What simulation software is generally used when making switching power supplies?

木犯001号

What simulation software is generally used when making switching power supplies? [Copy link]

There are many common simulation software, but for switching power supplies, because of the higher requirements for parameters, simple simulation models often cannot get correct results, and even the simulation results are far from the actual results. So, what simulation software will be more competent?

Everyone is welcome to talk about the simulation software you use and share your opinions.

The following is an analysis of various simulation software that I found, the original author is unknown:

Author: Zhihu user
Link: https://www.zhihu.com/question/263844056/answer/273847914

For device-level simulation, LTspice is recommended, which is easy to use. However, PSpice has the most resources and Saber has the strongest modeling capabilities. For circuit-level simulation, Matlab/Simulink is recommended, which has many control-related tools and learning resources. To do simulation well, the key is to have a deep understanding of circuit principles.

The simulation software that may be used in power electronics include PSpice, Saber, LTspice, PSIM, Matlab/Simulink, Ansys, Simetrix/Simplis, etc. To understand these simulation software, you must first understand the problems to be solved:

1. Numerical methods, analytical methods and simulation

Take solving a step-excitation RC charge-discharge circuit as an example. First, list the equations based on Kirchhoff's voltage-current law and the voltage and current constraints of resistors and capacitors, and then solve the differential equations. To solve differential equations, you can directly calculate a general solution by hand (analytical method), or you can use a computer to solve the equation to get a specific numerical solution (numerical method). Under a certain excitation, the method of solving the equation by computer to get the numerical solution of the problem of interest and presenting it in the form of curves or text is called simulation.

2. Electric field, magnetic field and circuit, magnetic circuit, electromagnetic field simulation and circuit simulation

In essence, the electromagnetic problems we encounter are all problems of electromagnetic field distribution. In most cases, the distribution of electromagnetic fields is constrained by the medium. The study of electromagnetic field problems becomes the study of circuit magnetic circuits. The description of electromagnetic fields is simplified from partial differential equations about space and time to differential equations about time. When the three-dimensional characteristics of the electromagnetic field cannot be ignored, it is necessary to study the spatial and temporal distribution of the electromagnetic field, that is, it is necessary to solve partial differential equations (dx, dy, dz and dt). Ansys is a software that can solve partial differential equations, that is, it can simulate the field. There is also a similar software called COMSOL. In the design of high-frequency transformers, the three-dimensional spatial distribution of the electromagnetic field has a great influence on the electromagnetic performance of the device, so it is necessary to study the electromagnetic field distribution, that is, to use Ansys simulation. Similarly, Ansys can also simulate thermal fields and study thermal design. The numerical method for solving three-dimensional fields is usually the finite element method. When the three-dimensional characteristics of the electromagnetic field can be ignored, the electromagnetic field becomes a circuit magnetic circuit. At this time, it is only necessary to solve differential equations, that is, software that can simulate the circuit. Pspice, LTspice, Saber, Matlab, etc. belong to this category. The electromagnetic fields of most electronic components we come into contact with are carefully designed, and the spatial distribution is very regular. From the user's perspective, the device can be described by differential equations, so it is generally studied using circuit simulation software. In the same way, the thermal field can be simplified into a thermal circuit, and the temperature distribution can be studied using the concepts of thermal resistance and thermal capacitance. Some circuit simulation software can be used to simulate temperature transients.

3. Dynamic characteristics simulation, switch ripple simulation, switch loss conduction interference simulation - distinguish research problems from the frequency domain, distinguish simulation software from the switch model

The three questions distinguish the three frequency domains we are concerned about, low frequency, switching frequency and radio frequency. The corresponding simplest switch models that can simulate the corresponding frequency domain characteristics are the average switch model, the ideal switch model simulated by resistance (equivalent to milliohm resistance when on, equivalent to megohm resistance when off) and the behavioral model considering parasitic capacitance and parasitic inductance. The average switch model is less intuitive and is used less frequently. Most simulations of control loops still use the ideal switch model, and the corresponding simulation time is much longer than that of the average switch model. MATLAB/SIMULINK and PSIM only provide ideal switch models, so they generally simulate control loops and switch ripple level waveforms. If you need to care about high-frequency switching losses and EMI characteristics, that is, the radio frequency range, you need a more accurate model, that is, a behavioral model considering parasitic capacitance and parasitic inductance. Spice-type simulation software such as PSPICE, LTSPICE, SIMETRIX and Saber will provide a library of detailed parasitic parameter models, so they can be used for device-level simulation. It should be emphasized that it is not that SIMULINK cannot build a more accurate model, but that SIMULINK does not have the relevant model resources, that is, the library, so SIMULINK is generally not used to simulate device behavior. The frequency range of interest determines the accuracy of the modeling, the accuracy of the required model determines the model we need, and the support for the required model determines the selection of the simulation platform, that is, the resources of the platform determine the availability of the platform [1].

