+ Post New Thread
Results 1 to 8 of 8

28th December 2019, 19:43 #1
 Join Date
 Apr 2019
 Posts
 13
 Helped
 0 / 0
 Points
 197
 Level
 2
Noise analysis for diff amp in Cadence
Hello guys!
I want to understand how to run noise analysis in cadence for differential amplifier. How to do it and come up with a value of spectral density for the noise present in the circuit. Thanks in advance.

Advertisement

5th January 2020, 19:22 #2
 Join Date
 Nov 2013
 Posts
 747
 Helped
 205 / 205
 Points
 5,094
 Level
 16
Re: Noise analysis for diff amp in Cadence
It depend on the circuit. Linear diff.pair should be checked with AC noise or pnoise analysis, for switched diff.pair pnoise or transient noise should be used. Otherwise I don't understand what are you curious about, "how to run analysis" is a bit vague question. Share details please (circuit, application, which analysis available in Cadence for you, etc.)
"Try SCE to AUX." /John Aaron/

Advertisement

5th January 2020, 23:40 #3
 Join Date
 Apr 2019
 Posts
 13
 Helped
 0 / 0
 Points
 197
 Level
 2
Re: Noise analysis for diff amp in Cadence
I have designed opamp previously. But have no idea on how noise is measured as seen in data sheet of opamp in terms of gaussian distribution. I want to understand how it is simulated in cadence for linear differential pair circuit. Generically, I have simulated gain, Phase margin, slew rate. Would be helpful if you can tell me how simulation is done for noise as I have no idea on it in terms of cadence simulation. I am a novice circuit designer. I was following a lecture to understand the effects of noise in terms of hand calculation. I want to realize it in cadence simulation.
In the attached image, noise is considered to be generated from all sources present in a linear differential opamp. Considering no effect from current source transistor at bottom, how to simulate the effect of noise from other transistors to obtain noise spectral density

Advertisement

6th January 2020, 19:03 #4
 Join Date
 Nov 2001
 Location
 US
 Posts
 888
 Helped
 307 / 307
 Points
 10,241
 Level
 24
Re: Noise analysis for diff amp in Cadence
Use .noise analysis in ADEL. Define the frequency range, the output node and if you want the input referred noise, define also the voltage source to which you want to refer the noise. It will give you the PSD of noise, which then you can integrate to get the total noise rms.
BTW, the tail current source noise doesn't matter only if the two inputs are at commonmode and the circuit is balanced. If you tilt the diff pair, then you will have some contribution of that nose to the output,
1 members found this post helpful.

6th January 2020, 19:59 #5
 Join Date
 Nov 2013
 Posts
 747
 Helped
 205 / 205
 Points
 5,094
 Level
 16
Re: Noise analysis for diff amp in Cadence
In OPAmp datasheets normally the input referred noise is given. You can get the value of it with simulation of the power spectral density function (PSD).
Connect your OPAmp as unity gain buffer, with a DC source sets its commonmode input voltage in the middle of your commonmode range, then run AC noise analysis (.noise as sutapanaki said).
The analysis automatically adds the theoretical AC noise sources to the small signal equvivalent model of your OPAmp.
After the simulation plot the output node's noise vs. frequency curve (you can pick it from the results browser after simulation or write an expression at your signal outputs, like: VF("/opamp_output_node_name") ).
In unity gain buffer connection the output noise is equal with the input reffered noise at the center of your bandwidth, its unit should be nV/sqrt(Hz), sometimes V^2/Hz, they are the same basically. Or as sutapanaki said, bit advanced, but you could define an input source and an output node in the analysis and it can tell you the exact input referred noise over the full bandwidth, even your OPAmp has a limited bandwidth or you are using it in a different connection (like an inverting amplifier with bigger gain than 1 for example).Last edited by frankrose; 6th January 2020 at 20:07.
"Try SCE to AUX." /John Aaron/
1 members found this post helpful.

6th January 2020, 22:08 #6
 Join Date
 Apr 2019
 Posts
 13
 Helped
 0 / 0
 Points
 197
 Level
 2
Re: Noise analysis for diff amp in Cadence
The simulation result of the noise analysis gives us the noise spectral density. How to choose the bandwidth so that to get (NSD * BW) to obtain value in volts(mostly in nv) or should I consider BW of the opamp or what do you mean by full bandwidth?
https://www.ti.com/lit/ds/sbos481d/sbos481d.pdf
In the above link, first one mentioned is normal noise spectral density (nv/sqrt(hz) for 1KHz. I couldn't understand the second term? Can you explain what is that.
Also how to run simulation to find offset voltage?
thanks

7th January 2020, 01:40 #7
 Join Date
 Nov 2001
 Location
 US
 Posts
 888
 Helped
 307 / 307
 Points
 10,241
 Level
 24
Re: Noise analysis for diff amp in Cadence
You probably know that any amplifier can be characterized by two equivalent noise sources at the input  a voltage noise source and a current noise source. Voltage source alone is good for low or 0 source resistance. Current noise source alone is good for very big or infinite source resistance. Both of them are needed for any source resistance in between. My guess is that Fig2 and Fig.3 show those equivalent noise sources. Fig.6 shows the flicker noise in time domain,because it says this is for frequency range from 0.1Hz to 10Hz. I assume this is input voltage noise. If you integrate the flicker noise in that frequency range you get 18nV which should be considered as the standard deviation of the flicker noise process. +/3 sigma is +/ 54nV. Form the variations in fig.6 you have something like +50nv and 30nV variation.
For NSD*BW you can use the integrate function in spectre calculator and integrate the NSD for the BW you want. Just a reminder, when you integrate you have to use the PSD i.e. V^2/Hz and not the voltage spectral density.

Advertisement

7th January 2020, 19:15 #8
 Join Date
 Nov 2013
 Posts
 747
 Helped
 205 / 205
 Points
 5,094
 Level
 16
Re: Noise analysis for diff amp in Cadence
BW is the desired signal frequency range. It can be the OPAmp bandwidth, or if you have any filter with lower bandwidth use that value. I guess if you have low noise amplifier you want to amplify a DC, or AC signal, with low noise. To reduce noise it is highly recommended to use the minimal necessary bandwidth by a filter.
How to find offset? Run montecarlo mismatch simulation with DC analysis. Plenty of tutorials available via browser, if you arrived to a special problem then come back to talk about it, but use browser first, google is your friend too."Try SCE to AUX." /John Aaron/
+ Post New Thread
Please login