gsch2pcb-rnd(1)

1gsch2pcb-rnd(1)                 1.8.2.20130925                 gsch2pcb-rnd(1)
2
3
4

NAME

6       gsch2pcb-rnd - Update pcb-rnd layouts from gEDA/gaf schematics
7

SYNOPSIS

9       gsch2pcb-rnd [OPTION ...] {PROJECT | FILE ...}
10

DESCRIPTION

12       gsch2pcb-rnd  is  a  frontend to gnetlist(1) which aids in creating and
13       updating pcb-rnd(1) printed circuit board layouts based  on  a  set  of
14       electronic schematics created with gschem(1).
15
16
17       Instead of specifying all options and input gEDA schematic FILEs on the
18       command line, gsch2pcb-rnd can use a PROJECT file instead.
19
20
21       gsch2pcb-rnd first runs gnetlist(1) with the `PCB' backend to create  a
22       `<name>.net'  file  containing  a  pcb-rnd(1) formatted netlist for the
23       design.
24
25
26       The second step is to run gnetlist(1)  again  with  the  `gsch2pcb-rnd'
27       backend  to  find  any  M4(1) elements required by the schematics.  Any
28       missing elements are found by searching a set of file element  directo‐
29       ries.  If no `<name>.pcb' file exists for the design yet, it is created
30       with the required elements; otherwise, any new elements are output to a
31       `<name>.new.pcb' file.
32
33
34       If  a `<name>.pcb' file exists, it is searched for elements with a non-
35       empty element name with no matching schematic symbol.   These  elements
36       are   removed   from   the  `<name>.pcb'  file,  with  a  backup  in  a
37       `<name>.pcb.bak' file.
38
39
40       Finally, gnetlist(1) is run a third time with the `pcbpins' backend  to
41       create  a  `<name>.cmd'  file.   This  can be loaded into pcb-rnd(1) to
42       rename all pin names in the PCB layout to match the schematic.
43
44

OPTIONS

46       -o, --output-name=BASENAME
47               Use output filenames `BASENAME.net', `BASENAME.pcb', and `BASE‐
48               NAME.new.pcb'.  By default, the basename of the first schematic
49               file in the list of input files is used.
50
51       -d, --elements-dir=DIRECTORY
52               Add DIRECTORY to the list of directories to search for PCB file
53               elements.
54
55       -r, --remove-unfound
56               Don't  include  references to unfound elements in the generated
57               `.pcb' files.  Use if you want pcb-rnd(1) to be  able  to  load
58               the (incomplete) `.pcb' file.  This is enabled by default.
59
60       -k, --keep-unfound
61               Keep  include  references  to unfound elements in the generated
62               `.pcb' files.  Use if you want to hand edit or  otherwise  pre‐
63               process the generated `.pcb' file before running pcb(1).
64
65       -p, --preserve
66               Preserve  elements  in  PCB  files  which  are not found in the
67               schematics.   Since  elements  with  an  empty   element   name
68               (schematic  "refdes")  are never deleted, this option is rarely
69               useful.
70
71       --gnetlist BACKEND
72               In addition to the default backends, run gnetlist(1)  with  `-g
73               BACKEND', with output to `<name>.BACKEND'.
74
75       --gnetlist-arg ARG
76               Pass ARG as an additional argument to gnetlist(1).
77
78       --empty-footprint NAME
79               If  NAME  is not `none', gsch2pcb-rnd will not add elements for
80               components with that name to the PCB file.  Note  that  if  the
81               omitted components have net connections, they will still appear
82               in the netlist and pcb-rnd(1) will warn that they are missing.
83
84       --fix-elements
85               If a schematic component's `footprint' attribute is  not  equal
86               to  the  `Description' of the corresponding PCB element, update
87               the `Description' instead of replacing the element.
88
89       -q, --quiet
90               Don't  output  information  on  steps  to  take  after  running
91               gsch2pcb-rnd.
92
93       -v, --verbose
94               Output  extra debugging information.  This option can be speci‐
95               fied twice (`-v -v') to obtain additional  debugging  for  file
96               elements.
97
98       -h, --help
99               Print a help message.
100
101       -V, --version
102               Print gsch2pcb-rnd version information.
103
104

PROJECT FILES

106       A gsch2pcb-rnd project file is a file (not ending in `.sch') containing
107       a list of schematics to process and some options.  Any  long-form  com‐
108       mand  line  option can appear in the project file with the leading `--'
109       removed, with  the  exception  of  `--gnetlist-arg',  `--fix-elements',
110       `--verbose',  and  `--version'.   Schematics should be listed on a line
111       beginning with `schematics'.
112
113       An example project file might look like:
114
115            schematics partA.sch partB.sch
116            output-name design
117
118

ENVIRONMENT

120       GNETLIST
121               specifies the gnetlist(1)  program  to  run.   The  default  is
122               `gnetlist'.
123
124

AUTHORS

126       See the `AUTHORS' file included with this program.
127
128

COPYRIGHT

130       Copyright © 1999-2011 gEDA Contributors.  License GPLv2+: GNU GPL
131       version 2 or later.  Please see the `COPYING' file included with this
132       program for full details.
133
134       This is free software: you are free to change and redistribute it.
135       There is NO WARRANTY, to the extent permitted by law.
136
137