Optimizing BNC PCB Footprint Designs for Digital Video Equipment

How to choose a BNC connector and properly design the BNC footprint on a high-speed printed circuit board — with the goal of meeting the tight requirements for SMPTE return loss. This article provides an overview of the types of BNCs in the broadcast video market, the test to determine the BNC’s electrical quality, common mistakes in BNC footprint designs, techniques for designing good BNC footprints and the use of 3D simulation tools to determine layout decisions.

By Tsun-kit Chin
Applications Engineer, Member of Technical Staff National Semiconductor Corp.

Page 5 of 8
Video/Imaging DesignWire
(9/10/2010 1:05:28 AM)

BNC Selections
The choice of BNCs is primarily determined by their mechanical construction and compatibility to the equipment’s enclosure. On the electrical front, the BNCs are expected to support up to 3Gbit/s transmission with little insertion loss. They are also expected to maintain uniformity and a fairly constant characteristic impedance in their coaxial structure. They preferably have small signal pins, such that the smallest possible through-hole or landing pads can be used in the footprint designs with the goal of minimizing impedance discontinuity.

Transparent BNC Footprints – Surface-mount BNCs
A transparent footprint is one that has identical characteristic impedance as the BNC connector, and does not significantly add circuit parasitic that impacts the BNC’s bandwidth. Several techniques are explored here. One effective method is to walk through the signal path, look for board geometry that deviates from the target impedance, and devise means to restore the impedance back to the target value.

In the case of the surface mount BNC shown in Figure 7, the large landing pad creates a huge impedance drop. Raising its impedance requires the use of larger dielectric separation (H>>15mils), which is not an option. One way to raise the pad’s impedance is to shave off the excessive parasitic capacitance by using relief in one or more power plane layers under the pad. The size of the relief opening is designed to provide just enough fringing capacitance to restore the landing pad’s impedance to its target. Figure 11 illustrates this technique of using plane relief under the pad. The footprint is dependent on the location of the first GND plane, and the location as well as the number of power planes used in the board.
null
Figure 11: Use of Plane Relief for Surface-mount BNC footprint

View full size

Figure 12 shows an example of an improved footprint. In this example, a larger GND/VCC relief is used on all the power planes under the pad. This step raises the characteristic impedance of the pad well above 75Ω (the target impedance for this example). To bring the impedance back to the target 75Ω, strips of ground metal are added on both sides of the pad. The ground strips are placed at a pre-determined distance from the pad, such that they introduce just enough ground coupling to achieve the desired impedance2. This structure has the advantage of being fairly independent from different board stack-ups, and can be re-used in multiple board designs.

null
Figure 12: Use of GND relief and GND guards for a surface mount BNC footprint

View full size

NEXT: Transparent BNC Footprints – Through-hole BNCs

Page 5: next page

Pages: 1 2 3 4 5 6 7 8



MOST POPULAR ARTICLES