• State Resolved
  • Locked Locked
  • Replies 3 replies
  • Answers 1 answer
  • Subscribers 41 subscribers
  • Views 2328 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

TINA/Spice/OPA365: Common mode power supply model response

Andrew Clark
Prodigy 20 points
Part Number: OPA365
Other Parts Discussed in Thread: TINA-TI,

Tool/software: TINA-TI or Spice Models

I am having a problem with the OPA365 in simulation (and possibly in a real life circuit) when dealing with a common mode step voltage on the power supply.

I put the model in LTSpice (sorry:-) and configured it for a unity gain buffer.  I put 1V relative to the opamp ground on the IN+ pin.  I then step the 4.096V supply from -25V to +25V (the differential voltage does not change but relative to the simulation ground it does step).  The input to the opamp stays at 1V relative to the opamp ground but has a small 1uV disturbance on it.  The output of the opamp responds with a decent size spike.

This response from op amp doesn't make sense to me.

Is this the expected response from the opamp or is this a modeling issue? Any insight would be appreciated.

I am using this part in a current sense circuit which is a diff amp and I am seeing a similar response from the real circuit.  I was surprised to see this response in a simple unity gain buffer sim but that's why i am questioning my knowledge of what is going on.

Thank you,

Andy

  • 0
    TI__Intellectual 820 points

    Hi Andy,

    Usually in model the measurement set-up that we use to test & report PSRR-p and PSRR-n,(may have common-mode error) is shown below,

     

    PSR-p/n curves have a nature of “High pass filter”, which means for easy understanding we can stay it acts as a kind of differentiator.

    So for simple sine/cosine perturbation of say 1KHz applied at VDD/VSS, its effect in output in the transient response can be hence calculated by the below approach:

    Amplitude at output: (Amplitude of input sine wave) * Attenuation factor at 1KHz(show in eg fig)

    Nature: Cosine if input is sine or vice-versa (as PSRR transfer curve acts like differentiator)

    Similarly for a non-sinusoidal disturbance, like the one you have used (square wave), will obviously appear in the output multiplied by the approx. attenuation factor, which can be found out by looking at the AC transfer function of the supply to Vout path.

    Also the nature will be Spike-like, as the differentiated version of pulse will is a spike like waveform and this will be superimposed on the actual output of the op-amp(resulting from Vin source).
    On an other note, it is always good to use the model in TINA as it is developed & tested in TINA.

  • 0 in reply to Ahana Ghosh
    Prodigy 20 points

    Ahana,

    Thank you for the quick response to my question.  It is good information and I have never had the need to worry about PSRR to this point in my career, but it makes sense.

    I interpret the information that you sent me to be a differential power supply noise applied to the opamp, and not a common mode noise relative to the "GND" node in the simulation.

    I think the problem is with the way the model is created which is giving me these funny results.  It seems that the model uses the SPICE "node 0" ground in the netlist, even though it is technically not connected to the part in my simulation. See picture below for location with "node 0" use.

    Does this make sense to you? I tried replacing the "node 0" with the V- "node 2" in the netlist with little hope of it working and of course it did not. Blind squirrel still looking for the nut :-)

    I think at this point I don't believe what the simulation is showing me.

    Thanks,

    Andy 

  • 0 in reply to Andrew Clark
    TI__Intellectual 820 points
    Hi Andy,

    I tried to convey that the nature of the LTSpice results(Vout,Agnd) which you had shared, is expected to happen at the output.
    Also about the differential power supply noise, I said that though ideally differential change should be applied at the supplies to measure PSRR, all tested & reported PSRR in models are done by applying the AC source on respective(VDD/VSS) source only.
    Moreover models are not exact replicas of real design architecture, their implementations are different and simple to capture the predominant features(reported in datasheet). Changing the 0V nodes will not help because in the model these components are intended not to change w.r.t supply & the PSRR is also modeled in this scenario.