On Thu, 2010-03-04 at 07:31 +0900, John Doty wrote: > On Mar 4, 2010, at 6:19 AM, Peter Clifton wrote: > > > (:1 refers to the pin(number?) of a component which the named net > > connects to when using the net= attribute on a component). > > pinseq, not pinnumber. No, it IS _pinnumber_. pinseq is for slotting and spice ordering only. When wiring up a net to a pin (no attributes involved), it is ONLY ever "pinnumber" which makes it into the netlist. I've just tested with the "geda" backend to gnetlist with the attached test schematic. The connector has 3 pins.. their pinseq are 1, 2, 3, their pinnumbers are PN1, PN2, PN3, and for sake of disambiguation, their pinlabels are PL1, PL2, PL3. I've tested net= attributes with names matching a pinlabel, a pinnumber and a pinseq. gnetlist correctly treats the :? part of the net=<netname>:<pinnumber> as a pinnumber. net=TEST1:PL1 defines a new pin, pinnumber "PL1" net=TEST2:PN2 correctly connects to the existing pin numbered "PN2" net=TEST3:3 defines a new pin, pinnumber "3" The symbolic pins with name PN1 and PN3 are only connected to their respective unnamed nets. -- 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!)
Attachment:
output.net
Description: application/pcb-netlist
Attachment:
test.sch
Description: application/geda-schematic
_______________________________________________ geda-user mailing list geda-user@xxxxxxxxxxxxxx http://www.seul.org/cgi-bin/mailman/listinfo/geda-user