• State Resolved
  • Locked Locked
  • Replies 4 replies
  • Subscribers 38 subscribers
  • Views 1122 views
  • Users 0 members are here
Support feedback
Options
Options
Related

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/OPA627: TINA/Spice/OPA627:

Jubayer Jalil
Prodigy 200 points
Part Number: OPA627
Other Parts Discussed in Thread: TINA-TI,

Tool/software: TINA-TI or Spice Models

Hi All,

The attached circuit exhibit wrong noise analysis. Is this because of spice model of OPA627 or software limitation?

Kind regards

Jubayer

OPA627_Noise analysis.TSC

  • 0
    TI__Mastermind 40295 points

    Jubayer,

    It looks like the resistors are affecting the noise sim results.

    A second circuit was added to your TSC file. The revised file is attached to this thread.

    In the second circuit, the resistors were replaced by voltage-controlled current sources (VCCS).
    They act as equivalent resistances, but don't contribute noise to the circuit.

    A noise sim shows the input-referred noise for the  new circuit is 4.82 nV/rt(Hz), which is close to the voltage noise in the datasheet.
    The TINA plot is shown below.

    I hope this helps. Please let me know if you have any questions.

    Regards,
    John

    OPA627_Noise analysis_revised.TSC

  • 0 in reply to John Miller - Sensing
    Prodigy 200 points
    Dear Mr. John,

    Thanks for your prompt response. However, I am looking for different solution!

    Actually I want to simulate the output noise analysis of the RC circuit coupled amplifier what I provided earlier without any modification and substituition of components.

    There few issues arises in the circuit which are given below:
    1. By hand calculation, this circuit's output noise voltage density is 452.64 nV/rtHz at 10KHz. But in simulation, it is found 169.17 nV/rtHz at 10KHz. Interestingly , this circuit's input noise voltage density is 232 nV/rtHz at 10KHz, which should not be higher than output noise volatge density! These discrepencies of input and output noise results are conatrdictory with theoritical analysis.

    2. Then, I replaced two pF range capacitors by two nF capacitors and recalculated circuit's output noise volatge density and estimated circuit's output noise volatge density of 20.65 nV/rtHz at 10KHz. After simulating the modified circuit, we found the circuit's output noise volatge density of 20.72 nV/rtHz at 10KHz. Hence, the simulation result shows the good agreement with the theoretical/hand calculation analysis.

    3. Shunt resistor at input, gain and feedback resistors are kept unchanged for above mentioned simulations.

    Now my questions are:
    1. Why does the software comply theoritical noise analysis while coupling and shunt capacitors are selected in nano F range instead of picoF range?
    2. Is this the limitation of TINA software or Spice model of TI for pico farad range capacitor?

    I hope I have explained the problem now clearly!

    Looking forward to hearing from you soon.

    Regards

    Jubayer
  • 0 in reply to Jubayer Jalil
    TI__Mastermind 40295 points

    Jubayer,

    An AC sim shows the forward gain in the pass-band is -2.77dB, so it makes sense the input-referred noise is larger than the output noise.
    With the reported output noise (169nV/rt(Hz)) and gain, the corresponding input noise should be 169*(10^(2.77/20)) = 232 NV/rt(Hz).
    So the TINA sim seems to be working fine.

    The simulation results are different from the hand calculations because of the input capacitance of the op amp (model).
    The total external capacitance at the noninverting pin to ground is 4pF. Simulations show internal capacitance of the noninverting input is about 7.1pF which is consistent with the data sheet value of 7pF.

    My hand calculations show that with 4pF of total capacitance, you get 442nV/rt(Hz) of output noise for your circuit, which is close to your result. 
    If you take into account the device/model input capacitance of 7pF and add that to the 4pF of external capacitance, the calculated output noise drops to 164 nV/rt(Hz), which is pretty close to the 169 NV/rt(Hz) sim results.

    When you increase the external capacitance to the nF range, the device/model input capacitance becomes negligible and the calculations need only take the external capacitance into account. That's why your calculated results for 2nF caps agrees with the simulations.

    So it looks like the OPA627 model aligns pretty well with the data sheet specs.
    The TINA noise simulation seems to agree pretty well with theoretical calculations, so it seems to be okay as well.

    I hope this helps.
    Please let me know if you have any more questions.

    Regards,
    John

  • 0 in reply to John Miller - Sensing
    Prodigy 200 points

    Dear Mr. John,

    I would like to thank you for your explanation and useful solution.

    Now, to verify the output noise of the attahced new cirucit (OPA627 in inverting mode), sim result shows output noise of 61 nV/rt(Hz) at 10KHz. By hand calculation, I found 64.72 nV/rt(Hz) at 10KHz considering only two external capacitance of 2 pF.  Now, for this configuartion, if I take into account the device/model input capacitance of 15pF (differential i/p cap. + CM i/p Cap from datasheet) in addition with two external capacitors , my hand calculation shows 68.4 nV/rt(Hz) at 10KHz exhibiting significant difference from the hand calculation.

    Now my questions is:

    1. Why does the hand calculation of 64.72 nV/rt(Hz) at 10KHz show  the good agreement with the simulation result of 61 nV/rt(Hz) at 10KHz even though the device/model input capacitance of 15pF (differential i/p cap. + CM i/p Cap) is disregarded in the caluclation?

    Look forward to hearing fro you soon.

    Kind regards

    Jubayer

    Inverting mode.TSC