FreeBSD Manual Pages
lepton-sch2pcb(1) 1.9.18.20220529 lepton-sch2pcb(1) 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 elec- tronic 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 contain- ing a pcb(1) formatted netlist for the design. The second step is to run lepton-netlist(1) again with the `gsch2pcb' back- end (or backend specified by --backend-pcb) to find any M4(1) elements re- quired 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 `BASE- NAME.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 el- ements. 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 (in- complete) `.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 schemat- ics. 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 omit- ted 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 `De- scription' 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 (C) 2012-2017 gEDA Contributors. Copyright (C) 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. SEE ALSO lepton-schematic(1), lepton-netlist(1), pcb(1) Lepton EDA May 29, 2022 lepton-sch2pcb(1)
NAME | SYNOPSIS | DESCRIPTION | OPTIONS | PROJECT FILES | ENVIRONMENT | AUTHOR | COPYRIGHT | SEE ALSO
Want to link to this manual page? Use this URL:
<https://man.freebsd.org/cgi/man.cgi?query=lepton-sch2pcb&sektion=1&manpath=FreeBSD+Ports+15.1.quarterly>