Re: gEDA-user: Hi.... first post

[Stuart Brorson <sdb@xxxxxxxxxx>]

> Change the pin names to numbers in the schematic symbol files. Then
> the footprint pin numbers will map to schematic symbol pin numbers.

Yeah, like John pointed out this is a problem with the symbol 
${geda install dir}/share/gEDA/sym/analog/npn-2.sym.  It uses B, C,
and E as the pin numbers.  The pinnumber needs to be a number, and
the numbers should correspond to the numbers on the footprint you want
to use.

Do this:

1.  Figure out how your preferred footprint is numbered.

2.  Copy npn-2.sym into a local symbol directory under your project
directory.  Call it symbols/

3.  Edit your local gafrc file to include the line

(component-library "./symbols")

4.  Edit the copy of npn-2.sym in ./symbols.  Number each pin to
correspond to your footprint's numbering scheme.

5.  Nuke your old netlist.

6.  Re-run gsch2pcb, and then re-read teh netlist into PCB.

7.  Please file a bug report at the gEDA Bugzilla site about this
symbol.

FWIW, I did a shortened version of the above, and was able to get rats
attached to the TO-92s after I changed the transistor's pinnumber
attributes to numbers.

You can read more about handling local gafrc configuration here:

http://www.geda.seul.org/wiki/geda:faq-gschem#how_do_i_configure_my_local_gafrc_to_find_my_local_symbol_directory

Stuart


_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user