Added secondary files

2 files changed, 330 insertions, 0 deletions

diff --git a/demos/python_scripts_examples/gen_gerber_and_drill_files_board.py b/demos/python_scripts_examples/gen_gerber_and_drill_files_board.py
new file mode 100644
index 0000000..55c1698
--- /dev/null
+++ b/demos/python_scripts_examples/gen_gerber_and_drill_files_board.py
@@ -0,0 +1,119 @@
+'''
+    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)     #do not change it
+popt.SetLineWidth(FromMM(0.35))
+
+popt.SetAutoScale(False)        #do not change it
+popt.SetScale(1)                #do not change it
+popt.SetMirror(False)
+popt.SetUseGerberAttributes(True)
+popt.SetUseGerberProtelExtensions(False)
+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])
+    print 'plot %s' % pctl.GetPlotFileName()
+    if pctl.PlotLayer() == False:
+        print "plot error"
+
+#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")
+    print 'plot %s' % pctl.GetPlotFileName()
+    if pctl.PlotLayer() == False:
+        print "plot error"
+
+
+# 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)
+# 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 = True
+print 'create drill and map files in %s' % pctl.GetPlotDirName()
+drlwriter.CreateDrillandMapFilesSet( pctl.GetPlotDirName(), genDrl, genMap );
+
+# One can create a text file to report drill statistics
+rptfn = pctl.GetPlotDirName() + 'drill_report.rpt'
+print 'report: %s' % rptfn
+drlwriter.GenDrillReportFile( rptfn );
diff --git a/demos/python_scripts_examples/plot_board.py b/demos/python_scripts_examples/plot_board.py
new file mode 100644
index 0000000..6fd55d0
--- /dev/null
+++ b/demos/python_scripts_examples/plot_board.py
@@ -0,0 +1,211 @@
+'''
+    A python script example to create various plot files from a board:
+    Fab files
+    Doc files
+    Gerber files
+
+    Important note:
+        this python script does not plot frame references.
+        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.
+'''
+
+import sys
+
+from pcbnew import *
+filename=sys.argv[1]
+
+board = LoadBoard(filename)
+
+pctl = PLOT_CONTROLLER(board)
+
+popt = pctl.GetPlotOptions()
+
+popt.SetOutputDirectory("plot/")
+
+# 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)
+
+pctl.SetLayer(F_SilkS)
+pctl.OpenPlotfile("Silk", PLOT_FORMAT_PDF, "Assembly guide")
+pctl.PlotLayer()
+
+# 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
+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()
+
+# Our fabricators want two additional gerbers:
+# An assembly with no silk trim and all and only the references
+# (you'll see that even holes have designators, obviously)
+popt.SetSubtractMaskFromSilk(False)
+popt.SetPlotReference(True)
+popt.SetPlotValue(False)
+popt.SetPlotInvisibleText(True)
+
+pctl.SetLayer(F_SilkS)
+pctl.OpenPlotfile("AssyTop", PLOT_FORMAT_PDF, "Assembly top")
+pctl.PlotLayer()
+
+# And a gerber with only the component outlines (really!)
+popt.SetPlotReference(False)
+popt.SetPlotInvisibleText(False)
+pctl.SetLayer(F_SilkS)
+pctl.OpenPlotfile("AssyOutlinesTop", PLOT_FORMAT_PDF, "Assembly outline top")
+pctl.PlotLayer()
+
+# The same could be done for the bottom side, if there were components
+popt.SetUseAuxOrigin(False)
+
+## For documentation we also want a general layout PDF
+## I usually use a shell script to merge the ps files and then distill the result
+## Now I can do it with a control file. As a bonus I can have references in a
+## different colour, too.
