# Enhanced SPICE Simulation of Inductive Component Behavior

Sven Fieber, Ulf Schwalbe

► To cite this version:

Sven Fieber, Ulf Schwalbe. Enhanced SPICE Simulation of Inductive Component Behavior. The 26th European Conference on Power Electronics and Applications, GDR SEEDS France & EPE Association, Mar 2025, Paris, France. 10.34746/epe2025-0086. hal-05088845

HAL Id: hal-05088845

https://utc.hal.science/hal-05088845v1

Submitted on 28 May 2025

HAL is a multi-disciplinary open access
archive for the deposit and dissemination of sci-
entific research documents, whether they are pub-
lished or not. The documents may come from
teaching and research institutions in France or
abroad, or from public or private research centers.

L'archive ouverte pluridisciplinaire HAL, est
destinée au dépôt et à la diffusion de documents
scientifiques de niveau recherche, publiés ou non,
émanant des établissements d'enseignement et de
recherche français ou étrangers, des laboratoires
publics ou privés.

<figure><img src="image_1.png" /></figure>

Distributed under a Creative Commons Attribution 4.0 International License
# Enhanced SPICE Simulation of Inductive Component Behavior: Integrating Impedance Measurement and Core Loss Models for Transient Simulations

Sven Fießer, Ulf Schwalbe

University of Applied Sciences Fulda

Leipziger Str. 123, 36037 Fulda

Fulda, Germany

Tel.: +49 / (0) - 0661 96400

E-Mail: sven.fiesser@et.hs-fulda.de

URL: http://www.hs-fulda.de

**Index Terms**—Magnetic device, Simulation, Design optimization.

**Abstract**—This paper presents an enhanced method to model impedance data of inductive components for accurate simulation in transient SPICE simulations by utilizing vector fitting algorithms. These models are extended by a core loss model based on the improved generalized Steinmetz equation (iGSE). Through practical measurements, we demonstrate that the resulting models closely replicate the behavior of real inductors. These results present a more precise approach to simulating inductive components, particularly in scenarios where losses play a crucial role.

## I. INTRODUCTION

Accurate characterization of passive components is crucial for the design and optimization of modern power electronics systems, where components like inductors and transformers play a fundamental role in energy conversion, filtering, and signal processing. The impedance characteristics of these components, which are frequency-dependent due to different effects and loss characteristics, significantly impact the performance and reliability of switched-mode power supplies (SMPS) or other power electronic circuits. Therefore, precise modeling of inductive components in the design stage of the development process is essential to optimize them to save time and cost by shortening development iterations.

This paper presents a comprehensive approach to measure the impedance of passive components, primarily chokes in this paper, across a wide frequency range and to model the measured data using the vector fitting

algorithm. Vector fitting is a numerical technique that efficiently generates rational function models, which accurately represent the complex impedance behavior over the measured frequency spectrum [1]–[3]. The outputs of this fitting algorithm are state-space models that can be translated into SPICE syntax in order to simulate them in AC- as well as in transient simulations. The advantage of simulating the impedance model in a transient simulation is that it is possible to simulate the actual behavior and loss mechanisms of the device accurately.

In addition to the impedance model it is necessary to include a core loss model into the simulation model due to the fact, that typical impedance measurements are performed at low voltage and therefore cannot incorporate the core losses. By combining the impedance model with a core loss model using the improved Generalized Steinmetz Equation (iGSE) it is possible to simulate with this procedure accurately and efficiently the real behavior of inductive components.

Compared to traditional methods of modeling inductive components, such as using simple lumped element circuits or empirical fitting, the approach presented in this paper offers significant advantages. In the case of fitting the impedance data to a lumped model as shown in [4] it is necessary to fit the data to a predefined model. This task can be time-consuming because finding a suitable lumped model is often very complex. Therefore a lot of experience is required to find a suitable lumped model, that fits well enough to the impedance and phase data. Using an impedance network consisting of resistors and inductors as shown in [5] has the benefit of being more flexible, but the drawback is the insufficient accuracy of the resulting model, especially in the phase
response. Another approach shown in [6] also uses impedance network, but cannot be confirmed to due the closed source code. In contrast to these mentioned traditional approaches the in this paper presented modeling procedure is highly accurate over the entire measured frequency range, has a broader applicability, and can be used with ease, because no complex lumped circuit models are needed.

The methodology outlined in this paper involves the measurement of impedance data with an impedance analyzer, the application of the vector fitting algorithm to generate the impedance model, and the integration of this model with a core loss model into SPICE simulations. The approach is validated through a series of case studies, demonstrating its effectiveness in improving the accuracy of circuit simulations involving inductive components.

## II. MODELING PROCEDURE

### A. Measurement and fitting of impedance data

To model measurements of passive components in transient SPICE simulation the passive component has to be measured first. In this paper this is done with the "Vector Network Analyzer - Bode 100", which can perform impedance measurements down to single digit frequencies, which helps modeling the DC resistance of the measured device correctly. The measurement data can then be exported and be converted for the vector fitting algorithm. To model the impedance data in a SPICE simulation it is mandatory to invert the data in order to model the measurement data as an admittance instead of an impedance. This way it is easier to include the model as shown in Fig. 5.

To start the vector fitting algorithm it also mandatory to define the order of the fitting algorithm. It was found, that an order between five and seven works for most chokes the best, whereby a higher order implies a higher fitting accuracy but also results in a less efficient simulation model. The vector fitting algorithm outputs a state-space model with the corresponding order as previously mentioned. This resulting continuous time-invariant model, or it's corresponding matrix operations, can then be translated into SPICE syntax using non-linear dependent sources [7]. In the proposed model the input vector $\vec{u}$ and the output vector $\vec{y}$ are representing the two terminals of the inductor. Fig. 1 shows an exemplary mapping of an order two state-space model to SPICE syntax in LTspice to visualize the conversion procedure. It is noted that this example was created by hand for illustrative purposes and the conversion

procedure is done automatically and without a graphical representation of the resulting SPICE subcircuit.

<figure><img src="image_2.png" /><figcaption>Fig. 1: Exemplary mapping of a state-space model according to vector fitting of second order in LTspice.</figcaption></figure>

Due to the scaling of the state-space model and its resulting matrix operation it is therefore mentioned that the resulting models efficiency scales according to $O(n^2)$. Therefore a lower order of the fitting algorithm is to be preferred.

The left side of Fig. 2 shows the modeling procedure of the impedance data visually. For the in the verification used inductor Ind2 as shown in Fig. 6 (b) we also included the measurement and fitting data as shown in Fig. 3 and Fig. 4. It is shown in this case that an order of seven results in a very high fitting accuracy over the entire frequency range.

<figure><img src="image_3.png" /><figcaption>Fig. 2: Flowchart for measuring and modeling an inductor in SPICE using vector fitting and creating a core loss model with the iGSE.</figcaption></figure>
<figure><img src="image_4.png" /><figcaption>Fig. 3: Amplitude response of the impedance measurement and fitting of the inductor Ind2. Order of the vector fitting is seven. The impedance measurement values are inverted for modeling in SPICE.</figcaption></figure>

<figure><img src="image_5.png" /><figcaption>Fig. 4: Phase response of the impedance measurement and fitting of the inductor Ind2. Order of the vector fitting is seven. The impedance measurement values are inverted for modeling in SPICE.</figcaption></figure>

## B. Modeling of core losses

To model the necessary core losses next to the impedance model the winding and core information of the choke are needed to accurately model the core losses. With the information of the winding number N, the effective core area $A_e$, and the inductance the current magnetic field $B(t)$ can be calculated in a transient SPICE simulation according to Eq. 1.

$$B(t) = \frac{Li(t)}{NA_e} \qquad (1)$$

Using the momentary value of the magnetic field $B(t)$, it is possible to calculate the momentary core losses in the transient SPICE simulation. The formula

needed, that is based on the GSE as shown in Eq. 2, for this operation is given in Eq. 3. [8]

$$P_C(t) = V_C k f^{\alpha} B^{\beta} \qquad (2)$$

$$P_C(t) = V_C k_1 \left| \frac{dB}{dt} \right|^{\alpha} |B(t)|^{\beta-\alpha} \qquad (3)$$

## C. SPICE-Simulation of impedance and core loss model

The last step in the modeling algorithm is to incorporate this core loss calculation into the simulation and connect it to the impedance model. In this paper this is done by translating the core losses into a resistance (see Eq. 4) and connect it in parallel to the impedance model as shown in Fig. 5 [9]. The core loss modeling procedure is shown on the right side of Fig. 2.

