Demonstrates projects the specified set of curves onto the specified set of faces using the specified method of projection.
Before running: No open document is required; the script creates a new design (or additional documents) as it runs.
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
allOccs = rootComp.occurrences
transform = adsk.core.Matrix3D.create()
# Create three components under root component
occ1 = allOccs.addNewComponent(transform)
subComp1 = occ1.component
occ2 = allOccs.addNewComponent(transform)
subComp2 = occ2.component
occ3 = allOccs.addNewComponent(transform)
subComp3 = occ3.component
# Create a sketch in sub component 1
sketches1 = subComp1.sketches
sketch1 = sketches1.add(rootComp.yZConstructionPlane)
# Get sketch lines
sketchLines = sketch1.sketchCurves.sketchLines
# Create sketch rectangle
startPoint = adsk.core.Point3D.create(-8.0, 0, 0)
endPoint = adsk.core.Point3D.create(8.0, 8.0, 0)
sketchLines.addTwoPointRectangle(startPoint, endPoint)
# Get the profile of the first sketch
prof1 = sketch1.profiles.item(0)
# Create an extrusion input
extrudes1 = subComp1.features.extrudeFeatures
extInput1 = extrudes1.createInput(prof1, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
# Define that the extent is a distance extent of 2 cm
distance1 = adsk.core.ValueInput.createByReal(2.0)
# Set the distance extent
extInput1.setDistanceExtent(False, distance1)
# Set the extrude type to be solid
extInput1.isSolid = True
# Create the extrusion
ext1 = extrudes1.add(extInput1)
# Create construction plane
planes = rootComp.constructionPlanes
planeInput = planes.createInput()
offsetValue = adsk.core.ValueInput.createByReal(8.0)
planeInput.setByOffset(rootComp.yZConstructionPlane, offsetValue)
plane = planes.add(planeInput)
# Create a sketch in sub component 2
sketches2 = subComp2.sketches
sketch2 = sketches2.add(plane)
# Create the spline.
points = adsk.core.ObjectCollection.create()
points.add(adsk.core.Point3D.create(0, 8, 0))
points.add(adsk.core.Point3D.create(5, 6, 0))
points.add(adsk.core.Point3D.create(-5, 5, 0))
sketch2Curves = sketch2.sketchCurves
spline = sketch2Curves.sketchFittedSplines.add(points)
# Create sketch rectangle
sketch2Lines = sketch2Curves.sketchLines
startPoint2 = adsk.core.Point3D.create(-4, 2, 0)
endPoint2 = adsk.core.Point3D.create(3, 4, 0)
sketch2Lines.addTwoPointRectangle(startPoint2, endPoint2)
# Get the profile of the second sketch
prof2 = sketch2.profiles.item(0)
# Create an extrusion input
extrudes2 = subComp2.features.extrudeFeatures
extInput2 = extrudes2.createInput(prof2, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
# Define that the extent is a distance extent of 2 cm
extent_distance_2 = adsk.fusion.DistanceExtentDefinition.create(adsk.core.ValueInput.createByString("2cm"))
# Define that the taple angle is 10 degree
deg10 = adsk.core.ValueInput.createByString("10 deg")
extInput2.setOneSideExtent(extent_distance_2, adsk.fusion.ExtentDirections.PositiveExtentDirection, deg10)
# Set the extrude type to be solid
extInput2.isSolid = True
# Create the extrusion
ext2 = extrudes2.add(extInput2)
# Get the body with the first extrude
body = ext1.bodies.item(0)
# Get faces
faceList = []
for face in body.faces:
faceList.append(face)
# Get curves
curveList = []
for curve in sketch2Curves:
curveList.append(curve)
# Get points
for point in sketch2.sketchPoints:
curveList.append(point)
# Get the body with the second extrude
body2 = ext2.bodies.item(0)
# Get eges
for edge in body2.edges:
curveList.append(edge)
# Get construction axis
curveList.append(rootComp.yConstructionAxis)
# Get construction point
curveList.append(rootComp.originConstructionPoint)
sketches3 = subComp3.sketches
# Create a sketch in sub component 3
skAlongVecProject = sketches3.add(rootComp.yZConstructionPlane)
# sketch project to surface (along vector)
projectedEntities = skAlongVecProject.projectToSurface(faceList, curveList, adsk.fusion.SurfaceProjectTypes.AlongVectorSurfaceProjectType, rootComp.xConstructionAxis)
projectedEntities = []
# Create a sketch in sub component 3
skClosestPtProject = sketches3.add(rootComp.yZConstructionPlane)
# sketch project to surface (closest point)
projectedEntities = skClosestPtProject.projectToSurface(faceList, curveList, adsk.fusion.SurfaceProjectTypes.ClosestPointSurfaceProjectType)
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/Geometry/Point3D.h>
#include <Core/UserInterface/UserInterface.h>
#include <Core/Application/ObjectCollection.h>
#include <Core/Geometry/Matrix3D.h>
#include <Fusion/Construction/ConstructionPlanes.h>
#include <Fusion/Construction/ConstructionPlane.h>
#include <Fusion/Construction/ConstructionPlaneInput.h>
#include <Fusion/Construction/ConstructionAxes.h>
#include <Fusion/Construction/ConstructionAxis.h>
#include <Fusion/Construction/ConstructionAxisInput.h>
#include <Fusion/Construction/ConstructionPoints.h>
#include <Fusion/Construction/ConstructionPointInput.h>
#include <Fusion/Construction/ConstructionPoint.h>
#include <Fusion/Fusion/Design.h>
#include <Fusion/Sketch/Sketch.h>
#include <Fusion/Sketch/Sketches.h>
#include <Fusion/Sketch/SketchCurves.h>
#include <Fusion/Sketch/SketchCurve.h>
#include <Fusion/Sketch/SketchPoints.h>
#include <Fusion/Sketch/SketchPoint.h>
#include <Fusion/Sketch/SketchLines.h>
#include <Fusion/Sketch/SketchLine.h>
#include <Fusion/Sketch/SketchFittedSplines.h>
#include <Fusion/Sketch/SketchFittedSpline.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/Features/DistanceExtentDefinition.h>
#include <Fusion/BRep/BRepBodies.h>
#include <Fusion/BRep/BRepBody.h>
#include <Fusion/BRep/BRepFaces.h>
#include <Fusion/BRep/BRepFace.h>
#include <Fusion/BRep/BRepEdges.h>
#include <Fusion/BRep/BRepEdge.h>
#include <Fusion/Components/Occurrence.h>
#include <Fusion/Components/Occurrences.h>
#include <Fusion/Components/Component.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> 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 three sub components under root component
Ptr<Occurrences> occs = rootComp->occurrences();
if (!occs)
return false;
Ptr<Matrix3D> transform = adsk::core::Matrix3D::create();
if (!transform)
return false;
Ptr<Occurrence> subOcc1 = occs->addNewComponent(transform);
if (!subOcc1)
return false;
Ptr<Component> subComp1 = subOcc1->component();
if (!subComp1)
return false;
Ptr<Occurrence> subOcc2 = occs->addNewComponent(transform);
if (!subOcc2)
return false;
Ptr<Component> subComp2 = subOcc2->component();
if (!subComp2)
return false;
Ptr<Occurrence> subOcc3 = occs->addNewComponent(transform);
if (!subOcc3)
return false;
