The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> RF Simulators >> PSS accuracy in oscillator simulation
https://designers-guide.org/forum/YaBB.pl?num=1303196971

Message started by jqjqjq on Apr 19^th, 2011, 12:09am

Title: PSS accuracy in oscillator simulation
Post by jqjqjq on Apr 19^th, 2011, 12:09am

Hi everyone, I'm simulating an oscillator working around 3GHz
and I did the pss simulation to get the frequency.

Yet I want the simulation result to be a bit accurate , for instance,
to be within the accuracy of 10kHz, however, when I redid the
simulation without changing anything, the resulting frequency
fluctuated with about 100kHz at least, so my result seems to
have little physical meaning.

I wondered what should I do to increase the simulation accuracy.

I read the cadence design manual, the sections on PSS options form.
I tried change maxstep to 10p and steadyratio to 1e-8, but they never
worked.

Thanks for any helpful advices.

jqjqjq

Title: Re: PSS accuracy in oscillator simulation
Post by rfidea on Apr 25^th, 2011, 1:19pm

Hi, first of all you should use "conservative" in the PSS settings to increase the tolerance. Then I think it is better to work with the basic tolerances, reltol, vabstol and iabstol instead of steadyratio. For example start with reltol=1e-5, vabstol=1e-8 and iabstol=1e-13. Since steadyratio is setting the tolerance of the whole fundamental period there is no point in tighten this without increasing the basic tolerances.

Then a question about your goal of 10kHz at a 3GHz oscillator. This is 3ppm! That is low, very low, much less than the tolerance of a crystla oscillator and I'm sure this is not a crystal oscillator.