Produkte

Produkte

Leistung

HF

Transformatoren

Tools für Design-Support

Nutzen Sie unsere ‚Suite of Tools‘ für die Auswahl, die Analyse und den Vergleich von Induktivitäten

Alle Tools anzeigen
Parametrische Suche

Lassen Sie sich die Liste unserer Induktivitäten und Filter zu Ihren Parametern anzeigen.

Erforschen
Datenblätter

Sie suchen nach einem Datenblatt? Suchen Sie nach Produkt und laden Sie das PDF herunter

Liste anzeigen
Automobiltechnik

Informationsmaterial

Informationsmaterial

Produktdokumentation

Handhabung und Verarbeitung

Modelle und Layout-Tools

Kurse/Schulung

Video-Bibliothek

Cx Family Common Mode Chokes

0402CT Low Profile Chip Inductors

XAL7050 High-inductance Shielded Power Inductors

XGL4020 Ultra-low DCR Power Inductors

Student Support

Learn more about magnetics, request free samples or ask our engineers a question.

Get Support
Quality

Quality

Qualitätszertifizierung

Materialzertifizierung

Sicherheitszertifizierung

Zuverlässigkeit

Handhabung / Verarbeitung

Über

Über

Über

Jobs

Standorte

Informationsmaterial

Inductor SPICE models are intended to be virtual representations that behave in simulations like real inductors do in physical circuits. For this to be true, models must be designed carefully to capture all the appropriate characteristics of the inductor. Furthermore, the simulation may give the wrong impression if it is being used to verify operating conditions other than those originally intended by the model creator.

In part I of this series, we will discuss the challenges and limitations of modeling inductors. Then we will provide examples of how to select the appropriate inductor model for various types of simulations. Ultimately, we will explore the variety of Coilcraft inductor models for meaningful simulations in each type of application.

Frequency-domain models are typically made from

Power supply simulations involve switched voltages, which include startup transients and steady-state time-domain

It is important to note that you cannot assume that low-current, frequency sweep-based models have been verified against the high-current time-domain conditions of a power supply. If current is high enough to cause the inductance to change due to saturation, the simulation results will suffer. A saturation model is needed to simulate saturation effects.

When using inductor models for loss or efficiency analysis, the model must capture current-dependent and frequency-dependent loss. Traditional models that use a fixed value parallel resistor to model core loss do not capture frequency-dependent (AC) loss. Even when a frequency-dependent parallel resistor is used, this type of model often has poor correlation with real measurements of core loss at higher current.

The Steinmetz equation is typically employed to describe the flux-density- and frequency-dependence of core loss. Core manufacturers curve-fit measurements to facilitate calculations of core loss over a range of operating conditions. As evidenced by various core material loss curves, the Steinmetz equation is only useful over a narrow range of frequencies. Therefore, a single Steinmetz equation for core loss does not fully capture all operating conditions and ignores conductor losses.

While the brightest minds in magnetics are working to develop improved loss models, a universal inductor SPICE model that captures all AC loss mechanisms (core loss, skin effect, proximity effect, radiation) does not yet exist. Physics-based models for capturing such loss mechanisms appear to be on the horizon, however, a practical model is not yet available to inductor manufacturers.

The error of an inductor measurement is calculated from the measurement instrument, test fixture, and calibration standard specifications. For a very low inductance value ceramic core chip inductor with ±2% inductance tolerance, there is little room for measurement error. For a higher value power inductor with ±20% inductance tolerance, more variation in the measurement is expected. A Monte Carlo analysis may be useful for simulating the inductance tolerance effects on the circuit, however, the variation of parasitic capacitance and other parasitics is never part of the model.

Meaningful low inductance value RF inductor models require capturing the interaction between the inductor and the printed circuit board. The interaction will have a significant effect at higher frequencies, determining the resonant frequency of the PCB-mounted inductor. Adding such parasitics requires measurement, experience, or the availability of a substrate-dependent model for a realistic simulation at high frequencies.

For this example, a basic (e.g. LTspice) inductor model that includes only L and DCR is likely sufficient. If the simulated current is close to the I

A basic model that does not include self-resonating parallel capacitance would not suffice in this case. Choosing a frequency-domain model – such as the Coilcraft RF inductor model – that includes Laplace elements and parallel capacitance with series resistance to capture the peak of resonance, is more appropriate. Using a substrate-dependent model, or adding PCB parasitics to the model, will increase the likelihood of the simulation matching real-world measurements of the LC filter.

Because the inductor simulation is in the time domain (transient), a model with Laplace elements is not appropriate. To capture the impedance, a time-domain model that includes a resistive element in series with the parallel capacitance, is most appropriate. Coilcraft has developed “Impedance” models for simulating this type of application. These models are based on low-current measurements. If the magnitude of the current pulse is near the I

Basic inductor models are made from low-current measurements that do not capture the drop in inductance with current. A saturation model is needed for this simulation. Coilcraft has created “Saturation” models to address this type of simulation.

