Re: gEDA-user: Multivibrator Simulation

[Andy Fierman <andyfierman@xxxxxxxxxxxxxxx>]

Hi Michael,

Another way to do this is to use the "OFF" option in the bipolar
transistor model to force one of the transistors into a known initial
state.

I'm not sure how you introduce this parameter into you particular
simulation schematic, you may have to just hand edit the device model
in your spice netlist.

Here's an example of the model options similar to what you'll find in
most generic Spice device documentation.

-------------------------
Qxxxx collector base emitter [substrate] modelname [area] [OFF]
      [IC=vbe,vce] [TEMP=local_temp] [M=mult] [DTEMP=dtemp]

collector           Collector node name

base                Base node name

emitter             Emitter node name

substrate           Substrate node name

modelname           Name of model. Must begin with a letter but can contain any
                    character except whitespace and ' . ' .

area                Area multiplying factor. Area scales up the
device. E.g. an area
                    of 3 would make the device behave like 3
transistors in parallel.
                    Default is 1.

OFF             Instructs the simulator to calculate operating point
analysis with
                    the device initially off. This is used in latching
circuits such as
                    thyristors and bistables to induce a particular state.
-------------------------

Notes about ‘OFF’ Parameters:

Some semiconductor devices such as diodes, bipolar and MOSFET
transistors feature
the device parameter OFF. If there are devices in the circuit which
specify this parameter,
the bias point solution is found in two stages.

In the first stage, the devices with OFF specified are treated as if
their output terminals
are open circuit and the operating point algorithm completes to
convergence. In the
second stage, the OFF state is then released and the solution
restarted but initialised
with the results of the first stage.

The result of this procedure is that OFF devices that are part of
latching circuits are
induced to be in the OFF state. Note that the OFF parameter only
affects circuits that
have more than one possible DC solution such as bistables. Specifying the OFF
parameter in a non-latching circuit such as an amplifier which will
generally have a
unique solution, will work OK but may slow down arrival at the correct
final state.
the same. It will just take a little longer to arrive at it.

Other ways already mentioned in this thread that will usually start up
circuits in unstable equilibrium are to introduce a ramp or small step
in the power supply voltage .

Cheers,

         Andy.

http://signality.co.uk



2009/6/23 John Doty <jpd@xxxxxxxxx>:
>
> On Jun 23, 2009, at 9:45 AM, Michael B Allen wrote:
>
>> I'm trying to run a simple multivibrator simulation but both SPICE and
>> GNU-Cap do not yield anything that even oscillates. Here is the
>> circuit:
>>
>>   http://207.192.69.113/~miallen/mv_1.pdf
>>
>> Is there anything wrong with this? Is there any trick to getting
>> something like this to work?
>
> You've created a simulation of a pencil perfectly balanced on its
> point. Break the symmetry somehow. Lots of ways to do it:
>
> Change one of your resistor values a skosh. They won't be perfectly
> equal in reality anyway.
>
> Or use different transistor models.
>
> Or force one of the node voltages away from equilibrium with a .IC
> command and specify UIC in your .TRAN command.
>
> Or force the charge on your capacitors away from equilibrium with
> IC=, and UIC as above.
>
> 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
>


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