Re: gEDA-user: netname attrib on input symbols

[John Doty <jpd@xxxxxxxxx>]

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/
jpd@xxxxxxxxx




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