Gaps in return planes - yes or no?

-April 19, 2014

As a participant during the panel discussion on EMC versus SI at the recent DesignCon 2014, I sensed (along with some in the audience) that there was disagreement as to whether it was OK to cross a gap in the return plane with a high speed, fast-edged, signal. Unfortunately, there was too little time in which to come to an agreement or to illustrate the conditions in which it was OK, or not OK.

I maintain that in the usual case, crossing a gap in the return plane is bad from both an EMI, as well as a SI point of view. In 2008, Doug Smith described why the scenario was bad from a SI viewpoint. Eric Bogatin also presented a paper in 2009 for the Altera Signal Integrity Workshop, “Impact of Return Path Discontinuities in High Speed Serial Links”, that describes several issues with gaps and other discontinuities in the return path of high speed signals. There are numerous other papers on this issue. In this posting, I’d like to illustrate why it’s bad from an EMI viewpoint.

Besides the obvious reflections noted by both Smith and Bogatin, there is also a differential to common “mode conversion” that occurs (also noted by Bogatin), which causes the first of two bad things:  (1) common-mode currents to be generated, which causes board resonance with resulting radiated emissions and (2) the gap forces the magnetic field normally around the trace to “wrap around” the entire PC board, rather than staying relatively confined around the signal trace. This expanded magnetic flux couples to other nearby traces, causing cross-coupled noise (or crosstalk).

A simple experiment was set up based on the experimental PC board Smith devised. The board consists of two wires taped down to a copper clad board. These represent (near 50 ohm) circuit traces, one end of which is terminated to a 49.9 ohm resistive load and the other end connected to the center pin of a BNC connector attached to the board. One trace has a 4cm gap in the return plane - the other trace has a solid return path.

The experiment consists of three parts: tracing and observing the path of the electromagnetic wave in the return path (both gapped and untapped traces), observing crosstalk in the non-driven trace when the gapped trace is driven and observing harmonic currents in a clip lead attached to the board plane when the gapped trace is driven (simulating a radiating I/O cable).

The board is driven with a USB-powered harmonic comb generator from Applied Electromagnetic Technology (AET), which is essentially a fast-edged pulse generator. The pulse generator is connected to each BNC connector in turn and an H-field probe is used to trace the path of HF current.


Figure 1 - A graphic drawing of the test board.


Figure 2 - Tracing the return path of the gapped trace. The electromagnetic wave current can be measured all around the gap (lower trace in the screen).


Figure 3 - Screen capture of cross-coupled harmonics (lower trace) on the un-powered (ungapped) trace as measured by an H-field probe as the gapped trace is being driven.


Figure 4 - Driving the gapped trace and measuring the harmonic currents with a current probe in a simulated I/O cable attached to the return plane. As you can see in the bottom trace, the harmonics are maximized at the resonant frequencies of the board/cable combination.

In summary, routing high speed fast-edged traces over gaps in return planes causes both radiated emissions and cross-coupled noise. If gaps must be used (and I can’t really think of any good reasons), the return path can be controlled by adding stitching capacitors across the gap and near the high speed trace (really best added on both sides of the trace). This experiment is easily reproduced. I’d be interested in cases or exceptions where it might be considered OK to cross a gap in the return plane from a SI or EMI viewpoint.

For more:

PCB gaps lead to unwanted emissions

Using current probes to estimate E-fields

Measuring resonance in cables

PC board resonance and the "balloon effect"

Questions on PC boards for EMC mitigation

Loading comments...

Write a Comment

To comment please Log In

FEATURED RESOURCES