$$R_{Pc} = \frac{(U_p - U_m)^2}{P_c(t)} \qquad (4)$$

<figure><img src="image_6.png" /></figure>

<table><tr><td>Winding parameters</td><td>Steinmetz coefficients (iGSE)</td></tr><tr><td>.param N=14</td><td>.param k1=0.00097</td></tr><tr><td>.param L=19.1u</td><td>.param a=1.79</td></tr><tr><td>.param Ae=0.000107</td><td>.param b=2.56</td></tr><tr><td>.param V=0.000010600</td><td></td></tr></table>

<table><tr><td>Calculation of current<br>magn. Field B</td><td>Alternative calculation of current<br>magn. Field B<br>(w/o current measurement)</td></tr><tr><td>V=(I(Rm)*{L})/({Ae*N})</td><td>V=idt(V(Lp,Ln))/(N/{Ae})</td></tr></table>

<table><caption>Fig. 5: LTspice simulation of the fitted inductor Ind2 including the core loss model.</caption><tr><td>Calculation of current core losses</td></tr><tr><td>V={k1} * abs(V(Lp,Ln))/(N*Ae))**{a} * abs(V(B))**{(b-a)} * {V}</td></tr></table>

Depending on the used SPICE simulation program it might be necessary to use a different approach to calculate the momentary magnetic flux due to possible
solver issues. In this case an alternative formula as shown in Fig. 5 can be used to mitigate convergence issues.

### III. VERIFICATION

To demonstrate the accuracy of the here presented algorithm we built two different chokes and compared practical results with results that were obtained through SPICE simulations. The two chokes are depicted in Fig. 6 and their winding information are shown in Tab. I.

<figure><img src="image_7.png" /><figcaption>(a) Inductor Ind1.</figcaption></figure>

<figure><img src="image_8.png" /><figcaption>(b) Inductor Ind2.</figcaption></figure>

<caption>Fig. 6: Two of the inductors used for the verification of the fitting algorithm.</caption>

<table><caption>TABLE I: Winding information of the chokes used to verify the modeling method of passive components.</caption><thead><tr><th></th><th>Inductor Ind1</th><th>Inductor Ind2</th></tr></thead><tbody><tr><td>Core type</td><td>TDK ETD39</td><td>Magnetics<br>toroidal 254</td></tr><tr><td>Core material</td><td>TDK E97</td><td>Magnetics<br>KoolMμ</td></tr><tr><td>Windings</td><td>8</td><td>15</td></tr><tr><td>Wire</td><td>Pack LitzWire Rul-<br>palit Classic 60</td><td>2x 2.5 mm²</td></tr><tr><td>Air gap</td><td>(none)</td><td>(none)</td></tr><tr><td>Inductance</td><td>136,5 μH</td><td>18 μH</td></tr></tbody></table>

First, the simulation models were verified to ensure they performed as expected. As shown in Fig. I, the simulated voltage and current waveforms of the inductor Ind2 closely match the measured waveforms. This confirms that the modeling algorithm functions as intended.

Second, we compared the losses (core and winding losses combined) of the simulation model and the real inductors at different frequencies and currents. The simulated losses were directly taken from the SPICE simulation program by adding the losses occurring in the core loss model and the state-space model. To accurately determine the losses in the real inductors, we measured both voltage and current directly at the component and calculated the losses accordingly. It is noted, that these

<figure><img src="image_9.png" /><figcaption>Fig. 7: Comparison of the simulated and measured current of inductor Ind2 at 50 kHz.</figcaption></figure>

measurements were performed without an applied DC-bias due to the nature of the iGSE, that doesn't support the inclusion of DC-bias losses. The results of the comparison of the losses are shown in Fig. 8 for the inductor Ind1 and in Fig. 9 for the inductor Ind2.

As seen in those charts the simulated losses of the chokes are matching nearly the real measured losses at most frequencies and currents. For Ind1 the deviations are between only 3,0 % and at higher currents 17,6 %. For Ind2 the deviations are between 2,9 % and 13,2 %.

