Designer’s Guide Community

bunny

New Member

Offline

huh...analog
design..

Posts: 8

SNR in spectre wavescan calculator tool
Dec 07^th, 2005, 4:49am

Hello all,
I have a doubt in using the SNR function in the spectre wavescan calculator. I am trying to
find the SNR of a 10bit ADC. I interfaced it with an ideal 10bit DAC (spectreHDL model).
I performed the FFT of reconstructed signal(a sine wave) from ideal DAC output. I followed all the rules
of coherent sampling.
Now I used the SNR function and performed the following operation

snr(fft(V(vo),2.6u,259u,128),27.3k,249.6k,27.3k,249.6k)

where my input freq: 27.3K
Fs= 499.2K (Fs/2= 249.6k)
I am performing 128-point fft
i.e.,
signal_from:27.3K
signal_to: 249.6K (Fs/2)
Noise_from: 27.3K
Noise_to: 249.6K

but it resulted in InfinitydB

Now I reduced the signal_to range from 249.6K to 245K i.e.,

snr(fft(V(vo),2.6u,259u,128),27.3k,245k,27.3k,249.6k)

it results in SNR= 80.768dB (I am not sure of this value as I was expecting SNR around 60dB for 10-bit ADC)

can anybody explain me if I am doing it right. I am not sure abt the frequency ranges I am using for SNR.
Even a small change in the frequency range is affecting my SNR values as they are jumping wildly
from one value to another.

One more doubt...the magnitude of the fundamental(27.3K in my case) in the fft plot is exactly half of the
maximum value of the reconstructed sinewave. I was expecting it to be Vm/root(2)(rms value). Why is it showing Vm/2?

thanq

Back to top

IP Logged

sheldon

Community Fellow

Offline

Posts: 751

Re: SNR in spectre wavescan calculator tool
Reply #1 - Dec 24^th, 2005, 5:33am

Bunny,

The signal window should include the signal and
not the noise. The signal window should be the center
frequency +/- resolution bandwidth for the Rectangular
window. For other FFT windowing functions this
recommendation will change. In this case, 27343.75
+/- 3906.25 Hz --> 23437.5 Hz - 31250 Hz.

Next, it would be better to directly reconstruct the
analog signal in the calculator, fft( (1/Vfull_scale) *
V(msb)/2 + V(msb-1)/4 + V(msb-2)/8 + ..., from, to,
# points). Using a DAC can introduce new issues.
Performing the calculation once is some work.
However, you can save it as an output or as a
calculator memory and re-use it later.

Some other comments:

1) Using the snr function you are really calculating the
SINAD of the ADC. For non-sampled circuits, the
distortion is at integer multiples of the fundamental
frequency. Usually, the distortion is outside the
frequencies of interest. In this case, you are including
the noise and distortion in the frequency of interest.

2) The snr and thd functions are not intended for
sampled circuits. For normal circuits, the distortion
occurs at integer multiples of the fundamental
frequency. For sampled circuits, the distortion occurs
at the same frequencies, however, the sampling
process folds the distortion back into the baseband.

Best Regards,

Sheldon

Back to top

IP Logged

bunny

New Member

Offline

huh...analog
design..

Posts: 8

Re: SNR in spectre wavescan calculator tool
Reply #2 - Dec 25^th, 2005, 4:54am

sheldon,

Thanks for the reply. This is working perfectly. One more question. I have a Sigma delta modulator for which I need to measure the performance metrics. How do I measure the SNR and other parameters of a sigma delta modulator? Is there any way to reconstruct the modulated output signal with spectre wavescan calculator tool?

Thanq

Back to top

IP Logged

sheldon Community Fellow Offline Posts: 751	Re: SNR in spectre wavescan calculator tool Reply #3 - Dec 25^th, 2005, 6:18am Bunny, You shouldn't need to reconstruct the analog, just perform the FFT directly on the output pulse train. Best Regards, Sheldon
Back to top	IP Logged

bunny

New Member

Offline

huh...analog
design..

Posts: 8

Re: SNR in spectre wavescan calculator tool
Reply #4 - Jan 4^th, 2006, 2:49am

Sheldon,
I have tried to plot the fft of the output pulse train(+1 and -1) of a second order SDM. The input to my SDM is a sinewave with amplitude=1v and input frequency fin=5.1K. �In the FFT output, the amplitude of the fundamental spike (at fin=5.1K) is shown to be in microvolts (2.7uV). The clock frequency is (Fs=819.2K). I was expecting the amplitude of the fundamental spike to be around 1V. Can u tell me where I went wrong? I am attaching the FFT output for clarity.
Thanks
bunny

Back to top

fft.png

IP Logged