AN90053
Rev. 1.0 — 31 May 2024

Application note

Advanced SPICE models for Nexperia
cascode Gallium Nitride (GaN) FETs

Abstract:

This application note presents Nexperia's advanced SPICE models for cascode GaN FETs. Detailsof the model versions and structures are included together with their application in circuit simulations.
Comparisons of the simulation results and actual measurement data are provided, showing an excellent
fit. Guidance on using the models is given e.g. solving convergance issues.

Keywords:

SPICE, GaN, electrothermalAN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

1. Introduction
Recently Nexperia released an advanced SPICE model for the new GAN039-650NBB device withextended precision. The advanced SPICE model has the following features:
•
•
•
•
•
•

High quality fitting to experimental DC, AC and transient characteristics
Frequency-dependent parasitic inductances of package interconnections (skin-effect)
Leakage currents and drain-source breakdown modeling
Model is fitted across full temperature range: -55 to 175 °C
Smooth current characteristics, including their derivatives, across the whole voltage andtemperature range
Dynamic electrothermal version of the model – first GaN cascode electrothermal model on themarket.

2. Available versions
Models are currently available for using in two simulators – LTspice and SIMetrix. They are
encrypted due to advanced modelling techniques used to create them. For all simulators there are
3 versions of the same model:
Table 1. Model versions
VersionDescription

Name format

Isothermal

Electrical model with
global temperaturedependence, local
temperature of device
equal to the global
temperature andremains constantduring transient
analysis.

part_name.asy

4Isothermal
without
package strayinductances

Electrical model with
global temperaturedependence

part_name_NO_IND.asy

3

Electrothermal

Electrical model with
part_name_ETH.asy
dynamic thermal
capability that includes
self-heating of thedeviceLTspice symbol

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

SIMetrix symbol

Pins

5

© Nexperia B.V. 2024. All rights reserved

2 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

3. Internal structures of the model versions
Isothermal electric model.
Fig. 1 shows the basic variant of the model, and it should be used at the main design stage with
global fixed temperature. It consists of a GaN FET connected in series with a low-voltage power
MOSFET, including body diode, and frequency-dependent (skin effect) parasitic inductances andresistances of the package. The mounting base terminal, MB, is internally connected to the source
and may be left unconnected in the simulation schematic, or it may be connected to impedances
which model the physical MB connection.

Fig. 1.

Internal structure of the cascode Isothermal electric model

Cascode Isothermal electric model without parasitic inductances.
This model version allows you to speed up simulation time as well as define package parasitics
externally to get access to internal nodes of the device, see Fig. 2.

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

3 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Fig. 2.

Internal structure of the cascode Isothermal electric model without parasitic
inductances

Electrothermal modelFig. 3 shows the Electrothermal version which has a built-in Cauer thermal network the valuesof which are fitted to Zth experimental data. Each internal device has its own source of heat, that
produces real active heat loss power.

Fig. 3.

Internal structure of the cascode Electrothermal model

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

4 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

4. Fitting accuracy of the new advanced models
The characteristic curves generated using the new advanced models show an excellent match withthe measured values. See Fig. 4, Fig. 5, Fig. 6 and Fig. 7.

Fig. 4.

Ciss, Crss and Coss as a function of drain-source voltage; solid = experiment, dashed = model

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

5 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Fig. 5.

Drain-source on-state resistance as a function of gate-source voltage at different temperatures (-55, 25,
85, 125, 175°C); solid = experiment, dashed = model

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

6 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Fig. 6.

Drain-source current as a function of gate-source voltage (pulsed); solid = experiment, dashed = model

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

7 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Fig. 7.

Transient termal impedance as a function of time; solid = experiment, dashed = model

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

8 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

4.1. Application tests of the new advanced model
The measured and simulated power loss and efficiency curves are shown in Fig. 8 and Fig. 9,
using the circuit and conditions given in Table 2.
Table 2. Buck-mode configuration
Parameter
Value / Range

Circuit diagram

output power

150 - 4800 W

test inductor

330 µH MPP toroid

VDD

400 V

Vout

230 V

VGS

0 - 12 V

RG

15 Ω

gate ferrite bead30Ω @ 100 MHz (std. BLM type)

Tamb

22 °C

fswitching

100 kHztdead

100 nsNote: Simulation uses experimental temperature data ofeach cascode device and also takes into consideration theload inductor core losses in its final calculations. Core losses
are calculated using the core manufacturer's method thattakes into account nonlinear magnetization and current ripple
oscillation frequency.

