Intel 82562EX, Руководство по конструкции

Страница: 31 / 68

82540EP/82541(PI/GI/EI) & 82562EZ(EX) Dual Footprint Design Guide
23
4.1.3 Board Stackup Recommendations
Printed Circuit Boards (PCBs) for these designs typically have four, six, eight, or more layers.
Following is a description of a typical four-layer board stackup:
•
Layer 1 is a signal layer. It can contain the differential analog pairs from the Ethernet device to
the magnetics module.
•
Layer 2 is a signal ground layer. Chassis ground may also be fabricated in Layer 2 under the
connector side of the magnetics module.
•
Layer 3 is used for power planes.
•
Layer 4 is a signal layer.
This board stackup configuration can be adjusted to conform to an OEM’s design rules.
4.1.4 Differential Pair Trace Routing
Trace routing considerations are important to minimize the effects of crosstalk and propagation
delays on sections of the board where high-speed signals exist. Signal traces should be kept as short
as possible to decrease interference from other signals, including those propagated through power
and ground planes. Observe the following suggestions to help optimize board performance:
•
Maintain constant symmetry and spacing between the traces within a differential pair.
•
Keep the signal trace lengths of a differential pair equal to each other. Do not use serpentines
to try to match trace lengths in the differential pair. Serpentines cause impedance variations
causing signal reflections, which can be a source of signal distortion. Try to keep the length
difference of the differential pair less than 100 mil (~15 pS). Always go straight to the required
via or pad.
•
Keep the total length of each differential pair under four inches. Designs with differential
traces longer than five inches are much more likely to have degraded receive Bit Error Rate
(BER) performance, IEEE PHY conformance failures, or excessive Electromagnetic
Interference (EMI) radiation.
•
Do not route the transmit differential traces closer than 100 mils to the receive differential
traces for 10/100 Mbps.
•
Do not route any other signal traces (including other differential pairs) parallel to the
differential traces and closer than 100 mils to the differential traces.
•
Separate traces within a differential pair as small as possible down to five to eight mils. Close
separation of the traces allows the traces to couple well to each other.
•
For high-speed signals, the number of corners and vias should be kept to a minimum. If a 90°
bend is required, it is recommended to use two 45° bends instead. (see
Figure 6 .)