The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design >> RF Design >> time domain pnoise simulation problem?
https://designers-guide.org/forum/YaBB.pl?num=1165469055

Message started by Aigneryu on Dec 6^th, 2006, 9:24pm

Title: time domain pnoise simulation problem?
Post by Aigneryu on Dec 6^th, 2006, 9:24pm

Dear all,

Does anybody know why in pnoise simulation, if time domain is chosen, it can only give voltage noise?
I use an iprobe in series with the drain of a MOS, and a sine wave is applied at the gate node. If "sources"
is chosen as the noise type, the output noise would be current noise in A/sqrt(Hz) or A^2/sqrt.

However, when the noise type is switched to "timedomain", the result turns out to be voltage noise in V/sqrt(Hz)
or V^2/Hz. Why is that?

Title: Re: time domain pnoise simulation problem?
Post by Aigneryu on Dec 6^th, 2006, 11:10pm

Continued,

I also make a test:

I use a DC current source idc and set the noise vector to [1Hz 400n] [100MHz 400n]. the idc is in series with an iprobe and
a noiseless 1 ohm resistor to GND.

1. in AC noise simulation it gives me noise PSD of 400n (V^2/Hz) and if I integrated over 1GHz, it gives me 400 (V^2)

2. then I do the similar thing in PSS,
I add a 1ns cycle signal source to the testbench, and run pnoise, set noise type to "sources", compute 10-1GHz from the 0th fundamental, which means DC. And I get exactly the same result as the AC noise.

3. Finally I switched the noise type to time domain, unlike the previous two case, I only compute the 1MHz offset from the DC.
This time in the direct plot menu, the unit of the magnitude is changed to V^2/Hz, which is very strange because I am looking
the noise current. And I choose "Output Noise" and "sweep" to "time", and choose "modifier" to "magnitude (V^2/Hz)", and "Frequency" to 1MHz. I got a 40.4u (V^2/Hz) over the 1ns time index.
If I choose "Integ Output Noise" from 0 to 1GHz, and I get a 201 V/sqrt(Hz) over the time index

How do I relate the numbers from case3 to the previous two? Since it is only a white noise current, I simply assume that I should get the signal power v.s. time index, of which average should be the same as the integral of the noise PSD from the previous two cases.

Am I doing something wrong? Or did I mistake the meaning for the time domain noise? I thought it is the noise power v.s PSS phase.

Title: Re: time domain pnoise simulation problem?
Post by spevchin on Dec 7^th, 2006, 6:28pm

SpectreRF seems to have a problem with switching the units for your example (Amp instead of Volts).
The gui team is planning to fix it soon. If one in doubts, it is always helpful to look at results using
Result Browser tool or to go directly to the files in /psf directory and look it up.

As far as tdnoise results, one need to realise that it is a sampled noise measurement, not power vs. time index. There is
an aliasing effect due to the sampling, more information is available online and in the Switch Capacitor paper on this site(Analysis section).

To compare (which is only possible for a stationary white noise case), it is important to select the proper value for maxsidebands in
PNoise, and to integrate from 0+ to FreqPSS/2 only. The fact that you get such a high value for sampled noise PSD at 1MHz (40.4u)
tells me that you set maxsideband to something like "100". Due to sampling nature, it gives you 101X higher results for both PSD
and integrated total power. There might be a factor of two somewhere (like maxsideband is 50) but it is hard to say without exactly
reproducing what you are doing.

Again, tdnoise is sampled (or strobed) periodic noise analysis, not simply noise power vs. PSS phase. Please read the
document: http://www.designers-guide.org/Analysis/sc-filters.pdf

Regards,
SP.