ICEpower amps

Spice is only as good as your models... At least that's what nearly 30 years of using it has taught me.

Capacitors, could be another techie article...

DonH50 said:

Spice is only as good as your models... At least that's what nearly 30 years of using it has taught me

Click to expand...

Exactly. I get the impression this is where a lot of people go astray, sticking "perfect" components everywhere. The best one, of course, is that just about every circuit is run off "perfect" power supplies, zero impedance at all frequencies ...

Frank

You'd love my power supply models, though they have given students (and some working engineers) fits over the years when they discover their circuits don't behave at all like they thought when they had ideal voltage sources on the rails. Mine are real-world, though. Most power supplies (sans caps) are an open over anywhere from a few tens to a thousand or so Hz.

Hello everybody,

thanks again for all your input concerning power supplies, I must admit that until know I only used PSUD2 from the Duncan Tools site, and even that one only superficially.

I might be wrong on this one but it seemed to me that having a constant current draw (class A) in my previous amps, made them far less demanding as far as PSU design was concerned.


I just downloaded LTSpice and will dig into it later today.

As far as the caps are concerned, I will try to modell a PSU that seems "suitable" to me and post it here.

Gentleman, thanks again, I think this is gonna be quite educational... well at least for me.

Cheers,

Max

All I can say is, "Yeah, what he said."

Class A means all the current, all the time, so "less demanding" is a matter of definition. What is different about Class D is the amount of HF energy they require, all the time, and the fact that the power supply rails can directly modulate the output signal, something not true in Class A or AB amps (within reason, the reason being the PSRR of the amp).

For cap models, most manufacturers provide static ESR and self-resonance; some provide shunt conductance as well. You can use those to derive a simple RLC(G) model of the caps:

Series R = ESR
Shunt R = 1/G
C = nominal C value
L = series L to create the self-resonance point for the series LC

HTH - Don

DonH50 said:

Class A means all the current, all the time, so "less demanding" is a matter of definition. What is different about Class D is the amount of HF energy they require, all the time, and the fact that the power supply rails can directly modulate the output signal, something not true in Class A or AB amps (within reason, the reason being the PSRR of the amp).

For cap models, most manufacturers provide static ESR and self-resonance; some provide shunt conductance as well. You can use those to derive a simple RLC(G) model of the caps:

Series R = ESR
Shunt R = 1/G
C = nominal C value
L = series L to create the self-resonance point for the series LC

HTH - Don

Click to expand...

OK,

I'll give this a try although I feel really lost trying to use LTSpice for the moment.

Please bear with me, as I am almost feeling like doing painting by numbers...

The datasheet does not provide any "direct" information concerning self-resonance as far as I can tell.

After reading up a little I found the following formula for calculating the self-resonance of a capacitor:

1/(2*pi*sqrt(L*C))

ESR as per datasheet: 0,016 Ohm
ESL as per datasheet: typically 16nH
Capacitance @ 100hz: 15000µF

giving me: 1/(2*pi*sqrt(0,000000016 H * 0,015 F)) = 16137,4306091976 Hz

If I get it right my capacitor is capacitive up to roughly 16 kHz, resistive at the calculated frequency and inductive from there on..

Should I just model a capacitor using the ESR for R, the ESL for L and the capacitance @100 Hz for C ?

I actually found a capacitor model for Spice, the above is for my better understanding only.. or non-understanding.

Max

Good choice, coolnose, going with LTspice. An excellent program, very much worth persisting with. I am pretty familiar with it, I know amir uses it, so don't hesistate to ask! There is an excellent forum on yahoo, with plenty of people there who know the ins and outs of the program intimately. A very good start is to play with the many examples that come with the package, plus if you're more comfortable with pdf's the help is available as such from Linear.

LTspice makes all of the capacitor stuff very easy; all you need to know is the ESR and ESL, which you already have. If the datasheet doesn't tell you there are various ways of making pretty accurate guesses for these, close enough to do the job properly. Critical to remember with ESL is that this comes into play because the capacitor looks like a piece of wire of a certain length at high frequencies, therefore any length of lead connecting the capacitor to the guts of the next component also comes into play. To give you an idea of how important, one rule of thumb is 7nH per cm -- see, a total length of an inch of connecting lead gives you as much inductance as in the cap itself! That's why how you actually precisely hook everything together can make a huge difference!!

So, to add the values into LTspice, just right click the cap. in a schematic, and type in Equiv. Series R and L. The program itself worries about all the resonance issues ...

Frank

@coolnose: Yes.

Smaller capacitors typically have higher self-resonant frequencies so provide wider bandwidth decoupling. But, of course, they are smaller so it takes more of them.

Hi Folks,

I am (more or less steck with simulating my transformer in LTspice.. although I read up quite a bit about is it, it seems to be a recurrent problem.

Should I bother trying to sim it or rather take a voltage source a some suggest ?

Any hints appreciated.

Best regards,

Max

coolnose said:

Hi Folks,

I am (more or less steck with simulating my transformer in LTspice.. although I read up quite a bit about is it, it seems to be a recurrent problem.

Should I bother trying to sim it or rather take a voltage source a some suggest ?

Any hints appreciated.

Best regards,

Max

Click to expand...

Sorry, Max, I don't quite follow you here. I have used LTspice to simulate a realistic transformer, this has helped me a great deal in truly understanding what's going on in power supplies. Using a voltage source will give you straightforward results, but it won't tell you what's really going on under the hood.

So if you want real accuracy, yes, sim. You might need to tell us a bit more where your problems are ...

Frank

Are you asking about the power transformer? If so, you can use a transformer model, assuming you can get some non-ideal parameters in there. Otherwise, the ideal inductance provides infinite Q (or as close as SPICE can get) and that can cause all sorts of problems (at best, huge voltage spikes that aren't real, often extends sim time greatly, and at worst non-convergence).

FWIWFM, I use an ideal voltage source with a large series inductor (fcL ~ 250 - 1000 Hz) plus series resistor roughly equal to the wire resistance as a starting point. That is easier to simulate and converges better than using a transformer. I only use a transformer when I have a good model of it, either from the manufacturer or via my own measurements.

HTH - Don