Modeling Power GaN-HEMTs Using Standard MOSFET Equations and Parameters in SPICE

Abstract

The device library in the standard circuit simulator (SPICE) lacks a gallium nitride based high-electron-mobility-transistor (GaN-HEMT) model, required for the design and verification of power-electronic circuits. This paper shows that GaN-HEMTs can be modeled by selected equations from the standard MOSFET LEVEL 3 model in SPICE. A method is proposed for the extraction of SPICE parameters in these equations. The selected equations and the proposed parameter-extraction method are verified with measured static and dynamic characteristics of commercial GaN-HEMTs. Furthermore, a double pulse test is performed in LTSpice and compared to its manufacturer model to demonstrate the effectiveness of the MOSFET LEVEL 3 model. The advantage of the proposed approach to use the MOSFET LEVEL 3 model, in comparison to the alternative behavioral-based model provided by some manufacturers, is that users can apply the proposed method to adjust the parameters of the MOSFET LEVEL 3 model for the case of manufacturers who do not provide SPICE models for their HEMTs.

1. Introduction

Gallium nitride (GaN)-based high-electron-mobility transistors (HEMTs) are emerging as a promising power switching device for high-efficiency, high-density, and high-frequency power converters [1]. Compared to the Si counterparts, GaN-based power devices offer higher breakdown voltage and higher thermal conductivity [1]. These excellent properties enable GaN-based power devices to meet the high-performance requirements for modern power converters.

For any power-conversion application, the power circuit designers have to evaluate the impact of the power-semiconductor devices used in the circuits. From an optimization point-of-view, there is a need to reduce the number of hardware prototypes. Therefore, simulation tools are gaining more attention in the development of power electronic systems [2]. Many researchers are evaluating the high-power and high-frequency circuits with GaN-HEMT using various device models [1,2,3]. Hence, accurate modeling of GaN-HEMTs is an important research area for the simulation of power electronic systems. Various modeling approaches for GaN-HEMTs are available in the literature and are classified into four categories [1,3,4]: Behavioral models, semiphysics-based models, physics-based models, and numerical models. Numerical modeling requires detailed information regarding internal structure, device geometry, and material properties of the GaN-HEMT and uses complex simulation tools such as SILVACO, TCAD, et cetera [5,6]. The accuracy of numerical models is very good but complexity is very high and computation is very intensive [1]. The physics-based models involve solving semiconductor physics equations in order to obtain the electrical behavior of GaN-HEMTs [7,8,9,10,11]. However, these models are not suitable for power electronics simulation because of the complex parameter extraction and long computational time [1,4]. Semiphysics-based models are partly based on behavioral equations and partly on semiconductor physics [12,13,14,15]. The models are accurate, fast, and applicable to different devices from the same class even though some of their empirical parameters lack physical meaning [1]. A popular modeling approach is to fit mathematical equations to experimental data without any information about the physical mechanism of operation, which is an approach called behavioral modeling [16,17,18,19,20]. The major advantage of behavioral models is their computational efficiency [1,4]. However, when the operating conditions are changing, the accuracy of behavioral models is quite low [3]. Since, the exact information of internal parameters, device structure, device geometry, and material properties are unknown and very difficult to obtain by a power-electronics engineer, the numerical and physics-based models are unpractical [4]. The issues with the behavioral models are that they do not perform well in all operating conditions and cannot be adapted to different devices from the same class. Hence, for accuracy and computational speed, this paper utilizes semiphysics-based model developed in the Simulation Program with Integrated Circuit Emphasis (SPICE) for modeling GaN-HEMTs.

