The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> how to simulate the noise of a chopped amplifier?
https://designers-guide.org/forum/YaBB.pl?num=1250358943

Message started by subgold on Aug 15^th, 2009, 10:55am

Title: how to simulate the noise of a chopped amplifier?
Post by subgold on Aug 15^th, 2009, 10:55am

the removal of the 1/f noise by chopping seems to be a correlated effect between two time points (or periods). i am not able to see the reduction of 1/f noise, unless I choose "timedomain" in the "Noise Type" option from the pnoise simulation, and sum the noise from two corresponding time points afterwards.

however, if the amplifier is used in continuous-time signal processing, i suppose that the noise should be simulated in pnoise with "sources" in the "Noise Type" option. in this case, how to correctly observe the effect of the chopping on the 1/f noise? or in other words, is there an efficient way to measure (i mean in the lab) the noise of the chopping amplifier in a continuous-time manner?

i think lots of people here have done chopping amplifier design. i would appreciate some sharing of your experience on this question. thanks in advance.

Title: Re: how to simulate the noise of a chopped amplifier?
Post by thechopper on Aug 18^th, 2009, 4:45am

Hi subgold,

Running a pnoise analysis with "sources" in the Noise type option is correct, as you suggested.
The effect of 1/f removal can be observed in two different ways:

1) From pnoise you should see the 1/f noise components modulated at odd harmonics of your chopping frequency...
2) Simply look at the pnoise results at base band and compare them to a plain noise analysis on your amplifier (without chopping clock activated). The difference betwen both cases should be clear.

In the lab: with an oscilloscope just set your time base at - say - 2s/div and stop the chopper clock. You should see the typical noise floor (like a noise band) slowing drifting upwards and downwards, always around its mean value.
If you turn on the chopper clocks, you should see the same noise floor (or band) wihtout any drift, i.e. just a straight noise band.
The pkpk noise from that band is the white noise.

Hope this helps
Tosei

Title: Re: how to simulate the noise of a chopped amplifier?
Post by subgold on Aug 19^th, 2009, 3:08am

HdrChopper wrote on Aug 18^th, 2009, 4:45am:

Hi Tosei,

although i have already known what you said, thanks for your reply anyway.

maybe i should state my question more specifically: how to observe the 1/f noise removal effect in frequency domain?

i have seen many papers presenting a nice picture of noise PSD with a flat white noise down to near 1Hz or even dc (e.g. C. Enz et al "A CMOS chopper amplifier" JSSC 1987). is this really possible unless we do some data processing afterwards? according to my design experience, the chopping does reduce 1/f noise significantly, but there is always some residual noise up to at least 100Hz, which is as expected and understood. i never see a complete 1/f noise removal.

do you have any comments?

Title: Re: how to simulate the noise of a chopped amplifier?
Post by thechopper on Aug 19^th, 2009, 3:56pm

subgold wrote on Aug 19^th, 2009, 3:08am:

i have seen many papers presenting a nice picture of noise PSD with a flat white noise down to near 1Hz or even dc (e.g. C. Enz et al "A CMOS chopper amplifier" JSSC 1987). is this really possible unless we do some data processing afterwards? according to my design experience, the chopping does reduce 1/f noise significantly, but there is always some residual noise up to at least 100Hz, which is as expected and understood. i never see a complete 1/f noise removal.

do you have any comments?

Hi subgold,

The residual noise you are referring to might be related to the ratio of chopper frequency vs flicker corner frequency. If such ratio is not high enough some spectral leakage from the modulated 1/f into the base band might be observed.
Otherwise you should not see residue.

As for the noise measurement, if you capture data from your scope at a sufficiently long base time and then you process it with matlab for estimating its PSD you are going to be able to see the 1/f removed when your amp is chopped.

Hope this helps clarify things a little bit more
Regards
Tosei

Title: Re: how to simulate the noise of a chopped amplifier?
Post by subgold on Aug 20^th, 2009, 12:32am

hi Tosei,

thanks for your reply.

HdrChopper wrote on Aug 19^th, 2009, 3:56pm:

[

Hi subgold,

The residual noise you are referring to might be related to the ratio of chopper frequency vs flicker corner frequency. If such ratio is not high enough some spectral leakage from the modulated 1/f into the base band might be observed.
Otherwise you should not see residue.

i dont think it is due to the spectral leakage, because the shape of the noise PSD looks like just 1/f (only the values are smaller). i think it is because of:
1) the spikes resulting from the charge injection or whatever similar;
2) the mismatch between the two chopping phases

Quote:

As for the noise measurement, if you capture data from your scope at a sufficiently long base time and then you process it with matlab for estimating its PSD you are going to be able to see the 1/f removed when your amp is chopped.

does "a sufficiently long base time" simply mean i need to have sufficient time points when i capture the data from the oscilloscope?

Title: Re: how to simulate the noise of a chopped amplifier?
Post by thechopper on Aug 20^th, 2009, 5:41pm

subgold wrote on Aug 20^th, 2009, 12:32am:

Usually spikes from charge injection get aliased to the baseband causing what is called residual offset. Consequently its harmonics components are located at theeven (rather than odd) harmonics of the chopper frequency. Therefore I think it is much harder to observe "tail" of their PSD in the base band.
Mistmach between two chopping phases usually can be observed as a gain loss, not as residual noise.

subgold wrote on Aug 20^th, 2009, 12:32am:

does "a sufficiently long base time" simply mean i need to have sufficient time points when i capture the data from the oscilloscope?

I meant you need both: sufficient time points and during sufficient time: the key is to capture your noise waveform long enough in order to be able to see the low frequency components of your signal. Additionally the more resolution you have while acquiring your signal the better estimation you will get.

Best Regards
Tosei