-
Notifications
You must be signed in to change notification settings - Fork 0
/
Copy pathplot_gerber_and_drill.py
225 lines (172 loc) · 6.69 KB
/
plot_gerber_and_drill.py
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
56
57
58
59
60
61
62
63
64
65
66
67
68
69
70
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
92
93
94
95
96
97
98
99
100
101
102
103
104
105
106
107
108
109
110
111
112
113
114
115
116
117
118
119
120
121
122
123
124
125
126
127
128
129
130
131
132
133
134
135
136
137
138
139
140
141
142
143
144
145
146
147
148
149
150
151
152
153
154
155
156
157
158
159
160
161
162
163
164
165
166
167
168
169
170
171
172
173
174
175
176
177
178
179
180
181
182
183
184
185
186
187
188
189
190
191
192
193
194
195
196
197
198
199
200
201
202
203
204
205
206
207
208
209
210
211
212
213
214
215
216
217
218
219
220
221
222
223
224
225
# coding: utf8
# plot_gerber_and_drill.py
#
# Copyright (C) 2019-2023 Eldar Khayrullin <eldar.khayrullin@mail.ru>
#
# This program is free software: you can redistribute it and/or modify
# it under the terms of the GNU General Public License as published by
# the Free Software Foundation, either version 3 of the License, or
# (at your option) any later version.
#
# This program is distributed in the hope that it will be useful,
# but WITHOUT ANY WARRANTY; without even the implied warranty of
# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE. See the
# GNU General Public License for more details.
#
# You should have received a copy of the GNU General Public License
# along with this program. If not, see <http://www.gnu.org/licenses/>.
''' KiCad PCBNew Action Plugin for plot gerber and drill files '''
import getpass
import os
import pcbnew
import re
import shutil
import sys
import tempfile
import zipfile
from datetime import datetime
from platform import platform
from version import VERSION
OUTPUT_NAME = 'gerber'
OUTPUT_DIR = '_generated_files' + os.path.sep + OUTPUT_NAME
EOL = u'\r\n'
class plot_gerber_and_drill(pcbnew.ActionPlugin):
def defaults(self):
self.name = "Plot gerber and drill files"
self.category = "Plot files"
self.description = "Plot gerber and drill files"
self.icon_file_name = self.get_icon_file_name()
def Run(self):
process_board(pcbnew.GetBoard())
def get_icon_file_name(self):
dirname = os.path.dirname(os.path.abspath(__file__))
filename = os.path.splitext(os.path.basename(__file__))[0]
return dirname + os.path.sep + 'bitmaps' + os.path.sep + filename + '.png'
def process_board(board):
clean_output(get_output_abs_path(board))
plot_layers_and_apply(board)
plot_drill(board)
zip_output(get_output_abs_path(board), get_board_name(board))
def clean_output(path):
if os.path.exists(path):
shutil.rmtree(path, ignore_errors=False, onerror=None)
os.makedirs(path)
def get_output_abs_path(board):
path = os.path.dirname(os.path.abspath(board.GetFileName()))
return path + os.path.sep + OUTPUT_DIR
def get_board_name(board):
name = os.path.splitext(os.path.basename(board.GetFileName()))[0]
number = try_to_find_pcb_number(board)
if number != '':
if number[0] == '_':
name += number
else:
name = number
return name
def try_to_find_pcb_number(board):
number = ''
rev = ''
for item in board.GetDrawings():
if type(item) is pcbnew.PCB_TEXT:
text = item.GetText()
result = re.search('^rev\.\d', text, re.IGNORECASE)
if result:
rev = text
if number != '':
break
continue
result = re.search('^\S*\.\d*\.\d*', text)
if result:
number = text
if rev != '':
break