Among many simulation platforms that are used for designing and evaluating circuits, SPICE is widely used by researchers and manufacturers. Another reason for the popularity of SPICE is because almost all the semiconductor manufacturers provide free SPICE behavioral models for their discrete semiconductor devices. The standard SPICE library of devices was developed at the time when the focus was on bipolar-junction transistors (BJTs), junction field-effect transistors (JFETs), and metal-oxide-semiconductor field-effect transistors (MOSFETs). Because of that, it does not include a library model for the GaN-HEMTs. Given the need to simulate circuits with GaN-HEMTs, GaN manufacturers such as GaN Systems, Efficient Power Conversion Corporation (EPC), Transphorm, et cetera, provide behavioral-based SPICE models in the form of sub-circuits for their respective GaN-HEMTs. Furthermore, many researchers have proposed GaN-HEMT models that can be incorporated into SPICE [2,4,12,15,16,20]. However, these SPICE models are obscure and are not transparent. Furthermore, a large number of fitting parameters makes use of these models difficult. In addition, some of these models create convergence problems, require extensive computational time, and are not easily adaptable to other GaN-HEMTs. Endruschat et al. [2] investigated the possibility of using the MESFET equation in SPICE (Curtice model), but they showed that its use as a GaN-HEMT model required modification by the introduction of non-physical parameters. The modified Curtice equations turn into a behavioral model; they are analytical equations solved using tabular data obtained from either the measurements or datasheet. However, the discrete nature of the tabular data and the uneven arrays create convergence problems [21].

To address these problems, we show in this paper that the standard MOSFET LEVEL 3 model in SPICE can be utilized to model GaN-HEMTs. This is achieved by the following key contributions:

• Selection of relevant equations from the quite complex set of equations comprising the MOSFET LEVEL 3 model in SPICE.
• Development of a verified method to extract the initial values of all SPICE parameters in the selected equations, which is necessary to enable proper nonlinear fitting to measured characteristics of an arbitrary GaN-HEMT.

This paper is divided into the following sections: Section 2 will introduce the GaN structure studied in this paper. Section 3 will present the selection of static equations and the method for respective parameters extraction. Section 4 and Section 5 will verify the experimental static and dynamic characteristics, respectively. Section 6 will present the results of a double-pulse test (DPT) test to compare the effectiveness of the MOSFET LEVEL 3 model with the manufacturer model in LTSpice. Section 7 will conclude and foreshadow potential future work.

2. GaN Structure

The internal structure of a normally-off GaN-HEMT is shown in Figure 1 [22]. For HEMT fabrication on the silicon substrate, as is the case in the structure shown in Figure 1, aluminum nitride is used as a buffer layer to enable epitaxial growth of the active GaN layer. The formation of the two-dimensional electron gas (2-DEG) is achieved by the growth of a resistive AlGaN layer on top of the highly-resistive GaN layer. The transition from GaN to AlGaN creates polarization charge, which attracts mobile electrons that form the 2-DEG. To form a normally-off HEMT, which is required for power applications, the electrons under the gate are repelled by various techniques, such as embedding negative charge in the AlGaN layer and using gate materials with a suitable work function. Given that a positive gate voltage is needed to re-establish the 2-DEG under the gate, this region of the HEMT is analogous to a normally-off MOSFET. The gate-to-drain and gate-to-source regions are different from the MOSFET structure; however, they can be modeled as fixed drain and source resistances.

The switching ability of power devices depend on its parasitic capacitances, which are gate-to-source capacitance (C_GS), gate-to-drain capacitance (C_GD), and drain-to-source capacitance (C_DS). The three parasitic capacitances, shown in Figure 1, are analogous to the parasitic capacitances in the MOSFET structure. An important quantitative difference is that the parasitic capacitances in HEMTs are much smaller, enabling operation at much higher switching frequencies. A major difference between GaN-HEMT and MOSFET is the lack of an intrinsic body diode. However, the intrinsic diode in MOSFET models can be easily eliminated by adopting zero values of its key parameters. Therefore, standard MOSFET equations can be applied to GaN-HEMTs.

