Using Ideal Frequency Divider Block in Cadence

HI Astroshey,

Transient noise.  

If you are able to simulate a PLL with spectreRF, count yourself lucky.   Typically, they won't converge.

If you are simulating dividers with SpectreRF, you need to look at Article 20491924: How to set up pss/pnoise sampled(jitter) when simulating a driven circuit or a VCO, both containing dividers.   This is a NEED.   I'm writing an appNote with R&D that discusses this (currently in review) and many other aspects of pnoise.  Sorry I can't devote much time to answering your questions as much as I'd dearly love to do so.  My day job keeps me busy late into the night.

There are a ton of useful SpectreRF articles and best practices on https://support.cadence.com .  When you get access, ping me and I'll point you to them so you can download them.

best regards,

Tawna

Hi Shawn, 

Thank you very much for all your insight and support on this! I appreciate all the time you spent on it. I will follow your suggestion of stepping back and looking at the transient simulations of the circuit. I just have one last concern for now. I get this warning message (see attached screenshot, the yellow highlighted portion). Does this mean that there is a possibility that my solution does not fully converge and this lack of complete convergence results in degraded phase noise? And using Transient Noise analysis (as Tawna suggested) could resolve this issue? BTW, I am not sure if my cadence version (version IC6.1.8-64b.500.14) has transient noise analysis option. Thanks again for all your time and efforts!

best regards~

Dear astroshey,

You are most welcome, but I am just trying to provide a thought or two. I know how frustrating it can be!

astroshey said:

I will follow your suggestion of stepping back and looking at the transient simulations of the circuit.

I think your effort will be well worth it. I know it may seem to be delaying you from getting your desired result, but the fact that your current phase noise result appears so unusual suggests something is amiss with the pss solution. I am glad you are doing this!

astroshey said:

I just have one last concern for now. I get this warning message (see attached screenshot, the yellow highlighted portion). Does this mean that there is a possibility that my solution does not fully converge and this lack of complete convergence results in degraded phase noise?

Certainly the warning message is not expected and does indicate the convergence process is abnormal. However, I was more surprised to observe that the pnoise analysis is using a 700 MHz signal!

I looked back in your Forum post and see you have specified a relative harmonic of 7! I thought the output frequency of your phase-locked loop (i.e. input to the PFD) was 100 MHz?  You noted your feedback divider was 1000 and with a 100 GHz VCO, that suggests only a 100 MHz output frequency is available. Hence, the relative harmonic should be set to 1.

Is my understanding correct astroshey?

astroshey said:

And using Transient Noise analysis (as Tawna suggested) could resolve this issue? BTW, I am not sure if my cadence version (version IC6.1.8-64b.500.14) has transient noise analysis option.

Transient noise is definitely an option, but does introduce some additional processing that is, what I will term, non-trivial. Specifically, you will need to perform a Fourier analysis of your output waveform that requires some specific settings to provide a good phase noise estimate.

My personal thought - and this is my thought only - is that you consider running a few transient simulations to validate the loop is behaving as you expect. If all looks well, make any adjustments to the pss settings (for example, allowing a longer stabilization time if required), change the relative harmonic to 1 if you are attempting to simulate the phase noise of a 100 MHz output, and re-run a pss analysis following by a pnoise analysis. You can compare the pss transient waveform (the converged solution) and make sure it looks close to your transient only simulation to assure yourself the pss solution is reasonable.

However, please use your best judgement as you know your circuit and the time you have available!!

Shawn

Hi Shawn, 

Thank you for pointing that out. I must have overlooked it! I just changed it to 1. Thank you for giving me the debugging tips! I am on it. Instead of using pss and pnoise, I am using hb and hbnoise (shouldn't be any difference, right?). Again, thank you for your support! You definitely made this time easier for me!

PS: I just wanted to share my PPL performance with you. I think it looks good. I will proceed with changing relative harmonic to 1 and increasing the tstab, and rerun the simulations. Thank you~

Best regards~

If the simulation setups are done properly (this is key), you should get the same answer with shooting pss and harmonic balance.  For strongly nonlinear circuits, shooting will be faster.  For nearly linear circuits, hb will be faster.  

If you have circuits with fast rise times (think square waves and more nonlinear), we recommend using pss-shooting (pss).  It's faster.  hb would take many harmonics (slow) - if you don't have enough harmonics, your answer will be incorrect.

If your waveform shapes are more "sinusoidalish", then use harmonic balance (hb).  It's going to be faster.

It's a matter of using the right tool for the job.  You can use a hammer to pound a screw into a wall, but really the proper tool is a screwdriver.  Similarly, you can use a screwdriver to pound a nail into a wall, but it's pretty darned inefficient.  A hammer is the better tool.  Same thing with pss shooting vs hb.  Use the right tool for the job. 

There is an appnote that I recommend having your professor download for you: Getting the Most Out of Spectre® X-RF 21.1: Maximizing Performance .   It discusses when it's appropriate to use Shooting pss vs hb. If you have dividers in your circuit, you need to use pss shooting (not hb).   

There are many articles on https://support.cadence.com that discuss topics like this.  I hope you're making headway with your professor to be able to download some of our valuable "best practices" articles.  It'll save you much time and help with your understanding.

best regards,

Tawna

If you are going to use transient noise, you really want to read the appnotes on this topic. Setup is so important to get accurate results. 

You can look in the spectre hierarchy for some good workshops (you don't need to download anything from https://support.cadence.com .  They are located here: <SPECTRE21.1>/tools.lnx86/spectre/examples/SpectreRF_workshop/spectrerf_workshop_21.1.tar.gz.  You need to copy spectrerf_workshop_21.1.tar.gz to a location where you have write permission.

gunzip spectrerf_workshop_21.1.tar.gz 

tar xf spectrerf_workshop_21.1.tar

And look inside for: 

• SpectreRF APS Workshop for Full Spectrum Shooting  Pnoise spectreRF_fullspectrum.pdf
• SpectreRF APS Workshop for HBnoise Timeaverage and Transient Noise Correlation spectreRF_hbnoise_tranNoise_correlation.pdf
• SpectreRF APS Workshop for Pnoise Sampled and Transient Noise Correlation spectreRF_pnoise_sampled_tranNoise_correlation.pdf
• SpectreRF APS Workshop for Ring Oscillators    spectreRF_ring_oscillator.pdf
• SpectreRF APS Workshop for Transient Noise Calibration   spectreRF_tranNoise_calibration.pdf
• SpectreRF APS Workshop for Wireless Simulation   spectreRF_wireless.pdf
• Instructions for downloading and installing the GPDK for the above workshops   gpdk_download_install.pdf   

All are very good.  (By the way, there's more good stuff like this listed in Article:  SpectreRF Application Notes and Tutorials - One of our best kept secrets! )

best regards, 

Tawna