**Steady
State Sinusoidal Transient Analysis**

University of Evansville

In addition to LTspice IV, this tutorial assumes that you have installed the University of Evansville Simulation Library for LTspice IV. This library extends LTspice IV by adding symbols and models that make it easier for students with no previous SPICE experience to get started with LTspice IV.

**An
Example Circuit****
**

In
this tutorial you will learn to determine the sinusoidal steady
response of RLC circuits. We will use LTspice IV to determine the
currents *i*_{1} and *i*_{2} in the circuit
shown in Figure 1. The source voltages are equal to *v*_{1}
= 10 cos 1000*t* V and
*v*_{2}
= 20 cos(1000*t* –
30º)
V.

Figure 1: Example Circuit

The
corresponding LTspice IV schematic is shown in Figure 2. The
resistors R1 and R2 are oriented in agreement with the desired
current directions in Figure 1. (The currents through L1 and L2
could also be used to determine *i*_{1}
and *i*_{2}.)

Figure 2: LTspice IV Schematic

The
settings for voltage source *v*_{1} and *v*_{2}
are shown in Figure 3. Note
that the Freq value shown in Figure 3 corresponds to ω/(2π)
where ω = 1000 rad/s for this source. You can enter
mathematical expressions for values, but the entire expression must
be enclosed in curly braces. Note also that LTspice IV uses a sine
function as its reference sinusoidal waveform whereas *v*_{1}
and *v*_{2}
were specified as being cosine functions. Although we could
transform the LTspice IV sine function to a cosine function by adding
in a +90º phase shift, it is easier just to pretend that our
sources are sine functions instead and measure
the phase shifts of the current relative to a reference sine
function.

The
voltage settings for *v*_{2}
are very similar to those for *v*_{1}
except that the Amplitude is equal to 20 and the phase angle is -30.

Figure
3: Voltage Source *v*_{1} and *v*_{2}
Settings

The
*Transient* analysis
settings are shown in Figure 4. The source voltages have a period of
about 6.3 ms, selecting a *Stop Time*
of 63 ms will run the simulation for 10 cycles of the waveform.
We want to simulate for long enough that sinusoidal steady-state is
reached, but blindly entering a large number for the *Stop
Time* can generate huge data
files.

Figure
4: *Transient *Analysis*
*Settings

The
currents through R1 and R2 and a reference sine wave are shown in
Figure 5. The phase angles of the current waveforms will be measured
relative to this reference. The amplitude of the reference was
chosen to be about the same as the amplitudes of the two currents.
(The reference waveform was added using the *Add Trace* feature
of the Waveform Viewer. Note that the LTspice IV sine function
requires its argument to be in degrees, not radians. The 180/pi term
that appears in the argument of the sine function converts from
radians to degrees.) The largest amplitude waveform is the 10mA
reference. The smallest amplitude waveform is the *i*_{2}
(I(R2)) waveform. The
transient portion of each current waveform
appears to decay pretty quickly here and the amplitudes and phases
appear to reach their steady-state values in less than a single cycle
of the reference waveform.

Figure 5: First 63ms of Simulation

Although
we can obtain a pretty good estimate of the amplitudes of the two
desired current waveforms from Figure 5 it would be difficult to
obtain good phase estimates because the zero-crossings are too close
together. To make phase measurement easier we can zoom in on the
waveform using the *zoom* tool.
Figure
6 shows the result of using the *zoom*
tool to expand a portion of a single cycle of the waveforms.

From
Figure 6 we see that both current waveforms lead the reference
waveform so that both will have positive phase angles. (They *lead*
the reference because the time from the positive peak of the waveform
to a trailing positive peak of the reference is smaller than the time
from the positive peak to a leading positive peak of the reference.)
You can use the LTspice IV waveform cursors to find the amplitudes of
the current waveforms and the amount of time by which the current
waveforms lead the reference. *i*_{1} (the second
largest waveform) has an amplitude of 6.735 mA and leads the
reference waveform by 0.670 ms. This corresponds to a phase
angle of 38.4º (φ
= ω Δt =
(1000 rad/s) (0.670 ms) = 0.670 rad = 38.4º). *i*_{2}
has an amplitude of 5.946 mA and leads the reference by 2.291 ms
(a phase angle of 131.3º). So the steady-state currents are:

* i*_{1}
= 6.735 cos(1000 *t* +
38.4º) mA

* i*_{2}
= 5.946 cos(1000 *t* +
131.3º) mA

Figure 6: A Complete Cycle of the Simulation

A phasor domain analysis of the circuit in Figure 1 yields:

* i*_{1}
= 6.735 cos(1000 *t* +
38.5º) mA

* i*_{2}
= 5.946 cos(1000 *t* +
131.3º) mA

The theoretical phasor results are in excellent agreement with the LTspice IV simulation results.

**Phasor
Domain Circuits****
**

You
can use LTspice IV and *Transient* analysis to obtain results
for phasor domain circuits. Set the sinusoidal voltage and current
sources to use amplitude and phases equal to that of the
corresponding phasor sources. Set all sources to use a frequency of
ω = 1 rad/s (or
rather Freq = {1/(2*pi)} Hz). For an inductor with an impedance of
jX use an inductance value of L = X in the simulation. For a
capacitor with an impedance of -jX use a capacitance of C = 1/X.
(Recall that the impedance of a capacitor is equal to -j/( ωC).
Setting this equal to -jX and solving for C at ω = 1
yields C = 1/X.) Run a *Transient*
analysis and let the waveforms reach sinusoidal steady state. (Since
the frequency is so low you may need to simulate out to 60 seconds or
longer to reach steady-state.) The amplitudes and phase angles of
the waveforms will equal the amplitudes and phase angles of the
corresponding phasor quantities.

Having
said that it is possible, let me advise against using *Transient*
analysis to solve phasor domain circuits. Use *AC*
analysis instead, it is much easier. Actually, *AC*
analysis is a much easier and accurate method for solving
steady-state sinusoidal response problems, such as the one in this
tutorial. The *Transient*
analysis method described here corresponds to how you would find
amplitude and phase using an oscilloscope in the lab. Working
problems using both *Transient*
and *AC* analysis will
also help you to understand phasors. *AC*
analysis only yields meaningful results for linear circuits.
*Transient* analysis can
be use with both linear and nonlinear circuits. *AC*
analysis is the subject of the next tutorial where we will rework the
same problem given here.

**Tips****
**

Use the Waveform Viewer's attached cursors feature to accurately measure amplitudes and time differences. The cursors were used (after zooming in on the waveform) to get the results given here. See the online documentation regarding the Waveform Viewer in order to get information about the attached cursors.

If you want to restore the original waveform graph after a zoom, just click on the

*Zoom to Fit*icon or press CTRL-E. (The*Zoom to Fit*icon is just to the right of the*Zoom Back*icon.) You can also select*Zoom to Fit*from the*View*menu.

After setting up the plot screen the way you want it, you can save your plot configuration (number of plot panes, which traces in each pane, etc) from the

*Plot Settings*menu. If you save the plot configuration with the same basename as the schematic file name, but with a .plt extension. The configuration will automatically be reloaded after running a simulation.

LTspice IV compresses raw data files as they are generated. A lossy compression algorithm is used. You may get slightly more accurate time difference measurements by turning compression off before running the simulation. You turn compression off via the control panel. (Compression is on by default and the compression setting is not remembered between program invocations. You must turn it off again after restarting LTspice IV.) I recommend leaving compression on (the default), you typically get pretty accurate results. (See the discussion regarding compression in the online documentation.)