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)
sketchCircles = sketch.sketchCurves.sketchCircles
centerPoint = adsk.core.Point3D.create(0, 0, 0)
circle = sketchCircles.addByCenterRadius(centerPoint, 3.0)
# 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)
extInput.setDistanceExtent(False, distance)
# Create the extrusion.
ext = extrudes.add(extInput)
# Get the end face of the extrusion
endFaces = ext.endFaces
endFace = endFaces.item(0)
# Create a construction plane by offsetting the end face
planes = rootComp.constructionPlanes
planeInput = planes.createInput()
offsetVal = adsk.core.ValueInput.createByString('2 cm')
planeInput.setByOffset(endFace, offsetVal)
offsetPlane = planes.add(planeInput)
# Create a sketch on the new construction plane and add four sketch points on it
offsetSketch = sketches.add(offsetPlane)
offsetSketchPoints = offsetSketch.sketchPoints
sPt0 = offsetSketchPoints.add(adsk.core.Point3D.create(1, 0, 0))
sPt1 = offsetSketchPoints.add(adsk.core.Point3D.create(0, 1, 0))
sPt2 = offsetSketchPoints.add(adsk.core.Point3D.create(-1, 0, 0))
sPt3 = offsetSketchPoints.add(adsk.core.Point3D.create(0, -1, 0))
# Add the four sketch points into a collection
ptColl = adsk.core.ObjectCollection.create()
ptColl.add(sPt0)
ptColl.add(sPt1)
ptColl.add(sPt2)
ptColl.add(sPt3)
# Create a hole input
holes = rootComp.features.holeFeatures
holeInput = holes.createSimpleInput(adsk.core.ValueInput.createByString('2 mm'))
holeInput.setPositionBySketchPoints(ptColl)
holeInput.setDistanceExtent(distance)
hole = holes.add(holeInput)
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/ObjectCollection.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/Construction/ConstructionPlane.h>
#include <Fusion/Construction/ConstructionPlanes.h>
#include <Fusion/Construction/ConstructionPlaneInput.h>
#include <Fusion/Features/Features.h>
#include <Fusion/Features/ExtrudeFeature.h>
#include <Fusion/Features/ExtrudeFeatures.h>
#include <Fusion/Features/ExtrudeFeatureInput.h>
#include <Fusion/Features/HoleFeature.h>
#include <Fusion/Features/HoleFeatures.h>
#include <Fusion/Features/HoleFeatureInput.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/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
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<Point3D> centerPoint = Point3D::create(0, 0, 0);
if (!centerPoint)
return false;
Ptr<SketchCircle> circle = sketchCircles->addByCenterRadius(centerPoint, 3.0);
if (!circle)
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
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::NewBodyFeatureOperation);
if (!extInput)
return false;
// Define that the extent is a distance extent of 5 cm.
Ptr<ValueInput> distance = ValueInput::createByReal(5);
if (!distance)
return false;
extInput->setDistanceExtent(false, distance);
// Create the extrusion.
Ptr<ExtrudeFeature> ext = extrudes->add(extInput);
if (!ext)
return false;
// Get the end face of the extrusion
Ptr<BRepFaces> endFaces = ext->endFaces();
if (!endFaces)
return false;
Ptr<BRepFace> endFace = endFaces->item(0);
if (!endFace)
return false;
// Create a construction plane by offsetting the end face
Ptr<ConstructionPlanes> planes = rootComp->constructionPlanes();
if (!planes)
return false;
Ptr<ConstructionPlaneInput> planeInput = planes->createInput();
if (!planeInput)
return false;
Ptr<ValueInput> offsetVal = ValueInput::createByString("2 cm");
if (!offsetVal)
return false;
planeInput->setByOffset(endFace, offsetVal);
Ptr<ConstructionPlane> offsetPlane = planes->add(planeInput);
if (!offsetPlane)
return false;
// Create a sketch on the new construction plane and add four sketch points on it
Ptr<Sketch> offsetSketch = sketches->add(offsetPlane);
if (!offsetSketch)
return false;
Ptr<SketchPoints> offsetSketchPoints = offsetSketch->sketchPoints();
if (!offsetSketchPoints)
return false;
Ptr<Point3D> p0 = Point3D::create(1, 0, 0);
if (!p0)
return false;
Ptr<SketchPoint> sPt0 = offsetSketchPoints->add(p0);
if (!sPt0)
return false;
Ptr<Point3D> p1 = Point3D::create(0, 1, 0);
if (!p1)
return false;
Ptr<SketchPoint> sPt1 = offsetSketchPoints->add(p1);
if (!sPt1)
return false;
Ptr<Point3D> p2 = Point3D::create(-1, 0, 0);
if (!p2)
return false;
Ptr<SketchPoint> sPt2 = offsetSketchPoints->add(p2);
if (!sPt2)
return false;
Ptr<Point3D> p3 = Point3D::create(0, -1, 0);
if (!p3)
return false;
Ptr<SketchPoint> sPt3 = offsetSketchPoints->add(p3);
if (!sPt3)
return false;
// Add the four sketch points into a collection
Ptr<ObjectCollection> ptColl = ObjectCollection::create();
if (!ptColl)
return false;
ptColl->add(sPt0);
ptColl->add(sPt1);
ptColl->add(sPt2);
ptColl->add(sPt3);
// Create a hole input
Ptr<HoleFeatures> holes = feats->holeFeatures();
if (!holes)
return false;
Ptr<HoleFeatureInput> holeInput = holes->createSimpleInput(ValueInput::createByString("2 mm"));
if (!holeInput)
return false;
holeInput->setPositionBySketchPoints(ptColl);
holeInput->setDistanceExtent(distance);
Ptr<HoleFeature> hole = holes->add(holeInput);
if (!hole)
return false;
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