Provided by: pcb-rnd_1.2.5-1_amd64 bug


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


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


       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

       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.


       -o, --output-name=BASENAME
               Use  output  filenames  `',   `BASENAME.pcb',   and
               `'.   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

       -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

       --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.

               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

       -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.


       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


               specifies the gnetlist(1)  program  to  run.   The  default  is


       See the `AUTHORS' file included with this program.


       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.


       gschem(1), gnetlist(1), pcb-rnd(1)