Performing a Patch Sweep in the API

[Anonymous]

I'm trying to recreate a helical sweep operation in the API, I want to use a sketch line as the sweep profile to create a helical path on which I can then do a solid sweep along but am having trouble finding out how to perform this patch sweep using the API. 

Trying to sweep the sketch line at the top of the construction line through the path to create an offset patch I can twist around the shaft.

Currently working in python, I've attempted to create the sweep but I'm unclear on how to use the patch feature in relation to the sweep feature. The current script is as follows:

        # Assign variables - units are in cm
        pitch_ratio = 0.2456    # use a dictionary for future use, this is a test value
        
        screw_radius = 100
        shaft_radius = 50
        screw_angle_deg = 22
        screw_angle = math.degrees(screw_angle_deg)
        head = 200
        
        screw_length = (head + screw_radius) / math.sin(screw_angle)
        pitch = ((2*math.pi*pitch_ratio) / math.tan(screw_angle)) * screw_radius

        
        revolutions = screw_length / pitch
        twist_angle = revolutions * 360
        
        print('Variables Assigned:\nScrew Radius = %s m\nShaft Radius = %s m\nScrew Length = %s m\nTwist Angle = %s°\n' % (screw_radius/100, shaft_radius/100, screw_length/100, twist_angle))
        
        # Document setup        

        app = adsk.core.Application.get()
        ui  = app.userInterface
        design = app.activeProduct
        
        # Get the root component of the design and create a sub component
        rootComp = design.rootComponent
        newOcc = rootComp.occurrences.addNewComponent(adsk.core.Matrix3D.create())
        screwComp = newOcc.component
        screwComp.name = 'Archimedean Hydroscrew'
        
        shaftOcc = screwComp.occurrences.addNewComponent(adsk.core.Matrix3D.create())
        shaftComp = shaftOcc.component
        shaftComp.name = 'Shaft'
        bladeOcc = screwComp.occurrences.addNewComponent(adsk.core.Matrix3D.create())
        bladeComp = bladeOcc.component
        bladeComp.name = 'Blades'
        

        # Create a sketch on xy (Front) and yz (Right) planes of the screw sub component
        sketches = screwComp.sketches
        shaft_sketches = shaftComp.sketches
        blade_sketches = bladeComp.sketches
        xyPlane = screwComp.xYConstructionPlane
        yzPlane = screwComp.yZConstructionPlane
        
        shaft_profile_sketch = shaft_sketches.add(xyPlane)
        shaft_profile_sketch.name = 'Shaft Profile'
        screw_path_sketch = sketches.add(xyPlane)
        screw_path_sketch.name = 'Screw_Path'
        
        # Draw the shaft profile and the screw path
        shaft_profile_circles = shaft_profile_sketch.sketchCurves.sketchCircles
        shaft_profile = shaft_profile_circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), shaft_radius)
     
        screw_path_line = screw_path_sketch.sketchCurves.sketchLines
        screw_path = screw_path_line.addByTwoPoints(adsk.core.Point3D.create(0, 0, 0), adsk.core.Point3D.create(0, 0, screw_length))
  
        # Get the profile defined by the circle
        shaft_profile_prof = shaft_profile_sketch.profiles.item(0)
        
        # Create a path form the screw_path
        screw_path_path = shaftComp.features.createPath(screw_path)
        
        # Create a sweep input
        shaft_sweeps = shaftComp.features.sweepFeatures
        shaft_sweep_input = shaft_sweeps.createInput(shaft_profile_prof, screw_path_path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        shaft_sweep_input.taperAngle = adsk.core.ValueInput.createByString('0 deg')
        shaft_sweep_input.twistAngle = adsk.core.ValueInput.createByString('0 deg')
        
        # Create the sweep
        shaft_sweep = shaft_sweeps.add(shaft_sweep_input)
        
        # Create a construction plane at the start of the path
        path_plane = screwComp.constructionPlanes
        path_plane_input = path_plane.createInput()
        distance = adsk.core.ValueInput.createByReal(0.0)
        path_plane_input.setByDistanceOnPath(screw_path, distance)
        path_plane.add(path_plane_input)
        
