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)
# Create sketch circle
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)
# Set the distance extent to be symmetric
extInput.setDistanceExtent(True, distance)
# Set the extrude to be a solid one
extInput.isSolid = True
# Create an cylinder
extrude = extrudes.add(extInput)
# Create sketch line
sketchLines = sketch.sketchCurves.sketchLines
startPoint = adsk.core.Point3D.create(5, 5, 0)
endPoint = adsk.core.Point3D.create(5, 10, 0)
sketchLineOne = sketchLines.addByTwoPoints(startPoint, endPoint)
endPointTwo = adsk.core.Point3D.create(10, 5, 0)
sketchLineTwo = sketchLines.addByTwoPoints(startPoint, endPointTwo)
# Create three sketch points
sketchPoints = sketch.sketchPoints
positionOne = adsk.core.Point3D.create(0, 5.0, 0)
sketchPointOne = sketchPoints.add(positionOne)
positionTwo = adsk.core.Point3D.create(5.0, 0, 0)
sketchPointTwo = sketchPoints.add(positionTwo)
positionThree = adsk.core.Point3D.create(0, -5.0, 0)
sketchPointThree = sketchPoints.add(positionThree)
# Get the profile again since the sketch has been edit.
prof = sketch.profiles.item(0)
# Get construction planes
planes = rootComp.constructionPlanes
# Create construction plane input
planeInput = planes.createInput()
# Add construction plane by offset
offsetValue = adsk.core.ValueInput.createByReal(3.0)
planeInput.setByOffset(prof, offsetValue)
planeOne = planes.add(planeInput)
# Get the health state of the plane
health = planeOne.healthState
if health == adsk.fusion.FeatureHealthStates.ErrorFeatureHealthState or health == adsk.fusion.FeatureHealthStates.WarningFeatureHealthState:
message = planeOne.errorOrWarningMessage
# Add construction plane by angle
angle = adsk.core.ValueInput.createByString('30.0 deg')
planeInput.setByAngle(sketchLineOne, angle, prof)
planes.add(planeInput)
# Add construction plane by two planes
planeInput.setByTwoPlanes(prof, planeOne)
planes.add(planeInput)
# Add construction plane by tangent
cylinderFace = extrude.sideFaces.item(0)
planeInput.setByTangent(cylinderFace, angle, rootComp.xYConstructionPlane)
planes.add(planeInput)
# Add construction plane by two edges
planeInput.setByTwoEdges(sketchLineOne, sketchLineTwo)
planes.add(planeInput)
# Add construction plane by three points
planeInput.setByThreePoints(sketchPointOne, sketchPointTwo, sketchPointThree)
planes.add(planeInput)
# Add construction plane by tangent at point
planeInput.setByTangentAtPoint(cylinderFace, sketchPointOne)
planes.add(planeInput)
# Add construction plane by distance on path
distance = adsk.core.ValueInput.createByReal(1.0)
planeInput.setByDistanceOnPath(sketchLineOne, distance)
planes.add(planeInput)
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/ValueInput.h>
#include <Core/Geometry/Point3D.h>
#include <Core/Geometry/Vector3D.h>
#include <Core/UserInterface/UserInterface.h>
#include <Fusion/Components/Component.h>
#include <Fusion/Construction/ConstructionPlane.h>
#include <Fusion/Construction/ConstructionPlanes.h>
#include <Fusion/Construction/ConstructionPlaneInput.h>
#include <Fusion/Fusion/Design.h>
#include <Fusion/Sketch/Sketch.h>
#include <Fusion/Sketch/Sketches.h>
#include <Fusion/Sketch/SketchPoints.h>
#include <Fusion/Sketch/SketchPoint.h>
#include <Fusion/Sketch/SketchCurves.h>
#include <Fusion/Sketch/SketchCircles.h>
#include <Fusion/Sketch/SketchCircle.h>
#include <Fusion/Sketch/SketchLines.h>
#include <Fusion/Sketch/SketchLine.h>
#include <Fusion/Sketch/SketchPoints.h>
#include <Fusion/Sketch/SketchPoint.h>
#include <Fusion/Sketch/Profiles.h>
#include <Fusion/Sketch/Profile.h>
#include <Fusion/Features/Features.h>
#include <Fusion/Features/ExtrudeFeatures.h>
#include <Fusion/Features/ExtrudeFeatureInput.h>
#include <Fusion/Features/ExtrudeFeature.h>
#include <Fusion/BRep/BRepFaces.h>
#include <Fusion/BRep/BRepFace.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> 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->xYConstructionPlane());
