Background on Traditional Techniques

A Technique to Reduce Cross Talk Between Copper Routes Under a 1 mm Pitch BGA (WP547)

Document ID
Release Date
1.0 English

A typical BGA pin is 0.5 mm/19.68th pad, with a 45-degree breakout. The traditional clearance rules to manufacture a PCB include:

  • 9 mil drill to trace
  • 3 mil trace to trace on internal
  • 4 mil trace to trace on outer layers
  • 8 mil via drill (finished hole size)

Inside the BGA breakout, exit lanes are created to allow the internal routing of signals from under the BGA region. The typical 1 pin 1 via 45° breakout creates a structure as shown in the following figure.

Figure 1. Internal Routing Lanes

This 1 pin 1 via structure is used to create routing lanes on multiple internal layers to allow a clear area for breakout. The following figures show routing on internal layers below the BGA device to break out multiple differential signal pairs.

Figure 2. Internal Layer 3 (Layer Top — 2)
Figure 3. Internal Layer 5 (Layer Top — 4)
Figure 4. Internal Multiple Layers of Available Routing
Important: These lanes must be maintained to allow the practical use of 1 mm pitch BGA. The vias are arranged in a 1 mm pitch manner equally spaced (see the following figure).
Figure 5. Lanes Maintained to Allow Practical Use of 1 mm Pitch