Why High-Speed Traces Stay Away From the Board Edge
Two rules in high-speed design appear to contradict each other. One says that a high-speed trace should never run along the edge of the board. The other says that an antenna on the board should be placed as close to the edge as possible. Both are correct, and the reason is the same in each case: the amount of energy that escapes as radiation depends on how well the conductor is coupled to a reference plane.
Why Radiation Increases With Frequency
Current in a conductor creates a magnetic field around it, and the charges in the conductor create an electric field. A changing electric field produces a changing magnetic field, and a changing magnetic field produces a changing electric field, so the two sustain each other and travel outward from the source. That is electromagnetic radiation.
The behaviour depends on frequency. At low frequencies the fields change slowly, and the energy returns to the circuit rather than leaving it. As the frequency rises, the fields change faster than the energy can return, and a growing fraction travels away as a wave. Every conductor carrying high-frequency current therefore radiates, and the radiated power rises with frequency. The difference between a signal trace and an antenna is not whether radiation occurs, but whether it is wanted: a data link or a clock is designed to keep the energy in the line, while an antenna is designed to launch it into space. The two requirements need opposite layouts.
The Trace-to-Plane Ratio
For a signal trace the goal is to keep the field coupled to the reference plane, and the geometry does most of that work. In a microstrip, the field between the trace and the plane underneath couples strongly when the two are close. A practical rule is to keep the ratio of trace width to dielectric height below about 1 to 3, which substantially reduces the radiated field from the transmission line. Bringing the reference plane closer achieves what no amount of shielding would.
The width of the plane matters as much as its distance. A reference plane should extend at least three trace widths beyond the trace on each side, and wider is better, because the coupling between the trace and the plane depends on how much plane there is to couple to. Where the plane is narrow relative to the trace, the field has nowhere to terminate and radiates outward instead.
Why the Board Edge Is a Problem
Put the two requirements together and the edge rule explains itself. A trace running parallel to the board edge has the reference plane extending beyond it on one side only, so the coupling available to it is a fraction of what it would be in the middle of the plane. The proportion of the field that escapes rises, and the trace radiates more than the same trace placed inboard. The situation is worse in a plane that has been pulled back from the outline, as it usually is to satisfy edge clearance requirements.
The rule extends to other high-speed structures. A fast integrated circuit or a crystal oscillator placed near the edge suffers the same problem: the wide, unbroken reference plane it needs for field containment is truncated by the board boundary. Keeping these parts inboard, with a generous plane around them, is a layout decision that costs nothing and removes a whole class of emissions problem. The related question of what else should be kept away from the edge is discussed in ESD and PCB edge traces.
The Antenna Case Is the Opposite
A PCB antenna wants the opposite of everything above. Its purpose is to launch energy into space, so the field must not be terminated by a plane, and the layout is arranged to keep the radiating element deliberately unshielded. That is why the antenna sits at the board edge rather than in the middle, and why the area around it is kept free of copper on every layer.
The copper keep-out is the part that most often goes wrong, because a plane that ends a few millimetres from the antenna is still close enough to detune it and to absorb part of the radiated power. The exclusion has to be applied to all layers, not only to the layer the antenna is drawn on, and the ground plane for the rest of the circuit has to be pulled back far enough that the antenna is genuinely separated from it. A matching network is usually needed between the antenna and the radio, and its placement and the length of the feed line both affect the result.
Applying the Rule in Practice
Two layout habits follow. Keep high-speed trace parallel to the board edge out of the design, or if the geometry makes that unavoidable, route the trace further inboard and let the plane extend well beyond it. Keep fast devices, oscillators, and their supply networks away from the outline for the same reason, and give them a wide, unbroken plane to couple to.
The microstrip geometry that governs how tightly the field couples to the plane is described in microstrip and stripline routing, and the broader set of techniques for reducing emissions is collected in EMI suppression design principles. The underlying point is that the same physical effect produces both the problem and the solution, and that the design intent, not the effect itself, decides which layout is correct.
Where the Edge Rule Does Not Apply
The rule is about signal and component placement, not about connectors. A high-speed link that has to leave the board through an edge connector obviously has to reach that connector, and the connector is designed for the impedance and the return path it presents. What the rule discourages is running a long trace parallel to the edge and close to it, a few millimetres from the outline, for most of the board length. A short approach to a connector at a defined point is a different case from a lengthy run alongside the boundary.
The same distinction applies to a board whose edge sits inside a shielded enclosure. Screening reduces what escapes, but it does not restore the coupling that the truncated plane failed to provide, so the impedance and the local field distribution still differ from the inboard case. Treating the edge as ordinary routing space and relying on the enclosure to absorb the difference is the assumption that produces emissions problems in the first place.
FAQ
Why does a trace at the board edge radiate more? Because the reference plane extends beyond it on one side only, so the field has less plane to couple to and a larger fraction escapes.
What ratio of trace width to dielectric height should I target? Below about 1 to 3. Closer coupling between the trace and the plane substantially reduces the radiated field from the line.
How wide should the reference plane be? At least three trace widths beyond the trace on each side, and wider wherever the layout allows.
Why must the antenna keep-out apply to every layer? Because a plane on any layer near the antenna absorbs radiated power and shifts the tuning. The exclusion is three dimensional, not confined to the antenna layer.
