Positioning a footprint with pcbnew's Python API

With pcbnew, you retrieve the FOOTPRINT object directly from the in-memory board, usually by its reference designator (U1, R4, etc.):

import pcbnew

board = pcbnew.GetBoard()
fp = board.FindFootprintByReference("U1")

With the IPC API, your script is a separate process talking to a running KiCad instance. You fetch the board, then filter its footprints by reference:

from kipy import KiCad

kicad = KiCad()
board = kicad.get_board()
fp = next(f for f in board.get_footprints() if f.reference_field.text.value == "U1")

Position is set with SetPosition, which expects a VECTOR2I object expressed in KiCad’s internal units (nanometers). Most scripts use an mm → internal-units conversion helper to stay readable:

from pcbnew import VECTOR2I, FromMM

fp.SetPosition(VECTOR2I(FromMM(30), FromMM(20)))

The IPC API works directly in real-world units (mm) through a Vector2 class, with no manual conversion. Changes are then pushed back to KiCad explicitly:

from kipy.geometry import Vector2

fp.position = Vector2.from_xy_mm(30, 20)
board.update_items(fp)

Rotation is set separately, in degrees, with SetOrientationDegrees:

fp.SetOrientationDegrees(90)

On the IPC API side, orientation is an Angle object, not a plain number: build it with Angle.from_degrees, then sync with the same update_items call:

from kipy.geometry import Angle

fp.orientation = Angle.from_degrees(90)
board.update_items(fp)