Signal to noise ratio of the operational amplifier

Status
Not open for further replies.

Dear FvM,

Thank you once again,

I will try next time to use different type of window, like the Hann you suggested then I will update my result,

I see that you all agree that the value of the THD I am reading from spectrum or by Suta setup is real, Ok then I will consider this measurement to improve my linearity.

You also agree that there is no source of noise is included in my circuit so basically I can not measure the SNR, then the question is how the spectrum is calculating the ENOB ?
if you say that Spectrum is mistakenly considering the non real noise appears in the spectrum then it means I should not consider these values from my Spectrum, I will only consider the THD.

Please FvM I can see some papers are giving the SNR for their opamp, and the paper is only about the opamp no ADC or oter circuit is included, so how they provide such value ??

the last but not the least, can the THD effect the ENOB, for me I don't think so, as you already said THD is related to non-linearity distortion, and ENOB is related to the noise and signal level.

Thank you very much once again
Best Regards
 

Hi,

You also agree that there is no source of noise is included in my circuit so basically I can not measure the SNR, then the question is how the spectrum is calculating the ENOB ?
Click to expand...

Maybe "THD+N / FS" ...
--> THD causes error, noise causes error, both degrading ENOB.

for me I don't think so, as you already said THD is related to non-linearity distortion, and ENOB is related to the noise and signal level.
Click to expand...
Don´t guess. Search the internet.
The information can be easily found in the internet.
* https://en.wikipedia.org/wiki/Effective_number_of_bits
* https://en.wikipedia.org/wiki/SINAD
(There are many other sources...)

Opamp noise:
Read this: https://www.analog.com/media/en/reference-design-documentation/design-notes/dn015f.pdf

Klaus
 


Dear Klaus,
I found this from "Opamp for every one", he is measuring the SNR by deviding the output voltage span to the output noise

 

Dear Klaus you are right if I am running (THD+Noise, which I don't know how), but I am currently only running the THD,
please see this also from Texas Instruments
 

ENOB is not only about noise. ENOB reflects all non-idealities, in other word all the garbage that's in the output and that you don't want. So, if you have an ideal ADC with no distortion and thermal noise, only quantization noise, then your SNR is usually given by the ratio of the full scale signal power to the power of the quantization noise, which at the end reduces to the famous formula of SNR[dB]=6.B+1.76 (B - the number of ADC bits). When in addition to the quantization noise you also include thermal noise power and power from harmonics or other spurs in the spectrum, for the same full scale signal you get different value of SNR (or in this case it is SNDR really). Then you can back-calculate B from the formula and this is your ENOB. So, even though you don't have noise per se, but you have distortion, the tool still calculates ENOB based on that distortion.

Perhaps in the papers you read where they cite SNR for an opamp, they did measure noise and thus calculated SNR.

To measure SNR you need a simulation in which your circuit generates noise. In the case of an ADC, just by it working, it produces quantization noise and you can measure SQNR. In the case of and amplifier, you could run a transient noise simulation, which is like your regular transient simulation but with noise on top of it. Then, the FFT will also have noise in it and distortion, of course.
 
Hi,

Dear Klaus you are right if I am running (THD+Noise, which I don't know how), but I am currently only running the THD,
Click to expand...
All the given documents are correct.

Please understand:
* FFT: transforms data from time domain into frequency domain. It doesn't care, whether the frequency components are from the "signal", or from "noise" or from "distortion"...it's just a conversion.

The result of the FFT enables you to calculate a lot of values
* SNR: Signal to Noise Ratio. A noise only value
* SINAD: SIgnal to Noise And Distortion. A combined measure of noise and distortion
* THD: Total Harmonic Distortion. A distortion only value
* ENOB: Effective Nomber Of Bits. A combined measure of noise and distortion
... and so on

Klaus
 
Dear Suta,
Dear Klaus,

Thank you very much for your kind explanation,
Now I fully understand from you that FFT includes all types of error, and specially the ENOB it includes any non-ideal parameter in my design weather it due to linearity or noise.

Also I see that when you talk about ENOB you just refer to ADC, it means for my case where I am only designing and simulating an opamp, it might be meaningless ? I would say I never seen from data sheet of any opamp where people giving the ENOB, it was just an idea from me because in my next readout circuit the ADC will come, therefore I assumed that if my ADC has a 12 bit resolution then my opamp must provide the same ENOB at the output or even greater, again it was my assumption.

When I read the manual book from Texas "Op-amp for every one", This book as surely you read never state about the ENOB. The only parameter he give to consider about the non linearity and noise are :
1.THD
2. THD+Noise
3. SNR in which he find it from the input referred noise.

Now I will characterize my opamp according to this standard

To find the SNR I will find it from two ways, the first as in the data sheet by measuring the input referred noise , the second way is by running the THD+Noise which I am going to learn now,

Dear Suta, can you told me THD+Noise is like a regular transient but with noise at the top, can you please tell me about it more.

