Hole Feature API Sample

import adsk.core, adsk.fusion, traceback

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui = app.userInterface
        
        # Create a document.
        doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)
 
        product = app.activeProduct
        design = adsk.fusion.Design.cast(product)

        # Get the root component of the active design.
        rootComp = design.rootComponent
        
        # Create sketch
        sketches = rootComp.sketches
        sketch = sketches.add(rootComp.xZConstructionPlane)
        sketchCircles = sketch.sketchCurves.sketchCircles
        centerPoint = adsk.core.Point3D.create(0, 0, 0)
        circle = sketchCircles.addByCenterRadius(centerPoint, 3.0)
        
        # Get the profile defined by the circle.
        prof = sketch.profiles.item(0)

        # Create an extrusion input
        extrudes = rootComp.features.extrudeFeatures
        extInput = extrudes.createInput(prof, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        
        # Define that the extent is a distance extent of 5 cm.
        distance = adsk.core.ValueInput.createByReal(5)
        extInput.setDistanceExtent(False, distance)

        # Create the extrusion.
        ext = extrudes.add(extInput)
        
        # Get the end face of the extrusion
        endFaces = ext.endFaces
        endFace = endFaces.item(0)
        
        # Create a construction plane by offsetting the end face
        planes = rootComp.constructionPlanes
        planeInput = planes.createInput()
        offsetVal = adsk.core.ValueInput.createByString('2 cm')
        planeInput.setByOffset(endFace, offsetVal)
        offsetPlane = planes.add(planeInput)
        
        # Create a sketch on the new construction plane and add four sketch points on it
        offsetSketch = sketches.add(offsetPlane)
        offsetSketchPoints = offsetSketch.sketchPoints
        sPt0 = offsetSketchPoints.add(adsk.core.Point3D.create(1, 0, 0))
        sPt1 = offsetSketchPoints.add(adsk.core.Point3D.create(0, 1, 0))
        sPt2 = offsetSketchPoints.add(adsk.core.Point3D.create(-1, 0, 0))
        sPt3 = offsetSketchPoints.add(adsk.core.Point3D.create(0, -1, 0))
        
        # Add the four sketch points into a collection
        ptColl = adsk.core.ObjectCollection.create()
        ptColl.add(sPt0)
        ptColl.add(sPt1)
        ptColl.add(sPt2)
        ptColl.add(sPt3)
        
        # Create a hole input
        holes = rootComp.features.holeFeatures
        holeInput = holes.createSimpleInput(adsk.core.ValueInput.createByString('2 mm'))
        holeInput.setPositionBySketchPoints(ptColl)
        holeInput.setDistanceExtent(distance)
        
        hole = holes.add(holeInput)
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

#include <Core/Application/Application.h>
#include <Core/Application/Documents.h>
#include <Core/Application/Document.h>
#include <Core/Application/ObjectCollection.h>
#include <Core/Application/Product.h>
#include <Core/Application/ValueInput.h>
#include <Core/Geometry/Point3D.h>
#include <Core/UserInterface/UserInterface.h>
#include <Fusion/BRep/BRepFace.h>
#include <Fusion/BRep/BRepFaces.h>
#include <Fusion/Components/Component.h>
#include <Fusion/Construction/ConstructionPlane.h>
#include <Fusion/Construction/ConstructionPlanes.h>
#include <Fusion/Construction/ConstructionPlaneInput.h>
#include <Fusion/Features/Features.h>
#include <Fusion/Features/ExtrudeFeature.h>
#include <Fusion/Features/ExtrudeFeatures.h>
#include <Fusion/Features/ExtrudeFeatureInput.h>
#include <Fusion/Features/HoleFeature.h>
#include <Fusion/Features/HoleFeatures.h>
#include <Fusion/Features/HoleFeatureInput.h>
#include <Fusion/Fusion/Design.h>
#include <Fusion/Sketch/Profile.h>
#include <Fusion/Sketch/Profiles.h>
#include <Fusion/Sketch/Sketch.h>
#include <Fusion/Sketch/Sketches.h>
#include <Fusion/Sketch/SketchCircle.h>
#include <Fusion/Sketch/SketchCircles.h>
#include <Fusion/Sketch/SketchCurves.h>
#include <Fusion/Sketch/SketchPoint.h>
#include <Fusion/Sketch/SketchPoints.h>

using namespace adsk::core;
using namespace adsk::fusion;

Ptr<UserInterface> ui;

extern "C" XI_EXPORT bool run(const char* context)
{
    Ptr<Application> app = Application::get();
    if (!app)
        return false;

    ui = app->userInterface();
    if (!ui)
        return false;

    Ptr<Documents> documents = app->documents();
    if (!documents)
        return false;

    Ptr<Document> doc = documents->add(DocumentTypes::FusionDesignDocumentType);
    if (!doc)
        return false;

    Ptr<Product> product = app->activeProduct();
    if (!product)
        return false;

