Re: gEDA-user: symbol creation / spice netlisting

[sdb@xxxxxxxxxx (Stuart Brorson)]

> 
> Hello,
> 
> I tried to create a gschem-symbol for an operational amplifier (MAX427).
> I wanted to follow the guidelines given in the "symbol creation guide"
> so in stead of providing power pins I added the appropriate
> net-attributes. The device has two pins used for balancing the offset.
> 
> I experienced two problems while using the symbol:
> 
> 1. The spice-netlister "gnetlist -g spice-sdb" does not list the
> power-pins which are essential for the .SUBCKT-file to work. I
> downloaded it from the Maxim-Homepage.
> 
> 2. The spice-netlister lists the offset-balancing pins that are not
> supported by the model-file that I downloaded.
> 
> I see several possibilities to fix the two problems like:
> 
> -providing power pins
> -deleting the offset pins (that I don't use anyway)
> -fixing the spice-netlist by hand
> 
> But none of the solutions really satisfies me. What is the "official"
> solution to the two problems? How can I get one(!) gschem-symbol for the
> device that works with the spice-netlister as well as with the pcb-tool
> (eventually using the offset-pins)?

There is no "official" way to do anything with gEDA.  You do what
works best for you. 

My recommendations for you: 

1.  Create a symbol with explicit power pins.  It is usually a bad
idea to use implicit power pins, particularly in analog designs.  At
one time, when all logic was +5V, implicit pins were OK, but nowadays
logic voltages can be +5, +3.3, +2.5, +1.8, and +1.5V.  Hiding the
power connection in an implicit pin is a way to have  a disaster.
Therefore, always use explicit power pins.

2.  If your model doesn't have the offset null pins, then get a model
that does.  This is a functional part of the circuit, so you should
want to simulate it.

If you can't find a model with offset null connections, then you can
try omitting the pinseq attribute from teh offset pins.  I don't
recall if spice-sdb will not emit nodes when it doesn't find the
pinseq, but it should.  Note that "pinnumber" controlls the order in
whcih pins are emitted for layout, but "pinseq" controlls the order of
emission for spice-sdb.  Note, too, that the order is usually
different -- check your SPICE model to see what order you want to emit
your nodes to be compatible with the model.

3.  Don't get too involved with creating a schematic (or symbol) which
works with both SPICE and layout.  Although simulating your layout
schematic may sound like a good idea at first, experience will show
that your SPICE schematic will differ significantly from your layout
schematic.  For example, your SPICE schematic will have ideal voltage
sources (for power) and SPICE directives, while your layout schematic
will have all kinds of testpoints, connectors, and even non-SPICEable
components such as regulators, logic, etc. 

Therefore, it's better to have two schematics: one for layout and one
for simulation.

HTH,

Stuart