a version of my pcbannotate.py script that uses native api of kicad

pcbannotate.py

# -*- coding: utf-8 -*-
#
# This script will re-annotate board companents according to their x,y
# positions and back-annotate those changes to schematic files.
#
# Make sure you have backups of all your files!
#
# Forked from https://github.com/cculpepper/kicad-python/blob/master/examples/pcbannotate.py
#
# You should run the script from inside pcbnew script console. After
# running script, re-open your schematic files, update the netlist
# file and import net list changes to pcbnew. This should update some
# net names, but shouldn't change any component footprints.
#
# Copyright © 2015 Hasan Yavuz Özderya
#
# This program is free software; you can redistribute it and/or modify
# it under the terms of the GNU General Public License as published by
# the Free Software Foundation; either version 2 of the License, or
# (at your option) any later version.
#
# This program is distributed in the hope that it will be useful, but
# WITHOUT ANY WARRANTY; without even the implied warranty of
# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.  See the GNU
# General Public License for more details.
#
# You should have received a copy of the GNU General Public License
# along with this program; if not, write to the Free Software
# Foundation, Inc., 51 Franklin Street, Fifth Floor, Boston, MA
# 02110-1301, USA.
#

import pcbnew
import re
import glob
import os
import codecs
import sys

try:
    if len(sys.argv) != 2:
        print("Usage ", __file__, "<board.pcbnew")
        sys.exit(1)

    input_path = sys.argv[1]
    b = pcbnew.LoadBoard(input_path)

except AttributeError:
    b = pcbnew.GetBoard()
    input_path = b.GetFileName()

mods = list(b.GetModules())

def sortkeys(mod):
    return (mod.GetLayer(), mod.GetPosition()[0], mod.GetPosition()[1])
    return (mod.layer, mod.y, mod.x)
    #if mod.layer == Layer.Front:
        #return (mod.layer, mod.y, mod.x)
    #else: # Layer.Back
        ## Components in the back are sorted from right to
        ## left according to their canvas position. When you flip the
        ## board at your hand, they will be sorted 'left to right'.
        #return (mod.layer, mod.y, -mod.x)

mods = sorted(mods, key=sortkeys)

ref_counter = {} # dictionary of reference names
changes = [] # a list of tuples

for mod in mods:
    prev_ref = mod.GetReference()
    m = re.match('^((?:[a-zA-Z_\d]+[a-zA-Z_])|(?:[a-zA-Z_]+))(\d+)$', prev_ref)

    if m:
        name, number = m.groups()  # for ex: R16 -> name:'R' , number: '16'
    else:
        print("Skipping: %s." % prev_ref)
        continue

    if name in ref_counter:
        next_ref = name + str(ref_counter[name]+1)
        ref_counter[name] += 1
    else:
        next_ref = name + str(1)
        ref_counter[name] = 1

    if next_ref == prev_ref:
        continue

    print('Re-naming %s -> %s' % (prev_ref, next_ref))

    mod.SetReference(next_ref)
    changes.append((prev_ref, next_ref))

if changes:
    b.Save(input_path)
    print("PCB annotated.")

    # PCB annotation completed, now back-annotate schematics

    # prepare replacer
    changes = dict(changes)

    def replacer(match):
        return changes[match.group(0)]

    regx = re.compile('|'.join(r'\b%s\b' % k for k in changes.keys()))

    # get a list of schematic files by globbing
    directory = os.path.dirname(input_path)
    sch_files = glob.glob(directory + '/*.sch')

    for sch_file in sch_files:
        print("Updating %s..." % sch_file)
        # read file
        s = codecs.open(sch_file, mode='r+', encoding='utf-8').read()

        # make changes
        s = regx.sub(replacer, s)

        # update file contents
        codecs.open(sch_file, mode='w', encoding='utf-8').write(s)
else:
    print("No changes were made! This is normal if your components were already named in correct order.")

@nrrdzilla I'm sorry I haven't used KiCad in a while so I can't help atm. This is not a complicated script, as long as KiCad python API doesn't change you shouldn't have any problems.

I remember that there were other back annotation scripts on kicad forums. Maybe you can try those? FYI I've also heard that KiCad 6 will have builtin back annotation support.