    Ptr<Design> design = product;
    if (!design)
        return false;

    // Get the root component of the active design
    Ptr<Component> rootComp = design->rootComponent();
    if (!rootComp)
        return false;

    // Create sketch
    Ptr<Sketches> sketches = rootComp->sketches();
    if (!sketches)
        return false;
    Ptr<ConstructionPlane> xz = rootComp->xZConstructionPlane();
    if (!xz)
        return false;
    Ptr<Sketch> sketch = sketches->add(xz);
    if (!sketch)
        return false;
    Ptr<SketchCurves> sketchCurves = sketch->sketchCurves();
    if (!sketchCurves)
        return false;
    Ptr<SketchCircles> sketchCircles = sketchCurves->sketchCircles();
    if (!sketchCircles)
        return false;
    Ptr<Point3D> centerPoint = Point3D::create(0, 0, 0);
    if (!centerPoint)
        return false;
    Ptr<SketchCircle> circle = sketchCircles->addByCenterRadius(centerPoint, 3.0);
    if (!circle)
        return false;

    // Get the profile defined by the circle.
    Ptr<Profiles> profs = sketch->profiles();
    if (!profs)
        return false;
    Ptr<Profile> prof = profs->item(0);
    if (!prof)
        return false;

    // Create an extrusion input
    Ptr<Features> feats = rootComp->features();
    if (!feats)
        return false;
    Ptr<ExtrudeFeatures> extrudes = feats->extrudeFeatures();
    if (!extrudes)
        return false;
    Ptr<ExtrudeFeatureInput> extInput = extrudes->createInput(prof, FeatureOperations::NewBodyFeatureOperation);
    if (!extInput)
        return false;

    // Define that the extent is a distance extent of 5 cm.
    Ptr<ValueInput> distance = ValueInput::createByReal(5);
    if (!distance)
        return false;
    extInput->setDistanceExtent(false, distance);

    // Create the extrusion.
    Ptr<ExtrudeFeature> ext = extrudes->add(extInput);
    if (!ext)
        return false;

    // Get the end face of the extrusion
    Ptr<BRepFaces> endFaces = ext->endFaces();
    if (!endFaces)
        return false;
    Ptr<BRepFace> endFace = endFaces->item(0);
    if (!endFace)
        return false;

    // Create a construction plane by offsetting the end face
    Ptr<ConstructionPlanes> planes = rootComp->constructionPlanes();
    if (!planes)
        return false;
    Ptr<ConstructionPlaneInput> planeInput = planes->createInput();
    if (!planeInput)
        return false;
    Ptr<ValueInput> offsetVal = ValueInput::createByString("2 cm");
    if (!offsetVal)
        return false;
    planeInput->setByOffset(endFace, offsetVal);
    Ptr<ConstructionPlane> offsetPlane = planes->add(planeInput);
    if (!offsetPlane)
        return false;

    // Create a sketch on the new construction plane and add four sketch points on it
    Ptr<Sketch> offsetSketch = sketches->add(offsetPlane);
    if (!offsetSketch)
        return false;
    Ptr<SketchPoints> offsetSketchPoints = offsetSketch->sketchPoints();
    if (!offsetSketchPoints)
        return false;
    Ptr<Point3D> p0 = Point3D::create(1, 0, 0);
    if (!p0)
        return false;
    Ptr<SketchPoint> sPt0 = offsetSketchPoints->add(p0);
    if (!sPt0)
        return false;
    Ptr<Point3D> p1 = Point3D::create(0, 1, 0);
    if (!p1)
        return false;
    Ptr<SketchPoint> sPt1 = offsetSketchPoints->add(p1);
    if (!sPt1)
        return false;
    Ptr<Point3D> p2 = Point3D::create(-1, 0, 0);
    if (!p2)
        return false;
    Ptr<SketchPoint> sPt2 = offsetSketchPoints->add(p2);
    if (!sPt2)
        return false;
    Ptr<Point3D> p3 = Point3D::create(0, -1, 0);
    if (!p3)
        return false;
    Ptr<SketchPoint> sPt3 = offsetSketchPoints->add(p3);
    if (!sPt3)
        return false;

    // Add the four sketch points into a collection
    Ptr<ObjectCollection> ptColl = ObjectCollection::create();
    if (!ptColl)
        return false;
    ptColl->add(sPt0);
    ptColl->add(sPt1);
    ptColl->add(sPt2);
    ptColl->add(sPt3);

    // Create a hole input
    Ptr<HoleFeatures> holes = feats->holeFeatures();
    if (!holes)
        return false;
    Ptr<HoleFeatureInput> holeInput = holes->createSimpleInput(ValueInput::createByString("2 mm"));
    if (!holeInput)
        return false;
    holeInput->setPositionBySketchPoints(ptColl);
    holeInput->setDistanceExtent(distance);

    Ptr<HoleFeature> hole = holes->add(holeInput);
    if (!hole)
        return false;

    return true;
}