Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Noise analysis of op amp stage

Status
Not open for further replies.

glias

Full Member level 2
Joined
Jul 31, 2004
Messages
140
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,298
Activity points
1,076
Hello,
I'm not very familiar with noise analysis in specially for simulation on spice. I would want to evaluate the noise on the output of this schematic. I have also a question to know what is the best way to minimize the noise of the output, as I know the best way is to place the higher gain on the first stage isn't it ?
The first stage is made for creating a bias to the sensor (which is equivalent to a resistor with a typical impedance of 50 ohms), the variation of this impedance is amplify but I have a lot of noise (on the scope more than 4mV peak to peak !) despite of very low noise amplifier (ADA4898).
(MCT sensor is equivalent to a variable resistor (the value of the resistor varies with the IR beam))

So my first question is how could I reduce this noise ?
How can I simulate the output noise with LTspice ? I tried it but I don't know where I should place the input AC generator ... ? because the input is just the equivalent resistor of the sensor, do I should place the AC generator in parallel with the MCT sensor ? or in serie with the bias voltage ?
I also have a restriction of the gain of my first stage because the feedback resistor may have low value (see datasheet of the ADA4898), as the MCT sensor is fixed to have 50 ohms, I can't have play on it to have more gain... (or maybe by placing a resistor in // to reduce the equivalent resistor value of the MCT)

here is my schematic


as you can see the first gain is 40 and the second is about 20, so a total gain of 800.

I hope that you could help me !
thanks

PS : R14 is 1k not 100k.
 
Last edited:

glias

Full Member level 2
Joined
Jul 31, 2004
Messages
140
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,298
Activity points
1,076
Nobody to help me ?
 
  • Like
Reactions: abil10

    abil10

    Points: 2
    Helpful Answer Positive Rating

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
50,033
Helped
14,497
Reputation
29,264
Reaction score
13,430
Trophy points
1,393
Location
Bochum, Germany
Activity points
287,145
To determine input referred noise, you would place the voltage source in series with the sensor resistor.

Did you notice the LT1964 noise density diagram? The amount is several orders of magnitude above OP noise level, even considering the voltage divider, it's still the dominant source. Thus "a lot of noise" is what you can expect to get from this circuit. You should either go for a low noise voltage reference, that deserves the name, or filter the reference effectively in the frequency band of interest. You didn't by thew way specify the utilized frequency range. In most cases, a sensitive IR detector signal would be processed small bandwidth synchronous demodulation for optimal SNR, but I don't know the application.

Regarding noise analysis, I doubt if the voltage regulator model will have realistic noise parameters, so it's contribution is possibly ignored in the analysis. But you should get an overview of the resistor and OP noise share. I expect, it reveals, that the resistance measurement circuit should be optimized in a way, that sensor and OP noise are the dominant sources. This leads to a simple voltage divider and a feedback network with considerable lower resistance level.
 

glias

Full Member level 2
Joined
Jul 31, 2004
Messages
140
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,298
Activity points
1,076
thanks a lot for your reply FvM and sorry for my late answer, I'm going to make a noise analysis with a voltage generator that represent noise source of the reference. The application is a scanner which "see" a 50Hz to 350kHz IR signal. What do you suggest to me for the synchronous demodulation ?... I'm not sure that is relevant in my case because of the bandwidth, isn't it ?
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
50,033
Helped
14,497
Reputation
29,264
Reaction score
13,430
Trophy points
1,393
Location
Bochum, Germany
Activity points
287,145
If you are processing a wideband signal, synchronous demodulation actually isn't an option. It's also the case in FTIR spectrometers. The most important point is, to get an effective filtering of reference source noise. Also the 110 ohm resistor is acting as an unwanted noise source. Calculating the unavoidable dominant noise sources (50 ohm MCT and AD4898), 350 kHz bandwidth and a gain of 800, 4 mVpp isn't much above this level. so you are possibly expecting too much.
 

Prof78

Junior Member level 1
Joined
Jan 2, 2011
Messages
16
Helped
6
Reputation
12
Reaction score
5
Trophy points
1,283
Location
Manchester UK
Activity points
1,528
There is a very important matter in any use of noise analysis with Spice, particularly when including active devices such as opamps. Many device models are not configured so as to represent the noise performance and using these models will give improper results. To operate effectively the models have to be ‘denoised’ and then separate noise sources are added to the model to represent the ‘real’ device. The process is described in the article:
:
Buxton J (1992) Improve noise analysis with opamp macromodel. Electronic Design 2nd April 73,74, 76-81.

Many other references to noise analysis can be found in:

Hamilton S (2007) An Analog Electronics Companion (Cambridge University Press ISBN 0780521687805) p241-251.

You need to check whether the model has been adjusted for Spice noise analysis by examining the model description to see if there is a section headed ‘Noise sources’ or similar. The sources are usually based on the model of a diode (which has noise characteristics embedded) and passing an appropriate current through them to generate the appropriate voltage and current noise values. These currents can be very large so do not be surprised to see the reported power dissipation of the opamp as very large (e.g. ~0.5MW!)
As noted by FvM you also need to check the LT1964 model for noise characteristics, but the contribution will in any case not be ignored. Spice .takes every noise generating component (active or passive) computes its noise and propagates it to the designated output where they are added (in RMS fashion for uncorrelated signals). Since the model of say the opamp is behavioural and has little correspondence to the actual circuit the computed noise for the model also has no correspondence and hence the need for the process described by Buxton. If the LT1964 model does not have appropriate noise performance then you will have to replace it in the simulation circuit with a fixed (and noiseless) generator and then use the noise spectrum in the datasheet (noted by FvM) to manually add in the effect of its noise (not a simple operation but the application note sboa060 from TI.com may be of some assistance).
 
  • Like
Reactions: FvM

    FvM

    Points: 2
    Helpful Answer Positive Rating

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
50,033
Helped
14,497
Reputation
29,264
Reaction score
13,430
Trophy points
1,393
Location
Bochum, Germany
Activity points
287,145
I would basically expect a correct representation of the OP input stage shot noise (frequency independant) but the 1/f noise is most likely not modelled, because the respective transistor noise parameters aren't set. You would be able to correct the model parameters for a better correspendence with the empirical behaviour.

But the first point but be to check for the noise level and frequency characteristic generated by the models
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top