1gsch2pcb(1) 1.8.2.20130925 gsch2pcb(1)
2
6 gsch2pcb - Update PCB layouts from gEDA/gaf schematics
7
9 gsch2pcb [OPTION ...] {PROJECT | FILE ...}
10
12 gsch2pcb is a frontend to gnetlist(1) which aids in creating and updat‐
13 ing pcb(1) printed circuit board layouts based on a set of electronic
14 schematics created with gschem(1).
15 Instead of specifying all options and input gEDA schematic FILEs on the
18 command line, gsch2pcb can use a PROJECT file instead.
19 gsch2pcb first runs gnetlist(1) with the `PCB' backend to create a
22 `<name>.net' file containing a pcb(1) formatted netlist for the design.
23 The second step is to run gnetlist(1) again with the `gsch2pcb' backend
26 to find any M4(1) elements required by the schematics. Any missing
27 elements are found by searching a set of file element directories. If
28 no `<name>.pcb' file exists for the design yet, it is created with the
29 required elements; otherwise, any new elements are output to a
30 `<name>.new.pcb' file.
31 If a `<name>.pcb' file exists, it is searched for elements with a non-
34 empty element name with no matching schematic symbol. These elements
35 are removed from the `<name>.pcb' file, with a backup in a
36 `<name>.pcb.bak' file.
37 Finally, gnetlist(1) is run a third time with the `pcbpins' backend to
40 create a `<name>.cmd' file. This can be loaded into pcb(1) to rename
41 all pin names in the PCB layout to match the schematic.
42
45 -o, --output-name=BASENAME
46 Use output filenames `BASENAME.net', `BASENAME.pcb', and `BASE‐
47 NAME.new.pcb'. By default, the basename of the first schematic
48 file in the list of input files is used.
49 -d, --elements-dir=DIRECTORY
51 Add DIRECTORY to the list of directories to search for PCB file
52 elements. By default, the following directories are searched
53 if they exist: `./packages', `/usr/local/share/pcb/newlib',
54 `/usr/share/pcb/newlib', `/usr/local/lib/pcb_lib',
55 `/usr/lib/pcb_lib', `/usr/local/pcb_lib'.
56 -f, --use-files
58 Force use of file elements in preference to elements generated
59 with M4(1).
60 -s, --skip-m4
62 Disable element generation using M4(1) entirely.
63 --m4-file FILE
65 Use the M4(1) file FILE in addition to the default M4 files
66 `./pcb.inc' and `~/.pcb/pcb.inc'.
67 --m4-pcbdir DIRECTORY
69 Set DIRECTORY as the directory where gsch2pcb should look for
70 M4(1) files installed by pcb(1).
71 -r, --remove-unfound
73 Don't include references to unfound elements in the generated
74 `.pcb' files. Use if you want pcb(1) to be able to load the
75 (incomplete) `.pcb' file. This is enabled by default.
76 -k, --keep-unfound
78 Keep include references to unfound elements in the generated
79 `.pcb' files. Use if you want to hand edit or otherwise pre‐
80 process the generated `.pcb' file before running pcb(1).
81 -p, --preserve
83 Preserve elements in PCB files which are not found in the
84 schematics. Since elements with an empty element name
85 (schematic "refdes") are never deleted, this option is rarely
86 useful.
87 --gnetlist BACKEND
89 In addition to the default backends, run gnetlist(1) with `-g
90 BACKEND', with output to `<name>.BACKEND'.
91 --gnetlist-arg ARG
93 Pass ARG as an additional argument to gnetlist(1).
94 --empty-footprint NAME
96 If NAME is not `none', gsch2pcb will not add elements for com‐
97 ponents with that name to the PCB file. Note that if the omit‐
98 ted components have net connections, they will still appear in
99 the netlist and pcb(1) will warn that they are missing.
100 --fix-elements
102 If a schematic component's `footprint' attribute is not equal
103 to the `Description' of the corresponding PCB element, update
104 the `Description' instead of replacing the element.
105 -q, --quiet
107 Don't output information on steps to take after running
108 gsch2pcb.
109 -v, --verbose
111 Output extra debugging information. This option can be speci‐
112 fied twice (`-v -v') to obtain additional debugging for file
113 elements.
114 -h, --help
116 Print a help message.
117 -V, --version
119 Print gsch2pcb version information.
120
123 A gsch2pcb project file is a file (not ending in `.sch') containing a
124 list of schematics to process and some options. Any long-form command
125 line option can appear in the project file with the leading `--'
126 removed, with the exception of `--gnetlist-arg', `--fix-elements',
127 `--verbose', and `--version'. Schematics should be listed on a line
128 beginning with `schematics'.
129 An example project file might look like:
131 schematics partA.sch partB.sch
133 output-name design
134
137 GNETLIST
138 specifies the gnetlist(1) program to run. The default is
139 `gnetlist'.
140
143 See the `AUTHORS' file included with this program.
144
147 Copyright © 1999-2011 gEDA Contributors. License GPLv2+: GNU GPL
148 version 2 or later. Please see the `COPYING' file included with this
149 program for full details.
150 This is free software: you are free to change and redistribute it.
152 There is NO WARRANTY, to the extent permitted by law.
153
156 gschem(1), gnetlist(1), pcb(1)
157gEDA Project September 25th, 2013 gsch2pcb(1)