<figure><img src="image_10.png" /><figcaption>Fig. 8: Comparison of the simulated and measured power losses of inductor Ind1.</figcaption></figure>

### IV. DISCUSSION

As previously mentioned, the measurements were conducted without an applied DC-bias. This is because no existing core loss model accounts for DC-bias losses using only data sheet information [10]. If an appropriate core loss model is identified and adapted for transient
<figure><img src="image_11.png" /><figcaption>Fig. 9: Comparison of the simulated and measured power losses of inductor Ind2.</figcaption></figure>

SPICE simulations, the iGSE-model used in this study can be easily replaced by the user's own model. There exist some models to include DC-bias losses, as shown in [11] and [12], but these rely on extensive core loss measurements, making them impractical for this here presented approach. Consequently, this factor is neglected in this study. If an appropriate core loss model is identified and adapted for transient SPICE simulations, the iGSE-model used in this study can be easily replaced by the user's own model.

Additionally, incorporating core losses due to the air gap in the core presents challenges. Since impedance measurements are performed at low voltages, the effects of the air gap cannot be accurately represented in the impedance model [6].

However, this approach can be extended to accommodate other passive components, such as transformers and capacitors. For transformers, it may be possible to fit a multi-port model, though further investigation into these approaches will be pursued in future work.

## V. CONCLUSION

This paper introduces a new algorithm for accurately fitting impedance data to transient SPICE simulation models of inductive components. By performing an impedance measurement and applying the vector fitting algorithm, a state-space model of the component can be created. This model is then adapted and translated for use in transient SPICE simulations. Additionally, a core loss model based on the iGSE is incorporated to account for losses not captured by impedance measurements alone.

The results demonstrate that the simulation model performs as expected, with the deviations between simulated and measured losses being minimal. This highlights

the effectiveness of the approach in simulating the inductive components' behavior under real-world conditions, a feature that existing systems struggle to provide. Consequently, this fitting approach can be effectively used in the design stage of inductive components, such as in the development of SMPS (Switched-Mode Power Supplies), potentially reducing development time and improving the reliability of the final designs.

## REFERENCES

[1] B. Gustavsen and A. Semlyen, "Rational approximation of frequency domain responses by Vector Fitting," IEEE Trans. Power Delivery, vol. 14, pp. 1052-1061, 1999.

[2] B. Gustavsen, "Improving the pole relocating properties of vector fitting," IEEE Trans. Power Delivery, vol. 21, pp. 1587-1592, 2006.

[3] D. Deschrijver, M. Mrozowski, T. Dhaene, and D. De Zutter, "Macromodeling of Multiport Systems Using a Fast Implementation of the Vector Fitting Method," IEEE Microwave and Wireless Components Letters, vol. 18, pp. 383-385, 2008.

[4] G. Barrere, "Zfit Impedance Equivalent Circuit Fitter," 2019.

[5] L. Boehning and U. Schwalbe, "Modelling and loss simulation of magnetic components in power electronic circuit by impedance measurement," PCIM Europe digital days 2020; International Exhibition and Conference for Power Electronics, Intelligent Motion, Renewable Energy and Energy Management, pp. 1-7, 2020.

[6] R. Ridley, "Advanced Magnetics Practical Circuit Models," 2023.

[7] H. Vogt, G. Atkinson and P. Nenzi, "Ngspice Users's Manual Version 43plus," 2024.

[8] K. Venkatachalam, C. Sullivan, T. Abdallah, and H. Tacca, "Accurate prediction of ferrite core loss with nonsinusoidal waveforms using only Steinmetz parameters," 2002 IEEE Workshop on Computers in Power Electronics, pp. 36-41, 2002.

[9] A. Abramovitz and S. Ben-Yaakov, "RGSE-Based SPICE Model of Ferrite Core Losses," IEEE Transactions on Power Electronics, vol. 33, pp. 2825-2831, 2018.

[10] J. Mühlethaler, "Modeling and multi-objective optimization of inductive power components," PhD thesis, ETH Zürich, 2012.

[11] J. Mühlethaler, "Core losses under DC bias condition based on Steinmetz parameters," The 2010 International Power Electronics Conference - ECCE ASIA -, pp. 2430-2437, 2010.

[12] M. Esguerra, "Measurement of Power Losses with DC-Bias - The Displacement Factor," Proc. 41st Int. Conf. Power Conversion/Intelligent Motion (Nürnberg), 2000.