Split Face 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 a sketch that has a rectangle in it
        sketches = rootComp.sketches
        sketch = sketches.add(rootComp.xZConstructionPlane)
        sketchLines = sketch.sketchCurves.sketchLines
        point0 = adsk.core.Point3D.create(0, 0, 0)
        point1 = adsk.core.Point3D.create(10, 10, 0)
        sketchLines.addTwoPointRectangle(point0, point1)
        
        # Get the profile defined by the rectangle
        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(True, distance)

        # Create the extrusion
        ext = extrudes.add(extInput)

        # Get one edge of the extrusion body
        face = ext.endFaces.item(0)
        edge = face.edges.item(0)
        
        # Create a slant construction plane with an angle of 45 deg on the xZConstructionPlane
        planeInput = rootComp.constructionPlanes.createInput()
        planeInput.setByAngle(edge, adsk.core.ValueInput.createByString('45 deg'), rootComp.xZConstructionPlane)
        plane = rootComp.constructionPlanes.add(planeInput)
        
        # Create another sketch containing a circle profile on the slant plane
        toolSketch = sketches.add(plane)
        point3 = adsk.core.Point3D.create(-5, 3.5, 0)
        sketchCircles = toolSketch.sketchCurves.sketchCircles
        circle = sketchCircles.addByCenterRadius(point3, 3)
        
        # Get SplitFaceFetures
        splitFaceFeats = rootComp.features.splitFaceFeatures
        
        # Set faces to split
        facesCol = adsk.core.ObjectCollection.create()
        facesCol.add(face)
        
        # Create a split face feature of surface intersection split type
        splitFaceInput = splitFaceFeats.createInput(facesCol, circle, True)
        split = splitFaceFeats.add(splitFaceInput)
        split.deleteMe()
        
        # Create another split face feature of closest point split type   
        splitFaceInput.setClosestPointSplitType()
        split = splitFaceFeats.add(splitFaceInput)
        split.deleteMe()
        
        # Create another split face feature of along vector split type   
        splitFaceInput.setAlongVectorSplitType(face.edges.item(1))
        splitFaceFeats.add(splitFaceInput)
        
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

#include <Core/Application/Application.h>
#include <Core/Application/Document.h>
#include <Core/Application/Documents.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/BRep/BRepEdge.h>
#include <Fusion/BRep/BRepEdges.h>
#include <Fusion/Components/Component.h>
#include <Fusion/Construction/ConstructionPlane.h>
#include <Fusion/Construction/ConstructionPlanes.h>
#include <Fusion/Construction/ConstructionPlaneInput.h>
#include <Fusion/Features/ExtrudeFeature.h>
#include <Fusion/Features/ExtrudeFeatureInput.h>
#include <Fusion/Features/ExtrudeFeatures.h>
#include <Fusion/Features/Features.h>
#include <Fusion/Features/SplitFaceFeatureInput.h>
#include <Fusion/Features/SplitFaceFeatures.h>
#include <Fusion/Features/SplitFaceFeature.h>
#include <Fusion/Fusion/Design.h>
#include <Fusion/Sketch/Profile.h>
#include <Fusion/Sketch/Profiles.h>
#include <Fusion/Sketch/Sketch.h>
#include <Fusion/Sketch/SketchCircles.h>
#include <Fusion/Sketch/SketchCircle.h>
#include <Fusion/Sketch/SketchLines.h>
#include <Fusion/Sketch/SketchCurves.h>
#include <Fusion/Sketch/Sketches.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> docs = app->documents();
    if (!docs)
        return false;

    // Create a document.
    Ptr<Document> doc = docs->add(DocumentTypes::FusionDesignDocumentType);
    if (!doc)
        return false;

    Ptr<Design> design = app->activeProduct();
    if (!design)
        return false;

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

    // Create a sketch that has a rectangle in it
    Ptr<Sketches> sketches = rootComp->sketches();
    if (!sketches)
        return false;

