Scroll to navigation

lepton-netlist(1) 1.9.12.20201204 lepton-netlist(1)

NAME

lepton-netlist - Lepton EDA Netlist Extraction and Generation

SYNOPSIS

lepton-netlist [OPTION ...] [-g BACKEND | -f FILE] [--] 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 more 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

Quiet mode. Turns off all warnings/notes/messages.
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.
Load and use netlist backend from FILE. FILE is expected to have name like "gnet-NAME.scm" and contain entry point function NAME (where NAME is the backend's name).
Pass an option string to the backend.
Print a list of available netlist backends.
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.
Specify a Scheme file to be loaded before the backend is loaded or executed. This option can be specified multiple times.
Specify a Scheme file to be loaded between loading the backend and executing it. This option can be specified multiple times.
Specify a Scheme expression to be executed during lepton-netlist startup. This option can be specified multiple times.
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.
Print a help message.
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 netlist format.
Bartels Autoengineer netlist format.
Bill of materials generation.
Calay netlist format.
RF Cascade netlist format
Design rule checkers (drc2 is recommended).
Eagle netlist format.
Netlist format for National Instruments ULTIboard layout tool.
Futurenet2 netlist format.
Native gEDA netlist format (mainly used for testing and diagnostics).
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 netlist format.
PADS netlist format.
Bill of materials generation backends (alternatives to bom and bom2).
pcb(1) netlist format.
Generates a pcb(1) action file for forward annotating pin/pad names from schematic to layout.
Protel II netlist format.
RACAL-REDAC netlist format.
SPICE-compatible netlist format (spice-sdb is recommended). Suitable for use with gnucap(1).
SWITCAP switched capacitor simulator netlist format.
Structural SystemC code generation.
Tango netlist format.
Trivial EDA eXchange (tEDAx) format.
VHDL-AMS code generation.
Verilog code generation.
VHDL code generation.
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.

AUTHORS

See the `AUTHORS' file included with this program.

COPYRIGHT

Copyright © 2012-2017 gEDA Contributors.
Copyright © 2017-2020 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)

December 4, 2020 Lepton EDA