The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design >> RF Design >> LC VCO doesn't oscillate in transient analysis
https://designers-guide.org/forum/YaBB.pl?num=1129157771

Message started by boshiouke on Oct 12^th, 2005, 3:56pm

Title: LC VCO doesn't oscillate in transient analysis
Post by boshiouke on Oct 12^th, 2005, 3:56pm

Can anyone comment on how to get the LC VCO to oscillate in transient analysis please? Initial conditions are set, and PSS/Pnoise works fine. But in transient analysis VCO simply doesn't oscillate. Thank you.

Title: Re: LC VCO doesn't oscillate in transient analysis
Post by ywguo on Oct 13^th, 2005, 6:32pm

Hi, boshiouke,

Have you checked the netlist again? Most errors are caused by circuit design, typo error in the netlist, etc.

Best regards,
Yawei

Title: Re: LC VCO doesn't oscillate in transient analysis
Post by vborich on Oct 13^th, 2005, 8:59pm

A small current pulse in parallel with the resonator should help. Setting integration method to trapezoidal and max time step to something on the scale of the expected oscillation period may help too.

Title: Re: LC VCO doesn't oscillate in transient analysis
Post by zwtang on Dec 16^th, 2005, 4:20pm

How did you set initial conditions? In my experiment, one oscillating point is set VDD, the other side VSS, LC VCO will start up in transient analysis. You can try it.

Title: Re: LC VCO doesn't oscillate in transient analysis
Post by hrkhari on Jan 23^rd, 2006, 2:31am

Hi Guys:

I just don't know how true is this, but I find the transient response is better if a damped vsin source is applied at the Vdd, and for PSS analysis a pulse source at the Vdd and a parallel pulse current source is used across the LC tank, I would appreciate if anyone could comment further on this.

Rgds

Title: Re: LC VCO doesn't oscillate in transient analysis
Post by naren on Jun 16^th, 2006, 7:51pm

Hi,

The problem could be the following!

Let us say your freuency of oscillation Fosc = 5GHz.

This implies the time period Tosc = 0.2 n secs.

Now, if you check the converegence options in the transient anaylsis form the time step for simulation will be 1 n sec.

This means SpectreRF will solve the circuit every 1 n sec, hence it misses your 0.2 n sec sine wave completely!

1) Set the convergence option in the transient analysis form to "conservative".

2) Set the "MAXIMUM TIME STEP" to "1/100" th of Tosc so that you get good convergence or interpolation...i.e set it to 2p sec!

Since you are setting the maximum time step to 2 p sec, if you try to "greedily" analyse the waveform for say 200 cycles of the sine wave or 200 x Tosc = 40 n secs then it will mean you need to wait for 40 n secs/ 2 p sec calculations to complete..or 20000 steps this might take a longgg time!

So try simulating for 10 or 20 cycles i.e. 4 n secs first!

forget the extra impulse to be added and all that!

such current impulse "concepts" are introduced by useless academicians!