# Understanding opamp amplifier (simple) behavior - Having trouble understand basic opamp operation

I'm trying to understand the operation of opamps, especially how to amplify a voltage as illustrated in the images from a (for example) photoelement so these can be used a the following comparator.

One circuit I found and seems to be working in their model is here - circuit A from this webpage:
TI E2E forum - "OPA858: Amplifier for Fast and Standard output of Silicon Photomultipliers"

I'm currently using LTSpice (since that's what I'm most familiar with) but it doesn't supply the OPA858 or OPA656 opamps. Are there any comparable opamps I can use in LTspice? The aim is to understand and get a circuit that amplifies a simple small voltage to be processed by a comparator.

About the circuit (A) above, a small voltage to the opamp here (30mV) gives an output voltage of approx. 1V at V_amp. I've tried numerous times to do something similar with different opamps in LTSpice, but it doesn't work... I never get any amplification of the initial signal.

Can someone help me understand I could get a low voltage signal like the above (30mV) with an opamp amplified that in the end it can be used for further processing?

Here is my circuit in LTSpice:

Additionally, I tried another circuit which is in the opamps (LTC6268) datasheet - not working as well:

• Show your schematic what you are trying to get working. It might have important differences with the schematic you have based your circuit on. Commented Nov 6, 2022 at 13:43
• Hello everyone, thanks for taking the time to help me. I've added an image of the circuit I used last. There are already some problems with the input voltage - since it does not range from 0V to 30mV when connected to the opamp and the output is not amplified but just shifted upwards.
– ulix
Commented Nov 6, 2022 at 14:17

You need to understand the gain-bandwidth product (GBW) specification.

Your op-amp (LTC1357) has a typical gain-bandwidth product of 25 MHz.

That means when you multiply the gain of your circuit times the bandwidth of the signal, it needs to be less than 25 MHz for this op-amp to work.

You have a gain of 100, and a signal fundamental frequency (as Alex says in their answer) of 40 MHz. The product of these is 4 GHz, much higher than the 25 MHz offered by LT1357. Furthermore, if you want your output signal to at least roughly follow the waveform of your pulse signal, it will need to respond to higher harmonics of the pulse waveform, so bandwidth above 40 MHz is highly desirable here.

You should look for an op-amp with a gain-bandwidth product above 4 GHz (the OPA858 has 5.5 GHz, which is why this circuit worked with the TI part).

Note that 4 GHz is an exceptionally high GBW for an op-amp. Analog only has one offering at this level: LTC6268, which I haven't checked if it is otherwise appropriate for your circuit.

• Hi The Photon, have added another simulation with the LTC6268 but this doesn't work as well.
– ulix
Commented Nov 6, 2022 at 15:43
• @ulix, you need to use a current source, not a voltage source, for that circuit. Commented Nov 6, 2022 at 15:46
• @ulix, also read the discussion about that circuit in the LTC6268 datasheet...the bandwidth is around 11 MHz. Try lowering the feedback resistor by a factor of 10 or more for your first attempts with this circuit. Meaning, try 5 or 50 kOhms before you try to get it to work with 500 kohms. Commented Nov 6, 2022 at 15:49
• Hi @ThePhoton thank you for your input. I have changed the source to a current source (with 0.03uA output) and a parallel 1M resistor which should give 30mV at the input of the opamp - which it doesn't. I'm not getting simple voltage spikes of 30mV at the input. What can I change to get this done properly? Only getting an amplification of maybe 5 currently.
– ulix
Commented Nov 6, 2022 at 16:07
• The parallel resistor isn't required for this circuit. It's a transimpedance amplifier and it expects a current as its input signal. As for why it's not working, I don't know. Try it with a slower input at first (wider pulses, or even use a sine wave of known frequency to get a better understanding of the behavior) Commented Nov 6, 2022 at 16:10

There is PSpice model on TI site link, you can download model here and "adapt it" to LTspice (trust me, it's easy). Please show your circuit, because it's unclear why you don't have any amplification (since circuits shown in link should be working properly).

Edit: Issue you have is probably due to high frequency components of input signal (you can watch FFT of that signal in LTspice, first maximum at ~40MHz), which this op-amp can't handle (zero amplification frequency is ~25MHz). And output signal you have is just offset voltage multiplied by gain (causes constant voltage ~1V and low oscillations of input signal).