FreeBSD Manual Pages
gnetlist(1) 1.8.2.20130925 gnetlist(1) NAME 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 elec- tronic schematics as input, and outputs a netlist. A netlist is a machine- interpretable description of the way that components in an electronic cir- cuit 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 ex- port 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 diagnos- tics). 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). Suit- able 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 direc- tory. gnetlist requires that at least one schematic to be specified on the com- mand 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 de- fault 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. COPYRIGHT Copyright (C) 1999-2011 gEDA Contributors. 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 gschem(1), gsymcheck(1), pcb(1), gnucap(1) gEDA Project September 25th, 2013 gnetlist(1)
NAME | SYNOPSIS | DESCRIPTION | GENERAL OPTIONS | BACKENDS | EXAMPLES | ENVIRONMENT | AUTHORS | COPYRIGHT | SEE ALSO
Want to link to this manual page? Use this URL:
<https://man.freebsd.org/cgi/man.cgi?query=gnetlist&sektion=1&manpath=FreeBSD+Ports+15.1.quarterly>