Differential Pairs – coupling tight or not

This is another controversial topic where I have seen experts not being unanimous for or against it.

To quote Lee W. Ritchey in his book –“ Right The First Time”, Volume 1, Page 118

“When one signal is routed very close to other, several undesirable things happen. The first is the impedance of each line is lowered by the presence of other. As a result of this, the terminating resistor placed at its end will need to be lower value and the resulting voltage across it will be smaller. If this is not possible, each trace will need to be made narrower in order to restore the original impedance. As each trace gets narrower, the skin effect loss increases. Another undesirable side effect of routing pairs tightly together is that it induces crosstalk from one line to other. This crosstalk is not beneficial. It actually degrades the switching edges resulting in a poorer signal at the receiver.

Lee concludes –

“Differential pairs do not need to be routed side by side for proper operation. In fact, if they are routed too close to each other, destructive coupling occurs that causes the edges to be slowed down.

If differential pairs are routed side by side, it is imperative that they be kept far enough apart that they don’t destructively interact.”

Now the quote from the book “Signal Integrity Issues and Printed Circuit Board Design”, by Douglas Brooks , page 257 –

“ …if we want to keep EMI under control, we need to minimize this loop area. And the way we do that brings us to Design Rule 2 : Route Differential traces close together. There are people who argue against this rule, and indeed the rule is not necessary if rise time are slow and EMI is not an issue. However, in high speed environments, the closer we route the differential traces to each other, the smaller will be their own loop area and the loop area of the induced currents under traces, and the better control over EMI we will have.”

So where does it leaves us. As a PCB designer what conclusion are we expected to derive? The first is that don’t be afraid of to do your own analysis. When the experts are not unanimous on the topics how can ordinary PCB designer be derive his own rules with authority. But – keep yourself aware of the issues, methodologies of analysis and the reasons behind the rules given out by the Signal Integrity engineers. And do not be afraid of the attempting to do analysis and arrive at your own conclusions. If you always fear of drowning, you will never learn swimming.

That being said, I have seen recommendations of keeping the traces far away, as in the book by Dr. Howard Johnson ( High Speed Signal Propagation, Advanced Black Magic, page 390), where he writes – “ Unless absolutely pressed for space, I normally set the trace separation at about four times the height h. This setting usually yields a less than 6% reduction in impedance, a small enough value to simply ignore. All stripline traces, differential or not then have the same width. I instruct my layout professional to keep differential pairs near each other, but allow them to separate them from time to time as needed to go around the obstacles.”

The Howard Johnson’s approach simplifies the PCB design process in the sense that we do not need to keep two sets of trace widths for traces – one for single ended and other for differential traces. However this works only in PCB designs that have only couple of differential traces for example, only ethernet differential traces. Consider a differential bus like HyperTransport™, where 8 parallel differential bus need to be routed, mostly in dense environment. In such cases it is not possible to keep the traces as far away as we would wish. The only way in such scenario would be to reduce the trace thickness and keep the traces close.


Previous                    Next