Simulating Dark Current in a Photodiode

On page 2 of this  datasheet

https://www.hamamatsu.com/resources/pdf/ssd/g15553_series_kird1140e.pdf

there is a "Dark current vs. reverse voltage" graph. Can the LTspiceXVII diode model simulate this dark current?

I want to avoid if possible having read off that graph a parallel current,, and come up with an equivalent series voltage source, and resistance, for every reverse bias voltage value I want to simulate.

I seek to simulate both the overall TIA design's response to laser light signal, and also the noise.

A photodiode will produce shot noise. Its signal photocurrent flows in the direction opposite to that of diode forward bias. Can LTspiceXVII be made to simulate photocurrent shot noise produced by the signal photcurrent?

  • +1
    •  Analog Employees 
    •  Super User 
    on Apr 6, 2021 2:37 PM

    Hi spflanze,

    The implemented diode model in LTspice is an extended Berkeley-SPICE model (see Help Topics / F1 and http://bwrcs.eecs.berkeley.edu/Classes/IcBook/SPICE/UserGuide/elements.html#618). Therefore, you have to add e.g. a B-source in parallel with a table function to model the dark current characteristics shown in the datasheet graph. An equivalent series voltage source seem to be much more complicated.

    Shot noise can be regarded as independent of the signal frequency in most cases. Its power spectral density is constant over frequency as it is for a resistor. So you can e.g. calculate an equivalent shot noise R depending on the photodiode current for AC simulations. Just use a resistor and replace its value by "R={your_calculation}"
    If you like to simulate shot noise in the time domain (transient), you can use again a B-source, this time with the "white(x)" function. Be aware that a frequency limit exists which depends on the simulation time step. The power spectral density of white(x) will not stay constant above that limit. You can push it out by setting a minimum time step.