Multi-level Electro-Thermal Simulation of Power PCB Electronic Modules
for Motor Driving
KONSTANTIN O. PETROSYANTS, IGOR A. KHARITONOV, MIKHAIL S. TEGIN
National Research University “Higher School of Economics”,
Moscow Institute of Electronics and Mathematics,
Tallinskaya ul., 34, Moscow, 123458,
RUSSIA
Abstract: -A scheme of automated multi-level electro-thermal modeling of power PCB modules using software
tools Comsol at the device construction level, SPICE tool at the circuit level, and Asonika-TM tool at board level
was proposed to improve the conventional design approach. The effectiveness of the proposed methodology is
demonstrated in the example of electro-thermal analysis of real power MOSFET driver circuit realized on PCB.
Key-Words: - multi-level electro-thermal simulation, PCB power electronic module, SPICE simulation, COMSOL,
ASONIKA-TM, junction temperature jumps, thermal network.
Received: January 15, 2023. Revised: Octobert 12, 2023. Accepted: November 11, 2023. Published: December 12, 2023.
1 Introduction
To provide effective thermal management of power
electronic systems from the reliability viewpoint, the
electro-thermal simulation of the device/circuit
system in package placed on PCB with cooling
conditions is required, [1], [2]. To realize the electro-
thermal simulation flow, two approaches are used:
1) circuit analysis tool (SPICE like) is coupled
with 3D thermal numerical simulation tool (AnSYS,
[3], Comsol, [4], [5], [6]), for modeling of electro-
thermal processes in the 3D construction of the
electronic module under test;
2) only the circuit-based tool (SPICE like) is used
for electro-thermal simulation of the power PCB
modules. The electronic devices are described by the
electro-thermal SPICE models and packages/heatsinks
are described by the RC thermal networks according
to the thermo-electric analogy, [3], [7], [8], [9], [9],
[10].
The first approach provides the complete electro-
thermal solution for electronic modules. However, its
realization is difficult because of detailed description
of the 3D PCB module construction and much time
spent on numerical simulation of the 3D construction
using the finite-element (FEM) method.
The second approach is more understandable and
convenient for circuit designers because the approach
requires only the circuit simulator, [11]. Its advantage
is the possibility of fast analysis of electrical
characteristics, power, and temperature.
The acceleration of the motor rotor can cause high
current or voltage jumps in output circuit load that
increases the power loss and device junction
temperature. Therefore, the problem for designers is
to predict the junction temperature in the dynamic
operation. The main task is to minimize the CPU time
of transient response simulation in PCB modules.
Several studies have been done in the direction of
realizing the fast electro-thermal technique for
dynamic analysis. In, [4], the joint ELDO-COMSOL
tools for electro-thermal dynamic simulation of power
MOSFET in the package were used. Unfortunately,
the electrical circuit of the test module was not
considered and the passive device with equivalent
power loss instead of a real MOSFET was used for IR
thermal measurement.
The thermal Cauer networks of IGBTs, [12], and
MOSFETs, [13], were used to minimize the CPU time
for the dynamic analysis. Additional work needs to be
done to further verify the models with junction
temperature measurements.
In, [14], the fast ET simulation model for long
real-time thermal simulation of a three-phase IGBT
inverter power module was presented. The design
technique is original and does not use the standard
commercial tools like SPICE, COMSOL, ANSYS,
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
126
Volume 22, 2023
etc. So it is not easy for the engineers to implement
the new technique in the real design system for
practical use.
The authors of, [15], [16] have analyzed different
approaches to electro-thermal design and proposed
simple ET SPICE models of power semiconductor
transistors in packages to minimize simulation time.
Summarizing the critical analysis of the
publications we can conclude that the problem of fast
and easy for implementation electro-thermal
simulation technique is as usual under consideration.
Especially the works with the real practical solutions
that were proposed are required.
In this connection, the presented paper describes
the effective ET solution scheme for the dynamic
behavior of motor driving power module. The
complete chain is discussed: 1) compact SPICE ET
model of power MOSFET in package; 2) package RT
determination using Comsol solution; 3) coupled
SPICE-ASONIKA-TM technique for ET transient
analysis of PCB electronic module; 4) thermal models
verification by comparison with the results of IR
measurement of the module surface temperature; 5)
MOSFET junction temperature analysis and probable
failure detection; 6) improvement of the module
construction to guarantee the reliability of the driver
circuit and motor winding of coils.
2 Methodology
To provide an effective electro-thermal analysis of the
PCB electronic modules we used multi-level electro-
thermal simulation and both of the mentioned
approaches with addition of infra-red thermal
analysis, [17]. Furthermore, to automize and simplify
this procedure we have developed the special
software tools ST1, ST2, ST3, [18], which were
integrated into the electro-thermal iteration loop in
Figure 1.
Our important innovation in improving the electro-
thermal design process is the automation of the next
processes:
- circuit component powers calculation from the
SPICE analysis,
-transfer the component powers from the SPICE
tool to the thermal simulation tool,
- temperature values transfer from the thermal
simulation stage to the circuit SPICE simulation
stage,
- power electronic devices and ICs case thermal
subcircuit generation for SPICE electro-thermal
simulation.
For the first three tasks the special software tool
ST2 was developed. For the last task a special Table
with thermal parameters of standard component cases
was formed (Figure 1). The table contained standard
component case names and corresponding parameters
of the case thermal subcircuit. The data in the table
were taken from the components datasheets or the
universal 3D physical software tool Comsol was used
to generate Rti, and Cti elements when the required
thermal parameters were not presented in component
data sheets. The required thermal parameters were
selected from the Table using developed ST1 tool.
As a result the multi-level design methodology,
using Comsol at device construction level, SPICE at
the circuit level, and ASONIKA-TM at board level
was developed.
The tools Comsol, [19], and SPICE, [20], are well
known.
ASONIKA-TM software tool, [21], developed at
Moscow Institute of Electronics and Mathematics was
used for PCB thermal simulation. The tool has the
following advantage: very quick calculation of PCB
thermal mode due to using analytical thermal models
for components thermal and cooling parameters and
numerical simulation for analysis of temperature
distribution along PCB surface.
2.1 Special Software Tools Developed for
Processing Simulators Data and
Transferring Information between
Simulators
The details of the developed electro-thermal
simulation scheme are the next.
The tool ST2 (at the right in Figure 1) provides,
[18]:
- automated, user-controlled calculation of the
circuit element powers in SPICE tool;
- component power values transfer from SPICE to
thermal analysis packages (Comsol, ASONIKA-TM
etc.);
- component temperature values transfer back from
the thermal analysis packages to the SPICE analysis
tool.
The software tool ST1 (at the left in Figure 1)
provides automated generation of thermal subcircuits
for the power component cases and packages, [18], as
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
127
Volume 22, 2023
was described upper.
The tool ST3 (at the right in Figure 1) provides
automation of power- temperature transfer between
electrical and thermal subcircuits during SPICE
electro-thermal simulation (it will be illustrated later).
Fig. 1: Scheme of software tools interactions for electro-thermal modeling and simulation of power circuits on
PCBs used in the present paper
3 Joint Spice, Comsol, Asonika-TM
Simulation and Analysis of Electro-
Thermal Modes of Stepper Motor
Control Circuit
The described scheme of interactions of software
tools in Figure 1 was used by us for electro-thermal
modeling and simulation of power PCB modules and
analysis of power MOSFETs junction temperature
jumps for a power 4-phase stepper motor control
circuit realized on PCB (Figure 2). The circuit is a
bridge with 4 IRFB4615 DMOS transistors for one
phase control, [22]. The four output DMOS
transistors were placed on OMNI-UNI-30-50-D heat
sink, [23], with thermal resistance Rθ=4.06 °С/W
under natural convection conditions.
The values of IRFB4615 channel resistance Rds on=
35 Ohm and supply voltage 24 V were used.
3.1 Electro-thermal Simulation of the Step
Motor Driver Circuit using the SPICE
Analysis Package
For the electro-thermal simulation of DMOSFET
temperature jumps of the mentioned driver circuit
using the SPICE simulator, the electro-thermal SPICE
model for IRFB4615 DMOSFET has been built. The
model consisted of two interconnected parts:
- the electrical part for the IRFB4615 DMOSFET
with temperature dependent parameters for the
threshold voltage, mobility, and MOSFET channel
Ron and
- the thermal subcircuit for the IRFB4615
DMOSFET case with the current source describing
the dissipated power of the DMOSFET .
Parameters of the electro-thermal model were
defined using measured static and dynamic
characteristics of IRFB4615 DMOS FET with
account for the measured MOSFET temperature.
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
128
Volume 22, 2023
The hardest (from the electro-thermal point of
view) mode of the motor driver circuit is the motor
holding position mode – the maximum constant DC
current is consumed by the motor in this mode.
