PSS and TRAN jitter results not matching for very simplistic testcase

Update:

After reducing the integration bandwidth from 1GHz to 80MHz in both TRAN and PSS (to avoid the harmonics), the PSS jitter is in the same range as the TRAN result, but still ~4 times higher.

The TRAN result did not change much.

1) To measure the jitter Jcc, which integration bandwidth has to be used - is there any rule of thumb ?

2) Why do the harmonics increase the jitter in PSS so much - they should be in phase and not cause jitter, right ?

By adjusting the integration bandwidth from 1MHz to 50MHz, I could get the PSS rsults into the same range as the TRAN results.

But by adjusting the "k" (measurement cycles) or the BER-value (for peak-peak) I can just get any Jcc value I want.

Still not trustworthy results I think.

By adjusting the integration bandwidth from 1MHz to 50MHz, I could get the PSS rsults into the same range as the TRAN results.

But by adjusting the "k" (measurement cycles) or the BER-value (for peak-peak) I can just get any Jcc value I want.

Still not trustworthy results I think.

You might want to take a look at the following articles and RAK:
https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1O3w000009bh2QEAQ
https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1O0V000007MnBUUA0
https://support.cadence.com/apex/articleattachmentportal?id=a1O0V000009EVE2UAO 

Thanks Frank - I went thru most of them of them in the last days, but still have these open questions:

1. PSD Windows in transient setup: 

It says in the 3rd article (page 20): The larger number of PSD windows allows for more smoothing at the cost of longer transient simulations for a given PSD Min Frequency.

How can I make use of this PSD windows setting ?

The number of samles + time-intervall define the max. frequency in psd(). A larger window size will have more frequency points, a smaller will smooth the results.

 Which parameters can I change in the psd() analysis function to achieve more smoothing ?

2. If I have a PSS simulation with 100MHz at VCO and a div-by-100 frequency of 1MHz at the divider output (= beat frequency), and I want to measure the jitter for both signals VCO-out and DIV-out, what would be the integration limits for the 2 signals ?

DIV-out (Periode=1/1MHz): jitter integration bandwidth up tp 500kHz

VCO-out (Periode=1/100MHz): jitter integration bandwidth up to 50MHz  - or would it be also 500kHz  ?

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.

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 ?

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 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 ?

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.

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