Simon Lineykin and Sam Ben-Yaakov* Thank You, mister chairman. Good morning. The topic of this presentation is: [Large and small signal simulations of circuits driven by a modulated signal, using ENVELOPE SIMULATION METHOD.] The study was conducted at the power electronics laboratory of Ben-Gurion University A Unified SPICE Compatible Model for Large and Small Signal Envelope Simulation of Linear Circuits Excited by Modulated Signals Simon Lineykin and Sam Ben-Yaakov* Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev P. O. Box 653, Beer-Sheva 84105, ISRAEL Phone: +972-8-646-1561, Fax: +972-8-647-2949 Email: sby@ee.bgu.ac.il, Website: www.ee.bgu.ac.il/~pel

Power System Driven by a modulated signal The [simulation tool that was developed in this study] is related to the [problem of a power electronic systems] that are [driven by modulated signal]. [If the system is reactive] than the [frequency modulation] will translate into [amplitude modulation] Power System Driven by a modulated signal

Example 1: a Resonant Network Excited by a Modulated Signal For example: Consider the [Piezoelectric transformer], which is [in close-loop configuration]. The power is controlled by a frequency shift. So, in close loop, we measure the output voltage. The [error signal] is shifting the frequency. Since the Piezoelectric Transformer is, basically, resonant network,  the [frequency shift] will be translated into an [Amplitude Modulation]. So, [for designing the feedback loop] there is a need to get a transfer function between the [frequency shift] and the [envelope change]. Example 1: a Resonant Network Excited by a Modulated Signal

Example 2: Electronic Ballast Another example is an [electronic ballast for fluorescent lamp]. If we would like to operate the ballast in the close loop, then we would need to know, (in order to design the feedback), the small signal transfer function between the frequency shift and the envelope changes at the output. The method of envelope simulation was presented earlier, however, (for the sake of clarity), I will go now over some basic elements. So that we can get into the specific issues of the present study. Example 2: Electronic Ballast

A Primer to Envelope Simulation Any modulated signal can be broken into orthogonal components. One can show that general expression is equal to the REAL part of the phasor expression, where phasor of carrier frequency fc has a complex envelope. If the network is excited by modulated signal, all currents and voltages in the network will be also modulated. In a general way ->> we can express them again by the complex phasor form. A Primer to Envelope Simulation Any analog modulated signal (AM, FM or PM) can be described by the following expression: The Current in the network excited by u(t):

As was shown in a previous study, a reactive network that is excited by a modulated signal, can be broken into two sub-circuits: A REAL and IMAGINARY parts. After dropping the carrier component, an INDUCTOR, for example, will be split into two interdependent sub-circuits] ->>, ->>, ->>, ->> Phasor Analysis Inductance

Similarly a CAPACITOR will also be split into two interdependent sub-circuits. It should be noted that the carrier frequency is presented as constant parameter in the dependent sources of the reactive elements. Since resistance equation does not include any derivation or integration, the RESISTOR remains as is in both sub circuits, without coupling elements. All non-reactive elements like the resistor: Gains, Transformers etc. Will also stay as they are in REAL and IMAGINARY components. Phasor Analysis Capacitance Resistance

We can run SPICE simulation of a linear network, that is driven by a modulated signal, by splitting the network into the two components. ->> Splitting the Network into Two Cross-Coupled Components - Imaginary and Real

The REAL part and the IMAGINARY part, and running them simultaneously on the simulator. The amplitude of voltage at any given point of original network may be calculated by the square root of the sum of squares of the imaginary and real components of the equivalent circuit. The rules for breaking the circuit into the two sub circuits are given in our earlier papers, which are referenced in the printed proceeding. Splitting the Network into Two Cross-Coupled Components - Imaginary and Real Real Load Component Imaginary Load Component

Simulation Alternatives Cycle-by-cycle (full simulation) High and low frequencies Very long simulation Only transient AC transfer function -> point-by-point Envelope simulation (Large Signal -Previous study) Only low frequency

Example: Piezoelectric Transformer Driven by FM Signal (SPICE) As the example to the use of envelope simulation, according to the method developed earlier, we consider here again the network of Piezoelectric Transformer, driven by frequency modulated signal, including a rectifier and and a load. ->> Example: Piezoelectric Transformer Driven by FM Signal (SPICE)

Example: Piezoelectric Transformer Driven by FM Signal (SPICE) The Piezoelectric transformer is, basically, a resonant network, including input and output capacitors, and transformer, that emulated by dependent sources. The AC voltage, developed at the output, is fed to a rectifier. Using the method of equivalent circuit, one can emulate a rectifier plus load, as an linear reactive AC load.

