Nonlinear magnetic ring model based on impedance measurements with DC-bias current.

Skip to main content An official website of the United States government Here's how you know Here's how you know Official websites use .gov A .gov website belongs to an official government organization in the United States. Secure .gov websites use HTTPS A lock ( Lock Locked padlock icon ) or https:// means you've safely connected to the .gov website. Share sensitive information only on official, secure websites. Search Log in Dashboard Publications Account settings Log out Search… Search NCBI Primary site navigation Search Logged in as: Dashboard Publications Account settings Log in Search PMC Full-Text Archive Search in PMC Journal List User Guide PERMALINK Copy As a library, NLM provides access to scientific literature. Inclusion in an NLM database does not imply endorsement of, or agreement with, the contents by NLM or the National Institutes of Health. Learn more: PMC Disclaimer | PMC Copyright Notice Sci Rep . 2026 Mar 3;16:11846. doi: 10.1038/s41598-026-39594-1 Search in PMC Search in PubMed View in NLM Catalog Add to search Nonlinear magnetic ring model based on impedance measurements with DC-bias current Kamil Kutorasiński Kamil Kutorasiński 1 Faculty of Physics and Applied Computer Science, Department of Condensed Matter Physics, AGH University of Krakow, al. A. Mickiewicza 30, 30-059 Kraków, Poland Find articles by Kamil Kutorasiński 1, ✉ , Jarosław Pawłowski Jarosław Pawłowski 2 Institute of Theoretical Physics, Wrocław University of Science and Technology, Wyb. Wyspiańskiego 27 St., 50-370 Wrocław, Poland Find articles by Jarosław Pawłowski 2 , Michał Molas Michał Molas 3 Institute of Power Engineering – National Research Institute, Mory 8 St., 01-330 Warsaw, Poland Find articles by Michał Molas 3 , Marcin Szewczyk Marcin Szewczyk 4 Division of Power Apparatus, Protection and Control, Faculty of Electrical Engineering, Electrical Power Engineering Institute, Warsaw University of Technology, Koszykowa 75 St., 00-662 Warszawa, Poland Find articles by Marcin Szewczyk 4 Author information Article notes Copyright and License information 1 Faculty of Physics and Applied Computer Science, Department of Condensed Matter Physics, AGH University of Krakow, al. A. Mickiewicza 30, 30-059 Kraków, Poland 2 Institute of Theoretical Physics, Wrocław University of Science and Technology, Wyb. Wyspiańskiego 27 St., 50-370 Wrocław, Poland 3 Institute of Power Engineering – National Research Institute, Mory 8 St., 01-330 Warsaw, Poland 4 Division of Power Apparatus, Protection and Control, Faculty of Electrical Engineering, Electrical Power Engineering Institute, Warsaw University of Technology, Koszykowa 75 St., 00-662 Warszawa, Poland ✉ Corresponding author. Received 2026 Jan 2; Accepted 2026 Feb 5; Collection date 2026. © The Author(s) 2026 Open Access This article is licensed under a Creative Commons Attribution-NonCommercial-NoDerivatives 4.0 International License, which permits any non-commercial use, sharing, distribution and reproduction in any medium or format, as long as you give appropriate credit to the original author(s) and the source, provide a link to the Creative Commons licence, and indicate if you modified the licensed material. You do not have permission under this licence to share adapted material derived from this article or parts of it. The images or other third party material in this article are included in the article’s Creative Commons licence, unless indicated otherwise in a credit line to the material. If material is not included in the article’s Creative Commons licence and your intended use is not permitted by statutory regulation or exceeds the permitted use, you will need to obtain permission directly from the copyright holder. To view a copy of this licence, visit http://creativecommons.org/licenses/by-nc-nd/4.0/ . PMC Copyright notice PMCID: PMC13066542  PMID: 41776264 Abstract This paper presents a complete method for modeling nonlinear magnetic rings that captures frequency dependence, losses (hysteresis effect), and nonlinear effects including saturation. The approach relies on frequency-domain impedance measurements (here, 10 Hz – 10 MHz) under DC bias currents up to saturation (here, 800 A), and extends classical equivalent-circuit fitting to a two-dimensional impedance function of frequency and current. A key contribution is the formulation of a fully implementable modeling framework together with its realization as SPICE netlist code, enabling direct time-domain simulation under arbitrary excitation signals. The validity of the model is demonstrated through analytical verification, impedance measurements with DC bias, and high-current experiments. Furthermore, the paper investigates and discusses the applicability of the model, showing consistency with results obtained from a dedicated high-current test setup. The outcome is a novel, practical, and fully validated nonlinear modeling methodology, with its implementation released as SPICE code. Subject terms: Engineering, Mathematics and computing, Physics Introduction Background and motivation Accurate modeling of magnetic components is essential for the design and analysis of power electronic systems that rely on magnetic materials 1 , 2 . Due to the complex physics governing these materials, accurate modeling remains a significant challenge, particularly when nonlinear behavior and frequency-dependent hysteresis effects must be considered. In such cases, the response of the material depends strongly on the waveform of the excitation signals, including their peak values and frequency spectrum. The analysis and design of devices containing magnetic materials are commonly performed in the time domain through circuit simulations. Developing a circuit model that reflects the actual behavior of magnetic materials is therefore necessary, with particular emphasis on representing their frequency-domain properties, including frequency-dependent losses (hysteresis) and saturation effects. Although several approaches have been proposed to model the response of magnetic components to specific excitations, the problem has not yet been fully resolved 3 , 4 . Several physically based modeling approaches have been developed, including the well-known Jiles–Atherton (J-A) 5 – 7 , Preisach 8 – 10 , and Steinmetz 11 models. These models adapt parameters to reproduce measured BH hysteresis loops and can provide good agreement while accounting for nonlinear and hysteretic effects. However, they are generally limited in bandwidth and cannot accurately describe material behavior over a wide frequency range spanning several decades 8 , 12 . The relatively small number of model parameters and their limited flexibility further restrict their applicability in broadband scenarios. More recently, neural-network-based modeling techniques have been introduced, enabling effective fitting of models directly from time-domain waveforms 2 , 3 , 13 . Although accurate, these methods require training on large, application-specific datasets that span a wide variety of excitation cases, which are often difficult or impractical to obtain. An alternative approach is to construct equivalent circuit models directly from frequency-dependent impedance measurements of the material under test. Several well-established and effective fitting methods 14 – 17 allow the synthesis of Foster or Cauer ladder-type networks composed of lumped circuit elements, making their implementation in simulation tools such as SPICE straightforward. The required input data are impedance versus frequency characteristics, which can be measured accurately using impedance analyzers 18 , 19 or vector network analyzers 20 . Once the transfer function of a linear system is determined, equivalent passive circuit models consisting of inductors (L) and resistors (R) can be readily derived 21 . While this method is convenient, accurate, broadband-capable, and accounts for hysteresis effects, it is inherently restricted to linear systems or to linearized operation around a specific working point. A natural extension is therefore to generalize these methods to nonlinear systems, which is the main focus of this work. To extend impedance-based modeling to nonlinear regimes, the impedance must be characterized as a function not only of frequency but also of current bias, typically introduced via a superimposed DC current 19 , 20 , 22 . This results in a two-dimensional impedance function (frequency and current) rather than a one-dimensional characteristics (frequency). Although several methods exist for estimating transfer functions of nonlinear systems from time-domain measurements 23 – 25 , such approaches involve significant mathematical simplifications, since a single 1D function cannot capture the full behavior of the nonlinear object under investigation. A further challenge is the identification of nonlinear model parameters from the available measurement data. Although non-trivial, several methods have recently been proposed to address this problem 12 , 26 – 29 . Finally, the practical implementation of nonlinear equivalent circuits in simulation environments such as SPICE remains a critical barrier. Many existing models are defined through formulas or algorithms that are not directly compatible with SPICE or other universal simulation tools 20 , 30 – 35 . This often prevents their adoption in real-world design workflows. To