Fig. 8.

Simplified schematic of the test
circuit used for the efficiency sweep
See UM90028 for details.

Power loss as a function of output power; experiment vs model

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

9 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Fig. 9.

Efficiency as a function of output power; experiment vs model

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

10 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

5. Adding a model to the simulator
5.1. LTspice
Models can be used in two ways in LTspice:
1. Place the symbol .asy and library .lib files into the same folder as your circuit, see Fig. 10:

Fig. 10. Menus in LTspice, selecting the component using the symbol browser
Place symbol via menu Edit->Component->Select your folder in Top Directory menu-> Selectsymbol you want to add and place onto schematics.
Include the library file by using the .include statement with this syntax:
a. include <filename> where filename is the full path to libraryb. if .lib files are placed into the schematic directory, including .lib extension, entering the fullname is enough.

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

11 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs
2. Place symbol .asy and library .lib files into any directory you want and then add that directory
into search paths for symbols and libraries in menu Tools->Control Panel->Sym. and Lib.
Search Paths, see Fig. 11:

Fig. 11. Menus in LTspice, adding symbol and library search paths
Now you can access symbols in the same way as method 1), but now you don't need to
explicitly put “.include” statement onto schematic because the library file is already in search
path of LTspice and the name of that file is already in symbol attribute 'ModelFile', see Fig. 12.

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

12 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Fig. 12. Menus in LTspice, attribute properties of device symbol

5.2. SIMetrix
To use the models in SIMetrix follow these steps:
1. Import lib file: File -> Model Library -> Add/Remove Libraries -> Select Spice File folder -> Ok(or directly drag the model file into the command window of SIMetrix which is located in bottomleft corner by default), see Fig. 13:

Fig. 13. Menus in SIMetrix, adding library into SIMetrix.

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

13 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs
2. Import Symbol file: File -> Symbol Manager -> Add -> Select *.sxslb File -> Ok (or use filedragging as in previous step). see Fig. 14 and Fig. 15:

Fig. 14. Menus in SIMetrix, adding symbol into SIMetrix

Fig. 15. Menus in SIMetrix, adding symbol into SIMetrix; 2

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

14 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs
3. Associate Symbol file: File -> Model Library -> Associate models and symbols -> New Category-> Define Symbol -> Ok. See Fig. 16.

Fig. 16. Menus in SIMetrix, associate symbol with library file

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

15 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

6. Example of an application simulation using the base modelFig. 17 shows a double-pulse test circuit using a low-side switch. Here we use the standard model
without the dynamic thermal part. The simulation results are shown in Fig. 18.The default test
conditions are:
•
•
•
•
•

VDD = 400 V
Lpower_loop = 2.35 nH
IF = 20 A
RG =15 Ω
30 Ohm BLM ferrite beadFig. 17. Double pulse circuit in LTspice

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

16 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Fig. 18. Results of circuit simulation in LTspice

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

17 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

7. Using electrothermal models
The electrothermal models can be used in different ways, but you must remember that thermal andelectrical circuits are different from each other and can’t be mixed.
There are three correct ways to use electrothermal models:
1. The TMB node is connected to a constant voltage source with a value that represents constantambient temperature. If you connect TMB directly to this source, we will assume that theheatsink is ideal and is kept at constant temperature, while the junction temperature of device
could be different from ambient, see Fig. 19.

Fig. 19. Standard usage of electrothermal model in LTspice
2. Both TMB and TJ are connected to a constant voltage source. In this case we fix thetemperature of the device at the value of the voltage source, see Fig. 20.

Fig. 20. Fixed temperature usage of electrothermal model in LTspice

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

18 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs
3. You can connect TMB node to an external thermal circuit that represents a simple thermal
model of the heatsink, see Fig. 21.

