
3.3.1 Differential Pairs
The USB data lines, D- and D+, should be routed as a differential pair. The trace impedance should be matched to the USB cable
differential impedance, which is nominally 90 ohms for the signal pair.
The impedance of a signal track is mainly determined by its geometry (i.e. trace width and height above the reference plane) and the
dielectric constant of the material between the traces and a reference plane. When two tracks are closely spaced, they will be coupled
and the differential impedance will also be dependent on the distance between the two tracks comprising the pair.
In general one can say that if the two traces of a differential pair is spaced far apart, the differential impedance will be twice the impe-
dance of each trace. I.e. the two traces can be considered a shunt impedance. When the distance between the two traces is reduced,
coupling between the traces will cause the differential impedance to decrease. Thus to create a differential pair with 90 ohms impe-
dance, the single ended impedance of each trace should be above 45 ohms. Reducing the trace width will increase the single-ended
impedance while reducing the distance between the traces in a pair reduces the impedance. This allows routing of very closely spaced
differential pairs that use little PCB area. Note, however that thin traces will be more difficult to manufacture, and that for high frequen-
cies loss due to skin effect comes into play.
Most PCB design tools support differential pairs, and can create such pairs with specified parameters. If such a tool is not available,
there are many online impedance calculators that can calculate track parameters.
To avoid differential imbalance, skew (or trace length difference) between the two traces in a differential pair should be under control. A
common rule of thumb is to keep the skew less than 1/10th of the fastest rise time. For USB full-speed this translates to 400 ps or 60
mm. However, this is the total skew over the entire communication link so skew in the USB cable as well as in the other communicating
party must also be included. According to the USB specification the maximum allowed skew in a cable is 100 ps, which leaves a maxi-
mum of 300 ps (45 mm) of skew to be distributed amongst the host and device. Still, as you never know the characteristics of the other
end, good design practice is to keep skew at a reasonable minimum.
When high speed signals are routed from one layer to another, care should also be taken to provide a path for the return signals. Re-
member that even differential signals use a reference plane as return path. This is particularly important when designing PCBs with
many layers.
TOP
GND
BOTTOM
GND
Signal
path
Return
current
path
Figure 3.1. Changing layers on PCB
Stubs should also be avoided as they may cause signal reflections. For USB, this is seldom a problem as the data traces are point-to-
point. If a test point is desired, the signal should be routed through the test point, in a fly-by manner, rather than having a long trace
from the trace to the test point.
Figure 3.2. Recommended routing of test points
AN0046: USB Hardware Design Guidelines
PCB Design Guidelines
silabs.com | Building a more connected world. Rev. 1.02 | 10