3. Selection of Static Equations and Parameter Extraction

3.1. Selection of SPICE Equations

Modeling a GaN-HEMT requires mathematical equations for the drain current (I_D) as a function of the applied gate-to-source (V_GS) and drain-to-source (V_DS) voltages. In SPICE, there are different sets of equations, referred to as model levels. LEVEL 1 is the simplest MOSFET model, which is based on the rudimentary device equations. Shah et al. [12] have used the equations of MOSFET LEVEL 1 to model GaN-HEMTs. However, their approach ignored the transfer characteristic for small V_DS values, which in the case of any GaN-HEMT is impacted by the channel resistances outside the gate (these gate-to-source and gate-to-drain channel resistances do not exist in MOSFETs). In addition, the simulation accuracy of output characteristics is highly dependent on second-order effects, which are not included in [12]. The MOSFET LEVEL 2 model in SPICE includes second-order effects, but its equations are complex resulting in computational inefficiency and convergence issues. MOSFET LEVEL 3 is a much better choice, because its key equations are almost as simple as in MOSFET LEVEL 1 and as accurate as the complex equations in the MOSFET LEVEL 2 model. Therefore, the MOSFET LEVEL 3 model is utilized in this paper. In SPICE, a parameter labeled as LEVEL is assigned to MOSFET devices. By assigning LEVEL = 3, the SPICE LEVEL 3 model with the relevant equations and parameters is activated.

Equations (1) and (2), shown below, represent our selection from the rather complex MOSFET LEVEL 3 model, for the purpose of modeling GaN-HEMTs. The SPICE parameters that need to be specified to activate this selection are shown in the bold font. The list of these parameters is as follows: the transconductance parameter (KP), the threshold voltage (Vto), the channel length (L), the channel width (W), the drain resistance (Rd), the source resistance (Rs), the body-effect parameter (Gamma), the surface potential in strong inversion (Phi), and the mobility modulation constant (Theta). In this paper, we will also show that the subthreshold-current parameter (NFS) can be used to model the non-zero drain current for gate voltages below the threshold voltage. The default values of the remaining SPICE parameters ensure that all other equations are inactive [23].

$$\begin{gathered} I_D=\frac{\mathit{K}\mathit{P}}{1+\mathit{T}\mathit{h}\mathit{e}\mathit{t}\mathit{a}(V_{GS}-\mathit{V}\mathit{t}\mathit{o})}\frac{\mathit{W}}{\mathit{L}}(V_{GS}-\mathit{V}\mathit{t}\mathit{o})(V_{DS}-\mathit{R}\mathit{s}{I}_D-\mathit{Rd}{I}_D)-\left[1+\frac{\mathit{Gamma}}{2\sqrt{\mathit{Phi}}}\right]\frac{{(V_{DS}-\mathit{Rs}{I}_D-\mathit{Rd}{I}_D)}^2}{2} \\ \mathrm{Triode}\mathrm{Region} \end{gathered}$$

(1)

$$I_D=\frac{\mathit{KP}}{1+\mathit{Theta}(V_{GS}-\mathit{Vto})}\frac{\mathit{W}}{\mathit{L}}\left[\frac{2\sqrt{\mathit{Phi}}}{2\left(2\sqrt{\mathit{Phi}}+\mathit{Gamma}\right)}\right]{(V_{GS}-\mathit{Vto})}^2\times \mathrm{Saturation}\mathrm{Region}$$

(2)

3.2. Methods for Extraction of Initial Values of the Selected Parameters

In principle, the values of equation parameters can be obtained by nonlinear fitting to experimental data. However, the convergence of nonlinear fitting entirely depends on the specified initial values of the equation parameters. More importantly, an inadequate choice of the initial values can lead to poor fitting. Hence, this paper proposes a method for extraction of the initial values of selected key parameters as the first step, followed by nonlinear fitting to adjust the values of all parameters in Equations (1) and (2).

