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

FreeBSD Manual Pages


home | help
gsch2pcb(1)			   gsch2pcb(1)

       gsch2pcb	- Update PCB layouts from gEDA/gaf schematics

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

       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.

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

       --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

       --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.

	       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	speci-
	       fied  twice  (`-v  -v') to obtain additional debugging for file

       -h, --help
	       Print a help message.

       -V, --version
	       Print gsch2pcb version information.

       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

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

       See the `AUTHORS' file included with this program.

       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.

       gschem(1), gnetlist(1), pcb(1)

gEDA Project		     September 25th, 2013		   gsch2pcb(1)


Want to link to this manual page? Use this URL:

home | help