Creating a multi-layer copper zone with pcbnew's Python API

Published on September 22, 2026 by leZ

Apply the same copper zone to several layers at once with an LSET, instead of duplicating the zone layer by layer — with pcbnew or KiCad's IPC API.

A single copper zone filled on both F.Cu and B.Cu, defined with an LSET in Python in KiCad — One zone, filled on both F.Cu and B.Cu.

The copper zone tutorial creates a zone on a single layer via SetLayer. For an identical ground plane on both the top and bottom of the board, SetLayerSet applies the same zone to a set of layers as one object, instead of duplicating one per layer.

Applying the zone to several layers

LSET (Layer Set) represents a set of layers; assign it to the zone with SetLayerSet:

from pcbnew import LSET, F_Cu, B_Cu

layers = LSET()
layers.AddLayer(F_Cu)
layers.AddLayer(B_Cu)
zone.SetLayerSet(layers)

Same idea: zone.layers directly accepts a list of layers (resolved by name via get_layer_by_name), rather than a single layer:

from kipy import KiCad

board = KiCad().get_board()
zone.layers = [board.get_layer_by_name("F.Cu"), board.get_layer_by_name("B.Cu")]
board.update_items(zone)

Going further

A multi-layer zone shares the same outline across every selected layer — handy for a symmetric ground plane, but if the layers need different outlines (say, to dodge different components on each side), you’re back to separate zones, one per layer.