Skip site navigation (1)Skip section navigation (2)

FreeBSD Manual Pages

  
 
  

home | help
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  com-
       piles  them  to an in-memory netlist description.  Next,	a `backend' is
       used to export the connection and component data	to one	of  many  sup-
       ported 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 diag-
	       nostics).

       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  di-
       rectory.

       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)

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

Want to link to this manual page? Use this URL:
<https://www.freebsd.org/cgi/man.cgi?query=gnetlist&sektion=1&manpath=FreeBSD+12.0-RELEASE+and+Ports>

home | help