overcome these shortcomings, this work introduces a new approach for the modeling and implementation of nonlinear magnetic components. Paper aim and scope This paper introduces a comprehensive and complete method for deriving, implementing and simulating a nonlinear circuit model of a magnetic ring, based on frequency-domain measurements with DC-bias current. The method covers every step from measurements to the SPICE netlist code that can be used in simulations . The proposed model has been verified by comparing the simulated results with the corresponding results from analytical solution and with two types of experimental measurements (low-currents in frequency-domain with DC-bias current and high-currents in time-domain). The resulting circuit model can be used in time-domain simulations as part of a larger system, covering excitations across the full range of nonlinear operating conditions. The accuracy testing was performed providing insights into the model’s applicability beyond the measurement data for which the model was developed. The results presented in this paper conclude the findings and experience gained through the long-term efforts of a research aimed at developing universal, practical methods for creating high-precision magnetic ring models using frequency-domain measurements with DC-bias currents 16 , 19 , 26 – 29 , 36 , 37 . To increase the practical value of this work, the outcome of the method reported in this paper has been made-available as a code in an open-access repository, ready to be used in larger system simulations 38 . Paper structure Sections I and II provide the introduction, including background, motivation, state of the art, and the aim and scope of the paper, followed by statements of novelty and contribution. Section III outlines the overall concept corresponding to the paper’s structure, as illustrated in Fig. 1 . The subsequent sections present the study results. Fig. 1. Open in a new tab Concept of the proposed method: from measurements using a low-current impedance analyzer with a high DC-bias current, through circuit modeling and extraction of circuit parameters, SPICE implementation of the nonlinear circuit, to validation via simulations and comparison with measurement results in frequency and time domains, as well as with an analytical solution. Section IV presents the measurement data serving as input for the modeling method, followed by Section V, which introduces the modeling method itself: the mathematical model defined by Eq. 1 , its circuit representation shown in Fig. 3 , and two methods (NLS and NN) for determining the numerical values of the model’s nonlinear parameters, and . Fig. 3. Open in a new tab Circuit representation of the ring model with impedance , as defined in Eq. 1 . Section VI presents the implementation of the model in SPICE netlist code, with its core component being a single pair of parallel-connected LR elements, as shown in Fig. 6 . Fig. 6. Open in a new tab Schematic of the implementation of parallel-connected nonlinear LR elements in SPICE. On the left is a conceptual diagram, and on the right is its implementation using the basic elements of SPICE syntax. The implementation corresponds to a nonlinear LR element where , whereas allows this ratio to vary, . Section VII reports on the validation of the model, covering both the implementation method and the numerical stability of the simulations, as well as the validation of the overall magnetic ring modeling method using analytical solutions, low-signal experimental data, and high-current measurements. The paper concludes with Section VIII, which provides a summary and the final conclusions. Novelty and contribution The main contributions of this paper are as follows: A comprehensive and complete method is presented for modeling magnetic rings, capturing nonlinear and frequency-dependent hysteresis effects, with nonlinearity up to saturation, based on low-signal frequency-domain measurements with DC-bias currents. An implementation method in SPICE netlist code is introduced. The SPICE code and its use with the Python package PySpice have been made available in an open-access repository 38 to increase the practical value of this work. Validation of the complete method is carried out along with an assessment of the model’s applicability, based on: (i) analytical solution, (ii) low-signal measurements with DC-bias current, (iii) high current measurements. Concept outline The concept of the method and the structure of the paper are illustrated in Fig. 1 , as outlined below. Magnetic ring modeling method A key feature of the modeling method presented in this paper is the ability to use low-signal frequency-domain measurements with DC-bias current (see Fig. 2 ) to obtain a magnetic ring model in a form of a circuit with nonlinear parameters (see Fig. 3 ) that accounts for frequency characteristics, hysteresis, and nonlinearities up to saturation. The input for the modeling method are measurement data collected as a series of low-signal impedance characteristics obtained for a set of DC-bias currents , ranging from zero to the saturation level. The measurement method to obtain with an impedance analyzer and a high power DC current generator, was discussed in 19 . Fig. 2. Open in a new tab Measurement input data used for model development: a set of impedances measured for the investigated magnetic ring, , as a function of frequency f and DC-bias current . Based on 16 , 26 , the measured impedance has been represented by the model given in Eq. 1 and, equivalently, by its circuit representation formed as a series of parallel-connected nonlinear LR pairs, as shown in Fig. 3 . The nonlinear parameters are therefore the functions of current and or the pair of components in its circuit representation, in Fig. 3 . The parameters and were derived using two previously developed fitting methods: one based on classical parameter fitting using the nonlinear least squares method (hereafter referred to as the NLS fitting method) 27 , and the other employing AI techniques with unsupervised neural networks (hereafter referred to as the NN fitting method 28 ). The outcome of the parameter determination procedure is therefore a set of the model parameters defined as functions and . To conclude the above steps based on the previously published works 19 , 26 – 29 , the only missing elements of the overall magnetic ring modeling method were (i) the implementation in the SPICE netlist code of the nonlinear circuit representation of , including its nonlinear parameters and , and (ii) the validation of the final implemented circuit model. These missing elements are introduced here, providing a complete description of the modeling method and its validation. Implementation of the model in SPICE netlist code An implementation method was proposed in a form of the SPICE netlist code (Fig. 3 ) to represent a model building block (the LR pair) composed of two nonlinear elements, L ( i ) and R ( i ), connected in parallel and having two terminals, as shown in Fig. 6 a. The ring model shown in Fig. 3 is constructed as a series of such building blocks. Such a building block, as seen from its terminals, behaves like a lossy inductance characterized with nonlinear impedance. Model validation The correctness of the implementation method and the numerical stability of the simulations were examined to validate the proposed approach for representing the circuit model shown in Fig. 3 as a SPICE netlist code. The model was validated by comparing the voltage response of the magnetic ring, measured in a dedicated high-current experimental setup, with the corresponding simulation results, in order to assess its applicability in reproducing the ring’s behavior under real current conditions. Measurement data used as model input The input data (Fig. 2 ) used to build the model consists of frequency and current-dependent impedance, , measured for various values of DC-bias current, , ranging from zero to the magnetic material saturation. The data were collected using an impedance analyzer and a DC current generator following the method presented in 19 . The measured object was a magnetic ring with a circumference of 45 cm made of nanocrystalline material Nanoperm with a nominal (manufacturer-provided) relative permeability at 1 kHz and inductance H at 1 kHz, produced by Magnetec GmbH 39 . Impedance measurements were performed over a frequency range spanning 5 decades, from 100 Hz to 10 MHz, for selected DC-bias currents determining the magnetic ring operating point from zero up to saturation. In total, 32 values of the DC-bias current, , were selected for the measurements, ranging from 0 to 800 A. The values were distributed approximately log-uniformly, with increased density around A, where strong nonlinearity and the transition from the non-saturated to the saturated state occurred. The maximum current A ensured magnetic saturation of the ring material. In the frequency-domain, data were collected at 400 points spanning 5 decades. To obtain the parameters of the circuit model (see Sect. 5 ), it was sufficient to use only 50 points evenly distributed on a logarithmic scale. This selection represented a compromise between accuracy and the computational effort required to fit the circuit model parameters using the discussed below non-linear least squares (NLS) or neural network (NN) parameter fitting methods. The measurement data shown in Fig. 2 are also