**LTspice inductor model library**– Basic models included within the LTspice standard inductor library**Advanced frequency-domain models**- Coilcraft LTspice inductor library
- Coilcraft Pspice library
- Coilcraft SPICE model documents and s-parameters

**Substrate-dependent models**– Modelithics inductor library**Impedance models (time domain)**– Coilcraft LTspice inductor library**Saturation models (time domain)**– Coilcraft LTspice inductor library**Power inductor loss models**– Coilcraft Design Tools

While the basic LTspice inductor models include parallel capacitance to model self-resonance, Coilcraft leaves this value set to zero because the model does not include a resistor in series with that capacitance. This lack of resistive damping causes simulated narrow spikes that are not present in measurements of the real inductors. Most switching regulators switch at frequencies well below the inductor’s SRF, making these models appropriate under that condition.

For small-signal frequency-domain simulations near the inductor SRF, Coilcraft Advanced frequency-domain models are best. These are published as Coilcraft SPICE model documents and s-parameter files (for RF inductors), with netlists and symbols included in our LTspice and Pspice libraries.

These small-signal models capture frequency-dependent inductance and resistance using Laplace elements. The models are based on low-current frequency sweeps and can be used in most SPICE simulators. They are measurement-based, not basic/idealized models, providing realistic results at high frequencies. The capacitance with series resistance (R1) makes these models appropriate for a preliminary EMI analysis.

These small-signal models capture frequency-dependent inductance and resistance using Laplace elements. The models are based on low-current frequency sweeps and can be used in most SPICE simulators. They are measurement-based, not basic/idealized models, providing realistic results at high frequencies. The capacitance with series resistance (R1) makes these models appropriate for a preliminary EMI analysis.

Also for small-signal simulations, Modelithics’ MVP library of Coilcraft RF inductors captures substrate-dependent PCB parasitic effects. These measurement-based models were developed by Modelithics and are available for download from the Modelithics website.

To address the need for small-signal transient and steady state time-domain simulations of our power inductors and chokes, Coilcraft has developed measurement-based impedance models for LTspice. These are included in the Coilcraft LTspice inductor library. The impedance models use fixed value inductance, resistance and capacitance elements for time-domain simulations that avoid DC operating point errors involved with Laplace elements.

Coilcraft has also developed __large-signal__ inductor saturation models for our soft-saturating power inductors. These are included in the Coilcraft LTspice inductor library. The saturation models capture any inductance drop at higher current levels, which provides more meaningful ripple current simulations in power supplies. These models are based on inductance vs current measurements for each individual inductor.

While a universal SPICE model that captures all loss mechanisms is not readily available, Coilcraft has developed loss calculation tools for our power inductors. The loss calculations are based on measurements under a wide range of conditions. They include DC and AC loss, comprising core loss, skin effect, and proximity effect. These loss calculations are based on user-entered operating conditions, such as switching frequency, ripple current, and ambient temperature. The calculations are built into our online Power Inductor Finder and Analyzer and DC-DC Optimizer tools.

**See part II, to learn how to overcome challenges and limitations of modeling transformers in SPICE**

- Assistance with Safety Agency Approvals
- Basics of Inductor Selection (from Electronic Design magazine)
- Calibration, Compensation, and Correlation
- Current and Temperature Ratings
- Getting Started: An Introduction to Inductor Specifications
- Hipot Testing of Magnetic Components
- How Current and Power Relates to Losses and Temperature Rise
- Measuring Self Resonant Frequency
- Operating Voltage for Inductors
- Selecting Current Sensors and Transformers
- Simulation Model Considerations: Part II
- S-parameters for High-frequency Circuit Simulations
- Testing Inductors at Application Frequencies
- Working Voltage Ratings Applied to Inductors

- PCB Washing and Coilcraft Parts
- Selecting Flux for Soldering Coilcraft Components
- Soldering Surface Mount Components

- Broadband Chokes for Bias Tee Applications
- Inductors as RF Chokes
- Key Parameters for Selecting RF Inductors

- Beyond the Data Sheet: The Need for Smarter Power Inductor Specification Tools
- Choosing Inductors for Energy Efficient Power Applications
- Current Sense Transformers for Switched-mode Power Supplies
- Determining Inductor Power Losses
- Ferrite Vs Pressed Powder-core Inductors
- Forward or Flyback? Which is Better?
- Notes on Thermal Aging in Inductor Cores
- Selecting Coupled Inductors for SEPIC Applications
- Selecting Inductors to Drive LEDs
- Selecting the Best Inductor for Your DC-DC Converter
- Structured Design of Switching Power Transformers
- Transformers for SiC FETs

- Coilcraft LC Filter Reference Design
- Common Mode Filter Design Guide
- Common Mode Filter Inductor Analysis
- Data Line Filtering
- Fundamentals of Electromagnetic Compliance
- Passive LC Filter Design and Analysis
- Selecting Common Mode Filter Chokes for High Speed Data Interfaces

- Applying Statistical Techniques to the Design of Custom Magnetics
- Choosing Power Inductors for LiDAR Systems
- Coilcraft Conical Inductors
- Designing a 9th Order Elliptical Filter for MoCA® Applications
- Measuring Sensitivity of Transponder Coils
- Power-handling Capabilities of Inductors
- Signal Transformer Application
- Transponder Coils in an RFID System
- Using Baluns and RF Components for Impedance Matching
- Using Standard Transformers in Multiple Applications