Stitch 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)
        
        design = app.activeProduct

        # Get the root component of the active design.
        rootComp = design.rootComponent
        
        # Create two sketch lines on the xz plane.
        sketches = rootComp.sketches
        sketch = sketches.add(rootComp.xZConstructionPlane)
        sketchLines = sketch.sketchCurves.sketchLines
        startPoint = adsk.core.Point3D.create(0, 0, 0)
        endPoint = adsk.core.Point3D.create(1, 0, 0)
        sketchLine = sketchLines.addByTwoPoints(startPoint, endPoint)
        endPoint2 = adsk.core.Point3D.create(0, 1, 0)
        sketchLine2 = sketchLines.addByTwoPoints(startPoint, endPoint2)
        
        # Create surface one with ExtrudeFeature.
        features = rootComp.features
        extrudeFeatures = features.extrudeFeatures
        openProfile = rootComp.createOpenProfile(sketchLine)
        extrudeFeatureInput = extrudeFeatures.createInput(openProfile, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        extrudeFeatureInput.isSolid = False
        extrudeFeatureInput.setDistanceExtent(False, adsk.core.ValueInput.createByReal(1.0))
        extrudeFeature = extrudeFeatures.add(extrudeFeatureInput)
        
        # Create surface two with ExtrudeFeature.
        openProfile2 = rootComp.createOpenProfile(sketchLine2)        
        extrudeFeatureInput2 = extrudeFeatures.createInput(openProfile2, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        extrudeFeatureInput2.isSolid = False
        extrudeFeatureInput2.setDistanceExtent(False, adsk.core.ValueInput.createByReal(1.0))
        extrudeFeature2 = extrudeFeatures.add(extrudeFeatureInput2)
        
        # Get surface bodies and add them to object collection.
        surface = extrudeFeature.bodies.item(0)
        surface2 = extrudeFeature2.bodies.item(0)
        surfaces = adsk.core.ObjectCollection.create()
        surfaces.add(surface)
        surfaces.add(surface2)
        
        # Define tolerance with 1 cm.
        tolerance = adsk.core.ValueInput.createByReal(1.0)
        
        # Create a stitch input to be able to define the input needed for an stitch.
        stitches = features.stitchFeatures
        stitchInput = stitches.createInput(surfaces, tolerance, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        
        # Create a stitch feature.
        stitch = stitches.add(stitchInput)
    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/Product.h>
#include <Core/Application/ObjectCollection.h>
#include <Core/Application/ValueInput.h>
#include <Core/Geometry/Point3D.h>
#include <Fusion/Fusion/Design.h>
#include <Fusion/Components/Component.h>
#include <Fusion/Construction/ConstructionPlane.h>
#include <Fusion/BRep/BRepBodies.h>
#include <Fusion/BRep/BRepBody.h>
#include <Fusion/Features/Features.h>
#include <Fusion/Features/ExtrudeFeature.h>
#include <Fusion/Features/ExtrudeFeatures.h>
#include <Fusion/Features/ExtrudeFeatureInput.h>
#include <Fusion/Features/StitchFeatures.h>
#include <Fusion/Features/StitchFeatureInput.h>
#include <Fusion/Features/StitchFeature.h>
#include <Fusion/Sketch/Sketch.h>
#include <Fusion/Sketch/Sketches.h>
#include <Fusion/Sketch/SketchCurves.h>
#include <Fusion/Sketch/SketchLines.h>
#include <Fusion/Sketch/SketchLine.h>
#include <Fusion/Sketch/Profile.h>
#include <Fusion/Sketch/Profiles.h>
// startTest
#include "../../../TestUtils.h"
// endTest

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 circle on the xz plane.
    Ptr<Sketches> sketches = rootComp->sketches();
    if (!sketches)
        return false;
    Ptr<Sketch> sketch = sketches->add(rootComp->xZConstructionPlane());
    if (!sketch)
        return false;
    Ptr<SketchCurves> sketchCurves = sketch->sketchCurves();
    if (!sketchCurves)
        return false;
    Ptr<SketchLines> sketchLines = sketchCurves->sketchLines();
    if (!sketchLines)
        return false;
    Ptr<Point3D> startPoint = Point3D::create(0, 0, 0);
    Ptr<Point3D> endPoint = Point3D::create(1.0, 0, 0);
    Ptr<SketchLine> sketchLine = sketchLines->addByTwoPoints(startPoint, endPoint);
    Ptr<Point3D> endPoint2 = Point3D::create(0, 1.0, 0);
    Ptr<SketchLine> sketchLine2 = sketchLines->addByTwoPoints(startPoint, endPoint2);

    // Create a open profile.
    Ptr<Profile> openProfile = rootComp->createOpenProfile(sketchLine);
    Ptr<Profile> openProfile2 = rootComp->createOpenProfile(sketchLine2);

    // Create an extrusion input.
    Ptr<Features> features = rootComp->features();
    if (!features)
        return false;
    Ptr<ExtrudeFeatures> extrudes = features->extrudeFeatures();
    if (!extrudes)
        return false;
    Ptr<ExtrudeFeatureInput> extrudeInput =
        extrudes->createInput(openProfile, FeatureOperations::NewBodyFeatureOperation);
    if (!extrudeInput)
        return false;
    extrudeInput->isSolid(false);
    Ptr<ExtrudeFeatureInput> extrudeInput2 =
        extrudes->createInput(openProfile2, FeatureOperations::NewBodyFeatureOperation);
    if (!extrudeInput2)
        return false;
    extrudeInput2->isSolid(false);

    // Define the extent.
    Ptr<ValueInput> distance = ValueInput::createByReal(1.0);
    extrudeInput->setDistanceExtent(false, distance);
    extrudeInput2->setDistanceExtent(false, distance);

    // Create the extrusion.
    Ptr<ExtrudeFeature> extrude = extrudes->add(extrudeInput);
    if (!extrude)
        return false;
    Ptr<ExtrudeFeature> extrude2 = extrudes->add(extrudeInput2);
    if (!extrude2)
        return false;
    Ptr<BRepBodies> bodies = extrude->bodies();
    if (!bodies)
        return false;
    Ptr<BRepBody> body = bodies->item(0);
    Ptr<BRepBodies> bodies2 = extrude2->bodies();
    if (!bodies2)
        return false;
    Ptr<BRepBody> body2 = bodies2->item(0);
    Ptr<ObjectCollection> surfaces = ObjectCollection::create();
    if (!surfaces)
        return false;
    surfaces->add(body);
    surfaces->add(body2);

    // Define tolerance with 1 cm.
    Ptr<ValueInput> tolerance = ValueInput::createByReal(1.0);

    // Create a stitch input to be able to define the input needed for an stitch.
    Ptr<StitchFeatures> stitches = features->stitchFeatures();
    if (!stitches)
        return false;
    Ptr<StitchFeatureInput> stitchInput =
        stitches->createInput(surfaces, tolerance, FeatureOperations::NewBodyFeatureOperation);

    // Create a stitch feature.
    stitches->add(stitchInput);

    // startTest
    doc->close(false);
    // endTest

    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