bionic (1) gsch2pcb.1.gz

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 © 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)