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)
sketchCircle = sketchCircles.addByCenterRadius(centerPoint, 3.0)
# Create a open profile for extrusion.
openProfile = rootComp.createOpenProfile(sketchCircle)
# Create an extrusion input.
features = rootComp.features
extrudes = features.extrudeFeatures
extrudeInput = extrudes.createInput(openProfile, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
extrudeInput.isSolid = False
# Define the extent with a distance extent of 3 cm.
distance = adsk.core.ValueInput.createByReal(3.0)
extrudeInput.setDistanceExtent(False, distance)
# Create the extrusion.
extrude = extrudes.add(extrudeInput)
# Get the body created by extrusion
body = extrude.bodies[0]
# Create sketch 2.
sketch2 = sketches.add(rootComp.xYConstructionPlane);
sketchLines = sketch2.sketchCurves.sketchLines;
startPoint = adsk.core.Point3D.create(-5, 0, 0);
endPoint = adsk.core.Point3D.create(5, 0, 0);
sketchLine = sketchLines.addByTwoPoints(startPoint, endPoint);
openProfile2 = rootComp.createOpenProfile(sketchLine);
# Create a open profile for extrusion.
extrudeInput2 = extrudes.createInput(openProfile2, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
extrudeInput2.isSolid = False
# Define the extent
distance2 = adsk.core.ValueInput.createByReal(5.0)
extrudeInput2.setDistanceExtent(False, distance2)
# Create the extrusion.
extrudes.add(extrudeInput2)
# Create trim feature
trims = features.trimFeatures
trimInput = trims.createInput(body)
cells = trimInput.bRepCells
cells[0].isSelected = True
trims.add(trimInput)
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/ObjectCollection.h>
#include <Core/Application/ValueInput.h>
#include <Core/Geometry/Point3D.h>
#include <Fusion/Fusion/Design.h>
#include <Fusion/Components/Component.h>
#include <Fusion/Construction/ConstructionPlane.h>
#include <Fusion/BRep/BRepBodies.h>
#include <Fusion/BRep/BRepBody.h>
#include <Fusion/Features/BRepCells.h>
#include <Fusion/Features/BRepCell.h>
#include <Fusion/Features/Features.h>
#include <Fusion/Features/ExtrudeFeature.h>
#include <Fusion/Features/ExtrudeFeatures.h>
#include <Fusion/Features/ExtrudeFeatureInput.h>
#include <Fusion/Features/TrimFeatures.h>
#include <Fusion/Features/TrimFeatureInput.h>
#include <Fusion/Features/TrimFeature.h>
#include <Fusion/Sketch/Sketch.h>
#include <Fusion/Sketch/Sketches.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/Profile.h>
#include <Fusion/Sketch/Profiles.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 circle on the xz plane.
Ptr<Sketches> sketches = rootComp->sketches();
if (!sketches)
return false;
Ptr<Sketch> sketch = sketches->add(rootComp->xZConstructionPlane());
if (!sketch)
return false;
Ptr<SketchCurves> sketchCurves = sketch->sketchCurves();
if (!sketchCurves)
return false;
Ptr<SketchCircles> sketchCirles = sketchCurves->sketchCircles();
if (!sketchCirles)
return false;
Ptr<Point3D> centerPoint = Point3D::create(0, 0, 0);
if (!centerPoint)
return false;
Ptr<SketchCircle> sketchCircle = sketchCirles->addByCenterRadius(centerPoint, 3.0);
if (!sketchCircle)
return false;
// Create a open profile for extrusion.
Ptr<Profile> openProfile = rootComp->createOpenProfile(sketchCircle);
// Create an extrusion input.
Ptr<Features> features = rootComp->features();
if (!features)
return false;
Ptr<ExtrudeFeatures> extrudes = features->extrudeFeatures();
if (!extrudes)
return false;
Ptr<ExtrudeFeatureInput> extrudeInput =
extrudes->createInput(openProfile, FeatureOperations::NewBodyFeatureOperation);
if (!extrudeInput)
return false;
extrudeInput->isSolid(false);
// Define the extent with a distance extent of 3 cm.
Ptr<ValueInput> distance = ValueInput::createByReal(3.0);
if (!distance)
return false;
extrudeInput->setDistanceExtent(false, distance);
// Create the extrusion.
Ptr<ExtrudeFeature> extrude = extrudes->add(extrudeInput);
if (!extrude)
return false;
// Get the body created by extrusion.
Ptr<BRepBodies> bodies = extrude->bodies();
if (!bodies)
return false;
Ptr<BRepBody> body = bodies->item(0);
// Create sketch 2.
Ptr<Sketch> sketch2 = sketches->add(rootComp->xYConstructionPlane());
if (!sketch2)
return false;
Ptr<SketchCurves> sketchCurves2 = sketch2->sketchCurves();
if (!sketchCurves2)
return false;
Ptr<SketchLines> sketchLines = sketchCurves2->sketchLines();
if (!sketchLines)
return false;
Ptr<Point3D> startPoint = Point3D::create(-5.0, 0, 0);
Ptr<Point3D> endPoint = Point3D::create(5.0, 0, 0);
Ptr<SketchLine> sketchLine = sketchLines->addByTwoPoints(startPoint, endPoint);
// Create a open profile.
Ptr<Profile> openProfile2 = rootComp->createOpenProfile(sketchLine);
// Create an extrusion input.
Ptr<ExtrudeFeatureInput> extrudeInput2 =
extrudes->createInput(openProfile2, FeatureOperations::NewBodyFeatureOperation);
if (!extrudeInput2)
return false;
extrudeInput2->isSolid(false);
// Define the extent.
Ptr<ValueInput> distance2 = ValueInput::createByReal(5.0);
extrudeInput2->setDistanceExtent(false, distance2);
// Create the extrusion.
extrudes->add(extrudeInput2);
// Create trim feature.
Ptr<TrimFeatures> trims = features->trimFeatures();
if (!trims)
return false;
Ptr<TrimFeatureInput> trimInput = trims->createInput(body);
if (!trimInput)
return false;
Ptr<BRepCells> cells = trimInput->bRepCells();
if (!cells)
return false;
Ptr<BRepCell> cell = cells->item(0);
if (!cell)
return false;
cell->isSelected(true);
trims->add(trimInput);
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