Re: gEDA-user: Multivibrator Simulation

[al davis <ad252@xxxxxxxxxxxxxxxx>]

On Tuesday 23 June 2009, 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

It would help if you include a netlist, so I can try it.

> Is there anything wrong with this? Is there any trick to
> getting something like this to work?

Without trying it, my first guess is that it is stuck in a meta-
stable state.  This is a common "problem" with circuits of this 
type.  I put "problem" in quotes because it seems to be only a 
problem in simulation, where balance is perfect and there is no 
noise.  It's like trying to balance a pen on its point.

One way you can spot a situation like this is to do a DC (op) 
analysis.  It will show the circuit to be in perfect balance.  A 
real circuit would go one way or the other.

Since a DC analysis is equivalent to omitting the capacitors, it 
should show both transistors turned on.  When you run a 
transient analysis, it will stay that way.

Transient analysis starts with a DC analysis, so you are 
guaranteed to have this problem.

One trick is to unbalance the circuit slightly.  Maybe change 
one of the 1k resistors to 1.001k.  This may or may not be 
enough to make it start oscillating.  Probably not.

You need to explicitly start the oscillator.

In the real world, this happens when you turn on the power, so 
you must model turning on the power.

You need to ramp up the power supply.  Start it at zero, and 
increase it to the final voltage, just like what happens when 
you turn on the power to a real circuit.  If the circuit is in 
perfect balance, this may or may not be enough make it start 
oscillating.

To guarantee that it will oscillate, do both.  Unbalance the 
circuit a little, and ramp up the power supply.

> Note that I'm not an EE and I'm using gspiceui. I'm just
> trying to validate the theory before I start messing around
> with wires and such.

I don't use gspiceui.  It is too restrictive.  If you learn to 
use a simulator interactively it is amazing how much you can do.

To see an example of ramping up the power supply to properly 
start an oscillator, look at this example:
http://wiki.gnucap.org/dokuwiki/doku.php?id=gnucap:manual:examples:phase_shift_oscillator

This example does much more than you want, but the first part 
applies here.  The example measures distortion of a (supposedly) 
sine wave oscillator.


al.



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