[SI-LIST] : Diode Modeling

About this list Date view Thread view Subject view Author view

From: abe riazi ([email protected])
Date: Fri Mar 30 2001 - 19:35:42 PST

Dear Scholars:

The diode's PN junction and the base-emitter (or base-collector) junctions of bipolar transistors are governed by similar physical laws. Subsequently, diode model having numerous applications is regarded as fundamental to models of other semiconductor devices. Several stages of creating IBIS, SPICE and XTK diode models are described by this message.
IBIS model of a diode can be generated via simulation or measurements. Figure 1 is schematic for generating behavioral model of 1N4002 rectifier diode by way of simulation. Using PSPICE program, DC sweep was carried out from -15 to +15V to cover the (-Vcc to 2Vcc) voltage range recommended by IBIS specs.
Figure 2 presents simulation results for diode currents I(D1) and I(D2) as function of applied voltage. When generating I-V (or V-T) curves for an IBIS datasheet, higher accuracy is achievable by sampling more data points in the non-linear regions (such as knee areas ) of the curve as opposed to more linear sections . IBIS specs [Reference 1] require for the [POWER Clamp] data to be Vcc relative, as illustrated by Figure 3 which is a plot of current through D2 versus Vcc-Vx. A comparison of Figures 2 and 3 reveals a shift of I(D2) from the first to the second Cartesian quadrant.

A diode IBIS model can be produced by extracting the [POWER Clamp] table from I(D1) vs. (Vcc-Vx) of Figure 3, the [GND Clamp] data from I(D2) Vs. Vx of Figure 2, incorporating package/pin parasitic values, and inserting the necessary keywords [Reference 1] such as [IBIS Ver], [File Name], [File Rev], [Component], [Manufacturer], etc.

Regarding procedure for creating SPICE diode macromodels, the major steps [Reference 2] include: (i) Inspecting device data sheet for useable modeling information. (such as, plots of forward diode current vs. voltage, junction capacitance vs. diode voltage, etc.), (ii) conducting I-V and C-V measurements to extract remaining parameter values, and (iii) performing simulations to optimize model parameters.

The SPICE diode macromodel can contain fourteen parameters: IS (Reverse leakage current), RS (Diode series resistance), N (Emission coefficient), BV (diode breakdown voltage), IBV (Diode breakdown current), CJO (Zero-bias junction capacitance), VJ (Bulk junction potential), FC (Coefficient for capacitance), M (Grading coefficient), TT (transit time), EG (Energy band-gap), XTI (Temperature coefficient), KF (Flicker-noise coefficient), and AF (Flicker-noise exponent)). Each of above parameters has a default value assigned by SPICE program; however, it is frequently possible (based on application) to produce a sufficiently accurate diode model using just a subset of the 14 parameters. For instance, parameters KF, AF, EG and XT1 are needed only for AC noise analyses and temperature sweeps; hence, unnecessary if the diode model is intended for other types of simulations. As another example, SPICE model of a 1N4002 diode suitable for numerous applications [Reference 2] includes:

IS = 46.5Pa, RS=123MohmS, N=1.35, CJO=51.5pF, M=0.333, VJ=0.381, FC=0.5, TT=5.77uS.
(with remaining parameters at default values).

It should be added that SPICE model parameters are scalar variables of diode equation:

Id = IS * [exp(qVd/Nkt) - 1]

Where Id is diode DC current, q is electron charge, Vd is voltage across diode, K is Boltzmann's constant, and t is the diode temperature in degrees Kelvin ( IS and N as defined earlier).
Different forms of above equation exist (some being approximations) for describing three regions of diode operation namely: forward conduction, reverse conduction before breakdown, and reverse-bias breakdown .

SPICE or IBIS models can not be directly utilized by some simulators. For instance, XTK requires that models be in Quad format. A Quad diode model can be created from the IBIS version using IBIS2XTK, or written manually. A sample is presented:

#Schottky diode to 5.0 Volts
# Voltage given in Volts, Current in mA
POINTS V: 5.0 I:0.0
POINTS V: 5.5 I:3.0
POINTS V: 5.6 I: 5.0
POINTS V: 5.75 I: 30.0
#End of Model

The above discussed models have contained data limited to only one simulation corner, whereas a more complete model demands data for three (i.e. MIN, TYP and MAX) corners. Simulations results based on TYP models are often well suited for purpose of correlation with physical measured data. However, Fast and Slow corner runs are also frequently necessary to verify a design under all conditions.

A finished model also needs a package/pin parasitic section. Nevertheless, a model may lack parasitic portion mainly due to two reasons: (1) the model developer leaves it to the user to ascertain what package type and parasitic values are applicable, and (2) The model is intended for use at low frequencies where parasitics have negligible effects.

In conclusion, several phases of generating IBIS and SPICE diode models were explained. A XTK model was also exemplified to emphasize that some simulators do not directly employ IBIS or SPICE models and demand translation to simulator's native model format. One logical order for diode modeling consists of first creating SPICE diode via measurements, then IBIS model by means of simulation and finally the Quad version using IBIS2XTK.

1. IBIS (I/O Buffer Information Specification) Version 3.2, August 1999.
2. R. Kielkowski, "SPICE Practical Device Modeling", McGraw-Hill, Inc. 1995.

Your response is highly appreciated.


Abe Riazi
2251 Lawson Lane
Santa Clara, CA 95054



**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected] In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu

About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Thu Jun 21 2001 - 10:11:23 PDT