if (!sketch)
return false;
// Create sketch circle
Ptr<SketchCurves> curves = sketch->sketchCurves();
if (!curves)
return false;
Ptr<SketchCircles> circles = curves->sketchCircles();
if (!circles)
return false;
Ptr<Point3D> centerPoint = Point3D::create(0, 0, 0);
circles->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);
// Create an extrusion input
Ptr<Features> features = rootComp->features();
if (!features)
return false;
Ptr<ExtrudeFeatures> extrudes = features->extrudeFeatures();
if (!extrudes)
return false;
Ptr<ExtrudeFeatureInput> extInput = extrudes->createInput(prof, FeatureOperations::NewBodyFeatureOperation);
// Define that the extent is a distance extent of 5 cm
Ptr<ValueInput> distance = ValueInput::createByReal(5.0);
// Set the distance extent to be symmetric
extInput->setDistanceExtent(true, distance);
// Set the extrude to be a solid one
extInput->isSolid(true);
// Create an cylinder
Ptr<ExtrudeFeature> extrude = extrudes->add(extInput);
if (!extrude)
return false;
// Create sketch line
Ptr<SketchLines> sketchLines = curves->sketchLines();
if (!sketchLines)
return false;
Ptr<Point3D> startPoint = Point3D::create(5.0, 5.0, 0);
Ptr<Point3D> endPoint = Point3D::create(5.0, 10.0, 0);
Ptr<SketchLine> sketchLineOne = sketchLines->addByTwoPoints(startPoint, endPoint);
Ptr<Point3D> endPointTwo = Point3D::create(10.0, 5.0, 0);
Ptr<SketchLine> sketchLineTwo = sketchLines->addByTwoPoints(startPoint, endPointTwo);
// Create three sketch points
Ptr<SketchPoints> sketchPoints = sketch->sketchPoints();
if (!sketchPoints)
return false;
Ptr<Point3D> positionOne = Point3D::create(0, 5.0, 0);
Ptr<SketchPoint> sketchPointOne = sketchPoints->add(positionOne);
Ptr<Point3D> positionTwo = Point3D::create(5.0, 0, 0);
Ptr<SketchPoint> sketchPointTwo = sketchPoints->add(positionTwo);
Ptr<Point3D> positionThree = Point3D::create(0, -5.0, 0);
Ptr<SketchPoint> sketchPointThree = sketchPoints->add(positionThree);
prof = profs->item(0);
// Get construction planes
Ptr<ConstructionPlanes> planes = rootComp->constructionPlanes();
if (!planes)
return false;
// Create construction plane input
Ptr<ConstructionPlaneInput> planeInput = planes->createInput();
if (!planeInput)
return false;
// Add construction plane by offset
Ptr<ValueInput> offsetValue = ValueInput::createByReal(3.0);
planeInput->setByOffset(prof, offsetValue);
Ptr<ConstructionPlane> planeOne = planes->add(planeInput);
// Get the health state of a construction plane
adsk::fusion::FeatureHealthStates health = planeOne->healthState();
if (health == adsk::fusion::FeatureHealthStates::ErrorFeatureHealthState ||
health == adsk::fusion::FeatureHealthStates::WarningFeatureHealthState)
{
std::string msg = planeOne->errorOrWarningMessage();
}
// Add construction plane by angle
Ptr<ValueInput> angle = ValueInput::createByString("30.0 deg");
planeInput->setByAngle(sketchLineOne, angle, prof);
planes->add(planeInput);
// Add construction plane by two planes
planeInput->setByTwoPlanes(prof, planeOne);
planes->add(planeInput);
// Add construction plane by tangent
Ptr<BRepFaces> extSideFaces = extrude->sideFaces();
if (!extSideFaces)
return false;
Ptr<BRepFace> cylinderFace = extSideFaces->item(0);
planeInput->setByTangent(cylinderFace, angle, rootComp->xZConstructionPlane());
planes->add(planeInput);
// Add construction plane by two edges
planeInput->setByTwoEdges(sketchLineOne, sketchLineTwo);
planes->add(planeInput);
// Add construction plane by three points
planeInput->setByThreePoints(sketchPointOne, sketchPointTwo, sketchPointThree);
planes->add(planeInput);
// Add construction plane by tangent at point
planeInput->setByTangentAtPoint(cylinderFace, sketchPointOne);
planes->add(planeInput);
// Add construction plane by distance on path
distance = ValueInput::createByReal(1.0);
planeInput->setByDistanceOnPath(sketchLineOne, distance);
planes->add(planeInput);
// 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