docs/wiki/geda_gsch2pcb_readme.html

   1 <!DOCTYPE html PUBLIC "-//W3C//DTD XHTML 1.0 Transitional//EN"
   2  "http://www.w3.org/TR/xhtml1/DTD/xhtml1-transitional.dtd">
   3 <html xmlns="http://www.w3.org/1999/xhtml" xml:lang="en"
   4  lang="en" dir="ltr">
   5 <head>
   6   <meta http-equiv="Content-Type" content="text/html; charset=utf-8" />
   7   <title>geda:gsch2pcb_readme</title>
   8 <meta name="generator" content="DokuWiki Release rc2007-05-24" />
   9 <meta name="robots" content="index,follow" />
  10 <meta name="date" content="2007-05-24T22:27:24-0400" />
  11 <meta name="keywords" content="geda,gsch2pcb_readme" />
  12 <link rel="search" type="application/opensearchdescription+xml" href="http://geda.seul.org/wiki/lib/exe/opensearch.php" title="geda Wiki" />
  13 <link rel="start" href="http://geda.seul.org/wiki/" />
  14 <link rel="contents" href="http://geda.seul.org/wiki/geda:gsch2pcb_readme?do=index" title="Index" />
  15 <link rel="alternate" type="application/rss+xml" title="Recent Changes" href="http://geda.seul.org/wiki/feed.php" />
  16 <link rel="alternate" type="application/rss+xml" title="Current Namespace" href="http://geda.seul.org/wiki/feed.php?mode=list&ns=geda" />
  17 <link rel="alternate" type="text/html" title="Plain HTML" href="http://geda.seul.org/wiki/_export/xhtml/geda:gsch2pcb_readme" />
  18 <link rel="alternate" type="text/plain" title="Wiki Markup" href="http://geda.seul.org/wiki/_export/raw/geda:gsch2pcb_readme" />
  19 <link rel="stylesheet" media="all" type="text/css" href="lib/exe/css" />
  20 <link rel="stylesheet" media="screen" type="text/css" href="lib/exe/001css" />
  21 <link rel="stylesheet" media="print" type="text/css" href="lib/exe/002css" />
  22 </head>
  23 <body>
  24 <div class="dokuwiki export">
  25
  26
  27
  28 <h1><a name="gsch2pcb_gschem_to_pcb_readme" id="gsch2pcb_gschem_to_pcb_readme">gsch2pcb (gschem to PCB) README</a></h1>
  29 <div class="level1">
  30 <pre class="code">gsch2pcb
  31 --------
  32 gsch2pcb is a program that interfaces a set of schematics generated with
  33 with the gEDA gschem to PCB layout files.
  34
  35 gsch2pcb is conceptually similar to the gschem2pcb shell script, but
  36 additionally handles multiple schematics, handles file element footprints,
  37 and removes pc board elements corresponding to components deleted from the
  38 schematics.  It also forward annotates component value changes.
  39
  40 Using gsch2pcb allows you to drive all design changes from the gschem
  41 schematics without the headache of manually keeping PCB elements and
  42 element values in sync.
  43
  44 It requires that the gnet-gsch2pcb.scm file be install into the gEDA
  45 scheme directory.  On Debian this is /usr/share/gEDA/scheme, but see
  46 the INSTALL file.
  47
  48 Typical usage
  49 -------------
  50 1) Create your custom PCB elements and save each one into its own file.
  51    Some compatibility tips if you will be inserting elements into a
  52    layout manually as well as with gsch2pcb:
  53      *  Make the initial &quot;Description&quot; field of these elements the same
  54         as the file name because gsch2pcb depends on this name (which is
  55         the gschem footprint
  56         value) to know when footprints/elements are changed.
  57      *  Make the initial layout-name field (displayed when the &quot;name on PCB&quot;
  58         menu entry is selected) empty (ie &quot;&quot;) so that gsch2pcb
  59         will not delete your element when you want it to be in the layout
  60         even though it is not in the schematic.  You can later edit the
  61         layout-name to be some refdes value, but I&#039;m not sure it makes sense
  62         to name a PCB element that is not referenced in the schematic.
