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 two new components under root component allOccs = rootComp.occurrences transform = adsk.core.Matrix3D.create() subOcc0 = allOccs.addNewComponent(transform) # Create sketch 1 in sub component 1 subComp0 = subOcc0.component sketches0 = subComp0.sketches sketch0 = sketches0.add(subComp0.xZConstructionPlane) sketchCircles0 = sketch0.sketchCurves.sketchCircles centerPoint = adsk.core.Point3D.create(0, 0, 0) sketchCircles0.addByCenterRadius(centerPoint, 2.5) # Get the profile defined by the circle prof0 = sketch0.profiles.item(0) # Create an extrude input and make sure it's in the new component extrudes0 = subComp0.features.extrudeFeatures extInput0 = extrudes0.createInput(prof0, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) # Set the extrude input distance0 = adsk.core.ValueInput.createByString("5 mm") extInput0.setDistanceExtent(False, distance0) extInput0.isSolid = True # Create the extrude extrude0 = extrudes0.add(extInput0) # Get the end face of the created extrude endFaceOfExtrude0 = extrude0.endFaces.item(0) # Create a construction plane for extrude 2 constructionPlanes_ = subComp0.constructionPlanes constructionPlaneInput = constructionPlanes_.createInput() constructionPlaneInput.setByOffset(endFaceOfExtrude0, adsk.core.ValueInput.createByString("20 mm")) constructionPlane = constructionPlanes_.add(constructionPlaneInput) constructionPlaneProxy = constructionPlane.createForAssemblyContext(subOcc0) # Create sketch 2 in sub component 2 subOcc1 = allOccs.addNewComponent(transform) subComp1 = subOcc1.component sketches1 = subComp1.sketches sketch1 = sketches1.add(constructionPlaneProxy) sketchCircles1 = sketch1.sketchCurves.sketchCircles sketchCircles1.addByCenterRadius(centerPoint, 0.5) # Get the profile defined by the circle prof1 = sketch1.profiles.item(0) # Create an extrude input and make sure it's in the new component extrudes1 = subComp1.features.extrudeFeatures extInput1 = extrudes1.createInput(prof1, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) # Set the extrude input distance1 = adsk.core.ValueInput.createByString("50 mm") extInput1.setDistanceExtent(False, distance1) extInput1.isSolid = False # Create the extrude extrudes1.add(extInput1) # Create the AsBuiltJointInput asBuiltJoints_ = rootComp.asBuiltJoints asBuiltJointInput = asBuiltJoints_.createInput(subOcc0, subOcc1, None) # Create the AsBuiltJoint asBuiltJoints_.add(asBuiltJointInput) 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/ValueInput.h> #include <Core/Application/Viewport.h> #include <Core/Application/Camera.h> #include <Core/Geometry/Point3D.h> #include <Core/Geometry/Matrix3D.h> #include <Core/UserInterface/UserInterface.h> #include <Fusion/Fusion/Design.h> #include <Fusion/BRep/BRepFace.h> #include <Fusion/BRep/BRepFaces.h> #include <Fusion/Construction/ConstructionPlanes.h> #include <Fusion/Construction/ConstructionPlaneInput.h> #include <Fusion/Construction/ConstructionPlane.h> #include <Fusion/Components/Component.h> #include <Fusion/Components/AsBuiltJoints.h> #include <Fusion/Components/AsBuiltJointInput.h> #include <Fusion/Components/AsBuiltJoint.h> #include <Fusion/Components/Occurrence.h> #include <Fusion/Components/Occurrences.h> #include <Fusion/Features/Features.h> #include <Fusion/Features/ExtrudeFeature.h> #include <Fusion/Features/ExtrudeFeatures.h> #include <Fusion/Features/ExtrudeFeatureInput.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 sub component 1 under root component Ptr<Occurrences> occs = rootComp->occurrences(); if (!occs) return false; Ptr<Matrix3D> transform = adsk::core::Matrix3D::create(); if (!transform) return false; Ptr<Occurrence> subOcc0 = occs->addNewComponent(transform); if (!subOcc0) return false; // Create sketch 1 in sub component 1 Ptr<Component> subComp0 = subOcc0->component(); if (!subComp0) return false; Ptr<Sketches> sketches0 = subComp0->sketches(); if (!sketches0) return false; Ptr<ConstructionPlane> xzPlane = rootComp->xZConstructionPlane(); if (!xzPlane) return false; Ptr<Sketch> sketch0 = sketches0->add(xzPlane); if (!sketch0) return