Product specifications

Design Guide - VT82C694X Apollo Pro133 with VT82C686A
Preliminary Revision 0.5, November 19, 1999 15 Motherboard Design Guidelines
Technologies, Inc.
We ConnectWe Connect
2.2.3 Printed Circuit Board Description
A brief description of the Printed Circuit Board (PCB) for an Apollo Pro133A based system is provided in this section. From a
cost-effectiveness point of view, a four-layer board is recommended for the motherboard design. For better quality, a six-layer
board is preferred. These two types of boards will be discussed below:
2.2.3.1 Four-Layer Board
A four-layer stack-up with 2 signal layers and 2 power planes is shown in Figure 2-7. The two signal layers are referred to as the
component layer and the solder layer. The two power planes are the power layer and the ground layer. The sequence of
component layer-ground layer-power layer-solder layer is the most common stack-up arrangement from top to bottom. It is
recommended to place a 5~6 mil substrate between the solder layer and the power plane and between the component layer and the
ground plane, with a 42~45 mil substrate between the power and ground planes. Dielectric constant, E
r
, should be 4.5 for all
substrate materials.
Routing any signal trace on the power planes, either on the power layer or on the ground layer, is not recommended. If a signal
must be routed on the power planes, then it should be routed as short as possible on the power layer, not on the ground layer. The
impedance of all signal layers is to be in the range between 55 ohms and 75 ohms. Lower trace impedance providing better signal
quality is preferred over higher trace impedance for clock signals.
5~6 mils
42~45 mils
5~6 mils
Component layer (0.5 oz. Copper)
Ground layer (1 oz. Copper)
Solder layer (0.5 oz. Copper)
Power layer (1 oz. Copper)
Figure 2-7. Four-Layer Stack-up with 2 Signal Layers and 2 Power Planes