Hi,

I am working on an oscillator.
I am trying to shorten my corner PSS simulations (shooting method).
I am working with spectre, mmsim13.1.0

Convergence seems tricky on that circuit, so I tried (more or less) successfully what was proposed e.g. in http://community.cadence.com/cadence_technology_forums/f/33/t/28744 and other places:
* do a long "liberal" tstab simulation,
* write the result with "writepss" (from PSS options)
* change convergence options to conservative & tighten lteratio, eliminate tstab but read the final result from the previously specified file with "readpss"
* rerun sim & enjoy
* I subsequently start also a phase noise simulation.

--> the simulation appears to converge immediately after loading that file.

Now, if I change process corners and temperature
(a) I have the same immediate apparent convergence at 1st shot
(b) the amplitude of oscillation does not change at all, which is an indication of fault; in previous  simulation I always saw PVT variance, of course)
(c) phase noise simulations DO vary over PVT, but the results are a bit strange - did I invent a circuit that gets less noisy at higher temperature?  ;)
Obviously I'm not really getting trustworthy results.

==> QUESTION:
? can I reuse tstab results from nominal process corner @ T=300K  and expect that in subsequent PVT sims the deviation from this starting point will be recalculated to satisfy corner/temperature conditions?
? if I can expect that: which parameters do I have to set to force the simulator to do so?

many thanks in advance for your comments!

Martin

Hi Ken,
thanks for your quick reply and for putting this into the right category.

Quote:

Well, this is exactly where I have doubts. From previous simulations I know that the oscillatopr amplitude changes over PVT, and now, giving the nominalPriocess/27C tstab+pss "psswrite" result as a starting point, it "converges" in the first iteration, and the amplitude is exactly as in nominalProcess/27C, regardless of process/temp  - this is why I doubt that it converges to the process/temp that I select in ADE.

Quote:

well, normally I would like to do everything from the start with conservative settings, that was always my starting point.
As convergence gets difficult (for some reason in the modified circuit that I haven't found out till now), I tried the approach of loosening tolerances for an initial run for the "psswrite", and then do the fine bit starting from there with "conservative". That was the motivation. "Conservative" would be fine for me in general.
I'm also setting lteratio usually to 6 or so (when I do "conmservative", but that's what I found in one of your papers...

The motivation to use the 2 step approach ("liberal" -> writepss -> "conservative" + readpss + PVT variation) is of course the hope to save time. Running 100us tstab for every corner in "conservative" is a lot of processing time.
Maybe that's asking too much. Any clues?

Martin

You should not default to conservative. You should default to the defaults, meaning that by default you should specify no accuracy settings. With SpectreRF you must specify the errpreset, which you should set to moderate by default.

You should not complain about speed or convergence issues until you have tried the default settings.

It is my experience that a significant fraction of Spectre users, and perhaps the majority of SpectreRF users, are running simulations that are slow and problematic because they unnecessarily tighten tolerances. In fact, at one large company, the CAD group has changed the default tolerances in ADE so that are 100× tighter than Spectre's defaults. I pointed this out to one of their engineers when he was complaining that many of his corner simulations were not completing. Once he erased the CAD group defaults, all of his corner simulations completed and the simulations finished in one tenth the time with no noticeable degradation in accuracy.

-Ken