Furthermore, this maximal current is provided by the
same MOSFET in this mode. So the motor driver
circuit was simulated and analyzed by us in this mode
of work.
Our measurements showed that the driver circuit
reaches a stationary thermal mode for about 50
minutes. Electro-thermal simulation of the driver
circuit with SPICE tool using the original electronic
circuit and with additional thermal sub-circuit (Figure
4) did not allow to reach a stationary thermal mode,
because the time step in SPICE simulation was about
1 µs (due to the operating frequency of the circuit 30
(a)
(b)
Fig. 2: Simplified schematic (a) and PCB realization (b) of stepper motor driver circuit
Fig. 3: Electro-thermal model of IRFB4615 DMOSFET
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
129
Volume 22, 2023
kHz) , but the time constant for the thermal part was
many orders larger (due to large values of thermal
capacitances of transistor case and heat sink). This
problem with very large differences of time constants
for electronic and thermal parts is well known, [24]).
We applied the following simple approach,
accelerating electro-thermal calculation.
Fig. 4: Thermal subcircuit for 4 output power
transistors mounted on heatsink
Fig. 5: SPICE simulated temperature-time
dependences for power transistor cases in the circuit
Figure 2 after the 4th iteration (the motor is in the
holding position mode)
The process of temperature and power transfer
was repeated automatically several times (using ST3
tool). This iterative process was finished when small
changes of the power transistor temperature values
(0.5 oC) were reached from one iteration to the next
iteration. In our case it took 4 iterations. Figure 5
shows SPICE simulated temperature dependences of
output power transistors cases on time after the 4-th
iteration. The y-axis displays power transistor (tvt8,
tvt2, tvt9, tvt3) cases and heatsink (trad) temperatures
in degrees Celsius as the voltage’s values. The x-axis
displays time of the driver working in ksec after its
switched on.
3.2 Electro-thermal Simulation of the Motor
Driver Circuit on PCB using SPICE and
Comsol Packages
To check the correctness of the thermal subcircuit
(Figure 3 and Figure 4) electro-thermal simulation of
the motor driver circuit on PCB was performed using
SPICE and Comsol packages/ The power values of
the output transistors (VT2, VT3, VT8, VT9) of the
circuit Figure 2 were automatically determined from
a SPICE analysis of the circuit when a stationary
thermal regime was reached (see previous paragraph).
Figure 6 (a) shows a 3D image of the power
transistors placed on the heatsink package in Comsol
tool, and Figure 6 (b) shows Comsol simulated
temperature distribution in the power transistors and
heatsink. The temperature values of power transistors
were close to the values obtained from SPICE
analysis of the circuit. A detailed comparison of
thermal analysis results obtained using different
simulation tools will be presented below.
(а)
(b)
Fig. 6: 3D view (a) and thermal simulation results of
stepper motor driver power MOSFETs (1 phase) (b)
using Comsol software tool
3.3 Electro-thermal Simulation of the Motor
Driver Circuit on PCB using SPICE and
ASONIKA-TM Software Packages
ASONIKA-TM tool allows quick (few seconds)
thermal analysis of circuits realized on PCB with
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
130
Volume 22, 2023
account for real PCB construction features: layer
thicknesses, PCB and electronic component sizes,
convection conditions and more details . The power
values of the transistors (VT2, VT3, VT8, VT9) were
determined from the SPICE analysis of the operation
of the circuit when a stationary thermal mode was
reached (as described in the previous section) and
were transferred from SPICE to Asonika-TM tool,
(using ST2 tool) and the temperature values of power
elements were transferred back to SPICE tool using
the same software tool, at the right in Figure 1).
(a)
(b)
Fig. 7: 3D view (a) and thermal simulation results (b)
of all 4 phases of stepper motor driver using Asonika
TM software tool
Figure 7 (a) presents a 3D image of power transistors
placed on heatsink (for all 4 phases) in Asonika-TM
software package. Powers were supplied to 2 bridges
of 4. Figure 7 (b) presents the simulated temperature
distribution in power transistors and PCB.
3.4 Infrared Thermal Analysis of the
Thermal Mode of the Stepper Motor
Driver Circuit
Flir A-40 thermal imaging camera was used for study
of the thermal model of the stepper motor control
circuit and for verification of the simulation results.
The obtained temperature distribution on power
transistors (of one phase) in a steady state thermal
mode and the motor in the holding position mode is
presented in Figure 8.
