gnetlist

NAME
SYNOPSIS
DESCRIPTION
GENERAL OPTIONS
BACKENDS
EXAMPLES
ENVIRONMENT
AUTHORS
COPYRIGHT
SEE ALSO

NAME

gnetlist - gEDA/gaf Netlist Extraction and Generation

SYNOPSIS

gnetlist [OPTION...] [-p BACKEND|-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 multiple 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. Then, a BACKEND is used to export the connection and component data to one of many supported netlist formats.

gnetlist is extensible in Python and Scheme.

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 Python backends, Scheme backends, and other Scheme files.

-p BACKEND

Specify the Python netlist backend to be used.

-g BACKEND

Specify the Scheme netlist backend to be used.

-O STRING

Pass an option string to the backend.

--list-backends

Print a list of available netlist backends. A backend name is prefixed with the letters ’P’ and ’G’ in brackets if it is available as a Python and as a Scheme backend, respectively.

-o FILE

Specify the filename for the generated netlist. By default, output is directed to ’output.net’. If ’-’ is given instead of a filename, the output is directed to the standard output.

-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 the netlist generated, enter an interactive Python interpreter. The netlist structure is available as ’netlist’ in the local dictionary.

--report-gui

Report warnings and errors in a GUI dialog.

-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).

dumpindent, dumpjson, dumplihata, dumptext, dumpxml

Dump the netlist in various generic formats.

eagle

Eagle netlist format.

ewnet

Netlist format for National Instruments ULTIboard layout tool.

futurenet2

Futurenet2 netlist format.

geda

Internal gEDA netlist format (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.

guile

Compatibility layer for old backends written in Scheme.

liquidpcb

LiquidPCB netlist format.

makedpend

Auto-generate dependencies for Makefiles.

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.

pcbfwd

Internally used by pcb(1)’s "Import Schematics" mechanism.

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-noqsi

SPICE-compatible netlist format (spice-sdb and spice-noqsi are recommended). Suitable for use with gnucap(1).

switcap

SWITCAP switched capacitor simulator netlist format.

systemc

Structural SystemC code generation.

tango

Tango netlist format.

tedax

tEDAx netlist format (used by pcb-rnd(1)).

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 schematic file ’stack_1.sch’ in the current directory.

gnetlist requires that at least one schematic and either a Python backend, a Scheme backend, or interactive mode are specified on the command line. If a backend name is specified with ’-p BACKEND’ (for a Python backend) or ’-g BACKEND’ (for a Scheme backend), gnetlist will output a netlist:

gnetlist -p dumptext 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 -p dumptext -o /tmp/stack.netlist stack_1.sch

Output will now be directed to ’/tmp/stack.netlist’.

You could run (for example) the ’spice-sdb’ backend against the
schematic if you specified ’-p spice-sdb’, or you could generate a
bill of materials for the schematic using ’-p partslist1’.

To obtain a Python prompt to run Python commands directly, you can
use the ’-i’ option.

gnetlist -i stack_1.sch

gnetlist will load ’stack_1.sh’ and then enter an interactive
Python interpreter. The netlist structure is available as ’netlist’
in the local dictionary.

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 © 1999-2020 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), pcb-rnd(1), gnucap(1)