Kontron COMe Starterkit Eval T2 - Manual (Page 175)

Carrier Board PCB Layout Guidelines
6.3. Trace-Impedance Considerations
Most high-speed interfaces used in an COM Express design for a Carrier Board are differential
pairs that need a well-defined and consistent differential and single-ended impedance. The
differential pairs should be edge-coupled (i.e. the two lines in the pair are on the same PCB
layer, at a consistent spacing to each other). Broadside coupling (in which the two lines in the
pair track each other on different layers) is not recommended for mainstream commercial PCB
fabrication.
There are two basic structures used for high-speed differential and single-ended signals. The
first is known as a “microstrip”, in which a trace or trace pair is referenced to a single ground or
power plane.
The outer layers of multi-layer PCBs are microstrips. A diagram of a microstrip cross section is
shown in Figure 71: Microstrip Cross Section below.
The second structure is the “stripline”, in which a trace or pair of traces is sandwiched between
two reference planes, as shown in Figure 72: Strip Line Cross Section below. If the traces are
exactly halfway between the reference planes, then the stripline is said to be symmetric or
balanced. Usually the traces are a lot closer to one of the planes than the other (often because
there is another orthogonal trace layer, which is not shown in Figure 72: Strip Line Cross Section
below). In this case, the striplines are said to be asymmetric or unbalanced. Inner layer traces
on multi-layer PCBs are usually asymmetric striplines.
Before proceeding with a Carrier Board layout, designers should decide on a PCB stack-up and
on trace parameters, primarily the trace-width and differential-pair spacing. It is quite a bit harder
to change the differential impedance of a trace pair after layout work is done than it is to change
the impedance of a single-ended signal. That is because (with reference to Figure 71: Microstrip
Cross Section below, Figure 72: Strip Line Cross Section below, Table 60 'Trace Parameters'
below) the geometric factors that have the biggest impact on the impedance of a single-ended
trace are H1 and W1.
Both H1 and W1 can be manipulated slightly by the PCB vendor. The differential impedance of a
trace pair depends primarily on H1, W1 and the pair pitch. A PCB vendor can easily manipulate
H1 and W1 but changing the pair pitch cannot generally be done at fabrication time. It is more
important for the PCB designer and the Project Engineer to determine the routing parameters for
differential pairs ahead of time.
Work with a PCB vendor on a suitable board stack-up and do your own homework using a PCB-
impedance calculator. An easy to use and comprehensive calculator is available from Polar
Instruments (www.polarinstruments.com). Many PCB vendors use software from Polar
Instruments for their calculations. Polar Instruments offers an impedance calculator on a low-
cost, per-use basis. To find this, search the Web for a “Polar Instruments subscription”.
Alternatively, impedance calculators are included in many PCB layout packages, although these
are often incomplete when it comes to differential-pair impedances. There also are quite a few
free impedance calculators available on the Web. Most are very basic, but they can be useful.
PICMG ® COM Express ® Carrier Board Design Guide Rev. 2.0 / December 6, 2013
175/218