Fig. 8: Temperature distribution in 1 phase of stepper
motor driver (Figure 2) measured with Flir A40
thermal imaging camera (in a steady state thermal
mode when the motor is in the holding position
mode)
3.5 Analysis of the Obtained Results
Table 1 presents the comparison of the power
transistors temperature values (circuit Figure 2)
obtained by the IR measurement method and by the
simulation methods with the different tools (SPICE,
Comsol и Аsonika-ТМ).
It is seen that the results obtained using the
different thermal analysis packages are quite close to
each other and are confirmed by the results of thermal
IR camera imaging that confirms the correctness of
our electro-thermal simulation process.
3.6 Analysis of the Power MOSFETs
Temperature Jumps
The most important parameter of PCB driver module
directly related to thermal condition is the reliability.
From this point of view, the motor driver module was
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
131
Volume 22, 2023
analyzed in the most hard electro-thermal mode:
ambient temperature 40°C, maximal value of
IRFB4615 channel resistance Rds on= 39 mOhm,
supply voltage 28 V and the stepper motor has to be
in the holding position mode.
Table 1. comparison of the power transistor
temperature values IR measured and simulated with
SPICE, Comsol and Asonika-TM tools
Power,
W
T, °C
( IR
measured)
T, °C
(Spice
)
T, °C
(Asonika
)
T, °C
(Comsol)
3,04
72,1
70,7
66,76
69,2
1,91
72,7
68,6
55,35
67,2
0
67,7
64,9
52,37
63,4
4
74,5
72,5
77,84
70,9
0
67,3
64,9
-
63,9
For comparison, the conventional operational
mode was simulated with the following PCB module
parameters: Tamb=25oC, Rds on= 35 mOhm, supply
voltage 24 V and the motor is in the holding position
mode too.
Since the MOSFET parameters and power depend
on junction temperature value it is necessary to use
the developed and verified the electro-thermal SPICE
models for power MOS FETs to get the maximal
temperature estimation.
SPICE simulated temperature values of IRFB4615
MOSFET for the most hard electro-thermal mode are
presented in Figure 9 (a). At the upper picture, the y-
axis displays DMOS FETs powers (pavg_tvt8,
pavg_tvt2, pavg_tvt9, pavg_tvt3) as the voltage
values. At the bottom picture, the y-axis displays
power transistor (tvt8, tvt2, tvt9, tvt3) cases and
heatsink (trad) temperatures in digress Celsius as the
voltage values. The x-axis displays the time of the
driver's work in ksec after it was switched on. The
circuit entered the holding mode at 6 msec. It is seen
from the Figure 9 (a) (V(tjvt8) curve) that VT3
MOSFET junction maximal temperatures were nearly
115°C – it could result to the MOSFET failure.
(a)
(b)
Fig. 9: SPICE simulated DMOSFET powers and
DMOSFET junction temperature jumps for the
hardest thermal mode (a) and for enhanced cooling
conditions - the larger heat sink with Rθ=2.5 °С/W
(b).
To guarantee more reliability of the driver circuit
and to enhance MOSFET cooling conditions, a larger
heat sink with less thermal resistance Rθ=2.5 °С/W
(instead of 4.06 °С/W) under natural convection
conditions was used Figure 9 (b) presents SPICE
simulated results for this case. It is seen that the
DMOSFET junction maximal temperature (top
graphs on Figure 9 (b)) decreased to 84°C, which
enhances reliability.
4 Conclusion
1. The scheme for multilevel joint electro-thermal
design of power electronic circuits on PCBs using
software tools Comsol, SPICE, ASONIKA-TM and
IR thermal analysis was realized and verified.
2. The special software tools and data table with
the power component thermal properties including
the names of the component cases and the parameters
of their thermal subcircuit (RTi, СTi) were developed
to atomize and simplify the forming thermal models
for power components.
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
132
Volume 22, 2023
3. The significant acceleration of electro-thermal
SPICE-ASONIKA-TM simulation process was
achieved (more than 10 times in comparison with the
conventional electro-thermal simulation technique
using coupled SPICE-Comsol tools).
4. The effectiveness of the proposed methodology
was demonstrated at the example of real PCB
construction for motor driver with power MOSFETs.
5. The results obtained using the different thermal
analysis packages were quite close to each other and
were confirmed by the results of thermal IR camera
imaging.
6. The probable thermal failures were detected and
the ways to reduce the MOSFET junction
temperature were proposed.
