Help on executing an API custom command

2way3dtext — Thu, 19 Aug 2021 16:58:53 GMT

The following code asks the user to select the desired path and diameter of the pipe, however, nothing occurs after all the inputs are selected.

Would this be an issue with how the inputs are defined?

# Select all of the inputs.

um = des.unitsManager

path_Input = inputs.addSelectionInput('path_Input', 'Path', 'Select path of pipe')

path_Input.setSelectionLimits(1,1)

pipeDiameter_input = inputs.addValueInput('pipeDiameter_Input', 'Diameter', um.defaultLengthUnits, adsk.core.ValueInput.createByString('1'))

# Event handler for the execute event.

class RoundedEndPipeCommandExecuteHandler(adsk.core.CommandEventHandler):

def __init__(self):

super().__init__()

def notify(self, args):

eventArgs = adsk.core.CommandEventArgs.cast(args)

inputs = eventArgs.command.commandInputs

# Get the values of all of the inputs.

path = inputs.itemById('path_Input').selection(0).entity

pipeDiameter = inputs.itemById('pipeDiameter_Input').value

CreateRoundedEndPipe(path, pipeDiameter)

I will be very grateful for any suggestions or feedback on fixing this issue.

Re: Help on executing an API custom command

kandennti — Fri, 20 Aug 2021 00:25:07 GMT

Hi @2way3dtext .

There are many things going on, but the yellow part is an error because it is None.
In addition, when I reached the green part "except:", the error message was not displayed because ui was also None.

Also, when I use UserInterface.selectEntity with the command dialog dialogs displayed, it crashes. (red part)
It has been reported somewhere in the forum that this method is undesirable.

I can't explain it in detail, but I've got it working.
Please compare.

・・・ #Create Rounded End Pipe def CreateRoundedEndPipe(path, pipeDiameter) : try: pipeRadius =pipeDiameter/2 product = _app.activeProduct design = adsk.fusion.Design.cast(product) comp = design.rootComponent selObj: adsk.fusion.BRepEdge = path # create path feats = comp.features chainedOption = adsk.fusion.ChainedCurveOptions.connectedChainedCurves if adsk.fusion.BRepEdge.cast(selObj): chainedOption = adsk.fusion.ChainedCurveOptions.tangentChainedCurves path = adsk.fusion.Path.create(selObj, chainedOption) path = feats.createPath(selObj) # create profile_1 planes = comp.constructionPlanes planeInput_1 = planes.createInput() planeInput_1.setByDistanceOnPath(selObj, adsk.core.ValueInput.createByReal(0)) plane_1 = planes.add(planeInput_1) sketches = comp.sketches sketch_1 = sketches.add(plane_1) center_1 = plane_1.geometry.origin center_1 = sketch_1.modelToSketchSpace(center_1) sketch_1.sketchCurves.sketchCircles.addByCenterRadius(center_1, pipeRadius) profile_1 = sketch_1.profiles[0] # create profile_2 planeInput_2 = planes.createInput() planeInput_2.setByDistanceOnPath(selObj, adsk.core.ValueInput.createByReal(1)) plane_2 = planes.add(planeInput_2) sketches_2 = comp.sketches sketch_2 = sketches_2.add(plane_2) center_2 = plane_2.geometry.origin center_2 = sketch_2.modelToSketchSpace(center_2) circle_2 = sketch_2.sketchCurves.sketchCircles sketch_2.sketchCurves.sketchCircles.addByCenterRadius(center_2, pipeRadius) sk_2 = comp.sketches.add(plane_2) circles_2 = sk_2.sketchCurves.sketchCircles circle_2 = circles_2.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), pipeRadius) lines_2 = sk_2.sketchCurves.sketchLines axisLine_2 = lines_2.addByTwoPoints(adsk.core.Point3D.create(-pipeRadius, 0, 0), adsk.core.Point3D.create(pipeRadius, 0, 0)) profile_2 = sk_2.profiles.item(0) # create profile_3 sketches_3 = comp.sketches sketch_3 = sketches.add(plane_1) center_3 = plane_1.geometry.origin center_3 = sketch_1.modelToSketchSpace(center_1) sketch_3.sketchCurves.sketchCircles.addByCenterRadius(center_1, pipeRadius) profile_3 = sketch_1.profiles[0] sk_3 = comp.sketches.add(plane_1) circles_3 = sk_3.sketchCurves.sketchCircles circle_3 = circles_3.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), pipeRadius) lines_3 = sk_3.sketchCurves.sketchLines axisLine_3 = lines_3.addByTwoPoints(adsk.core.Point3D.create(-pipeRadius, 0, 0), adsk.core.Point3D.create(pipeRadius, 0, 0)) profile_3 = sk_3.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 = comp.features.revolveFeatures revInput_2 = revolves.createInput(profile_2, axisLine_2, adsk.fusion.FeatureOperations.NewComponentFeatureOperation) revInput_3 = revolves.createInput(profile_3, axisLine_3, adsk.fusion.FeatureOperations.NewComponentFeatureOperation) # Define that the extent is an angle of 2*pi to get a sphere angle = adsk.core.ValueInput.createByReal(2*math.pi) revInput_2.setAngleExtent(False, angle) revInput_3.setAngleExtent(False, angle) # Create the extrusion. ext_2 = revolves.add(revInput_2) ext_2 = revolves.add(revInput_3) # create sweep sweepFeats = feats.sweepFeatures sweepInput = sweepFeats.createInput(profile_1, path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) sweepInput.orientation = adsk.fusion.SweepOrientationTypes.PerpendicularOrientationType sweepFeat = sweepFeats.add(sweepInput) _app.activeViewport.refresh() except: if _ui: _ui.messageBox('Failed:\n{}'.format(traceback.format_exc())) ・・・ # Event handler for the commandCreated event. class MyCommandCreatedHandler(adsk.core.CommandCreatedEventHandler): ・・・ path_Input = inputs.addSelectionInput('path_Input', 'Path', 'Select path of pipe') path_Input.setSelectionLimits(1,1) path_Input.addSelectionFilter('Edges') path_Input.addSelectionFilter('SketchCurves') ・・・

Re: Help on executing an API custom command

2way3dtext — Mon, 23 Aug 2021 02:00:37 GMT

Hello @kandennti

Thank you so much for looking over my code and pointing out the lines where the errors arise!

When I revised the code just as you have shown me, the add-in worked perfectly.

Thank you again for your generous time and help.

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Help on executing an API custom command

Re: Help on executing an API custom command

Re: Help on executing an API custom command