The channel length and width, L and W, are the geometric-design parameters specific to the power device under test. For commercial power-semiconductor devices these values are undisclosed by the manufactures and are very hard to determine. However, for the purpose of circuit simulation, it is sufficient to set the value of W and L to 1 µm, which makes the ratio W/L = 1. That leaves the transconductance parameter KP as the active parameter whose value will determine the value of the drain current in response to the applied voltages. In addition to KP, the initial values of Vto, Rs, and Rd are also needed to enable successful nonlinear fitting. Therefore, the proposed method for the extraction of initial parameter values includes KP, Vto, Rs, and Rd. The values of the remaining parameters can be adjusted by nonlinear fitting using their typical or default values.

3.2.1. Extraction of KP, and Vto

The values of KP and Vto can be determined from measured transfer characteristic of the corresponding GaN-HEMT, biased in the linear region by a small V_DS, such as V_DS = 100 mV. To illustrate the extraction method, we chose a commercial 600 V GaN power transistor, GS66504B, manufactured by GaN Systems. The transfer characteristic of GS66504B was measured with an Agilent Power Device Analyzer (B1505A) and is shown in Figure 2. This transfer characteristic was measured at V_DS = 100 mV to ensure that the quadratic term in (1) is negligible. In the linear section of the measured transfer characteristic, marked by the dashed line in Figure 2, the values of Theta(V_GS-Vto), RsI_D, and RdI_D are negligible, simplifying (1) to the following linear form:

$$I_D=\mathit{KP}\left(\mathit{W}/\mathit{L}\right)(V_{GS}-\mathit{Vto})V_{DS}$$

(3)

Equation (3) shows that the intersection between the extrapolated linear section of the measured transfer characteristic and the V_GS axis that corresponds to Vto = 1.26 V. The slope of the linear section is 0.879 A/V, which corresponds to KP = 8.79 A/V² for the specific case of V_DS = 100 mV and W = L = 1 µm.

3.2.2. Extraction of Rs, and Rd

As Figure 2 shows, the measured transfer characteristic deviates from the linear dependence (the dashed line) for higher V_GS and I_D values, mainly due to the impact of the channel resistances outside the gate. MOSFET LEVEL 3 model has embedded source and drain resistances, Rs and Rd, which we can use to model the impact of gate-to-source and gate-to-drain channel resistances in HEMTs as shown in Figure 3. Assuming that the dashed line in Figure 2 corresponds to the HEMT channel under the gate, we can model this section of the channel by the linear equation:

$$I_D=\beta (V_{GS0}-\mathit{Vto})V_{DS0}$$

(4)

where, β = KP(W/L), V_DS0 = V_DS − (Rs + Rd) I_D, and V_GS0 = V_GS − RsI_D. From Equation (4), V_GS0 can be expressed as:

$$V_{GS0}=\left(I_D/\beta V_{DS0}\right)+\mathit{Vto}$$

(5)

For smaller I_D values, where the solid and dashed lines overlap, (Rs + Rd) I_D is negligible and V_GS0 = V_GS. However, for larger I_D values, (Rs + Rd) I_D is not negligible and a larger V_GS is required to achieve the same I_D. According to Equation (3), the measured value of V_GS is given by

$$V_{GS}=\left(I_D/\beta V_{DS}\right)+\mathit{Vto}$$

(6)

The difference ΔV_G = V_GS0 − V_GS, which is illustrated in Figure 2, can be obtained from (5) and (6) as:

$$\Delta V_G=\frac{I_D}{\beta }\left[\frac{1}{V_{DS}-(\mathit{Rs}+\mathit{Rd})I_D}-\frac{1}{V_{DS}}\right]$$

(7)

$$\Rightarrow \mathit{Rs}+\mathit{Rd}=\frac{V_{DS}}{I_D}-\frac{1}{\left(I_D/V_{DS}\right)+\beta \Delta V_G}$$

(8)

Practically, a sufficiently high I_D should be selected for the determination of Rs + Rd, because a sufficiently large ΔV_G is needed to avoid a large error in the determined value for Rs + Rd. For the specific data shown in Figure 2, ΔV_G = 0.8 V, V_DS = 100 mV, I_D = 0.84 A, and consequently Rs + Rd is obtained as 54.3 mΩ. For simplification of the model we assume equal drain and source resistances, which are Rs = Rd = 27.15 mΩ.

