![](bg1.png)
Practical Implementation of Diode SPICE Model with Reverse Recovery
Denys Igorovych Zaikin
a
Advent Technologies A/S, Lyngvej 8, Aalborg DK-9000, Denmark
Keywords:
Diode Reverse Recovery, SPICE, Circuit Simulation.
Abstract:
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.
1 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 elec-
tronics simulation. These SPICE simulators use a ba-
sic diode model. Adding a feature to simulate diode
reverse recovery will improve loss estimation and cir-
cuit behaviour simulation. This is especially attrac-
tive 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 gener-
ate a diode macro model using only parameters from
the diode manufacturer’s datasheet or measurement
data.
2 DIODE MODEL DESCRIPTION
Original work (Lauritzen and Ma, 1991) provides the
following three equations for diodes with reverse re-
covery:
i(t) =
(q
E
− q
M
)
T
M
, (1)
a
https://orcid.org/0000-0003-4080-5631
0 =
dq
M
dt
+
q
M
τ
−
(q
E
− q
M
)
T
M
, (2)
q
E
= I
s
τ(e
(
v
nV
T
)
− 1). (3)
From equations (1)-(3), the forward DC-bias char-
acteristic can be obtained:
i =
I
s
(1 + T
M
/τ)
(e
(
v
nV
T
)
− 1). (4)
Here, i is the diode current, v is diode junction
voltage, V
T
= kT /q is the thermal voltage, I
s
is satura-
tion current (similar to the SPICE basic diode model
parameter) and n is the emission coefficient (similar
to the SPICE basic diode model parameter). The vari-
ables from (Lauritzen and Ma, 1991) are as follows:
T
M
represents diffusion time, τ recombination life-
time, 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.
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 Figure 2.
92
Zaikin, D.
Practical Implementation of Diode SPICE Model with Reverse Recovery.
DOI: 10.5220/0012096500003546
In Proceedings of the 13th International Conference on Simulation and Modeling Methodologies, Technologies and Applications (SIMULTECH 2023), pages 92-96
ISBN: 978-989-758-668-2; ISSN: 2184-2841
Copyright
c
2023 by SCITEPRESS – Science and Technology Publications, Lda. Under CC license (CC BY-NC-ND 4.0)