KiCad5でガーバデータ出力するスクリプト。FusionPCB向けに改造。

action_menu_gerber_zip.py

# file : action_menu_gerber_zip.py
#
# (gerber_zip)
#
# Copyright (C) 2018 g200kg
#   Released under MIT License
#
 
import pcbnew
from pcbnew import *
import wx
import os
import zipfile
 
#
# Setup params
#
 
gerber_subdir = "Gerber"
merge_npth = True
use_aux_origin = False
excellon_format = EXCELLON_WRITER.DECIMAL_FORMAT
#excellon_format = EXCELLON_WRITER.SUPPRESS_LEADING
 
#
#
#
 
class GerberZip( pcbnew.ActionPlugin ):
    '''
    Make Gerber Zip-file for Elecrow / FusionPCB
    '''
    layers = [
        [ F_Cu,     'GTL', None ],
        [ B_Cu,     'GBL', None ],
        [ F_SilkS,  'GTO', None ],
        [ B_SilkS,  'GBO', None ],
        [ F_Mask,   'GTS', None ],
        [ B_Mask,   'GBS', None ],
        [ Edge_Cuts,'GML', None ],
#        [ In1_Cu,   'GL2', None ],
#        [ In2_Cu,   'GL3', None ],
#        [ In3_Cu,   'GL4', None ],
#        [ In4_Cu,   'GL5', None ],
    ]
    max_layer = 7
 
    def defaults( self ):
        self.name = "Make Gerber-Zip (Elecrow/FusionPCB style)"
        self.category = "Plot"
        self.description = "Make Gerber-Zip-file for Elecrow / FusionPCB"
 
    def forcedel( self, fname ):
        if os.path.exists(fname):
            os.remove(fname)
 
    def forceren( self, src, dst ):
        self.forcedel(dst)
        os.rename(src, dst)
 
    def Run( self ):
        board = pcbnew.GetBoard()
        board_fname = board.GetFileName()
        board_dir = os.path.dirname(board_fname)
        board_basename = (os.path.splitext(os.path.basename(board_fname)))[0]
        gerber_dir = '%s/%s' % (board_dir, gerber_subdir)
        drill_fname = '%s/%s.TXT' % (gerber_dir, board_basename)
        npth_fname = '%s/%s-NPTH.TXT' % (gerber_dir, board_basename)
        zip_fname = '%s/%s.zip' % (gerber_dir, board_basename)
        if not os.path.exists(gerber_dir):
            os.mkdir(gerber_dir)
 
        max_layer = board.GetCopperLayerCount() + 5
# PLOT
        pc = pcbnew.PLOT_CONTROLLER(board)
        po = pc.GetPlotOptions()
 
        po.SetFormat(PLOT_FORMAT_GERBER)
        po.SetOutputDirectory(gerber_dir)
        po.SetPlotValue(True)
        po.SetPlotReference(True)
#        po.SetExcludeEdgeLayer(False)
        po.SetExcludeEdgeLayer(True)
        po.SetLineWidth(FromMM(0.1))
#        po.SetSubtractMaskFromSilk(True)
        po.SetSubtractMaskFromSilk(False)
        po.SetUseAuxOrigin(use_aux_origin)
        po.SetPlotViaOnMaskLayer(False)
# Options
        po.SetUseGerberProtelExtensions(True)
        po.SetCreateGerberJobFile(False)
        po.SetSubtractMaskFromSilk(False)
        po.SetUseGerberX2format(False)
        po.SetIncludeGerberNetlistInfo(False)

        for layer in self.layers:
            targetname = '%s/%s.%s' % (gerber_dir, board_basename, layer[1])
            self.forcedel(targetname)
        self.forcedel(drill_fname)
        self.forcedel(npth_fname)
        self.forcedel(zip_fname)
 
        for i in range(max_layer):
            layer = self.layers[i]
            pc.SetLayer(layer[0])
            pc.OpenPlotfile(layer[1],PLOT_FORMAT_GERBER,layer[1])
            pc.PlotLayer()
            layer[2] = pc.GetPlotFileName()
        pc.ClosePlot()
 
        for i in range(max_layer):
            layer = self.layers[i]
            targetname = '%s/%s.%s' % (gerber_dir, board_basename, layer[1])
            self.forceren(layer[2],targetname)
# DRILL
        ew = EXCELLON_WRITER(board)
        ew.SetFormat(True, excellon_format, 3, 3)
        offset = wxPoint(0,0)
        if(use_aux_origin):
            offset = board.GetAuxOrigin()
        ew.SetOptions(False, False, offset, merge_npth)
        ew.CreateDrillandMapFilesSet(gerber_dir,True,False)
        if merge_npth:
            self.forceren('%s/%s.drl' % (gerber_dir, board_basename), drill_fname)
        else:
            self.forceren('%s/%s-PTH.drl' % (gerber_dir, board_basename), drill_fname)
            self.forceren('%s/%s-NPTH.drl' % (gerber_dir, board_basename), npth_fname)
# ZIP
        with zipfile.ZipFile(zip_fname,'w') as f:
            for i in range(max_layer):
                layer = self.layers[i]
                targetname = '%s/%s.%s' % (gerber_dir, board_basename, layer[1])
                f.write(targetname, os.path.basename(targetname))
            f.write(drill_fname, os.path.basename(drill_fname))
            if not merge_npth:
                f.write(npth_fname, os.path.basename(npth_fname))
 
        wx.MessageBox('GerberZip Complete.\n\n%s' % zip_fname, 'Gerber Zip', wx.OK|wx.ICON_INFORMATION)
 
GerberZip().register()