The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design >> RF Design >> Oscillator Gain Kvco
https://designers-guide.org/forum/YaBB.pl?num=1137769284

Message started by hrkhari on Jan 20^th, 2006, 7:10am

Title: Oscillator Gain Kvco
Post by hrkhari on Jan 20^th, 2006, 7:10am

Hi Guys:

How to compute oscillator gain Kvco, for different tuning voltages?. Thanks in advance

Rgds

Title: Re: Oscillator Gain Kvco
Post by Jess Chen on Jan 20^th, 2006, 8:28am

Are you asking about how Kvco is defined in general, how to compute Kvco analytically, or how to simulate a Kvco measurement? If you are asking about a simulation, we will need to know what tools you are using.

Title: Re: Oscillator Gain Kvco
Post by hrkhari on Jan 20^th, 2006, 6:48pm

Hai Jess :

I really want to know, how Kvco is obtained through simulation for different value of tuning voltages, for a given oscillator?. Currently I'm using Spectre-RF for the simulation. Thanks in advance

Rgds

Title: Re: Oscillator Gain Kvco
Post by svensl on Jan 21^st, 2006, 2:38am

To obtain the tuning sensitivity and linearity of your oscillator you need to run a swept PSS analysis. When setting up the PSS analysis you can enable the sweep button at the bottom and enter the control voltage as variable. Just specify the sweep range and number of steps. Once the simulation is finished you can click results, then direct plot, then main form, click on the harmonic frequency button, highlight the 1st harmonic in the harmonic frequency section and press the Plot button. This will give you the frequency plot as a function of the control voltage. Kvco, or the sensitivity is just the derivative of this plot. You can use the calculator function deriv() to create this plot.

Hope this helps.
Sven

Title: Re: Oscillator Gain Kvco
Post by hrkhari on Jan 21^st, 2006, 7:39pm

Thx svensi

I have a problem in the setup of the PSS analysis of the designed -gm differential oscillator, I'm using a damped vsin source at the Vdd to start up the ckt, with a freq of 3.5G, amplitude 1mV and 50M of damping factor. Then I terminate the ac coupled differential output by 50ohms port, respectively. The first question is do I have to convert the ac coupled differential output to single ended output using a balun, prior to 50ohms termination, for simulation prupose?. The second question is, when I use the damped vsin source as a start-up, PSS form setup does not finalize, stating a form error:

Periodic Steady State: Fundamental Tone 1 has a blank name
For each tone that is not "Small" signal and has a SrcId listed, the schematic instance (SrcId) must have a name entered under
the appropriate frequency name property. Please edit the top level schematic to assign these names, save the schematic and
then click the "Update From Schematic" button on the analysis form.

This problem does not occur if I setup the PSS and then insert the start-up source to execute the simulation. Please advise

Rgds

Title: Re: Oscillator Gain Kvco
Post by svensl on Jan 22^nd, 2006, 1:50am

I am no expert, but I don't think you can have periodic sources in PSS in autonomous mode. Try using a pulse source for start-up, just don't specify a period. With independent sources used for start-up, set the PSS start time to a large enough value to be sure these sources are all inactive at the start of the PSS. Maybe someone else can give some more advice on how to solve your start-up problem.

Regards,
sven

Title: Re: Oscillator Gain Kvco
Post by hrkhari on Jan 22^nd, 2006, 8:51am

Thnx again svensi

With regard to your earlier explanation in obtianing the Kvco plot, I had managed to obtain the 1st harmonic vs tuning voltage plot, but how do I select /search the function to deriv() in the calculator. Please do guide me.

Rgds

Title: Re: Oscillator Gain Kvco
Post by svensl on Jan 22^nd, 2006, 12:15pm

The deriv() function should be in the Special Function Menue in the calculator. You can select the wave you just plotted with the Wave button and then use the deriv() on it. For a full list of all the calculator functions you can look at the cadence manual files. You can use cdsdoc in a terminal to open those.

Regards,
Sven