3.2.3. Typical Initial Values for Gamma, Phi, Theta, and NFS

Two parameters, Gamma and Phi, impact the drain current in the triode and saturation regions. The complete MOSFET LEVEL 3 equations in SPICE use Gamma and Phi to model second-order effects that we do not need in the case of HEMT modeling. As can be seen from the square brackets in Equations (1) and (2), it is sufficient to adjust the value of only one of these parameters. From semiconductor physics, we know that the value of Phi is set by the energy gap of the material. For the case of GaN, we can set Phi = 2 V, which leaves Gamma to be determined by the nonlinear fitting. For this purpose, the default value in SPICE, which is Gamma = 0, can be used as the initial value.

The default value for the parameter Theta in SPICE is also Theta = 0. This is sufficient as the initial value for the nonlinear fitting, which will adjust the final value of Theta to improve the fitting of both the transfer and the output characteristics. Finally, note that we can specify the parameter NFS to fit the subthreshold current on the transfer characteristic. The typical value of this parameter is 10¹¹ cm⁻². However, in the triode and saturation region, the NFS does not affect the I_D as can be seen from Equations (1) and (2). Hence, the value of this parameter can be adjusted in SPICE simulation after the non-linear fitting is completed.

3.3. Non-Linear Fitting

Using the set values of W = L = 1 µm and Phi = 2 V, along with the initial values obtained in the previous sub-section (KP = 8.79 A/V², Vto = 1.26 V, Rs = Rd = 27.15 mΩ) and the default values Theta = 0, and Gamma = 0, non-linear fitting is applied to Equations (1) and (2) to obtain the MOSFET LEVEL 3 parameters for GS66504B. The obtained fitted parameters are typed directly into SPICE and are verified by the experimental transfer and output characteristics as described in the next section. Note that, without NFS, the drain current calculated by SPICE will be zero for V_GS < Vto. Hence, in order to fit the sub-threshold region for GS66504B, the value of NFS can be determined by running SPICE simulations with tried numbers around its typical value of 10¹¹ cm⁻².

4. Experimental Verification of the Static Characteristics

In addition to GS66504B GaN-HEMT, we have also selected a 650 V GaN transistor GS66506T to demonstrate the effectiveness of the selected MOSFET LEVEL 3 equations and the proposed parameter-extraction method. Putting the fitted values of the selected parameters directly into SPICE, the simulated transfer and output characteristics for both GS66504B and GS66506T are compared with the measured results in Figure 4. It is evident that SPICE simulations are in very good agreement with the measured results, which demonstrates that the selected MOSFET LEVEL 3 equations in SPICE can be used to model GaN-HEMTs. Precise modeling in the linear region of the output characteristics, shown in Figure 4b,d, is the most significant, as it corresponds to the operation of HEMTs as switches in on mode and thus, determines the on-state resistance.

5. Modeling Dynamic Characteristics and Experimental Verification

The dynamic characteristics of GaN-HEMTs are determined by their inherent voltage-dependent parasitic capacitances. For the designers of power-conversion circuits, the capacitance of utmost interest is the output capacitance, C_OSS = C_DS + C_GD. Hence, modeling of C_DS and C_GD is crucial. The desired individual capacitance data from the datasheet is extracted using the grabit.m command in MATLAB and is shown in Figure 5.

The MOSFET LEVEL 3 model includes voltage-independent gate-to-source and gate-to-drain overlap capacitances, through Cgso and Cgdo as the respective parameters. By observing the datasheets of many GaN-HEMTs, it can be perceived that the C_GS and C_GD are fairly constant for most of the voltage ranges; hence the voltage-independent parameters Cgso and Cgdo can be used to model these capacitances. Note that Cgso and Cgdo are defined as capacitances per unit of the channel width. Therefore, extracting the values of Cgso and Cgdo can be achieved by taking the values of C_GS and C_GD at the maximum V_DS.

