--- name: "gsch2pcb" section: "1" platform: "linux" package: "geda-utils" version: "1:1.8.2-11" release: "Debian 10 (Buster)" platforms: ["linux"] url: "https://new.carta.tech/gsch2pcb" --- # gsch2pcb(1) Update PCB layouts from gEDA/gaf schematics ## NAME gsch2pcb - Update PCB layouts from gEDA/gaf schematics ## SYNOPSIS **gsch2pcb** \[*OPTION* ...\] {*PROJECT* \| *FILE* ...} ## DESCRIPTION **gsch2pcb** is a frontend to [**gnetlist**(1)](/gnetlist/1.md) which aids in creating and updating [**pcb**(1)](/pcb/1.md) printed circuit board layouts based on a set of electronic schematics created with [**gschem**(1)](/gschem/1.md). Instead of specifying all options and input gEDA schematic *FILE*s on the command line, **gsch2pcb** can use a *PROJECT* file instead. **gsch2pcb** first runs [**gnetlist**(1)](/gnetlist/1.md) with the \`PCB' backend to create a \`\.net' file containing a [**pcb**(1)](/pcb/1.md) formatted netlist for the design. The second step is to run [**gnetlist**(1)](/gnetlist/1.md) 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 \`\.pcb' file exists for the design yet, it is created with the required elements; otherwise, any new elements are output to a \`\.new.pcb' file. If a \`\.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 \`\.pcb' file, with a backup in a \`\.pcb.bak' file. Finally, [**gnetlist**(1)](/gnetlist/1.md) is run a third time with the \`pcbpins' backend to create a \`\.cmd' file. This can be loaded into [**pcb**(1)](/pcb/1.md) 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)](/pcb/1.md). - **-r**, **--remove-unfound** Don't include references to unfound elements in the generated \`.pcb' files. Use if you want [**pcb**(1)](/pcb/1.md) 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)](/pcb/1.md). - **-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)](/gnetlist/1.md) with \`-g *BACKEND*', with output to \`\.*BACKEND*'. - **--gnetlist-arg** *ARG* Pass *ARG* as an additional argument to [**gnetlist**(1)](/gnetlist/1.md). - **--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)](/pcb/1.md) 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)](/gnetlist/1.md) 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)](/gschem/1.md), [**gnetlist**(1)](/gnetlist/1.md), [**pcb**(1)](/pcb/1.md)