Skip site navigation (1)Skip section navigation (2)

FreeBSD Manual Pages

  
 
  

home | help 
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	schemat-
     ics 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  re-
     quired   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 cre-
     ate 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 `BASE-
	     NAME.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 el-
	     ements.  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 (in-
	     complete) `.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 schemat-
	     ics.   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 BACK-
	     END', 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 compo-
	     nents 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 `De-
	     scription' 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 op-
     tion can appear in the project file with the leading `--' removed, with the
     exception of `--gnetlist-arg', `--fix-elements', `--verbose',  and  `--ver-
     sion'.  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)

Want to link to this manual page? Use this URL:
<https://man.freebsd.org/cgi/man.cgi?query=gsch2pcb&sektion=1&manpath=FreeBSD+Ports+15.1.quarterly>

home | help