Stats

  • Locked Locked
  • Replies 19
  • Subscribers 126
  • Views 17031
  • 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

PSS and TRAN jitter results not matching for very simplistic testcase

HoWei

In order to better understand the PSS and TRAN noise simulations, I created a very simple testbench "Vsource+Buffer" (see below) and compared the PSS and TRAN phasenoise and jitter results.

The phasenoise curves are matching okay, but the jitter results (Jcc) are completely off and not matching at all.

The VCO (Vsource) frequency is 100MHz with 0.75V amplitude and the phase noise values are given as source parameters.

Transient noise is enabled with a PSD frequency range from 1M to 1G.

The jitter intergation bandwidth is from 1M to 1GHz as well.

The TRAN phasenoise is the PSD of the absolute jitter, normalized to the 0.75V amplitude (-5.51dBVrms).

Some questions I do have:

1. Why do the jitter values differ so significantly between PSS and TRAN ?

2. What does the PSD averaging value mean in the TRAn setup (did not find any useful description in the documentation) ?

All the settings are shown in the pictures below:

And here the results:

Phasenoise results are matching well from 1MHz to 50MHz, but

3) Why do I not see the harmonics in the TRAN result ? Is it due to sinx/x of the PSD/DFT ?

Below you see the expressions and the huge difference in the Jitter results:

Why are those jitter results differing so much ?

How can I get reliable and trustworthy jitter results ?

  • in reply to HoWei

    1. I have never used this feature, but I believe that in order to achieve more smoothing, you should increase the number in the field "Number of PSD Windows"

    2. You always have to integrate up to half the "beat frequency" of the PSS analysis, so 500 kHz in your case.

  • in reply to Frank Wiedmann

    Thanks for the clear answer !

    One more thing:

    When doing "sampled(jitter)" in the PNOISE setup is - can the "Start-Stop" fields values be ignored or are these values used in the simulation ?

    Because after simulation, when doing "DirectPlot-pnoise" I have to set the integration limits anyway.

    Is there any relation between those two frequency ranges ?

    Do they have to overlap somehow ?

  • in reply to HoWei

    Well, it only makes sense to integrate over data that actually exist in your simulation results. You should also make sure that the steps in the sweep are small enough so that you don't get a significant error from the interpolation between the simulated points.

  • in reply to Frank Wiedmann

    In other words:

    The settings in the PNOISE setup is the parameter for the noise generator and it should "at least" cover the frequency range I am interested in - either relative to the carrier (time-avaraged) or absolute (sampled-jitter).

    In the Direct-plot Jcc setup I only give the bandwidth for the integrating function. Integrating over a wider bandwidth than given in the PNOISE setup is not meaningful.

    I much better understand now the PSS setup, because previously I had the impression that in PNOISE we only define the bandwidth for analysis functions - I was not aware that those settings are defining in which bandwidth the noise is generated.

    This then causes the next question: How is the noise density or noise amplitude defined, since the is no parameter or field to define it ?  Is it thermal noise, or any other kind ?

  • in reply to HoWei

    Stupid me - the noise is defined by the "Vsource" in the schematic of course - its too late ...

    But now we have:

    - The Vsource defining noise power in a given frequency range (e.g. phase-noise values)

    - The PNOISE setup to define which frequency band is considered during the simulation

    - The Direct-Plot analysis functions, which may select only a fraction of the bandwidth e.g. Jcc

    And all those bandwidth definitions have to match/overlap, puhhh - very error prone for beginners.

  • in reply to HoWei

    And that's not all, in some cases you also need to take care of parameters like maxacfreq, see https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000000nTjQEAU 

  • in reply to HoWei

    This too is killing me - I did the next test by adding a div-by-8 after the VCO:

    - beat-freq=12.5MHz

    - tstab is changed from 100ns to 800ns

    - PNOISE is setup with multiple noise simulations 2x phasenoise and 2xsampled-jitter for VCO and DIV8 out.

    - PNOISE harmonic for VCO-out is set to "8", harmonic for DIV8-out is set to "1"

     


    Now the pnoise2 result is NOT showing the proper phase-noise plot anymore - it is selecting the harm=1 instead of harm=8 when plotting with direct plot and the values is constant at -50dBc/Hz - why ?

    The phasenoise for the DIV8-output is matching well with the transient phasenoise.

  • in reply to HoWei

    Doing a single (not multiple )noise analysis with the same settings, then the phasenoise plot selects the 8th harmonic and shows the correct results

    This clearly seems to be a bug, right ?

  • in reply to HoWei

    It looks like the plotting interface is getting confused by the multiple noise simulations. You should probably report this to Cadence Support.

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.