lepton-sch2pcb - Update PCB layouts from Lepton EDA schematics
lepton-sch2pcb [OPTION ...] {PROJECT |
FILE ...}
lepton-sch2pcb is a frontend to lepton-netlist(1)
which aids in creating and updating pcb(1) printed circuit board
layouts based on a set of electronic schematics created with
lepton-schematic(1).
Instead of specifying all options and input schematic FILEs
on the command line, lepton-sch2pcb can use a PROJECT file
instead.
lepton-sch2pcb first runs lepton-netlist(1) with the
`PCB' backend (or backend specified by --backend-net) to create a
`<name>.net' file containing a pcb(1) formatted netlist for the
design.
The second step is to run lepton-netlist(1) again with the
`gsch2pcb' backend (or backend specified by --backend-pcb) 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, lepton-netlist(1) is run a third time with the
`pcbpins' backend (or backend specified by --backend-cmd) 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 lepton-sch2pcb 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.
- --backend-cmd
BACKEND
- Use BACKEND to generate `<name>.cmd' file instead of the
default one (`pcbpins').
- --backend-net
BACKEND
- Use BACKEND to generate `<name>.net' file instead of the
default one (`PCB').
- --backend-pcb
BACKEND
- Use BACKEND to generate `<name>.pcb' file instead of the
default one (`gsch2pcb').
- --gnetlist
BACKEND
- In addition to the default backends, run lepton-netlist(1) with `-g
BACKEND', with output to `<name>.BACKEND'.
- --gnetlist-arg
ARG
- Pass ARG as an additional argument to
lepton-netlist(1).
- If NAME is not `none', lepton-sch2pcb 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
lepton-sch2pcb.
- -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 lepton-sch2pcb version information.
A lepton-sch2pcb 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
See the `AUTHORS' file included with this program.
Copyright © 2012-2017 gEDA Contributors.
Copyright © 2017-2018 Lepton Developers.
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.