Fig. 21. External thermal part usage together with electrothermal model in LTspice
Also, if you have multiple devices on the board, you can set the individual temperature of eachdevice, see Fig. 22:

Fig. 22. Setting different fixed temperatures for each device in LTspice
This could be helpful if you have already measured steady-state temperatures of individual
devices from the PCB and want to check the simulation result at the same conditions, without
the necessity to wait until the transient simulation reaches steady-state condition.
Caution 1: Do not leave TMB floating in transient analysis and connect both TJ and TMB to
fixed temperature source in DC/AC characterization analysis to avoid overheating of device.
Caution 2: use the startup option in transient modeling mode with caution for electrothermal
models, because in this mode all sources start from zero, including the temperature source, as
it takes a long time to reach the actual value due to large time constants in the thermal analysis.

7.1. Example of simulation with electrothermal model
In this example you can see the long simulation with external thermal resistor connected between
TMB node and ambient temperature source that represents thermal resistance from mounting basepoint to ambient, see Fig. 23.

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

19 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Fig. 23. Example of electrothermal model usage in LTspice
Since the time constant of thermal RC-network is in the order of seconds, we must simulate
circuits for a long time to reach the steady-state condition. In this case the temperature has settled
after about 2s of simulation time, see Fig. 24. Such simulations could be very time and resource
consuming and should be done at the final stage of thermal design verification.

Fig. 24. Result of electrothermal simulation in LTspice
In order to significantly reduce the simulation time, you could loosen some tolerances to achieve
faster convergence, for example in this case the following settings were used:.options method=gear reltol=0.003 chgtol=1e-12 abstol=1e-9 trtol=6
vntol=1e-4 gmin=1e-9 noopiter gminsteps=0

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

20 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs
You should also keep in mind that these settings could introduce some error in the final settled
temperature, but it is usually no more than 1°C. Also, in such long simulations the size of the output
data could be very large, so it is helpful to make sure that compressing of transient waveforms is
selected on in this tab, see Fig. 25:

Fig. 25. Compression tab in LTspice
The other option to reduce saved data is set for saving only necessary node voltages, in this case
we save only V(thtsnk) and V(tj) with this command:.save v(tj1) v(thtsnk)

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

21 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

8. Convergence settings and how to solve convergence issues
8.1. General recommendations (applies to all simulators)
1. Use realistic models for all circuit components as much as possible:• Add realistic resistors in series with inductors, even for ones representing parasitic
resistance of wires/PCB tracks.
• Use proper models for decoupling/bypass/load capacitors with resistance (ESR) and
inductance (ESL) in series:

Fig. 26. Possible model of capacitor with parasitics included•

Add resistance in series with power supply source/waveform generator source such that it
models the finite resistance of real power supply.

2. It is good practice to make sure that at start of the transient analysis all gate-controlled devices
are in the off state, it gives better performance during DC solution searching before start oftransient.
3. In circuits with strong oscillations during switching the convergence could be improved byswitch integration method from trap (most accurate single-step method) to gear (multistep
method) that is more stable but provides additional damping. The Gear method is especiallyhelpful when used with electrothermal models.

8.2. LTspice recommendations
1. If you observe non-physical voltage/current spikes or error “Time step too small”, you could
turn on alternate solver that has significantly higher accuracy (you could do this through Tools>Control Panel->SPICE).
2. Increase abstol and vntol to aid faster convergence during DC analysis, including initialconditions analysis prior to transient analysis, the upper limits are 1e-9 for abstol and 1e-4 forvntol.
3. Increase ITL1 and ITL4 up to 500, these settings represent the number of iterations per solution
point for DC and transient analysis correspondingly.
4. Set noopiter flag and gminsteps=0 to skip initial Newton iterations and Gmin stepping algorithm.
It helps with the accuracy of the initial DC solution prior to transient simulation. A bad initialsolution could lead to bad convergence or error in the transient analysis.
5. If you experience difficulties in finding the DC solution before transient analysis, you could turnon the startup option in TRAN settings. Caution: this does not work well with electrothermal

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

22 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETsmodels because temperature voltage source also starts from zero, and overall circuit
temperature will be changing very slowly due to large time constant of thermal system

