DragonFly On-Line Manual Pages
gnetlist(1) 1.8.2.20130925 gnetlist(1)
NAME
gnetlist - gEDA/gaf Netlist Extraction and Generation
SYNOPSIS
gnetlist [OPTION ...] [-g BACKEND] [--] FILE ...
DESCRIPTION
gnetlist is a netlist extraction and generation tool, and is part of
the gEDA (GPL Electronic Design Automation) toolset. It takes one or
electronic schematics as input, and outputs a netlist. A netlist is a
machine-interpretable description of the way that components in an
electronic circuit are connected together, and is commonly used as the
input to a PCB layout program such as pcb(1) or to a simulator such as
gnucap(1).
A normal gnetlist run is carried out in two steps. First, the gnetlist
frontend loads the specified human-readable schematic FILEs, and
compiles them to an in-memory netlist description. Next, a `backend'
is used to export the connection and component data to one of many
supported netlist formats.
gnetlist is extensible, using the Scheme programming language.
GENERAL OPTIONS
-q Quiet mode. Turns off all warnings/notes/messages.
-v, --verbose
Verbose mode. Output all diagnostic information.
-L DIRECTORY
Prepend DIRECTORY to the list of directories to be searched for
Scheme files.
-g BACKEND
Specify the netlist backend to be used.
-O STRING
Pass an option string to the backend.
--list-backends
Print a list of available netlist backends.
-o FILE Specify the filename for the generated netlist. By default,
output is directed to `output.net'.
-l FILE Specify a Scheme file to be loaded before the backend is loaded
or executed. This option can be specified multiple times.
-m FILE Specify a Scheme file to be loaded between loading the backend
and executing it. This option can be specified multiple times.
-c EXPR Specify a Scheme expression to be executed during gnetlist
startup. This option can be specified multiple times.
-i After the schematic files have been loaded and compiled, and
after all Scheme files have been loaded, but before running the
backend, enter a Scheme read-eval-print loop.
-h, --help
Print a help message.
-V, --version
Print gnetlist version information.
-- Treat all remaining arguments as schematic filenames. Use this
if you have a schematic filename which begins with `-'.
BACKENDS
Currently, gnetlist includes the following backends:
allegro Allegro netlist format.
bae Bartels Autoengineer netlist format.
bom, bom2
Bill of materials generation.
calay Calay netlist format.
cascade RF Cascade netlist format
drc, drc2
Design rule checkers (drc2 is recommended).
eagle Eagle netlist format.
ewnet Netlist format for National Instruments ULTIboard layout tool.
futurenet2
Futurenet2 netlist format.
geda Native gEDA netlist format (mainly used for testing and
diagnostics).
gossip Gossip netlist format.
gsch2pcb
Backend used for pcb(1) file layout generation by gsch2pcb(1).
It is not recommended to use this backend directly.
liquidpcb
LiquidPCB netlist format.
mathematica
Netlister for analytical circuit solving using Mathematica.
maxascii
MAXASCII netlist format.
osmond Osmond netlist format.
pads PADS netlist format.
partslist1, partslist2, partslist3
Bill of materials generation backends (alternatives to bom and
bom2).
PCB pcb(1) netlist format.
pcbpins Generates a pcb(1) action file for forward annotating pin/pad
names from schematic to layout.
protelII
Protel II netlist format.
redac RACAL-REDAC netlist format.
spice, spice-sdb
SPICE-compatible netlist format (spice-sdb is recommended).
Suitable for use with gnucap(1).
switcap SWITCAP switched capacitor simulator netlist format.
systemc Structural SystemC code generation.
tango Tango netlist format.
vams VHDL-AMS code generation.
verilog Verilog code generation.
vhdl VHDL code generation.
vipec ViPEC Network Analyser netlist format.
EXAMPLES
These examples assume that you have a `stack_1.sch' in the current
directory.
gnetlist requires that at least one schematic to be specified on the
command line:
./gnetlist stack_1.sch
This is not very useful since it does not direct gnetlist to do
anything.
Specify a backend name with `-g' to get gnetlist to output a
netlist:
./gnetlist -g geda stack_1.sch
The netlist output will be written to a file called `output.net'
in the current working directory.
You can specify the output filename by using the `-o' option:
./gnetlist -g geda stack_1.sch -o /tmp/stack.netlist
Output will now be directed to `/tmp/stack.netlist'.
You could run (for example) the `spice-sdb' backend against the
schematic if you specified `-g spice-sdb', or you could generate a
bill of materials for the schematic using `-g partslist1'.
To obtain a Scheme prompt to run Scheme expressions directly, you can
use the `-i' option.
./gnetlist -i stack_1.sch
gnetlist will load `stack_1.sh', and then enter an interactive
Scheme read-eval-print loop.
ENVIRONMENT
GEDADATA
specifies the search directory for Scheme and rc files. The
default is `${prefix}/share/gEDA'.
GEDADATARC
specifies the search directory for rc files. The default is
`$GEDADATA'.
AUTHORS
See the `AUTHORS' file included with this program.
COPYRIGHT
Copyright (C) 1999-2011 gEDA Contributors. License GPLv2+: GNU GPL
version 2 or later. Please see the `COPYING' file included with this
program for full details.
This is free software: you are free to change and redistribute it.
There is NO WARRANTY, to the extent permitted by law.
SEE ALSO
gschem(1), gsymcheck(1), pcb(1), gnucap(1)
gEDA Project September 25th, 2013 gnetlist(1)