Improving SMT pad design for high-frequency signal transmission

Impedance mismatch is often encountered at SMT pads of AC coupling (also known as DC blocking) capacitors, board-to-board connectors, and cable-to-board connectors (such as SMA).

In the case of the AC coupling capacitor SMT pad as shown in Figure 1, a signal propagating along a PCB trace with a 100Ω differential impedance and a 5mil copper width will encounter an impedance discontinuity when it reaches an SMT pad with a wider copper (such as 30mil width for 0603 package). This phenomenon can be explained by equations (1) and (2). The increase in the cross-sectional area or width of the copper will increase the strip capacitance, which in turn brings a capacitive discontinuity to the characteristic impedance of the transmission channel, i.e., a negative surge.

To minimize the capacitance discontinuity, the reference plane area directly under the SMT pad needs to be cut out and a copper fill is created on the inner layer, as shown in Figure 2 and Figure 3, respectively. This increases the distance between the SMT pad and its reference plane or return path, thereby reducing the capacitance discontinuity. Micro stitching vias should also be inserted to provide an electrical and physical connection between the original reference plane and the new reference copper foil on the inner layer to establish a proper signal return path and avoid EMI radiation issues.

However, the distance "d" should not be increased too much, otherwise the strip inductance will exceed the strip capacitance and cause inductance discontinuity. Where:

Strip capacitance (unit: pF);

Strip inductance (unit: nH);

Characteristic impedance (unit: Ω);

ε = dielectric constant;

Pad width;

Pad length;

The distance between the pad and the reference plane below;

The thickness of the pad.

The same concept can also be applied to SMT pads for board-to-board (B2B) and cable-to-board (C2B) connectors.

The above concept will be verified by TDR and insertion loss analysis. The analysis is done by building a 3D model of the SMT pad in EMPro software and then importing it into Keysight ADS for TDR and insertion loss simulation.

Analyzing the SMT pad effect of AC coupling capacitors

A 3D model of an SMT with a medium-loss substrate is created in EMPro, where a pair of microstrip differential traces are 2 inches long and 5 mil wide, in single-ended mode, 3.5 mils away from their reference plane. The traces enter from one end of a 30 mil wide SMT pad and exit from the other end.

Figures 4 and 5 show the simulated TDR and insertion loss plots, respectively. The SMT design without reference plane cutouts results in an impedance mismatch of 12Ω and an insertion loss of -6.5dB at 20GHz. Once the reference plane area under the SMT pad is cutout (where “d ” is set to 10mil), the mismatch impedance is reduced to 2Ω and the insertion loss at 20GHz is reduced to -3dB. Further increasing “d ” causes the strip inductance to exceed the capacitance, resulting in an inductance discontinuity, which in turn worsens the insertion loss (i.e., -4.5dB).

Analyzing the SMT pad effect of B2B connectors

A 3D model of the SMT pad of a B2B connector is created in EMPro, where the connector pin pitch is 20 mils, the pin width is 6 mils, and the pad is connected to a pair of 5-inch long, 5-mil wide, single-ended microstrip differential traces, 3.5 mils from their reference plane. The thickness of the SMT pad is 40 mils, which is almost 40 times the thickness of the microstrip PCB trace, including the connector pins and solder.

The increase in copper thickness will result in capacitance discontinuity and higher signal attenuation. This phenomenon can be seen in the TDR and insertion loss simulation graphs shown in Figure 6 and Figure 7, respectively. The impedance mismatch can be minimized by cutting out the copper area with an appropriate spacing "d" (i.e. 7mil) just below the SMT pad.

summary

The analysis in this article proves that cutting off the reference plane area directly under the SMT pad can reduce the impedance mismatch and increase the bandwidth of the transmission line. The distance between the SMT pad and the internal reference copper foil depends on the width of the SMT pad and the effective thickness of the SMT pad including the connector pin and solder. 3D modeling and simulation should be performed before the PCB is put into production to ensure that the constructed transmission channel has good signal integrity.