Stats

  • Locked Locked
  • Replies 10
  • Subscribers 126
  • Views 16830
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Integrated noise for opamp is not converged.

Jacki

Hello,

I am simulating a traditional two-stage operational amplifier with miller and lead compensation. The DC gain is 70dB, and gain bandwidth is 580MHz, with the phase margin 115 deg.

After I achieve the specifications above, I start to simulate the integrated noise. The opamp is fully differential, the load is pure capacitor in each branch with the value 350fF. According to the first-order filter theory, the final integrated noise should be KT/C. For each branch, the integrated noise is 1.08e-4 volt.

When I use ADE L/print/noise summary to plot the integrated noise, the results are as follows,
When integrated band is from 1KHz to 10MHz,
total summarized noise = 0.132026V, total input referred noise = 6.20415e-5V.

When integrated band is from 1KHz to 100MHz,
total summarized noise = 0.132042V, total input referred noise = 1.10047e-4V. According to the simulation results, it seems the total summarized noise is converged, and the input referred noise is increasing when the band is higher (not converged).

When I show this results to my boss, he told me how the total summarized noise can be so large, it is around 132mV!!! For the opamp, the noise cannot be so high. Compared with the value of KT/C, it seems the integrated noise is huge.

    1. My first question, why the integrated noise of the opamp is so large. How does spectre calculate the input referred noise?

According to Ken's view from designer guide "the input-referred noise is the ratio of the output noise to the gain". When the integrated band is larger, the gain of the opamp is dropping, maybe it is the reason why the input referred noise becomes worse as integrated band is higher. But my boss told me when the band is larger, the gain of the opamp is dropping, the noise of the opamp at higher frequency is dropping as well, therefore the input referred noise should be converged too even for the infinite integrated band.

    2. My second question is how to get the converged integrated input referred noise if the integrated band is going to infinite. How Cadence Spectre calculate the input referred noise in ADE L->results->print->noise summary?

  
    I am confused now. Anybody can tell me give me some help. Thanks!

Parents
  • Andrew Beckett

    Spectre (as do all circuit simulators) compute the total output noise - that's the primary output. They do this by adding a number of noise sources around each device, where the magnitude of the noise at the source is dependent upon the size/value of the device and the operating point (depending on the type of noise). It also computes the transfer function from this noise source to the output of the circuit. It multiplies the noise at the source by this transfer function, and then sums up the total noise power at the output of the circuit. This can then be represented in either V^2/Hz or V/sqrt(Hz). If you plot the waveform representing the noise at the output, you'll get one of these - noise versus frequency. You can then integrated it over a band, e.g. using the rmsNoise function in the calculator, or using the noise summary form - it does a straightforward integration to give the noise in a certain bandwidth.

    Input referred noise is computed by simply dividing the total output noise by the transfer function from the designated input source to the output. If there's more gain, there's less input referred noise (at a particular frequency) and vice versa. So whether it "converges" is dependent upon the bandwidth of the circuit. Note that input referred noise is not terribly meaningful - it's only useful with knowledge of the transfer function of the circuit - and is just a way of representing the output noise in a different (and sometimes more convenient) manner to aid hand calculations and noise budgeting in your design.

    Now, I can't comment on your circuit (without having seen it), but the first step would be to look at the noise summary in ADE (Results->Print->Noise Summary) which allows you to filter the devices and identify which are causing the biggest noise contribution. It's very unlikely that it is wrong unless you have some fundamental modelling error or the devices are not the size you thought they were. Note that all the noise contributors are in terms of the output referred noise they produce - so you can compare their impact.

    Regards,

    Andrew.

Reply
  • Andrew Beckett

    Spectre (as do all circuit simulators) compute the total output noise - that's the primary output. They do this by adding a number of noise sources around each device, where the magnitude of the noise at the source is dependent upon the size/value of the device and the operating point (depending on the type of noise). It also computes the transfer function from this noise source to the output of the circuit. It multiplies the noise at the source by this transfer function, and then sums up the total noise power at the output of the circuit. This can then be represented in either V^2/Hz or V/sqrt(Hz). If you plot the waveform representing the noise at the output, you'll get one of these - noise versus frequency. You can then integrated it over a band, e.g. using the rmsNoise function in the calculator, or using the noise summary form - it does a straightforward integration to give the noise in a certain bandwidth.

    Input referred noise is computed by simply dividing the total output noise by the transfer function from the designated input source to the output. If there's more gain, there's less input referred noise (at a particular frequency) and vice versa. So whether it "converges" is dependent upon the bandwidth of the circuit. Note that input referred noise is not terribly meaningful - it's only useful with knowledge of the transfer function of the circuit - and is just a way of representing the output noise in a different (and sometimes more convenient) manner to aid hand calculations and noise budgeting in your design.

    Now, I can't comment on your circuit (without having seen it), but the first step would be to look at the noise summary in ADE (Results->Print->Noise Summary) which allows you to filter the devices and identify which are causing the biggest noise contribution. It's very unlikely that it is wrong unless you have some fundamental modelling error or the devices are not the size you thought they were. Note that all the noise contributors are in terms of the output referred noise they produce - so you can compare their impact.

    Regards,

    Andrew.

Children
No Data

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.