I am using an OPA846 as a TIA to detect a 38 MHz pulse train with 12 ps pulse duration. The photodiode is a Lumentum EPM605 (2 GHz bandwidth, 0.75 pF capacitance). The circuit has been implemented on a PCB, and the schematic is shown below. Including the photodiode capacitance (0.75 pF) and the OPA846 input capacitance specified in the datasheet (3.8 pF), the total input capacitance is approximately 4.55 pF.



Initially, the feedback network consisted of a 510 Ω resistor and a 0.3 pF capacitor. However, I observed oscillations at the output (osicllates at 300-500MHz). I then increased the feedback capacitor to 1 pF, but the oscillation is still there. After changing back to 0.3 pF, the oscillation still remained, although I noticed that the current drawn from the power supply decreased from 67 mA to 61 mA. I am unsure whether this reduction in current indicates that the oscillation has been partially reduced, since I have read that oscillating circuits can exhibit increased supply current.

The reason I reverted to 0.3 pF is that the OPA846 datasheet states that the device is stable for gains greater than 7. My understanding is that, in a TIA, this corresponds to the high-frequency noise gain, given approximately by

Noise gain ≈ 1 + Cin/Cf.

Therefore:

For Cf = 1 pF:

Noise gain ≈ 1 + 4.55/1 ≈ 5.6

For Cf = 0.3 pF:

Noise gain ≈ 1 + 4.55/0.3 ≈ 16.2

Based on this, I would expect the 0.3 pF case to be more stable. Please correct me if my understanding of the gain requirement is incorrect.

To investigate further, I performed a loop-gain analysis and evaluated different combinations of feedback resistor and capacitor values. I ran the AC transient and plot the ratio of open loop to noise gain to get the loop gain, and find the corresponding phase at which the loop gain intersects at 0dB gain. of The corresponding phase margins are shown in the attached figure.




According to the simulation, a feedback resistor of 4 kΩ together with a feedback capacitor of 0.5 pF gives a phase margin of approximately 45°, suggesting that this combination should provide adequate stability.

However, I have the following concern:

Since increasing the feedback resistor from 510 Ω to 4 kΩ increases the transimpedance gain by nearly a factor of eight, would this not cause the output voltage to become excessively large and potentially drive the OPA846 into saturation?

And another thing that I dont quite get is I tried to put these values to TI's PD circuit design tool and they gave me a different values of capacitor and resistor for the feedback network.




I would appreciate any comments or suggestions regarding whether this interpretation is correct and whether the 4 kΩ / 0.5 pF combination is a practical solution.

Thanks.

 

hi flying,
This is a rough LTSpice simulation of the Texas circuit, it shows a 'kink' at approx 600Mhz.?
E

Updated, using the actual listed Specs.

 

hi flyer,
This is your original circuit showing the output oscillation.
What signal output amplitude do you require on the finalised design?
E

 

hi flyer,
This is your original circuit showing the output oscillation.
What signal output amplitude do you require on the finalised design?
E
View attachment 368493

Hi Eric,

Thanks for that.

Somewhere between 0.5V-0.8V would be ideal, as the signal is set to go through another low pass filter and op amp in the next stage.

 

hi flyer,
This is the closest solution that I can see, using LTSpice.
Do you have a value for the voltage/current amplitude of the pulse signal from the actual PD.?
Also, the PD's internal impedance?
E

 

Of course this circuit can oscilate! Several conditions point that way! First, no supply bypass capacitors , nnext, no input resistor, so Rin=0, and gain =Rf/Ri, probably greater than intended. With the high gain, Any resistance between the suply common and the signal ground can provide positive feedback.
At leqast that is how it looks to me.

AND there is no output load shown. An outout load often improves stability.

 

Of course this circuit can oscilate! Several conditions point that way! First, no supply bypass capacitors , nnext, no input resistor, so Rin=0, and gain =Rf/Ri, probably greater than intended. With the high gain, Any resistance between the suply common and the signal ground can provide positive feedback.
At leqast that is how it looks to me.

AND there is no output load shown. An outout load often improves stability.

Hi,

Thanks for the reply.

I should have note that there are bypass 0.1uF capacitors on the both supply pins, I forgot to mention that.

Regarding the input resistor, this opamp is configured as TIA and the gain is defined as the noise gain, which is 1+ Cin/Cd, the ratio of the input capacitance over the diode capacitance. At least this is what I understand after reading through TIA configs and the datasheet hence why there's no input resistor.

I might be wrong in my understanding and would greatly appreciate if you could point out my mistake here

 

Hi flying,
As we all know that on an LTS simulation power supply capacitors are not necessary.
Also, a TIA OPA does not have an actual input resistor.
The reference to a load resistor is misleading,
My best advice is to disregard post #6 as misinformed.

Do you have this information to post?
Do you have a value for the voltage/current amplitude of the pulse signal from the actual PD.?
Also, the PD's internal impedance?
E

Useful link:
https://www.analog.com/en/resources...-transimpedance-amplifier-circuit-design.html

 

You all take into account the input capacity of the operational amplifier twice. The Spice model already has it. So I modeled the scheme in QSPICE. I also used it to build a photodiode model. I came to the conclusion that the feedback resistance is fine with 4 kOhms. Keep in mind that increasing the incident light power after 10 mW leads to non-linearity.

 

Hi Alex,
Where do I include the input capacity of the OPA twice in my simulations, when using this example circuit?

E

 

Where do I include the input capacity of the OPA twice in my simulations, when using this example circuit?

The photodiode has CPD = 0.7pF (0.6pF @ -5V bias). The actual op amp (OPA846) contributes another 3.8pF (Cdm + Ccm) which the TI PD design tool already accounts for, no need to consider it twice by making CPD = 4.5pF.

 

Calculation of the input capacity of the operational amplifier: