Ubuntu Manpage: gsch2pcb-rnd - Update pcb-rnd layouts from gEDA/gaf schematics

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.