SPICE Diode Model

Here we review the physical model on which the SPICE diode model parameters are based. Three applets will be provided which help us understand better the diode forward I-V characteristics, the diode C-V characteristics, and an example SPICE simulation of a simple diode circuit.

The model used for the pn-junction diode in SPICE is depicted in the Figure shown below. This SPICE diode model is also applicable to the Schottky-barrier diodes.

A single linear resistor RS represents both the external contact resistance and any voltage drop in the neutral n and p regions. The voltage drop in the neutral regions is significant under a high level injection condition. The dc characteristic of the device is modeled by a nonlinear current source which in SPICE follows the ideal diode equation:

where N, the emission coefficient, is almost always 1, but can be larger than 1 for Schottky diodes. Three parameters in the SPICE parameter table describe the diode dc characteristics: IS, the saturation current, N, the emission coefficient, and RS, the ohmic resistance. Deviation from the ideal diode I-V characteristic, particularly at low currents (<1 nA, due to generation in transition region) and at high currents (> 1mA, due to ohmic voltage drop in neutral regions) are discussed further below using an applet that calculates the diode I-V characteristic.

The charge storage element QD in the above Figure models both the charge storage by injected minority carriers and the charge stored in the depletion region. The total stored charge QD is given by

Here, the first term is the stored charge by injected minority carriers (diffusion charge), and the second term is the stored charge in the depletion region. The diffusion charge depends on the transit-time parameter TT (=electron lefetime, hole lifetime or a combination of the two), and the diffusion charge, hence the diffusion capacitance vary with the forward current. m in the above formula is the grading coefficient, equal to 1/2 for an abrupt junction and 1/3 for a linearly graded junction.

The total capacitance is given by

Therefore, as the parameters can be found in the SPICE parameter table, the diffusion capacitance is modeled by the parameters TT, IS, and N, and the transition capacitance is modeled by Cj0, FC, M, and Vj.

[Applet to learn more about the forward I-V characteristics of a pn junction diode.]

[Applet to learn more about the capacitance-voltage (i.e., diffusion capacitance and transition capacitance) of a pn junction diode.]

[Applet that simulates a simple diode circuit in a manner that is similar to SPICE.]