- Describing Signal-Integrity Solutions in Terms of Impedance
- What Is Impedance?
- Real vs. Ideal Circuit Elements
- Impedance of an Ideal Resistor in the Time Domain
- Impedance of an Ideal Capacitor in the Time Domain
- Impedance of an Ideal Inductor in the Time Domain
- Impedance in the Frequency Domain
- Equivalent Electrical Circuit Models
- Circuit Theory and SPICE
- Introduction to Modeling
- The Bottom Line
3.9 Circuit Theory and SPICE
There is a well-defined and relatively straightforward formalism to describe the impedance of combinations of ideal circuit elements. This is usually referred to as circuit theory. The important rule in circuit theory is that when two or more elements are in series, that is, connected end-to-end, the impedance of the combination, from one end terminal to the other end terminal, is the sum of the impedances of each element. What makes it a little complicated is that when in the frequency domain, the impedances that are summed are complex and must obey complex algebra.
In the previous section, we saw that it is possible to calculate the impedance of each individual circuit element by hand. When there are combinations of circuit elements it gets more complicated. For example, the impedance of an RLC model approximating a real capacitor is given by:
We could use this analytic expression for the impedance of the RLC circuit to plot the impedance versus frequency for any chosen values of R, L, and C. It can conveniently be used in a spreadsheet and each element changed. When there are five or ten elements in the circuit model, the resulting impedance can be calculated by hand, but it can be very complicated and tedious.
However, there is a commonly available tool that is much more versatile in calculating and plotting the impedance of any arbitrary circuit. It is so common and so easy to use, every engineer who cares about impedance or circuits in general, should have access to it on their desktop. It is SPICE.
SPICE stands for Simulation Program with Integrated Circuit Emphasis. It was developed in the early 1970s at UC Berkeley as a tool to predict the behavior of transistors based on the as-fabricated dimensions. It is basically a circuit simulator. Any circuit we can draw with R, L, C, and T elements can be simulated for a variety of voltage or current-exciting waveforms. It has evolved and diversified over the past 30 years, with over 30 vendors each adding their own special features and capabilities. There are a few either free versions or student versions for less than $100 that can be downloaded from the Web. Some of the free versions have limited capability but are excellent tools to learn about circuits.
In SPICE, only ideal circuit elements are used and every circuit element has a well-defined, precise behavior. There are two basic types of elements: active and passive. The active elements are the signal sources, current or voltage waveforms, or actual transistor or gate models. The passive elements are all the ideal circuit elements described above. One of the distinctions between the various forms of SPICE is the variety of ideal circuit elements they provide. Every version of SPICE includes at least the R, L, C, and T (transmission-line) elements.
SPICE simulators allow the prediction of the voltage or current at every point in a circuit, simulated either in the time-domain or the frequency domain. A time-domain simulation is called a transient simulation and a frequency-domain simulation is called an AC simulation. SPICE is an incredibly powerful tool.
For example, a driver connected to two receivers located very close together can be modeled with a simple voltage source and an RLC circuit. The R is the impedance of the driver, typically about 10 Ohms. The C is the capacitance of the interconnect traces and the input capacitance of the two receivers, typically about 5 pF total. The L is the total loop inductance of the package leads and the interconnect traces, typically about 7 nH. The set-up of this circuit in SPICE and the resulting time-domain waveform, showing the ringing that might be found in the actual circuit, is shown in Figure 3-9.
Figure 3-9. Simple equivalent circuit model to represent a driver and receiver fanout of two, including the packaging and interconnects, as set up in Agilent's Advanced Design System (ADS), a version of SPICE, and the resulting simulation of the internal-voltage waveform and the voltage at the input of the receivers. The rise time simulated is 0.5 nsec. The lead and interconnect inductance plus the input-gate capacitance dominate the source of the ringing.
If the circuit schematic can be drawn, SPICE can simulate the voltage and current waveforms. This is the real power of SPICE for general electrical engineering analysis.
SPICE can be used to calculate and plot the impedance of any circuit in the frequency domain. Normally, it plots only the voltage or current waveforms at every connection point, but a trick can be used to convert this into impedance.
One of the circuit elements SPICE has in its toolbox for AC simulation is a constant-current sine-wave-current source. This current source will output a sine wave of current, with a constant amplitude, at a predetermined frequency. When running an AC analysis, the SPICE engine will step the frequency of the sine-wave-current source from the start frequency value to the stop frequency value with a number of intermediate frequency points.
It generates the constant-current amplitude by outputting a sin wave voltage-amplitude sine wave. The amplitude of the voltage wave is automatically adjusted to result in the specified constant amplitude of current.
To build an impedance analyzer in SPICE, we set the current source to have a constant amplitude of 1 Amp. No matter what circuit elements are connected to the current source, SPICE will adjust the voltage amplitude to result in 1-Amp current amplitude through the circuit. If the constant-current source is connected to a circuit that has some impedance associated with it, Z(ω), then to keep the amplitude of the current constant, the voltage it applies will have to adjust. The voltage applied to the circuit, from the constant-current source, with a 1-Amp current amplitude, is V(ω) = Z(ω) × 1 Amp. The voltage across the current source, in volts, is numerically equal to the impedance of the circuit attached, in Ohms.
For example, if we attach a 1-Ohm resistor across the terminals, in order to maintain the constant current of 1 Amp, the voltage amplitude generated must be V = 1 Ohm × 1A = 1 v. If we attach a capacitor with capacitance C, the voltage amplitude at any frequency will be V = 1/ωC. Effectively, this circuit will emulate an impedance analyzer. Plotting the voltage versus the frequency is a measure of the magnitude of the impedance versus frequency for any circuit. The phase of the voltage is also a measure of the phase of the impedance.
To use SPICE to plot an impedance profile, we construct an AC constant-current source with amplitude of 1 A and connect the circuit under test across the terminals. The voltage measured across the current source is a direct measure of the impedance of the circuit. An example of a simple circuit is shown in Figure 3-10. As a trivial example, we connect a few different circuit elements to the impedance analyzer and plot their impedance profiles.
Figure 3-10. Left: An impedance analyzer in SPICE. The voltage across the constant-current source is a direct measure of the impedance of the circuit connected to it. Right: An example of the magnitude of the impedance of various circuit elements, calculated with the impedance analyzer in SPICE.
We can use this impedance analyzer to plot the impedance of any circuit model. Impedance is complex. It has not only magnitude information but also phase information. We can plot each of these separately in SPICE. The phase is also available in an AC simulation in SPICE. In Figure 3-11, we illustrate using the impedance analyzer to simulate the impedance of an RLC circuit model, approximating a real capacitor, plotting the magnitude and phase of the impedance across a wide frequency range.
Figure 3-11. Simulated magnitude and phase of an ideal RLC circuit. The phase shows the capacitive behavior at low frequency and the inductive behavior at high frequency.
It is exactly as expected. At low frequency, the phase of the impedance is –90 degrees, suggesting capacitive behavior. At high frequency the phase of the impedance is +90 degrees, suggesting inductive behavior.