The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl Design >> Analog Design >> SNR in spectre wavescan calculator tool https://designers-guide.org/forum/YaBB.pl?num=1133959761 Message started by bunny on Dec 7th, 2005, 4:49am |
Title: SNR in spectre wavescan calculator tool Post by bunny on Dec 7th, 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 |
Title: Re: SNR in spectre wavescan calculator tool Post by sheldon on Dec 24th, 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 |
Title: Re: SNR in spectre wavescan calculator tool Post by bunny on Dec 25th, 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 |
Title: Re: SNR in spectre wavescan calculator tool Post by sheldon on Dec 25th, 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 |
Title: Re: SNR in spectre wavescan calculator tool Post by bunny on Jan 4th, 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 |
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |