Rework on EXCELLON_WRITER class, to allow gerber and drill files creation from a python script.

added the example gen_gerber_and_drill_files_board.py in demos, which shows how to do that.
Fix a Printf format issue (shown in Debug mode) in Libedit (%d used for a size_t, changed in %zu)

demos/python_scripts_examples/gen_gerber_and_drill_files_board.py

@@ -0,0 +1,110 @@
+'''
+    A python script example to create plot files to build a board:
+    Gerber files
+    Drill files
+    Map dril files
+
+    Important note:
+        this python script does not plot frame references (page layout).
+        the reason is it is not yet possible from a python script because plotting
+        plot frame references needs loading the corresponding page layout file
+        (.wks file) or the default template.
+
+        This info (the page layout template) is not stored in the board, and therefore
+        not available.
+
+        Do not try to change SetPlotFrameRef(False) to SetPlotFrameRef(true)
+        the result is the pcbnew lib will crash if you try to plot
+        the unknown frame references template.
+
+        Anyway, in gerber and drill files the page layout is not plot
+'''
+
+import sys
+
+from pcbnew import *
+filename=sys.argv[1]
+
+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.SetExcludeEdgeLayer(False);
+popt.SetScale(1)
+popt.SetUseAuxOrigin(True)
+
+# This by gerbers only (also the name is truly horrid!)
+popt.SetSubtractMaskFromSilk(False)
+
+# Once the defaults are set it become pretty easy...
+# I have a Turing-complete programming language here: I'll use it...
+# param 0 is a string added to the file base name to identify the drawing
+# param 1 is the layer ID
+# param 2 is a comment
+plot_plan = [
+    ( "CuTop", F_Cu, "Top layer" ),
+    ( "CuBottom", B_Cu, "Bottom layer" ),
+    ( "PasteBottom", B_Paste, "Paste Bottom" ),
+    ( "PasteTop", F_Paste, "Paste top" ),
+    ( "SilkTop", F_SilkS, "Silk top" ),
+    ( "SilkBottom", B_SilkS, "Silk top" ),
+    ( "MaskBottom", B_Mask, "Mask bottom" ),
+    ( "MaskTop", F_Mask, "Mask top" ),
+    ( "EdgeCuts", Edge_Cuts, "Edges" ),
+]
+
+
+for layer_info in plot_plan:
+    pctl.SetLayer(layer_info[1])
+    pctl.OpenPlotfile(layer_info[0], PLOT_FORMAT_GERBER, layer_info[2])
+    pctl.PlotLayer()
+
+#generate internal copper layers, if any
+lyrcnt = board.GetCopperLayerCount();
+
+for innerlyr in range ( 1, lyrcnt-1 ):
+    pctl.SetLayer(innerlyr)
+    lyrname = 'inner%s' % innerlyr
+    pctl.OpenPlotfile(lyrname, PLOT_FORMAT_GERBER, "inner")
+    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 = False
+drlwriter.SetOptions( mirror, minimalHeader, offset, mergeNPTH )
+
+metricFmt = True
+drlwriter.SetFormat( metricFmt )
+
+genDrl = True
+genMap = True
+drlwriter.CreateDrillandMapFilesSet( plotDir, genDrl, genMap );
+
+# One can create a text file to report drill statistics
+rptfn = plotDir + '/drill_report.txt'
+drlwriter.GenDrillReportFile( rptfn );