• State Resolved
  • Locked Locked
  • Replies 3 replies
  • Answers 1 answer
  • Subscribers 48 subscribers
  • Views 261 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.

TL082: TL082 TINA simulation

Maggie Li
Intellectual 2220 points
Part Number: TL082

Tool/software:

Hi team,

In the following circuit, when Vin inputs a steady-state voltage or a sine wave, Vout will oscillate. I have suggested customers before that it is caused by the output capacitive load. Reducing C65 or increasing R24 can solve this problem.

I tried several different boards at that time and found that the parameter threshold that caused the oscillation was not fixed.

The problem now is that in the new designs, in order to confirm in advance whether it will cause output oscillation, I want to use simulation software such as TINA to analyze the rationality of the design parameters. However, I modeled the circuit parameters that will cause oscillation and input a -10V step signal, but it did not produce abnormal oscillation in the simulation results.

May I ask: 1. Why can't the following model reproduce the oscillation?

2. In addition to actual measurement, is there any simulation method that can reproduce the oscillation?

Thank you!

Regards,

Maggie

  • +1
    TI__Mastermind 29186 points

    Hey Maggie,

    There are a couple changes you can make to see the stability of this circuit, however the TL082 model is fairly outdated and may not accurately model stability.

    There is a newer version of this device, the TL082H, which I will use for this example.

    Stability is a small signal specification, and should be observed with a small-signal input.

    Taking this same circuit, and applying a 200mVpp step at the input (25.4mVpp step at the amplifier input), you can see there is quite a bit of overshoot (17mV of overshoot!)

    A better way to look at the stability of this circuit would be an AC open loop analysis. This can be done with the below circuit.

    This circuit only has 11 degrees of phase margin.

    However, it seems more than just the capacitive loading is at play here. Because your feedback resistor is 15kOhms, this interacts with the input capacitance to create a pole that reduces your phase margin. Keeping the ratios the same but lowering the value of this resistor yields a stable circuit.

    Best,
    Jerry

  • 0 in reply to Gerasimos Madalvanos
    TI__Intellectual 2220 points

    Hi Jerry,

    Today I do some simulation based on the circuit introduced by TI Precision Lab. But the result is 0.676 degrees of Phase Margin. 

    1. Why the result is different from yours?  What's the difference between these two models?

    2. Could you kindly send me your TINA file?

    Thank you so much!

    Regards,

    Maggie

  • 0 in reply to Maggie Li
    TI__Mastermind 29186 points

    Hey Maggie,

    The difference between the two circuits is how the loop is broken. Please see the following video for the explanation on how the different loop breaks influence analysis. https://www.ti.com/video/series/precision-labs/ti-precision-labs-op-amps.html?videoId=6341906518112

    TL082_Stability.TSC

    Please see my TINA file above.

    Best,
    Jerry