false; Ptr<SketchCurves> sketchCurves0 = sketch0->sketchCurves(); if (!sketchCurves0) return false; Ptr<SketchCircles> sketchCircles0 = sketchCurves0->sketchCircles(); if (!sketchCircles0) return false; Ptr<Point3D> centerPoint = Point3D::create(0, 0, 0); if (!centerPoint) return false; Ptr<SketchCircle> sketchCircle0 = sketchCircles0->addByCenterRadius(centerPoint, 2.5); if (!sketchCircle0) return false; // Get the profile defined by the circle Ptr<Profiles> profs0 = sketch0->profiles(); if (!profs0) return false; Ptr<Profile> profile0 = profs0->item(0); if (!profile0) return false; // Create an extrude input Ptr<Features> feats0 = subComp0->features(); if (!feats0) return false; Ptr<ExtrudeFeatures> extrudes0 = feats0->extrudeFeatures(); if (!extrudes0) return false; Ptr<ExtrudeFeatureInput> extInput0 = extrudes0->createInput(profile0, FeatureOperations::NewBodyFeatureOperation); if (!extInput0) return false; // Set the extrude input Ptr<ValueInput> distance0 = ValueInput::createByString("5 mm"); if (!distance0) return false; extInput0->setDistanceExtent(false, distance0); extInput0->isSolid(true); // Create the extrude Ptr<ExtrudeFeature> ext = extrudes0->add(extInput0); if (!ext) return false; // Get the end face of the created extrude Ptr<BRepFaces> endFaces = ext->endFaces(); if (!endFaces) return false; Ptr<BRepFace> endFace = endFaces->item(0); if (!endFace) return false; // Create a construction plane for extrude 2 Ptr<ConstructionPlanes> ctorPlanes = subComp0->constructionPlanes(); if (!ctorPlanes) return false; Ptr<ConstructionPlaneInput> ctorPlaneInput = ctorPlanes->createInput(); if (!ctorPlaneInput) return false; ctorPlaneInput->setByOffset(endFace, adsk::core::ValueInput::createByString("20 mm")); Ptr<ConstructionPlane> ctorPlane = ctorPlanes->add(ctorPlaneInput); if (!ctorPlane) return false; Ptr<ConstructionPlane> ctorPlaneProxy = ctorPlane->createForAssemblyContext(subOcc0); if (!ctorPlaneProxy) return false; // Create sub component 2 under root component Ptr<Occurrence> subOcc1 = occs->addNewComponent(transform); if (!subOcc1) return false; // Create sketch 2 in sub component 2 Ptr<Component> subComp1 = subOcc1->component(); if (!subComp1) return false; Ptr<Sketches> sketches1 = subComp1->sketches(); if (!sketches1) return false; Ptr<Sketch> sketch1 = sketches1->add(ctorPlaneProxy); if (!sketch1) return false; Ptr<SketchCurves> sketchCurves1 = sketch1->sketchCurves(); if (!sketchCurves1) return false; Ptr<SketchCircles> sketchCircles1 = sketchCurves1->sketchCircles(); if (!sketchCircles1) return false; Ptr<SketchCircle> sketchCircle1 = sketchCircles1->addByCenterRadius(centerPoint, 0.5); if (!sketchCircle1) return false; // Get the profile defined by the circle Ptr<Profiles> profs1 = sketch1->profiles(); if (!profs1) return false; Ptr<Profile> profile1 = profs1->item(0); if (!profile1) return false; // Create an extrude input Ptr<Features> feats1 = subComp1->features(); if (!feats1) return false; Ptr<ExtrudeFeatures> extrudes1 = feats1->extrudeFeatures(); if (!extrudes1) return false; Ptr<ExtrudeFeatureInput> extInput1 = extrudes1->createInput(profile1, FeatureOperations::NewBodyFeatureOperation); if (!extInput1) return false; // Set the extrude input Ptr<ValueInput> distance1 = ValueInput::createByString("50 mm"); if (!distance1) return false; extInput1->setDistanceExtent(false, distance1); extInput1->isSolid(false); // Create the extrude Ptr<ExtrudeFeature> extrude1 = extrudes1->add(extInput1); if (!extrude1) return false; // Create the AsBuiltJoint Ptr<AsBuiltJoints> asBuiltJoints_ = rootComp->asBuiltJoints(); if (!asBuiltJoints_) return false; Ptr<AsBuiltJointInput> asBuiltJointInput = asBuiltJoints_->createInput(subOcc0, subOcc1, nullptr); if (!asBuiltJointInput) return false; Ptr<AsBuiltJoint> asBuiltJoint = asBuiltJoints_->add(asBuiltJointInput); if (!asBuiltJoint) return false; // Fit to window Ptr<Viewport> viewPort = app->activeViewport(); if (!viewPort) return false; Ptr<Camera> cam = viewPort->camera(); if (!cam) return false; cam->isFitView(true); viewPort->camera(cam); 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