gsch2pcb man page on DragonFly
[printable version]
gsch2pcb(1) 1.8.2.20130925 gsch2pcb(1)
NAME
gsch2pcb - Update PCB layouts from gEDA/gaf schematics
SYNOPSIS
gsch2pcb [OPTION ...] {PROJECT | FILE ...}
DESCRIPTION
gsch2pcb is a frontend to gnetlist(1) which aids in creating and updat‐
ing pcb(1) printed circuit board layouts based on a set of electronic
schematics created with gschem(1).
Instead of specifying all options and input gEDA schematic FILEs on the
command line, gsch2pcb can use a PROJECT file instead.
gsch2pcb first runs gnetlist(1) with the `PCB' backend to create a
`<name>.net' file containing a pcb(1) formatted netlist for the design.
The second step is to run gnetlist(1) 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 `<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, gnetlist(1) is run a third time with the `pcbpins' backend 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
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).
-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 pre‐
process 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.
--gnetlist BACKEND
In addition to the default backends, run gnetlist(1) with `-g
BACKEND', with output to `<name>.BACKEND'.
--gnetlist-arg ARG
Pass ARG as an additional argument to gnetlist(1).
--empty-footprint NAME
If NAME is not `none', gsch2pcb will not add elements for com‐
ponents 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 `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 speci‐
fied 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) 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), gnetlist(1), pcb(1)
gEDA Project September 25th, 2013 gsch2pcb(1)
[top]
List of man pages available for DragonFly
Copyright (c) for man pages and the logo by the respective OS vendor.
For those who want to learn more, the polarhome community provides shell access and support.
[legal]
[privacy]
[GNU]
[policy]
[cookies]
[netiquette]
[sponsors]
[FAQ]
Polarhome, production since 1999.
Member of Polarhome portal.
Based on Fawad Halim's script.
....................................................................
|
|
Vote for polarhome
|