Thank you a lot
 

Hi,

Now I fully understand from you that FFT includes all types of error
Click to expand...
FFT is not related to "errors" or "not errors" .... it's just a mathematical conversion..

and specially the ENOB it includes any non-ideal parameter in my design weather it due to linearity or noise.
Click to expand...
And ENOB is not related to FFT. There are other ways to calculate ENOB, but when you work with computers, then the FFT solution is simple and precise.

Also I see that when you talk about ENOB you just refer to ADC, it means for my case where I am only designing and simulating an opamp, it might be meaningless ?
Click to expand...
In "ENOB" the "B" stands for "bits"..... does your OPAMP work with bits? "Bit" is a digital unit, while an OPAMP is a purely analog device.
That's why ENOB is not used with OPAMPs.

For analog devices use "SINAD", because this is the pendant to ENOB in the digital world.

As pendant to the "analog nonlinearities" you may see INL and DNL.

Klaus
 
KlausST said:
In "ENOB" the "B" stands for "bits"..... does your OPAMP work with bits? "Bit" is a digital unit, while an OPAMP is a purely analog device.
That's why ENOB is not used with OPAMPs.

Klaus
Click to expand...

Hi Klaus,
Thank you very much for correcting me,
Yes obviously my opamp has no bits , if you see my former post I was telling that I only wanted to simulate the ENOB to be sure that my output signal from my opamp is suitable to drive 12 bit ADC resolution, However, it is mistake of me to think to measure the ENOB for an amplifier.

I will only perform the SNR, SINAD, THD and THD+Noise.

I am convinced more by your explanation that normal transient analyses has no inclusion of noise devices model, therefore I will run the Transient Noise (only need your setup suggestion please).
Still I have the other way of finding the input and output noise from AC noise analyses.

Hope I could implement the simulation tomorrow so we could please have further discussion on it.

Thank you very much once again
 

ENOB is indeed something related mostly to data converters, because it is a measure in terms of bits. However, sometimes you may hear people talking about an opamp being, for example 10 bits linear, which already makes the connection between opamps and ENOB. Especially in the case when the opamp is supposed to interface somehow with an ADC. So, if your opamp has THD in the order of -60dB, then loosely it is 10 bit linear, or 10 bit accurate, because people make the relation with SNDR (or SINAD) and if it is 60db, than from the formula SNDR=6*B+... it follwos that B is about 10.In other words, it is kind of a measure of how much the amplifier transfer curve deviates from a straight line.

I'll put something together about how to run transient noise.
 
First of all, you should know that transient noise simulation is a long simulation (depending on the circuit you are simulating) and makes sense to use more powerful computer with enough memory and cpu cores.
You can actually not run transient noise. You could only run normal noise simulation, integrate the noise psd within your bandwidth and calculate the SNR. I simulated just an RC circuit but put some dc current through the resistor so I can also get flicker noise, not only thermal. I then ran ac simulation to show the frequency response and after that I ran noise simulation to get the noise psd. I also used the calculator iinteg function to integrate the noise psd and where the integrated noise saturates, this will be the total integrated noise you can use for the SNR calculation. Also, it will show after what frequency the integrated noise doesn't change anymore - in this example it is at about 20GHz. I'll use this value later for transient noise settings. In order to capture some flicker noise, I can start looking after 10KHz. All this is in the following picture.




I ran two transient simulations - one without transient noise and the other with transient noise. Since I wanted to start looking at noise from about 10KHz, I need to simulate something like 100us at least. That's why I modified the number of cycles and the sampling frequency, but keeping about the same input frequency as in the previous example that we discussed few days ago. Transient noise setup is in the transient simulation menu. You have to set up the max frequency, which in this case is 20GHz, because that's where noise integral saturates in the example. In your case it will be different. Then, in the transient noise options you can also set the min frequency, 10KHz. The rest of the transient simulation remains the same as before - stop time and strobeperiod. You run the simulation and plot the fft as before and you can do with it whatever you want. I have plotted two results - one without noise, and one with it. Since I'm using real resistor models (not from analogLib), it has a voltage coefficient and distorts a bit. You can see the distortion in the spectrum without noise. But when I include also noise from the transient noise simulation, those harmonics are completely buried in the noise. All this on the following picture.

 
Dear Suta,

I don' know how to thank you for your continuous support.

I would like to split you explanation in to two parts
1. simulating the SNR from the values I get from AC noise analyses
2. simulating the SNR with the help of the transient + Noise analyses

I will discuss with you my result according to the part one before moving to the part 2,

Below you find please my AC noise simulation at the differential output with the test bench and ADE noise setup.

**broken link removed**
**broken link removed**
**broken link removed**

According to your explanation, and if I understand right, the region of saturation at of the integrated signal (the second wave is the iintig of the first wave) is my output total noise which is about 239 nV. If it is right then I can use it for the formula of SNR,
However, this value has no relationship with bandwidth. may be I didn,t get exactly your point.

