The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl Design >> Mixed-Signal Design >> How to simulate the harmanic distortion of S/H? https://designers-guide.org/forum/YaBB.pl?num=1146818154 Message started by tuza2000 on May 5th, 2006, 1:35am |
Title: How to simulate the harmanic distortion of S/H? Post by tuza2000 on May 5th, 2006, 1:35am i want to simulate the harmanic distortion of the sampling&holding circuit of a pipeline ADC ,but i dont know how to do ? can anybody help me? thanks!!! |
Title: Re: How to simulate the harmanic distortion of S/H Post by ywguo on May 5th, 2006, 3:17am tuza2000, Here is an example. .tran 1ns 12.8us .fft v(op,on) from=1ns to=12.8us NP=512 window=Kaiser-Bessel where the sampling rate is 40MS/s, the period is 25ns. At least I figure out which harmonic is larger using that method. Best regards, Yawei |
Title: Re: How to simulate the harmanic distortion of S/H Post by Ken Kundert on May 5th, 2006, 7:30am If you are using Spectre you should add a 25ns strobe interval to the transient analysis statement to eliminate any errors from interpolation. -Ken |
Title: Re: How to simulate the harmanic distortion of S/H Post by sheldon on May 6th, 2006, 2:13am Tuza2000, First , there has been a detailed discussion of this issue in the thread, http://www.designers-guide.org/Forum/?board=ms_design;action=display;num=1118555 245;start=7#7 For a pipeline ADC, the methodology for simulating an ADC is identical to the methodology a S/H. In the case of the S/H, the noise is not limited by the quantization noise of the ADC, or the thermal/shot/... noise of the S/H. So the FFT noise floor is only limited by the numerical noise of the simulation and the FFT. The largest noise source in the FFT is usually the interpolation noise. Interpolation noise occurs because FFTs have very strict requirements about how the signal is sampled, 2^N equally spaced samples. Since SPICE-type simulators do not usually stop at the correct time points without help, the FFT noise floor is often limited by the error in estimating the actual value from the available time points. The easiest solution is to set the maximum step size to be small to minimize the error. However, this increases the simulation unacceptably so Spectre provides the strobe option. It forces a time step at the instant required for the FFT. One other option to consider is using a Spectre's zvcvs source as an ideal sample and hold. It has the same effect as strobe and allows the use of Spectre's built-in Fourier integral calculation. Also, as mentioned in the thread above, the rectangular window is sufficient. Using windowing functions introduces error. You might want to leave some additional time in the simulation at the start.Usually there is some delay required to reach sinusiodal steady-state. For example, common-mode feedback loops usually require time to settle. So you might want to add an additional 100-200ns to the simulation. Best Regards, Sheldon |
Title: Re: How to simulate the harmanic distortion of S/H Post by schehrazi on May 23rd, 2006, 1:58pm Hi, I have a question on this. This is related to the strobe interval which Ken mentioned in his reply. Suppose in the transient simulation, MaxStep is 1ns and the simulation length is 100us. MaxStep only defines the maximum time step which is used in the transient simulation right? so, in a simulation, the actual time step which used can be sometimes smaller. which means, the simulator does not calculate the desired node voltage at all integer multiples of MaxStep (1ns). Now, my question is if strobe periode (which for example 25ns) forces the transient simulation to do the calculations at all integer multiples of 25ns? What I myself understand, is that strobe periode only strobes the desired node voltage at integer multiples of 25ns and because the actual time steps can be smaller than 1ns, an interpolated point might be picked instead of a real calculated point. |
Title: Re: How to simulate the harmanic distortion of S/H Post by schehrazi on May 23rd, 2006, 2:53pm Hi, Again, I found the answer myself after looking at Ken's book "The designer's guide to Spice and Spectre" carefully. On page, 240, in the paragraph right before it enumerates the useful characteristics of strobing, it says that in contrast to SPICE, Spectre actually places a time point at the sample time and interpolation will not be a used." |
Title: Re: How to simulate the harmanic distortion of S/H Post by mikki33 on May 24th, 2006, 12:57am In HSPICE you also can do it. Use option called INTERP to write output with the step defined in the .TRAN statement. Another option called DELMAX will define max simulation step. So the above example will looks like .options interp=1 delmax=1ns .tran 25ns 12.8us Michael |
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |