Input Referred Noise Calculation!!

input referred noise

Hi Guys,

I have question here regarding the Input Referred Noise Calculation for my Transimpedance Amplifier Design of my research project. I measured the total input equivalent noise and it showed me about 15pA/√Hz . This is the value i got over frequency at 1Ghz since im designing for 1.25Gbps. Now my question, how do I convert this value to nA RMS. My data operating rate is 100Mbps to 1.25Gbps and my low cutoff frequency is about 50kHz. By having this values, how do I make use of them. Your feedback is very much appreciated.

Thanks,
Suria

input refered noise

Let me try:
Your output reffered noise voltage is Rf times higher than input reffered noise:
Vn,out=Rf*In,in
You can calculate output noise power voltage by taking integral vn,out,rms^2= ∫Vn,out^2 df.
Lower integral limit is 0. The key point is to determine higher limit. It is dependent on TIA transfer characteristics and it is some factor greater from TIA bandwidth.
For the case of Butterworth response NEB=1.1*TIAbw. ( Search for Equivalent Noise Bandwidth and Personic Integrals in Saeckinger´s book- Broadband receivers for optical fiber communication p 67-70)
Iin,rms=Vn,out,rms/Rf=15p*√(TIAbw*1.1)=15p√(0.7BitRate*1.1)

In,in,rms=0,131uA for TIABW=70M
In,in,rms=0,465uA for TIABW=875M

->For example in the case of bit error rate =10-9, you have electrical sensitivity in the range:
12*In,in,rms=1.17uA-5.5uA

input-referred noise

Hi Pixel,

Thanks for your valuable feedback.I will click the helped button for you soon. Then i have another question here. When i get the Equivalent input noise which is 15pA/√Hz, I took it at the frequency 1Ghz for 1.25Gbps. Actually, at what frequency i need to take the equivalent noise value. Is its at 625Mhz at the fundamental frequency (half of data rate) or at the 1.25Ghz as per bit rate.

Then when someones say this "the input referred noise current density was below 20pA/√Hz within the amplifer frequency band", are they telling the operating band freqeuncy of the TIA they design. Like my case my operating frequency is from 50kHz to 875Mhz (low cutoff frequecy - Tia BW) or something else. Please clarify me at this part as well.

Then you replied that "in the case of bit error rate =10-9, you have electrical sensitivity in the range: 12*In,in,rms=1.17uA-5.5uA " , actually how u did u get the value of 12 and your calculation proves as my input sensitivity is also in the range from simulation.


Thanks,
Suria

equivalent input referred noise

The most important information for optical receiver is the lowest detectable peak-to-peak current (ip-p) for specified BER, which is called electrical sensitivity. If you assume equal probability of ones and zeroes and white noise it can be calculated that sensitivity is proportional to input rms current with factor Q:
ip-p=2*Q*in,in,rms,
Q depends on BER, such that for lower BER, you need higher signal. You can remember that for for BER change of 10-3, Q is approx. changed for 1.
...
BER 10-6 Q=5.753
BER 10-9 Q=5.998
BER 10-12 Q=7.035
...
in,in,rms=vn,out,rms/Rf
You can notice that if you want to determine sensitivity and i,inrms, you have to find first vn,out rms, which is done by integrating output noise spectral density in the whole frequency range... i.e. from 0.1... 100G .
* If you simulate
In Cadence there is a function rmsNoise that gives you rms noise at the point that you specified in noise setting as the output. Just put interval 0.1... 100G, and set TIA out as noise output.
For example
in,in,rms=rmsNoise(0.1,100G)/value(abs(TIAout),1000))
,where value(abs(TIAout),1000)) is low frequency TIA gain at 1000 Hz (Rf)

**If you calculate
For vn,our rms you also have to find output noise density, and then to integrate it form 0 to infinite...
Output noise density is determined as a sum of noise densities from every component:
-Rf
-amplifier-voltage noise
-amplifier -current noise
but you have to take care how this noise is shaped from input to output

calculate rms noise

pixel said:

The most important information for optical receiver is the lowest detectable peak-to-peak current (ip-p) for specified BER, which is called electrical sensitivity. If you assume equal probability of ones and zeroes and white noise it can be calculated that sensitivity is proportional to input rms current with factor Q:
ip-p=2*Q*i,in,rms,
Q depends od BER. You can remember that for for BER change of 10-3, Q is approx. changed for 1.
...
BER 10-6 Q=5.753
BER 10-9 Q=5.998
BER 10-12 Q=7.035
...
You calculate i,in,rms=v,out,rms/Rf

Click to expand...

Hi Pixel,

Ok, i got the way of calculating the input electrical sensitiviy as per your reply. Please answer me the top 2 question I asked you in the early reply as well, as im quite confused at them.

Thanks,
Suria

input reffered noise

Input reffered noise density is just mathematical model which enables comparision of TIA with different gain and bandwididth.
Notice that you can not:
-calculate input noise power directly by integrating input noise density because you have no information on bandwidth , and integral would not convergate
-you can not measure it directly, because it is not measurable (does not exist - just mathematical model !!!)

The key point for your measuerement should be rms noise at the output.

1. From this value you can determine input noise rms (and thus sensitivity) by dividing it by the TIA gain Rf.
2. You can also determine input reffered noise in,rms^2 by dividing output noise power at the ourput vn,out,rms^2, by Rf^2 and TIA Bandwidth. Someone insetad of whole bandith takes just part where ampliification is lowest (for example before dominant pole = 50k), which gives smaller (but inaccurate) input reffered noise. Be sure that in such papers with unusually small input reffered noise, without specified freq range in which noise was measured, or noise rms, are usually inacurrate.

Then when someones say this "the input referred noise current density was below 20pA/√Hz within the amplifer frequency band", are they telling the operating band freqeuncy of the TIA they design. Like my case my operating frequency is from 50kHz to 875Mhz (low cutoff frequecy - Tia BW) or something else. Please clarify me at this part as well.

Click to expand...

Your TIA frequency band starts from 0 if you do not have ac coupling. In this case noise is also transferred to the output and should be considered. Upper limit can be TIAbw,and you should specify it.

rms noise
Ideally you should measure output rms noise in the whole frequency range from 0 to infinity. In reality uper limit is defined by your measurement equipement.
How much is enough? I would take as starting point some value greater than TIAbw, ENB, or some higher value say 1.25G ..2G.
After some frequency, because of noise shaping input reffered noise will not affect on output. This is because noise is low passed shaped from freq TIAbw with slope -40dB/dec (notice that at TIAbw is not enough).
How much? It should be defined defined by ENB (1.1bw for Butterworth response).
For your case you can prove simulating your circuit noise by Cadence, taking different values for your rmsNoise upper limit.
If same rmsnoise was calculated for intervals 0.1..1G, 0.1 .. 2G , 0.1 .. 10G and 0.1 .. 100G, which differs significantly from 0.1 .. 675k, 1G should be enough.

To sumarize:
-The most valuable information for your receiver is rms noise voltage. Rms noise is determined for the range from 0 to frequency that is larger for some factor of TIA bw.
-Input reffered noise concept is suitable for different receivers comparision, because it has noise information normalized by gain, and TIA bw. For complete comparision you should know also the bandwidth in which input reffered noise was calculated, and this bw should be equal to TIA bw.
-If someone insetad of whole TIA bw, takes part where noise is more or less attenuated, than it can have smaller/higher values of input reffered noise than actual.