sketch1 = newSketch(context, id + "sketch1", {
                "sketchPlane" : splane
            });
        skCircle(sketch1, "circle1", {
                    "center" : vector(0, 0) * millimeter,
                    "radius" : (diameter / 2) * millimeter,
                    "construction" : true
                });
        skLineSegment(sketch1, "line1", {
                    "start" : vector(-diameter / 2, 0) * millimeter,
                    "end" : vector(diameter / 2, 0) * millimeter,
                    "construction" : true
                });
        skLineSegment(sketch1, "line2", {
                    "start" : vector(0, diameter / 2) * millimeter,
                    "end" : vector(0, -diameter / 2) * millimeter,
                    "construction" : true
                });
        skSolve(sketch1);

        // Composite parts can't contain sketch bodies, so copy each sketch edge
        // into a standalone wire body first. Edges are extracted one at a time
        // because opExtractWires fails when edges cross or 3+ meet at a point
        // (the lines cross at the center and touch the circle at their ends).
        for (var entityId in ["circle1", "line1", "line2"])
        {
            opExtractWires(context, id + "wires" + entityId, {
                        "edges" : sketchEntityQuery(id + "sketch1", EntityType.EDGE, entityId)
                    });
        }

        opCreateCompositePart(context, id + "compositePart", {
                    "bodies" : qCreatedBy(id + "wires", EntityType.BODY),
                    "closed" : true
                });
    });

Categories