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
# Get extrude features
extrudes = rootComp.features.extrudeFeatures
# 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, 5.0)
# Get the profile defined by the circle
prof = sketch.profiles.item(0)
# Create another sketch
sketchVertical = sketches.add(rootComp.yZConstructionPlane)
sketchCirclesVertical = sketchVertical.sketchCurves.sketchCircles
centerPointVertical = adsk.core.Point3D.create(0, 1, 0)
cicleVertical = sketchCirclesVertical.addByCenterRadius(centerPointVertical, 0.5)
# Get the profile defined by the vertical circle
profVertical = sketchVertical.profiles.item(0)
# Extrude Sample 1: A simple way of creating typical extrusions (extrusion that goes from the profile plane the specified distance).
# Define a distance extent of 5 cm
distance = adsk.core.ValueInput.createByReal(5)
extrude1 = extrudes.addSimple(prof, distance, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
# Get the extrusion body
body1 = extrude1.bodies.item(0)
body1.name = "simple"
# Get the state of the extrusion
health = extrude1.healthState
if health == adsk.fusion.FeatureHealthStates.WarningFeatureHealthState or health == adsk.fusion.FeatureHealthStates.ErrorFeatureHealthState:
message = extrude1.errorOrWarningMessage
# Get the state of timeline object
timeline = design.timeline
timelineObj = timeline.item(timeline.count - 1);
health = timelineObj.healthState
message = timelineObj.errorOrWarningMessage
# Create another sketch
sketch = sketches.add(rootComp.xZConstructionPlane)
sketchCircles = sketch.sketchCurves.sketchCircles
centerPoint = adsk.core.Point3D.create(0, 0, 0)
circle1 = sketchCircles.addByCenterRadius(centerPoint, 13.0)
circle2 = sketchCircles.addByCenterRadius(centerPoint, 15.0)
outerProfile = sketch.profiles.item(1)
# Create taperAngle value inputs
deg0 = adsk.core.ValueInput.createByString("0 deg")
deg2 = adsk.core.ValueInput.createByString("2 deg")
deg5 = adsk.core.ValueInput.createByString("5 deg")
# Create distance value inputs
mm10 = adsk.core.ValueInput.createByString("10 mm")
mm100 = adsk.core.ValueInput.createByString("100 mm")
# Extrude Sample 2: Create an extrusion that goes from the profile plane with one side distance extent
extrudeInput = extrudes.createInput(outerProfile, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
# Create a distance extent definition
extent_distance = adsk.fusion.DistanceExtentDefinition.create(mm100)
extrudeInput.setOneSideExtent(extent_distance, adsk.fusion.ExtentDirections.PositiveExtentDirection)
# Create the extrusion
extrude2 = extrudes.add(extrudeInput)
# Get the body of the extrusion
body2 = extrude2.bodies.item(0)
body2.name = "distance, from profile"
# Extrude Sample 3: Create an extrusion that starts from an entity and goes the specified distance.
extrudeInput = extrudes.createInput(profVertical, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
# Create a distance extent definition
extent_distance_2 = adsk.fusion.DistanceExtentDefinition.create(mm10)
# Create a start extent that starts from a brep face with an offset of 10 mm.
start_from = adsk.fusion.FromEntityStartDefinition.create(body1.faces.item(0), mm10)
# taperAngle should be 0 because extrude start face is not a planar face in this case
extrudeInput.setOneSideExtent(extent_distance_2, adsk.fusion.ExtentDirections.PositiveExtentDirection)
extrudeInput.startExtent = start_from
# Create the extrusion
extrude3 = extrudes.add(extrudeInput)
body3 = extrude3.bodies.item(0)
body3.name = "distance, from entity"
# Edit the distance extent of the extrusion.
disDef = adsk.fusion.DistanceExtentDefinition.cast(extrude3.extentOne)
distanceMP = adsk.fusion.ModelParameter.cast(disDef.distance)
distanceMP.value = 5.0
# Edit the start entity of the extrusion.
startDef = adsk.fusion.FromEntityStartDefinition.cast(extrude3.startExtent)
outerFace = body2.faces.item(1)
extrude3.timelineObject.rollTo(True)
startDef.entity = outerFace
design.timeline.moveToEnd()
# Edit the offset to the start entity in the extrusion.
startDef = adsk.fusion.FromEntityStartDefinition.cast(extrude3.startExtent)
offsetMP = adsk.fusion.ModelParameter.cast(startDef.offset)
