Data Sheet

Design Considerations—Ethernet Controller I210
823
12.5.6.6 Signal Termination and Coupling
The I210 has internal termination on the MDI signals. External resistors are not needed. Adding pads
for external resistors can degrade signal integrity.
12.5.6.7 Signal Trace Geometry for 1000 BASE-T Designs
The key factors in controlling trace EMI radiation are the trace length and the ratio of trace-width to
trace-height above the reference plane. To minimize trace inductance, high-speed signals and signal
layers that are close to a reference or power plane should be as short and wide as practical. Ideally, this
trace width to height above the ground plane ratio is between 1:1 and 3:1. To maintain trace
impedance, the width of the trace should be modified when changing from one board layer to another if
the two layers are not equidistant from the neighboring planes.
Each pair of signal should have a differential impedance of 100  ± 15%. Refer to the Intel
®
1G
Servers and Client LANs – Copper Loss Calculator for more details.
When performing a board layout, do not allow the CAD tool auto-router to route the differential pairs
without intervention. In most cases, the differential pairs will have to be routed manually.
Note: Measuring trace impedance for layout designs targeting 100  often results in lower actual
impedance. Designers should verify actual trace impedance and adjust the layout accordingly.
If the actual impedance is consistently low, a target of 105 – 110  should compensate for
second order effects.
It is necessary to compensate for trace-to-trace edge coupling, which can lower the differential
impedance by up to 10 , when the traces within a pair are closer than 30 mils (edge to edge).
Figure 12-16.MDI Trace Geometry