the total input reffered noise definition

[chang830]

input referred noise definition

Hi,
I know how the total output reffered noise is caculated in noise simulation. But I have spme puzzles on how the total input reffered noise is computed. originally,I thought it is the integrated value of the input reffered noise for the bandwidth of the circuit, kust like teh caculation of the total output reffered noise. But some papers said it is the total output reffered noise divided the gain(mid-band gain).

Anyone help to clarify it?

Thanks in advance

 

[sankudey]

input referred noise calculation

Hi,
I also have heard and think its right.....if the output referred noise is predicted/calculated rightly.....then u can think of as the circuit as noise less with a input noise voltage (in series) equivalent to op noise divide by the gain......now midband gain is considered....

In cadence...i had some problem with noise simulation.....although it was of dynamic comparator along with some digital cells those not at all biased ... i used the above method......

pls. give ur comments...if i am wrong.....

sankudey

 

[chang830]

integrating noise in pspice

Hi,
I also have heard and think its right.....if the output referred noise is predicted/calculated rightly.....then u can think of as the circuit as noise less with a input noise voltage (in series) equivalent to op noise divide by the gain......now midband gain is considered....

In cadence...i had some problem with noise simulation.....although it was of dynamic comparator along with some digital cells those not at all biased ... i used the above method......

pls. give ur comments...if i am wrong.....

sankudey

If your comparator with some digital cells are not biased to linear region, the noise analysis seemed no meaningful. It is nolinear circuit, while the noise analysis is for linear circuit.

 

[maxwellequ]

iinteg calculator

As I also did in the past, you are mixing two different things:
- What you say that you find in the papers has to do with the SNR calculation: first the output noise power is calculated or obtained from a simulation, and then you divide it by the (square) of the gain that the amplifier has at the frequency of interest (usually the gain in the pass-band), to obtain the SNR.

-What SPICE gives you is an entirelly different thing: it is the noise spectrum that would have to be generated by a noise source at the input of the amplifier, to have the same output noise spectrum. THIS HAS NO PHYSICAL MEANING, I.E. THIS NOISE DOES NOT EXIST. For example, if the amplifier has a low-pass characteristic, the input noise given by SPICE increases with frequency and, if you integrate it, you get ∞.

 

[obovolo]

definition noise profile

look at the units.
V/Hz^0.5 and V or power are quite different.
u have to add all noise at each Hz points to get total noise power.


btw, if u run .noise in spice, it will give u input refered noise.

 

[sankudey]

cadence noise analysis input output define

As I also did in the past, you are mixing two different things:
- What you say that you find in the papers has to do with the SNR calculation: first the output noise power is calculated or obtained from a simulation, and then you divide it by the (square) of the gain that the amplifier has at the frequency of interest (usually the gain in the pass-band), to obtain the SNR.

-What SPICE gives you is an entirelly different thing: it is the noise spectrum that would have to be generated by a noise source at the input of the amplifier, to have the same output noise spectrum. THIS HAS NO PHYSICAL MEANING, I.E. THIS NOISE DOES NOT EXIST. For example, if the amplifier has a low-pass characteristic, the input noise given by SPICE increases with frequency and, if you integrate it, you get ∞.

Hi maxwellequ,
How SNR could be defined in the way u wrote. SNR == S/N (power) ...i.e. (Signal power) / (Noise Power) ..... be it at INPUT or OUTPUT.....we are generally interested of Output SNR......and u wrote N/Gain....=> having Dimension of Noise.....I think its not write......

Regarding SPICE (as in Cadence).....I am not pretty sure....but what I think is that...in noise simulation ( a simulation type like 'tran').....it basically put the noise equivalent circuit of the devices.....then it calculate the equivalent noise at output or input......thus it may vary for the same circuit with different biasing...as mentioned earlier by "chang830" it is for linear circuit.....so we can take it as the noise generated by the circuit components/devices....... like kT/C noise....and its input equivalent 'amount' is called as 'Input referred' noise......

any comment or correction to the baove is welcome.....definitely we are not that much familiar with the internal workings of the tools we use....any input from experianced persons or persons from proper domain may enrich this discussion.....


thanx.
sankudey

 

[chang830]

input noise site:edaboard.com

-What SPICE gives you is an entirelly different thing: it is the noise spectrum that would have to be generated by a noise source at the input of the amplifier, to have the same output noise spectrum. THIS HAS NO PHYSICAL MEANING, I.E. THIS NOISE DOES NOT EXIST. For example, if the amplifier has a low-pass characteristic, the input noise given by SPICE increases with frequency and, if you integrate it, you get ∞.

Hi,maxwellqu,
As far as I know for the noise computation in SPICE, the noise of single device in circuit is first caculated, and be multiplied by the gain of these noise source to th e output. Then the noise is added at the output. The output noise is not generated by a noise source at the input of the amplifier.

Pls. correct me if i misunderstanding.

 

[wonbef]

calculate integrated noise in amplifier bw

now i am blurry to it, too.in cadence design tool: i think .noise analysis results is not correct:
device noise ...
input reffered noise ...
the total input reffered noise ...
the total output reffered noise ...

pls if anyone know! thanks in advance.

 

[pixel]

vnin cadence

Input reffered noise density is just mathematical model which enables comparision of amplifiers with different gain and bandwididth. It can be seen as normalized value of output noise trough bandwidth and gain...

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
(at the output you can because circuit will shape noise in some bandwidth)
-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 by dividing it by the ampliifier 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 amplifier Bandwidth. Someone insetad of whole bandwith takes just part where noise ampliification is lowest , 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.

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 amplifiers's BW. 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 amplifier's BW. How much? It should be defined defined by equivalent noise BW - 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 amplifier's bw (ideally infinite).
-Input reffered noise concept is suitable for different receivers comparision, because it has noise information normalized by gain, and amplifier's bw. For complete comparision you should know also the bandwidth in which input reffered noise was calculated, and this bw should be equal to amplifier's bw.
-If someone insetad of whole amplifiers bw, takes part where noise is more or less attenuated, than it can have smaller/higher values of input reffered noise than actual.

 

[Maxmegen]

pspice snr total output noise voltage

Hi all,

In my opinion, there are several Cadence functions that help to understand the calculations done by Cadence regarding noise.

The first one is the use of the iinteg() function in the calculator to calculate the cumulative output noise of the circuit:

Vout_integ=sqrt(iinteg(VN()**2))

The shape of this curve becomes normally flat at high frequencies because of the dependance of the circuit gain with frequency. The point in which this curve becomes flat is representative of the bandwidth in which it makes sense to integrate the output noise.

If the same curve is calculated for the input referred noise:
Vin_integ=sqrt(iinteg(VNIN()**2))

then it can be observed that this curve does not become flat. This is because of mathematical tricks done by Cadence: at high frequencies there's still noise at the output, but the circuit has almost no gain, o even a very strong attenuation. Then mathematically speaking it is needed to assume a very high input noise to still have a certain amount of noise at the output when there's a huge attenuation.

A third tool that helps is to observe the transfer function calculated by the noise analysis. This function can be accessed through the Results -> Direct Plot ->Main Form menu. It can be checked that the output referred noise and the input referred noise relationship obbeys to the shape of this transfer function.

I hope this will help. Any feedback is more than welcomed.