Because of the Thanksgiving holiday in the U.S., TI E2E design support forum responses may be delayed the week of Nov. 21. Thank you for your patience.

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.

High gain ac simulation OPA349

Other Parts Discussed in Thread: OPA349

I have ac simulation of OPA349 in inverting configuration that has large feedback resistor (<10K).  With very large gains, the simulation shows a drastic drop in low freq gain (> 1M no gain at all).  Does anyone know what might be wrong with the circuit setup and/or the simulation model.  I have tried impulse response and the same circuit seems to work AOK.  Just problems with looking at the closed loop bandwidth for high gains.  The TINA simulation file is attached.  

  • Perry,

    Could you check the attachment? It doesn't ahow up on our end.



    John, i have tried to upload the circuit file again.  Perry

  • Perry,

    The gain of your circuit (80dB) is high enough that the model's input offset voltage is causing the output to go to the rail. If you run a DC bias point sim, you can see the output is almost at ground.

    I added a small (-612uV) DC offset to the signal source and that seemed to bring the DC output voltage to mid-rail. Running an AC response gave a gain curve with ~90dB max gain.

    The modified circuit is attached.


  • John,

    Your answer makes sense.  But the circuit you returned actually had a 2.5V offset connected to the output via a 1M resistor.  I did not see the small DC offset you referred to in your email.   I did run the AC simulation and got good results.  However, as I dropped the power supply from 5V to 4.6 (and below) I started seeing the gain die off.  I did adjust the offset voltages to 1/2 the power supply voltage in each case.  I have attached the 4.6V case.  This device is good down to 1.8V, it would seem that dropping the power supply voltage in the operating range would not effect the gain of the circuit.  Thanks again for your help understanding what is going on with the simulation.

    Using this op amp with large Rf and no Ri is commonly used in transimpedance amplifiers for optical detectors.  Are there problems that can arise form using too large an Rf?

  • Perry,

    The -612uV input offset was implemented in the DC level of the signal source Vin. The input DC source (Vdc) was left unchanged. This seemed easier than applying the offset by decreasing the 2.5V Vdc source by 612uV.
    Sorry for the confusion.
    The other half-supply offsets are left as you made them. I did change the output load to 1M, but it can probably be anything, within the limits set in the device data sheet.

    It can be normal for an op amp's input offset to vary with the power supplies.
    You can see this in two ways:

    1. Some device data sheets show a plot of the typical VOS vesus power supplies.
    2. The PSRR parameter specifies the shift in VOS versus a shift in the device power supplies.

    The attached schematic is the same as your last one, except the DC offset for the signal source Vin has been changed from -612uV to -684uV. This moves the quiscent output voltage from almost ground to about half supply. The gain pops back up to about 90dB.

    The issues you are seeing have more to do with the gain of the circuit rather than the actual value of RF. That being said, RF can be critical for some kinds of amplifiers, like some high speed op amps. Its best to check with the apps engineers who support the devices. You can reach them through the E2E Amplifier Forum, as well as the forums specific for the kind of device you're interested in, like Precision or High Speed.