Divider noise in a PLL

Dear Nalaeg,

Nalaeg said:

check the phase noise and the jitter. I calculate the phase noise as follows: I check the delay between the input signal and the feedback signal, subtract its average and then get the rms of the whole thing.

If I understand correctly, you are not including the phase noise of the reference signal as you are assuming it is ideal. I am not sure if this is your intention.

Nalaeg said:

The weird thing comes now: I define the transient noise at 20G only for the divider, to check only the effect of the noise of the divider both at phase noise and at jitter. I

I do not understand your terminology "define transient noise at 20G" and your simulation. There are many subtleties when trying to get an accurate noise result from a transient noise simulation and hence knowing the specific details of a transient noise simulation and its netlist is very important. Hence, speaking (writing) for myself, I really cannot provide any helpful comments to you - sorry!

Shawn

Dear Shawnlogan,

Yes, I am not including the noise of the reference signal. I just want to see only the effect of the divider noise at the output and when I compare the feedback signal with the reference signal.

I am redefining one more time the problem as follows:

I am running a transient PLL simulation. I check the phase noise and the jitter. I calculate the
phase noise as following: I check the delay between the input signal and the feedback signal,
subtract its average and then get the rms of the whole thing. I also calculate jitter at the output
of the PLL using jitter function. The weird thing: I define the transient noise only for the divider, to
check only the effect of the noise of the divider both at phase noise and at jitter of the whole
PLL. I find the phase noise(delay between input and feedback signal) and the jitter at the output
to have the same value in cadence. Next, I take the divider in a separate testbench, apply ideal
input signal, run a pss and pnoise and get the noise plot. I put the values in Matlab and Matlab
shows that these "2 jitters", the one between input and feedback signal and the other one at the
output, to have different values. I think Matlab calculation is reasonable because the noise of the
divider sees a high pass function (modelled in Matlab) for the jitter between input and feedback
signal and a low pass function (modelled in Matlab) when I check at the output of the PLL. What
is your opinion about this thing? Why cadence shows that the noise of divider has the same
effect when I look at the input (delay between input signal and feedback signal) and whe
at the jitter at the output? Any idea will be very helpful.

Yes, at the transient analysis, I put the 20 GHz value and I made it "on" only for the divider subblock of the whole PLL? What other subtleties do you need to know?

I am looking forward to your reply!

Dear Nalaeg,

Nalaeg said:

I am redefining one more time the problem as follows:

As I mentioned, getting accurate results using a transient noise simulation requires a lot of attention to the details of the simulation. I specifically mentioned the netlist and nature of your test bench. The netlist is necessary to see the exact transient noise simulation settings and the test bench in order to understand exactly what measurements you are making and the exact expressions used to compute the noise. You did a more thorough job of explaining your tests, which is helpful but I can only guess on most of the simulator settings and measurements. In the interest of trying to help as best I can, I spent some time reading and re-reading your latest information to try to "guess" about possible reasons for your observations. 

Nalaeg said:

What
is your opinion about this thing? Why cadence shows that the noise of divider has the same
effect when I look at the input (delay between input signal and feedback signal) and whe
at the jitter at the output? Any idea will be very helpful.

It sounds as if you are using the same method to estimate the jitter for the standalone test bench and the test bench containing the divider. Your method of observation has an inherent bandwidth defined by the length of your simulation and the time interval of your samples. In other words, you cannot estimate any periodic jitter components below the frequency of 1/TSTOP where TSTOP is your simulation end time. Similarly, if the time interval of the samples you are studying is Tperiod, then the Nyquist rate limits your upper bandwidth to 1/(2*Tperiod). Aliasing of the higher frequency noise will fold energy back into band between 1/TSTOP and 1/(2*Tperiod). You did not specify, but if you are using a noisefmax of 20 GHz, you will clearly get a significant amount of aliasing which will impact the jitter measurement significantly.

I have no idea of the bandwidth of your PLL, but if either of the two frequencies of 1/TSTOP or 1/(2*Tperiod) are anywhere close to the bandwidth of the PLL, your transient noise results will not represent any effect of the PLL on the spectrum and noise. This could be responsible for why your results are the same as you are not examining the jitter over the same bandwidth as your pnoise/pss result.

Once again, I am forced to guess about all your simulation and test bench - so this may not be relevant nor even helpful.

Shawn

Dear Shawn,

You made a very good point and now I am in the right path.  Thank you very much! 

I have another question: Do you know how to specify the noise bandwidth in pss/pnoise analysis? 

Basically, how to transfer that Noise Fmax that I define in transient, to the noise in pss/pnoise? Or how to influence the noise bandwidth in pss/pnoise? Because that is the spectrum I use in matlab.

Dear Nalaeg,

Nalaeg said:

and now I am in the right path. 

This is great to read!

Nalaeg said:

Do you know how to specify the noise bandwidth in pss/pnoise analysis? 

Basically, how to transfer that Noise Fmax that I define in transient, to the noise in pss/pnoise? Or how to influence the noise bandwidth in pss/pnoise?

A pss/pnoise simulation is fundamentally different than a transient noise simulation although both strive to produce an accurate estimate of noise components.