shown in Figs. 4 a-b and 5 a-b as dots in an equivalent form , where . A strong nonlinearity can be observed around the current of approximately 200 A. For currents 800 A, the inductance decreases by factor approximately 50, which is interpreted as the magnetic saturation of the ring material. Fig. 4. Open in a new tab Impedance of the ring (a-d) obtained from measurements (dots) as a function of frequency f and DC-bias current , presented as inductance (a, c) and resistance (b, d) in the series impedance model ; solid lines represent corresponding parameters calculated from the circuit model (Eq. 1 ) fitted using the NLS method; (e) Error map (RAE, see Eq. 3 ) of of the circuit model compared to the measurements; (f) Characteristic frequencies for k -th LR pair as functions of f and ; (g-h) Values of the functions and for all LR pairs of the circuit model (data for and do not fit within the window range); (i-n) Maps presenting how contributing k -th LR pair (see Eq. 2 ) is across frequency range f and . Fig. 5. Open in a new tab Impedance of the ring (a-d) obtained from measurements (dots) as a function of frequency f and DC-bias current , presented as inductance (a, c) and resistance (b, d) in the series impedance model ; solid lines represent corresponding parameters calculated from the circuit model (Eq. 1 ) fitted using the NN method; (e) Error map (RAE, see Eq. 3 ) of of the circuit model compared to the measurements; (f) Characteristic frequencies for k -th LR pair as functions of f and ; (g-h) Values of the functions and for all LR pairs of the circuit model; (i-m) Maps presenting how contributing k -th LR pair (see Eq. 2 ) is across frequency range f and . Magnetic ring model based on measured impedance characteristics with DC-bias current Model structure and its circuit representation The measurement data shown in Fig. 2 as were used to construct a nonlinear model in the form of first-order partial fractions consisting of a set of nonlinear parameters, interpreted as inductances and resistances that are current-dependent, and, importantly, positive (and thus physically meaningful): 1 The nonlinear model given in Eq. 1 is represented by the circuit shown in Fig. 3 . Since the measured phase ranges from 0 to 90 deg, and the impedance value is always a rising function of frequency, a model consisting of a series of parallel-connected inductors and resistors was chosen as the most valid representation of the measured impedance . When the measured phase falls outside the 0 to 90 degree range and exhibits a predominantly capacitive component within certain frequency range, an LR-based model becomes insufficient. This situation can occur, for instance, in the presence of dimensional resonance, as observed in ferrites 40 . Model parameters from NLS and NN fitting methods Obtaining the parameters of the circuit model, i.e., the sets of functions and in Eq. 1 and Fig. 3 , is a challenging task, especially when aiming to ensure that the model impedance, , closely matches the measured impedance accross wide ranges of f and , and at the same time ensuring that and functions are smooth. To derive the circuit model parameters, two numerical fitting methods were employed: NLS fitting method : Employs nonlinear least-squares (NLS) function fitting 27 . This method uses a constraint that the ratio is constant for each k -th component of the circuit model. The parameters obtained with use of this fitting method for the measurement data used in this paper yield the smallest error for the circuit model in Fig. 3 consisting of six , pairs. NN fitting method : Employs an unsupervised neural network (NN) with an autoencoder architecture 28 . This method is more general than NLS and does not impose the restriction ; therefore, it has twice as many free parameters as the NLS method. The NN architecture was designed to have five , pairs as its output. The primary difference between the NLS and the NN methods is that the first one assumes the values are not dependent of i , while the second one does not impose this restriction. Constant is forced in the NLS method and helps to ensure smooth and functions. In the NN method, this is not necessary because, due to the specific architecture of neutral network, the algorithm itself yields smooth and functions without this assumption. The benefit of the NLS method with a forced constant is the ability to compare the voltage response of the simulated model with the voltage response of an analytical formula based on the inverse Laplace transform (see Appendix), which is relevant for the constant only. This allows for verifying the simulation accuracy and correctness of implementation. The analytical formula is relevant for the constant only, see Eq. 6 in Appendix. The sole reason for introducing and using the simplified model provided by the NLS method in this work is to enable comparison of the simulated voltage with the analytically obtained result, thereby verifying the correctness of the implementation and the numerical accuracy. The position of on the frequency scale is part of the parameter search process in both methods and indicates whether a k -th pair has an inductive or resistive nature. The analysis of makes it possible to examine of the LR series generated in the fitting algorithm and to determine the frequency ranges in which the individual LR pairs contribute. The k -th pair exhibits an inductive character when is above the operating frequency, whereas it exhibits a resistive character when is below the operating frequency. Discussion on fitting methods accuracy Figures 4 and 5 present, respectively, a summary of the two fitting methods (NLS and NN) used for obtaining nonlinear parameters of . An important and noteworthy achievement of both fitting methods is that the functions and are smooth in the domain of i . Circuits with parameters obtained using the NLS and NN methods differ in terms of fitting accuracy, as shown in Figs. 4 e and 5 e, respectively. Additionally, the two resulting circuits differ in the number of ”active” (contributing) pairs (in terms of the pair contribution to the overall impedance). How contributing the specific pair is within the overall circuit is defined as the relative impedance value of a given k -th element for various frequencies f and currents : 2 This is visualized for the circuits with parameters obtained via the NLS and NN fitting methods, as maps in Figs. 4 (i-n) and 5 (i-m), respectively. Some LR pairs significantly contribute to the overall impedance only in the pre-saturation range ( A), while others do so only in the post-saturation range ( A). This occurs, for example, in the circuit with parameters obtained using the NLS fitting method for (see Fig. 4 k) and (see Fig. 4 n). In the circuit with parameters obtained using the NLS method, the algorithm attempted to fit six pairs, but adjusted the parameters to make two pairs non-contributing (for and , see Fig. 4 i-n). Using the NN fitting method, five pairs were fitted, with one pair similarly remaining non-contributing ( , see Fig. 5 i-m). The value of for the circuit model with parameters obtained using the NLS method is below 10 Hz (see Fig. 4 f), indicating that the pair with contributes only resistive behavior to the total impedance of the circuit. Figures 4 g-h and 5 g-h present the functions and for circuits parameterized using the NLS and NN fitting methods, respectively. Figures 4 a-d and 5 a-d, respectively, show the impedance of the model with these parameters, calculated using Eq. 1 , alongside the measurement data . It is evident that the models featuring fitted parameters perform well in reflecting key properties of the ring, i.e., the saturation effect and the reduction of inductance with increasing frequency. A quantitative assessment of the model’s fit to the measurement data for various frequencies and DC-currents is shown in Figs. 4 e and 5 e as the relative absolute error (RAE model) of the impedance magnitude, defined as: 3 Discussion on modeling method applicability It is worth commenting on the extrapolation that occurs when developing the model based on data measured from an impedance analyzer with applied DC-bias current, . The resulting circuit model has an impedance that depends on the current i and, in general, can be used for any waveform, regardless of peak current or frequency components. However, the measurement data were collected for specific signals of the form , where is a small harmonic signal and is a time-constant (and possibly significant) component, such that for any t . ”Small” here means that within the range, the nonlinearity of the magnetic material is negligible. This requirement is fulfilled by measurements conducted using an impedance analyzer that operates with a signal amplitude of approx. 20 mA. Applying the model for any i , which means to perform transition from to , is therefore an extrapolation of the model beyond the range for which it was created. The model with impedance , on the other hand, ensures proper physical behavior, and thus fully accurate results, when the current takes the form . Here, is a signal of any shape with a frequency spectrum within the range of the measurement input data (in our case, Hz) and a small maximum value (to ensure linearity around working point defined by ). On the other hand, the type of signal that is the most difficult to describe using such a model is the one with the large maximal values of alternating component ( ), i.e., a current causing transitioning from saturation to saturation of the magnetic material. The validation of the model’s performance and its correctness in this range can only be carried out by comparing simulations and measurements for such currents, as described in Sect. 7 . Model implementation in SPICE netlist code The magnetic ring model described above, represented as a series of nonlinear parallel-connected LR elements (Fig. 3 ), requires a numerically stable implementation. To achieve this, the implementation of a single pair of parallel-connected nonlinear L and R elements is necessary. An effective method for implementing nonlinear elements relies on arbitrary behavioral current and voltage sources 35 , 41 . Due to the non-linearity of two parallel-connected components (L nad R) which values are controlled by the same current, the problem exhibits considerable complexity. Such a system cannot be considered as two independent nonlinear elements, L and R, but rather as a current-dependent complex impedance with a phase angle ranging between 0 and 90 degrees. The current determining the operating point of the inductance L or resistance R cannot be the current flowing through these individual elements, but must be the total current flowing through the entire LR pair. To fulfill this requirement, an implementation is proposed, as illustrated in Fig. 6 as a SPICE syntax diagram. The purpose of the SPICE implementation is to create a nonlinear subcircuit corresponding to an LR pair, featuring two terminals (labeled pos and neg in Fig. 6 ). From the perspective of the external circuit, this subcircuit behaves as a lossy inductance with nonlinear impedance. Such a subcircuit can be used like a standard lumped element and can be directly integrated into simulations of larger and more complex systems. A key challenge in the implementation is to develop a solution that ensures: (i) the impedance of the LR pair depends on the instantaneous value of current passing through it; (ii) its impedance corresponds exactly to the values derived from the L ( i ) and R ( i ) curves; (iii) variations in the simulated impedance are smooth, even if the and tables are provided for only a limited number of current points, ; (iv) the LR pair operates with any type of current signal; and (v) the implementation remains numerically stable. Ensuring numerical stability is both critically important and challenging, as the impedance of the LR element may be highly nonlinear and can vary by several orders of magnitude within very short time intervals. The implementation of the lossy inductance L is based on a method where, instead of calculating the voltage drop across a time-dependent inductance, the voltage drop is calculated across a constant unit inductance, H, using an auxiliary ”current” defined as . The voltage drop across the unit inductance is thus equal to the drop across the nonlinear inductance: . Two SPICE implementations are considered. The first one, (where stands for non-linear device in version 1), shown in Fig. 6 , corresponds to the case where current dependent functions and of the LR pair has a constant ratio that does not depend on i . The represents a simplified version of the implementation that follows in . The implementation can be used to simulate the circuit model with parameters obtained using the NLS fitting method where is met, while the implementation allows for a current-dependent ratio . Thus, the implementation enables the simulation of a more general circuit model with function (e.g., obtained using the NN) while remaining applicable to models with constant . There are two main advantages of the implementation over the more general implementation . First, its simplicity, which makes it faster in simulations. Second, its ability to yield solutions that can be directly compared with the analytical approach, which also requires a constant (see Appendix). The input for the implementation is only one function and one value . The implementation requires two functions as input: and . These functions are provided as tabular data and interpolated into smooth functions using SPICE’s syntax with spline interpolation. This approach ensures that even a small number of data points used to define or U ( i ) can result in smooth time-domain current and voltage output. In this paper, all the current dependent functions are defined at 32 discrete i points corresponding to the currents for which the impedance measurements are made (see Figs. 2 , 4 a-b, and 5 a-b). The SPICE implementations shown in Fig. 6 are constructed using the following basic SPICE syntax elements: Vm – A Voltage Source with zero voltage, used solely to obtain current between the nodes pos and neg. Ex – A Voltage Dependent Voltage Source. The output voltage is controlled by the voltage difference between the ground node (0) and the control node (1). Bx – An Arbitrary Behavioral Current Source where the source current is controlled by the current through the source Vm, according to the formula . L – A linear unit inductor with a value of . This element is used to calculate the derivative of the auxiliary current . R – A linear resistor with a value of (only used in ). This element represents the resistance of the system and accounts for energy dissipation. VmR – A Voltage Source with zero voltage (used only in ), used solely to obtain the current through this voltage source. BXR – Arbitrary Behavioral Voltage Sources (used only in ). The voltage value produced by this source is given by formula . This element represents the resistance of the system and energy dissipation, serving as a generalization of the resistor R in . The behavior of the circuit defined as described above can be illustrated by considering two limiting cases: : In this case, the LR circuit behaves effectively as a purely resistive circuit with resistance R ( i ), and the unit inductance (1H) can be neglected. The voltage u between the nodes 0-1 (see Fig. 6 ), and consequently between the nodes pos and neg, is: for : for : : In this case, the circuit behaves effectively as a purely inductive circuit with inductance L ( i ), thus the resistance R ( i ) can be neglected. The voltage u between the nodes 0-1(see Fig. 6 ) originates from the voltage across the inductor through which the total current passes, is given by: Model validation Overview The validation of the implementation method and the numerical stability of the simulations were carried out using two approaches: For the circuit model shown in Fig. 3 (implemented as a SPICE netlist code) simulations for selected frequencies were performed to conduct harmonic analysis, with the use of the current , where the term represents a small harmonic current, and the term denotes a DC-bias current with a constant value over time, ranging from zero up to the saturation level. As a result, a set of impedances was obtained through simulations and compared with the impedances describing the model according to Eq. 1 . Time-domain analysis was performed, where in the system shown in Fig. 7 , the voltage responses: obtained from simulations and obtained analytically, were compared, both in response to the same time-dependent input current i ( t ) ranging from zero up to saturation in an oscillatory-damped form. The voltage responses were obtained for the circuit model shown in Fig. 3 and the corresponding voltage responses were obtained with analytical formula based on the inverse Laplace transform (Eq. 6 , see Appendix), both for the very same current trace i ( t ). Fig. 7. Open in a new tab Circuit diagram used in SPICE simulations; i ( t ) — forcing signal, v ( t ) — voltage response. Subsequently, the overall modeling approach was validated as follows: The voltage drop across the physical magnetic ring component, , was first measured in the dedicated test setup with a high-current pulse generator. The voltage response corresponded to a time-dependent input current , ranging from zero up to saturation in an oscillatory-damped form. The numerical record of the measured current was also applied in simulations to evaluate the voltage response of the circuit model shown in Fig. 3 . Finally, the simulated was compared with the previously measured . The above points - are discussed in the following subsections. Correctness of implementation method and numerical stability of simulations: low-signals In the simulations conducted for this test, harmonic analysis was performed by applying a small AC current signal superimposed on a steady DC-bias current, following the procedure used in data acquisition with an impedance analyzer and a DC current generator 19 , and subsequently in the model parameter fitting procedure. The results of the harmonic analysis from the simulations were directly compared with the model impedance given by Eq. 1 . The assumption of harmonic analysis is that the analyzed system is linear, meaning that its response is proportional to the magnitude of the input signal. The considered model (Eq. 1 and Fig. 3 ) does not meet these conditions. Consequently, the harmonic analysis is defined here as the analysis of a system linearized around a given operating point determined by the DC-bias current . The harmonic analysis of the circuit model implemented in SPICE netlist code was thus performed using simulations in which the current was passed through the ring model (Fig. 7 ). The amplitude of the AC current