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 © 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.

RELATED TO gnetlist…

gschem(1), gsymcheck(1), pcb(1), gnucap(1)

gnetlist (1)