    Ptr<Sketch> sketch = sketches->add(rootComp->xZConstructionPlane());
    if (!sketch)
        return false;

    Ptr<SketchCurves> curves = sketch->sketchCurves();
    if (!curves)
        return false;

    Ptr<SketchLines> sketchLines = curves->sketchLines();
    if (!sketchLines)
        return false;

    Ptr<Point3D> point0 = adsk::core::Point3D::create(0, 0, 0);
    if (!point0)
        return false;
    Ptr<Point3D> point1 = adsk::core::Point3D::create(10, 10, 0);
    if (!point1)
        return false;

    sketchLines->addTwoPointRectangle(point0, point1);

    // 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(true, distance);

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

    // Get one edge of the extrusion body
    Ptr<BRepFaces> faces = ext->endFaces();
    if (!faces)
        return false;
    Ptr<BRepFace> face = faces->item(0);
    if (!face)
        return false;
    Ptr<BRepEdges> edges = face->edges();
    if (!edges)
        return false;
    Ptr<BRepEdge> edge = edges->item(0);
    if (!edge)
        return false;

    // Create a slant construction plane with an angle of 45 deg on the xZConstructionPlane
    Ptr<ConstructionPlanes> planes = rootComp->constructionPlanes();
    if (!planes)
        return false;

    Ptr<ConstructionPlaneInput> planeInput = planes->createInput();
    if (!planeInput)
        return false;
    planeInput->setByAngle(edge, adsk::core::ValueInput::createByString("45 deg"), rootComp->xZConstructionPlane());
    Ptr<ConstructionPlane> plane = planes->add(planeInput);

    // Create another sketch containing a circle profile on the slant plane
    Ptr<Sketch> toolSketch = sketches->add(plane);
    if (!toolSketch)
        return false;
    Ptr<SketchCurves> toolCurves = toolSketch->sketchCurves();
    if (!toolCurves)
        return false;
    Ptr<SketchCircles> sketchCircles = toolCurves->sketchCircles();
    if (!sketchCircles)
        return false;
    Ptr<SketchCircle> circle = sketchCircles->addByCenterRadius(point0, 5.0);
    if (!circle)
        return false;

    // Get SplitFaceFetures
    Ptr<SplitFaceFeatures> splitFaceFeats = feats->splitFaceFeatures();
    if (!splitFaceFeats)
        return false;

    // Set faces to split
    Ptr<ObjectCollection> facesCol = ObjectCollection::create();
    if (!facesCol)
        return false;
    facesCol->add(face);

    // Create Create a split face feature of surface intersection split type
    Ptr<SplitFaceFeatureInput> splitFaceInput = splitFaceFeats->createInput(facesCol, circle, true);
    if (!splitFaceInput)
        return false;
    Ptr<SplitFaceFeature> split = splitFaceFeats->add(splitFaceInput);
    if (!split)
        return false;
    split->deleteMe();

    // Create another split face feature of closest point split type
    splitFaceInput->setClosestPointSplitType();
    split = splitFaceFeats->add(splitFaceInput);
    if (!split)
        return false;
    split->deleteMe();

    // Create another split face feature of along vector split type
    Ptr<BRepEdge> dirEdge = edges->item(1);
    if (!dirEdge)
        return false;
    splitFaceInput->setAlongVectorSplitType(dirEdge);
    splitFaceFeats->add(splitFaceInput);

    return true;
}

#ifdef XI_WIN

#include <windows.h>

BOOL APIENTRY DllMain(HMODULE hmodule, DWORD reason, LPVOID reserved)
{
    switch (reason)
    {
    case DLL_PROCESS_ATTACH:
    case DLL_THREAD_ATTACH:
    case DLL_THREAD_DETACH:
    case DLL_PROCESS_DETACH:
        break;
    }
    return TRUE;
}

#endif // XI_WIN