When designing a switchmode power supply, the input EMI filter is often considered the most difficult part because simple means are missing to predict the power supply signature. However, if a SPICE simulator can't give you the complete picture, it can at least help you assess the conducted differential signature and thus give you an idea of the input filter size.
Fig. 1, below, represents a flyback converter whose primary is supplied by the dc voltage stored in the bulk capacitor. This device supplies the high-frequency current pulses, whereas the mains refuels it at a low rate via the diode bridge. The primary current shown by the arrow is called the signature of the supply. Its shape depends on many factors, including conduction mode and any switching glitches.
To size the input LC filter, you must know the level of harmonics generated by the power supply. In a typical EMI laboratory, the SMPS would be supplied by a CISPR-16 compliant Line Impedance Stabilization Network (LISN). The purpose of this network is to:
- Shield the measurement equipment from any incoming parasitics.
- Offer a stabilized 50Ω output impedance from 150 kHz up to 30 MHz and route the noise to the equipment input. The EMI receiver then sweeps the spectrum of interest and displays the energy content at different frequencies.
SPICE can do nearly the same by implementing an equivalent LISN network and Fast Fourier Transform (FFT). The FFT function of a SPICE graphic processor usually implements the Sande-Tooke algorithm. This algorithm evaluates the harmonic coefficients from an array consisting of a binary radix of data points (128, 256, etc.). Depending on the software editor, the processing method can differ.
During the simulation, SPICE continuously modifies its internal time step to provide accurate results. The time step can either be shorter or longer than the TSTEP variable (in the .TRAN statement), depending on the activities of the computed signals. Generally, the minimum time step can't drop below 10E-9 times TMAX, but this boundary also depends upon the proprietary SPICE algorithm.
Without specification, TMAX is fixed at (TSTOP-TSTART)/50. At the end of the simulation, some SPICE simulators, such as Intusoft's IsSpice, invoke before storing the data a linear interpolation algorithm to produce an evenly spaced output at a TSTEP interval. The results are placed in an ASCII SPICE compatible output file that can be examined with the IntuScope investigation tool.
IntuScope also offers the ability to explore the raw simulated data and reinterpolate them with a different step to let the user change the analysis width. CADENCE's PSpice doesn't interpolate the data in its .DAT file, and the user navigates through the raw acquisitions via the PROBE graphical interface.
When the FFT algorithm is initiated, PROBE first interpolates the data to convert the unevenly spaced acquisitions into fixed time step data. It then places the new acquisitions into a data array of the nearest binary radix of points (For example, 128 locations for a 100-point simulation).
The following is a possible SPICE TRANsient command you can use to obtain a 30-MHz analysis bandwidth:
.TRAN TSTEP TSTOP [TSART] [TMAX] [UIC] [optional]
.TRAN 16.6NS 500US 400US 8NS UIC ; 30-MHz sweep range, 10-kHz analysis BW, 6024 points.
To test your SMPS SPICE signature, you need to route the current circulating in the input voltage source to the equivalent model of the real bulk capacitor. An F1 source can do the job, as illustrated by Fig. 2.
Once the simulation has elapsed, an FFT can be run to unveil the harmonic content. The vertical scale is expressed into dBµV by a Log compress of the Y-axis to which 120 is added. Fig. 3 shows you a comparison of simulation and true measurement, the results obtained using the method.
Without avoiding having to run a bench measurement, the SPICE method helps to quickly portray the harmonic content of a given SMPS signature and gives an idea of the needed differential filter. To link to models, examples, circuits etc., you can download these files from the Web at perso.wanadoo.fr/cbasso/Spice.htm — a site which is dedicated to my book, “Switch-Mode Power Supply SPICE Simulation Cookbook.”
For more information on this article, CIRCLE 339 on Reader Service Card CIRCLE 238 on Reader Service Card