Click to edit Master text styles
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.
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.
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 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
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
In a general way we can express
them again by the complex phasor form. [>>]
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
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
can run SPICE simulation of a linear network, that is driven by a modulated
signal, by splitting the network into the two components. The real part and the imaginary part, and
running them simultaneously on the simulator.
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.
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.
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
This method, which was developed
by our group, is also referenced in the printed paper.
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,
can represent the modulated signal as two orthogonal components, which are the
envelope vector parts U1 and U2. [>>]
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
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.
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
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
For example: amplitude
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.
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 [>>].
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 [>>] [>>] [>>]
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.
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  of
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.
results of output voltage versus carrier frequency are shown here. The
analysis was repeated for different resistive loads.
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