Demonstrates creating a joint with cylindrical joint motion.
Before running: No open document is required; the script creates a new design (or additional documents) as it runs.
#Author- #Description- 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 in root component sketches = rootComp.sketches sketch = sketches.add(rootComp.xZConstructionPlane) sketchPts = sketch.sketchPoints point = adsk.core.Point3D.create(1, 0, 1) sketchPt = sketchPts.add(point) sketchLines = sketch.sketchCurves.sketchLines point1 = adsk.core.Point3D.create(1, 0, 2) point2 = adsk.core.Point3D.create(2, 0, 1) point1SketchSpace = sketch.modelToSketchSpace(point1) point2SketchSpace = sketch.modelToSketchSpace(point2) lines = sketchLines.addTwoPointRectangle(point1SketchSpace, point2SketchSpace) # Get the profile defined by the circle prof = sketch.profiles.item(0) # Create an extrusion input and make sure it's in a new component extrudes = rootComp.features.extrudeFeatures extInput = extrudes.createInput(prof, adsk.fusion.FeatureOperations.NewComponentFeatureOperation) # Set the extrusion input distance = adsk.core.ValueInput.createByReal(5) extInput.setDistanceExtent(True, distance) extInput.isSolid = True # Create the extrusion ext = extrudes.add(extInput) # Get the end face of the created extrusion body endFace = ext.endFaces.item(0) # Get the occurrence of the new component occ = rootComp.occurrences.item(0) # Create a new sketch in the occurrence sketchInOcc = sketches.add(endFace, occ) # Get the sketch curve projected to the sketch curve = sketchInOcc.sketchCurves.item(0) # Create the first joint geometry with the sketch curve geo0 = adsk.fusion.JointGeometry.createByCurve(curve, adsk.fusion.JointKeyPointTypes.StartKeyPoint) # Create the second joint geometry with sketch point geo1 = adsk.fusion.JointGeometry.createByPoint(sketchPt) # Create joint input joints = rootComp.joints jointInput = joints.createInput(geo0, geo1) # Set the joint input jointInput.setAsCylindricalJointMotion(adsk.fusion.JointDirections.CustomJointDirection, curve.createForAssemblyContext(occ)) # Create the joint joint = joints.add(jointInput) cylindricalMotion = joint.jointMotion rotLimits = cylindricalMotion.rotationLimits rotLimits.isRestValueEnabled = True rotLimits.restValue = 3.14 / 3 slideLimits = cylindricalMotion.slideLimits slideLimits.isMinimumValueEnabled = True slideLimits.minimumValue = 0.1 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/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/Components/Joint.h>
#include <Fusion/Components/JointGeometry.h>
#include <Fusion/Components/JointInput.h>
#include <Fusion/Components/JointLimits.h>
#include <Fusion/Components/Joints.h>
#include <Fusion/Components/CylindricalJointMotion.h>
#include <Fusion/Components/Occurrence.h>
#include <Fusion/Components/Occurrences.h>
#include <Fusion/Construction/ConstructionPlane.h>
#include <Fusion/Features/Features.h>
#include <Fusion/Features/ExtrudeFeature.h>
#include <Fusion/Features/ExtrudeFeatures.h>
#include <Fusion/Features/ExtrudeFeatureInput.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/SketchCurve.h>
#include <Fusion/Sketch/SketchCurves.h>
#include <Fusion/Sketch/SketchLine.h>
#include <Fusion/Sketch/SketchLines.h>
#include <Fusion/Sketch/SketchLineList.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 in root component
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<SketchPoints> sketchPts = sketch->sketchPoints();
if (!sketchPts)
return false;
Ptr<Point3D> point = Point3D::create(1, 0, 1);
if (!point)
return false;
Ptr<SketchPoint> sketchPt = sketchPts->add(point);
if (!sketchPt)
return false;
Ptr<SketchLines> sketchLines = sketchCurves->sketchLines();
if (!sketchLines)
return false;
Ptr<Point3D> point1 = Point3D::create(1, 0, 2);
if (!point1)
return false;
Ptr<Point3D> point2 = Point3D::create(2, 0, 1);
if (!point2)
return false;
Ptr<Point3D> point1SketchSpace = sketch->modelToSketchSpace(point1);
if (!point1SketchSpace)
return false;
Ptr<Point3D> point2SketchSpace = sketch->modelToSketchSpace(point2);
if (!point2SketchSpace)
return false;
Ptr<SketchLineList> lines = sketchLines->addTwoPointRectangle(point1SketchSpace, point2SketchSpace);
if (!lines)
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 and make sure it's in a new component
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::NewComponentFeatureOperation);
if (!extInput)
return false;
// Set the extrusion input
Ptr<ValueInput> distance = ValueInput::createByReal(5);
if (!distance)
return false;
extInput->setDistanceExtent(true, distance);
extInput->isSolid(true);
// Create the extrusion
Ptr<ExtrudeFeature> ext = extrudes->add(extInput);
if (!ext)
return false;
// Get the end face of the created extrusion body
Ptr<BRepFaces> endFaces = ext->endFaces();
if (!endFaces)
return false;
Ptr<BRepFace> endFace = endFaces->item(0);
if (!endFace)
return false;
