## 2 Computation Method  
The methods of electrothermal analyses of electronic networks with the use of SPICE need a special electrothermal model implemented in this software. On the other hand, the manufacturers give on their websites the models of their products dedicated for SPICE. Such models are in the form of subcircuits and they do not take into account the self-heating phenomenon. The proposed computation method makes it possible to use such models in computations and obtain a much shorter time of computations. This method includes the six steps:  
1. Setting the value of the transistor temperature TEMP equal to ambient temperature \(T_{a}\). 2. Transient analysis of the tested circuit for a time equal to two periods of the control signal and registrations of the waveforms of \(p(t)\) and \(T_{j}(t)\). 3. Calculation of the average value of power \(p_{avg}\) dissipated in the transistor using the results of the SPICE computations. 4. Calculation of the junction temperature \(T_{j}\) value at the steady state using the formula \[T_{j}=T_{a}+R_{th}\cdot p_{avg}\] (2)
5. Comparing the values of TEMP and \(T_{j}\). If the difference is bigger than 1 K, TEMP should be substituted by \(T_{j}\) and then jump to point (b). If this condition is not fulfilled, jump to point (f). 6. Waveforms of \(p(t)\) and \(T_{j}(t)\) obtained in point (b) correspond to the waveforms of these quantities at the steady state. Practical implementation of the proposed method is presented below on the example of a power SiC-MOSFET offered by ROHM semiconductor [31]. The network representation of the model of the considered transistor is presented in Figure 1.  
In this model, terminals D, G and S represent drain, gate and source of the modeled transistor, respectively. Controlled current sources G1 and G11 describe DC components of the drain current. Voltage sources V1, V2, V3, V11 and V12 of zero values are used to monitor the current flowing through selected branches and used in the description of selected controlled sources. Resistors R3 and R11 have very high values and they are used due to the formal requirements of the SPICE software. Linear capacitors C11, C1 and C2 and controlled current sources G2 and G11 represent internal capacitances of the transistor. Inductor L1 describes the inductance of the source. The output voltages or currents of the following controlled voltage and current sources E3, E4, E1, G1 and G11 depend on temperature TEMP. Controlled voltage sources E1 and E2 describe series resistances of the gate and the drain taking into account an influence of temperature. Controlled voltage source E11 describes non-linear series resistance of the source. Controlled voltage sources E3 and E4 are used to calculate the formulas used in the descriptions of other currents or voltages sources contained in this model. Many of the used controlled voltage and current sources are described using splines. In order to perform computations with the use of the proposed method in SPICE, an input file should be included with the schema of the analyzed network with the transistor model presented in Figure 1 and the network representation of its thermal model in the form shown in Figure 2. In this network-controlled current source, \(p_{th}\) represents power dissipated in the transistor, which is equal to the product of drain current \(i_{D}\) and voltage between the drain and the source \(v_{DS}\). Resistors occurring in this network represent thermal resistance of each component of the heat flow path, whereas capacitors represent thermal capacitances of these components. Values of these resistors are equal to the product of thermal resistance \(R_{th}\) and coefficients \(a_{i}\), whereas thermal time constants \(\tau_{thi}\) are equal to the products of thermal capacitances \(C_{thi}\) and thermal resistances \(R_{thi}\). Of course, the number of components \(R_{thi}\) and \(C_{thi}\) as well as their values depend on properties of the used cooling system of the tested transistor.