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	updat-
       ing 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 el-
       ements 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
       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	`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
	       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 pre-
	       process 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  com-
	       ponents with that name to the PCB file.	Note that if the omit-
	       ted 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	speci-
	       fied  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  `--'  re-
       moved,	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 (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)

NAME | SYNOPSIS | DESCRIPTION | OPTIONS | PROJECT FILES | ENVIRONMENT | AUTHORS | COPYRIGHT | SEE ALSO

Want to link to this manual page? Use this URL:
<https://www.freebsd.org/cgi/man.cgi?query=gsch2pcb&sektion=1&manpath=FreeBSD+12.0-RELEASE+and+Ports>

home | help