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)