High-frequency effects were not always a major concern for digital-system board designers. Slow clock speeds made crosstalk and transmission-line reflections minor problems, especially when compared with fitting hundreds of components on the board and making the board manufacturable. However, at the high speeds of recent systems (and the even higher speeds yet to come), digital signals can cause RF problems. However, at high speeds, digital problems become RF problems. You can determine the wiring interactions and RF effects in high-speed digital systems by treating the interconnection traces as transmission lines, which obey the laws of electromagnetic-field theory.

Magnetic fields that change with time induce electric fields, and electric fields that change with time induce magnetic fields. This relationship arises along conducting and dielectric boundaries and causes waves that the boundaries define and guide. These waves guide electromagnetic energy from a source to a target device or system. You can identify the inductance per unit length by the flux that the directed currents produce. When these currents vary with time, a voltage change occurs along the line. Similarly, when the voltages vary with time, the capacitance per unit length produces displacement currents between the conductors. The capacitance induces a current change along the conductors.

One of the simplest systems to understand is the two-conductor transmission line. The most common of these systems are microstrip and stripline transmission lines. The stripline transmission line in Figure 1 comprises a conduction strip lying between, and parallel to, two wide-conduction planes. The characteristic impedance of this line is given by

where w=trace width, d=conduction-plane separation, t=trace thickness, and Er=dielectric constant.

The microstrip transmission line in Figure 2 comprises the conduction strip lying above, and parallel to, one wide-conduction plane. The characteristic impedance is given by

where w=trace width, t=trace thickness, h=dielectric thickness, and Er=dielectric constant.

You must tightly control the layer stacking of the board to obtain the desired characteristic impedance. To obtain this impedance, you need to reference each signal layer to a ground layer and optimize the line width and gap spacing. At high frequencies, even the most minute problems within a circuit can cause poor performance. Therefore, you need to pay special attention to all critical aspects of the pc-board design.

Most transmission-line problems occur at junctions between a given line and an element of different characteristic impedance, such as a load resistance or some other element that introduces a discontinuity. The reflection coefficient is the ratio of the voltage of the reflected wave to that of the incident wave. The impedances that determine this ratio are P=(R_L=Z₀)/(R_L+Z₀). If the load resistance is lower than the characteristic impedance of the line, the reflection coefficient is negative, as is the reflection.

Similarly, if the load resistance is greater than the line’s impedance, the reflection is positive. You can minimize the reflection coefficient by matching the impedances at the discontinuity. In doing so, you have access to several termination techniques. Series termination entails adding the correct-value resistor in series with the transmission line to create a match (Figure 3a). Although this technique is valid, it introduces a voltage divider into the network. Parallel termination entails adding the correct-value resistor in parallel with the line (Figure 3b). This method matches the line, but upsets the dc-bias conditions.

A better mathching method is Thevenin termination (Figure 3c). This method involves adding two resistors in an ac-parallel connection. You select the resistors to maintain the proper bias on the transmission line. The main drawback in these three techniques is the increase in power dissipation that accrues from increased loading of the line.

The last matching technique is reactance termination (Figure 3d). To use this technique, you add a resistor and series capacitor in parallel with the line.

Crosstalk is the undesirable coupling of signals on one conductor to a nearby conductor. The possibility for such signal coupling increases as the length along which the traces run parallel increases. You can attenuate crosstalk by separating the adjacent traces as much as possible. Ground striping, or shielding, is another effective way to reduce crosstalk, and it makes better use of the available board area. Ground striping is a ground trace run between the two parallel traces. When it’s feasible, the best way to minimize crosstalk is to route traces on separate layers of the board, with embedded ground or power-supply traces between the layers.

You can use Fourier analysis to express an arbitrary waveshape (such as a digital signal) as a sum of sinusoidal waves. If the phase velocity is the same for each frequency component and no attenuation exists, then the component waves add in proper phase at each point along the line to reproduce the exact original waveshape, delayed by the propagation time. The phase velocity, or the velocity of propagation, is the rate at which the wave moves down the line. In an ideal, loss-free transmission line, the phase velocity is 1/(sqr root)LC.

If the phase velocity changes with frequency, dispersion occurs, and the signal may change shape as it travels. This distortion limits the frequency at which you can transmit data signals. You must take considerable care in selecting and processing pc boards to ensure that the dielectric constant is as uniform as possible. If you encounter problems arising from nonuniformity, then you should consider changing materials (possibly to Teflon or ceramic).

Another area of concern with transmission lines is the electrical line length. Because of the propagation delay of digital transmission, you must take extreme care to ensure that the electrical lengths (not necessarily the physical lengths) of all lines are equal. For example, the propagation delay for microstrip is 147 psec per linear in. The delay for stripline is 188 psec per linear in.

Minimize ringing

Imbalances in impedances generally cause undesirable effects in a circuit. When the reflection coefficients of the source and the load are of opposite polarity, the reflections alternate in polarity. The signal oscillates, or "rings," about its final, steady-state value. You can reduce the ringing by making the electrical line length short compared with the rise and fall times of the waveform. You can also cut ringing by providing better matching of the source and load impedances to that of the transmission line.

Switching large currents magnifies ringing effects. In practical terms, the magnitude of the voltage swing is the product of the current-switching rates and the inductive loading. For high-current switching, you must take great care to minimize the inductive loading. Note: If the load is highly capacitive and the signal has fast rise and fall times, signal degradation occurs because of the time required to charge and discharge the capacitance.