number.strip()
rev.strip()
result = re.search('rev\.\d', number, re.IGNORECASE)
if result:
s = number.split()
number = s[0] + '_' + s[1]
elif rev != '':
number += '_' + rev
return number
def plot_layers_and_apply(board):
plot_ctrl = pcbnew.PLOT_CONTROLLER(board)
plot_opts = plot_ctrl.GetPlotOptions()
plot_opts.SetOutputDirectory(OUTPUT_DIR)
#plot_opts.SetExcludeEdgeLayer(True)
plot_opts.SetPlotFrameRef(False)
plot_opts.SetPlotInvisibleText(False)
plot_opts.SetPlotMode(pcbnew.FILLED)
#plot_opts.SetPlotPadsOnSilkLayer(False)
plot_opts.SetPlotReference(True)
plot_opts.SetPlotValue(False)
plot_opts.SetPlotViaOnMaskLayer(False)
plot_opts.SetSkipPlotNPTH_Pads(False)
plot_opts.SetSubtractMaskFromSilk(True)
plot_opts.SetUseAuxOrigin(True)
plot_opts.SetCreateGerberJobFile(True)
plot_opts.SetGerberPrecision(6)
plot_opts.SetIncludeGerberNetlistInfo(False)
plot_opts.SetUseGerberAttributes(False)
plot_opts.SetUseGerberProtelExtensions(False)
plot_opts.SetUseGerberX2format(False)
board.SetPlotOptions(plot_opts)
plot_ctrl.SetLayer(pcbnew.Edge_Cuts)
plot_ctrl.OpenPlotfile('Edge_Cuts', pcbnew.PLOT_FORMAT_GERBER, 'Edge_Cuts')
plot_ctrl.PlotLayer()
plot_ctrl.SetLayer(pcbnew.F_SilkS)
plot_ctrl.OpenPlotfile('F_SilkS', pcbnew.PLOT_FORMAT_GERBER, 'F_SilkS')
plot_ctrl.PlotLayer()
plot_ctrl.SetLayer(pcbnew.B_SilkS)
plot_ctrl.OpenPlotfile('B_SilkS', pcbnew.PLOT_FORMAT_GERBER, 'B_SilkS')
plot_ctrl.PlotLayer()
plot_ctrl.SetLayer(pcbnew.F_Mask)
plot_ctrl.OpenPlotfile('F_Mask', pcbnew.PLOT_FORMAT_GERBER, 'F_Mask')
plot_ctrl.PlotLayer()
plot_ctrl.SetLayer(pcbnew.B_Mask)
plot_ctrl.OpenPlotfile('B_Mask', pcbnew.PLOT_FORMAT_GERBER, 'B_Mask')
plot_ctrl.PlotLayer()
plot_ctrl.SetLayer(pcbnew.F_Cu)
plot_ctrl.OpenPlotfile('F_Cu', pcbnew.PLOT_FORMAT_GERBER, 'F_Cu')
plot_ctrl.PlotLayer()
cu_layer_count = board.GetDesignSettings().GetCopperLayerCount()
for i in range(cu_layer_count - 2):
plot_ctrl.SetLayer(pcbnew.In1_Cu + i)
plot_ctrl.OpenPlotfile('In{0}_Cu'.format(i + 1), pcbnew.PLOT_FORMAT_GERBER, 'In{0}_Cu'.format(i + 1))
plot_ctrl.PlotLayer()
plot_ctrl.SetLayer(pcbnew.B_Cu)
plot_ctrl.OpenPlotfile('B_Cu', pcbnew.PLOT_FORMAT_GERBER, 'B_Cu')
plot_ctrl.PlotLayer()
plot_ctrl.SetLayer(pcbnew.F_Paste)
plot_ctrl.OpenPlotfile('F_Paste', pcbnew.PLOT_FORMAT_GERBER, 'F_Paste')
plot_ctrl.PlotLayer()
plot_ctrl.SetLayer(pcbnew.B_Paste)
plot_ctrl.OpenPlotfile('B_Paste', pcbnew.PLOT_FORMAT_GERBER, 'B_Paste')
plot_ctrl.PlotLayer()
plot_ctrl.ClosePlot()
def plot_drill(board):
gen_drill = pcbnew.EXCELLON_WRITER(board)
gen_drill.SetFormat(True, pcbnew.GENDRILL_WRITER_BASE.KEEP_ZEROS)
gen_drill.SetOptions(False, False, board.GetDesignSettings().GetAuxOrigin(), False)
gen_drill.SetRouteModeForOvalHoles(True)
gen_drill.CreateDrillandMapFilesSet(get_output_abs_path(board), True, False)
#TODO apply drill options to project
def zip_output(path, name):
temp_dir = tempfile.mkdtemp()
zip_name = temp_dir + os.path.sep + name
shutil.make_archive(zip_name, 'zip', path)
zf = zipfile.ZipFile(zip_name + '.zip', 'a')
zf.comment = bytes(get_shtamp_comment(), 'utf-8')
zf.close()
shutil.move(zip_name + '.zip', path)
os.rmdir(temp_dir)
def get_shtamp_comment():
return EOL + 'Author: ' + getpass.getuser() + EOL + \
'Timeshtamp: ' + datetime.now().isoformat(timespec='seconds') + EOL + \
'Plugin: ' + VERSION + EOL + \
'OS: ' + platform()
if __name__ == '__main__':
board = pcbnew.LoadBoard(sys.argv[1])
process_board(board)
else:
plot_gerber_and_drill().register()