oermens wrote on Dec 2^nd, 2008, 9:56am:

If you read Cadence Spectre documents surely, you can find all answers to your questions easilly.

oermens wrote on Dec 2^nd, 2008, 9:56am:

If you use Shooting Newton PSS, you have to set fundamental frequency lesser than actual steady state oscillation frequency.

oermens wrote on Dec 2^nd, 2008, 9:56am:

You should set Accuracy=Moderate in your first simulation.
With Accuracy=Conservative, you might encounter convergence problem in PSS.

oermens wrote on Dec 2^nd, 2008, 9:56am:

You had better set reference node as Vo-.
But even though you set reference node as /gnd!, there is no problem.

oermens wrote on Dec 2^nd, 2008, 9:56am:

When master PSS analysis is autonomous, sweeptype is relative and Relative harmonic=1 by your setting. This is implicit setting.
If you are still worried, you may set sweeptype=relative and Relative harmonic=1 clearly.

oermens wrote on Dec 2^nd, 2008, 9:56am:

You had better set Negative output node as Vo-.
But even though you set Negative output node as /gnd!, phase noise results is not changed if you set reference node as Vo- in pss setting.

oermens wrote on Dec 2^nd, 2008, 9:56am:

Basically there is no critical problem in your settings.

http://www.designers-guide.org/Forum/YaBB.pl?num=1223659963/0#1

Explain in detail and correctly.

oermens wrote on Dec 3^rd, 2008, 7:46am:

Does the above mean that simulation fails ?

oermens wrote on Dec 3^rd, 2008, 7:46am:

It seems simulation itself can complete without fail. Right ?

Again explain correctly.

oermens wrote on Dec 3^rd, 2008, 5:17pm:

Error is different from Warning.
Does Spectre report "convergence errors" and "Error" regarding  "imelt" and "vbox" truely ?
Actually Spectre report like following, doesn't it ?

   WARNING (CMI-2377): I50.I_left.I0.I39.I11.I5.g4_N5: Vgd has exceeded the oxide breakdown voltage of `vbox' = 8.673 V.

   WARNING (CMI-2139): I50.I_left.I0.I39.I11.I5.g3_N2: The bulk-source junction current exceeds `imelt'.  The results computed by Virtuoso(R) Spectre(R) are now incorrect because the junction current model has been linearized.

   WARNING (CMI-2144): I50.I_left.I0.I39.I11.I5.g4_N5: The bulk-drain junction current exceeds `imax'.

If so, these are warning.
If these are reported only during shooting newton iterations, generally you can ignore these warnings.

If Spectre report "Errors", spectre simulation will fail and not complete.

oermens wrote on Dec 3^rd, 2008, 7:46am:

Voltage at time=0 is truely 5V ?
Show me your result graph around time=0.

Your post is usage of specific EDA vendor's simulator not "Phase Noise and Jitter Measurements".
Please post to "The Designer's Guide Community Forum ≫ Simulators ≫ RF Simulators".

oermens wrote on Dec 4^th, 2008, 7:32am:

I want to know voltage value at time=0.
So show me waveform during time=0~500psec.

oermens wrote on Dec 4^th, 2008, 7:32am:

Is it truely "Error" not "Warning" this time ?
Such reports from Cadence Spectre are very common in Cadence Shooting Newton PSS.

oermens wrote on Dec 4^th, 2008, 7:32am:

Again the initial guess of the fundamental frequency must be lesser than steady state oscillation frequency.

oermens wrote on Dec 4^th, 2008, 7:32am:

Maybe internal time step is too small and very large memeory is consumed due to convergence difficulty, so simulation is almost hang.
We often encounter such convergence problem in Cadence Shooting Newton PSS.

Increase tstab value.
Loosen your accuarcy setting.
Or try autonomous HB analysis.

I would go farther than simply saying you should loosen your tolerances. I would say that the tolerances you using are very extreme, so extreme that they may be the cause of some of your problems. By default you should use the default tolerances, and only tighten them if , after simulation, you find you are not getting the accuracy you need. The default tolerances were chosen for a reason, because they work in most cases and provide a reasonable tradeoff between accuracy and efficiency. In my experience a large percentage of the problems people have with SpectreRF are self-induced by use of extremely tight tolerances. In addition to creating unnecessary convergence problems, simulations are running 5-10x slower than they need to because people are so conservative in setting the tolerances.

SpectreRF issues the message "V(Vout) is too small to reliably detect the period" when the oscillation dies during the tstab interval. You need to do a better job of starting the oscillator.

Trying to set initial conditions on an LC tank is fraught with problems. In particular, if you try to set the voltage on the capacitor, the inductor interferes and the result is a very large initial current through the inductor. A similar problem occurs if you try to set the current through the inductor. I discuss this issue in some depth in my "Spice and Spectre" book. The end result is you either end up with unexpectedly large initial conditions, which results in "melting" and "vbox" messages, or very small initial conditions, which results in the "too small" message.

You should tell Spectre to save the waveforms during the tstab interval and display them, and then adjust your initial condition and tstab settings to assure that you are getting a good strong oscillation at the end of the tstab interval, and that frequency estimate you give the PSS analysis is roughly correct (there is no constraint that it be greater than or less than the actual frequency, only that it be close, and by close I mean within 10% or so should be plenty).

You might consider starting the oscillator with a damped sinusoidal current source. I find that works best on oscillators with parallel LC resonators.

-Ken

oermens, I suggested you not to set Accuracy=Conservative as first answer to your question like following.
Do you read my post surely. And why do you refer "Warning" as "Error" ?
pancho_hideboo wrote on Dec 2^nd, 2008, 10:34pm:


But we can't often get reasonable results at all in Cadence Shooting Newton PSS or QPSS even though we loosen accuracy setting.
Such issues are well known between RF guys who have other simulators than Cadence Spectre.

http://www.designers-guide.org/Forum/YaBB.pl?num=1220476173/0

i have set the tolerances to defaults (reltol=1e-3, vabstol=1e-6, iabstol=1e-12) and moderate accuracy preset. my simulations no longer give the convergence warnings and as Ken mentioned, they complete much faster. the results are also consistent with the higher tolerance's results.  it is my understanding that flexbalance was made available in MMSIM6.2. we are using MMSIM6.1 so we don't have flexbalance option, i will talk to our network admin about upgrading to 6.2 (we don't download via sourcelink, we get our tools from 3rd party)

---
i just read another post related to flex balance, it seems we did not have the environment variable CDS_SPECTRERF_FBENABLE in our setup script. i will try flexbalance now.
--------

sorry if i'm squeezing too many things into one topic, but i set the environment variable but when i run pss it says 'flexbalance' is not a valid parameter for an instance of 'pss'. Ignored. any idea how to correct this?