was set to mA, to achieve the linear approximation of the system around the operating point defined by the DC-bias current, . Simulations were conducted for frequency f ( Hz) and for selected values of ( A), and subsequently the voltage across the ring model was analyzed. This allows for a point-by-point evaluation of how accurately the model reflects the impedance over the entire range of frequency and DC current. The simulations were conducted using the PySpice package 42 . The impedance of the linearized system was then determined by fitting a three-parameter sinusoidal function, , to both the current signal (excitation) and to the voltage signal (response). Based on the obtained pairs of three parameters for voltage ( , , ), and current ( , ), the value of impedance was computed. Figures 8 a-b show the impedances obtained from simulations for small-amplitude harmonic signals (AC analysis) with a DC-bias current , compared with the corresponding impedances derived from the formula in Eq. 1 , representing the expected impedance of this circuit. Fig. 8. Open in a new tab (a-b) Comparison of the impedance of the ring model impedance represented as a series model obtained from harmonic simulation (points) and the impedance calculated analytically (Eq. 1 ) from the model parameters (solid line) for selected frequencies f and DC-bias current . Simulations were conducted for two models: (a) Model based on NLS classical parameter fitting method and implementation, and (b) Model based on NN AI-driven fitting method and implementation. (c) Error map (RAE, see Eq. 3 ) of the simulations for different frequencies f and DC-bias currents for NN and implementation. The agreement between the curves in Fig. 8 derived from simulations (dots) and from the formula in Eq. 1 (solid lines) demonstrates that the simulated circuit model and its SPICE implementations operate correctly. A quantitative analysis of the accuracy is provided in the form of an error map, shown in Fig. 8 c, calculated as the relative absolute error (RAE sim) of the impedance absolute value according to the following formula: 4 where: represents the impedance obtained from SPICE simulations (AC analysis), and is the circuit model impedance calculated using the formula in Eq. 1 . The impedance was obtained using two implementation methods: , corresponding to the model with parameters obtained via the NLS fitting method, and , corresponding to the model with parameters obtained using the NN fitting method. The RAE sim is presented (Fig. 8 c) only for the case of the model with parameters obtained with use of NN method and the implementation. The simulation results for the model with parameters derived using the NLS method and the implementation has a similar average error of , compared to the for NN fitting method and implementation, with a qualitative distribution similar to that shown in Fig. 8 c, and therefore, it has been omitted from the presentation. For both the considered simulation cases (NLS/ and NN/ ), the region of inaccuracy is concentrated in the current range where strong nonlinearity occurs, i.e., for the DC-bias currents around A. This is due to the relatively large amplitude of in the harmonic simulation, resulting in partial violation of linearity assumption for the circuit model around the operating point. The error from harmonic simulations is significantly smaller than the error associated with fitting the circuit model parameters to the measurement data, indicating the stability and accuracy of the simulations across a wide range of frequencies and currents. Correctness of implementation method and numerical stability of simulations: high-signals To investigate the model’s behavior for large signals, an oscillatory-damped signals were used, spanning a wide range of values, from saturation to saturation (for the given ring, from A to A). Such a signal represents the highest level of deviation from the measurement data used to build the circuit model. To investigate the numerical stability of the simulation and to verify the suitability of the developed model for such demanding conditions (high currents spanning the whole range up to saturation), simulations were performed to analyze the voltage response of the model to an oscillatory current signal with a decaying amplitude. The results are shown in Fig. 9 and Fig. 10 for the circuit model with parameters derived using two methods (NLS and NN) and implemented in SPICE using two methods ( and ). Simulations were conducted at two selected frequencies: 100 kHz and 1 MHz. Fig. 9. Open in a new tab On the left ( a ), the plots show the current flowing through the magnetic ring model (black line) and the voltage across the model (red line) for two circuit models: (top) the model obtained using NLS method and implemented with , and (bottom) the model obtained using NN method and implemented with . Thin lines represent the voltage contributions from individual LR pair within the series. For the model implemented with , the analytically calculated voltage for the entire model (black dashed line) is also shown, overlapping with the simulated voltage (red line). The analytical solution does not apply to since . The middle column ( b ) plots zoom in on the region around the first peak. The plot on the right ( c ) shows the BH curves derived from the presented current and voltage waveforms, according to Eq. 5 . The current in the presented results has a frequency of 100 kHz. Fig. 10. Open in a new tab The notations are consistent with those in Fig. 9 . The driving current in the presented results has a frequency of 1 MHz. For the circuit model with parameters obtained using NLS and implemented with (requiring constant for all currents for each k ), it is possible to derive an analytical solution. The analytical formula allows calculation of the voltage across the ring model as a function of time for any current i ( t ), but is only feasible to obtain under the assumption of constant (see Appendix), therefore, it is applicable only to the implementation. The agreement between the analytical solution for the circuit model, , and the voltage response from the simulation, (see Fig. 9 and Fig. 10 top rows, red solid and black dotted lines) confirms that the simulations are numerically stable and accurate in both linear and nonlinear regions, yielding the expected results. The simulation results for the implementation (see Fig. 9 and Fig. 10 bottom rows, red solid lines), while lacking confirmation through an analytical solution, are qualitatively similar to the implementation results and exhibit no non-physical behaviors. This indirectly confirms the stability and correctness of the implementation. The BH curves shown in Fig. 9 c and Fig. 10 c are plots of B ( t ) as a function of H ( t ), defined as: 5 where, for the considered ring 39 : and are geometric parameters representing the ring cross-sectional area and the magnetic path length, respectively. The agreement between the analytical and simulated solutions also demonstrates that the discrepancies between the NLS- and NN-based models do not arise from the simulation approach or its numerical accuracy. Instead, they are primarily due to differences in the accuracy of the model parameter fitting. Validation of overall modeling approach with experiment The circuit model of the magnetic ring should be applicable to simulations with any excitation signal, including signals with high peak values, ranging from saturation to saturation. Mathematically, this represents an extrapolation of the model beyond the measurement data that was used as input for its construction, obtained using an impedance analyzer and a DC current generator. he saturation-to-saturation signal constitutes a worst-case scenario, being the signal that diverges most significantly from the model’s source data. To verify the correctness of the magnetic ring circuit model for high-peak-value current traces, experimental validation was performed using current traces that spanned the entire nonlinear operating signal range of the ring for given frequency. For this purpose, a dedicated high-current experimental setup was built, where current was generated in an oscillatory circuit consisting of series-connected L and C elements (see Fig. 12 ). In this setup, a capacitor bank was discharged through a high voltage spark gap, generating a damped oscillatory current with a frequency of . Fig. 12. Open in a new tab The schematic of the experimental setup used to verify the voltage drop across the magnetic ring for damped oscillatory currents. The voltage drop across the ring was recorded using a voltage probe connected around the ring, while the current was measured with a shunt resistor. The measured current (see Fig. 11 , black dash-dotted line) was then used as an input to the SPICE simulation with magnetic ring model. In the simulation, the voltage across the ring model with parameters obtained using three different fitting methods (see Fig. 11 , red ,green and yellow line) was analyzed and compared with the experimentally measured voltage across the ring (see Fig. 11 , black line). This approach ensures that if the simulated ring circuit model accurately represents the physical ring behavior, the simulated voltage and the measured voltage should match closely. Fig. 11. Open in a new tab Comparison of the voltage response of the circuit model in transient SPICE simulation with experimental data. Current (black dashed line) represents the current flowing through the generator circuit and the ring in the experiment. The voltage response from the simulation (three color lines) was obtained by feeding the experimentally measured current into the simulation model. Red line represents model obtained with NN fitting method fed with measurement data with calibration (reduction of inductance) while green dashed line is without calibration. Gray range represents spread measured as rms in variation analysis with input data disturbed by average . Yellow dashed line represents voltage from simulation with use of model obtained with NLS fitting method. The black line represents the voltage measured on the ring. Figures b,c,e,f show the same data as (a) with different scales Fig. d presents BH curves of the circuit model in a transient SPICE simulation with experimental data. BH curve obtained with data represents on Fig.11 with corresponding color obtained by formulas Eq. 5 . The comparison results are shown in Fig. 11 . A good agreement between the simulated voltage and the measured voltage is observed except for certain specific areas discussed in Sect. 7.5 below. To gain deeper insight into the discrepancies between measurements and simulations and to assess the impact of the input data and the modeling method itself on the resulting voltage response of the ring, three different ring models are presented and analyzed: Model #1, with parameters obtained using NN fitting method, as in Fig. 4 . Model #2, with parameters obtained using NN fitting method fed with measurement data with calibration. For our measurements, calibration involved subtracting the impedance analyzer fixture impedance, which amounted to subtracting an inductance of H across the entire current range. Model #3, with parameters obtained using NLS fitting method, as in Fig. 5 . Furthermore, an additional analysis, here referred to as a variation analysis, was conducted to statistically and quantitatively evaluate the impact of model discrepancy on the voltage waveform generated by the ring model in simulation. In this analysis, a single neural network (NN) architecture was employed, while 50 distinct sets of perturbed measurement data (impedance as a function of DC-bias current and frequency) were provided as inputs. For each perturbed dataset, the NN produced a corresponding ring model. The measurement data were perturbed by adding low-frequency Gaussian noise. On average, the models generated from perturbed data differed from the model obtained from the original data by approximately (according to the definition in Eq. 3 ). This procedure emulates the inaccuracy of model fitting to experimental data. As a result, 50 modified sets of LR parameters (perturbed models) were derived from the NN when fed with disturbed measurement datasets. Under current excitation derived from high-current measurements, these models yielded 50 various voltage responses, which were subsequently used to compute the root mean squared error (RMSE) between the reference waveform (obtained from noise-free data) and those produced by the perturbed models. The RMS error is shown as a gray area superimposed on the voltages obtained using the original (unperturbed) model. Based on the simulated and measured voltage, the BH curves were calculated using the Eq. 5 and are presented in Fig. 11 d. Discussion From the comparison between the simulated and measured voltage on the ring, together with their corresponding BH characteristics, the following conclusions can be made: The discrepancy between measured voltage responses and simulated ones is mainly observed in the voltage peak range for high currents, particularly in their maximum values and shape. This is due to the fact that the integral of voltage is proportional to the integral of inductance , which causes the error from an inaccurate L ( i ) fit to accumulate at high voltages. The BH curves show that model mismatch strongly affects the maximum B value (post-saturation region). This is because the maximum B is proportional to , which accumulates errors from the inaccurate L ( i ) fit. This is directly related to the integral under the peak and the inaccuracy discussed at the upper bullet point. Voltage waveforms under small current excitation remain robust against model parameter mismatch. The RMS error value is within of the signal magnitude. This is likely due to the absence of error accumulation. The voltage error is then proportional to the error in the model L ( i ). Overestimation of the data used to build the model due to the measurement instrument impedance (i.e., neglecting calibration), which slightly but constantly overestimates the measured inductance (as a function of current), results in increased voltage in the high-current region. This is shown in the enlargement in Fig. 11 f, where the red curve for currents A is almost constant, which agrees with the measurement (black curve). This is also consistent with expectations, i.e., voltage decrease due to the loss of ring impedance after saturation. Overestimation of inductance in the high-current region (see green and yellow curves in Fig. 11 f, for A) translates into a non-zero slope of the BH curve (see green and yellow curves in Fig. 11 d for A). The expected behavior is a zero slope, corresponding to the loss of the material’s magnetic properties. Maximum B is expected to be achieved regardless of current (see black and red curves in Fig. 11 d and Fig. 11 f for A). This indicates the necessity of using correctly measured post-saturation inductance data for the magnetic ring material (calibration involving subtracting the fixture impedance). Models fitted using NLS and NN methods differ within the RMS error range, indicating model consistency within the bounds of parameter mismatch error. Differences in current peak width are observed (see Fig. 11 e, black vs. red curves). Measured peaks are more blurred, i.e., wider and lower. The most probable causes are either inaccuracies in high-current experimental measurements or limitations of the model assumptions. This aspect requires further experimental verification. Five potential causes for the inaccurate matching of simulated and measured voltage responses in the high current region have been identified: Numerical errors arising from simulation or implementation errors – analysis in earlier sections showed that these errors are negligible. Errors resulting from inaccuracies in current or voltage measurements in the experiment - this scenario is possible, but its verification requires extensive dedicated measurement campaign, which is beyond the scope of this work. We consider as possible measurement errors of in the measured voltage and current traces, along with possible unaccounted parasitic inductances or capacitances. Errors resulting from the inaccuracy of model fitting – the parameter fitting process is not exact; an average impedance fitting error of approximately was achieved. Variation analysis showed how fitting inaccuracies affect the voltage waveform and the BH curve. This aspect could be improved by developing better algorithms for determination of model’s parameters. Errors resulting from the quality of data used to build the model – the process of obtaining may contain systematic or statistical errors affecting model accuracy. It is also challenging to accurately measure the frequency dependent ring impedance after saturation, where the residual inductance of the measurement instrument, despite being relatively small, must be properly accounted for. Errors resulting from limitations of the model itself – it is likely that the structure or level of sophistication of the model, consisting of a series of LR elements, is insufficient to capture all features and behavior of the magnetic material. In such cases, the approximation is no longer accurate. Comparison analysis between measurements and simulations indicates that such an effect may exist. Conclusion Although the ring circuit model was developed based on measurements obtained from an impedance analyzer (designed for measuring small-signal responses under a given DC-bias current), the model also qualitatively well reflects the waveform shape of the measured voltage under large current conditions. However, the quantitative accuracy for large currents above saturation ( A) and around the inflection point of the BH curve ( A) is lower than for small currents. It has been shown that the quantitative inaccuracies in the saturation region require further investigation if higher accuracy of the model in this region is desired. In particular, experimental analysis and comparison of the model simulation results with high-current experiments using oscillating currents from saturation to saturation are necessary. This type of signal has been identified as the worst-case scenario, and ensuring accuracy in this region should guarantee model reliability across the entire range of frequencies and currents. Summary and conclusions Summary The study presents a complete method for obtaining a nonlinear magnetic ring model, along with its SPICE implementation, based on low-signal impedance measurements over a wide frequency range and under DC-bias conditions reaching magnetic saturation The measurement data were used to construct a magnetic ring model which, owing to a novel SPICE implementation, is capable of providing a numerically stable response to arbitrary excitation signals. The SPICE implementation of the magnetic ring model was proposed and applied in simulations. Simulation results were discussed for signals with both small and large signal values in order to verify accuracy and numerical stability. A comparison with analytical results, in both the frequency and time domains, demonstrated high numerical accuracy across the full operating range of the model. The implementation, including code and examples, has been made available in a public repository. The developed model was validated against measurement results from the impedance analyzer, with respect to its ability to reproduce the small-signal behavior of the magnetic ring under a superimposed DC current. Harmonic analysis simulations reproduced the measurement data used for model identification with high quantitative accuracy. The model was further verified for large-signal current excitations, i.e., those driving the material from saturation to saturation. This validation was carried out by comparing the simulated ring voltage with that obtained in a dedicated high-current experiment under identical current excitation. The results showed qualitative agreement, although full quantitative consistency was not achieved in certain regions of the signal. These discrepancies were discussed, outlining directions for future research. Parameters fitting procedures of LR elements were identified as the critical factor introducing the largest error for signals entering the nonlinear region, yet they can be improved through more advanced algorithms. In this work, two algorithms were employed: one based on neural networks and the other on classical fitting. In both cases, further refinement of these algorithms is expected to improve the accuracy of parameter estimation. Parameters fitting errors manifest mainly at high current levels due to the accumulation of numerical errors. The fitted function L ( i ), when inaccurate, introduces a cumulative error proportional to . A promising solution appears to be basing the model on fitting the function instead of L ( i ). The limitations of the model arise from the assumptions inherent in the chosen modeling approach. These limitations become apparent at higher current levels and during transitions from the magnetically linear region to saturation. Addressing these limitations may require modifications and refinements to the model, making it a topic for future research. The inaccuracy is probably due to physical effects in the magnetic material, induced by rapidly varying high-peak currents, that are not accounted for in the impedance measurement input data. One suspected effect is the reduction of the skin effect and less deeper field penetration into the material 43 , caused by saturation and the associated loss of magnetic permeability in the core material. A further limitation of the model lies in its confinement to an LR series, which inherently precludes any capacitive behavior in the ring impedance data, such as that observed in phenomena like dimensional resonance. Extending beyond purely inductive-resistive models requires the fitting of a different series, one that incorporates a capacitive (C) element. Conclusions A method based on a series of nonlinear LR elements with positive values provides a straightforward and general way of representing a nonlinear magnetic material in the form of a magnetic ring. A lumped-element model can operate over a wide frequency range. With proper implementation, such a model ensures numerical stability across a broad range of frequencies and currents. A model based on impedance analyzer data under DC-bias can be also applied to high-current signals. By design, the model is expected to and indeed does provide accurate results for signals of the form , where represents any small signal (not necessarily harmonic) with frequency components within the measurement range (here Hz), and a constant current also within the measurement range (here A). The model’s extrapolation accuracy for an arbitrary current i ( t ) depends on how closely i ( t ) is to . The model can be used, for example, to investigate the attenuation of low-level noise and surges with high-frequency components superimposed on a 50/60 Hz slow-varying signal. It can also be applied to dc–dc converters, where the inductor commonly operates under a relatively high DC bias. The applicability and accuracy for signals beyond those used to construct the model are not as precise as for small-signal conditions, yet remain sufficiently reliable to motivate further research. Thanks to this, along with the introduced numerically stable implementation, the model constitutes a ready-to-use nonlinear formulation that operates effectively across a wide range of conditions. Resolving the accuracy limitations for large signals would make this model the ”ultimate model” – one that accurately represents any signal, rendering other models unnecessary. Appendix In the case of a single pair of parallel-connected LR elements, it is possible to derive an analytical formula for the voltage response to any current waveform, even when the system is nonlinear, i.e., when the values of L and R elements are functions of the current, i . The analytical formula exists under the condition that the ratio R ( i )/ L ( i ) remains constant for all values of the current. In the -domain, the impedance of a single LR pair is given by: where . The voltage response of the system to a current passing through the LR element is therefore: 6 where denotes the convolution in the time-domain and ”prime” denotes time derivative. It is important to note that i ( t ) refers to the current entering the LR pair, not the ”local” currents through the separate L or R components. Additionally, it is worth mentioning that only such an approach yields a stable solution in time-domain simulations. If the current were the local current flowing through L or R elements, and the and were decreasing functions of i , the system would have two solutions that are mathematically valid. One solution would correspond to the case in which most of the current flows through the inductance, and the other solution to the case in which most of the current flows through the resistor. In practice, such a system could switch between these two stable solutions during the iterative solving process of the next time step in time-domain simulations, leading to numerical instability manifested by jumping between the two solutions. To analyze the correctness of the derived formula for u ( t ) given in Eq 6 , it is useful to consider two limiting cases: Limiting Case 1 : (resistance dominates, inductance is conducting current), i.e., . For , we have , and thus: Limiting Case 2 : (inductance dominates, resistance is conducting current), i.e., . When (i.e., the total signal time is much smaller than the exponential time constant), we can approximate , and by the definition of convolution: It is worth mentioning that when the current is not provided in an analytical form, but, for instance, as a table of values, the convolution must be performed numerically. Consequently, the solution for in Eq. 6 is not fully analytical. Nevertheless, such a solution is still referred to as analytical in this paper for simplicity and consistency. Author contributions K.K., J.P., M.M., and M.S. contributed to the conceptualization of the study. Methodology and formal analysis were developed by K.K. with input from M.S. Investigation was carried out by K.K. and M.M., with contributions from M.S. Data curation was carried out by K.K. and M.M. Software development, validation, and visualization were performed by K.K. K.K. led the writing of the manuscript, prepared the original draft, and coordinated the integration of revisions throughout the writing process. M.S. critically reviewed and restructured the manuscript including the organization of concepts, definitions, and section structure. All authors reviewed and approved the final version. Funding This work was supported by the National Science Centre, Poland (NCN), under Grant 2019/34/E/ST7/00187. Data Availability The datasets used and/or analysed during the current study are available upon the corresponding author on reasonable request. These include the impedance measurement results Zmsr of the ring presented in Fig.2, Fig.4, and Fig.5, the parameters Lk(i),Rk(i) of the two models used (NLS and NN) and the measurement data (umsr, imsr) presented in Fig.11. The SPICE implementation of the nonlinear LR element shown in Fig. 6 is publicly available at https://github.com/Kamil-KK/nLRSpice, together with an example of its use in a Python script. Declarations Competing interests The authors declare no competing interests. Footnotes Publisher’s note Springer Nature remains neutral with regard to jurisdictional claims in published maps and institutional affiliations. References 1. Hurley, William G, & Wölfle, Werner H. Transformers and inductors for power electronics: theory, design and applications . John Wiley & Sons, (2013). 2. Serrano, D., Li, H., Wang, S., Guillod, T., Luo, M., Bansal, V., Jha, N K., Chen, Yuxin, S., Charles R., & Chen, M. Why magnet: Quantifying the complexity of modeling power magnetic material characteristics. IEEE Transactions on Power Electronics , (2023). 3. Li, H., Serrano, D., Wang, S., & Chen, M. Magnet-ai: Neural network as datasheet for magnetics modeling and material recommendation. IEEE Transactions on Power Electronics , (2023). 