// Get the occurrence of the new component
Ptr<Occurrences> occs = rootComp->occurrences();
if (!occs)
return false;
Ptr<Occurrence> occ = occs->item(0);
if (!occ)
return false;
// Create a new sketch in the occurrence
Ptr<Sketch> sketchInOcc = sketches->add(endFace, occ);
if (!sketchInOcc)
return false;
// Get the sketch curve projected to the sketch
Ptr<SketchCurves> sketchCurvesInOcc = sketchInOcc->sketchCurves();
if (!sketchCurvesInOcc)
return false;
Ptr<SketchCurve> curve = sketchCurvesInOcc->item(0);
if (!curve)
return false;
// Create the first joint geometry with the sketch curve
Ptr<JointGeometry> geo0 = JointGeometry::createByCurve(curve, JointKeyPointTypes::StartKeyPoint);
if (!geo0)
return false;
// Create the second joint geometry with sketch point
Ptr<JointGeometry> geo1 = JointGeometry::createByPoint(sketchPt);
if (!geo1)
return false;
// Create joint input
Ptr<Joints> joints = rootComp->joints();
if (!joints)
return false;
Ptr<JointInput> jointInput = joints->createInput(geo0, geo1);
if (!jointInput)
return false;
// Set the joint input
Ptr<SketchLine> line = curve->cast<SketchLine>();
if (!line)
return false;
Ptr<SketchLine> lineProxy = line->createForAssemblyContext(occ);
if (!lineProxy)
return false;
jointInput->setAsCylindricalJointMotion(JointDirections::CustomJointDirection, lineProxy);
// Create the joint
Ptr<Joint> joint = joints->add(jointInput);
if (!joint)
return false;
Ptr<CylindricalJointMotion> cylindricalMotion = joint->jointMotion();
if (!cylindricalMotion)
return false;
Ptr<JointLimits> rotLimits = cylindricalMotion->rotationLimits();
if (!rotLimits)
return false;
rotLimits->isRestValueEnabled(true);
rotLimits->restValue(3.14 / 3);
Ptr<JointLimits> slideLimits = cylindricalMotion->slideLimits();
if (!slideLimits)
return false;
slideLimits->isMinimumValueEnabled(true);
slideLimits->minimumValue(0.1);
return true;
}
/** * CylindricalJointMotion API Sample * Demonstrates creating a joint with cylindrical joint motion. */ import { adsk } from '@adsk/fusion'; function run() { // Get the Fusion API's application object const app = adsk.core.Application.get(); if (!app) throw Error("No adsk.core.Application."); // Create a document. const doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType) const design = app.activeProduct as adsk.fusion.Design; // Get the root component of the active design. const rootComp = design.rootComponent // Create sketch in root component const sketches = rootComp.sketches const sketch = sketches.add(rootComp.xZConstructionPlane) const sketchPts = sketch.sketchPoints const point = adsk.core.Point3D.create(1, 0, 1) const sketchPt = sketchPts.add(point) const sketchLines = sketch.sketchCurves.sketchLines const point1 = adsk.core.Point3D.create(1, 0, 2) const point2 = adsk.core.Point3D.create(2, 0, 1) const point1SketchSpace = sketch.modelToSketchSpace(point1) const point2SketchSpace = sketch.modelToSketchSpace(point2) const lines = sketchLines.addTwoPointRectangle(point1SketchSpace, point2SketchSpace) // Get the profile defined by the circle const prof = sketch.profiles.item(0) // Create an extrusion input and make sure it's in a new component const extrudes = rootComp.features.extrudeFeatures const extInput = extrudes.createInput(prof, adsk.fusion.FeatureOperations.NewComponentFeatureOperation) // Set the extrusion input const distance = adsk.core.ValueInput.createByReal(5) extInput.setSymmetricExtent(distance, false) extInput.isSolid = true // Create the extrusion const ext = extrudes.add(extInput) // Get the end face of the created extrusion body const endFace = ext.endFaces.item(0) // Get the occurrence of the new component const occ = rootComp.occurrences.item(0) // Create a new sketch in the occurrence const sketchInOcc = sketches.add(endFace, occ) // Get the sketch curve projected to the sketch const curve = sketchInOcc.sketchCurves.item(0) // Create the first joint geometry with the sketch curve const geo0 = adsk.fusion.JointGeometry.createByCurve(curve, adsk.fusion.JointKeyPointTypes.StartKeyPoint) // Create the second joint geometry with sketch point const geo1 = adsk.fusion.JointGeometry.createByPoint(sketchPt) // Create joint input const joints = rootComp.joints const jointInput = joints.createInput(geo0, geo1) const line = curve as adsk.fusion.SketchLine const proxyLine = line.createForAssemblyContext(occ) // Set the joint input jointInput.setAsCylindricalJointMotion(adsk.fusion.JointDirections.CustomJointDirection, proxyLine) // Create the joint const joint = joints.add(jointInput) const cylindricalMotion = joint.jointMotion as adsk.fusion.CylindricalJointMotion const rotLimits = cylindricalMotion.rotationLimits rotLimits.isRestValueEnabled = true rotLimits.restValue = 3.14 / 3 const slideLimits = cylindricalMotion.slideLimits slideLimits.isMinimumValueEnabled = true slideLimits.minimumValue = 0.1 // Unground component from parent occ.isGroundToParent = false } run();