Re: [LTSPICE] Too many Teravolts!

----- Original Message -----
From: "Chris Carlen" <crcarleRemoveThis@xxxxxxxxxxxxxxx>
Newsgroups: sci.electronics.cad
Sent: Tuesday, April 19, 2005 11:14 PM
Subject: [LTSPICE] Too many Teravolts!


> Greetings:
> Notice how this circuit causes some major voltage spikes to gazillions of
> TV. When the alternate solver is used, no problem.
>
> Also notice that if the entire right half of the circuit containing all
> the op-amps is deleted (it is presently not doing anything useful, so may
> be deleted) and solved with the default SPICE options, then the TV spikes
> don't occur.
>
> Any explanations? Some sort of math routine glitch?
> Thanks.
> Good day!

Hello Chris,
I had a hard time with your circuit. I first tried with the
usual SPICE parameters, but this hasn't really helped.

After that I looked to your component values.

Lfilta: 25 Henry
Lfiltb: 25 Henry
L1: 250 Henry
C5: 4 Farad

What real word circuit contains an ideal 250H coil or
an ideal capacitor with 4 Farad?

Please add the following parasitics by clicking the right
mouse button over the appopriate component. A dialog will pop up.

Lfilta: Parallel Resistance: 1e7
Lfiltb: Parallel Resistance: 1e7
L1: Parallel Resistance: 1e7
C5: Serial Resistance: 0.01

The simulation will then run with the normal and the
Alternate solver. There are also no more "super spikes".

My learning from this:
Add a little bit loss to circuit elements if they
have such extreme values of ideal inductance and capacitance.
This helps to make it better solveable for any (LT-)SPICE engine.
Your real parts will have decades more loss than I
have added in your example.

Best regards,
Helmut


.