Sketch fillet and offset API 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
        
        # Get the root component of the active design.
        rootComp = design.rootComponent

        # Create a new sketch on the xy plane.
        sketches = rootComp.sketches
        xyPlane = rootComp.xYConstructionPlane
        sketch = sketches.add(xyPlane)

        # Draw two connected lines.
        lines = sketch.sketchCurves.sketchLines
        line1 = lines.addByTwoPoints(adsk.core.Point3D.create(0, 0, 0), adsk.core.Point3D.create(3, 1, 0))
        line2 = lines.addByTwoPoints(line1.endSketchPoint, adsk.core.Point3D.create(1, 4, 0))
        
        # Add a fillet.
        arc = sketch.sketchCurves.sketchArcs.addFillet(line1, line1.endSketchPoint.geometry, line2, line2.startSketchPoint.geometry, 1)

        # Add the geometry to a collection. This uses a utility function that
        # automatically finds the connected curves and returns a collection.
        curves = sketch.findConnectedCurves(line1)
               
        # Create the offset.
        dirPoint = adsk.core.Point3D.create(0, .5, 0)
        offsetCurves = sketch.offset(curves, dirPoint, 0.25)
    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/UserInterface/UserInterface.h>
#include <Core/Geometry/Point3D.h>
#include <Core/Geometry/Line3D.h>
#include <Core/Application/ObjectCollection.h>
#include <Fusion/Fusion/Design.h>
#include <Fusion/Components/Component.h>
#include <Fusion/Sketch/Sketches.h>
#include <Fusion/Sketch/Sketch.h>
#include <Fusion/Sketch/SketchCurves.h>
#include <Fusion/Sketch/SketchLines.h>
#include <Fusion/Sketch/SketchLine.h>
#include <Fusion/Sketch/SketchPoint.h>
#include <Fusion/Sketch/SketchArcs.h>
#include <Fusion/Sketch/SketchArc.h>
#include <Fusion/Construction/ConstructionPlane.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;

    // Create a new sketch on the xy plane.
    Ptr<Sketches> sketches = rootComp->sketches();
    if (!sketches)
        return false;
    Ptr<ConstructionPlane> xyPlane = rootComp->xYConstructionPlane();
    if (!xyPlane)
        return false;
    Ptr<Sketch> sketch = sketches->add(xyPlane);
    if (!sketch)
        return false;

    // Draw two connected lines.
    Ptr<SketchCurves> curves = sketch->sketchCurves();
    if (!curves)
        return false;
    Ptr<SketchLines> lines = curves->sketchLines();
    if (!lines)
        return false;
    Ptr<SketchLine> line1 =
        lines->addByTwoPoints(adsk::core::Point3D::create(0, 0, 0), adsk::core::Point3D::create(3, 1, 0));
    if (!line1)
        return false;
    Ptr<SketchLine> line2 = lines->addByTwoPoints(line1->endSketchPoint(), adsk::core::Point3D::create(1, 4, 0));
    if (!line2)
        return false;

    // Add a fillet.
    Ptr<SketchArcs> arcs = curves->sketchArcs();
    if (!arcs)
        return false;
    Ptr<SketchArc> arc =
        arcs->addFillet(line1, line1->endSketchPoint()->geometry(), line2, line2->startSketchPoint()->geometry(), 1);
    if (!arc)
        return false;

    // Add the geometry to a collection. This uses a utility function that
    // automatically finds the connected curves and returns a collection.
    Ptr<ObjectCollection> connectedCurves = sketch->findConnectedCurves(line1);
    if (!connectedCurves)
        return false;

    // Create the offset.
    Ptr<Point3D> dirPoint = adsk::core::Point3D::create(0, 0.5, 0);
    if (!dirPoint)
        return false;
    Ptr<ObjectCollection> offsetCurves = sketch->offset(connectedCurves, dirPoint, 0.25);
    if (!offsetCurves)
        return false;

    return true;
}