lepton-netlist - Lepton EDA Netlist Extraction and Generation
lepton-netlist [OPTION ...] [-g
BACKEND] [--] FILE ...
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.
- -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 `-'.
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.
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.
- 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'.
See the `AUTHORS' file included with this program.
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.