gsch2pcb man page

gsch2pcb — Update PCB layouts from gEDA/gaf schematics


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


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.


-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.
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


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


See the `Authors' file included with this program.

See Also

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

Referenced By


Explore man page connections for gsch2pcb(1).

gEDA Project September 25th, 2013