gEDA-dev: Diode symbols in GSchem and PCB

[Stuart Brorson]

The rough idea is this:

Here's a typical component instantiated in a .sch file:

C 69700 50400 1 0 0 resistor-1.sym
{
T 69950 50700 5 10 1 1 0 0 1
refdes=R102
T 70000 50200 5 10 1 1 0 0 1
value=100
}

Now here's a typical pin instantiated in a .sym file:

P 3300 1600 3600 1600 1 0 1
{
T 3400 1650 5 8 1 1 0 0 1
pinnumber=13
T 2700 1600 9 10 1 1 0 0 1
pinlabel=C
}


In the proposed scheme, one could overwrite the .sym pin by having the
following component in the .sch file:

C 69700 50400 1 0 0 resistor-1.sym
{
T 69950 50700 5 10 1 1 0 0 1
refdes=R102
T 70000 50200 5 10 1 1 0 0 1
value=100
P 3300 1600 3600 1600 1 0 1
{
T 3400 1650 5 8 1 1 0 0 1
pinnumber=15
}
}

This would overwrite the attribs of the pin located at 3300 1600 3600
1600.  In particular, it would overwrite pin 13, making it pin 15 in
the schematic.

To effect this, gnetlist would just need to recognize that the pin at
location 3300 1600 3600 1600 is being overridden by the attribs
between the {}, and then build the correct netlist accordingly.
Gschem would need to display the correct pinnumber also, meaning that
the internal datastructure must support this overwriting.


Or do we need to do something more involved?


>> Having had a not-so-brief inspection of the .sch file specification,
>> this would most certainly require a non-backwards-compatible and
>> major change to the file format.

Old gschem versions don't need to read new .sch file formats.
However, new gschem versions must read old file formats.  I think that
is possible using this scheme, or am I confused?

Stuart