Electronic – How to model a noisy Zener diode in LTSPICE

ltspicezener

I'm trying to simulate a white noise generator of the Zener diode style. I'm going with current amplification, rather than the more traditional voltage amplification just because. My problem is that I don't know how to simulate the behaviour of the diode, D1. With the 30 volt supply, I'm hoping that the 24 volt Zener will be running in full avalanche mode, spewing out a whole pile of white noise.

I'm using LTSpice, but that only has models for the reverse breakdown voltage of Zeners. Consequently the following circuit only produces a steady DC voltage at the “noise” node. How can I fully model this transistorised circuit shown below? Is it even possible, or do I have to actually build it and physically measure the noise? My sense is that as tens of these diodes have probably been sold world wide, there must be data out there that I can't find. I'm looking for concrete numbers rather than theory (or any sort of integration symbol) that I can plug into LTSpice.

Zener + transistor circuit

Supplemental:

I've got as far as adding a white 1 mV P-P noise source (@1 MHz???) in front of the Zener, with a 15-0-15 supply as so:

Circuit + noise source

which seems to kinda work producing the following trace at "noise". This seems to me as perhaps how a noisey breakdown at the diode would appear. It looks as if LTSpice has set a voltage gain of 100ish. Of course, this is a somewhat moot without a better estimate of the actual noise levels.

enter image description here

Best Answer

Spice models generally do not include noise in transient simulations. The "noise" model in spice is used only in AC sweeps, where the noise power is calculated as a function of frequency. While resistor (Johnson–Nyquist) noise is in the model, semiconductor models often do not have accurate noise models. The spice diode model does include flicker noise, but not other noise sources.

For your purposes, AC analysis may be sufficient assuming that your diode has a proper model, since what you want is to see if the noise power density is flat. But, I doubt that the Zener model includes accurate noise parameters. The spice model of the diode mentioned in this question (EDZV24B) does not include any noise parameters (which are the AF, KF, and FFE parameters).

Another option (for transient simulations) is to include a voltage sources controlled by a random number. For a description of using this approach to noise modeling, this website from Giorgio Vazzana has good information. But, to follow this approach, you have to know how much noise to expect. Also, the transient simulation would not normally include noise added by the transistor.

An example noise voltage source (from the above mentioned website) is:

Vn 1 n1 dc 0V ac 1mV trrandom (1 5us 0s 125m 0m)