1gnetlist(1) 1.8.2.20130925 gnetlist(1)
2
3
4
6 gnetlist - gEDA/gaf Netlist Extraction and Generation
7
9 gnetlist [OPTION ...] [-g BACKEND] [--] FILE ...
10
11
13 gnetlist is a netlist extraction and generation tool, and is part of
14 the gEDA (GPL Electronic Design Automation) toolset. It takes one or
15 electronic schematics as input, and outputs a netlist. A netlist is a
16 machine-interpretable description of the way that components in an
17 electronic circuit are connected together, and is commonly used as the
18 input to a PCB layout program such as pcb(1) or to a simulator such as
19 gnucap(1).
20
21 A normal gnetlist run is carried out in two steps. First, the gnetlist
22 frontend loads the specified human-readable schematic FILEs, and com‐
23 piles them to an in-memory netlist description. Next, a `backend' is
24 used to export the connection and component data to one of many sup‐
25 ported netlist formats.
26
27 gnetlist is extensible, using the Scheme programming language.
28
29
31 -q Quiet mode. Turns off all warnings/notes/messages.
32
33 -v, --verbose
34 Verbose mode. Output all diagnostic information.
35
36 -L DIRECTORY
37 Prepend DIRECTORY to the list of directories to be searched for
38 Scheme files.
39
40 -g BACKEND
41 Specify the netlist backend to be used.
42
43 -O STRING
44 Pass an option string to the backend.
45
46 --list-backends
47 Print a list of available netlist backends.
48
49 -o FILE Specify the filename for the generated netlist. By default,
50 output is directed to `output.net'.
51
52 -l FILE Specify a Scheme file to be loaded before the backend is loaded
53 or executed. This option can be specified multiple times.
54
55 -m FILE Specify a Scheme file to be loaded between loading the backend
56 and executing it. This option can be specified multiple times.
57
58 -c EXPR Specify a Scheme expression to be executed during gnetlist
59 startup. This option can be specified multiple times.
60
61 -i After the schematic files have been loaded and compiled, and
62 after all Scheme files have been loaded, but before running the
63 backend, enter a Scheme read-eval-print loop.
64
65 -h, --help
66 Print a help message.
67
68 -V, --version
69 Print gnetlist version information.
70
71 -- Treat all remaining arguments as schematic filenames. Use this
72 if you have a schematic filename which begins with `-'.
73
74
76 Currently, gnetlist includes the following backends:
77
78
79 allegro Allegro netlist format.
80
81 bae Bartels Autoengineer netlist format.
82
83 bom, bom2
84 Bill of materials generation.
85
86 calay Calay netlist format.
87
88 cascade RF Cascade netlist format
89
90 drc, drc2
91 Design rule checkers (drc2 is recommended).
92
93 eagle Eagle netlist format.
94
95 ewnet Netlist format for National Instruments ULTIboard layout tool.
96
97 futurenet2
98 Futurenet2 netlist format.
99
100 geda Native gEDA netlist format (mainly used for testing and diag‐
101 nostics).
102
103 gossip Gossip netlist format.
104
105 gsch2pcb
106 Backend used for pcb(1) file layout generation by gsch2pcb(1).
107 It is not recommended to use this backend directly.
108
109 liquidpcb
110 LiquidPCB netlist format.
111
112 mathematica
113 Netlister for analytical circuit solving using Mathematica.
114
115 maxascii
116 MAXASCII netlist format.
117
118 osmond Osmond netlist format.
119
120 pads PADS netlist format.
121
122 partslist1, partslist2, partslist3
123 Bill of materials generation backends (alternatives to bom and
124 bom2).
125
126 PCB pcb(1) netlist format.
127
128 pcbpins Generates a pcb(1) action file for forward annotating pin/pad
129 names from schematic to layout.
130
131 protelII
132 Protel II netlist format.
133
134 redac RACAL-REDAC netlist format.
135
136 spice, spice-sdb
137 SPICE-compatible netlist format (spice-sdb is recommended).
138 Suitable for use with gnucap(1).
139
140 switcap SWITCAP switched capacitor simulator netlist format.
141
142 systemc Structural SystemC code generation.
143
144 tango Tango netlist format.
145
146 vams VHDL-AMS code generation.
147
148 verilog Verilog code generation.
149
150 vhdl VHDL code generation.
151
152 vipec ViPEC Network Analyser netlist format.
153
154
155
157 These examples assume that you have a `stack_1.sch' in the current
158 directory.
159
160 gnetlist requires that at least one schematic to be specified on the
161 command line:
162
163 ./gnetlist stack_1.sch
164
165
166 This is not very useful since it does not direct gnetlist to do
167 anything.
168
169 Specify a backend name with `-g' to get gnetlist to output a
170 netlist:
171
172 ./gnetlist -g geda stack_1.sch
173
174
175 The netlist output will be written to a file called `output.net'
176 in the current working directory.
177
178
179 You can specify the output filename by using the `-o' option:
180
181 ./gnetlist -g geda stack_1.sch -o /tmp/stack.netlist
182
183
184 Output will now be directed to `/tmp/stack.netlist'.
185
186
187 You could run (for example) the `spice-sdb' backend against the
188 schematic if you specified `-g spice-sdb', or you could generate a
189 bill of materials for the schematic using `-g partslist1'.
190
191
192 To obtain a Scheme prompt to run Scheme expressions directly, you can
193 use the `-i' option.
194
195 ./gnetlist -i stack_1.sch
196
197
198 gnetlist will load `stack_1.sh', and then enter an interactive
199 Scheme read-eval-print loop.
200
201
203 GEDADATA
204 specifies the search directory for Scheme and rc files. The
205 default is `${prefix}/share/gEDA'.
206
207 GEDADATARC
208 specifies the search directory for rc files. The default is
209 `$GEDADATA'.
210
211
213 See the `AUTHORS' file included with this program.
214
215
217 Copyright © 1999-2011 gEDA Contributors. License GPLv2+: GNU GPL
218 version 2 or later. Please see the `COPYING' file included with this
219 program for full details.
220
221 This is free software: you are free to change and redistribute it.
222 There is NO WARRANTY, to the extent permitted by law.
223
224
226 gschem(1), gsymcheck(1), pcb(1), gnucap(1)
227
228
229
230gEDA Project September 25th, 2013 gnetlist(1)