Split Body 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)
        sketchCircles.addByCenterRadius(centerPoint, 5.0)
        
        # 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(True, distance)

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

        # Get the body created by the extrusion
        body = ext.bodies.item(0)
        
        # Create SplitBodyFeatureInput
        splitBodyFeats = rootComp.features.splitBodyFeatures
        splitBodyInput = splitBodyFeats.createInput(body, rootComp.xZConstructionPlane, True)
        
        # Create split body feature
        splitBodyFeats.add(splitBodyInput)
    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/Product.h>
#include <Core/Application/ValueInput.h>
#include <Core/Geometry/Point3D.h>
#include <Core/UserInterface/UserInterface.h>
#include <Fusion/BRep/BRepBodies.h>
#include <Fusion/BRep/BRepBody.h>
#include <Fusion/Components/Component.h>
#include <Fusion/Construction/ConstructionPlane.h>
#include <Fusion/Features/ExtrudeFeature.h>
#include <Fusion/Features/ExtrudeFeatureInput.h>
#include <Fusion/Features/ExtrudeFeatures.h>
#include <Fusion/Features/Features.h>
#include <Fusion/Features/SplitBodyFeatureInput.h>
#include <Fusion/Features/SplitBodyFeatures.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/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 sketch
    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<SketchCircles> sketchCircles = curves->sketchCircles();
    if (!sketchCircles)
        return false;

    Ptr<Point3D> centerPoint = adsk::core::Point3D::create(0, 0, 0);
    if (!centerPoint)
        return false;
    sketchCircles->addByCenterRadius(centerPoint, 5.0);

    // 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 the body created by the extrusion
    Ptr<BRepBodies> bodies = ext->bodies();
    if (!bodies)
        return false;

    Ptr<BRepBody> body = bodies->item(0);
    if (!body)
        return false;

    // Create SplitBodyFeatureInput
    Ptr<SplitBodyFeatures> splitBodyFeats = feats->splitBodyFeatures();
    if (!splitBodyFeats)
        return false;

    Ptr<SplitBodyFeatureInput> splitBodyInput =
        splitBodyFeats->createInput(body, rootComp->xZConstructionPlane(), true);
    if (!splitBodyInput)
        return false;

    // Create split body feature
    splitBodyFeats->add(splitBodyInput);

    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