Ptr<Component> subComp3 = subOcc3->component();
if (!subComp3)
return false;
// Create sketch 1 in sub component 1
Ptr<Sketches> sketches1 = subComp1->sketches();
if (!sketches1)
return false;
Ptr<ConstructionPlane> yzPlane = rootComp->yZConstructionPlane();
if (!yzPlane)
return false;
Ptr<Sketch> sketch1 = sketches1->add(yzPlane);
if (!sketch1)
return false;
// Get sketch curves
Ptr<SketchCurves> sketchCurves = sketch1->sketchCurves();
if (!sketchCurves)
return false;
// Get sketch lines
Ptr<SketchLines> sketchLines = sketchCurves->sketchLines();
if (!sketchLines)
return false;
// Create sketch rectangle
Ptr<Point3D> startPoint = Point3D::create(-8.0, 0, 0);
Ptr<Point3D> endPoint = Point3D::create(8.0, 8.0, 0);
sketchLines->addTwoPointRectangle(startPoint, endPoint);
// Get the profile
Ptr<Profiles> profs1 = sketch1->profiles();
if (!profs1)
return false;
Ptr<Profile> prof1 = profs1->item(0);
// Create an extrusion input
Ptr<Features> feats1 = subComp1->features();
if (!feats1)
return false;
Ptr<ExtrudeFeatures> extrudes1 = feats1->extrudeFeatures();
if (!extrudes1)
return false;
Ptr<ExtrudeFeatureInput> extInput1 = extrudes1->createInput(prof1, FeatureOperations::NewBodyFeatureOperation);
// Define that the extent is a distance extent of 2 cm
Ptr<ValueInput> distance1 = ValueInput::createByReal(2.0);
// Set the distance extent
extInput1->setDistanceExtent(false, distance1);
// Set the extrude type to be solid
extInput1->isSolid(true);
// Create the extrusion
Ptr<ExtrudeFeature> ext1 = extrudes1->add(extInput1);
if (!ext1)
return false;
// Create construction plane
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(8.0);
planeInput->setByOffset(rootComp->yZConstructionPlane(), offsetValue);
Ptr<ConstructionPlane> plane = planes->add(planeInput);
// Create sketch 2 in sub component 2
Ptr<Sketches> sketches2 = subComp2->sketches();
if (!sketches2)
return false;
Ptr<Sketch> sketch2 = sketches2->add(plane);
if (!sketch2)
return false;
// Create an object collection for the points.
Ptr<ObjectCollection> points = ObjectCollection::create();
if (!points)
return false;
// Define the points the spline with fit through.
points->add(Point3D::create(0, 8, 0));
points->add(Point3D::create(5, 6, 0));
points->add(Point3D::create(-5, 5, 0));
// Get sketch curves
Ptr<SketchCurves> sketch2Curves = sketch2->sketchCurves();
if (!sketch2Curves)
return false;
// Create the spline.
Ptr<SketchFittedSplines> splines = sketch2Curves->sketchFittedSplines();
if (!splines)
return false;
Ptr<SketchFittedSpline> spline = splines->add(points);
if (!spline)
return false;
// Get sketch lines
Ptr<SketchLines> sketch2Lines = sketch2Curves->sketchLines();
if (!sketch2Lines)
return false;
// Create sketch rectangle
Ptr<Point3D> startPoint2 = Point3D::create(-4, 2, 0);
Ptr<Point3D> endPoint2 = Point3D::create(3, 4, 0);
sketch2Lines->addTwoPointRectangle(startPoint2, endPoint2);
// Get the profile
Ptr<Profiles> profs2 = sketch2->profiles();
if (!profs2)
return false;
Ptr<Profile> prof2 = profs2->item(0);
// Create an extrusion input
Ptr<Features> feats2 = subComp2->features();
if (!feats2)
return false;
Ptr<ExtrudeFeatures> extrudes2 = feats2->extrudeFeatures();
if (!extrudes2)
return false;
Ptr<ExtrudeFeatureInput> extInput2 = extrudes2->createInput(prof2, FeatureOperations::NewBodyFeatureOperation);
