A Touch of Spice
by Peter J. Stonard
Most SPICE work stimulates a proposed circuit with a pulse or
sine wave signal. In this final part, we’ll look at oscillator circuits
that create their own signal during simulation in LTspice, plus a
"hollow state" oscillator, just for fun!
Following the earlier articles, you probably have LTspice
on your computer's desktop, ready to use. So, we'll jump
right in with a simple sine wave oscillator.
Rcircuit with amplification
and frequency selectivity
ecall that an oscillator is a
components. The old joke goes that
"my amplifier oscillates, but my
oscillator doesn't." An oscillator needs
an amplifier with a feedback path
from output back to the input that
replaces energy lost in both the
feedback network and the load.
The feedback network selects the
resulting output frequency. Another
name for this arrangement is
Harmonic Oscillator, as noted in
lwpe7. For a low distortion sine
wave, two distinct feedback paths are
required, as illustrated in Figure 1.
The positive feedback path builds the
output and defines the frequency,
while the negative feedback path controls the gain to cancel all the losses.
Many of these basic oscillators
are named for their inventors, and
may use inductor-capacitor (LC) or
resistor-capacitor (RC) networks for
frequency control. Perhaps you've
already found the examples bundled
with the LTspice download; these
include several oscillator designs.
Use your computer's file directory
tree to find them. Figure 2 is a list of
oscillators circuits; there are more
files in the download bundle.
■ FIGURE 1. Oscillator basics.
Phase Shift Sine
A popular and easily constructed
sine wave oscillator uses the phase
shift in a chain of capacitor-resistor
(CR) stages to define the frequency.
The circuit starts automatically due
to inherent noise in the amplifier,
and after a few cycles it stabilizes
Each CR stage contributes 60
degrees of the 180 degree phase
shift needed, and attenuates the
signal by one half. So, the theoretical
amplifier voltage gain is: 1/ (1/2*1/2*
1/2) = 8 (or 18dB). The frequency is
defined as 1.73/CR (assuming all
of the C and all of the R timing
elements are the same value). By
isolating the three
phase shift stages
from each other
with buffer amplifiers, we can see
what is happening at each one. The
LTspice schematic is shown in Figure
3 and the simulation waveforms
are in Figure 4. Notice the SPICE
directive .tran 3ms startup This tells
LTspice to start the power supply (our
9V battery equivalent) at zero volts
and collect data for 3 ms, showing us
how this circuit starts up. Also notice
in Figure 4 the output shoots up and
hits the supply rail, followed by a few
cycles of correction as the oscillator
comes into balance.
I built this circuit on a solderless
breadboard (shown in Figure 5) using
two dual op-amps (LM1458) and some
10K and 100K 1/4W resistors. The
results are shown in Figures 6 and 7.
Luckily, my scope can display all three
■ FIGURE 2. LTspice supplied oscillators.
■ FIGURE 3. Phase shift oscillator.