# What's wrong with my diode SPICE model for the HSMS-2860?

To be brief, I am as new as they get to creating SPICE models for components so I'm walking blind.

I was trying to create a SPICE model for the HSMS-2860 diode.

HSMS-2860 Schottky Diode Datasheet

Here is the .lib file I wrote for the diode, I got the parameters from the datasheet above.

.MODEL HSMS2860 D
+BV = 7
+CJO = 0.18E-12
+EG = 0.69
+IBV = 1E-5
+IS = 5E-8
+N = 1.08
+RS = 6.0
+VJ = 0.65
+XTI = 2
+M = 0.5


What I noticed is when I import this file into ANSYS Circuit Designer, it doesn't behave like a diode. When I apply a sinusoidal source to it (half-wave rectifier) I still encounter negative peaks on the output even though I have the peak input voltage amplitude below the reverse breakdown voltage of the model.

The goal of modeling this diode is so that I can determine a input impedance at a certain input power so that I can design a matching circuit to match that input impedance to my receiving antenna's impedance.

I'm sure the rabbit hole for SPICE modeling goes deep. I would appreciate some assistance with the matter.

• What frequency excitation were you applying? Feb 17, 2021 at 1:10
• @ThePhoton Sorry, forgot to mention that. I am exciting it with a 5.8Ghz Pure Sinusoid.
– EECE
Feb 17, 2021 at 1:43
• Two things that might be going on: The diode capacitance is high enough to give it low impedance at 5.8 GHz (this would happen if Ansys has different default values than typical Spice simulators); or you are doing an AC analysis that inherently linearizes the device behavior (this analysis simply doesn't capture rectifying behavior of diodes). I don't know enough about Ansys Circuit Designer to know which is more likely (or if there's some other pitfall you could have run into). Feb 17, 2021 at 6:43

While a practical design of an RF detector with the Schottky diode use distributed elements

(see, for example, the AVAGO Technologies datasheet HSMS-286x Series Surface Mount Microwave Schottky Detector Diodes, Figure 21 5.8 GHz Matching Network for the HSMS-286x Series at 3 µA Bias), and these circuits should be developed using specialized design tools, the origin of "negative peaks" can be traced with a general-purpose SPICE simulator.

Sure there is always a reverse current through a diode, even for DC current, only it can be very small and you would not see it in your simulation plots. With AC current, a reverse current has two components: the reverse leakage current, which can be high for Schottky diodes when compared with p-n diodes, and the reverse recovery current, which is much smaller for Schottky diodes when compared with p-n diodes but still reveals itself when the signal waveform period $$\T_{sig}\$$ is on the order of Schottky diode's reverse recovery time $$\t_{rr}\$$ (switching time). The voltage sensitivity of HSMS2860 is halved at the frequency of 5.8GHz (ref value at 915MHz). At this frequency, the reverse recovery time effects become noticeable in the waveform of detected signals ("rectified" waveforms).

To mitigate the visible "negative peaks" in your "Half-Wave Rectifier" simulations, you can decrease a load resistance (impedance) in order to provide a sufficient reverse current.

For reference, the "Half-Wave Rectifier" circuit to be simulated:

, to easily see the effects of load, I first simulate your "Half-Wave Rectifier" with a 0.58GHz V1 source and 100 Ohm (R1) load:

You see "negative peaks" in graphs of both a voltage across the load and a diode current.