1 files changed, 259 insertions, 0 deletions
diff --git a/src/ee/kicad/export_gerber.py b/src/ee/kicad/export_gerber.py
new file mode 100755
index 0000000..511f9ee
--- /dev/null
+++ b/src/ee/kicad/export_gerber.py
@@ -0,0 +1,259 @@
+#!/usr/bin/env python
+from __future__ import print_function
+import sys
+import os
+import argparse
+from pcbnew import *
+
+def layer_name_parser(s):
+    parts = s.split('=')
+    if len(parts) != 2:
+        raise argparse.ArgumentTypeError("Invalid layer renaming: " + s)
+    else:
+        return parts
+
+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',
+                    help='Don\'t create the GERBER files, just write a list of 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 instead of .gbr')
+
+parser.add_argument('--extended-gerber-attributes',
+                    dest='extended_gerber_attributes',
+                    action='store_true',
+                    help='Use extended Gerber attributes')
+
+parser.add_argument('--uppercase-extensions',
+                    action='store_true',
+                    help='Uppercase all extensions')
+
+parser.add_argument('--layer-extension',
+                    dest='layer_extensions',
+                    metavar='LAYER_AND_EXTENSION',
+                    action='append',
+                    type=layer_name_parser,
+                    help='Set the file extension of a KiCAD layer. Format: <KiCAD Layer>=<extension>, example: F.SilkS=GSILK')
+
+args = parser.parse_args()
+# print "args: " + str(args)
+# print "args.name_layer: " + str(args.name_layers)
+
+renames = {}
+if args.layer_extensions is not None:
+    for s in args.layer_extensions:
+        renames[s[0]] = s[1]
+# print("renames: " + str(renames))
+
+board = LoadBoard(args.pcb)
+
+class Plan:
+    def __init__(self, layerNum, layerName, description):
+        self.layerNum = layerNum
+        self.layerName = layerName
+        self.description = description
+        self.postfix = ""
+        self.ext = None
+
+    @staticmethod
+    def standard(layerNum, description):
+        layerName = board.GetLayerName(layerNum)
+        return Plan(layerNum, layerName, description)
+
+    @staticmethod
+    def copper(layerNum):
+        layerName = board.GetLayerName(layerNum)
+        description = "Copper Layer " + layerName
+        return Plan(layerNum, layerName, description)
+
+plot_plan = [Plan.standard(layerNum, description) for (layerNum, description) in [
+    (F_SilkS, "Silk front"),
+    (F_Mask, "Mask front"),
+    (F_Paste, "Paste front"),
+    (B_SilkS, "Silk bottom"),
+    (B_Mask, "Mask bottom"),
+    (B_Paste, "Paste bottom"),
+    (Edge_Cuts, "Edges")]]
+
+layers = board.GetEnabledLayers()
+for layerNum in layers.CuStack():
+    plot_plan.append(Plan.copper(layerNum))
+
+pctl = PLOT_CONTROLLER(board)
+popt = pctl.GetPlotOptions()
+
+output_directory = args.output_directory
+popt.SetOutputDirectory(output_directory)
+
+if not os.path.isdir(output_directory):
+    try:
+        os.makedirs(output_directory)
+    except:
+        print("Could not make output directory", file=sys.stderr)
+        sys.exit(1)
+
+# 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()
+
+# "Use protel filename extensions", default=False
+popt.SetUseGerberProtelExtensions(args.protel_extensions)
+
+basename = os.path.splitext(filename)[0]
+
+drlFileOut = drlFile = basename + "-PTH.drl"
+drlNpthFileOut = drlNpthFile = basename + "-NPTH.drl"
+
+if args.uppercase_extensions:
+    n, e = os.path.splitext(drlFileOut)
+    drlFileOut = n + e.upper()
+    n, e = os.path.splitext(drlNpthFileOut)
+    drlNpthFileOut = n + e.upper()
+
+values = vars(args)
+for plan in plot_plan:
+    pctl.SetLayer(plan.layerNum)
+    pctl.OpenPlotfile("", PLOT_FORMAT_GERBER, plan.description)
+    filename = pctl.GetPlotFileName()
+    pctl.ClosePlot()
+    # By opening and closing the plot we create an empty plot file.
+    try:
+        os.remove(filename)
+    except:
+        pass
+
+    filename, ext = os.path.splitext(filename)
+    if args.uppercase_extensions:
+        ext = ext.upper()
+
+    if plan.layerName in renames:
+        ext = "." + renames[plan.layerName]
+
+    # if plan.arg is not None:
+    #     newExt = values[plan.arg]
+    #     if newExt is not None:
+    #         ext = "." + newExt
+
+    plan.postfix = plan.layerName
+    plan.filename = basename + "-" + plan.postfix + ext
+
+    # print "filename = " + plan.filename + ", postfix=" + plan.postfix
+    # print "filename: " + plan.filename
+
+if args.detect_files_only:
+    with open(args.detect_files_only, "w") as f:
+      for plan in plot_plan:
+          print(plan.filename, file=f)
+
+      print(drlFileOut, file=f)
+      print(drlNpthFileOut, file=f)
+    sys.exit(0)
+
+# Set some important plot options:
+popt.SetPlotFrameRef(False)
+
+# "Default line width (mm)", default=0.1mm
+popt.SetLineWidth(FromMM(0.1))
+
+popt.SetAutoScale(False)
+
+# "Mirrored plot", default=False. Not applicable for Gerber
+popt.SetMirror(False)
+
+# "Include extended attributes", default=False
+popt.SetUseGerberAttributes(args.extended_gerber_attributes)
+
+# "Drill marks"
+popt.SetDrillMarksType(PCB_PLOT_PARAMS.NO_DRILL_SHAPE)
+
+# "Scaling"
+popt.SetScale(1)
+
+# "Use auxilary axis as origin"
+popt.SetUseAuxOrigin(False)
+
+# This by gerbers only (also the name is truly horrid!)
+popt.SetSubtractMaskFromSilk(False)
+
+for plan in plot_plan:
+    pctl.SetLayer(plan.layerNum)
+
+    # print "filename = " + plan.filename + ", postfix=" + plan.postfix
+    pctl.OpenPlotfile(plan.postfix, PLOT_FORMAT_GERBER, plan.description)
+
+    actualFilename = pctl.GetPlotFileName()
+    expectedFilename = plan.filename
+
+    if expectedFilename != actualFilename:
+        os.rename(actualFilename, expectedFilename)
+
+    pctl.PlotLayer()
+    pctl.ClosePlot()
+
+drlwriter = EXCELLON_WRITER(board)
+drlwriter.SetMapFileFormat(PLOT_FORMAT_GERBER)
+
+# "Drill file options"
+
+# "Mirror y axis", default=False
+mirror = False
+
+# "Minimal header", default=True
+minimalHeader = True
+
+offset = wxPoint(0, 0)
+
+# "Merge PTH and NPTH into one file", default=False
+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)
+
+# This has to be verified that this is the right way to do it.
+if False:
+# Check that the drill files actually was generated
+    if not os.path.isfile(drlFile):
+        print("No drill file generated: {}".format(drlFile), file=sys.stderr)
+
+    if not os.path.isfile(drlNpthFile):
+        print("No drill file generated: {}".format(drlNpthFile), file=sys.stderr)
+
+if drlFile != drlFileOut:
+    os.rename(drlFile, drlFileOut)
+
+if drlNpthFile != drlNpthFileOut:
+    os.rename(drlNpthFile, drlNpthFileOut)