+
+popt.SetPlotReference(True)
+popt.SetPlotValue(True)
+popt.SetPlotInvisibleText(False)
+# Remember that the frame is always in color 0 (BLACK) and should be requested
+# before opening the plot
+popt.SetPlotFrameRef(False)
+pctl.SetLayer(Dwgs_User)
+
+pctl.OpenPlotfile("Layout", PLOT_FORMAT_PDF, "General layout")
+pctl.PlotLayer()
+
+# Do the PCB edges in yellow
+popt.SetColor(YELLOW)
+pctl.SetLayer(Edge_Cuts)
+pctl.PlotLayer()
+
+## Comments in, uhmm... green
+popt.SetColor(GREEN)
+pctl.SetLayer(Cmts_User)
+pctl.PlotLayer()
+
+# Bottom mask as lines only, in red
+#popt.SetMode(LINE)
+popt.SetColor(RED)
+pctl.SetLayer(B_Mask)
+pctl.PlotLayer()
+
+# Top mask as lines only, in blue
+popt.SetColor(BLUE)
+pctl.SetLayer(F_Mask)
+pctl.PlotLayer()
+
+# Top paste in light blue, filled
+popt.SetColor(BLUE)
+#popt.SetMode(FILLED)
+pctl.SetLayer(F_Paste)
+pctl.PlotLayer()
+
+# Top Silk in cyan, filled, references in dark cyan
+popt.SetReferenceColor(DARKCYAN)
+popt.SetColor(CYAN)
+pctl.SetLayer(F_SilkS)
+pctl.PlotLayer()
+
+popt.SetTextMode(PLOTTEXTMODE_STROKE)
+pctl.SetLayer(F_Mask)
+pctl.OpenPlotfile("Assembly", PLOT_FORMAT_SVG, "Master Assembly")
+pctl.SetColorMode(True)
+
+# We want *everything*
+popt.SetPlotReference(True)
+popt.SetPlotValue(True)
+popt.SetPlotInvisibleText(True)
+
+# Remember than the DXF driver assigns colours to layers. This means that
+# we will be able to turn references on and off simply using their layers
+# Also most of the layer are now plotted in 'line' mode, because DXF handles
+# fill mode almost like sketch mode (this is to keep compatibility with
+# most CAD programs; most of the advanced primitive attributes required are
+# handled only by recent autocads...); also the entry level cads (qcad
+# and derivatives) simply don't handle polyline widths...
+
+# Here I'm using numbers for colors and layers, I'm too lazy too look them up:P
+popt.SetReferenceColor(19)
+popt.SetValueColor(21)
+
+popt.SetColor(0)
+#popt.SetMode(LINE)
+pctl.SetLayer(B_SilkS)
+pctl.PlotLayer()
+popt.SetColor(14)
+pctl.SetLayer(F_SilkS)
+pctl.PlotLayer()
+popt.SetColor(2)
+pctl.SetLayer(B_Mask)
+pctl.PlotLayer()
+popt.SetColor(4)
+pctl.SetLayer(F_Mask)
+pctl.PlotLayer()
+popt.SetColor(1)
+pctl.SetLayer(B_Paste)
+pctl.PlotLayer()
+popt.SetColor(9)
+pctl.SetLayer(F_Paste)
+pctl.PlotLayer()
+popt.SetColor(3)
+pctl.SetLayer(Edge_Cuts)
+pctl.PlotLayer()
+
+# Export the copper layers too... exporting one of them in filled mode with
+# drill marks will put the marks in the WHITE later (since it tries to blank
+# the pads...); these will be obviously great reference points for snap
+# and stuff in the cad. A pctl function to only plot them would be
+# better anyway...
+
+popt.SetColor(17)
+#popt.SetMode(FILLED)
+popt.SetDrillMarksType(PCB_PLOT_PARAMS.FULL_DRILL_SHAPE)
+pctl.SetLayer(B_Cu)
+pctl.PlotLayer()
+popt.SetColor(20)
+popt.SetDrillMarksType(PCB_PLOT_PARAMS.NO_DRILL_SHAPE)
+pctl.SetLayer(F_Cu)
+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()
+
+# We have just generated 21 plotfiles with a single script