Provided by: lepton-eda_1.9.6-1_amd64 bug

NAME

       lepton-netlist - Lepton EDA Netlist Extraction and Generation

SYNOPSIS

       lepton-netlist [OPTION ...] [-g BACKEND] [--] FILE ...

DESCRIPTION

       lepton-netlist  is a netlist extraction and generation tool, and is part of the Lepton EDA
       (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  lepton-netlist  run  is  carried  out  in two steps.  First, the lepton-netlist
       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.

       lepton-netlist 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'.   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  lepton-netlist  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.

       -w      Do not display warnings about missing configuration files.

       -h, --help
               Print a help message.

       -V, --version
               Print lepton-netlist version information.

       --      Treat  all  remaining  arguments  as  schematic filenames.  Use this if you have a
               schematic filename which begins with `-'.

BACKENDS

       Currently, lepton-netlist 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.

       lepton-netlist requires that at least one schematic to be specified on the command line:

            ./lepton-netlist stack_1.sch

       This is not very useful since it does not direct lepton-netlist to do
       anything.

       Specify a backend name with `-g' to get lepton-netlist to output a
       netlist:

            ./lepton-netlist -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:

            ./lepton-netlist -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.

            ./lepton-netlist -i stack_1.sch

       lepton-netlist 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/lepton-eda'.

       GEDADATARC
               specifies the search directory for rc files.  The default is `$GEDADATA'.

AUTHORS

       See the `AUTHORS' file included with this program.

COPYRIGHT

       Copyright © 2012-2017 gEDA Contributors.
       Copyright © 2017-2018 Lepton Developers.
       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

       lepton-schematic(1), lepton-symcheck(1), pcb(1), gnucap(1)