Provided by: geda-gnetlist_1.8.2-11_amd64 bug


       gnetlist - gEDA/gaf Netlist Extraction and Generation


       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.

       -g BACKEND
               Specify the netlist backend to be used.

       -O STRING
               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.

               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 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.

               Protel II netlist format.

       redac   RACAL-REDAC netlist format.

       spice, spice-sdb
               SPICE-compatible netlist format (spice-sdb is recommended).  Suitable for use with

       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

       Specify a backend name with `-g' to get gnetlist to output a

            ./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.


               specifies  the  search  directory  for  Scheme  and  rc  files.   The  default  is

               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)