Ensuring signal integrity while compensating for curves.

You can tell when something isn’t as clear as it should be. The same questions come up time and again. You ask three experts and get three different answers.

Routing differential pairs can be like that. Why? Because “it depends” on exactly what signals those pairs are carrying and what kind of PCB you’re creating. Hopefully, I can answer some of those repeat questions, so you can concentrate on the hard stuff.

Fan-out and end routing. Let’s start at that differential driver on the left (). Imagine the TRUE  () and COMPLEMENT () outputs are adjacent balls on a fine-pitch BGA, fanned-out to innerlayers. Whatever else you do, keep the trace lengths to fan-out vias equal, and keep the lengths after those vias equal until you start the parallel trace pattern. That parallel trace pattern is the coupled section because there’s electromagnetic coupling between the two sides.

Figure 1. Considerations for routing differential pairs.

Balance fan-out and end-routing patterns separately at both ends. When you reach that receiver on the right, do the same as you did at the driver end. Don’t consider the lengths within the coupled section at all when doing this. Once TRUE and COMPLEMENT are coupled, the signals travel in a different way. I think of coupled sections as apples and fan-out and end-routing as oranges – and you can’t add apples to oranges unless you want a fruit salad!

Corner angles and curves. If you only want good signal integrity, make no corner tighter than 135°. Many device application notes tell you the same. That angle works well for 45° routing. You’ll hear that curves give better signal integrity, but for most PCB traces – even for very fast signaling – that isn’t true. Get curves wrong and you’ll make it a whole lot worse, and what “wrong” means isn’t always obvious.

When routing on a flex, you need curves, but that’s for mechanical reasons. You have to follow mechanical constraints, so the skill there is in making sure you don’t break signal integrity in the process.

Matching to other differential pairs. Add length in coupled sections only, and keep the pair coupled all the way, because the differential impedance and delay-per-unit-length are different from the single-ended values, even within the same pair.

Matching between differential pairs and single-ended signals. In this case, you almost invariably need to add length to the pair, not the single-ended signal. As with matching between pairs, add length in coupled sections only. The application notes or standards documents will tell you how much.

Matching within a differential pair. Now you’ll remember we matched the fan-out and end-routing separately, so that’s not what I’m talking about here. This is about differences that arise within the coupled routing sections. This is sometimes called phase matching. The ideal is that TRUE and COMPLEMENT travel together in perfect complementary harmony, as shown on the left in FIGURE 2. There’s no such thing as perfection, so we get as close as we can. The faster the rising and falling edges get, the fussier phase matching requirements become. When slower edges get out of phase, the phase difference doesn’t affect the signal so much, as can be seen in Figure 2 in the center and the right. The phase difference matters most when TRUE or COMPLEMENT change state from low to high or high to low.

Figure 2. Differential pair phase matching.

Differential impedance and delay-per-unit-length depend on phase matching. Without it, those numbers are different. Good signal integrity requires pretty good matching. You shouldn’t be breaking out from the coupled pattern, so the usual culprits where phase mismatches are concerned are corners. The outside trace goes a bit further than the inside track.

The trap is to think you can just add the differences in length to the shorter sides, somewhere near the corners. Those are sometimes called phase bumps. There’s more to it than that because the bump couples differently, and the coupling around those corners gets quite fuzzy. You have to follow tight recommendations for exactly what those bumps should look like. If phase bumps aren’t really needed, do not add them.

The best place to start is to balance the number of 135° right and left turns and to try to minimize the number of turns. After that, compensate for any remaining difference with a phase bump, if needed.

Figure 3. PCI Express signals from a high-speed FPGA I/O bank to a connector.

John Berrie is PCB design specialist at Zuken (zuken.com); This email address is being protected from spambots. You need JavaScript enabled to view it..