Simple Revolve Feature Sample


Creates a new revolve feature, resulting in a new component.

Code Samples

import adsk.core, adsk.fusion, math, traceback

def run(context):
    ui = None
        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)
        if ui: