gnetlist man page

gnetlist — gEDA/gaf Netlist Extraction and Generation

Synopsis

gnetlist [OPTION ...] [-g BACKEND] [--] FILE ...

Description

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.

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'.
-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'.

Authors

See the `Authors' file included with this program.

See Also

gschem(1), gsymcheck(1), pcb(1), gnucap(1)

Referenced By

gsch2pcb(1), gschem(1), gsymcheck(1), pads_backannotate(1), pcb_backannotate(1).

September 25th, 2013 gEDA Project 1.8.2.20130925