  63
  64    Note: since once a layout element is named PCB won&#039;t let you reset it
  65    to an empty name, a sort of kludge is that setting the first character
  66    of the layout-name to a non-alphanumeric will protect the element from
  67    being deleted by gsch2pcb.
  68
  69    These file elements should be placed in a directory heirarchy that
  70    gsch2pcb will search.  The default directories /usr/local/pcb_lib and
  71    ./packages are searched in addition to any directories you specify with
  72    --elements-dir dirname arguments to gsch2pcb.
  73
  74 2) Create your schematic with gschem.  Make sure each component has a
  75    unique refdes attribute and a footprint attribute that matches either
  76    a PCB m4 element or one of your custom file element names.  Beware of
  77    file element names that collide with PCB m4 macro names (or specify the
  78    use-files option).
  79    Make a project file if you wish.
  80
  81 3) Run &quot;gsch2pcb foo.sch&quot; or &quot;gsch2pcb myproject&quot; if you&#039;ve created the
  82    myproject file.  If you didn&#039;t specify an output name, this will generate
  83    a foo.pcb and a foo.net file.
  84    If you get errors about footprints not found, you need to create PCB
  85    elements for them and repeat this step until you get no errors.
  86    Or, just run gsch2pcb again and it will shift unfound elements to
  87    foo.new.pcb and you can proceed using PCB on foo.pcb if you wish to
  88    fix the errors from inside of PCB.
  89
  90 4) Run &quot;pcb foo.pcb&quot;.  All the elements will be stacked on top of each other,
  91    so move them to desired locations.  Load the netlist file foo.net and
  92    proceed with using PCB.
  93
  94 5) Modify foo.sch and again run &quot;gsch2pcb foo.sch&quot;.
  95    * If components were added, PCB elements for them will be placed in the
  96      file foo.new.pcb.  If components were deleted, the elements for them
  97      will be removed from foo.pcb and the original foo.pcb will be renamed
  98      to a foo.pcb.bak sequence.
  99    * If elements can&#039;t be found for new schematic footprints, then the
 100      unfound elements will be indicated with PKG_ lines in foo.new.pcb
 101      unless you run &quot;gsch2pcb --remove-unfound foo.sch&quot; which will omit
 102      the PKG_ lines so you can go ahead and load foo.new.pcb into PCB.
 103    * Note that If you have added elements to the .pcb layout which
 104      will not exist on the schematics (mounting holes, etc), make sure
 105       there is no &quot;name on PCB&quot; (the gschem refdes) for them or else gsch2pcb
 106      will delete them when they don&#039;t match a schematic refdes and footprint.
 107      You could use the --preserve option to prevent deleting any elements at
 108      all, but this is really not the best way to use gsch2pcb.
 109
 110 6) Run &quot;pcb foo.pcb&quot; and clean up any dangling traces left over from removed
 111    elements.  Load any new elements in foo.new.pcb with the &quot;Load layout
 112    data to paste-buffer&quot; function.  Load the new netlist foo.net.
 113
 114
 115 Caveats
 116 -------
 117 * gsch2pcb uses a gnetlist backend gnet-gsch2pcb.scm, so be sure when you
 118   install gsch2pcb that the gnet-gsch2pcb.scm file gets installed into the
 119   right place.  Look at the INSTALL file in the tarball.
 120
 121 * WARNING:  if you wish to start processing with gsch2pcb any existing PCB
 122   files that have m4 elements and were originally generated with gschem2pcb,
 123   then be sure to run first with at least gsch2pcb 0.4:
 124
 125      gsch2pcb --fix-elements
 126
 127   on the PCB file schematics or else gsch2pcb will want to delete the
 128   m4 elements.
 129
 130 * footprint information is saved into PCB element&#039;s Description fields,
 131   so it&#039;s probably not a good idea to change element Description values
 132   in your layout while using gsch2pcb unless it is a protected element
 133   that has an empty layout-name.
 134
 135
 136
 137 Bill Wilson    billw@wt.net
 138 </pre>
 139
 140 </div>
 141 </div>
 142 </body>
 143 </html>