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.