Differences

This shows you the differences between two versions of the page.

@@ Line 1: / Line 1: @@
+====== gsch2pcb (gschem to PCB) README ======
+<code>gsch2pcb
+--------
+gsch2pcb is a program that interfaces a set of schematics generated with
+with the gEDA gschem to PCB layout files.
+gsch2pcb is conceptually similar to the gschem2pcb shell script, but
+additionally handles multiple schematics, handles file element footprints,
+and removes pc board elements corresponding to components deleted from the
+schematics.  It also forward annotates component value changes.
+Using gsch2pcb allows you to drive all design changes from the gschem
+schematics without the headache of manually keeping PCB elements and
+element values in sync.
+It requires that the gnet-gsch2pcb.scm file be install into the gEDA
+scheme directory.  On Debian this is /usr/share/gEDA/scheme, but see
+the INSTALL file.
+Typical usage
+-------------
+) Create your custom PCB elements and save each one into its own file.
+   Some compatibility tips if you will be inserting elements into a
+   layout manually as well as with gsch2pcb:
+     *  Make the initial "Description" field of these elements the same
+        as the file name because gsch2pcb depends on this name (which is
+        the gschem footprint
+        value) to know when footprints/elements are changed.
+     *  Make the initial layout-name field (displayed when the "name on PCB"
+        menu entry is selected) empty (ie "") so that gsch2pcb
+        will not delete your element when you want it to be in the layout
+        even though it is not in the schematic.  You can later edit the
+        layout-name to be some refdes value, but I'm not sure it makes sense
+        to name a PCB element that is not referenced in the schematic.
+   Note: since once a layout element is named PCB won't let you reset it
+   to an empty name, a sort of kludge is that setting the first character
+   of the layout-name to a non-alphanumeric will protect the element from
+   being deleted by gsch2pcb.
+   These file elements should be placed in a directory heirarchy that
+   gsch2pcb will search.  The default directories /usr/local/pcb_lib and
+   ./packages are searched in addition to any directories you specify with
+   --elements-dir dirname arguments to gsch2pcb.
+) Create your schematic with gschem.  Make sure each component has a
+   unique refdes attribute and a footprint attribute that matches either
+   a PCB m4 element or one of your custom file element names.  Beware of
+   file element names that collide with PCB m4 macro names (or specify the
+   use-files option).
+   Make a project file if you wish.
+) Run "gsch2pcb foo.sch" or "gsch2pcb myproject" if you've created the
+   myproject file.  If you didn't specify an output name, this will generate
+   a foo.pcb and a foo.net file.
+   If you get errors about footprints not found, you need to create PCB
+   elements for them and repeat this step until you get no errors.
+   Or, just run gsch2pcb again and it will shift unfound elements to
+   foo.new.pcb and you can proceed using PCB on foo.pcb if you wish to
+   fix the errors from inside of PCB.
+) Run "pcb foo.pcb".  All the elements will be stacked on top of each other,
+   so move them to desired locations.  Load the netlist file foo.net and
+   proceed with using PCB.
+) Modify foo.sch and again run "gsch2pcb foo.sch".
+   * If components were added, PCB elements for them will be placed in the
+     file foo.new.pcb.  If components were deleted, the elements for them
+     will be removed from foo.pcb and the original foo.pcb will be renamed
+     to a foo.pcb.bak sequence.
+   * If elements can't be found for new schematic footprints, then the
+     unfound elements will be indicated with PKG_ lines in foo.new.pcb
+     unless you run "gsch2pcb --remove-unfound foo.sch" which will omit
+     the PKG_ lines so you can go ahead and load foo.new.pcb into PCB.
+   * Note that If you have added elements to the .pcb layout which
+     will not exist on the schematics (mounting holes, etc), make sure
+      there is no "name on PCB" (the gschem refdes) for them or else gsch2pcb
+     will delete them when they don't match a schematic refdes and footprint.
+     You could use the --preserve option to prevent deleting any elements at
+     all, but this is really not the best way to use gsch2pcb.
+) Run "pcb foo.pcb" and clean up any dangling traces left over from removed
+   elements.  Load any new elements in foo.new.pcb with the "Load layout
+   data to paste-buffer" function.  Load the new netlist foo.net.
+Caveats
+-------
+* gsch2pcb uses a gnetlist backend gnet-gsch2pcb.scm, so be sure when you
+  install gsch2pcb that the gnet-gsch2pcb.scm file gets installed into the
+  right place.  Look at the INSTALL file in the tarball.
+* WARNING:  if you wish to start processing with gsch2pcb any existing PCB
+  files that have m4 elements and were originally generated with gschem2pcb,
+  then be sure to run first with at least gsch2pcb 0.4:
+     gsch2pcb --fix-elements
+  on the PCB file schematics or else gsch2pcb will want to delete the
+  m4 elements.
+* footprint information is saved into PCB element's Description fields,
+  so it's probably not a good idea to change element Description values
+  in your layout while using gsch2pcb unless it is a protected element
+  that has an empty layout-name.
+Bill Wilson    billw@wt.net
+</code>

gEDA Project Wiki

User Tools

Site Tools

Differences

Page Tools