Variable Extrude

jack_white396

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

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

@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

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

@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?

MichaelPascoe

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

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

@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