Spice diode model

After just submitting my post I can see how it's perhaps unclear. I am not looking for a spice diode model; e.g., .MODEL HSMS-285x D (IS=3E-6,CJO=0.18E-12,VJ=.

What I'm trying to do is add diode noise to a transient analysis simulation. Current causes shot noise, and diode resistance causes Johnson noise.

So far I've been able to add noise to my resistors, which is an easy task. For LTspice I came up with -->

Johnson noise source, in series with the resistor: V=white(time*BW+{flat(9999999)})*3.017494931E-11*((T*BW*R)**.5)

BW is bandwdith. T is temp is Kelvin R is the resistance of the resistor.

The last task is to add noise to diodes, perhaps not such an easy task.

Hello Paul,

Are you the same Paul with a similar question in sci.electronics.design ? I have just send the same answer to sci.electronics.design.

Hello Paul,

Shot noise is equal sqrt(2*q0*Id*BW). Just use I(D1) in the formula of a current noise source Bi, I=white(....). This noise current source has to be connected in parallel to the diode.

It would be more correct to use a Gauss noise source. A Gauss noise source can be made with a few independent random noise sources or with the Box-Mueller method.

Normally a noise analysis in SPICE will be done with the AC .NOISE analysis. The main reason is the small ratio of noise compared to the signal. A time domain simulation can have accuracy limits above your expected noise level.

Best regards, Helmut