|
The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl Simulators >> RF Simulators >> How to simulate an oscillator with two frequencies? https://designers-guide.org/forum/YaBB.pl?num=1216408113 Message started by didac on Jul 18th, 2008, 12:08pm |
|
Title: How to simulate an oscillator with two frequencies? Post by didac on Jul 18th, 2008, 12:08pm Hi, I've found an LC-oscillator(in measurement) that at certain point of Vcontrol sweep has two frequencies of oscillation, it first start at one frequency and periodically it jumps to another one and then returns to the original. It doesn't really bother me because we were measuring this oscillator for other things(we only need something that oscillates in fact) and we could change it's operation were it works as usual but I want to find the mechanism that causes this behaviour. It's transient the solution?, will pss be able to show this effect? Thanks for the help, |
|
Title: Re: How to simulate an oscillator with two frequencies? Post by buddypoor on Jul 18th, 2008, 12:42pm It sounds as if there is a kind of chaos in your system - caused by some non-linearities: If the oscillation amplitude comes to a certain limit it brings another part into action and vice versa. |
|
Title: Re: How to simulate an oscillator with two frequencies? Post by Ken Kundert on Jul 18th, 2008, 3:07pm PSS cannot be used, because a signal with two non-harmonically related frequencies is not periodic. You will have to use transient. -Ken |
|
Title: Re: How to simulate an oscillator with two frequencies? Post by didac on Jul 19th, 2008, 3:43am Hi, Thanks for the answers buddypoor and Ken, our first thought was a bad output buffer design that seems that could change operating point of the oscillator, the other cause that I could think about it's that in the same die are two other oscillators that although they are theoretically off maybe through magnetic coupling(they are quite close) are trying to built oscillation, but we measured the other two oscillators and they didn't show this behaviour(they are the same topology with small changes)... the problem is that we didn't designed this oscillator it's a HBT one that some friends from other university designed and they passed to us for some experiments that we want to do(this week we measured 4 or 5 different VCO's). For the transient simulation I will think a little bit how to do it because the oscillator it's at 5GHz and we are seeing this periodic behaviour in the order of seconds(we see it in a spectrum analyzer and you can count with your fingers the time that last to change from the original frequency to the "secondary" one) so maybe I will need to book for the Mare Nostrum supercomputer for disk space... Once more thanks for the tips, |
|
Title: Re: How to simulate an oscillator with two frequencies? Post by pancho_hideboo on Jul 20th, 2008, 1:11am didac wrote on Jul 19th, 2008, 3:43am:
If you have Agilent GoldenGate simulator, try envelope analysis. Or try envelope analysis of Agilent RFDE(ADS). A perfomance of envelope analysis of GoldenGate is very superior than RFDE(ADS) analysis engine. I don't know a perfomance of envelope analysis of current Cadence Spectre. Since envelope analysis of old Spectre was ultra very slow and wasn't practical use level at all, so a thinking of trying envelope analysis of Cadence Spectre does not rise in my mind even now. It could result in a waste of time. Even if you apply envelope analysis of Agilent GoldenGate or RFDE(ADS), you have to tune simulation set up for getting reasonable results and running envelope analysis effectively. If separation of two frequencies is fairly large, you should invoke two tone envelope analysis. Even if separation of two frequencies is relative small and then you invoke one tone envelope analysis, there are three options about choosing nominal frequency. (1) Lower oscillation frequency (2) Upper oscillation frequency (3) Average frequency of above two |
|
Title: Re: How to simulate an oscillator with two frequencies? Post by didac on Jul 20th, 2008, 7:08am Hi, Thanks for the info pancho, in fact I have RFDE and I think that I also have the possibility of using GoldenGate(there is a promise on tutorials of this tool around here but nothing settled up yet). The frequency deviation was around 100MHz or so, what I'm thinking it's to use something like perturbation over a transient in what I suspect are the sensible nodes, i.e. wait for start-up cycles and steady state(although that as seen in measurements it's not a steady state) and then apply a perturbation in the circuit to see if it occurs a bifurcation to the expected frequency with the hope to speed up simulation time, I'm also checking a book called:"Stabiltiy Analysis of Nonlinear Microwave Circuits",Almudena Suarez,Raymond Quere,Artech House 2003 that provides extensive mathematical analysis of this kind of things to see if I could understand better the behaviour and not just by simulation. Once more thanks for the tips to all, |
|
Title: Re: How to simulate an oscillator with two frequencies? Post by pancho_hideboo on Jul 20th, 2008, 7:22am didac wrote on Jul 20th, 2008, 7:08am:
Maybe there exists any long time constant mechanism in circuit. I suspect bias and power supply. |
|
Title: Re: How to simulate an oscillator with two frequencies? Post by didac on Jul 20th, 2008, 7:33am Hi, One of the nodes suspicious has in fact a bypass cap (huge one) so probably you are right. Thanks for the help, |
|
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |