import adsk.core, adsk.fusion, traceback
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)
design = app.activeProduct
design.designType = adsk.fusion.DesignTypes.ParametricDesignType
# Get the root component of the active design.
rootComp = design.rootComponent
# Create a base feature
baseFeats = rootComp.features.baseFeatures
baseFeat = baseFeats.add()
baseFeat.startEdit()
# Create construction plane in base feature
planes = rootComp.constructionPlanes
planeInput = planes.createInput()
planeInput.targetBaseOrFormFeature = baseFeat
planeInput.setByOffset(rootComp.xYConstructionPlane, adsk.core.ValueInput.createByReal(1))
plane = planes.add(planeInput)
# Create sketch in base feature
sketches = rootComp.sketches
sketch = sketches.addToBaseOrFormFeature(plane, baseFeat, True)
# Draw a circle.
circles = sketch.sketchCurves.sketchCircles
circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), 2)
# Get the profile defined by the circle.
prof = sketch.profiles.item(0)
# Create an extrusion input to be able to define the input needed for an extrusion
# while specifying the profile and that a new component is to be created
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)
extInput.baseFeature = baseFeat
# Create the extrusion.
ext = extrudes.add(extInput)
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/Construction/ConstructionPlane.h>
#include <Fusion/Construction/ConstructionPlaneInput.h>
#include <Fusion/Construction/ConstructionPlanes.h>
#include <Fusion/Features/BaseFeature.h>
#include <Fusion/Features/BaseFeatures.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>
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;
design->designType(ParametricDesignType);
// Get the root component of the active design
Ptr<Component> rootComp = design->rootComponent();
if (!rootComp)
return false;
Ptr<Features> feats = rootComp->features();
if (!feats)
return false;
// Create a base feature
Ptr<BaseFeatures> baseFeats = feats->baseFeatures();
if (!baseFeats)
return false;
Ptr<BaseFeature> baseFeat = baseFeats->add();
if (!baseFeat)
return false;
baseFeat->startEdit();
// Create construction plane in base feature
Ptr<ConstructionPlanes> planes = rootComp->constructionPlanes();
if (!planes)
return false;
Ptr<ConstructionPlaneInput> planeInput = planes->createInput();
if (!planeInput)
return false;
planeInput->targetBaseOrFormFeature(baseFeat);
planeInput->setByOffset(rootComp->xYConstructionPlane(), ValueInput::createByReal(1));
Ptr<ConstructionPlane> plane = planes->add(planeInput);
if (!plane)
return false;
// Create sketch in base feature
Ptr<Sketches> sketches = rootComp->sketches();
if (!sketches)
return false;
Ptr<ConstructionPlane> xyPlane = rootComp->xYConstructionPlane();
if (!xyPlane)
return false;
Ptr<Sketch> sketch = sketches->addToBaseOrFormFeature(xyPlane, baseFeat, true);
if (!sketch)
return false;
// Draw a circle.
Ptr<SketchCurves> sketchCurves = sketch->sketchCurves();
if (!sketchCurves)
return false;
Ptr<SketchCircles> circles = sketchCurves->sketchCircles();
if (!circles)
return false;
Ptr<Point3D> centerPoint = Point3D::create(0, 0, 0);
if (!centerPoint)
return false;
Ptr<SketchCircle> circle1 = circles->addByCenterRadius(centerPoint, 2);
if (!circle1)
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 to be able to define the input needed for an extrusion
// while specifying the profile and that a new component is to be created
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);
extInput->targetBaseFeature(baseFeat);
// Create the extrusion.
Ptr<ExtrudeFeature> ext = extrudes->add(extInput);
if (!ext)
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