Creating a copper zone (ground plane) with pcbnew's Python API

Instantiate a ZONE object, pick its layer, then add it to the board:

import pcbnew

board = pcbnew.GetBoard()
from pcbnew import ZONE, F_Cu

zone = ZONE(board)
zone.SetLayer(F_Cu)
board.Add(zone)

With the IPC API, you instantiate a blank Zone object, then set its type (copper):

from kipy import KiCad
from kipy.board_types import Zone, ZoneType

kicad = KiCad()
board = kicad.get_board()
zone = Zone()
zone.type = ZoneType.ZT_COPPER

The outline is a SHAPE_POLY_SET you append the polygon’s vertices to, in internal units:

from pcbnew import SHAPE_POLY_SET, FromMM

outline = SHAPE_POLY_SET()
outline.NewOutline()
for x, y in [(0, 0), (50, 0), (50, 30), (0, 30)]:
    outline.Append(FromMM(x), FromMM(y))
zone.SetOutline(outline)

On the IPC API side, the outline is built from a PolyLine of nodes (in nanometers, converted with from_mm), wrapped in a PolygonWithHoles:

from kipy.geometry import PolyLine, PolyLineNode
from kipy.common_types import PolygonWithHoles
from kipy.util.units import from_mm

outline = PolyLine()
for x, y in [(0, 0), (50, 0), (50, 30), (0, 30), (0, 0)]:  # last point closes the loop
    outline.append(PolyLineNode.from_xy(from_mm(x), from_mm(y)))

polygon = PolygonWithHoles()
polygon.outline = outline

zone.outline = polygon
zone.layers = [board.get_layer_by_name("F.Cu")]

Attach the zone to a net, then trigger the fill through ZONE_FILLER:

from pcbnew import ZONE_FILLER

zone.SetNet(board.FindNet("GND"))

filler = ZONE_FILLER(board)
filler.Fill(board.Zones())

Same idea for attaching the net. This is also the point, once every property is set, where the zone is actually created on the board — there’s no confirmed method for triggering a fill programmatically via the IPC API yet:

from kipy.board_types import Net

zone.net = Net(name="GND")
board.create_items(zone)