gnetlist1

Usage

Overview

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.

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'.

-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 `-'.

Backends

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

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.

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 anything.

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

	./gnetlist -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:

	./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 `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/gEDA'.

GEDADATARC

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