offsetMP.value = 1.5
# Extrude Sample 4: Create an extrusion that goes from the profile plane to a specified entity.
extrudeInput = extrudes.createInput(profVertical, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
# Create a to-entity extent definition
isChained = True
extent_toentity = adsk.fusion.ToEntityExtentDefinition.create(body1, isChained)
# Set the one side extent with the to-entity-extent-definition, and with a taper angle of 0 degree
extrudeInput.setOneSideExtent(extent_toentity, adsk.fusion.ExtentDirections.PositiveExtentDirection)
# Create an offset type start definition
start_offset = adsk.fusion.OffsetStartDefinition.create(mm10)
# Set the start extent of the extrusion
extrudeInput.startExtent = start_offset
# Create the extrusion
extrude4 = extrudes.add(extrudeInput)
body4 = extrude4.bodies.item(0)
body4.name = "to entity, from offset"
# Edit the start offset of the extrusion
startDef = adsk.fusion.OffsetStartDefinition.cast(extrude4.startExtent)
offsetMP = adsk.fusion.ModelParameter.cast(startDef.offset)
offsetMP.value = 0.5
# Edit the to-entity extent definition of the extrusion
negative = adsk.core.Vector3D.create(-1,0,0)
toDef = adsk.fusion.ToEntityExtentDefinition.cast(extrude4.extentOne)
extrude4.timelineObject.rollTo(True)
toDef.entity = body2
toDef.isMinimumSolution = False
toDef.directionHint = negative
toDef.isChained = False
design.timeline.moveToEnd()
# Extrude Sample 5: Create an extrusion that goes through all entities
extrudeInput = extrudes.createInput(profVertical, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
# Create an extent definition of through-all type.
extent_all = adsk.fusion.ThroughAllExtentDefinition.create()
extrudeInput.setOneSideExtent(extent_all, adsk.fusion.ExtentDirections.NegativeExtentDirection, deg2)
# Set the extrusion start with an offset
extrudeInput.startExtent = start_offset
# Create the extrusion
extrude5 = extrudes.add(extrudeInput)
body5 = extrude5.bodies.item(0)
body5.name = "through-all, from offset"
# Edit the start offset
startDef = adsk.fusion.OffsetStartDefinition.cast(extrude5.startExtent)
offsetMP = adsk.fusion.ModelParameter.cast(startDef.offset)
offsetMP.value = 0.5
# Edit the direction of the extrusion, make it in the same direction as the sketch plane.
allDef = adsk.fusion.ThroughAllExtentDefinition.cast(extrude5.extentOne)
extrude5.timelineObject.rollTo(True)
if allDef.isPositiveDirection:
allDef.isPositiveDirection = False
design.timeline.moveToEnd()
# Extrude Sample 6: Create a symmetric extrusion that goes 10 mm from the profile plane with a 5 degree taper angle.
isFullLength = True
extrudeInput = extrudes.createInput(profVertical, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
extrudeInput.setSymmetricExtent(mm10, isFullLength, deg5)
# Create the extrusion
extrude6 = extrudes.add(extrudeInput)
body6 = extrude6.bodies.item(0)
body6.name = "symmetric"
# Edit the measurement, distance and taper angle properties of the symmetric extrusion
symDef = adsk.fusion.SymmetricExtentDefinition.cast(extrude6.extentOne)
extrude6.timelineObject.rollTo(True)
symDef.isFullLength = not symDef.isFullLength
design.timeline.moveToEnd()
taperAngleMP = adsk.fusion.ModelParameter.cast(symDef.taperAngle)
taperAngleMP.expression = "6 deg"
distanceMP = adsk.fusion.ModelParameter.cast(symDef.distance)
distanceMP.expression = "3 mm"
# another way to get the symmetric extent definition
if (extrude6.extentType == adsk.fusion.FeatureExtentTypes.SymmetricFeatureExtentType):
symDef1 = extrude6.symmetricExtent
distanceMP1 = symDef1.distance
distanceMP1.value = 4
# Extrude Sample 7: Create a 2-side extrusion, whose 1st side is 100 mm distance extent, and 2nd side is 10 mm distance extent.
