On Nov 13, 2008, at 10:09 AM, Ethan Swint wrote: > Previously I've set the netname attribute on individual wires in > gschem, > but got annoyed at having to move the wire end and wire label > separately. I've tried the input symbols, input-1.sym, > input-2.sym, and > input-orcad-1.sym, but I haven't found a way to make the netname > attribute propagate through gnetlist -g pcb filename.sch, e.g. the net > attached to the input symbol and its other connections don't take > on the > netname attribute assigned to the input symbol. Do I have false > expectations as to the purpose or behavior of these symbols? >
Yes. And it's confusing. The netname= attribute is ignored when attached to a symbol. It's for net segments only. You want the net= attribute. So instead of attaching netname=foobar to the symbol, you should attach net=foobar:1 to force the net connected to pin 1 to have the name "foobar". This assumes that the symbol has a visible pin 1. The primary use of the "io" symbols is hierarchy, where the association is refdes= on the io symbol to pinlabel= on the pin of the symbol that represents the sub schematic. However, some of the io symbols also contain net= attributes: input-2.sym:net=INPUT:1 io-1.sym:net=IO:1 output-2.sym:net=OUTPUT:1 passive-1.sym:net=PASSIVE:1 This is dangerous, because unless you override these attributes, all of your "input-2" syms will wind up shorted to a net named "INPUT". SPICE netlisting is a whole different can of worms. John Doty Noqsi Aerospace, Ltd. http://www.noqsi.com/ [EMAIL PROTECTED] _______________________________________________ geda-user mailing list [email protected] http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
