BaseFeature Sample

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;
}

/**
 * BaseFeature Sample
 * Creates a new base feature.
 */

import { adsk } from '@adsk/fusion';

// 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 adsk.core.Application.");

  // 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

  // Create a base feature
  const baseFeats = rootComp.features.baseFeatures
  const baseFeat = baseFeats.add()

  baseFeat.startEdit()

  // Create construction plane in base feature
  const planes = rootComp.constructionPlanes
  const planeInput = planes.createInput()
  planeInput.targetBaseOrFormFeature = baseFeat
  planeInput.setByOffset(rootComp.xYConstructionPlane, adsk.core.ValueInput.createByReal(1))
  const plane = planes.add(planeInput)

  // Create sketch in base feature
  const sketches = rootComp.sketches
  const sketch = sketches.addToBaseOrFormFeature(plane, baseFeat, true)

  // Draw a circle.
  const circles = sketch.sketchCurves.sketchCircles
  circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), 2)

  // Get the profile defined by the circle.
  const 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

  const extrudes = rootComp.features.extrudeFeatures
  const extInput = extrudes.createInput(prof, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

  // Define that the extent is a distance extent of 5 cm.

  const distance = adsk.core.ValueInput.createByReal(5.0)
  const distanceExtentDef = adsk.fusion.DistanceExtentDefinition.create(distance)
  extInput.setOneSideExtent(distanceExtentDef, adsk.fusion.ExtentDirections.PositiveExtentDirection)
  extInput.targetBaseFeature = baseFeat

  // Create the extrusion.
  const ext = extrudes.add(extInput)

  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();