extrudeInput = extrudes.createInput(profVertical, adsk.fusion.FeatureOperations.CutFeatureOperation)
extent_distance_2 = adsk.fusion.DistanceExtentDefinition.create(adsk.core.ValueInput.createByString("20cm"))
extrudeInput.setTwoSidesExtent(extent_distance, extent_distance_2, deg5, deg0)
extrude7 = extrudes.add(extrudeInput)
# Edit the taper angles of both sides in the extrusion
angleMP_1 = adsk.fusion.ModelParameter.cast(extrude7.taperAngleOne)
angleMP_2 = adsk.fusion.ModelParameter.cast(extrude7.taperAngleTwo)
angleMP_1.expression = "30 deg"
angleMP_2.expression = "-1 deg"
# Get the extent definition of both sides
extent_1 = adsk.fusion.DistanceExtentDefinition.cast(extrude7.extentOne)
extent_2 = adsk.fusion.DistanceExtentDefinition.cast(extrude7.extentTwo)
# Edit the distances the extrusion
distanceMP_1 = adsk.fusion.ModelParameter.cast(extent_1.distance)
distanceMP_2 = adsk.fusion.ModelParameter.cast(extent_2.distance)
distanceMP_1.expression = "80 mm"
distanceMP_2.expression = "25 cm"
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/Geometry/Vector3D.h>
#include <Core/UserInterface/UserInterface.h>
#include <Fusion/BRep/BRepBody.h>
#include <Fusion/BRep/BRepBodies.h>
#include <Fusion/BRep/BRepFace.h>
#include <Fusion/BRep/BRepFaces.h>
#include <Fusion/Components/Component.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/Features/ExtentDefinition.h>
#include <Fusion/Features/DistanceExtentDefinition.h>
#include <Fusion/Features/FromEntityStartDefinition.h>
#include <Fusion/Features/OffsetStartDefinition.h>
#include <Fusion/Features/SymmetricExtentDefinition.h>
#include <Fusion/Features/ThroughAllExtentDefinition.h>
#include <Fusion/Features/ToEntityExtentDefinition.h>
#include <Fusion/Fusion/Design.h>
#include <Fusion/Fusion/ModelParameter.h>
#include <Fusion/Fusion/Timeline.h>
#include <Fusion/Fusion/TimelineObject.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;
// Get extrude features
Ptr<Features> feats = rootComp->features();
if (!feats)
return false;
Ptr<ExtrudeFeatures> extrudes = feats->extrudeFeatures();
if (!extrudes)
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, 5.0);
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 another sketch
Ptr<ConstructionPlane> yz = rootComp->yZConstructionPlane();
if (!yz)
return false;
Ptr<Sketch> sketchVertical = sketches->add(yz);
if (!sketchVertical)
return false;
Ptr<SketchCurves> sketchCurvesVertical = sketchVertical->sketchCurves();
if (!sketchCurvesVertical)
return false;
Ptr<SketchCircles> sketchCirclesVertical = sketchCurvesVertical->sketchCircles();
if (!sketchCirclesVertical)
return false;
Ptr<Point3D> centerPointVertical = Point3D::create(0, 1, 0);
if (!centerPointVertical)
return false;
Ptr<SketchCircle> cicleVertical = sketchCirclesVertical->addByCenterRadius(centerPointVertical, 0.5);
if (!cicleVertical)
return false;
// Get the profile defined by the vertical circle
Ptr<Profiles> profsVertical = sketchVertical->profiles();
if (!profsVertical)
return false;
Ptr<Profile> profVertical = profsVertical->item(0);
if (!profVertical)
return false;
// Extrude Sample 1: A simple way of creating typical extrusions (extrusion that goes from the profile plane the
// specified distance). Define that the extent is a distance extent of 5 cm
Ptr<ValueInput> distance = ValueInput::createByReal(5);
if (!distance)
return false;
Ptr<ExtrudeFeature> extrude1 =
extrudes->addSimple(prof, distance, adsk::fusion::FeatureOperations::NewBodyFeatureOperation);
if (!extrude1)
return false;
// Get the body created by the extrusion
Ptr<BRepBodies> bodies = extrude1->bodies();
if (!bodies)
return false;
Ptr<BRepBody> body1 = bodies->item(0);
if (!body1)
return false;
body1->name("simple");
// Get the state of the extrusion
adsk::fusion::FeatureHealthStates health = extrude1->healthState();
