Stats

  • Locked Locked
  • Replies 15
  • Subscribers 64
  • Views 22905
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Phase noise simulation in ring oscillator

Ayrin

I have two questions regarding the phase noise simulation results (PSS + Pnoise) for ring oscillators:

(1) How much the precision of the initial oscillation frequency is important in estimating phase noise ?

(2) The results that I get for the phase noise seems a bit high. I feel there is a shift up in all the frequencies. In very low frequencies (close to carrier) the phase noise is largely positive. Comparing with the analysis presented in [Abidi, JSSC 2006] the phase noise sounds very high. Does someone has any idea that what could be wrong?

 

The ring oscillator designed to oscillate at 2.4 GHz using CML gates with a tail bias current of about 200 uA. 

 

Thanks in advance for your help.

 

Armin

 

  • What version of the simulator are you using? Have you tried turning on "lorentzian" on the pnoise options form?

    Andrew.

  • Hi Andrew,
    • The version of the Cadence tool is IC6.1.5 and for MMSIM it is 7.2
    • I didn't try "Lorentzian", even I couldn't find it in the options of pnoise analysis

     

    Thanks,

     Armin

  • Hi Andrew,

    You can add the option  lorentzian=yes in the additional param record, you can find this record in the pnoise options form.

    Anyway if you used a modulated analysis ( e.g. jitter analysis ) it should be better to upgrade the version of MMSIM, because the oldest versions had a problem with this kind of analysis

    BR

    Raffaele

  • Hi,

     

    Coming back to the issue of phase noise simulation for a ring oscillator, I have seen again the two following issues:

    (1) for a differential ring oscillator, the simulated phase noise at 1 MHz offset is just very high (about 0 dBC/sq.Hz). I don't think this is correct. Here I introduce /voutp and /voutn as the outputs of the oscillator in the pnoise simulation table.

    (2) when I redo the simulation and  introduce the outputs in the pnoise simulation table as: /voutp and /gnd!, then the simulated phase noise goes done by about 100 dB ! Now this one sounds to me like a very good number, much better than the expected !

     

    Do you have any suggestion for a reliable simulations ?

     

    Thanks,

     

    A.

  • Hi Ayrin,

    There’s not much to go on here…   It would be helpful to have more information.

    For starters,

    • The subversion of MMSIM you are using
    • Your analyses and options statements from the netlist.
    • I assume you are using the shooting engine.
    • Is this an injection locked ring oscillator?
    • Have you looked at solution 11784002 on Cadence Online support and followed the suggestions there?

    Best regards,
    Tawna

  • Still not enough info to go on. Can you contact customer support instead so you can provide all the necessary information to understand what you're doing? Did you use a more recent version of the simulator? (I'm a bit surprised lorenzian wasn't there with MMSIM72, so something sounds a bit strange in your setup; maybe it was a very early MMSIM72 version - I can't quite remember when it was introduced).

    Either way, I'm not sure if that's what your problem is.

    Regards,

    Andrew.

  •  Hi,

    Thanks for your reply!

    The version of the tool I am using is: IC6.1.5 and for MMSIM it is 7.2.

    I set no special option: PSS (shoting method) pluse PNOISE. The oscillator is a ring oscillator with CMOS inverter type of delay elements. To make it differential, there is a weak cross-coupled between each two differential nodes.

     

    As I mentioned, the phase noise improves by about 100 dB when I set the output in PNOISE simulation /voutp and /gnd!. If I select the output as /voutp and /voutn, the reported phase noise  is very bad.

     

    Thanks,

    Armin

  • Hi Ayrin,

    You still haven’t provided the section of your netlist containing options and analysis statements.

    I’m sure it’s a setup issue.

    Also, you are using an extremely old version of spectre that is no longer supported.

    Please upgrade to MMSIM12.1.

    Best regards,

    Tawna

  • Hello Tawna,

     

    Thanks for your support. Here is the option section of my setup:

     

    analysis('pss ?fund "1.5e9"  ?harms "20"  ?errpreset "conservative"   ?oscana t  ?p "/xp<1>"  ?n "/gnd!"  ?ppv ""  )
    analysis('pnoise ?sweeptype "relative"  ?relharmnum "1"  ?start "1e3"  ?stop "1e7"  ?dec "11"  ?maxsideband "40"  ?p "/xp<1>"  
            ?n "/gnd!"  ?oprobe ""  ?iprobe ""  ?refsideband ""     )

    option( ?categ 'turboOpts  'uniMode  "APS" )

     

     

    Thanks,

     

    Armin

     

  • Hi Ayrin,

    You have probably resolved your issues by now - but if not - there are a few relatively straightforward items I noticed that will significantly impact the accuracy of your pnoise results  (especially since you noted you are examine the phase noise close to the carrier).

    1. I am not sure what the time length (TSTOP) of your simulation is. However, it does not appear you allowed for a finite TSTAB in your PSS analysis. The lack of a finite value for TSTAB suggests the PSS analysis will consider the transient start-up behavior in its estimate of the steady-state waveform. This will impact the PSS solution - and be especially important for frequencies close to the carrier as the time constants of the transient are likely long relative to the period of oscillation. I would recommend adding a value of TSTAB that encompasses the total time required for the start-up transients to become negligible. You might estimate this by running a transient simulation and plotting the frequency in percent or ppm from the final value at the end of the simulation and choosing a time when the frequency is within 0.1%, for example, of its steady-state value.

    2.  I noticed you did not include a value of integration parameter &quot;maxstep&quot; in your PSS analysis. With &quot;errpreset&quot; set to &quot;conservative&quot;, the default value for the minimum integration time will be used - which is computed from the TSTOP of the simulation. If this value does not represent, say 25 to 100 points per oscillation period, the accuracy of the resulting zero-crossing estimates may be significant. As you might imagine, this will also impact your phase noise estimate.

    3. To verify if any of these are potential issues, you might plot the resulting PSS waveforms in the differential and single-ended mode analyses you performed. Compare these waveforms to the respective steady-state transient analysis waveforms from a conventional transient simulation (with a low value of maxstep - 25-100 timepoints/period). If there appears to be a signficant discrepancy, items [1] and [2] might be worth considering.

    Good luck! Phase noise analyses require some care and feeding...

    Shawn

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.