// Create distance value input
Ptr<ValueInput> cm2 = adsk::core::ValueInput::createByString("2 cm");
// Create taper angle value input
Ptr<ValueInput> deg10 = adsk::core::ValueInput::createByString("10 deg");
// Create a distance extent definition
Ptr<DistanceExtentDefinition> extent_distance_2 = adsk::fusion::DistanceExtentDefinition::create(cm2);
extInput2->setOneSideExtent(extent_distance_2, adsk::fusion::ExtentDirections::PositiveExtentDirection, deg10));
// Set the extrude type to be solid
extInput2->isSolid(true);
// Create the extrusion
Ptr<ExtrudeFeature> ext2 = extrudes2->add(extInput2);
if (!ext2)
return false;
// Get the body with the first extrude
Ptr<BRepBodies> bodies = ext1->bodies();
if (!bodies)
return false;
Ptr<BRepBody> body = bodies->item(0);
if (!body)
return false;
// faces
std::vector<Ptr<BRepFace>> faceVec;
for (Ptr<BRepFace> face : body->faces())
{
faceVec.push_back(face);
}
// curves
std::vector<Ptr<Base>> curveVec;
for (Ptr<SketchCurve> curve : sketch2Curves)
{
curveVec.push_back(curve);
}
Ptr<SketchPoints> sketch2Points = sketch2->sketchPoints();
if (!sketch2Points)
return false;
for (Ptr<SketchPoint> point : sketch2Points)
{
curveVec.push_back(point);
}
// Get the body with the second extrude
Ptr<BRepBodies> bodies2 = ext2->bodies();
if (!bodies2)
return false;
Ptr<BRepBody> body2 = bodies2->item(0);
if (!body2)
return false;
for (Ptr<BRepEdge> edge : body2->edges())
{
curveVec.push_back(edge);
}
curveVec.push_back(rootComp->yConstructionAxis());
curveVec.push_back(rootComp->originConstructionPoint());
Ptr<Sketches> sketches3 = subComp3->sketches();
if (!sketches3)
return false;
// Create a sketch in sub component 3
Ptr<Sketch> skAlongVecProject = sketches3->add(yzPlane);
if (!skAlongVecProject)
return false;
// sketch project to surface (along vector)
std::vector<Ptr<SketchEntity>> projectedEntities = skAlongVecProject->projectToSurface(
faceVec, curveVec, AlongVectorSurfaceProjectType, rootComp->xConstructionAxis());
// Create a sketch in sub component 3
Ptr<Sketch> skClosestPtProject = sketches3->add(yzPlane);
projectedEntities.clear();
// sketch project to surface (closest point)
projectedEntities = skClosestPtProject->projectToSurface(faceVec, curveVec, ClosestPointSurfaceProjectType);
return true;
}
import { adsk } from "@adsk/fas";
// Params
// {
// "useCurrentDocument": false,
// "saveAsNewDocument": false,
// "message": "",
// "hubId": "wip1fqaautodesk4298",
// "fileURN": "urn:adsk.wipqa:dm.lineage:WlSCDh7RQN6zD2btrrO4SA"
// }
function run() {
// Read the parameters passed with the script
const scriptParameters = JSON.parse(adsk.parameters);
if (!scriptParameters) throw Error("Invalid parameters provided.");
// Get the Fusion API's application object
const app = adsk.core.Application.get();
if (!app) throw Error("No asdk.core.Application.");
// const doc: adsk.core.Document = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType);
// Create a new empty document
const doc = getDocument(
app,
scriptParameters.useCurrentDocument,
scriptParameters.hubId,
scriptParameters.fileURN,
);
if (!doc) throw Error("Invalid document.");
// Ensure we are in the Design environment.
const design = app.activeProduct as adsk.fusion.Design;
//Get the root component of the active design.