if (adsk::fusion::FeatureHealthStates::ErrorFeatureHealthState == health ||
adsk::fusion::FeatureHealthStates::WarningFeatureHealthState == health)
{
std::string strWarningMsgForExtrusion = extrude1->errorOrWarningMessage();
}
// Get the state of a timeline object
Ptr<Timeline> timeline = design->timeline();
Ptr<TimelineObject> timelineObj = timeline->item(timeline->count() - 1);
health = timelineObj->healthState();
std::string strMsg = timelineObj->errorOrWarningMessage();
// Create another sketch
sketch = sketches->add(rootComp->xZConstructionPlane());
sketchCurves = sketch->sketchCurves();
sketchCircles = sketchCurves->sketchCircles();
Ptr<SketchCircle> circle1 = sketchCircles->addByCenterRadius(centerPoint, 13.0);
Ptr<SketchCircle> circle2 = sketchCircles->addByCenterRadius(centerPoint, 15.0);
Ptr<Profiles> profiles = sketch->profiles();
Ptr<Profile> outerProfile = profiles->item(1);
// Create taper angle value inputs
Ptr<ValueInput> deg0 = adsk::core::ValueInput::createByString("0 deg");
Ptr<ValueInput> deg2 = adsk::core::ValueInput::createByString("2 deg");
Ptr<ValueInput> deg5 = adsk::core::ValueInput::createByString("5 deg");
// Create distance value inputs
Ptr<ValueInput> mm10 = adsk::core::ValueInput::createByString("10 mm");
Ptr<ValueInput> mm100 = adsk::core::ValueInput::createByString("100 mm");
// Extrude Sample 2: Create an extrusion that goes from the profile plane with one side distance extent
Ptr<ExtrudeFeatureInput> extrudeInput =
extrudes->createInput(outerProfile, adsk::fusion::FeatureOperations::NewBodyFeatureOperation);
// Create a distance extent definition
Ptr<DistanceExtentDefinition> extent_distance = adsk::fusion::DistanceExtentDefinition::create(mm100);
extrudeInput->setOneSideExtent(extent_distance, adsk::fusion::ExtentDirections::PositiveExtentDirection));
// Create the extrusion
Ptr<ExtrudeFeature> extrude2 = extrudes->add(extrudeInput);
// Get the body of the extrusion
bodies = extrude2->bodies();
Ptr<BRepBody> body2 = bodies->item(0);
body2->name("distance, from profile");
// Extrude Sample 3: Create an extrusion that starts from an entity and goes the specified distance.
extrudeInput = extrudes->createInput(profVertical, adsk::fusion::FeatureOperations::NewBodyFeatureOperation);
// Create a distance extent definition
Ptr<DistanceExtentDefinition> extent_distance_2 = adsk::fusion::DistanceExtentDefinition::create(mm10);
// Create a start extent that starts from a BRep face with an offset of 10 mm.
Ptr<BRepFaces> faces = body1->faces();
Ptr<BRepFace> face = faces->item(0);
Ptr<FromEntityStartDefinition> start_from = adsk::fusion::FromEntityStartDefinition::create(face, mm10);
extrudeInput->setOneSideExtent(extent_distance_2, adsk::fusion::ExtentDirections::PositiveExtentDirection));
// Create the extrusion
Ptr<ExtrudeFeature> extrude3 = extrudes->add(extrudeInput);
// Get the body of the extrusion
bodies = extrude3->bodies();
Ptr<BRepBody> body3 = bodies->item(0);
body3->name("distance, from entity");
// taperAngle is nullptr, because extrude start face is not a planar face in this case
Ptr<ModelParameter> taperAngle = extrude3->taperAngleOne();
// Edit the distance extent of the extrusion.
Ptr<ExtentDefinition> extent1 = extrude3->extentOne();
Ptr<DistanceExtentDefinition> disDef = extent1->cast<DistanceExtentDefinition>();
Ptr<ModelParameter> distanceMP = disDef->distance();
// Edit the start entity of the extrusion.
Ptr<FromEntityStartDefinition> startDef_from = extrude3->startExtent();
Ptr<BRepFaces> faces2 = body2->faces();
Ptr<BRepFace> outerFace = faces2->item(0);
Ptr<TimelineObject> extrudeTimelineObj = extrude3->timelineObject();
// Edit the offset to the start entity in the extrusion.
startDef_from = extrude3->startExtent();
Ptr<ModelParameter> offsetMP = startDef_from->offset();
// Extrude Sample 4: Create an extrusion that goes from the profile plane to a specified entity.
extrudeInput = extrudes->createInput(profVertical, adsk::fusion::FeatureOperations::NewBodyFeatureOperation);
// Create a to-entity extent definition
bool isChained = true;
Ptr<ToEntityExtentDefinition> extent_toentity = adsk::fusion::ToEntityExtentDefinition::create(body1, isChained);
// Set the one side extent with the to-entity-extent-definition, and with a taper angle of 0 degree
extrudeInput->setOneSideExtent(extent_toentity, adsk::fusion::ExtentDirections::PositiveExtentDirection, deg0));
// Create an offset type start definition
Ptr<OffsetStartDefinition> start_offset = adsk::fusion::OffsetStartDefinition::create(mm10);
// Create the extrusion
Ptr<ExtrudeFeature> extrude4 = extrudes->add(extrudeInput);
// Get the body of the extrusion
bodies = extrude4->bodies();
Ptr<BRepBody> body4 = bodies->item(0);
body4->name("to entity, from offset");
// Edit the start offset of the extrusion
Ptr<OffsetStartDefinition> startDef_offset = extrude4->startExtent();
offsetMP = startDef_offset->offset();
// Edit the to-entity extent definition of the extrusion
Ptr<Vector3D> negative = adsk::core::Vector3D::create(-1, 0, 0);
Ptr<ToEntityExtentDefinition> toDef = extrude4->extentOne();
extrudeTimelineObj = extrude4->timelineObject();
// Extrude Sample 5: Create an extrusion that goes through all entities
extrudeInput = extrudes->createInput(profVertical, adsk::fusion::FeatureOperations::NewBodyFeatureOperation);
// Create an extent definition of through-all type.
Ptr<ThroughAllExtentDefinition> extent_all = adsk::fusion::ThroughAllExtentDefinition::create();
extrudeInput->setOneSideExtent(extent_all, adsk::fusion::ExtentDirections::PositiveExtentDirection, deg2));
// Set the extrusion start with an offset
Ptr<ExtrudeFeature> extrude5 = extrudes->add(extrudeInput);
// Get the body of the extrusion
bodies = extrude5->bodies();
Ptr<BRepBody> body5 = bodies->item(0);
body5->name("through-all, from offset");
// Edit the start offset
startDef_offset = extrude5->startExtent();
offsetMP = startDef_offset->offset();
// Edit the direction of the extrusion, make it in the same direction as the sketch plane.
Ptr<ThroughAllExtentDefinition> allDef = extrude5->extentOne();
extrudeTimelineObj = extrude5->timelineObject();
if (allDef->isPositiveDirection())
{
}
// Extrude Sample 6: Create a symmetric extrusion that goes 10 mm from the profile plane with a 5 degree taper
// angle.
bool isFullLength = true;
extrudeInput = extrudes->createInput(profVertical, adsk::fusion::FeatureOperations::NewBodyFeatureOperation);
Ptr<ExtrudeFeature> extrude6 = extrudes->add(extrudeInput);
// Get the body of the extrusion
bodies = extrude6->bodies();
Ptr<BRepBody> body6 = bodies->item(0);
body6->name("symmetric");
// Edit the measurement, distance and taper angle properties of the symmetric extrusion
Ptr<SymmetricExtentDefinition> symDef = extrude6->extentOne();
extrudeTimelineObj = extrude6->timelineObject();
Ptr<ModelParameter> taperAngleMP = symDef->taperAngle();
distanceMP = symDef->distance();
// another way to get the symmetric extent definition
if (extrude6->extentType() == adsk::fusion::FeatureExtentTypes::SymmetricFeatureExtentType)
{
Ptr<SymmetricExtentDefinition> symDef1 = extrude6->symmetricExtent();
Ptr<ModelParameter> distanceMP1 = symDef1->distance();
}
// Extrude Sample 7: Create a 2-side extrusion, whose 1st side is 100 mm distance extent, and 2nd side is 10 mm
// distance extent.
extrudeInput = extrudes->createInput(profVertical, adsk::fusion::FeatureOperations::CutFeatureOperation);
Ptr<DistanceExtentDefinition> extent_distance_20cm =
adsk::fusion::DistanceExtentDefinition::create(adsk::core::ValueInput::createByString("20cm"));
Ptr<ExtrudeFeature> extrude7 = extrudes->add(extrudeInput);
// Edit the taper angles of both sides in the extrusion
Ptr<ModelParameter> angleMP_1 = extrude7->taperAngleOne();
Ptr<ModelParameter> angleMP_2 = extrude7->taperAngleTwo();
// Get the extent definition of both sides
Ptr<DistanceExtentDefinition> extent_1 = extrude7->extentOne();
Ptr<DistanceExtentDefinition> extent_2 = extrude7->extentTwo();
// Edit the distances the extrusion
Ptr<ModelParameter> distanceMP_1 = extent_1->distance();
Ptr<ModelParameter> distanceMP_2 = extent_2->distance();
return true;
}
