Add Makefile to create gerbers from *.kicad_pcb.

This also prepares the possibility to add a %%gitversion%%
string somewhere on the silkscreen which is replaced with the current
git version (but no such silkscreen is added in this commit).

KiCAD/Makefile

+# Create fab files.
+
+PocketBeagle-fab.zip:
+
+%-fab.zip : %-fab.kicad_pcb
+	python ../kicad-scripts/kicad-fab.py $< plot/
+	zip -r $@ plot/
+
+# Replacing any %%gitversion%% with a github version string.
+%-fab.kicad_pcb : %.kicad_pcb
+	sed "s/%%gitversion%%/`git log --date=short --pretty=format:'%h@%cd' -n 1 $^`/" < $^ > $@

kicad-scripts/kicad-fab.py

+'''
+  H. Zeller <h.zeller@acm.org>
+  Based on gen_gerber_and_drill_files_board.py in kicad/demos directory.
+'''
+
+import sys
+import os
+
+from pcbnew import *
+filename=sys.argv[1]
+plotDir = sys.argv[2] if len(sys.argv) > 2 else "plot/"
+
+board = LoadBoard(filename)
+
+plotDir = "plot/"
+
+pctl = PLOT_CONTROLLER(board)
+
+popt = pctl.GetPlotOptions()
+
+popt.SetOutputDirectory(plotDir)
+
+# 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.SetUseGerberProtelExtensions(True)
+popt.SetExcludeEdgeLayer(True);
+popt.SetScale(1)
+popt.SetUseAuxOrigin(True)
+
+# This by gerbers only (also the name is truly horrid!)
+popt.SetSubtractMaskFromSilk(False)
+
+# param 0 is the layer ID
+# param 1 is a string added to the file base name to identify the drawing
+# param 2 is a comment
+# Create filenames in a way that if they are sorted alphabetically, they
+# are shown in exactly the layering the board would look like. So
+#   gerbv *
+# just makes sense. The drill-file will be numbered 00 so that it is first.
+plot_plan = [
+    ( Edge_Cuts, "01-Edge_Cuts",   "Edges" ),
+
+    ( F_SilkS,   "02-SilkTop",     "Silk top" ),
+    ( F_Paste,   "03-PasteTop",    "Paste top" ),
+    ( F_Cu,      "04-CuTop",       "Top layer" ),
+    ( F_Mask,    "05-MaskTop",     "Mask top" ),
+
+    ( In1_Cu,    "06-CuIn1",       "Inner Layer1" ),
+    ( In2_Cu,    "07-CuIn2",       "Inner Layer2" ),
+
+    ( B_Mask,    "08-MaskBottom",  "Mask bottom" ),
+    ( B_Cu,      "09-CuBottom",    "Bottom layer" ),
+    ( B_Paste,   "10-PasteBottom", "Paste Bottom" ),
+    ( B_SilkS,   "11-SilkBottom",  "Silk top" ),
+]
+
+
+for layer_info in plot_plan:
+    pctl.SetLayer(layer_info[0])
+    pctl.OpenPlotfile(layer_info[1], PLOT_FORMAT_GERBER, layer_info[2])
+    pctl.PlotLayer()
+
+# At the end you have to close the last plot, otherwise you don't know when
+# the object will be recycled!
+pctl.ClosePlot()
+
+# Fabricators need drill files.
+# sometimes a drill map file is asked (for verification purpose)
+drlwriter = EXCELLON_WRITER( board )
+drlwriter.SetMapFileFormat( PLOT_FORMAT_PDF )
+
+mirror = False
+minimalHeader = False
+offset = wxPoint(0,0)
+mergeNPTH = True   # non-plated through-hole
+drlwriter.SetOptions( mirror, minimalHeader, offset, mergeNPTH )
+
+metricFmt = True
+drlwriter.SetFormat( metricFmt )
+
+genDrl = True
+genMap = True
+drlwriter.CreateDrillandMapFilesSet( plotDir, genDrl, genMap );
+
+# We can't give just the filename for the name of the drill file at generation
+# time, but we do want its name to be a bit different to show up on top.
+# So this is an ugly hack to rename the drl-file to have a 0 in the beginning.
+base_name = filename[:-10]
+print plotDir + base_name + ".drl"
+os.rename(plotDir + base_name + ".drl", plotDir + base_name + "-00.drl")