Comments related to calculating SNR from SPICE output or measurement results when using MATLAB

Ø Not specifying a maximum step size in a transient simulation will likely give varying results (up to 6 dB in SNR). For example using .tran 0 3.2u 200n doesn’t produce results as good as using .tran 10p 3.2u 200n 10p In the later statement the step size is limited to 10 ps. The variation in time step size inherent in SPICE leads to effects like clock jitter, see Secs. 5.2.1 and 5.2.2, and thus amplitude modulation (see Fig. 5.22) in the converter’s output. The cost of limiting the step size is increased simulation time, which can be significant.

Ø The ratio of the simulation time, T_stop , to the period of the input sinewave should be a whole number. For example, if f_in is 3 MHz (T_in = 333.33 ns) then a simulation time of 3 us (see .tran above where the first 200 ns of data isn’t saved to avoid start-up transients) results in a whole number of input sinewave cycles fitting in the simulation time (here T_stop/T_in = 3/0.3333 = 9). When we take the FFT of the data converter’s output the input sinewave fits perfectly into one bin (or 5 bins if a Hann window is used and the power spectral density of the signal and quantization noise is plotted, see Appendix A of [1] for additional discussions), that is, it doesn’t leak into adjacent bins.

Ø The length of the simulation (the length saved) sets the bin width of the FFT. For a 3 us simulation time the bin width is 333 kHz. This means that the FFT is calculated at f = 0, 333k, 666k, 1MEG, 1.33MEG, etc. The number of signal bins should be 20% of the number of noise bins (or smaller) in the bandwidth of interest when calculating the SNR. Using a short simulation time may result in the FFT only containing the desired tone (little to no noise) in the bandwidth of interest and thus artificially inflate the SNR.

Ø Selecting the input sinewave period and thus the simulation time based on the sampling frequency (period, T_s, again the ratios, T_stop/T_in and T_in/T_s, should be whole numbers) can, but not necessarily (e.g. a second-order noise-shaping modulator) result in coherent sampling (the quantization noise added to the signal isn’t white, page 175). Drastic changes in the SNR may be observed using this technique.

Example, if the sampling frequency is 176 MHz we might set the input frequency to 2.93333 MHz and the simulation stop time as 3.068 us, or .tran 10p 3.268u 200n 10p UIC and Vin Vin 0 DC 0 SIN 2.5 2 2.933333MEG.

Ø The concepts for selecting measurement time, sampling frequency, and input frequency should follow these comments too, where possible, when testing the data converter. This may be challenging requiring the oscillator generating the sampling clock be phase-locked to the oscillator generating the input to the data converter.

Having done all of these the SPICE-simulated SNR is still generally limited to < 50 dB (< 8-bits), not because of SPICE accuracy, but rather to keep the simulation time reasonable. To improve the SPICE-simulated SNR the tolerances, reltol and vntol, need to be reduced (say by a factor of 10). SPICE simulation is still useful to check connectivity, integrator output swing, and other basic behavior; however, the silicon will generally perform better, more in line with theory, than a SPICE simulation will indicate.

Additional Reading

[1] Saxena, V., "K-Delta-1-Sigma Modulators for Wideband Analog-to-Digital Conversion.pdf", Doctoral Dissertation, Boise State University, April 2010.

Return