The Designer's Guide Community Forum
Simulators >> Circuit Simulators >> pnoise simulation of integrator

Message started by yumi on Feb 21st, 2023, 1:08am

Title: pnoise simulation of integrator
Post by yumi on Feb 21st, 2023, 1:08am

1. Before the pnoise simulation, we have to run pss, how should the number of harmonics to be set? Does this value should same as the maximum sideband in pnoise simulation?
2. As article named "Simulating switched - capacitor Filter With SpectreRF" mentioned, we can simulation with unsampledNoise analysis and sampledNoise analysis. In the latest version of spectre, I cannot find these in analysis, how to realize these two simulations? By pnoise or other analysis?
If this can be realized by pnoise, how to set the parameters?

Title: Re: pnoise simulation of integrator
Post by Ken Kundert on Feb 21st, 2023, 7:04am

The harmonics parameter in PSS allows you to specify how many harmonics in the output spectrum you need.  If you don't plan to look at the output spectrum, then you would set it zero to avoid wasting time computing the output spectrum.  Spectre allows this.  However, for reasons I have never understood, ADE requires that you provide a non-zero value.  So you would set harmonics=1 to minimize the waste.

The sampled and unsampled noise analyses in the paper were being performed outside of ADE.  They names unsampledNoise and sampledNoise are arbitrary.  I chose them to be descriptive.  What is important is the parameters specified with each analysis.  To perform these analyses in ADE you would would configure the PNoise analysis to perform a sampled noise analysis.  Look for some kind of time-domain noise parameters and ask for one point at the time you select.

Title: Re: pnoise simulation of integrator
Post by yumi on Feb 21st, 2023, 6:01pm

Thanks for your reply, it helps a lot. Just for confirm, if I want to see the samplednoise (with noise aliased to fs/2), the noisetype should be set as sampled(jitter)?

Title: Re: pnoise simulation of integrator
Post by Ken Kundert on Feb 22nd, 2023, 11:46pm

I don't know. I don't recognize that version of the form, and the label seems self contradicting.

Title: Re: pnoise simulation of integrator
Post by smlogan on Mar 6th, 2023, 5:01pm

Dear yumi,

I am not sure of your objective, but if you set the noisetype=sampled(jitter), the noise is measured only on the threshold crossing you define in the GUI - the remaining portion of the waveform is not used.With the radio button selection you show ("Sampled phase"), you must specify times  within the pss analysis or a number of points within the period and the analysis will provide the sampled noise at those times or time intervals. With knowledge of the slope of the waveforms for the time(s) you specify, an estimate of the jitter can be computed for each.

I hope this helps yumi and I understood your question!


Title: Re: pnoise simulation of integrator
Post by Ken Kundert on Mar 7th, 2023, 10:24pm

I find the terminology used very confusing.  jJtter is always measured at a threshold crossing, whereas sampled noise is the noise sampled at a fixed point in time.  Sampled noise is a voltage or current or some other signal value, not time.  "sampled jitter" is nonsensical, and I don't know why they put parentheses around jitter.  Perhaps that has some significance I do not understand.  I also don't know the meaning of Sampled Phase (or the other choices) and how it relates to jitter.  And what is "1a" sample points? Is it a hexadecimal number? Is it "1 attosamples per period".

It is all very confusing.

The Designer's Guide Community Forum » Powered by YaBB 2.2.2!
YaBB © 2000-2008. All Rights Reserved.