Ubuntu Manpage: lepton-sch2pcb - Update PCB layouts from Lepton EDA schematics

NAME

       lepton-sch2pcb - Update PCB layouts from Lepton EDA schematics

SYNOPSIS

       lepton-sch2pcb [OPTION ...] {PROJECT | FILE ...}

DESCRIPTION

       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.

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 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).

--empty-footprint NAME
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.

PROJECT FILES

       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

ENVIRONMENT

       NETLISTER
               specifies the netlister(1) program to run.  The default is `lepton-netlist'.

AUTHOR

       Bill Wilson

COPYRIGHT

       Copyright © 2012-2017 gEDA Contributors.
       Copyright © 2017-2022 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.