Places components in Pcbnew in KiCad 5.x in a circle

place_circle.py

# Python script to place components in a circle
# based on http://kevincuzner.com/2017/04/28/arranging-components-in-a-circle-with-kicad/
# but ported to Python 3 and KiCad 5.x

# You can just open "Tools->Scripting Console" and paste the whole thing.
# Needs to be in 3 parts: first the import line, then the function definition (and hit enter twice),
# and finally the place_circle call.
# Since refs can't have spaces in the name, I also simplified the list creation with the split function.

import math, pcbnew

def place_circle(refdes, start_angle, center, radius, component_offset=0, hide_ref=True, lock=False):
    """
    Places components in a circle
    refdes: List of component references
    start_angle: Starting angle
    center: Tuple of (x, y) mils of circle center
    radius: Radius of the circle in mils
    component_offset: Offset in degrees for each component to add to angle
    hide_ref: Hides the reference if true, leaves it be if None
    lock: Locks the footprint if true
    """
    pcb = pcbnew.GetBoard()
    deg_per_idx = 360 / len(refdes)
    for idx, rd in enumerate(refdes):
        part = pcb.FindModuleByReference(rd)
        angle = (deg_per_idx * idx + start_angle) % 360;
        print("{0}: {1}".format(rd, angle))
        xmils = center[0] + math.cos(math.radians(angle)) * radius
        ymils = center[1] + math.sin(math.radians(angle)) * radius
        part.SetPosition(pcbnew.wxPoint(pcbnew.FromMils(xmils), pcbnew.FromMils(ymils)))
        part.SetOrientation(angle * -10)
        if hide_ref is not None:
            part.Reference().SetVisible(not hide_ref)
    pcbnew.Refresh()            
    print("Placement finished.")

place_circle("D1 D2 D3 D4 D5 D6 D7 D8".split(), 0, (0, 0), 728)

Hey Frank, thank you for your script. Unfortunately, it no longer works in KiCad 6. I had to replace the FindModuleByReference function with the FindFootprintByReference function. After that everything was OK again.

I am having this issue in Kicad 6 please help

AttributeError: 'BOARD' object has no attribute 'GetModules'

Hi par,
open the affected python script in an editor of your choice and search for
board.GetModules() and replace it with
board.GetFootprints()