kicad-developers team mailing list archive

[jp charras <jp.charras@xxxxxxxxxx>]

Le 31/07/2018 à 16:52, Jon Evans a écrit :
> It would be nice to have a fully-scriptable "output job" system so that you can save all the Gerber
> generation settings, all the drill generation settings, etc together, and set up a workflow of
> generating files, naming them a certain way, packaging them in a ZIP, etc.

It could be made by a Python script.
Attached a basic python script to create gerber and drill files from a board file.

Some latest options (creating a job file or a drill file in gerber format) are not available for
python scripts, but it should be easy (famous words) to add them to the Python scripting stuff.

> 
> On Tue, Jul 31, 2018 at 10:24 AM Ben Hest <bombledmonk@xxxxxxxxx <mailto:bombledmonk@xxxxxxxxx>> wrote:
> 
>     I'd give that a thumbs up from as a single user's opinion.
> 
>     On Tue, Jul 31, 2018 at 8:58 AM Adam Wolf <adamwolf@xxxxxxxxxxxxxxxxxxxx
>     <mailto:adamwolf@xxxxxxxxxxxxxxxxxxxx>> wrote:
> 
>         100% percent of the time when I make drill files, I also want to make
>         gerbers, and I want a zip file for uploading as well.
> 
>         Is there any interest in adding some way to do this automatically?  It
>         may be a little tricky since drills and Gerbers are two different
>         windows, but if this is considered a bad idea I will just stop
>         thinking about it now.
> 
>         Adam

-- 
Jean-Pierre CHARRAS

'''
    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/"

#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
gen_job_file=False
'''
gbr_job_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], 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=popt.GetOutputDirectory() + '.gbrjob'
    print 'create job file %s' % job_fn
    gbr_job_writer.CreateJobFile( job_fn )