Simple Revolve Feature Sample

Description

Demonstrates creates a new revolve feature, resulting in a new component.

Before running: No open document is required; the script creates a new design (or additional documents) as it runs.

Code Samples 

import adsk.core, adsk.fusion, math, 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 a circle.
        circles = sketch.sketchCurves.sketchCircles
        circle1 = circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), 2)
        
        # Draw a line to use as the axis of revolution.
        lines = sketch.sketchCurves.sketchLines
        axisLine = lines.addByTwoPoints(adsk.core.Point3D.create(-1, -5, 0), adsk.core.Point3D.create(1, -5, 0))

        # Get the profile defined by the circle.
        prof = sketch.profiles.item(0)

        # Create an revolution input to be able to define the input needed for a revolution
        # while specifying the profile and that a new component is to be created
        revolves = rootComp.features.revolveFeatures
        revInput = revolves.createInput(prof, axisLine, adsk.fusion.FeatureOperations.NewComponentFeatureOperation)

        # Define that the extent is an angle of pi to get half of a torus.
        angle = adsk.core.ValueInput.createByReal(math.pi)
        revInput.setAngleExtent(False, angle)

        # Create the extrusion.
        ext = revolves.add(revInput)
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
/**
 * Simple Revolve Feature Sample
 * Creates a new revolve feature, resulting in a new component.
 */

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

function run() {

  // Get the Fusion API's application object
  const app = adsk.core.Application.get();
  if (!app) throw Error("No adsk.core.Application.");

  // Create a document.
  const doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)

  // Create a document.
  const design = app.activeProduct as adsk.fusion.Design

  // Get the root component of the active design.
  const rootComp = design.rootComponent

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

  // Draw a circle.
  const circles = sketch.sketchCurves.sketchCircles
  const circle1 = circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), 2)

  // Draw a line to use as the axis of revolution.
  const lines = sketch.sketchCurves.sketchLines
  const axisLine = lines.addByTwoPoints(adsk.core.Point3D.create(-1, -5, 0), adsk.core.Point3D.create(1, -5, 0))

  // Get the profile defined by the circle.
  const prof = sketch.profiles.item(0)

  // Create an revolution input to be able to define the input needed for a revolution
  // while specifying the profile and that a new component is to be created
  const revolves = rootComp.features.revolveFeatures
  const revInput = revolves.createInput(prof, axisLine, adsk.fusion.FeatureOperations.NewComponentFeatureOperation)

  // Define that the extent is an angle of pi to get half of a torus.
  const angle = adsk.core.ValueInput.createByReal(Math.PI)
  revInput.setAngleExtent(false, angle)

  // Create the extrusion.
  const ext = revolves.add(revInput)
}

run();