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)
sketchCircles = sketch.sketchCurves.sketchCircles
sketchLines = sketch.sketchCurves.sketchLines
centerPoint = adsk.core.Point3D.create(0, 0, 0)
circle = sketchCircles.addByCenterRadius(centerPoint, 5.0)
point0 = adsk.core.Point3D.create(0, 10, 0)
point1 = adsk.core.Point3D.create(10, 10, 0)
line = sketchLines.addByTwoPoints(point0, point1)
# 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)
# Create the first joint geometry with the end face
geo0 = adsk.fusion.JointGeometry.createByPlanarFace(endFace, None, adsk.fusion.JointKeyPointTypes.CenterKeyPoint)
# Create the second joint geometry with the sketch line
geo1 = adsk.fusion.JointGeometry.createByCurve(line, adsk.fusion.JointKeyPointTypes.EndKeyPoint)
# Create joint input
joints = rootComp.joints
jointInput = joints.createInput(geo0, geo1)
# Set the joint input
angle = adsk.core.ValueInput.createByString('90 deg')
jointInput.angle = angle
offset = adsk.core.ValueInput.createByString('1 cm')
jointInput.offset = offset
jointInput.isFlipped = True
jointInput.setAsRevoluteJointMotion(adsk.fusion.JointDirections.ZAxisJointDirection)
# Create the joint
joint = joints.add(jointInput)
# Lock the joint
joint.isLocked = True
# Get health state of a joint
health = joint.healthState
if health == adsk.fusion.FeatureHealthStates.ErrorFeatureHealthState or health == adsk.fusion.FeatureHealthStates.WarningFeatureHealthState:
message = joint.errorOrWarningMessage
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/Geometry/Line3D.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/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/SketchCurves.h>
#include <Fusion/Sketch/SketchLine.h>
#include <Fusion/Sketch/SketchLines.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<SketchCircles> sketchCircles = sketchCurves->sketchCircles();
if (!sketchCircles)
return false;
Ptr<SketchLines> sketchLines = sketchCurves->sketchLines();
if (!sketchLines)
return false;
Ptr<Point3D> centerPoint = Point3D::create(0, 0, 0);
if (!centerPoint)
return false;
Ptr<SketchCircle> circle = sketchCircles->addByCenterRadius(centerPoint, 5.0);
if (!circle)
return false;
Ptr<Point3D> point0 = Point3D::create(0, 10, 0);
if (!point0)
return false;
Ptr<Point3D> point1 = Point3D::create(10, 10, 0);
if (!point1)
return false;
Ptr<SketchLine> line = sketchLines->addByTwoPoints(point0, point1);
if (!line)
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;
// Create the first joint geometry with the end face
Ptr<JointGeometry> geo0 = JointGeometry::createByPlanarFace(endFace, nullptr, JointKeyPointTypes::CenterKeyPoint);
if (!geo0)
return false;
// Create the second joint geometry with the sketch line
Ptr<JointGeometry> geo1 = JointGeometry::createByCurve(line, JointKeyPointTypes::EndKeyPoint);
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<ValueInput> angle = ValueInput::createByString("90 deg");
if (!angle)
return false;
jointInput->angle(angle);
Ptr<ValueInput> offset = ValueInput::createByString("1 cm");
if (!offset)
return false;
jointInput->offset(offset);
jointInput->isFlipped(true);
jointInput->setAsRevoluteJointMotion(adsk::fusion::JointDirections::ZAxisJointDirection);
// Create the joint
Ptr<Joint> joint = joints->add(jointInput);
if (!joint)
return false;
// Lock the joint
joint->isLocked(true);
// Get health state of a joint
adsk::fusion::FeatureHealthStates health = joint->healthState();
if (health == adsk::fusion::FeatureHealthStates::ErrorFeatureHealthState ||
health == adsk::fusion::FeatureHealthStates::WarningFeatureHealthState)
{
std::string msg = joint->errorOrWarningMessage();
}
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