NAME

       gsch2pcb-rnd - Update pcb-rnd layouts from gEDA/gaf schematics

SYNOPSIS

       gsch2pcb-rnd [OPTION ...] {PROJECT | FILE ...}

DESCRIPTION

       gsch2pcb-rnd  is  a frontend to gnetlist(1) which aids in creating and updating pcb-rnd(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-rnd can use a PROJECT file instead.

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

       The  second  step  is to run gnetlist(1) again with the `gsch2pcb-rnd' 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-rnd(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.

       -r, --remove-unfound
               Don't  include  references to unfound elements in the generated `.pcb' files.  Use
               if you want pcb-rnd(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-rnd 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-rnd(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-rnd.

       -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-rnd version information.

PROJECT FILES

       A gsch2pcb-rnd 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 © 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-rnd(1)