Update python scripts examples according to recent changes in pcbnew code.

Add a new example to plot files

pcbnew/python/examples/createFPC40.py

@@ -49,7 +49,7 @@ e.SetShape(S_SEGMENT)
 module.Add(e)
 
 # save the footprint to disk
-fpid = LIB_ID("FPC"+str(pads))   #the name in library
+fpid = LIB_ID("", "FPC"+str(pads))   #the curr lin nickname (empty) and the name in library
 module.SetFPID( fpid )
 
 lib_name = "fpc40.pretty"   #lib_path is actually a path, not a file

pcbnew/python/examples/createPcb.py

@@ -7,12 +7,13 @@ size_1_0mm = wxSizeMM(1.0,1.0)
 # create a blank board
 pcb = BOARD()
 
-pcb.m_NetClasses.GetDefault().SetClearance(FromMM(0.1))
+pcb.GetNetClasses().GetDefault().SetClearance(FromMM(0.1))
 
 # create a new module, it's parent is our previously created pcb
 module = MODULE(pcb)
 module.SetReference("M1")   # give it a reference name
-module.Reference().SetPos0(wxPointMM(-10,-10))
+module.Reference().SetPos0(wxPointMM(6,-2))
+module.Reference().SetDrawCoord()
 pcb.Add(module)             # add it to our pcb
 m_pos = wxPointMM(50,50)
 module.SetPosition(m_pos)
@@ -26,7 +27,7 @@ for y in range (0,10):
         pad.SetSize(size_1_0mm)
         pt = wxPointMM(1.27*x,1.27*y)
         pad.SetPos0(pt);
-        #pad.SetPosition(pt)
+        pad.SetDrawCoord()
         pad.SetName(str(n))
         module.Add(pad)
         n+=1
@@ -34,7 +35,6 @@ for y in range (0,10):
 
 # save the PCB to disk
 pcb.Save("my2.kicad_pcb")
-pcb.Save("my2.brd")
 
 pcb = LoadBoard("my2.kicad_pcb")
 
@@ -42,7 +42,7 @@ print map( lambda x: x.GetReference() , list(pcb.GetModules()))
 
 for m in pcb.GetModules():
     for p in m.Pads():
-        print p.GetName(), p.GetPosition(), p.GetOffset()
+        print 'pad ', p.GetName(), p.GetPosition(), p.GetOffset()
 
 
 # pcb.GetDesignSettings()

pcbnew/python/examples/gen_gerber_and_drill_files_board.py

@@ -0,0 +1,150 @@
+'''
+    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
+import os
+
+from pcbnew import *
+filename=sys.argv[1]
+
+board = LoadBoard(filename)
+
+plotDir = "plot/"
+
+#prepare the gerber job file
+gen_job_file=True
+
+pctl = PLOT_CONTROLLER(board)
+
+popt = pctl.GetPlotOptions()
+
+popt.SetOutputDirectory(plotDir)
+
+# Set some important plot options (see pcb_plot_params.h):
+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.SetIncludeGerberNetlistInfo(True)
+popt.SetCreateGerberJobFile(gen_job_file)
+popt.SetUseGerberProtelExtensions(False)
+popt.SetExcludeEdgeLayer(False);
+popt.SetScale(1)
+popt.SetUseAuxOrigin(True)
+
+# This by gerbers only
+popt.SetSubtractMaskFromSilk(False)
+# Disable plot pad holes
+popt.SetDrillMarksType( PCB_PLOT_PARAMS.NO_DRILL_SHAPE );
+# Skip plot pad NPTH when possible: when drill size and shape == pad size and shape
+# usually sel to True for copper layers
+popt.SetSkipPlotNPTH_Pads( False );
+
+
+#prepare the gerber job file
+jobfile_writer = GERBER_JOBFILE_WRITER( board )
+
+# 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:
+    if layer_info[1] <= B_Cu:
+        popt.SetSkipPlotNPTH_Pads( True )
+    else:
+        popt.SetSkipPlotNPTH_Pads( False )
+
+    pctl.SetLayer(layer_info[1])
+    pctl.OpenPlotfile(layer_info[0], PLOT_FORMAT_GERBER, layer_info[2])
+    print 'plot %s' % pctl.GetPlotFileName()
+    if gen_job_file == True:
+        jobfile_writer.AddGbrFile( layer_info[1], os.path.basename(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 ):
+    popt.SetSkipPlotNPTH_Pads( True );
+    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 );
+
+if gen_job_file == True:
+    #job_fn=os.path.splitext(pctl.GetPlotFileName())[0] + '.gbrjob'
+    job_fn=os.path.dirname(pctl.GetPlotFileName()) + '/' + os.path.basename(filename)
+    job_fn=os.path.splitext(job_fn)[0] + '.gbrjob'
+    print 'create job file %s' % job_fn
+    jobfile_writer.CreateJobFile( job_fn )
+

pcbnew/python/examples/listPcb.py

@@ -47,10 +47,10 @@ print ""
 print "LIST MODULES:"
 
 for module in pcb.GetModules():
-    print "* Module: %s at %s"%(module.GetReference(),ToUnits(module.GetPosition()))
+    print "* Module: %s at %s"%(module.GetReference(), ToUnits(module.GetPosition()))
 
 print ""
-print "Ratsnest cnt:",len(pcb.GetFullRatsnest())
+print "Nets cnt: ", pcb.GetNetCount()
 print "track w cnt:",len(pcb.GetTrackWidthList())
 print "via s cnt:",len(pcb.GetViasDimensionsList())