Example: Piezoelectric Transformer Driven by FM Signal (SPICE) This method , which was developed by our group, is also referenced in the printed paper. Example: Piezoelectric Transformer Driven by FM Signal (SPICE)

Example: Piezoelectric Transformer Driven by FM Signal (SPICE) In this example we drive the network by an FM-signal, which can be represented as shown here. The um is the modulating signal. If we assume that um is a harmonic signal,  - Harmonic modulating signal

Example: Piezoelectric Transformer Driven by FM Signal (SPICE) One can represent the modulated signal as two orthogonal components, which are the envelope vector parts U1 and U2. Example: Piezoelectric Transformer Driven by FM Signal (SPICE)

OrCAD Schematics for Envelope Simulation Following the procedure discussed above, we duplicate the original circuit, including the dependant sources to get the real component  And the imaginary component  And put two excitation components. To get the output, we need to calculate the square root of sum of squares  OrCAD Schematics for Envelope Simulation (Large Signal)

Results of Full and Envelope Transient Simulations Here are the result of the envelope simulation and the full simulation. The solid lines correspond to the envelope simulation and the gray area – to the full cycle-by-cycle simulation. This is a modulating signal. This is a FM input. We can not see the frequency changes, the amplitude stays constant and its envelope stays constant. At the output we will have the carrier, modulated both by frequency and amplitude. The envelope line shows the amplitude changes. Results of Full and Envelope Transient Simulations The modulating input signal Envelope The Frequency modulated signal Cycle-by-cycle Envelope Output signal Cycle-by-cycle

Objectives of this Study In this study we extended the method of envelope simulation to include an AC analysis directly, rather then running the transient analysis and collecting the data point-by-point. Another objective was to make the same model compatible with all three types of analysis: AC, DC, and Transient. The idea is to replace the two independent excitation components by a single signal source that is split into real and imaginary components. Once this is accomplished, the splitting network can be linearized to obtain the AC excitation components U1 and U2. Since the network itself is linear, it could be left as is. Objectives of this Study To extend the envelope simulation method to AC analysis A method that would not need an analytical derivation Same model compatible with DC, AC, and Transient analysis types

Proposed Method – Small Signal Analysis Using AC–Simulation For example: Amplitude Modulation. Expanding the expression of modulated signal into two orthogonal components, one can see that in the case of AM  only the real component U1 exists. The splitting network is driven by a single signal um is making the imaginary component – zero and real component U1. The dependent source multiplies the input signal by a constant and adds it to a DC source that represents the amplitude of carrier. The network is actually linear and we just have to replace the excitation um by phasor source VAC for analysis. Proposed Method – Small Signal Analysis Using AC–Simulation Amplitude modulation phasor The source is linear and suitable for AC analysis – as is

Linearization of Sources for Angle Modulation In the case of phase modulation there are two nonzero components of the real and imaginary parts of excitation. The splitting network multiplies the input signal by a constant and makes it as as argument of Cosine in the real component and the Sine in the imaginary component. This network includes nonlinear elements. Nevertheless, for small signal analysis, the Cosine of small angle is approximately one, and the Sine of small angle is approximately angle itself. Thus for real component we have a constant  And for imaginary component – the input signal multiplied by constant. This network is linear and suitable for AC analysis, using phasor input VAC Linearization of Sources for Angle Modulation Phase Modulation phasor =Ac Small signal Linear source =Ac*kp*u(t) Small signal PM – Nonlinear source

Linearization of Sources for Angle Modulation Using analogous procedure one can get the splitting network for FM signal. The only difference is the integration of the modulating signal. Under the same assumptions for small signal, one can linearize the network , ,  And use it for AC simulations with phasor source VAC. Linearization of Sources for Angle Modulation Frequency Modulation phasor =Ac Small signal Linear source =Ac*kp*u(t)dt Small signal FM – Nonlinear source

Here are the results of small signal envelope simulation using phasor source and linear splitting network, and the results of a point-by-point transient simulation method. Both simulations were carried out on the Piezoelectric Transformer with rectifier, driven by FM signal, for three different carrier frequencies. The solid lines are results of AC analysts, which runs quickly, And the marked points were done using point-by-point transient envelope simulation of large signal model of previous study. One point per analysis. As one can see, the agreement is very good. Results: Piezoelectric Transformer Driven by FM signal (AC and Point-by-Point) for Different Carrier Frequencies

One should note that an envelope analysis is not approximation. It is represents the numerical result of an exact analytical solution, both for large signal and AC analysis. So the agreement between the transient and AC simulations is not surprising. It just shows that we didn’t do any mistake preparing the files or taking the measurements. This simulation results were also verified against experimental results of reference [5] of printed paper. Results: Piezoelectric Transformer Driven by FM signal (AC and Point-by-Point) for Different Carrier Frequencies

Now, extending the ideas of envelope simulation, we can run the response of the network to a drive signal over a given frequency range. This case is, in fact, the steady-state solution. The amplitude of the carrier is constant, and the only parameter to sweep is the frequency fc. So we can run the circuit as it is with fc parameter sweep. Frequency Response of the Network (unmodulated input signal) using DC-sweep DC-sweep in envelope simulation is equivalent to frequency sweep in full simulation The parameter of DC sweep is a carrier frequency fc The source for DC sweep:

Simulation results of output voltage versus carrier frequency are shown here. The analysis was repeated for different resistive loads. Example: Frequency Response of Piezoelectric Transformer with Different Resistive Loads

Conclusions This bring us to the conclusion of this presentation. In this study we have extended the method of envelope simulation to include AC analysis and DC-sweep. The method is suitable for linear circuits. But by converting a non-linear parts of the circuit into an equivalent circuit which is linear, we can also simulate the nonlinear circuits by this method. thank you for your attention Conclusions Envelope simulation method was extended to cover all simulation types: Transient, AC, DC. Method is suitable for any linear circuit. Method is also suitable for nonlinear circuits that can be linearized for small signal.