#!/usr/bin/env python
import sys
import os
import argparse
from pcbnew import *

parser = argparse.ArgumentParser(description='KiCAD PCB to GERBER converter')

parser.add_argument('--pcb',
                    required=True,
                    dest='pcb',
                    action='store',
                    help='A foo.kicad_pcb file')

parser.add_argument('--output-directory',
                    required=True,
                    dest='output_directory',
                    action='store',
                    help='Directory to store output files')

parser.add_argument('--detect-files-only',
                    dest='detect_files_only',
                    action='store_true',
                    help='Don\'t create the GERBER files, just list the files to be created')

parser.add_argument('--create-drill-map-file',
                    dest='create_drill_map_file',
                    action='store_true',
                    help='Create drill map file')

parser.add_argument('--protel-extensions',
                    dest='protel_extensions',
                    action='store_true',
                    help='Use Protel filename extensions')

args = parser.parse_args()

filename = args.pcb

board = LoadBoard(filename)

plot_plan = [
    ("GTO", board.GetLayerName(F_SilkS), F_SilkS, "Silk front"),
    ("GTS", board.GetLayerName(F_Mask), F_Mask, "Mask front"),
    ("GBO", board.GetLayerName(B_SilkS), B_SilkS, "Silk bottom"),
    ("GBS", board.GetLayerName(B_Mask), B_Mask, "Mask bottom"),
    ("GBR", board.GetLayerName(Edge_Cuts), Edge_Cuts, "Edges"),
]

layers = board.GetEnabledLayers()
for i in layers.CuStack():
    name = board.GetLayerName(i)
    plot_plan.append(("", name, i, "Copper Layer " + name))

pctl = PLOT_CONTROLLER(board)
popt = pctl.GetPlotOptions()
popt.SetOutputDirectory(args.output_directory)

# A nasty hack to get the base filename
pctl.SetLayer(F_Cu)
pctl.OpenPlotfile("", PLOT_FORMAT_GERBER, "")
filename = pctl.GetPlotFileName()
try:
    os.remove(filename)
except:
    pass
pctl.ClosePlot()

basename = filename.replace('.gbr', '')
drlFile = basename + ".drl"
drlFileProtel = basename + ".txt"

if args.protel_extensions:
    popt.SetUseGerberProtelExtensions(True)

if args.detect_files_only:
    for layer_info in plot_plan:
        filenamePostfix = layer_info[1]
        layer_num = layer_info[2]
        pctl.SetLayer(layer_num)

        pctl.OpenPlotfile(filenamePostfix, PLOT_FORMAT_GERBER, layer_info[3])
        filename = pctl.GetPlotFileName()
        print filename
        try:
            os.remove(filename)
        except:
            pass

        pctl.ClosePlot()
    if args.protel_extensions:
        print drlFileProtel
    else:
        print drlFile
    sys.exit(0)

# Set some important plot options:
popt.SetPlotFrameRef(False)
popt.SetLineWidth(FromMM(0.35))

popt.SetAutoScale(False)
popt.SetScale(1)
popt.SetMirror(False)
popt.SetUseGerberAttributes(True)
popt.SetExcludeEdgeLayer(False)
popt.SetScale(1)
popt.SetUseAuxOrigin(True)

# This by gerbers only (also the name is truly horrid!)
popt.SetSubtractMaskFromSilk(False)

for layer_info in plot_plan:
    filenamePostfix = layer_info[1]
    layer_num = layer_info[2]
    pctl.SetLayer(layer_num)

    pctl.OpenPlotfile(filenamePostfix, PLOT_FORMAT_GERBER, layer_info[3])
    pctl.PlotLayer()
    pctl.ClosePlot()

popt.SetDrillMarksType(PCB_PLOT_PARAMS.FULL_DRILL_SHAPE)

drlwriter = EXCELLON_WRITER(board)
# drlwriter.SetMapFileFormat(PLOT_FORMAT_PDF)
drlwriter.SetMapFileFormat(PLOT_FORMAT_GERBER)

mirror = False
minimalHeader = False
offset = wxPoint(0, 0)
# False to generate 2 separate drill files (one for plated holes, one for non plated holes)
# True to generate only one drill file
mergeNPTH = False
drlwriter.SetOptions(mirror, minimalHeader, offset, mergeNPTH)

metricFmt = True
drlwriter.SetFormat(metricFmt)

genDrl = True
genMap = args.create_drill_map_file

drlwriter.CreateDrillandMapFilesSet(pctl.GetPlotDirName(), genDrl, genMap)

if args.protel_extensions:
    os.rename(drlFile, basename + ".txt")
    pass