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.

OPA858: AC coupled OPA858 non-inverting amplifier shows instable behaviour

Part Number: OPA858
Other Parts Discussed in Thread: OPA818


I want to setup an AC-coupled noninverting amplifier based on the OPA858 operating from a single 5V supply with an overall passband gain of 76V/V (37,6dB) and a minimum bandwidth of fCT = 30kHz. The schematic is shown below. Unfortunately the circuit is unstable and oscillates with a frequency of around 80MHz. I am quite unexperienced with such kind of circuits so any help would be much appriciated. How can i simulate the open loop in TINA to investigate the phase margin for that case?



  • Morning Olaf, 

    Nothing seems amiss here - however, what exactly is your load? 

  • Hello Michael,

    Thanks again for you excellent support. The load is a combination of 100kR to ground and another OPA858 (1GR + 0.82pF).

    I tried to simulate the open loop to inspect the phase margin like shown below. It looks to me like the phase margin is about 60 degree.

  • Hi Olaf,

    May I see the physical layout?


  • Hi,

    Of course! Please find the relevant section as image below and the the gerber files attached.

  • Morning Olaf, 

    Here are some physical things to try, isolate the V+ and Out pins with series 20ohms right at the pins if possible, and add 100pF on top of your large caps to move the self resonance up in frequency, 

  • Hello,

    We have added the additional caps but however the output is still oscillating. I will design a dedicated test circuit to the next PCB revision for easier debugging. Maybe there is an error with my design? I am using 100nF and 6.8uF for VCC decoupling. Could that be an issue?

  • Hi Olaf,

     Is ground only on the top layer?



  • I think you need those series 20ohms if you can tack those in to test

  • Hi Olaf,

    yes, everything looks good in the simulation...

    ...until real world parasitics are added:


    What is feeding the OPA858? I ask, because, if it's a low frequency OPAmp, the output impedance at arround 80MHz and above could also appear high ohmically, or at least high ohmically enough to make the OPA858 oscillate.

    Later more...


  • Here still some snap shots from the GERBER viewer:


  • Hi Sam,

    There is a dedicated inner ground layer and the outer layers are filled with ground. The feedback path of the OPA858 is marked by a keepout area for all layers.


  • Hi Michael,

    Yes, it seems that i forgot those (isolation?) resistors. I will add them in the next revision.


  • Hi Kai,

    My "ideal" simulation is looking the same. I have added some parasitics as well but the phase margin never dropped that far. Guess that i have added them at the wrong position. However, wouldn't C8 mean that the traces of IN+ and OUT are near to each other and form a tiny cap? The input signal itself is "generated" by a OPA818 TIA stage which is attenuated by a HMC542BLP4E. For testing we are directly feeding a signal generated by a NI Vector Signal Transmitter into the OPA858 amplifier.

    And regarding your annotations to the gerber files, the OPA858 data sheet (see below) recommends to remove the power and ground planes only around pin 1 and 2 which is what i did with the first OPA858 (U2). Is it clever to enlarge this area like i did with U3?


  • Hi Olaf,

    there's quite a lot to say. Let's start:

    1. The layout recommendation in figure 64 is not quite right. The ground plane remove should not so much take place under the output pin of OPA858 but all the more under the -input pin and the associated terminals of feedback components. The EVM has this done properly:

    OPA858 Op Amp EVM User's Guide

    2. As being a 5.5GHz OPAmp you need to consequently apply HF design practises. This especially means to use supply voltage filtering by the help of series resistances or ferrite beads. Apply this for each single OPAmp and each single supply voltage. Put the series resistors and/or ferrite beads closest to the decoupling caps which themselves should sit closest to the supply pins of OPAmps. This alone could already do the trick and prevent oscillations.

    By the way, I always use PI filters for this purpose. When doing so there's no need for an extra power supply plane.

    3. Yes, move the supply copper trace away from the OPAmp so that it no longer runs directly under the OPAmp. The way you have routed it allows direct capacitive feedback and results in instability.

    4. Your board should have wayyyyyy more vias connecting the individual ground planes to each other. Concerning this matter the EVM of OPA858 is no good example of doing this! It should look more like this:

    This is important, because a single via shows a relevant inductance and introduces complex impedances into the circuit. Because of this "ground" is longer "ground" and loses all its advantages (no low impedance over the whole range of frequencies, no shielding effect, etc.)

    5. As Michael already said, you should almost always have a small resistance directly at the +input pin and the output pin of OPAmp. The first to dampen eventual input stage oscillations and the second to isolate capacitive loads.

    6. At 100MHz and above a resistor doesn't look like a resistor any longer, but more like a cap of 100...300fF.

    An example: At 100MHz your 100k feedback resistor can show an impedance of terrible

    1/2/pi/100MHz/200fF = 8k Scream

    This is one tenth of your expected 100k Scream

    So your circuit looks totally different at high frequencies than your schematic.

    The one and only remedy is to drastically decrease all involved resistor values. A few kOhms might still be acceptable, but nothing in the 100kOhm range or even above. The lower the better!!!


  • Hi Olaf,

    Apologies for the delayed response. I think Michael and Kai have both made very good points here regarding your input/output and device power. The reason I asked about your ground configuration is that there are no adjacent ground vias to the devices, and U3 especially has a long path to system ground. A good rule is to just place a via for every ground pad at the very least. I would also make those 5V supply lines on the top layer wider. This package pinout will also allow for you to stack the bypass caps directly across the device power and ground if you rotate C9 and C6 and place them right up against the amps, and C7 , C10 similarly to the left of those. Another option is to make a local 5V power pour for this section of the board, since I don't see anything else routed on that layer.