The MOSFET LEVEL 3 model also contains a diode model for the MOSFET P‒N junction, which can be utilized to model the non-linear C_DS for GaN-HEMTs. The diode model with relevant SPICE parameters is given by

$$C_{DS}(v_{DS})=\mathit{Cj}{\left[1+\left(v_{DS}/\mathit{PB}\right)\right]}^{-\mathit{M}\mathit{j}}$$

(9)

where, Cj is the zero-bias capacitance per unit area, PB is the built-in voltage, and Mj is the grading coefficient. To obtain the values of these SPICE parameters requires non-linear fitting. For this purpose, the C_DS value from the datasheet at V_DS = 0 V, should be divided by W × L and used as the initial value of Cj. The initial value of PB can be set at 2 V (similar to Phi) and the initial value of Mj can be set at 0.5 (typical value for one-sided abrupt P‒N junctions and Schottky diodes).

The modeled capacitances were compared to the extracted capacitance for both GaN-HEMTs in Figure 5. Good agreement is achieved at higher voltages, but there is a discrepancy between the simulated and datasheet C_DS curves at lower voltages due to the internal physics of HEMTs.

The suitability of the capacitance modeling can be verified by comparing simulated and actual energy stored in the output capacitance (E_OSS). This energy is stored while the GaN-HEMT is turning-off and the same energy is dissipated while the GaN-HEMT is turning-on. As high-frequency converters with GaN-HEMTs always require soft-switching, the E_OSS curve is crucial for achieving this condition. The E_OSS curve can be calculated from the respective C_OSS curve as:

$$E_{OSS}={\displaystyle \underset{0}{\overset{V_{DS}}{\int }}{C}_{OSS}\left(v_{DS}\right)}\times v_{DS}d{v}_{DS}$$

(10)

The E_OSS curve calculated from Equation (10) for MOSFET LEVEL 3 modeling is compared to the datasheet and is shown in Figure 6. The results show that the proposed model is adequate for simple and fast simulation of HEMTs in power-electronic circuits.

6. Model Validation by LTSpice Simulation

For power applications, a good way to validate the dynamic characteristics is to check how the developed model behaves under switching conditions. The manufacturer of GS66506T, GaN Systems, provides their own developed LTSpice model to be used for simulation purposes (the model is shown in Appendix A). Moreover, GaN Systems has developed a half-bridge double-pulse test (DPT) in LTSpice to evaluate the switching performance of their developed models in comparison to experimental measurements. As shown in the application notes [24], the manufacturer model is in good agreement with the experimental switching conditions. Hence, an identical double-pulse test platform developed by GaN Systems is used in this paper to verify the switching characteristics of the developed MOSFET LEVEL 3 model. Since LTSpice shares the same core libraries as any other SPICE version, the MOSFET LEVEL 3 model can be used in LTSpice simulation with adequately set parameter values, as shown in Appendix B. It is worth noting that two more parameters, namely, gate resistance (RG) and drain-to-source shunt resistance (RDS), are added while converting SPICE to LTSpice models to avoid convergence problem in LTSpice. The addition of these parameters does not have much effect on the electrical characteristics of the modeled GaN-HEMT. The value of RG is directly taken from the GS66506T datasheet as 1.1 Ω. The RDS is theoretically infinite; hence a very high value of 1 MΩ is used in the model. The DPT test bench in LTSpice is shown in Figure 7. The parameters of the DPT circuit along with their values are given in

Table 1. Parameters of the double-pulse test (DPT) circuit used for LTSpice simulation.

