To control emissions, high-speed signals should not be routed near the edge of the ground-reference plane.

It is often difficult to route all the required traces on a PCB. There is a constant goal to keep costs at a minimum and so the number of layers available for routing is very limited. This can force designers to route traces too close to the edge of the PCB. Routing too close to the edge of the PCB can increase emissions from the edge of the ground-reference plane. Controlling these emissions is simply a matter of not routing high-speed signals near the edge of the ground-reference plane.

Amplitude of Current Along the Edge of the PCB Ground-Reference Plane

In the case of both microstrip and stripline, the majority of return current will flow in the plane nearest to the trace. However, some of the return current will spread away from the trace to find the path of least impedance. As the trace is routed further from the edge of the plane, less current is along that edge. However, it can still be significant for EMI/EMC purposes even when too low for signal integrity concerns.

Equation 1 gives the formula to find the current along the edge of a ground-reference plane for a microstrip transmission line1. The currents on each reference plane for a symmetrical strip line are simply one-half of those in Equation 1.

where:

I_signal = the current amplitude (in linear scale) for each harmonic of the current waveform.
wg = the width of the ground-reference plane (set to 1000 mils always)
d = the distance from the trace to the edge of the ground-reference plane in mils
h = the height between the trace and the ground-reference plane in mils

Equation 1 is plotted in Figure 1 for a microstrip with a variety of different trace heights and distances to the edge of the ground-reference plane. The amplitude of the current along the edge of the ground-reference plane decreases as the distance between the trace and the edge increases. Also, when the trace height is further from the reference plane, the current along the edge is higher.

Impact with Real-World Signals

Let’s consider a typical frequency spectrum for a clock signal’s current. In this case, we’ll assume the current waveform follows the voltage waveform, as in the case of a resistive termination for this clock net. Of course, if a non-resistive termination is used, the frequency spectrum will be different. Figure 2 shows the frequency spectrum for a 200 Mb/s square wave with a 1 ns rise and fall time.

For this case, the 5th harmonic occurs at 900 MHz, and its amplitude is approximately 40 dBuA (100 microamps). If the trace is 50 mils from the board edge, and the trace height is 10 mils from the plane, then the edge current will be expected to be approximately 60% of the trace current, or 60 microamps. However, if the trace is moved to 0.5˝ from the edge, the edge current falls to 6% of the trace current, or 6 microamps.

How Much is Too Much?

It is very difficult to calculate the expected far field radiated emissions without knowing specific information about PCB, including its size, shielding metal enclosures, etc. However we can consider that the edge of the reference plane will be an efficient radiator when it is one-half a wavelength long. Equation 2 shows the formula to find the wavelength. For example, at the 900 MHz the wavelength is only 33 cm and a half wavelength is 16.5 cm (approximately 5 inches). Clearly, many PCBs will be large enough to be efficient radiators at these frequencies.

where:

λ = wavelength
c = speed of light (300e8 m/s)
f = frequency
εr = relative dielectric constant

A general rule-of-thumb is that a few microamps of noise current on an unshielded and efficient wire antenna can cause emissions that will be over the commercial EMC emissions limits. So depending on the amount of shielding, emissions from edge currents may be important.

Summary

The distance between the trace and the edge of the ground-reference plane is important for EMI/EMC. Most of the return current will be below the trace, but some of this return current will spread out over the reference plane. If the trace is too close to the edge, then emissions will be higher than if the trace is further away from the edge. These emissions can easily be higher than allowed by commercial emissions standards.

This does not mean that the routing channels near the edge of the board may not be used and must be left blank. Most boards need every routing channel possible. Use these routing channels near the edge of the reference plane for low speed signals and keep the high-speed clock, data, address, etc. signals away from the edge of the reference plane. PCD&F

REFERENCES

1. M.Y. Koledintseva, J. Drewniak, T. Van Doren, D. Pommerenke, M. Cocchini, D. Hockanson, “Method of Edge Currents for calculating mutual external inductance in a microstrip structure,” Accepted for publication Progress in Electromagnetic Research (PIER), Feb 2008.

Dr. Bruce Archambeault is an IBM Distinguished Engineer and IEEE Fellow; This email address is being protected from spambots. You need JavaScript enabled to view it..