Additional notes:

Psim: Psim also supports Spice simulation, mainly because this software has two simulators, one for control simulation and the other for device simulation (SPICE simulation).

In fact, most simulation software has two simulators. Simetrix supports not only Spice but also Verilog, and Saber supports not only MAST but also VHDL. In addition, Simetrix/Simplis refers to two softwares, but they are integrated together, one is Simetrix and the other is Simplis. Simplis is different from the usual circuit simulation software. It models the components by piecewise linear method, so the solution speed is also faster. For details, please refer to the help document.

4. Hardware Description Language and Simulator, Macro Modeling

The circuit needs to be described in a language that the computer can understand, that is, the hardware description language. The computer uses simulation software (simulator) to understand the corresponding hardware description language, solve it, and output the result. The circuit described by a specific hardware description language needs to be solved by the corresponding simulator. Common hardware description languages include Spice language (SPICE-type simulation software such as PSpice, LTspice, Simetrix, etc. can be solved), MAST language (Saber simulation software can be solved), Verilog-HDL language (a standard language, Simetrix has a corresponding simulator), VHDL language (a standard language, Saber has a simulator), and SIMULINK has its own hardware description language, which can be seen by opening the model description. Components are defined by mathematical expressions. MAST, Verilog-HDL, and VHDL can directly define a component with mathematical expressions, which is true behavioral modeling. Therefore, this type of simulation software is also more suitable for modeling and simulation in multi-physics fields, as long as the mathematical relationship of the object is clear. You can see that there are many heat sink libraries in Saber. In addition to defining through mathematical expressions, you can also encapsulate the commonly used mathematical expressions of components into basic units, and describe the components through the combination of basic units. Generally, the basic units are capacitors, resistors, inductors, controlled voltage sources, current sources, etc. This modeling method is macro modeling, and SPICE is a macro modeling language. Obviously, true behavioral modeling languages also support macro modeling, but the advantage of macro modeling is that the physical meaning is clear. PSpice has a corresponding behavioral model library (ABM library) to enhance the ability to describe components, which is not much worse than a true behavioral modeling language.

5. Types of nonlinear time-varying system and circuit simulation analysis

When using Spice simulation software or Saber to analyze a circuit, you need to select the analysis type. Common ones include DC analysis, transient analysis, and AC small signal analysis. Here I will focus on DC analysis, mainly the question of whether a switching circuit needs DC analysis. A switching circuit is essentially a nonlinear, time-varying system. The so-called time-varying means that the circuit structure changes with time, and there is no concept of time in DC analysis, so DC analysis is meaningless for switching circuit analysis.

That’s all for now. I would like to recommend a few books. If I can only recommend one, I would recommend [4], which is very suitable for beginners. [6] and [7] are also very suitable for beginners. [3][4][6][7][8] all have corresponding Chinese translations. The English version can usually be downloaded.

[1] Dynamics and Control of Switched Electronic Systems, Chapter 13: An Overview of Simulation Tools

[2] The help of various simulation software. Saber’s help “The Designer’s Guide to Analog & Mixed-Signal Modeling” has a lot of modeling theory and is worth reading.

[3] Model-Based Engineering for Complex Electronic Systems-Elsevier Science (2011), various modeling theories and modeling methods, and Saber's The Designer's Guide to Analog & Mixed-Signal Modeling complement each other.

[4] SPICE for Power Electronics and Electric Power, third edition. Note that the PSpice schematic input mentioned there now only supports ORCAD input, while another type was supported historically.

[5] Inside Spice, detailed principles of simulation are also found in [2] and [3], but they all seem to be derived from this book.

[6] Analog Design and Simulation using OrCAD Capture and PSpice-Newnes (2011) is also relatively basic and very suitable for beginners.

[7] PSPICE and MATLAB for electronics _ an integrated approach - CRC Press (2010). I haven’t read much of it and it’s quite basic, so it’s suitable for beginners. Here, MATLAB is just a calculation tool, not a simulation software.

[8] Spice Simulation and Practical Design of Switching Power Supplies - Basso, a good introduction to switching converter modeling and simulation.

okhxyyo

Thank you for sharing~~ The download center also has relevant collections, and netizens who need it can download it