        # Create a 1D profile for a patch
        blade_patch_sketch = blade_sketches.add(xyPlane)
        blade_patch_sketch.name = 'Blade Patch Profile'
        
        blade_patch_line = blade_patch_sketch.sketchCurves.sketchLines
        blade_patch_offset = blade_patch_line.addByTwoPoints(adsk.core.Point3D.create(0, 0, 0), adsk.core.Point3D.create(0, screw_radius, 0))
        blade_patch_offset.isConstruction = True
        blade_patch_profile = blade_patch_line.addByTwoPoints(adsk.core.Point3D.create(0, screw_radius, 0), adsk.core.Point3D.create(0, screw_radius + 0.01, 0))
        
        # Sweep a blade in the patch workspace - this part is not working
        patch_sweeps = bladeComp.features.sweepFeatures
        patch_prof = blade_patch_sketch.profilecurve.item(0)
        patch_input = patch_sweeps.createInput(patch_prof, screw_path_path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        patch_input.taperAngle = adsk.core.ValueInput.createByString('0 deg')
        patch_input.twistAngle = adsk.core.ValueInput.createByReal(twist_angle)
        patch_input.isSolid = False
        
        patch_sweep = patch_sweeps.add(patch_input)

At the moment, the script produces this error:

Currently getting this error.

Can anyone help with this?

Cheers,

Jack

[goyals]

This error means there is no property like 'profileCurve' on sketch. To get the profile, you need to use 'profiles' property on sketch. It will return all the profiles of a sketch and then you can iterate over it to get a particular profile. I think your sketch contains just a line and no profile there.

[Anonymous]

Yeah I'm trying to sweep in the patch environment as opposed to the model environment, in the patch environment I can sweep using sketch lines I'm trying to figure out how to replicate this in the API.

This should be the end result, a patch sweep of the sketch line that revolves around the shaft.

[goyals]

I am afraid to mention commands of patch environment are not exposed through API unless some one contradicts me.

[BrianEkins · Accepted solution]

Most of the features in the Patch workspace are supported by the API.  In most cases, it's the same feature objects in the API just you just set the isSolid property to False to indicate that a surface should be created.  Here's a sample that creates the geometry you're trying to create.

def sweepTest():
    ui = None
    try:
        app = adsk.core.Application.get()
        ui = app.userInterface
        
        # Create a document.
        doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)
 
        product = app.activeProduct
        design = adsk.fusion.Design.cast(product)

        # Get the root component of the active design.
        rootComp = design.rootComponent
        
        # Create the line that will be the profile.
        profSketch = rootComp.sketches.add(rootComp.xZConstructionPlane)
        sketchLines = profSketch.sketchCurves.sketchLines
        profLine = sketchLines.addByTwoPoints(adsk.core.Point3D.create(0,0,0), 
                                              adsk.core.Point3D.create(0,5,0))
        
        # Create an open profile using the line.
        prof = rootComp.createOpenProfile(profLine, False)
        
        # Create a sketch to draw the path line.
        pathSketch = rootComp.sketches.add(rootComp.yZConstructionPlane)
        sketchLines = pathSketch.sketchCurves.sketchLines
        
        pathLine = sketchLines.addByTwoPoints(adsk.core.Point3D.create(0, 0, 0),
                                              adsk.core.Point3D.create(0, 30, 0))                                 
        
        # Create a path using the line.
        path = rootComp.features.createPath(pathLine)

        # Create a sweep input
        sweeps = rootComp.features.sweepFeatures
        sweepInput = sweeps.createInput(prof, path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        sweepInput.twistAngle = adsk.core.ValueInput.createByReal(math.pi * 5)
        sweepInput.isSolid = False

        # Create the sweep.
        sweep = sweeps.add(sweepInput)
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[Anonymous]

Yep this works perfectly, thanks!