TypeError: CombineFeatures_createInput() takes exactly 3 arguments (2 given).

[Anonymous]

I am trying to combine 3 solid bodies using the CombineFeatures in script environment. The part highlighted in blue is the target body, the other 2 bodies are tool bodies. However, I kept getting this error message:

TypeError: CombineFeatures_createInput() takes exactly 3 arguments (2 given). 

I have looked up the createInput() method, which requires only 2 arguments, I don't understand what should the 3rd argument to be. Below is a section of my code:

# Combine 3 solid bodies together

tool_bodies = adsk.core.ObjectCollection.create()

tool_bodies.add(rootComp.bRepBodies[0])

tool_bodies.add(rootComp.bRepBodies[2])

combines = adsk.fusion.CombineFeatures

combine_input = combines.createInput(rootComp.bRepBodies[1], tool_bodies)

Many thanks in advance.

[BrianEkins]

I'm not seeing the same problem.  My code below works as expected where the first body is the target and the next two are used as tool bodies.

def run(context):
    try:
        app = adsk.core.Application.get()
        ui = app.userInterface
        des = adsk.fusion.Design.cast(app.activeProduct)
        root = des.rootComponent
        
        combineFeatures = root.features.combineFeatures
        targetBody = root.bRepBodies[0]
        
        toolBodies = adsk.core.ObjectCollection.create()
        toolBodies.add(root.bRepBodies[1])
        toolBodies.add(root.bRepBodies[2])
        
        combineInput = combineFeatures.createInput(targetBody, toolBodies)
        combineInput.operation = adsk.fusion.FeatureOperations.CutFeatureOperation
        combineInput.isKeepToolBodies = False
        combineFeatures.add(combineInput)
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[Anonymous]

That's really weird...I still keep getting the same error. Do you mind taking a look at my whole code?

[BrianEkins]

Feel free to post it here, or you can send it to me directly using the email in my signature.

[Anonymous]

Thank you. Below is my code. Its a bit longwinded, as I am just working out the workflow first without simplifying it. Also, there are 3 parts where external data points are imported as csv, which I have replaced the actual file location with the pseudo 'filelocation'. Many thanks.

import adsk.core, adsk.fusion, adsk.cam, traceback
import io

def run(context):
    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)
        title = 'Create mask'
        rootComp = design.rootComponent
        
        
        if not design:
            ui.messageBox('No active Fusion design', title)
            return
  
        # import points in csv file: spline_points
        filename = r'filelocation.csv'
        with io.open(filename, 'r', encoding='utf-8-sig') as f:
            spline_points = adsk.core.ObjectCollection.create()
            line = f.readline()
            data = []
            while line:
                pntStrArr = line.split(',')
                for pntStr in pntStrArr:
                    try:
                        data.append(float(pntStr))
                    except:
                        break
            
                if len(data) >= 3 :
                    point = adsk.core.Point3D.create(data[0], data[1], data[2])
                    spline_points.add(point)
                line = f.readline()
                data.clear()            
        
        # Sketch spline through imported points: 
        # xYConstructionPlane, sketch0, seal_spline        
        if spline_points.count:
            sketch0 = rootComp.sketches.add(rootComp.xYConstructionPlane)
            seal_spline= sketch0.sketchCurves.sketchFittedSplines.add(spline_points)
        else:
            ui.messageBox('No valid points', title)  
            
        # Create sweep profile from imported csv points
        filename = r'filelocation.csv'
        with io.open(filename, 'r', encoding='utf-8-sig') as f:
            prof_points = adsk.core.ObjectCollection.create()
            line = f.readline()
            data = []
            while line:
                pntStrArr = line.split(',')
                for pntStr in pntStrArr:
                    try:
                        data.append(float(pntStr))
                    except:
                        break

        # Create points from imported csv data
                if len(data) >= 3 :
                    point = adsk.core.Point3D.create(data[0], data[1], data[2])
                    prof_points.add(point)
                line = f.readline()
                data.clear() 
        
        # Create sketch1 from xYConstructionPlane
        sketch1 = rootComp.sketches.add(rootComp.xYConstructionPlane)    
        lines = sketch1.sketchCurves.sketchLines
        line1 = lines.addByTwoPoints(prof_points[0], prof_points[1])
        line2 = lines.addByTwoPoints(line1.endSketchPoint, prof_points[2])
        line3 = lines.addByTwoPoints(line2.endSketchPoint, prof_points[3])
        line4 = lines.addByTwoPoints(line3.endSketchPoint, line1.startSketchPoint)
                
        # Create the sweep: seal_sweep
        sweeps = rootComp.features.sweepFeatures # Create a sweep input: sweeps
        prof = sketch1.profiles[0] # Define profile for sweep function
        path = rootComp.features.createPath(seal_spline) # Define path for sweep function
        sweepInput = sweeps.createInput(prof, path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        
        seal_sweep= sweeps.add(sweepInput)
        
        # Create new profiles for patch loft: xYConstructionPlane, sketch2, circle0-3      
        # Import offset data
        filename = r'filelocation.csv'
        with io.open(filename, 'r', encoding='utf-8-sig') as f:
            circle_ref = adsk.core.ObjectCollection.create()
            line = f.readline()
            data = []
            while line:
                pntStrArr = line.split(',')
                for pntStr in pntStrArr:
                    try:
                        data.append(float(pntStr))
                    except:
                        break
                if len(data) >=3:
                    point = adsk.core.Point3D.create(data[0],data[1],data[2])
                    circle_ref.add(point)
                line = f.readline()
                data.clear()
        
