gnetlist(1)

1gnetlist(1)                     1.8.2.20130925                     gnetlist(1)
2
3
4

NAME

6       gnetlist - gEDA/gaf Netlist Extraction and Generation
7

SYNOPSIS

9       gnetlist [OPTION ...] [-g BACKEND] [--] FILE ...
10
11

DESCRIPTION

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

GENERAL OPTIONS

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

BACKENDS

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

EXAMPLES

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

ENVIRONMENT

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

AUTHORS

213       See the `AUTHORS' file included with this program.
214
215

COPYRIGHT

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