Variable Extrude

jack_white396 · May 2022

I am trying the vary which direction I do an extrude based on where there is material. Essentially, this feature will take a point and make a specific hole pattern and extrude them, but if the point is on the opposite side of an object the feature does not work since there is nothing to be subtracted. I need to somehow be able to vary which direction I extrude based on where the point I select is in relation to the object I want extruded through. Here is my code- https://cad.onshape.com/documents/dd9b41942bbf9f447e9d9d6d/w/2b64a0a98ab7927062949adf/e/d176417788ab53093aeccb69

MichaelPascoe · May 2022

Hi @jack_white396, welcome to FeatureScript!

Try something like this:

This will measure the z distance of the point with respect to the plane. If the point is in the opposite direction of the plane, the distance will be a negative value.

const distance = worldToPlane3D(planey, point[2]);

A vector is an array, if you ever need the other values of the vector:

const x = point[0];
const y = point[1];
const z = point[2];

jack_white396 · May 2022

@MichaelPascoe thanks for that advice but what if my plane and point is not in the z direction? As if how do I tell whether I need to use the x, y, or z distances?

MichaelPascoe · May 2022

I usually measure normal to the plane I'm using, z. This is the local z of the plane, not the global Z of the studio. Can you describe your goal a little more? You may need more inputs, something that you can extract a plane from.

jack_white396 · May 2022

@MichaelPascoe In this example, the point right in the middle of the circle is the point I want. however, the distance between this point and the face of the sphere is along the x axis, not the z. How do I get it to measure the correct way no matter which way the body is oriented?

Image: https://us.v-cdn.net/5022071/uploads/editor/nu/253czr1gajah.png

MichaelPascoe · May 2022

If the cylinder will always be in the part studio, you can have the input be a cylindrical face. One click, I will show you if that is what you want, but I'm still a little confused. What is the feature expected to do? Is there always only a cylinder, or will there be other shapes and conditions?

jack_white396 · May 2022

The cylinder is just an object to test on. I am a member of an frc robotics team, and we often have to design parts to hold bearings in them. The idea of this feature is that the user can select a center point and then the bearing hole and three holes around it for rivets to hold the bearing in would automatically be made in the part.

MichaelPascoe · May 2022

@jack_white396
Try using an implicit mate connector. If you need to measure the distance instead of a manual entry, you can use the above technique that I mentioned and measure from the startPlane.

Code:

FeatureScript 1746;
import(path : "onshape/std/geometry.fs", version : "1746.0");

annotation { "Feature Type Name" : "Bearing mount" }
export const bearingMount = defineFeature(function(context is Context, id is Id, definition is map)
    precondition
    {       
       annotation { "Name" : "Start location", "Filter" : BodyType.MATE_CONNECTOR || BodyType.MATE_CONNECTOR, "MaxNumberOfPicks" : 1 }
       definition.mate is Query; 
       
       annotation { "Name" : "Distance" }
       isLength(definition.distance, LENGTH_BOUNDS);
    }
    {
        
    const startCsys = evMateConnector(context, {
            "mateConnector" : definition.mate
    });
    
    const startPlane = plane(startCsys);
    const point = startPlane.origin;
    
    const cent = worldToPlane(startPlane, point);
    const addition1 = vector(0, .690625) * inch;
    const addition2 = vector(((0.690625/2)*sqrt(3)), (-1*(0.690625/2))) * inch;
    const addition3 = vector((-1*((0.690625/2)*sqrt(3))), (-1*(0.690625/2))) * inch;
    const cent2 = (cent+addition1);
    const cent3 = (cent+addition2);
    const cent4 = (cent+addition3);
    
    const sketch1 = newSketchOnPlane(context, id + "sketch1", {
            "sketchPlane" : startPlane
    });
    skCircle(sketch1, "circle1", {
            "center" : cent,
            "radius" : (1.125/2) * inch
    });
    skCircle(sketch1, "circle2", {
            "center" : cent2,
            "radius" : (5/64) * inch
    });
        skCircle(sketch1, "circle3", {
            "center" : cent3,
            "radius" : (5/64) * inch
    });
        skCircle(sketch1, "circle4", {
            "center" : cent4,
            "radius" : (5/64) * inch
    });
    
    skSolve(sketch1);
    
    extrude(context, id + "extrude1", {
            "entities" : qSketchRegion(id + "sketch1"),
            "endBound" : BoundingType.BLIND,
            "depth" : definition.distance,
            "oppositeDirection" : true,
            "operationType" : NewBodyOperationType.REMOVE,
            "booleanScope" : qAllNonMeshSolidBodies(),
    });
    
    // opExtrude(context, id + "extrude1", {
    //         "entities" : qSketchRegion(id + "sketch1"),
    //         "direction" : -planey.normal,
    //         "endBound" : BoundingType.THROUGH_ALL,
    // });
    });

https://cad.onshape.com/documents/321704cdfedd9bd658ec2def/w/7ed9842c4e5b566356122040/e/29a0ec328e10902c13fd7099?renderMode=0&uiState=62750ae856487c0b606403ca

Variable Extrude

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