Other Parts Discussed in Post: OPA211

SPICE is a useful tool to help check for potential circuit stability problems. Here is one simple way to do it:

Figure 1 shows a non-inverting amplifier using the OPA211 with a couple of minor variations that are common in many applications. R3-C1 is an input filter. R4 is an output resistor to protect against abuse when connected to the outside world. CL models a five-foot cable.

Checking the response to a small-signal step function or square wave is the quickest and easiest way to look for possible stability problems. Figure 2 shows the simulation circuit. Notice that the input terminal is connected to ground and the input test signal is connected directly to the non-inverting input. The input filter would slow the input edge of a step function. If you want to know how a bell rings, hit it with a hammer, not a rubber mallet.

The response is probed at the output of the op amp, not just the Vout node of the circuit. R4 and CL filter the output response so that Vout will not show the true overshoot of the op amp. To check stability, we want to know what the op amp is doing.

Notice that the amplitude of the applied step is 1mV (creating a 4mV step at the output). We want the small-signal step response. A large input step that induces slewing will have less overshoot and will not clearly reveal potential instability.

The simulation shows approximately 27% overshoot at the op amp’s output, too much to be comfortable that this circuit will be stable under all conditions.  Assuming a second-order stability system, this would indicate a phase margin of approximately 38°. Also, notice that the frequency response shows considerable amplitude peaking, another sign of potential instability. The peaking occurs at 14MHz, the inverse of the period of the ringing in the time domain. A commonly accepted guideline for reasonable stability is a phase margin of 45° (or greater) which translates to 20% (or less) overshoot.

There are fancier analyses that can be done with SPICE—Bode analysis by breaking the loop, finding phase and gain margins. But for most relatively simple circuits (feedback loop involving one op amp) this approach is a very good indicator of possible problems. Of course, any SPICE simulation relies on the accuracy of the op amp’s macro model. Our best SPICE models are excellent but not perfect. Furthermore, circuit variation, non-ideal components, circuit board layout parasitics, poor supply bypassing—all can affect the circuit. That’s why you build it, test it, compare with simulation and optimize. SPICE is a useful tool, valuable but not sufficient.

How would you improve the stability of this circuit? Comments welcome below below…

Thanks for reading,

Bruce        thesignal@list.ti.com


          Simulations are performed with the free version of TINA-TI.

          Index to all The Signal blogs.

  • If I see that right, all this measures the input to output transfer. I do not see the inner loop, more like a black box.

    The feedback loop is closed by the divider R1/R2. When SPICE is doing an AC analysis, it applies short circuits to inductors and open circuit to capacitors. So inserting a very large inductor in between the OpAmp resistive divider and R2 would still result in a good operating point (the ESR of the inductor should be a few Ohms). Now I have a node - Inductor/R2 - which I can connect an AC source to with a very large capacitor value. This source would be blanked out at operating point calculation due to the capacitor.

    Now you can set the AC value of that source to '1' - a theoretical calculation will take place, which does not know saturation. With '1' at the AC source, the Opamp output node is the inner feedback loop. (Vtest=0!)

    This is how I would do such a simulation to have an information about stability - So far I did that with OpAmp/MOSFET current sources. My experience is that many sources looked critical but stable, but in reality they were not stable... I had to apply a compensation and with much margin in the loop the simulation did a good job.

    What you think aboit that?

  • I just accessed the files Time Sobering placed in his profile, I had no problems at all downloading them.  The Harris Ap Note looks quite good.  Thanks Tim!

  • Clyde...I put the files in my profile.  I'm assuming you can access them...never done that before.


  • My suggestion for improving the stability and for the same frequency bandwidth of this circuit is shunting the R2 resistor with 27pF capacitor and don't use the input R3, C1 filter.

  • I have downloaded both referenced app notes and bot come as as (secured) pdf files which will not let me print or save them.

    Any Iideas?