const rootComp = design.rootComponent
const allOccs = rootComp.occurrences
const transform = adsk.core.Matrix3D.create()
// Create three components under root component
const occ1 = allOccs.addNewComponent(transform)
const subComp1 = occ1.component
const occ2 = allOccs.addNewComponent(transform)
const subComp2 = occ2.component
const occ3 = allOccs.addNewComponent(transform)
const subComp3 = occ3.component
// Create a sketch in sub component 1
const sketches1 = subComp1.sketches
const sketch1 = sketches1.add(rootComp.yZConstructionPlane)
// Get sketch lines
const sketchLines = sketch1.sketchCurves.sketchLines
// Create sketch rectangle
const startPoint = adsk.core.Point3D.create(-8.0, 0, 0)
const endPoint = adsk.core.Point3D.create(8.0, 8.0, 0)
sketchLines.addTwoPointRectangle(startPoint, endPoint)
// Get the profile of the first sketch
const prof1 = sketch1.profiles.item(0)
// Create an extrusion input
const extrudes1 = subComp1.features.extrudeFeatures
const extInput1 = extrudes1.createInput(prof1, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
// Define that the extent is a distance extent of 2 cm
const distance1 = adsk.core.ValueInput.createByReal(2.0)
// Set the distance extent
const distanceExtentDef = adsk.fusion.DistanceExtentDefinition.create(distance1)
extInput1.setOneSideExtent(distanceExtentDef, adsk.fusion.ExtentDirections.PositiveExtentDirection)
// Set the extrude type to be solid
extInput1.isSolid = true
// Create the extrusion
const ext1 = extrudes1.add(extInput1)
// Create construction plane
const planes = rootComp.constructionPlanes
const planeInput = planes.createInput()
const offsetValue = adsk.core.ValueInput.createByReal(8.0)
planeInput.setByOffset(rootComp.yZConstructionPlane, offsetValue)
const plane = planes.add(planeInput)
// Create a sketch in sub component 2
const sketches2 = subComp2.sketches
const sketch2 = sketches2.add(plane)
// Create the spline.
const points = adsk.core.ObjectCollection.create()
points.add(adsk.core.Point3D.create(0, 8, 0))
points.add(adsk.core.Point3D.create(5, 6, 0))
points.add(adsk.core.Point3D.create(-5, 5, 0))
const sketch2Curves = sketch2.sketchCurves
const spline = sketch2Curves.sketchFittedSplines.add(points)
// Create sketch rectangle
const sketch2Lines = sketch2Curves.sketchLines
const startPoint2 = adsk.core.Point3D.create(-4, 2, 0)
const endPoint2 = adsk.core.Point3D.create(3, 4, 0)
sketch2Lines.addTwoPointRectangle(startPoint2, endPoint2)
// Get the profile of the second sketch
const prof2 = sketch2.profiles.item(0)
// Create an extrusion input
const extrudes2 = subComp2.features.extrudeFeatures
const extInput2 = extrudes2.createInput(prof2, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
// Define that the extent is a distance extent of 2 cm
const extent_distance_2 = adsk.fusion.DistanceExtentDefinition.create(adsk.core.ValueInput.createByString("2cm"))
// Define that the taple angle is 10 degree
const deg10 = adsk.core.ValueInput.createByString("10 deg")
extInput2.setOneSideExtent(extent_distance_2, adsk.fusion.ExtentDirections.PositiveExtentDirection, deg10)
// Set the extrude type to be solid
extInput2.isSolid = true
// Create the extrusion
const ext2 = extrudes2.add(extInput2)
// Get the body with the first extrude
const body = ext1.bodies.item(0)
// Get faces
const faceList = []
for(let i: number = 0; i < body.faces.count; i++){
faceList.push(body.faces.item(i))
}
// Get curves
const curveList = []
for(let i: number = 0; i < sketch2Curves.count; i++){
curveList.push(sketch2Curves.item(i))
}
// Get points
for(let i: number = 0; i < sketch2.sketchPoints.count; i++){
curveList.push(sketch2.sketchPoints.item(i))
}
// Get the body with the second extrude
