sweep works on rootComponent but not on newOccuranceComponent

[adminTCYL2]

Ich habe im folgenden Code ein möglichst einfaches Sweep erstellt (ein Kreis entlang eines geraden Pfades), um dem Fehler auf die Spur zu kommen. Es funktioniert auf der root Component, wenn ich Zeile 15 aktiviere. Ich will es aber auf der new_occurrence.component zum funktionieren bringen. Eine einfache Extrusion klappt, aber das Sweep bringt folgenden Fehler: 

..... line 24, in run

path = adsk.fusion.Path.create(pathLine, chainedOption)

^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^

File .....line 37652, in create

return _fusion.Path_create(curves, chainOptions)

^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^

RuntimeError: 2 : InternalValidationError : Utils::getObjectPath(obj.get(), objPath, nullptr, contextPath)

Hier mein Code: 

import adsk.core, adsk.fusion, traceback

def run(context😞

    ui = None

    try:

        app = adsk.core.Application.get()

        ui  = app.userInterface

        product = app.activeProduct

        design = adsk.fusion.Design.cast(product)

        new_occurrence = design.rootComponent.occurrences.addNewComponent(adsk.core.Matrix3D.create())

        comp = new_occurrence.component

        comp.isActive = True

        #comp = design.rootComponent

        # create pathline

        path_sketch = comp.sketches.add(comp.xYConstructionPlane)

        pathLine = path_sketch.sketchCurves.sketchLines.addByTwoPoints(adsk.core.Point3D.create(0,0,0), adsk.core.Point3D.create(9,0,0))

        feats = comp.features

        chainedOption = adsk.fusion.ChainedCurveOptions.connectedChainedCurves

        if adsk.fusion.BRepEdge.cast(pathLine😞

            chainedOption = adsk.fusion.ChainedCurveOptions.tangentChainedCurves

        path = adsk.fusion.Path.create(pathLine, chainedOption)

        path = feats.createPath(pathLine)

        # create circle-profile

        radius = 2.5

        profile_sketch = comp.sketches.add(comp.yZConstructionPlane)

        center = comp.yZConstructionPlane.geometry.origin

        center = profile_sketch.modelToSketchSpace(center)

        profile_sketch.sketchCurves.sketchCircles.addByCenterRadius(center, radius)

        profile = profile_sketch.profiles[0]

        # create sweep

        sweepFeats = feats.sweepFeatures

        sweepInput = sweepFeats.createInput(profile, path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

        sweepInput.orientation = adsk.fusion.SweepOrientationTypes.PerpendicularOrientationType

        sweepFeat = sweepFeats.add(sweepInput)

    except:

        if ui:

            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[adminTCYL2]

Jetzt bin ich einen Schritt weiter. Die ChainedOption funktioniert offensichtlich auf der new_occurrence.component nicht. Für mein einfaches Beispiel brauche ich sie nicht. Deaktiviere ich sie, so funktioniert das Sweep. 

import adsk.core, adsk.fusion, traceback

def run(context😞

    ui = None

    try:

        app = adsk.core.Application.get()

        ui  = app.userInterface

        product = app.activeProduct

        design = adsk.fusion.Design.cast(product)

        new_occurrence = design.rootComponent.occurrences.addNewComponent(adsk.core.Matrix3D.create())

        comp = new_occurrence.component

        comp.isActive = True

        #comp = design.rootComponent

        # create pathline

        path_sketch = comp.sketches.add(comp.xYConstructionPlane)

        pathLine = path_sketch.sketchCurves.sketchLines.addByTwoPoints(adsk.core.Point3D.create(0,0,0), adsk.core.Point3D.create(9,0,0))

        # chainedOption = adsk.fusion.ChainedCurveOptions.connectedChainedCurves

        # if adsk.fusion.BRepEdge.cast(pathLine):

        #     chainedOption = adsk.fusion.ChainedCurveOptions.tangentChainedCurves

        # path = adsk.fusion.Path.create(pathLine, chainedOption)

        path = comp.features.createPath(pathLine)

        # create circle-profile

        radius = 2.5

        profile_sketch = comp.sketches.add(comp.yZConstructionPlane)

        center = comp.yZConstructionPlane.geometry.origin

        center = profile_sketch.modelToSketchSpace(center)

        profile_sketch.sketchCurves.sketchCircles.addByCenterRadius(center, radius)

        profile = profile_sketch.profiles[0]

        # create sweep

        sweepFeats = comp.features.sweepFeatures

        sweepInput = sweepFeats.createInput(profile, path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

        sweepInput.orientation = adsk.fusion.SweepOrientationTypes.PerpendicularOrientationType

        sweepFeat = sweepFeats.add(sweepInput)

    except:

        if ui:

            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[kandennti]

Hi @adminTCYL2 -San.

This is a proxy problem.
A one-line modification like this will allow it to run without error.

・・・
        # create pathline
        path_sketch = comp.sketches.add(comp.xYConstructionPlane)
        path_sketch = path_sketch.createForAssemblyContext(new_occurrence) #Add here
        pathLine = path_sketch.sketchCurves.sketchLines.addByTwoPoints(adsk.core.Point3D.create(0,0,0), adsk.core.Point3D.create(9,0,0))
        feats = comp.features
・・・

For more information on proxies, see “Proxies” here.

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-88A4DB43-CFDD-4CFF-B124-7EE67915A07A