Re: gEDA-user: Generating PCB output

[Ales Hvezda <ahvezda@seul.org>]

[snip]
>No, I'm not using uref= in my schematics. The versions used so far have
>been 20021103 and 20030223, so there should be no uref anywhere.
>
>I've attached the error output, and the schematic. All symbols are from
>the standard libraries. The output was created with gschem2pcb.
>

	Ah yes, the schematics/error message cleared everything up.  The
input-1.sym is not netlistable in its current state the way you
are using it.  The netname= attribute was really only meant for net
segments, not components.  However, you have several choices here to
get a netlistable schematic:


1) Remove the input-1.sym's and place the netname= attribute directly
   on net itself and remove the input-1.sym symbols.  This is the "normal"
   way gschem/gnetlist likes to label nets.

-Or-

2) Modify (by creating a local copy) input-1.sym adding the following:

T 250 50 5 4 1 1 0 3
net=Unspecified:1

   And then when you place an input-1.sym in the schematic, edit the
Unspecified:1 to be netname:1  (The :1 is important).

-Or-

3) Just change all the netname= attributes on the input-1.sym to be
   net=signalname:1

-Or-

4) Modify (by creating a local copy) input-1.sym adding the following:

T 100 400 8 10 0 0 0 0
graphical=1

   And then just attach the netname= attribute to the net itself.  This
   seems to work for me, but I am not sure it will work in all cases, as
   the graphical=1 attribute is generally not used on connected comopnents.

Either way, the warning:
"Could not find uref on component and could not find any special attributes!"
needs to be updated to use "refdes".  I will fix this.  Thanks.

									-Ales