Is lofting to a single point possible using API?

[Anonymous]

Hello,

I want to create a pyramid like object where base is defined by a polygon (a square, triangle,  star ... any other) and top is one point. Using UI, it is quite simple. I create sketch for a polygon on XY plane, then I create second sketch on offset plane. Offset is in Z-axis and the distance defines the height of the pyramid. The top point is the only content of the second sketch. Then I use loft feature selecting the polygon area and the point. 

I would like to make the same by a python script.  But it doesn't work. It throws an exception when I try to get a profile item from the second sketch.  I understand that loft feature needs two sketch-profile-items. But as I read in the Fusion 360 API Object Model - Sketches - Profiles a points cannot be a profile-item (only loop).

I can make a workaround by creating a circle with very small (but not zero) radius.

Is it possible to make a loft to one point using API?

thanks

A code for creating star-pyramid. Comment and uncomment code to use circle or point.

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

def roll(field):
    #  shift items in an array by one in right to left direction
    #  that first element becomes the last
    #  example: roll([0, 1, 2, 3])  returns: [1, 2, 3, 0]
    #  field:  array of elements to be shifted
    #  retruns: shifted

    new_field = []
    for idx, item in enumerate(field):
        if idx == 0:
            continue
        new_field.append(item)
    new_field.append(field[0])
    return new_field    

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface
               
        product = app.activeProduct
        design = adsk.fusion.Design.cast(product)
        
        rootComp = design.rootComponent

        # star data

        inner_radius = 5
        outer_radius = 10
        num_of_pikes = 5
        z_height = 5
        angle = math.pi/num_of_pikes
        points = []
        
        trigger = True
        for n in range(2*num_of_pikes):
            current_angle = n*angle
            if trigger:
                l = inner_radius
                trigger = False
            else:
                l = outer_radius
                trigger = True
            x = l * math.cos(current_angle)                            
            y = l * math.sin(current_angle)
            z = 0
            points.append([x, y, z])
        
        # Create a new sketch on the xy plane.

        sketches = rootComp.sketches
        xyPlane = rootComp.xYConstructionPlane
        sketch0 = sketches.add(xyPlane)

        # Draw some circles.
        lines = sketch0.sketchCurves.sketchLines

        p0 = adsk.core.Point3D.create(points[0][0], points[0][1], points[0][2])
        p1 = adsk.core.Point3D.create(points[1][0], points[1][1], points[1][2])
        line0 = lines.addByTwoPoints(p0, p1)         
        
        for xyz in roll(points):           
            line1 = lines.addByTwoPoints(line0.endSketchPoint, adsk.core.Point3D.create(xyz[0], xyz[1], xyz[2]))
            line0 = line1
           
        # create offset construction plane
        #
        # Get construction planes
        # Get the profile defined by the circle
        sketch_profile0 = sketch0.profiles.item(0)
           
        planes = rootComp.constructionPlanes
        # Create construction plane input
        planeInput = planes.createInput()
        # Add construction plane by offset
        offsetValue = adsk.core.ValueInput.createByReal(z_height)
        planeInput.setByOffset(sketch_profile0, offsetValue)
        planeOne = planes.add(planeInput)
        
        sketch1 = sketches.add(planeOne)
        
        # circle work
        sketch1_circles = sketch1.sketchCurves.sketchCircles
        sketch1_circles.addByCenterRadius(adsk.core.Point3D.create(0,0,0), 0.0001) 
        # point doesnt work
        # sketch1_points = sketch1.sketchPoints
        # sketch1_points.add(adsk.core.Point3D.create(0, 0, 0))
       
        sketch_profile1 = sketch1.profiles.item(0)
        
        # Create an extrusion input
        loftFeature = rootComp.features.loftFeatures
        loftInput = loftFeature.createInput(adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        loftSectionsObjects =  loftInput.loftSections
        loftSectionsObjects.add(sketch_profile0)
        loftSectionsObjects.add(sketch_profile1)
        loftInput.isSolid = True
        
        # Create loft feature
        loftFeature.add(loftInput)
        
        
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[MichaelT_123 · Accepted solution]

Yes, Mr./Mrs/IRobot Xapo9966

loftSectionsObj.add( point_proxy )

Regards

MichaelT

[Anonymous]

Thanks it works,

Chris

snippet of updated code:

        # circle
        # sketch1_circles = sketch1.sketchCurves.sketchCircles
        # sketch1_circles.addByCenterRadius(adsk.core.Point3D.create(0,0,0), 0.0001) 
        # point
        sketch1_points = sketch1.sketchPoints
        top_point = sketch1_points.add(adsk.core.Point3D.create(0, 0, 0))
       
        # sketch_profile1 = sketch1.profiles.item(0)
        
        # Create an extrusion input
        loftFeature = rootComp.features.loftFeatures
        loftInput = loftFeature.createInput(adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        loftSectionsObjects =  loftInput.loftSections
        loftSectionsObjects.add(sketch_profile0)
        loftSectionsObjects.add(top_point)
        loftInput.isSolid = True