Article pointer: SPICE lying to ya?

[mlloyd1]

For all you SPICE heads, you may enjoy this article:

"My SPICE lied to me!

mlloyd1

[andy_c]

Yes, the vendor-supplied SPICE models can be quite bad. For instance, the MJL3281a model from On Semiconductor has a simulated ft at a DC current of 100 mA that's more than a factor of 6 low from the data sheet curves of ft vs Ic. For more info on this, see this thread: Evaluation results: MJL3281A/MJL1302A SPICE Models

The article you reference refers to one of the known problems with the Boyle op-amp macro model, namely that the simulated power supply current doesn't change as the load current varies. That's just ridiculous, and makes simulating some op-amp-based power amp topologies literally impossible. The Analog Devices op-amp models don't have this problem. See http://www.analog.com/UploadedFiles/...01016AN138.pdf for more details. If you're using LTSpice, all of the supplied op-amp models have this problem, so you'll need to import some Analog Devices or TI models in order to get accurate supply current simulation data.

Another gotcha - the SPICE level 1, level 2 and level 3 MOSFET models show a constant gate-drain capacitance as the gate-drain voltage varies. This makes them useless for predicting distortion due to gate-drain capacitance variation of vertical power MOSFETs such as the IRFP240 and IRFP9240. LTSpice has the VDMOS model which has a non-constant gate-drain capacitance, but you'll need to learn how to fit the parameters to data sheet values. This requires some nonlinear equation solving software such as MathCad.

There's a lot of misinformation and false assumptions about SPICE that can be found, which not surprisingly often originates from non-users. There are companies out there working on extending SPICE into the millimeter wave region. What changes to the simulator are required? Almost none, with the exception of some quirky numerical precision issues that happen with time steps on the order of picoseconds. The vast majority of the work is in the models.

Also, there are some highly experienced and respected audio designers here who are essentially SPICE naysayers, which might lead one to extrapolate that all highly experienced audio designers hold this view. Turns out that there are some very experienced audio designers who are in effect SPICE cheerleaders as well. See http://www.ampzilla2000.com/thequest1.html. As usual, the truth is likely to be somewhere in between the extreme views.

[janneman]

Andy,

Very interesting articles (and observation).
It reminds me of a problem I had with simulating a circuit with a floating opamp (bootstrapped supplies). It acted very strange, and I had to give it up. Now I know that the opamp model had internal nodes that were hard referenced to ground....

Jan Didden

[SY]

It's interesting how this author analogizes the SPICE software as a high tech razor, especially after Pease's examples of some really flaky convergence problems. You guys can console yourselves with one thing- the tube models are even worse.

[destroyer X]

We have to assemble and hear... and in a controled way....not an easy way, have to control many things, and listen with many people... short time (adaptation) and with different musics...because taste influenced results.

Blameless was the best simulation i already have made... and the worst sound i heard all life.

Carlos

[janneman]

Originally posted by SY
It's interesting how this author analogizes the SPICE software as a high tech razor, especially after Pease's examples of some really flaky convergence problems. You guys can console yourselves with one thing- the tube models are even worse.

Stuart,

Are you or anybody following Graham Maynards series on "Class A imagineering" in EW? He is strong on "first cycle distortion" in amplifiers and there is some criticism that this actually is a Spice artifact.

Jan Didden

[SY]

Haven't seen this, though I remember the discussion here where the only thing I learned is how difficult Fourier analysis is for most people. Do the articles relate the computer predictions to experiment?

[janneman]

SY,

Well, the series runs for 6 articles (!), no. 4 just came out. I don't wish to bash Graham, it's interesting reading, but very long winded and not easy to pick out the significant content. It takes real discipline to read it through.

Anyway, the core of it (if I correctly summarise it) is that he feels one important characteristic of amps is how they treat the initial cycle of a signal, he calls it "first cycle distortion". Depending on the amp characteristics and the (speaker) load characteristics, this initial cycle is distorted in a way that is not detected if you run a sim over many cycles in a kind of steady state situation.

For example, the combination of output inductor and speaker reactance would, according to his simulations, cause this type of distortion.

Now, there are some questions here. The start of a signal is abrubt: now there is 0V DC, and the next instant there is a rising waveform. This is a discontinuity and there are at least two aspects that make me critical.

Firstly, how does Spice handle this? It is known that Spice needs some time to converge to a steady state, but I don't have enough expertise to judge the significance here. So the "first cycle distortion" may be a Spice artifact;

Secondly, is this discontinuity at the start of the Spice input signal realistic at all? Audio input signals are band-limited anyway, and will not show the sharp start as in Spice. So, the "first cycle distortion" may also be a non-realistic test signal artifact.

To be honest, Graham puts his money where his mouth is and presents some amp designs (the first one published is an adaption of the famous JLH design) to minimise "first cycle distortion".

I'm not sure (yet) what to make of it. Maybe someone else on this forum has a clear and reasoned opinion?

Jan Didden

[SY]

Well, I'll try to slog through the articles, but a few questions immediately come to mind:

First, what happens in these models if you just bandwidth limit the input signal with a single pole filter at some really high frequency (say, 100-200 kHz)?

Second, in real amps fed real impulse or tone burst signals, do the predicted artifacts appear?

Third, how does the "distortion" compare to what Fourier theory and a "perfect" amp would be predicted to produce?

Fourth, what experimental evidence is used to validate these amp designs?

Fifth, why don't editors do their job?

[janneman]

SY,

I don't have the articles here, and I don't have them fully digested either. I do remember the point being made that he didn't want to bandlimit the input signal for some reason, although that would immediately lend credibility (or not depending on the result) to his arguments. I'll look it up tonight.

As for editors doing there work, EW has a new editor and the journal appears to me a bit direction-less, as if he is trying out by trial and error what the direction/content is that attracts the highest number of readers.
Maybe I should submit a reader letter...

Jan Didden