Fig. 27. Selected startup option in transient simulation option menu
6. Increase chgtol to get faster simulation during transient analysis, up to 1e-12
7. Add cshunt parameter in .option statement, value up to 1e-15, it could get rid of “Time step too
small” error
8. As a last resort you can decrease the maximum time step to force the solver to do smaller time
steps – it could improve stability but increases simulation time.
Template of .options setting:.options abstol=1e-10 vntol=1e-4 ITL1=500 ITL4=100 noopitergminsteps=0 chgtol=1e-12 method=trap chgtol=1e-15

8.3. SIMetrix recommendations
1. Change default iteration model to Extended precision.
2. Set shunt capacitance with value up to 1e-15, it could get rid of “Time step too small” error.
3. As a last resort you can decrease the maximum time step to force the solver to do smaller time
steps – it could improve stability but increases simulation time.
4. If you experience difficulties in finding the DC solution before transient analysis you could turnon the startup option in the TRAN settings.
Caution: it does not work well with electrothermal models because temperature/voltage source
also starts from zero, and overall circuit temperature will be changing very slowly due to large
time constant of thermal process.

9. Revision history
Table 3. Revision history
Revision
Date
numberDescription

1.0

Initial version.

2024-05-31

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

23 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

10. Legal information
Definitions
Draft — The document is a draft version only. The content is still underinternal review and subject to formal approval, which may result in
modifications or additions. Nexperia does not give any representations or
warranties as to the accuracy or completeness of information included hereinand shall have no liability for the consequences of use of such information.

Disclaimers
Limited warranty and liability — Information in this document is believed
to be accurate and reliable. However, Nexperia does not give any
representations or warranties, expressed or implied, as to the accuracy
or completeness of such information and shall have no liability for theconsequences of use of such information. Nexperia takes no responsibility
for the content in this document if provided by an information source outsideof Nexperia.
In no event shall Nexperia be liable for any indirect, incidental, punitive,
special or consequential damages (including - without limitation - lost
profits, lost savings, business interruption, costs related to the removalor replacement of any products or rework charges) whether or not suchdamages are based on tort (including negligence), warranty, breach ofcontract or any other legal theory.
Notwithstanding any damages that customer might incur for any reason
whatsoever, Nexperia’s aggregate and cumulative liability towards customer
for the products described herein shall be limited in accordance with theTerms and conditions of commercial sale of Nexperia.
Right to make changes — Nexperia reserves the right to make changes
to information published in this document, including without limitation
specifications and product descriptions, at any time and without notice. This
document supersedes and replaces all information supplied prior to the
publication hereof.
Suitability for use — Nexperia products are not designed, authorized or
warranted to be suitable for use in life support, life-critical or safety-criticalsystems or equipment, nor in applications where failure or malfunctionof an Nexperia product can reasonably be expected to result in personal
injury, death or severe property or environmental damage. Nexperia and its
suppliers accept no liability for inclusion and/or use of Nexperia products insuch equipment or applications and therefore such inclusion and/or use is at
the customer’s own risk.
Applications — Applications that are described herein for any of theseproducts are for illustrative purposes only. Nexperia makes no representation
or warranty that such applications will be suitable for the specified use
without further testing or modification.
Customers are responsible for the design and operation of their applications
and products using Nexperia products, and Nexperia accepts no liability forany assistance with applications or customer product design. It is customer’ssole responsibility to determine whether the Nexperia product is suitableand fit for the customer’s applications and products planned, as well as
for the planned application and use of customer’s third party customer(s).
Customers should provide appropriate design and operating safeguards tominimize the risks associated with their applications and products.
Nexperia does not accept any liability related to any default, damage, costs
or problem which is based on any weakness or default in the customer’s
applications or products, or the application or use by customer’s third party
customer(s). Customer is responsible for doing all necessary testing for thecustomer’s applications and products using Nexperia products in order toavoid a default of the applications and the products or of the application or
use by customer’s third party customer(s). Nexperia does not accept any
liability in this respect.
Export control — This document as well as the item(s) described herein
may be subject to export control regulations. Export might require a priorauthorization from competent authorities.
Translations — A non-English (translated) version of a document is forreference only. The English version shall prevail in case of any discrepancy
between the translated and English versions.

