Nuts and Volts - February 2009

A Touch of Spice

PART 3

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.

Oscillator Circuits

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 Wikipedia at:

http://tinyurl.com/

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 Wave Oscillator

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 on frequency.

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