Project To Surface API Sample

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();