Trademarks
Notice: All referenced brands, product names, service names andtrademarks are the property of their respective owners.

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

24 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

List of Tables
Table 1. Model versions....................................................... 2
Table 2. Buck-mode configuration........................................9
Table 3. Revision history....................................................23

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

25 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

List of Figures
Fig. 1. Internal structure of the cascode Isothermal
electric model....................................................................... 3
Fig. 2. Internal structure of the cascode Isothermal
electric model without parasitic inductances........................4
Fig. 3. Internal structure of the cascode Electrothermal
model.................................................................................... 4
Fig. 4. Ciss, Crss and Coss as a function of drainsource voltage; solid = experiment, dashed = model...........5
Fig. 5. Drain-source on-state resistance as a functionof gate-source voltage at different temperatures (-55,25, 85, 125, 175°C); solid = experiment, dashed = model... 6
Fig. 6. Drain-source current as a function of gatesource voltage (pulsed); solid = experiment, dashed =model.................................................................................... 7
Fig. 7. Transient termal impedance as a function oftime; solid = experiment, dashed = model........................... 8
Fig. 8. Power loss as a function of output power;
experiment vs model............................................................9
Fig. 9. Efficiency as a function of output power;
experiment vs model..........................................................10
Fig. 10. Menus in LTspice, selecting the component
using the symbol browser.................................................. 11
Fig. 11. Menus in LTspice, adding symbol and library
search paths.......................................................................12
Fig. 12. Menus in LTspice, attribute properties ofdevice symbol.................................................................... 13
Fig. 13. Menus in SIMetrix, adding library into SIMetrix..... 13
Fig. 14. Menus in SIMetrix, adding symbol into SIMetrix... 14
Fig. 15. Menus in SIMetrix, adding symbol into
SIMetrix; 2.......................................................................... 14
Fig. 16. Menus in SIMetrix, associate symbol withlibrary file............................................................................15
Fig. 17. Double pulse circuit in LTspice..............................16
Fig. 18. Results of circuit simulation in LTspice..................17
Fig. 19. Standard usage of electrothermal model in
LTspice................................................................................18
Fig. 20. Fixed temperature usage of electrothermal
model in LTspice................................................................ 18
Fig. 21. External thermal part usage together withelectrothermal model in LTspice.........................................19
Fig. 22. Setting different fixed temperatures for eachdevice in LTspice................................................................19
Fig. 23. Example of electrothermal model usage in
LTspice................................................................................20
Fig. 24. Result of electrothermal simulation in LTspice...... 20
Fig. 25. Compression tab in LTspice.................................. 21
Fig. 26. Possible model of capacitor with parasitics
included.............................................................................. 22
Fig. 27. Selected startup option in transient simulation
option menu....................................................................... 23

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

26 / 27

AN90053

Nexperia

Advanced SPICE models for Nexperia cascode Gallium Nitride (GaN) FETs

Contents
1. Introduction................................................................... 2
2. Available versions........................................................ 2
3. Internal structures of the model versions.................. 3
4. Fitting accuracy of the new advanced models...........5
4.1. Application tests of the new advanced model..............95. Adding a model to the simulator.............................. 11
5.1. LTspice....................................................................... 11
5.2. SIMetrix......................................................................13
6. Example of an application simulation using thebase model....................................................................... 16
7. Using electrothermal models.................................... 18
7.1. Example of simulation with electrothermal model...... 19
8. Convergence settings and how to solve
convergence issues......................................................... 228.1. General recommendations (applies to all simulators) 22
8.2. LTspice recommendations......................................... 228.3. SIMetrix recommendations........................................ 23
9. Revision history..........................................................23
10. Legal information......................................................24© Nexperia B.V. 2024. All rights reserved

For more information, please visit: http://www.nexperia.com
For sales office addresses, please send an email to: salesaddresses@nexperia.com
Date of release: 31 May 2024

AN90053
Submit document feedback

All information provided in this document is subject to legal disclaimers.

Application note

Rev. 1.0 — 31 May 2024

© Nexperia B.V. 2024. All rights reserved

27 / 27