# How to model a noisy Zener diode in LTSPICE?

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.

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:

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.

• Tens of zener diodes is not much in the scheme of things.. Pretty small market!
– pipe
Mar 17, 2016 at 23:12

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)

• Yeh, I saw that one, but he's physically measured the noise in a jig. Is there no model anywhere? Mar 17, 2016 at 23:26
• I've tried inserting a voltage source between D1 and the base of Q1, but again I have no data as to the scale of the signal. Either someone tells me the AC Vpp to insert there, or I'll just have to build the damn thing. Seems a shame as isn't that what simulation is for? Mar 18, 2016 at 4:21
• I have not seen any good noise models. Note that the noise from low-voltage Zener devices will be quite different than the noise from higher-voltage avalanche breakdown devices. I also expect that there is significant part-to-part variation since the manufactures do not control for noise. I did see Linear Technologies design note 70 which has a circuit with feedback to control the amplitude of the noise. Mar 18, 2016 at 4:30
• There is an application note at Maxim that suggests the noise power of a zener is in the order of -90dBm. maximintegrated.com/en/app-notes/index.mvp/id/3469 Mar 19, 2016 at 16:05