## Differential Routing

Clint Lieser writes:

I've recently started my first high-speed digital design and have found your book to be extremely valuable.

I have a question regarding the routing of differential pairs such as ECL or LVDS. It has been suggested that routing differential pairs as overlapping signal traces on adjacent layers is superior to routing them as adjacent traces on the same layer.

For example, the layer stack might look like this:

```        ----------------------        Ground
---                  Diff Pair +
---                  Diff Pair -
----------------------        Ground ```

I have been unable to find any literature that characterizes this geometry and was wondering if you could recommend a reference or had any comments on the subject.

Thank you,
Clint Lieser

Thanks for your interest in High-Speed Digital Design.

I don't have any references to give you but I do have a couple of comments.

First, either structure can work.

Second, with either structure it's not particularly important that the lines be coupled tightly together. In fact, you couldn't achieve very tight coupling even if you tried. The coupling ratios (effectively the common-mode rejection of the structure) for typical differential lines on PCB's are only in the 20-50 percent range.

In contrast, for a well-balanced differential twisted pair, the coupling is 99.9 percent. That is, if I transmit a signal down one wire of a twisted pair, with the other wire grounded, at the far end I will receive two signals, each of half size, and having opposite polarities. This is the property called "good common-mode rejection".

To get good common-mode rejection what you need is a coupling coefficient of 99.9 percent. Differential traces on a PCB won't do that. Fortunately, we don't need the tight-coupling property for PCB applications.

Here's a list of the reasons we normally use differential pairs on a PCB:

1. To match to an external, balanced differential transmission medium (some kind of cabling). For this purpose, the inter-trace coupling is irrelevant. Two independent, 50-ohm traces can couple a perfectly fine signal into a 100-ohm differential transmission line. What we want in this application is to make sure that the signal is generated in a purely differential manner (no common-mode components that would radiate off the cable). Furthermore, we want to make sure that the two PCB traces have equal impedances to ground (that is, they need to be symmetrical, but not necessarily close together).
2. To defeat ground bounce. A differential signal naturally comes with its own built-in reference voltage. The receiver of a differential signal therefore does not need to rely on its own built-in reference, which could be corrupted by ground bounce voltages internal to the receiving device. For this purpose, we need only supply the receiver with two antipodal signals, with equal delays from the driver. There is no requirement here for particularly close coupling.