S. No.	Parameters		Value
	Symbol	Description
1	VBUS	DC bus voltage	400 V
2	ISW	Switching current	22.5 A
3	RGON	Turn-on gate resistor	10 Ω
4	RGOFF	Turn-off gate resistor	2 Ω
5	VDRV_P	Turn-on gate voltage	6 V
6	VDRV_N	Turn-off gate voltage	2 V
7	DT	Dead time	100 ns
8	T_ON	Turn-on period	2 μs
9	T_P	Total period	2.5 μs
10	L_DPT	Switching current inductance	64 μH
11	L_GATE	Gate inductance	1 nH
12	LS_EX	External source inductance	10 pH
13	L_DS	Power loop inductance	1 nH

. The switching waveforms of the DPT circuit with both the manufacturer’s and MOSFET LEVEL 3 models as the device under test (DUT) are shown in Figure 8.

Figure 8a,b shows the results with an operating DC bus voltage of 400 V and Figure 8c,d shows the results with an operating switching current of 22.5 A. Despite the simplicity of MOSFET LEVEL 3 model, the turn-off transients shows satisfactory agreement with the manufacturer model, whereas a bigger difference can be seen in Figure 8a,c during turn-on transients for both operating points. This deviation during the turn-on interval is most likely caused by the mismatch of modeled C_DS and C_GD at lower voltages. In addition, the MOSFET LEVEL 3 model does not include any parasitic inductances, which results in more pronounced oscillations as seen in Figure 8. However, for power applications, the power distributions during switching intervals are more relevant. The turn-on and turn-off power losses using the MOSFET LEVEL 3 model and manufacturer model for the two operating points are shown in Figure 9. Furthermore, the total energy losses during switching transients are presented in

Table 2. Energy losses during switching transients.

$\mathbf{Energy}\mathbf{Losses}\mathit{E}={\displaystyle \underset{{\mathit{t}}_1}{\overset{{\mathit{t}}_2}{\int }}\left({\mathit{v}}_{\mathit{D}\mathit{S}}\times {\mathit{i}}_{\mathit{D}}\right)\mathit{d}\mathit{t}}$	Manufacturer Model	MOSFET LEVEL 3 Model
EON	35.92 μJ	42.50 μJ
EOFF	7.23 μJ	5.05 μJ
ESW = EON + EOFF	43.15 μJ	47.55 μJ

.

Figure 9 and Table 2 demonstrate the effectiveness of the simple MOSFET LEVEL 3 model approach in comparison to the complex manufacturer model. Despite the observed deviation in the switching waveforms shown in Figure 8, the switching energy losses for the full current rating calculated from both models are quite close. In order to further evaluate the switching performance of the MOSFET LEVEL 3 model, the drain current was varied keeping the dc bus voltage constant and the comparison to the manufacturer model is shown in Figure 10. As can be seen, the simple MOSFET LEVEL 3 model provides adequate results in comparison to the complex manufacturer model. The observed variation between both curves in Figure 10 is acceptable in terms of designing power circuits, whereas the availability, transparency, and simplicity of the MOSFET LEVEL 3 model enables fast and effective simulations during the design of practical power-switching circuits.

7. Conclusions

This paper demonstrates that standard MOSFET equations, available in the SPICE circuit simulator, can be used to model commercial GaN-HEMTs. A set of equations from the available MOSFET LEVEL 3 equations in SPICE has been selected and a method for the extraction of the related SPICE parameters has been proposed. The validity of this approach, including the proposed parameter-extraction techniques, is verified by demonstrating an adequate match between simulated and measured static and dynamic characteristics. Furthermore, a DPT is performed for one of the GaN-HEMTs and is compared to its manufacturer model. It is demonstrated that the simple MOSFET LEVEL 3 model provides adequate results in terms of total switching energy losses. The transparency of the MOSFET LEVEL 3 model is further helpful in adapting to any GaN-HEMTs which is quite difficult in the manufacturer model. Due to the simplicity of this approach and the familiarity of circuit designs with the standard MOSFET SPICE model, this approach is ideally suited for the analysis and design of circuits with GaN-HEMTs. Future work may include an improvement of modeling of voltage-dependent capacitances to obtain switching energy losses as close as possible to the complex manufacturer model while keeping the model simple and transparent.