OPA847 TIA excessive input capacitance?

Hello,

  I would like to simulate the circuit in TINA Spice to see what kind of noise the models predict and see how it correlates with your measurement. What is the photo-diode capacitance? Could you also please share your test results?

Thanks,

Samir

Hi Samir,

thanks for taking the time to look at my problem. The photodiode will have <1pF capacitance, much less than the input capacitance of the OPA847 (around 4pF). For the noise tests I left it out completely - all there is to the circuit is the OPA847, a feedback resistor Rf and a Cf approx 0.2-0.3pF (including parasitic). 

For Rf=5kOhm the noise measurement gives output voltage noise 28nV/sqrt(Hz) at 10MHz, rising to 64nV/sqrt(Hz) at 95MHz. The 10MHz value corresponds to 5.6pA/sqrt(Hz) equivalent input current noise, far too much. For comparison, the same circuit with LMH6624 achieves 3.4pA/sqrt(Hz) at 10MHz. 

I also tried Rf=10kOhm and Cf=0.2-0.3pF - this gives 53nV/sqrt(Hz) at 10MHz (5.3pA/sqrt(Hz)), rising to  82nV/sqrt(Hz) (8.2pA/sqrt(Hz)) at 55MHz. 

Regards, Jochen 

Hello Jochen,

   Your measurements assume that all the noise is purely current noise. There is a significant proportion of the noise that is coming from the feedback resistor. Please see the attached link for how to calculate the noise from individual components in a transimpedance amplifier. This could explain why the noise is so much higher with a 10K resistor.

http://www.ti.com/lit/an/sboa122/sboa122.pdf

At the end of the app. note it shows a comparison of using a JFET input amplifier like the OPA656/OPA657 vs a bipolar amplifier OPA846/OPA847. According to the calculations, with a 5K feedback resistor a JFET amplifier could meet your needs better (from a noise perspective)

I ran a TINA simulation with your setup of 5K Rf and assumed around 0.5pF Cf(your feedback cap and parasitics). I made a couple of observations:

1. There is a bit of peaking in the noise curve. The location of the peak could shift easily due to board parasitics. Try using 0402 size components whereever possible to minimize parasitics.

2. Have you calibrated out the noise from your spectrum analyzer?

3. I did some simulations in TINA to check the stability of the OPA847 with your configuration and I noticed that the amplifier doesnt seem to be properly compensated with enough phase margin. By adding a Cdiode of 10pF, it looks like you have some more phase margin..of course this is going to kill your bandwidth a little bit. It comes to around 80MHz. Will this suffice for your application? One comment here is that there seems to be some problem with the model and the numbers arent always adding up.

My measurements:

In the past I have done some measurements on the OPA847 with a 10pF diode cap, 130Ohm series resistor, 0.5pF feedback cap and 1kOhm feedback resistor. I got an output referred noise of 5.9nV/rtHz which is pretty close to simulations. One disclaimer, at higher frequencies, (>500 MHz) the noise did get worse than simulation (about 30% error). Also, with my setup and 100Mhz I measure pretty close to simulation. Again the caveat here is that there is peaking in the noise curve. This kind of non-linearity can easily cause inaccuracies in real world measurements because of extraneoous parasitics.

 Let me know your thoughts/comments.

Samir

Hi Samir,

thanks for your input.

I've had a look at the document you linked to. I believe the comparison between FET and bipolar was done for significantly lower bandwidths than I'm aiming at, hence e_n is less critical and the lower i_n of a FET is beneficial. I think for my case bipolar is still the preferred choice. A 10k Rf will lead to higher noise than 5k, but the resistor's noise is contribution itself is only 12nV/rtHz, less than op-amp current noise multiplied by Rf. This should not be the root of the problem.

 Responding to your points,

1. I use 0603 parts in the the feedback branch and they are located directly below the op-amp (SOIC package). The board is a simple double layer 1.6mm thick. Parasitic capacitance should be less than 0.2pF - the fact that an LMH6624 works with the same board demonstrates that.

2. I use a low-noise pre-amplifier, and have checked that both the amplifiers noise and the spectrum analyser noise floor are far below what I measure with the TIA.

3. I've taken more measurements with an additional 8pF capacitor across the input (C_d). With an otherwise identical circuit, this shifts the noise peak from 95MHz to 75MHz and the peak is 3-4dB higher. The only way I have found to model this behaviour consistently is to assume about 12pF op-amp input capacitance - at least 3x of what it should be according to the datasheet.  

It could be that with a diode capacitance as low as 1pF, the high frequency gain of the om-amp is just not high enough to make it properly stable. What puzzles me though is that the datasheet for the OPA847 actually recommends a TIA circuit (figure 3 in "Applications information") with very similar parameters to my design, which claims a bandwidth of 100MHz and around 3.0pA/rtHz equivalent input current noise. I wonder if this has ever been checked with a real circuit, or in a simulation incorporating the actual open-loop characteristics of the amplifier (rather than the simple GBW model leading to equation 1)? 

For now I'll probably stick to the LMH6624 which works well. Maybe I was somehow unlucky with the particular batch of op-amps I received. 

Again, thanks for your thoughts!

Regards, Jochen