In signal launch terminology, the "stub effect" is denoted as the resonant effect created when a trace enters a hole on a top layer of the board and leaves the hole on another top layer, creating a length of unused hole in the board that is left to ring and to create an effective decrease in impedance. An example of stub effect can be seen in Figure 7.

Figure 7.

A reflection profile is shown of two plated through holes on the same board at raw TDR rise times. The holes are exactly the same except for the length of metal stub on the launch. The first hole has approximately 0.220" of stub and the second launch has approximately 0.010" of metal stub. The impedance mismatch is greater for the maximum stub, with an impedance of 31.43 ohms compared to an impedance of 40.65 ohms.

Expanded Ground Clearances

Another way to improve PCB hole impedance is to expand the anti-pads in the ground planes of the boards. Enlarging the clearances reduces the effective capacitance between inner ground clearances and the barrel of the plated through holes.

Figure 8 shows the improvement in the time domain produced by enlarging the anti-pads on a standard hole.

Figure 8.

Counter Bore

Counter boring effectively reduces the capacitive effect of plated through holes by making the printed circuit board look electrically thinner (any removed portion of the plated through hole decreases the amount of anti-pad to barrel capacitance generated) and reduces the stub effect.

From the data measured, an improved impedance matched hole can be produced using current technologies. By decreasing the diameter of the plated through hole, reducing the amount of unused hole, removing non-functional pads (DesignCon 2000), and increasing the anti-pad diameter, the reflections are reduced and signal attenuation is minimized.

Figure 9.

Laminate selection is another variable to be considered in designing a 10 Gbps system. In this case study, two materials will be considered. The traditional material (FR-4) and a more exotic laminate with a lower dielectric constant and reduced loss tangent. Both test fixtures had an equal number of layers and identically layouts (trace topologies, minimal stubs, improved SMA launch) with thickness variations caused only by changes in material thickness to get a 50 ohm transmission line. Board thickness was approximately 0.80" and trace length was limited to 6" At 2.5 Gbps rates, differences between materials and line widths may be small, but as speeds approach 10 Gbps, even incremental line length changes begin to show measurable differences.

Figure 10.