Re: gEDA-user: PC/104 footprint problems

[DJ Delorie <dj@xxxxxxxxxxx>]

Ok, based on the board you sent me, I have an idea.  The problem is
that the PC/104 footprint you have is an old style footprint (before
the hi-res patch) and specifies pin *names* but not pin *numbers*.
The netlist is based on pin numbers, so it doesn't match.

What you want to do is save your layout, and edit it in a text editor.
You'll now see new-style pins:

Element["" "pc104" "J1" "unknown" 145000 81000 20000 0 3 100 ""]
(
        Pin[40000 25000 6000 3000 6600 3000 "A1" "1" "square,edge2"]
        Pin[40000 35000 6000 3000 6600 3000 "A2" "2" "edge2"]
        Pin[40000 45000 6000 3000 6600 3000 "A3" "3" "edge2"]
        Pin[40000 55000 6000 3000 6600 3000 "A4" "4" "edge2"]
        Pin[40000 65000 6000 3000 6600 3000 "A5" "5" "edge2"]
        Pin[40000 75000 6000 3000 6600 3000 "A6" "6" "edge2"]

Change all the numbers to match the names.  Load the board in PCB
again, disperse elements, and "o" and they'll connect.

Note: if you then run the script gsch2pcb gives you, it changes the
pin *names* to match the labels in the schematics, like DRQ3 or SA8.


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