const body2 = ext2.bodies.item(0)
// Get eges
for(let i: number = 0; i < body2.edges.count; i++){
curveList.push(body2.edges.item(i))
}
// Get construction axis
curveList.push(rootComp.yConstructionAxis)
// Get construction point
curveList.push(rootComp.originConstructionPoint)
const sketches3 = subComp3.sketches
// Create a sketch in sub component 3
const skAlongVecProject = sketches3.add(rootComp.yZConstructionPlane)
// Create sketch project to surface (along vector)
const projectedEntitiesAlongVector = skAlongVecProject.projectToSurface(faceList, curveList, adsk.fusion.SurfaceProjectTypes.AlongVectorSurfaceProjectType, rootComp.xConstructionAxis)
// Create a sketch in sub component 3
const skClosestPtProject = sketches3.add(rootComp.yZConstructionPlane)
// Create sketch project to surface (closest point)
const projectedEntitiesClosestPoint = skClosestPtProject.projectToSurface(faceList, curveList, adsk.fusion.SurfaceProjectTypes.ClosestPointSurfaceProjectType)
saveDocument(
doc,
scriptParameters.saveAsNewDocument,
scriptParameters.message,
doc.dataFile.parentFolder,
);
while (app.hasActiveJobs) {
wait(2000);
}
}
function wait(ms: number) {
const start = new Date().getTime();
while (new Date().getTime() - start < ms) adsk.doEvents();
}
function getDocument(
app: adsk.core.Application,
useCurrentDocument: boolean,
hubId: string,
fileURN: string,
): adsk.core.Document {
if (useCurrentDocument === true) {
adsk.log(`Using currently open document: ${app.activeDocument.name}.`);
return app.activeDocument;
}
if (hubId) {
// Possible hubId formats: base64 encoded string, or business:<id>,
// or personal:<id> (deprecated)
const hub =
app.data.dataHubs.itemById(hubId) ||
app.data.dataHubs.itemById(`a.${adsk.btoa(`business:${hubId}`, true)}`) ||
app.data.dataHubs.itemById(`a.${adsk.btoa(`personal:${hubId}`, true)}`);
if (!hub) throw Error(`Hub with id ${hubId} not found.`);
adsk.log(`Setting hub: ${hub.name}.`);
app.data.activeHub = hub;
}
const file = app.data.findFileById(fileURN);
if (!file) throw Error(`File not found ${fileURN}.`);
adsk.log(`Opening ${file.name}`);
const document = app.documents.open(file, true);
if (!document) throw Error(`Cannot open file ${file.name}.`);
return document;
}
function saveDocument(
doc: adsk.core.Document,
saveAsNewDocument: boolean,
message: string,
destinationFolder: adsk.core.DataFolder,
): boolean {
if (saveAsNewDocument) {
adsk.log("Saving as new document.");
try {
destinationFolder.parentProject;
} catch (e) {
adsk.log(
"Destination folder is not in a project, setting folder to Fusion Automation Service project.",
);
destinationFolder = defaultFolder(
doc.parent,
"Fusion Automation Service",
);
}
if (
doc.saveAs(doc.name + " Additive Ready", destinationFolder, message, "")
) {
adsk.log("Document saved successfully.");
return true;
} else {
adsk.log("Document failed to save.");
return false;
}
}
if (!doc.isModified) {
adsk.log("Document not modified, not saving.");
return true;
}
adsk.log(`Saving with message: "${message}".`);
if (doc.save(message)) {
adsk.log("Document saved successfully.");
return true;
} else {
adsk.log("Document failed to save.");
return false;
}
}
function defaultFolder(app: adsk.core.Application, defaultProjectName: string) {
const projects = app.data.activeHub.dataProjects;
if (!projects) throw Error("Unable to get active hub's projects.");
for (let i = 0; i < projects.count; ++i) {
const project = projects.item(i)!;
if (project.name === defaultProjectName) {
return project.rootFolder;
}
}
adsk.log(`Creating new project: ${defaultProjectName}`);
const project = projects.add(defaultProjectName);
if (!project) throw Error("Unable to create new project.");
return project.rootFolder;
}
run();