Hi,
   I carried out a PNoise simulation on a ring VCO I have. The plot I got was typical to the phase noise plot of a VCO, but It gives positive values of phase noise in dBc/Hz for offset of 1Hz to about 500Hz relative to the carrier. The corner frequency of the CMOS process is around 100k.
1. Is positive values meaningful & can it be expected
   if the design is'nt very good?
2. If yes, is these positive values of phase noise going to
   greatly affect the measured phase jitter?

Regards
Tom

I also get similar response when i use the Matlab script given in "Predicting the Phase noise and Jitter ...." tutorial. ???

Nick,
   Check out page 31 of http://www.designers-guide.org/Theory/cyclo-preso.pdf.

The term "Power Spectral Density" implies the spectral density of a power-like quantity, in the case of S_phi, the units are radians²/Hz, which is power-like because it is in terms of radians² rather than radians. In this case, the power-like quanity is not a true power.

-Ken

Nick,
   Just so we are clear, the inability to compute the corner frequency is a weakness shared by all simulators that use small-signal assumtions in their noise analysis. Thus it is not just Cadence's simulator SpectreRF that has this characteristic, it is shared by all commercial RF simulators.

You can estimate the corner frequency by using the fact that the total area under the noise curve must equal oscillator output power (noise in phase does not add power to the signal, it simply redistributes the power in frequency). So if P_out is the output power and you can model the noise with a/(1+f_c²/f²), then you solve for a by matching the model to the noise at frequencies above the corner, and then you solve for f_c using P_out = a/(1+f_c²/f²).

Artist does compute L, the normalized noise. This is what you get when you ask for "phase noise" when using the basic PNoise analysis (when you have not gone to the trouble of specifically asking Spectre to compute the PM and AM components to the noise).

-Ken

Nick,
1. Given the units of dBc/Hz, I would say that you used Artist to compute these number and did not use the new AM/PM noise capabilities. When you ask Artist to compute the "phase noise", what it really gives you is the normalized noise, or S_v/V_out.

The numbers you give for output noise are nonsensical for two reasons. First, the numbers look like they are in dB, but you do not indicate they are in dB. Let's assume they are. The second problem is that the noise is measured in A/rt(Hz) while the output is described as being in terms of volts. This prevents the computing of the normalized noise.

2. The phase noise and the output noise should differ by a constant factor because the reported phase noise (which is actually L, the normalized noise) equals the output noise power divided by the output power.

3. At low frequencies SpectreRF will report the normalized noise L as being greater than 1 (positive in dB). That only occurs when the frequency you choose is below the corner frequency. As such, it is not real.

-Ken

I have noticed the same problem with units. I select output voltage, click on a node, then see A/sqrt(Hz) dispayed. The numbers seem to make sense if I simply replace "A" with "V". Personally, I suspect it's a display bug but it would be nice to hear from Cadence on this one.

Nick,
   Just to be clear, when you say phase noise, you mean L as computed with the standard PNoise analysis. When you say PM noise, you mean S_ph as computed using the new AM/PM capabilities of PNoise. Correct?

Remember that L = S_v/P_out. Also remember that it is S_v that has the corner, not S_ph. Thus for low frequencies, S_ph >> L. Above the corner, S_ph and L should be within a factor of two of each other. If they are not, that is an indication something is going wrong.

-Ken

Hi again,

Ken thanks. You were crystal clear.

I was expecting too something like a constant 3dB difference between my pnoise-Phase Noise and my PM noise. Let me explain a bit.

I do pnoise analysis from freq offset 100Hz up to 100MHz. Then I ask cadence to plot PM and AM noise. What I get as a plot (by default) is AM and PM from frequ offset of 10MHz and above. The plot is nothing but a straight horizontal line. Despite the graph being wrong, AM and PM are equal for the plotted range of frequencies.

If I manually ask it to show me the waveforms for the whole range of freq I have simulated (i.e. for freq 100 Hz till 100 MHz) I get the 3dB difference as expected, but only at the very beginning of the waveforms. Meaning, if I simulate from 1Hz to 100 MHz, I will see that 3dB difference only at 1Hz. If I simulate from 10 KHz to 100 MHz, I will see that difference at 10 KHz.

What happens afterwards is this. My PM noise drops with a big slope, forming a notch and rises up again to a value of about 10 dBs lower to the initial value it has. It then maintains that value for the rest of the frequencies. What Cadence actually shows me when I plot the graph is the part right after the notch, when AM and PM have settled to that value. Both PM and AM keep that value for the rest of the frequencies simulated, resulting in that horizontal line on my plot. To this I should add that the y-value of this horizontal line varies depending on the frequ from which I start the pnoise simulation.

To sum up: the only correct part of the graph is at its beginning, where I get the 3 dB difference. Whatever is wrong, I am guessing that it is the reason why cadence by default chooses not to plot the peculiar part of the graph. I don’t get any error messages. However, I think it is somehow related to the fact that I start my oscillator with a damped vsin. What do you think of all this?

Nick