        # Create 4 circles from first point in circle_ref
        sketch2 = rootComp.sketches.add(rootComp.xYConstructionPlane)
        circles = sketch2.sketchCurves.sketchCircles
        circle0 = circles.addByCenterRadius(circle_ref[0], 0.1)
        circle1 = circles.addByCenterRadius(circle_ref[0], 0.12)
        circle2 = circles.addByCenterRadius(circle_ref[1], 0.1)
        circle3 = circles.addByCenterRadius(circle_ref[1], 0.12)
        
        # Create patch loft:
        # Define profiles:
        # Profile0
        body = rootComp.bRepBodies.itemByName('Body1')        
        edges = body.edges
            
        path0 = adsk.fusion.Path.create(edges[6], adsk.fusion.ChainedCurveOptions.connectedChainedCurves)
        path1 = adsk.fusion.Path.create(edges[1], adsk.fusion.ChainedCurveOptions.connectedChainedCurves)
       
        # Define profiles for patch loft
        profile0 = path0         
        profile1 = sketch2.profiles.item(1)
        profile2 = sketch2.profiles.item(0)
        profile3 = path1
        profile4 = sketch2.profiles.item(3)
        profile5 = sketch2.profiles.item(2)
        
        # Create loft feature input0 for inner patch loft
        loftInput0 = rootComp.features.loftFeatures.createInput(adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        loftSectionObj0 = loftInput0.loftSections
        loftSectionObj0.add(profile0)
        loftSectionObj0.add(profile1)
        loftSectionObj0.add(profile2)
        
        # Create loft feature input1 for outer patch loft
        loftInput1 = rootComp.features.loftFeatures.createInput(adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        loftSectionObj1 = loftInput1.loftSections
        loftSectionObj1.add(profile3)
        loftSectionObj1.add(profile4)
        loftSectionObj1.add(profile5)
        
        # Create loft feature input2 to close the inlet end
        loftInput2 = rootComp.features.loftFeatures.createInput(adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        loftSectionObj2 = loftInput2.loftSections
        loftSectionObj2.add(profile2)
        loftSectionObj2.add(profile5)

        # Create loft feature input3 to close the seal end
        loftInput3 = rootComp.features.loftFeatures.createInput(adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        loftSectionObj3 = loftInput3.loftSections
        loftSectionObj3.add(profile0)
        loftSectionObj3.add(profile3)
        
        # Create loft feature        
        loftInput0.isSolid = False
        loftInput1.isSolid = False
        loftInput2.isSolid = False
        loftInput3.isSolid = False

        shell_inner = rootComp.features.loftFeatures.add(loftInput0)
        shell_outer = rootComp.features.loftFeatures.add(loftInput1)
        close_inlet = rootComp.features.loftFeatures.add(loftInput2)
        close_seal = rootComp.features.loftFeatures.add(loftInput3)
        
        # Stich the four patch lofts
        # Define tolerance with 1 cm.
        tolerance = adsk.core.ValueInput.createByReal(1.0)
        
        # Create a stitch input to be able to define the input needed for an stitch.
        stitch = rootComp.features.stitchFeatures
        surfaces = adsk.core.ObjectCollection.create()
        for i in range(rootComp.bRepBodies.count-1):
            surfaces.add(rootComp.bRepBodies.item(i+1))
            
        stitchInput = stitch.createInput(surfaces, tolerance, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        
        # Create a stitch feature.
        the_body = stitch.add(stitchInput)
        
        # Create inlet from extrusion
        # Identify profile for extrusion through areas comparison
        profiles = sketch2.profiles
    
        # Create extrude: inlet
        extrudes = rootComp.features.extrudeFeatures
        extrude_input = extrudes.createInput(profiles[1], adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        distance = adsk.core.ValueInput.createByString('0.5mm')
        extrude_distance = adsk.fusion.DistanceExtentDefinition.create(distance)
        extrude_input.setOneSideExtent(extrude_distance, adsk.fusion.ExtentDirections.PositiveExtentDirection)
        inlet = extrudes.add(extrude_input)
        
        # Combine 3 solid bodies together
        targetbody = rootComp.bRepBodies[1]
        
        tool_bodies = adsk.core.ObjectCollection.create()
        tool_bodies.add(rootComp.bRepBodies[0])
        tool_bodies.add(rootComp.bRepBodies[2])
            
        combines = adsk.fusion.CombineFeatures        
        combine_input = combines.createInput(targetbody, tool_bodies)        
        combine_input.operation = adsk.fusion.FeatureOperations.JoinFeatureOperation
        combine_input.isKeepToolBodies = False        
        mask = combines.add(combine_input)
        
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[BrianEkins · Accepted solution]

It's a simple mistake that I should have noticed in your original post.  The line:

combines = adsk.fusion.CombineFeatures

should be

combines = rootComp.features.combineFeatures

[Anonymous]

Yes, it is. I have changed and now it works. Thank you Brian.