This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

opa657 noise from TINA simulation

Other Parts Discussed in Thread: OPA657, OPA277, TINA-TI, OPA656

I have a question regarding to the OPA657 noise from TINA device model. Attached is the schematic and the output noise plot of the circuit from the simulation. the approximation I did is to measure the noise 41nv at 1MHz  3db increase (84nv) is then close to 100MHz. but based on the formula the zero is 1/(2PI*Rf*Cs). The input capacitance of  opa657 will be less than 2pf. The data sheet shows 5.6pf. I also notice subcircuit inside of opa657 is opa277. Anything wrong on my thinking.

opa657_opa695 noise.docx

  • Hi Jeff,

    I think your issue is that the OPA657 1st stage has peaking / oscillations the way you've configured the circuit.

    The 1pF across your input current source is being "seen" by the 5k feedback resistor and that's causing enough phase shift to cause sharp gain peaking. I've increased the 10ohm series resistance (to 500ohm) and I've adjusted the value of the compensation cap across RF to get a much flatter response, as shown below:

    Here is the TINA-TI circuit:

    /cfs-file/__key/communityserver-discussions-components-files/14/4617.OPA657-Compensation-E2E-Hooman-3_5F00_18_5F00_15.TSC

    Please give this modified circuit a try and see how noise simulation works now.

    Regards,

    Hooman

  • Hello Jeff,

      The OPA657 input capacitance has been incorrectly modeled. I realized this issue a little while back and informed the modeling team about this but they are quite backed up and havent had a chance to get to this as yet.

    To see the fact that the capacitance is not modeled correctly, please see attached sim. With 1K resistance and 4.5pF capacitance, I would expect to see a pole at 36MHz, which we dont.

    Can you please let me know the potential application and I can see if I can fudge a model to give better results.

    -Samir

    OPA657_ZCM.TSC

  • good test. Unfortunately we are a small company. I will guess the high end of qty will be hundreds.

  • Since the model of OPA657 does not accurately model the input capacitance. Does it matter the input resistance?

    Can I correct model by adding a external capacitor? I feel the model capacitance is less than it should.

    The 10 ohm resistor is part of model of photodiode.  Do you have photodiode model in the Tina library?

    another subject is the noise peaking. It has shown on my board from 200MHZ-500MHZ. How can I remove the peaking noise?

  • Your solution to the OPA657 gain peaking problem raises the 300MHz NBW total noise by 2.5x, but this does not address the basic problem-- the OPA657 input capacitance was omitted from its macromodel. I pointed this out to TI over 5 years ago and it still has not been fixed.

    Until TI fixes this problem with the OPA657 model, a user must place the appropriate data sheet capacitance on the input pin of the TINA symbol to ground.

    It is a shame that such a good high speed FET op amp is so neglected by its manufacturer.

  • Hello Jeff,

      You can add an external capacitance to match up with the datasheet number. Also, the noise peak you are seeing in your test is from the amplifier itself and occurs at the 2nd pole in the Aol response. This can be removed by filtering prior to the ADC and also by adding filtering in the single to diff output stage.

    We do not have photodiode library in TINA. This will have to be created from the photodiode datasheet.

    We do have some Webench photodiode models. I am not quite sure how to use these models. I will direct your question to someone who might be able to help.

    http://www.ti.com/lsds/ti/analog/webench/sensors-photodiode.page

    -Samir

  • Jeff,

    We do not have photodiode models for TINA. However, we do have a tool that will help you design photo detector circuits, starting at the site that Samir has given you. After you click on his url you will see the following panel.

    From there you select photodiode in the next panel

    You will be presented with a table of photodiodes. In this table select the photodiode you are interested in and start you design.

    With your design, you will see a panel of options. Select the Operating Values, Performance panel, the second one from the top left.

    You can see calculated values that include the photodiode specificaitons and errors. Additionally, the circuit that is generated is calcualted using the input capacitance of the amplifiers and photodetector.

     

     

     

     

     

     

     

     

     

     

     

     

     

     

  • Does OPA657 model have any input common and differential mode capacitance? In other words, should I add 0.7 pf common mode and 4.5 pf differential mode capacitor externally as specified in the data sheet? OPA656 is very similar to OPA657, Does OPA656 have correct TINA model?

  • Can Webench do bode plot, noise analysis, transient response as TINA does?
  • Hello Jeff,
    I just checked the differential capacitance and it isnt modeled either, so you will have to add both the common mode and differential capacitance.
    The OPA656 seems to model around 0.94pF of common-mode capacitance and 0.6pF of differential capacitance, so while its a little closer it still doesnt match up with the datasheet.
    -Samir