DragonFly On-Line Manual Pages

gsch2pcb(1)                     1.8.2.20130925                     gsch2pcb(1)

NAME
       gsch2pcb - Update PCB layouts from gEDA/gaf schematics

SYNOPSIS
       gsch2pcb [OPTION ...] {PROJECT | FILE ...}

DESCRIPTION
       gsch2pcb is a frontend to gnetlist(1) which aids in creating and
       updating pcb(1) printed circuit board layouts based on a set of
       electronic schematics created with gschem(1).

       Instead of specifying all options and input gEDA schematic FILEs on the
       command line, gsch2pcb can use a PROJECT file instead.

       gsch2pcb first runs gnetlist(1) with the `PCB' backend to create a
       `<name>.net' file containing a pcb(1) formatted netlist for the design.

       The second step is to run gnetlist(1) again with the `gsch2pcb' backend
       to find any M4(1) elements required by the schematics.  Any missing
       elements are found by searching a set of file element directories.  If
       no `<name>.pcb' file exists for the design yet, it is created with the
       required elements; otherwise, any new elements are output to a
       `<name>.new.pcb' file.

       If a `<name>.pcb' file exists, it is searched for elements with a non-
       empty element name with no matching schematic symbol.  These elements
       are removed from the `<name>.pcb' file, with a backup in a
       `<name>.pcb.bak' file.

       Finally, gnetlist(1) is run a third time with the `pcbpins' backend to
       create a `<name>.cmd' file.  This can be loaded into pcb(1) to rename
       all pin names in the PCB layout to match the schematic.

OPTIONS
       -o, --output-name=BASENAME
               Use output filenames `BASENAME.net', `BASENAME.pcb', and
               `BASENAME.new.pcb'.  By default, the basename of the first
               schematic file in the list of input files is used.

       -d, --elements-dir=DIRECTORY
               Add DIRECTORY to the list of directories to search for PCB file
               elements.  By default, the following directories are searched
               if they exist: `./packages', `/usr/local/share/pcb/newlib',
               `/usr/share/pcb/newlib', `/usr/local/lib/pcb_lib',
               `/usr/lib/pcb_lib', `/usr/local/pcb_lib'.

       -f, --use-files
               Force use of file elements in preference to elements generated
               with M4(1).

       -s, --skip-m4
               Disable element generation using M4(1) entirely.

       --m4-file FILE
               Use the M4(1) file FILE in addition to the default M4 files
               `./pcb.inc' and `~/.pcb/pcb.inc'.

       --m4-pcbdir DIRECTORY
               Set DIRECTORY as the directory where gsch2pcb should look for
               M4(1) files installed by pcb(1).

       -r, --remove-unfound
               Don't include references to unfound elements in the generated
               `.pcb' files.  Use if you want pcb(1) to be able to load the
               (incomplete) `.pcb' file.  This is enabled by default.

       -k, --keep-unfound
               Keep include references to unfound elements in the generated
               `.pcb' files.  Use if you want to hand edit or otherwise
               preprocess the generated `.pcb' file before running pcb(1).

       -p, --preserve
               Preserve elements in PCB files which are not found in the
               schematics.  Since elements with an empty element name
               (schematic "refdes") are never deleted, this option is rarely
               useful.

       --gnetlist BACKEND
               In addition to the default backends, run gnetlist(1) with `-g
               BACKEND', with output to `<name>.BACKEND'.

       --gnetlist-arg ARG
               Pass ARG as an additional argument to gnetlist(1).

       --empty-footprint NAME
               If NAME is not `none', gsch2pcb will not add elements for
               components with that name to the PCB file.  Note that if the
               omitted components have net connections, they will still appear
               in the netlist and pcb(1) will warn that they are missing.

       --fix-elements
               If a schematic component's `footprint' attribute is not equal
               to the `Description' of the corresponding PCB element, update
               the `Description' instead of replacing the element.

       -q, --quiet
               Don't output information on steps to take after running
               gsch2pcb.

       -v, --verbose
               Output extra debugging information.  This option can be
               specified twice (`-v -v') to obtain additional debugging for
               file elements.

       -h, --help
               Print a help message.

       -V, --version
               Print gsch2pcb version information.

PROJECT FILES
       A gsch2pcb project file is a file (not ending in `.sch') containing a
       list of schematics to process and some options.  Any long-form command
       line option can appear in the project file with the leading `--'
       removed, with the exception of `--gnetlist-arg', `--fix-elements',
       `--verbose', and `--version'.  Schematics should be listed on a line
       beginning with `schematics'.

       An example project file might look like:

            schematics partA.sch partB.sch
            output-name design

ENVIRONMENT
       GNETLIST
               specifies the gnetlist(1) program to run.  The default is
               `gnetlist'.

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), gnetlist(1), pcb(1)

gEDA Project                 September 25th, 2013                  gsch2pcb(1)