lepton-netlist

NAME
SYNOPSIS
DESCRIPTION
GENERAL OPTIONS
BACKENDS
EXAMPLES
AUTHORS
COPYRIGHT
SEE ALSO

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

-q, --quiet

Quiet mode. Turns off all warnings/notes/messages.

-v, --verbose

Verbose mode. Output all diagnostic information.

-L, --lepton-path=DIRECTORY

Prepend DIRECTORY to the list of directories to be searched for Scheme files. It is done before loading and/or evaluating any Scheme code. This option can be specified multiple times.

-g, --backend=BACKEND

Specify the netlist backend to be used.

-f, --file-backend=FILE

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).

-O, --backend-option=STRING

Pass an option string to the backend.

-b, --list-backends

Print a list of available netlist backends.

-o, --output=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, --pre-load=FILE

Specify a Scheme file to be loaded before the backend is loaded or executed. This option can be specified multiple times.

-m, --post-load=FILE

Specify a Scheme file to be loaded between loading the backend and executing it. This option can be specified multiple times.

-c, --eval-code=EXPR

Specify a Scheme expression to be executed during lepton-netlist startup. This option can be specified multiple times.

-i, --interactive

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 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.
	tEDAx		Trivial EDA eXchange (tEDAx) 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.

AUTHORS

See the ‘AUTHORS’ file included with this program.

COPYRIGHT

This is free software: you are free to change and redistribute it.
There is NO WARRANTY, to the extent permitted by law.