The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design >> Analog Design >> SNR ,THD simulation
https://designers-guide.org/forum/YaBB.pl?num=1111052911

Message started by neurocat on Mar 17^th, 2005, 1:48am

Title: SNR ,THD simulation
Post by neurocat on Mar 17^th, 2005, 1:48am

:) :)

hi
how to simulate the SNR and THD of a class AB Power amplifier. would u please give me some advices.
thanks a lot

Title: Re: SNR ,THD simulation
Post by benis on Mar 24^th, 2005, 2:20pm

to have an estimatin of your THD make a dft of your output to see how high are your armonic frequencies.

Title: Re: SNR ,THD simulation
Post by James on Mar 24^th, 2005, 5:33pm

Then how to see the SNR result?

Title: Re: SNR ,THD simulation
Post by analogic on Mar 25^th, 2005, 11:58am

what i did is use the "prints" in Cadence calculator to export the spectrum points, then use Matlab to calculate SNR

Title: Re: SNR ,THD simulation
Post by gsuarez on Mar 26^th, 2005, 7:08am

Hi,

Check this site and this pdf. Remeber if using Matlab that log base 10 is log10. I don't know much about amplifier characterization but in ADCs you need to have a coherent signal at the input with respect to the number of samples you measure at the output. If the coherent sampling condition is no met, you will have spectral leakage.

http://moon.pr.erau.edu/~lyallj/ee412/sinad_exp.html

http://www.strategic-test.com/support/download/uf_an-02_measuring%20dynamic%20specifications.pdf

If you need more about coherent sampling then go to http://www.maxim-ic.com and check for their application notes, they are really good.

George

Title: Re: SNR ,THD simulation
Post by sheldon on Mar 26^th, 2005, 6:13pm

Neurocat,

If the input is a sine wave, one alternative would
be to use the Spectre fourier component to calculate
the THD. In general the fourier component is very
accuracte and simplifies the THD measurement. The
only limitations are that it doesn't work for sampled
data applications, that is, for ADCs. In addition, you
need to be careful about calculating SNR from a dft.
The issue is that normally transient analysis does not
include device noise unless you specifically add[using behavioral models] so the noise floor of the spectrum
is set by the numerical noise in the simulation.

If you do want to calculate SNR from the large signal
performance, a reasonable goal since this circuit is a
class-AB amplifier, try transient noise analysis. Don't
forgot to subtract the numerical noise floor from the
original spectrum(by RSS).

BTW, as a thought experiment if you are using
Spectre, run your transient simulation using different
relref options: sigglobal, alllocal, pointlocal. You should
see that the amplitude of the fundamental and the
harmonics are constant, however, the amplitude of
the "noise" falls of significantly as the accuracy of the
simulation increases.

Best Regards,

Sheldon

Title: Re: SNR ,THD simulation
Post by Andrew Beckett on Mar 29^th, 2005, 8:33pm

Some other pointers on this topic:

a) use the strobeperiod option to transient, to ask spectre to solve at the points you're going to sample at in the fft - this removes the interpolation error you'd get when sampling. If you're using fft that is...

b) There's a THD function in the ADE calculator's special functions. This does an fft and then calculates the ratio of the first harmonic (I think this is controllable) to the other harmonics.

c) spectre now has a transient noise analysis, BTW, from MMSIM60 onwards. As with all transient noise analyses you have to be careful to average the noise over a long enough period of time (you do have control over the maximum noise bandwidth, which in turn sets the maximum timestep within the transient). It's another way to look at noise in non-periodic systems if the RF analyses aren't appropriate, and also to look at circuits with a nonlinear response to the noise.

Regards,

Andrew.