In a pas/pnoise simulation, an optional initial transient simulation is performed for a period of time (tstab). Following this time period, the simulator attempts to determine a periodic solution of the system of equations with some "help" from the simulator settings one provides. Once a converged steady-state solution is achieved, the pss portion of the simulation is complete and its results can be viewed in the time and frequency domain. Following the pss portion, and armed with a periodic steady-state solution, the noise spectrum is derived from the noise sources of the devices after considering its time average and any aliasing due any non-linearity in the steady-state periodic response.

An analogous setting to "noisefmax" in a transient noise simulation in a pnoise simulation is the number of sidebands or harmonics to be used in the pnoise simulation. This is quantified with the "maxsidebands" term.

However, you must also set the number of harmonics in the pss portion of the simulation to provide a pss solution that contains a realistic number of harmonics to represent the steady-state solution. This is specified by the parameter "Number of harmonics" in its GUI. The "Number of harmonics" indicates the number of Fourier components to compute from the periodic time domain solution for use in the pnoise portion of the simulation. Increasing the pss "Number of harmonics" increases the number of timepoints used in the pss portion of the simulation and increases simulation time. 20 timepoints/period are used to assure simulator accuracy for the highest specified harmonic's period.

As a result, it appears that the pss simulation parameter "Number of harmonics" and the pnoise "maxsidebands" both contribute to the amount of frequency folding and its magnitude in a pss/pnoise simultion. These two settings, in my understanding, are analogous to the Transient Noise "noisefmax" term.

Shawn

Dear Nalaeg,

Nalaeg said:

and now I am in the right path. 

This is great to read!

Nalaeg said:

Do you know how to specify the noise bandwidth in pss/pnoise analysis? 

Basically, how to transfer that Noise Fmax that I define in transient, to the noise in pss/pnoise? Or how to influence the noise bandwidth in pss/pnoise?

A pss/pnoise simulation is fundamentally different than a transient noise simulation although both strive to produce an accurate estimate of noise components.

In a pas/pnoise simulation, an optional initial transient simulation is performed for a period of time (tstab). Following this time period, the simulator attempts to determine a periodic solution of the system of equations with some "help" from the simulator settings one provides. Once a converged steady-state solution is achieved, the pss portion of the simulation is complete and its results can be viewed in the time and frequency domain. Following the pss portion, and armed with a periodic steady-state solution, the noise spectrum is derived from the noise sources of the devices after considering its time average and any aliasing due any non-linearity in the steady-state periodic response.

An analogous setting to "noisefmax" in a transient noise simulation in a pnoise simulation is the number of sidebands or harmonics to be used in the pnoise simulation. This is quantified with the "maxsidebands" term.

However, you must also set the number of harmonics in the pss portion of the simulation to provide a pss solution that contains a realistic number of harmonics to represent the steady-state solution. This is specified by the parameter "Number of harmonics" in its GUI. The "Number of harmonics" indicates the number of Fourier components to compute from the periodic time domain solution for use in the pnoise portion of the simulation. Increasing the pss "Number of harmonics" increases the number of timepoints used in the pss portion of the simulation and increases simulation time. 20 timepoints/period are used to assure simulator accuracy for the highest specified harmonic's period.

As a result, it appears that the pss simulation parameter "Number of harmonics" and the pnoise "maxsidebands" both contribute to the amount of frequency folding and its magnitude in a pss/pnoise simultion. These two settings, in my understanding, are analogous to the Transient Noise "noisefmax" term.

Shawn

Dear Shawn,

Thank you very much for your reply.

If you have time, my next questions are:

How to correctly define (for my case)  the number of harmonics in the pss I need, depending on the input and output frequency of the divider? I have an input frequency of 3G and an output frequency of the divider 750M?

I am still unclear about these "maxsidebands". If I define maxsidebands = 10, does it mean that the upper limit of my noise bandwidth added at the output signal is 10*750M = 7.5G?

Dear Nalaeg,

Let me try to help out with your added questions...

Nalaeg said:

How to correctly define (for my case)  the number of harmonics in the pss I need, depending on the input and output frequency of the divider? I have an input frequency of 3G and an output frequency of the divider 750M?

Mr. Andrew Beckett and I had a discussion on the Forum a few years ago with someone who was trying to perform a pss simulation of a divided VCO and was looking for guidance in simulator pss settings. There were a number of issues that we discussed - including the number of harmonics and appropriate settings for the beat frequency in the presence of a "real" divider. The Forum poster summarized his learning in a number of points at the end of the post. There are also a number of Cadence On-line support links that may be of interest.

In your case, your divider is 3 GHz/750 MHz = 4 which is a modest value and will not produce subharmonics - so that makes the pss settings a bit less difficult to determine. However, as noted in the post, you should make sure your minimum integration timestep is chosen to include a good number of points in your 3 GHz period.

I would recommend you examine the relative magnitude of the harmonics of your divided output and the bandwidth of its transition times to determine how many harmonics to include. You certainly want your pss Fourier solution to accurately represent the divided output clock.

https://community.cadence.com/cadence_technology_forums/f/custom-ic-design/48474/pll-pss-pnoise-convergence/1376831#1376831

Nalaeg said:

I am still unclear about these "maxsidebands". If I define maxsidebands = 10, does it mean that the upper limit of my noise bandwidth added at the output signal is 10*750M = 7.5G?

Yes. The parameter maxsidebands is relative to the frequency of the pss solution. This represents the number of sidebands that will be used in frequency translation. Too few will result in a low estimate of folded noise.

Shawn