On Fri, 2007-07-20 at 10:45 -0400, devrin talen wrote: > Thanks for the reply. I'm a bit confused, however: > > > Check your netlist to see if the power pins are connected. If you are using > > the > > 74126 symbol that comes with gschem the power net is probably called Vcc. > > I only see three pins on the 74126 symbol that I'm using from gschem > (A, EN, and Y). I have two separate instances of this symbol, and I've > edited the attributes to make them part of the same package. Is there > a different way I should be going about this? Or is there something > else I need to do in addition to see the power net?
My recollection is that gsch2pcb doesn't understand slotted parts very well, and that unless you name them the same "U1" for example, you will get two separate packages spat onto your PCB. (I usually come unstuck naming things U1a and U1b, and have to hand-edit the netlist to merge them back by removing the 'a' or 'b' suffix.) So you've got two instances of the 74126 symbol, and have given one the "slot=1" attribute and the other "slot=2". The part has 4 slots, so you may want to instantiate the other two as well and tie the inputs to logic 0 / 1 to avoid them floating. The symbol has a built in "net=GND:7" and "net=Vcc:14" which should connect pin 7 to the net named "GND" and pin 14 to the net named "Vcc". If you don't have multiple supply voltage requirements, it should be possible to drop the "vcc" symbol onto the page (which has a "net=Vcc:1" attribute), and the "gnd" symbol (which has a "net=GND:1" attribute). Presumably your power comes in via a connector. Just wire up the connector with the "vcc" and "gnd" symbols, and you should see the output netlist will include the socket, and the power pins on the IC. Hope this helps Regards, -- Peter Clifton Electrical Engineering Division, Engineering Department, University of Cambridge, 9, JJ Thomson Avenue, Cambridge CB3 0FA Tel: +44 (0)7729 980173 - (No signal in the lab!) _______________________________________________ geda-user mailing list geda-user@moria.seul.org http://www.seul.org/cgi-bin/mailman/listinfo/geda-user