User Tools

Site Tools



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

Link to this comparison view

geda:gsch2pcb_readme [2012/02/20 15:14] (current)
Line 1: Line 1:
 +====== gsch2pcb (gschem to PCB) README ======
 +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
 +1) 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.
 +2) 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.
 +3) 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 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
 +   ​ and you can proceed using PCB on foo.pcb if you wish to
 +   fix the errors from inside of PCB.
 +4) 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 and
 +   ​proceed with using PCB.  ​
 +5) Modify foo.sch and again run "​gsch2pcb foo.sch"​.
 +   * If components were added, PCB elements for them will be placed in the
 +     file ​ 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
 +     ​unless you run "​gsch2pcb --remove-unfound foo.sch"​ which will omit
 +     the PKG_ lines so you can go ahead and load 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.
 +6) Run "pcb foo.pcb"​ and clean up any dangling traces left over from removed
 +   ​elements. ​ Load any new elements in with the "Load layout
 +   data to paste-buffer"​ function. ​ Load the new netlist
 +* 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 ​
geda/gsch2pcb_readme.txt ยท Last modified: 2012/02/20 15:14 (external edit)