References:
[1] Rencz, M.; Szekely, V.; Poppe, A.; Courtois,
B., "Cosimulation of dynamic compact models
of packages with the detailed models of printed
circuit boards," 27th Annual IEEE/SEMI
International, San Jose, CA USA, vol., no.,
pp.285,290, 2002 doi:
10.1109/IEMT.2002.1032768.
[2] T. Shinoda, “Three Thermal Simulation & Test
Innovations for Electronics Equipment Design.
Electronics Cooling”, 2019, [Online].
https://www.electronics-
cooling.com/2019/06/three-thermal-simulation-
test-innovations-for-electronics-equipment-
design/ (Accessed Date: April 15, 2023).
[3] T. Hauck, W. Teulings, W. Teulings, E.
Rudnyi, “Electro-Thermal Simulation of Multi-
channel Power Devices on PCB with SPICE”,
15-th Thermal Investigations of ICs and
Systems International Workshop, (THERMINIC
2009), Leuven, Belgium, pp.124-129, 2009.
[4] G. De Falco, M. Riccio, G. Romano, L.
Maresca, A. Irace and G. Breglio, “ELDO-
COMSOL based 3D electro-thermal
simulations of power semiconductor devices”,
2014 Semiconductor Thermal Measurement
and Management Symposium (SEMI-THERM),
San Jose, CA, USA, pp.35-40, 2014.
[5] C. T. Kao, A. -Y. Kuo and Y. Dai,
"Electrical/thermal co-design and co-
simulation, from chip, package, board to
system,", 2016 International Symposium on
VLSI Design, Automation and Test (VLSI-
DAT), Hsinchu, Taiwan, pp.1-4, 2016.
[6] Yi. Jia , F. Xiao, Ya. Duan , Yi Luo , Bi. Liu ,
Y. Huang. “PSpice-COMSOL-Based 3-D
Electrothermal–Mechanical Modeling of IGBT
Power Module, IEEE Journal of Emerging and
Selected Topics in Power Electronics, vol. 8,
No. 4, pp.4173-4185, 2020.
[7] K. Mohamad Ali, R. Sommet, S. Mons, E.
Ngoya. “Behavioral Electro-thermal Modeling
of Power Amplifier for System-Level Design”,
Intern. Workshop on Integrated Nonlinear
Microwave and Millimeterwave Circuits
(INMMIC-2018), Brive La Gaillarde, France,
pp.1-3, 2018.
[8] L. Codecasa, V. d’Alessandro, A. Magnani, A
Irace. “Circuit-Based Electrothermal
Simulation of Power Devices by an Ultrafast
Nonlinear MOR Approach”, IEEE
Transactions on Power Electronics, Vol.31,
No. 8, pp.5906-5916, 2016.
[9] Dan Eddleman, “LTspice: SOAtherm Support
for PCB and Heat Sink Thermal Models” ,
[Online]. https://www.analog.com/en/technical-
articles/ltspice-soatherm-support-for-pcb-and-
heat-sink-thermal-models.html (Accessed Date:
April 1, 2023). Tutorial: ngspice electro-
thermal simulation, [Online].
http://ngspice.sourceforge.net/ngspice-
electrothermal-tutorial.html (Accessed Date:
March 3, 2023).
[10] Byron Blackmore, “Electrothermal circuit
simulation enabled by VHDL-AMS thermal
netlists”, [Online].
https://blogs.sw.siemens.com/simcenter/electrot
hermal-simulation-thermalnetlist-vhdl-ams-
flotherm/ (Accessed Date: December 8, 2023).
[11] Byron Blackmore, “The future of thermal
design – earlier electrothermal analysis”, 2020,
[Online].
https://blogs.sw.siemens.com/simcenter/future-
of-thermal-design-electrothermal-modeling-bci-
rom-vhdl-ams/ (Accessed Date: March 1,
2023).
[12] Kojima, T., Nishibe, Y., Yamada, Y., Ueta, T.,
Torii, K., Sasaki, S., & Hamada, K. (2006,
June). Novel electro-thermal coupling
simulation technique for dynamic analysis of
HV (hybrid vehicle) inverter. In 37th IEEE
Power Electronics Specialists Conference, Jeju,
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
133
Volume 22, 2023
Korea (South), 2006, pp.1-5, doi:
10.1109/pesc.2006.1712076.
[13] Van Cappellen, L., Deckers, M., Alavi, O.,
Daenen, M., & Driesen, J. (2022, September).