4. Jie, Huamin, Zhao, Zhenyu, Li, Hong, Wang, Changdong, Chang, Yongqi, & See, Kye Yak. Characterization and circuit modeling of electromagnetic interference filtering chokes in power electronics: A review. IEEE Transactions on Power Electronics , (2024). 5. Jiles, D.C. & Atherton, D.L. Theory of ferromagnetic hysteresis (invited). Journal of Applied Physics , 55(6):2115–2120 6. Liorzou, F., Phelps, B. & Atherton, D. L. Macroscopic models of magnetization. IEEE Trans. Magn. 36 (2), 418–428 (2000). [ Google Scholar ] 7. Zhang, H., Wang, Z., Long, J., Li, X., Yang, W., Chen, M., Xu, Y., Shi, J., & Ren, L. Research on the magneto-mechanical coupling effect of ferromagnetic cavity based on improved jiles-atherton theory. IEEE Transactions on Instrumentation and Measurement , (2023). 8. Wunsch, B., Skibin, S., Forsstrom, V. & Christen, T. Broadband modeling of magnetic components with saturation and hysteresis for circuit simulations of power converters. IEEE Trans. Magn. 54 (11), 1–5 (2018). [ Google Scholar ] 9. Wunsch, B., Christen, T., Skibin, S. & Forsstrom, V. Broadband circuit model of a ferrite core, including dimensional resonance, saturation, and hysteresis. IEEE Trans. Magn. 55 (7), 1–5 (2019). [ Google Scholar ] 10. Li, X., Kim, D., Neumayer, SM., Ahmadi, Mahshid, & Kalinin, SV. Estimating preisach density via subset selection. IEEE Access , 8:61767–61774, (2020). 11. Salas, R. A. & Pleite, J. Equivalent electrical model of a ferrite core inductor excited by a square waveform including saturation and power losses for circuit simulation. IEEE Trans. Magn. 49 (7), 4257–4260 (2013). [ Google Scholar ] 12. Ravera, A., Oliveri, A., Lodi, M., Beatrice, C., Ferrara, E., Fiorillo, F., Storace, M. Modeling amorphous-core inductors up to magnetic saturation. IEEE Transactions on Power Electronics , (2024). 13. Li, H., Serrano, D., Guillod, T., Wang, S., Dogariu, E., Nadler, A., Luo, M., Bansal, V., Jha, N. K., Chen, Yuxin et al. How magnet: Machine learning framework for modeling power magnetic material characteristics. IEEE Transactions on Power Electronics , (2023). 14. Gustavsen, B. & Semlyen, A. Rational approximation of frequency domain responses by vector fitting. IEEE Trans. Power Deliv. 14 (3), 1052–1061 (1999). [ Google Scholar ] 15. Gustavsen, B. Improving the pole relocating properties of vector fitting. IEEE Trans. Power Deliv. 21 (3), 1587–1592 (2006). [ Google Scholar ] 16. Szewczyk, M., Pawlowski, J., Kutorasinski, K., Burow, S., Tenbohlen, S., Piasecki, W. Identification of rational function in s-domain describing a magnetic material frequency characteristics. In 9th IET International Conference on Computation in Electromagnetics (CEM 2014) , pages 1–2. IET, (2014). 17. Kartci, A. et al. Synthesis and optimization of fractional-order elements using a genetic algorithm. IEEE Access 7 , 80233–80246 (2019). [ Google Scholar ] 18. Kącki, M., Ryłko, M. S., Hayes, J. G. & Sullivan, C. R. Measurement methods for high-frequency characterizations of permeability, permittivity, and core loss of mn-zn ferrite cores. IEEE Trans. Power Electron. 37 (12), 15152–15162 (2022). [ Google Scholar ] 19. Kutorasinski, K., Szewczyk, M., Molas, M., & Pawlowski, J. Measuring impedance frequency characteristics of magnetic rings with dc-bias current. ISA Transactions , (2023). [ DOI ] [ PubMed ] 20. Schröder, Arne, Savca, Alexandru, & Bormann, Dierk. High frequency permeability measurements and modeling of magnetic powder cores under dc bias. IEEE Transactions on Power Electronics , (2024). 21. Mijat, N., Jurisic, D. & Moschytz, G. S. Analog modeling of fractional-order elements: A classical circuit theory approach. IEEE access 9 , 110309–110331 (2021). [ Google Scholar ] 22. Schröder, A., Bradde, T., Bormann, D., Savca, A., & Grivet-Talocia, S. Permeability macromodels for magnetic powder materials under dc bias. IEEE Transactions on Power Electronics , (2025). 23. Ramirez, A., Gustavsen, B. & Ramirez, I. Rational approximation of nonlinear systems via nl-vf. IEEE Trans. Power Delivery 38 (3), 1918–1926 (2022). [ Google Scholar ] 24. Tamayo, J E., Ramirez, A., Ramirez, J M. Rational approximation of a three-phase photovoltaic system via td-vf and nl-vf. In 2023 IEEE Texas Power and Energy Conference (TPEC) , pages 1–5. IEEE, (2023). 25. Ramirez, A., & Gustavsen, B. Relaxed nonlinear vector fitting for calculation of rational approximation of systems defined by input/output responses in the frequency domain. IEEE Transactions on Power Delivery , (2024). 26. Szewczyk, M., Kutorasinski, K., Pawlowski, J., Piasecki, W. & Florkowski, M. Advanced modeling of magnetic cores for damping of high-frequency power system transients. IEEE Trans. Power Delivery 31 (5), 2431–2439 (2016). [ Google Scholar ] 27. Kutorasiński, K., Pawłowski, J., Leszczyński, P. & Szewczyk, M. Nonlinear modeling of magnetic materials for circuit simulations. Sci. Rep. 13 (1), 17178 (2023). [ DOI ] [ PMC free article ] [ PubMed ] [ Google Scholar ] 28. Pawlowski, J., Kutorasinski, K. & Szewczyk, M. Multifrequency nonlinear model of magnetic material with artificial intelligence optimization. Sci. Rep. 12 (1), 19784–19784 (2022). [ DOI ] [ PMC free article ] [ PubMed ] [ Google Scholar ] 29. Leszczynski, P., Kutorasinski, K., Szewczyk, M., & Pawłowski, J. Machine-learned models for power magnetic material characteristics. IEEE Transactions on Power Electronics , (2024). 30. Nagel, L W. SPICE2: A Computer Program to Simulate Semiconductor Circuits . PhD thesis, EECS Department, University of California, Berkeley, (May 1975). 31. Zeltser, I. & Ben-Yaakov, S. On spice simulation of voltage-dependent capacitors. IEEE Trans. Power Electron. 33 (5), 3703–3710 (2017). [ Google Scholar ] 32. Endruschat, A. et al. A universal spice field-effect transistor model applied on sic and gan transistors. IEEE Trans. Power Electron. 34 (9), 9131–9145 (2018). [ Google Scholar ] 33. Corti, F., Reatti, A., Cardeli, E., Faba, A. & Rimal, H. Improved spice simulation of dynamic core losses for ferrites with nonuniform field and its experimental validation. IEEE Trans. Industr. Electron. 68 (12), 12069–12078 (2020). [ Google Scholar ] 34. Cui, H. & Ngo, K. D. T. Transient core-loss simulation for ferrites with nonuniform field in spice. IEEE Trans. Power Electron. 34 (1), 659–667 (2018). [ Google Scholar ] 35. Górecki, K. & Detka, K. Application of average electrothermal models in the spice-aided analysis of boost converters. IEEE Trans. Industr. Electron. 66 (4), 2746–2755 (2018). [ Google Scholar ] 36. Szewczyk, M., Kutorasiński, K. & Piasecki, W. Quantitative analysis of high-frequency material properties in thin-ribbon magnetic cores. IEEE Trans. Magn. 51 (8), 1–6 (2015).26203196 [ Google Scholar ] 37. Szewczyk, M. et al. High-frequency model of magnetic rings for simulation of vfto damping in gas-insulated switchgear with full-scale validation. IEEE Trans. Power Delivery 30 (5), 2331–2338 (2015). [ Google Scholar ] 38. Kutorasinski, K. nLRSpice, (January 2025). 39. MAGNETEC. Product specification for inductive components: M-676 core datasheet. MAGNETEC GmbH , Jan, 2020. 40. Kącki, M., Ryłko, M. S., Hayes, J. G. & Sullivan, C. R. Analysis and experimental investigation of high-frequency magnetic flux distribution in mn-zn ferrite cores. IEEE Trans. Power Electron. 38 (1), 703–716 (2022). [ Google Scholar ] 41. Kaiser, J. & Duerbaum, T. An overview of saturable inductors: Applications to power supplies. IEEE Trans. Power Electron. 36 (9), 10766–10775 (2021). [ Google Scholar ] 42. Salvaire, F. Pyspice. https://pyspice.fabrice-salvaire.fr , (2024). 43. Manterola, A. M., Angulo, L. M., & Diaz, B. Alberto Gascón, Tekbaş, Kenan, Tijero, María, Moreno, Roberto, & Garcia, Salvador G Impedance modeling of common mode ferrite chokes using transmission line theory. IEEE Transactions on Power Electronics 39 (4), 4224–4233 (2024). Associated Data This section collects any data citations, data availability statements, or supplementary materials included in this article. Data Availability Statement The datasets used and/or analysed during the current study are available upon the corresponding author on reasonable request. These include the impedance measurement results Zmsr of the ring presented in Fig.2, Fig.4, and Fig.5, the parameters Lk(i),Rk(i) of the two models used (NLS and NN) and the measurement data (umsr, imsr) presented in Fig.11. The SPICE implementation of the nonlinear LR element shown in Fig. 6 is publicly available at https://github.com/Kamil-KK/nLRSpice, together with an example of its use in a Python script. Articles from Scientific Reports are provided here courtesy of Nature Publishing Group ACTIONS View on publisher site PDF (7.3 MB) Cite Collections Permalink PERMALINK Copy RESOURCES Similar articles Cited by other articles Links to NCBI Databases Cite Copy Download .nbib .nbib Format: AMA APA MLA NLM Add to Collections Create a new collection Add to an existing collection Name your collection * Choose a collection Unable to load your collection due to an error Please try again Add Cancel Follow NCBI NCBI on X (formerly known as Twitter) NCBI on Facebook NCBI on LinkedIn NCBI on GitHub NCBI RSS feed Connect with NLM NLM on X (formerly known as Twitter) NLM on Facebook NLM on YouTube National Library of Medicine 8600 Rockville Pike Bethesda, MD 20894 Web Policies FOIA HHS Vulnerability Disclosure Help Accessibility Careers NLM NIH HHS USA.gov Back to Top