Quick Navigator

Search Site

Unix VPS
A - Starter
B - Basic
C - Preferred
D - Commercial
MPS - Dedicated
Previous VPSs
* Sign Up! *

Contact Us
Online Help
Domain Status
Man Pages

Virtual Servers

Topology Map

Server Agreement
Year 2038

USA Flag



Man Pages

Manual Reference Pages  -  GNETLIST (1)


gnetlist - gEDA/gaf Netlist Extraction and Generation


General Options
See Also


gnetlist [OPTION ...] [-g BACKEND] [--] FILE ...


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.


-q Quiet mode. Turns off all warnings/notes/messages.
-v, --verbose
  Verbose mode. Output all diagnostic information.
  Prepend DIRECTORY to the list of directories to be searched for Scheme files.
  Specify the netlist backend to be used.
  Pass an option string to the backend.
  Print a list of available netlist backends.
-o FILE Specify the filename for the generated netlist. By default, output is directed to ‘’.
-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 ‘-’.


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 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 netlist format.
  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.


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 ‘’ 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 ‘’, and then enter an interactive Scheme read-eval-print loop.


GEDADATA specifies the search directory for Scheme and rc files. The default is ‘${prefix}/share/gEDA’.
  specifies the search directory for rc files. The default is ‘$GEDADATA’.


See the ‘AUTHORS’ file included with this program.


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.


gschem(1), gsymcheck(1), pcb(1), gnucap(1)
Search for    or go to Top of page |  Section 1 |  Main Index

gEDA Project GNETLIST (1) September 25th, 2013

Powered by GSP Visit the GSP FreeBSD Man Page Interface.
Output converted with manServer 1.07.