A Real-time Physics Based Digital Twin for
Online MOSFET Condition Monitoring in PV
Converter Applications. In 28th International
Workshop on Thermal Investigations of ICs and
Systems (THERMINIC), Dublin, Ireland, pp. 1-
4, 2022. doi:
10.1109/THERMINIC57263.2022.9950636.
[14] Zhongfu Zhou, M.S. Kanniche, S. G. J. Batcup,
Petar Igic, “High-speed electro-thermal
simulation model of inverter power modules for
hybrid vehicles”, IET Electric Power
Applications, vol.5(8), pp.636-643, 2011.
[15] Ma K.and Blaabjerg F., “Multi-timescale
modeling for the loading behaviors of power
electronics converter”, presented at the IEEE
Energy Conversion Congress and Exposition
(ECCE 2015), Montreal, Quebec, Canada,
pp.5749–5756, 2015.
[16] J. Urkizu, M. Mazuela, A. Alacano, et al,
Electric Vehicle Inverter Electro-Thermal
Models Oriented to Simulation Speed and
Accuracy Multi-Objective Targets, Energies,
MDPI, vol.12(19), pp.1-29, 2019.
[17] Petrosyants K.O., Kharitonov I.A., Ryabov
N.I., “Electro-Thermal Design of Smart Power
Devices and Integrated Circuits”, Advanced
Materials Research, vol.918, pp.190-194. 2014.
[18] Igor Kharitonov, Gleb Klopotov, Valentin
Kobyakov, Michael Tegin, Evelina Silchenko,
Konstantin Ivlev, Dmytry Loktionov,
“Extension of the capabilities of SPICE
analysis tools for electro-thermal simulation of
power electronic circuits”, 2022 Moscow
Workshop on Electronic and Networking
Technol. (MWENT). Moscow, Russia. pp.1-5,
2022.
[19] Simulate real-world designs, devices, and
processes with multiphysics software from
COMSOL, [Online]. https://www.comsol.com
(Accessed Date: December 4, 2022).
[20] The Spice Page (by Jan M. Rabaey),
[Online].http://bwrcs.eecs.berkeley.edu/Classes
/IcBook/SPICE/ (Accessed Date: June 20,
2021).
[21] Asonika Tool, [Online]. https://asonika-
online.ru (Accessed Date: October 18, 2022).
[22] IRFB4615PbF datasheet, International
Rectifier, 2008, [Online].
https://www.alldatasheet.com/view.jsp?Search
word=IRFB4615PBF&sField=4 (Accessed
Date: December 8, 2023).
[23] Wakefield-Vette OMNI-UNI-30-50-D,
[Online].
https://eu.mouser.com/ProductDetail/Wakefield
-Vette/OMNI-UNI-30-50-D (Accessed Date:
February 3, 2023).
[24] Ceccarelli L., Kotecha R. M., Bahman A. S.,
Iannuzzo F., Alan H.. “Mission-Profile-Based
Lifetime Prediction for a SiC MOSFET Power
Module Using a Multi-Step Condition-Mapping
Simulation Strategy”, IEEE Transactions on
Power Electronics. vol.34, pp.9698-9708,
2019.
Contribution of Individual Authors to the
Creation of a Scientific Article (Ghostwriting
Policy)
- Konstantin Petrosyants - the methodology of
electro-thermal analysis and simulation of power
circuits on PCB development and convergence
analysis of Section I, Section II.
- Igor. Kharitonov was responsible for the scheme of
software tools interactions for electro-thermal
modeling and simulation and executed the IR
experiments of Section III.
- Mikhail S. Tegin was responsible for the SPICE,
COMSOL simulation and simulation results
analysis of Section III.
Sources of Funding for Research Presented in a
Scientific Article or Scientific Article Itself
The study was carried out within the strategic project
"Digital Transformation: Technologies, Effects and
Performance", part of the HSE University "Priority
2030" Development Programme".
Conflict of Interest
The authors have no conflicts of interest to declare.
Creative Commons Attribution License 4.0
(Attribution 4.0 International, CC BY 4.0)
This article is published under the terms of the
Creative Commons Attribution License 4.0
https://creativecommons.org/licenses/by/4.0/deed.en_
US
WSEAS TRANSACTIONS on CIRCUITS and SYSTEMS
DOI: 10.37394/23201.2023.22.14
Konstantin O. Petrosyants,
Igor A. Kharitonov, Mikhail S. Tegin
E-ISSN: 2224-266X
134
Volume 22, 2023