Moving assembly components with an API script

greenmica — Wed, 20 May 2026 17:07:36 GMT

Hello,

I am creating a biomimetic tail in Fusion360, and I want to model the motion of a cable passing through the ends of the tail segments.

I have printed the tail out using TPU have constrained it to create a helical shape. I want to model this helical shape using Fusion's API, and I have written an AI-assisted code to demonstrate that the math works.

Primary Issue:

When the script is run, there is a new sketch created that models the mathematical motion I wanted, however none of the segments in the assembly move with the points. I have suppressed all constraints and joints before running the script, but I have not placed all of the segments at one origin.

Any suggestions on how to get the pieces to move according to the API script?

Re: Moving assembly components with an API script

kandennti — Thu, 21 May 2026 08:31:09 GMT

Hi @greenmica -san.

If possible, I would have liked to see a sample.

I think calling `fusion.Design.computeAll` will solve the problem.

# Fusion360API Python script import traceback import adsk import adsk.core as core import adsk.fusion as fusion def run(context): ui: core.UserInterface = None try: app: core.Application = core.Application.get() ui = app.userInterface # Create a new document with parametric (hybrid) design mode app.documents.add(core.DocumentTypes.FusionDesignDocumentType) des: fusion.Design = app.activeProduct des.designType = fusion.DesignTypes.ParametricDesignType root: fusion.Component = des.rootComponent # Create a sketch on the XY plane skt: fusion.Sketch = root.sketches.add(root.xYConstructionPlane) # Add 5 control points and create a fitted spline pts: core.ObjectCollection = core.ObjectCollection.create() pts.add(core.Point3D.create(-5, 0, 0)) pts.add(core.Point3D.create(2, 3, 0)) pts.add(core.Point3D.create(4, 1, 0)) pts.add(core.Point3D.create(6, 4, 0)) pts.add(core.Point3D.create(8, 0, 0)) spline: fusion.SketchFittedSpline = skt.sketchCurves.sketchFittedSplines.add(pts) # Create cylinder components jointed to control points 2, 3, 4 (index 1, 2, 3) add_cylinder_component(root, spline, 1) add_cylinder_component(root, spline, 2) add_cylinder_component(root, spline, 3) # Refresh the viewport and notify that components were created adsk.doEvents() app.activeViewport.refresh() ui.messageBox("3 cylinder components created and jointed to control points 2, 3, 4.") # Move spline control points 2, 3, 4 offsets: list[tuple[float, float, float]] = [ (0, 3, 0), (0, -3, 0), (0, 3, 0), ] for i, (dx, dy, dz) in enumerate(offsets): spline.fitPoints.item(i + 1).move(core.Vector3D.create(dx, dy, dz)) # Refresh the viewport and notify that control points were moved adsk.doEvents() app.activeViewport.refresh() ui.messageBox("Spline control points 2, 3, 4 moved.") # Recompute all features to update joint positions after moving spline control points des.computeAll() ui.messageBox("Computing all features to update component positions...") except Exception: if ui: ui.messageBox("Failed:\n{}".format(traceback.format_exc())) def add_cylinder_component( root: fusion.Component, spline: fusion.SketchFittedSpline, fit_pt_idx: int, ) -> fusion.Joint: """Create a cylinder component and rigidly joint it to a spline fit point.""" occ: fusion.Occurrence = root.occurrences.addNewComponent(core.Matrix3D.create()) occ.isGroundToParent = False comp: fusion.Component = occ.component cyl_skt: fusion.Sketch = comp.sketches.add(comp.xYConstructionPlane) cyl_skt.sketchCurves.sketchCircles.addByCenterRadius( core.Point3D.create(0, 0, 0), 1.0 ) prof: fusion.Profile = cyl_skt.profiles.item(0) ext_input: fusion.ExtrudeFeatureInput = comp.features.extrudeFeatures.createInput( prof, fusion.FeatureOperations.NewBodyFeatureOperation ) ext_input.setDistanceExtent(False, core.ValueInput.createByReal(2.0)) comp.features.extrudeFeatures.add(ext_input) fit_pt: fusion.SketchPoint = spline.fitPoints.item(fit_pt_idx) geo1: fusion.JointGeometry = fusion.JointGeometry.createByPoint(comp.originConstructionPoint) geo2: fusion.JointGeometry = fusion.JointGeometry.createByPoint(fit_pt) joint_input: fusion.JointInput = root.joints.createInput(geo1, geo2) joint_input.setAsRigidJointMotion() return root.joints.add(joint_input)

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Moving assembly components with an API script

Re: Moving assembly components with an API script