Therefore I have simulated for you the output noise in term of V/Sqrt(Hz) as shown below, I put a cursor at my region of interest that is between 1M Hz to 2 MHz.

**broken link removed**

as you can se from the graph I have about 94 nV/sqrt(Hz) which covers my range of frequency,

now let me again post the procedure from Analog Devices to find the SNR

**broken link removed**

Then Output noise (I am plotting the output directly no need to multiply the input with the gain) = [94 nV/sqrt(Hz)]*[sqrt(2 MHz-1 MHz)]= 95 uV.

Now if I go to the ADE, Result--Print--Noise Summary-- then the setting is shown below to show the direct integration of the noise at my region of interest (1MHz-2MHz)



and the result is shown below, it gives easily the same value comparing to the hand calculation of the Analog device method

 

Attachments

  • 6.png
    23.4 KB · Views: 101

Your attachments can't be viewed, except the last two.

I guess there are different ways of getting the noise values. The integration I showed is kind of the worst case (which may not always be applicable) since it integrates noise for the all frequencies it was simulated - loosely speaking to infinity. You are only looking into a limited bandwidth and that's OK - you should put those limits in you transient noise setup if you decide to do it.
 
Dear Suta,
Thank you for the fast response,

I will correct the images, however this time I am only interested in one frequency, this because my opamp will read single sinusoidal frequency sensor signal, let me assume it now = 2 MHz.
it means I must find the SNR at this frequency, my output is buffered connected and Vo= 0.9 Vp-p

first below is the output noise simulation



as you can see that is my noise is 93 nV,

other way I can get is from the Noise summary print as shown below



with direct result given below



- - - Updated - - -

Now I will go for the SNR calculation based on the first method before I move to the transient method one

SNR = 20 log(Vo/Vnoise)..... the noise is given be default in r.m.s value, output voltage = 0.9 Vp-p = 0.318 V

SNR = 20 log (0.318 V/93 nV) = 130.6 dB

Please confirm me this result, is it ok
 

Hi,

it means I must find the SNR at this frequency...
as you can see that is my noise is 93 nV,
Click to expand...

SNR = SIGNAL to NOISE ratio.

SIGNAL is the signal you want to refer to. It´s OK to choose 2MHz.
But NOISE is a complete bandwidth. NOISE is never a single frequency.

But what bandwidth to use:
* with an OPAMP circuit you always have an upper frequency limit. This may be limited by GBP or by your external circut (low pass filter).
(when you do ADConversions I always recommend to use an LPF. As anti aliasing filter, as EMC filter, or at a lower frequency for bandwidth limiting and noise suppression. Mind: anti aliasing cutoff frequency must be chosen, that it has enough attenution at Nyquist frequency. If you want alias frequencies to be attenuated to 1 LSB at a 10 bit ADC then the worst case attenuation need to be 80dB. It depends on the worst case expected noise amplitude. Often 20dB may be sufficient.)

* lower frequency limit can be DC, or a very low frequency, or - if you have - your HPF (OPAMP feedback or HPF between OPAMP and ADC) cutoff frequency.

Klaus
 

Dear Klaus,

You are absolutely right and thank you for correcting me
Now I repeated the simulation, assuming for the moment I don't have HPF nor LPF, so the lower limit of my noise frequency I made it worst case down to 1 HZ and the upper noise frequency limit of integration up to 20 MHz (my GBW is 16 MHZ)

the results are shown below




- - - Updated - - -

Now I will repeat my SNR calculation based on the last updated results

SNR = 20 log (0.318 V/410.4 u) = 57 dB ............(note both the noise and the output voltage are in r.m.s value)

roughly speaking and by ignoring any kind of other non linearity distortion which also affect the ENOB, if we ignore it all I would say my output can drive an ADC with 7.4 bit of resolution
 

Attachments

  • y1.png
    16 KB · Views: 95
  • y2.png
    17 KB · Views: 101

Hi,

SNR = 20 log (0.318 V/41.4 u) = 77.7 dB
Click to expand...
sadly the results show 414uV noise, not 41.4uV.

But the noise is in the region of 1LSB.

Thus I think it is OK.

Klaus
 

Dear Klaus, Thank you again for reply

Actually I have noticed the mistake and I updated it in the same time you were replying ))

- - - Updated - - -

Dear Klaus,

I am convinced by your argument, that the range of the noise is different from the range of my signal value, but now I am watching a video where he only integrate the noise at region of interest, kindly you can see it below, also the Analog Device hand book is considering the noise at the range of signal bandwidth,
I would follow your suggestion, because they might not showing the filter in there explanation

https://www.youtube.com/watch?v=Y0jkPLuFdnM

Any way I would please again ask you, you told that this voltage is below the LSB value of 10 bit converter, How can I calculate it ? it will be very useful
 

Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…