Practical Implementation of Diode SPICE Model with Reverse Recovery

: Peter O. Lauritzen and Cliff L. Ma proposed an approach for creating a physical model of reverse recovery for soft recovery diodes in 1991. The current paper demonstrates how to create the proper SPICE sub-circuit using only the specifications from the diode datasheet from the manufacturer. Software for characterization tools has been developed, tested, and is now openly accessible for use.


INTRODUCTION
Of the many SPICE-based simulators on the market, most still use the old standard diode SPICE model that does not cover reverse recovery correctly.Both LTspice (Analog Devices, Inc., 2008) and Pspice (Cadence Design Systems, Inc., 2015) are powerful pieces of software that are widely used for power electronics simulation.These SPICE simulators use a basic diode model.Adding a feature to simulate diode reverse recovery will improve loss estimation and circuit behaviour simulation.This is especially attractive for LTspice, which is a powerful, free simulator that can be used in complex design simulation.This paper applies original theoretical work (Lauritzen and Ma, 1991) to the practical implementation of a SPICE macro model of diodes with reverse recovery.The model described in (Lauritzen and Ma, 1991) is based on real physical processes in a diode and, because of this, is robust.
A Windows OS application was created to generate a diode macro model using only parameters from the diode manufacturer's datasheet or measurement data.

DIODE MODEL DESCRIPTION
Original work (Lauritzen and Ma, 1991) provides the following three equations for diodes with reverse recovery: a https://orcid.org/0000-0003-4080-5631 ) − 1). (3) From equations ( 1)-( 3), the forward DC-bias characteristic can be obtained: Here, i is the diode current, v is diode junction voltage, V T = kT /q is the thermal voltage, I s is saturation current (similar to the SPICE basic diode model parameter) and n is the emission coefficient (similar to the SPICE basic diode model parameter).The variables from (Lauritzen and Ma, 1991) are as follows: T M represents diffusion time, τ recombination lifetime, q M total stored charge and q E charge variable.This model is completed with ohmic resistance R s and junction capacitance C j , as shown in Figure 1.

EXTRACTION OF MODEL PARAMETERS
Equations ( 1)-( 3) fully describe diode reverse recovery and DC bias characteristics of the diode.To use these equations, it is necessary to define τ, T M , n and I s parameters.Parameters τ and T M are defined with the approach used in (Lauritzen and Ma, 1991).An additional intermediate parameter -reverse recovery time constant τ rr -is used and can be measured directly from the reverse recovery waveform or defined from the diode datasheet's parameter T rr , the reverse recovery time.From Figure 3, τ rr can be found as follows: Now, when τ rr is known, parameters τ and T M can be found using numerical equation solving of the following equations from reference (Lauritzen and Ma, 1991): To find parameters I s , n and ohmic resistance R s in equation ( 4), the standard diode forward DC-bias SPICE model equations are used (Figure 1): Based on Equation ( 9) and Figure 4, it can be seen that I s ' is the leakage reverse current at the maximum reverse voltage according to the datasheet's reverse DC-bias characteristic of the diode.Using Equations ( 4) and (9), I s can be found:

V -I
To find R s and n, two points should be defined on the DC-bias diode characteristic (Figure 4).From equations ( 8) and ( 9), there is system of equations with two unknown variables, R s and n: (11) After system ( 11) is solved, R s and n are found: To simulate non-linear junction capacitance, equations from the standard diode SPICE model are used (Kielkowski, Ron M, 1995): In this model for junction capacitance, fixed parameters are assumed: V J = 2.0 and F C = 0.5.It is also necessary to find parameters M and C J0 using two points on the datasheet's reverse bias capacitance curve in Figure 5.Using these two points, a system of equations can be obtained based on Equation ( 14): After ( 16) is solved, M and C J0 can be found: To implement junction capacitance in the new diode model, the standard SPICE diode model is placed in parallel with the diode body (Figure 2).
The new diode SPICE model implements the behavior of the diode at a fixed temperature.Lead inductances should be added externally for parasitic simulation.

SIMULATION RESULTS
The newly generated model was tested in two simulators -LTspice and Pspice.The LTspice IV simulation results for the MUR460 diode are shown in Figure 6.

SOFTWARE DESCRIPTION
To generate the diode SPICE model using the manufacturer's datasheet characterization, the software (SW) tool "DiodeRRSubmodel" was made (Figure 9).It is a Windows OS application and can be freely downloaded from the link (ZAIKIN D.I., 2021).
Next, input data from the datasheet are used as fol-  lows: • user enters diode name; • user defines work temperature of diode; • user enters two points on the DC-bias forward characteristic for the specified temperature (Figure 4, Figure 10).Points far enough away from each other should be chosen; • user enters reverse leakage current for diode at specified temperature; • user enters two points on the junction capacitance (Figure 5, Figure 11).Points far enough away from each other should be chosen; • user enters the reverse recovery specification from the diode datasheet at the specified temperature: I f , di/dt, I RM , and T rr (Figure 3, Figure 12).
The extracted model file is placed in the same folder as the .exefile of the SW.An example of a generated netlist is shown in Figure 13.

CONCLUSION
In the work that is being presented, the diode SPICE model is implemented together with an accurate simulation of reverse recovery.The study that is given is based on the physical representation that was first created in the source (Lauritzen and Ma, 1991).The current work offers automated diode model development based on datasheet specifications from the manufacturer.Open source software is publicly accessible for diode characterisation and model generation (ZAIKIN D.I., 2021).

Figure 1 :Figure 2 :
Figure 1: Diode model components.The practical implementation of equations (1)-(4) in the SPICE model, along with ohmic resistance and junction capacitance, are shown in Figure2.

Figure 3 :
Figure 3: JEDEC reverse recovery time T rr definition and waveform.

Figure 6 :
Figure 6: Comparison of current and standard waveform LTspice IV simulation results for the MUR460 diode.The MUR460 standard diode model was taken from the LTspice IV library.Pspice 16.6 simulation results for the HFA25TB60 diode are shown in Figure 7.

Figure 7 :
Figure 7: Comparison of current and standard waveform Pspice 16.6 simulation results for the HFA25TB60 diode.The HFA25TB60 standard diode model was taken from the Pspice 16.6 library.The Pspice 16.6 simulation results for ISL9R3060 diode are shown in Figure 8.

Figure 8 :
Figure 8: Comparison of current and standard waveform Pspice 16.6 simulation results for the ISL9R3060 diode.The ISL9R3060 standard diode model was taken from the manufacturer webpage.

Figure 9 :
Figure 9: Windows OS application SW for diode model extraction.

Figure 10 :
Figure 10: Two points selected on the DC-bias characteristic.

Figure 11 :
Figure 11: Two points selected on the junction capacitance characteristic.