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.

  • Resolved

TINA/Spice/OPA549-HIREL: Composite amplifier for OPA549-HiRel using OPA192 with improved DC accuracy and drift

Intellectual 575 points

Replies: 53

Views: 1662

Part Number: OPA549-HIREL

Tool/software: TINA-TI or Spice Models

Hi, I want to build a composite amplifier using OPA192 + OPA549-HiRel with improved dc accuracy and drift performance. Could you please help me with this circuit? I build one using TI-Tina, but there are simulation convergence errors, I also do not know whether it can improve the dc and temperature drift performances or not.


  • Hi,
    The applications engineer supporting these devices will respond to your inquiry upon his return to the office on Friday.
    Thank you.
  • Hi Byliu,

    Can you please describe the issues you are having? When I run the file you have provided I do not run into convergence issues.

    Composite amplifiers are generally used when you need an amplifier with good dc precision and either strong drive capability or good AC performance as well. Because the loop of the first amplifier is closed around the output of the second, the dc error arises entirely from the front amplifier. Thus your drift and dc performance will derive from OPA192 and your output drive capability from OPA549.

    The trick is in making sure that both amplifiers are stable. Since the OPA549 output is fed back to the OPA192 and subsequently to the non-inverting input of the OPA549, there are 2 feedback loops to contend with when conducting a stability analysis.

    For the OPA192, there is an amplifier with gain in the feedback loop, and this creates an unusual case where your feedback factor can be greater than one. You need to have a local feedback loop (cap from input to output) to compensate for this.

    If you simulate this circuit you will see that it is very unstable with excessive ringing on the output and ~8dB of gain peaking in the AC response.

    If you aren't very familiar with amplifier stability analysis, here are two presentations that go through various analysis techniques!

    3056.Solving Op Amp Stability 2015_TG.pptx

    3441.Dual FB Beta_plus and Beta_minus RevD.pptx




    Zak Kaye
    Precision Data Converter Applications

  • In reply to Zak Kaye:

    Thank you for your reply.

    I found that the simulation oscillates when the signal goes from positive to negative. I changed the first stage to a unit-gain follower, but the instability is still there. I found that this phenomenon is related to the Rload (R4). For example, if I change R4 to 20 Ohm or higher, the simulation is ok. If R4=5 Ohm or lower, the simulation went wrong.  So, I guess maybe it is related to the current limiting feature of OPA549?

    My concern is

    1. should I trust the simulation? If I fabricate such circuit, will it be unstable when R<5 Ohm and stable when R>10 Ohm?

    2. Will the choice of OPA192 improves the overall DC performances? We want to design a high drive buffer for a DC motor, the RMS current requirement is 3A and the peak current might be 5A or more. We choose OPA549 and a 18/20 bit precision DAC for our application. In the datasheet of OPA549-HiRel, the voltage offset and the voltage offset temperature drift is too high (also the voltage noise) for a 18/20 bit DAC. We want to build a composite amplifier to mitigate the DC errors, especially the temperature drift. Your helps are greatly appreciated.



  • In reply to byliu:

    Hello all, thanks for the TINA file, that makes it trivial to set up and run a LG phase margin sim,

    This circuit is well known but hazardous as all get out. Essentially you have injected a huge prop delay inside the loop. At an IC design level whenever we want to introduce a high power output stage (see the THS3491) we get into a lot of prop delay issues that hurt phase margin - same here.

    Anyway, couple of key points

    1. The power stage needs to be powered up and stable before the input stage comes up, I might tie a 1k to ground on the V+ input of the OPA549 to give it a reference point powering up. If not, you get into an odd stability issue we used to call motorboating as the whole thing tries to find a DC operating point. I often run an RC pole on the supplies from the output stage back to the input stage to enforce this.

    2. Your current circuit is way unstable - couple of ways to fix this, but the easiest comes along with running inverting - is that an option???????

    Composite ckt with OPA549 and OPA192.docx

    Original LG sim.TSC

    Michael Steffes

  • In reply to Michael Steffes:

    Thank you (I still could not open your tsc file, but the drawings in the word file is fine, can you open my tsc?).

    1. Inverting is OK for me. I modify the circuit, add R10 to the inverting input, add R6 to the non-inverting port of OPA192. Add R11 of non-inverting port of OPA549 to ground, add a snubber circuit at the output. This circuit works when R4=11 or more, but it get unstable (in the tina simulation) when I changed R4 to 10 Ohm or less, i.e., 4 Ohm. I do not know where this instability comes from when R4=4 Ohm, is it because of the spice model of OPA549? is it about the architecture of Tina? or it is unstable in the final PCB board?

    2. Should I give up the composite amplifier architecture? I am really not good at analyzing the stability of OPA192 + OPA549. And what's more, if I build this PCB, will it get the desired dc performance of OPA192 (low voltage offset, low voltage temperature drift) and the high current driving capability of OPA549?


  • In reply to byliu:

    Hi Byliu,

    this scheme would work:



  • In reply to kai klaas69:

    This would be the step response:

    And this would be the frequency resposne:


  • In reply to kai klaas69:

    And here comes the phase stability analysis:



  • In reply to kai klaas69:

    Thanks! your circuit works! BTW, the current limiting feature of OPA549 also works if I change R3 to 4.99k and R4 to 1 Ohm.

    1, I found that you change R2, R7 to 10k and add a compensation C3 to OPA192, which one plays a vital role in this circuit? I found that C3 is important in this circuit, If I removed it or change it to a smaller value, this circuit fails.

    2, If I changed R2=1k R7=1k, How to calculate the response of this circuit?

    3, If I build this PCB out (I am currently design one using KiCAD), will it be stable and will I get the desired dc performance?
  • In reply to kai klaas69:

    Thank you !!

    I am going to build one. How could I test the DC performance (my primary concern is the temperature drift) in the final PCB?

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.