Tips about printed circuit board design: Part 1 - Dealing with harmful PCB effects
Double-Sided vs Multilayer PCBs
Each PCB in the system should have at least one complete layer dedicated to the ground plane. Ideally, a double-sided board should have one side completely dedicated to ground and the other side for interconnections. In practice this is not possible, since some of the ground plane will certainly have to be removed to allow for signal and power crossovers, vias, and through-holes. Nevertheless, as much area as possible should be preserved, and at least 75% should remain.
After completing an initial layout, the ground layer should be checked carefully to make sure there are no isolated ground “islands,” because IC ground pins located in a ground “island” have no current return path to the ground plane.
Also, the ground plane should be checked for “skinny” connections between adjacent large areas which may signifi cantly reduce the effectiveness of the ground plane. Needless to say, autorouting board layout techniques will generally lead to a layout disaster on a mixed-signal board, so manual intervention is highly recommended.
Systems that are densely packed with surface-mount ICs will have a large number of interconnections; therefore multilayer boards are mandatory. This allows at least one complete layer to be dedicated to ground. A simple four-layer board would have internal ground and power plane layers, with the outer two layers used for interconnections between the surface mount components.
Placing the power and ground planes adjacent to each other provides additional interplane capacitance which helps high-frequency decoupling of the power supply. In most systems, four layers are not enough, and additional layers are required for routing signals as well as power. Figure C.8 below summarizes the key issues relating to ground planes.
Figure C.8: Ground planes are mandatory!
Multicard Mixed-Signal Systems
The best way of minimizing ground impedance in a multicard system is to use a “motherboard” PCB as a backplane for interconnections between cards, thus providing a continuous ground plane to the backplane. The PCB connector should have at least 30–40% of its pins devoted to ground, and these pins should be connected to the ground plane on the backplane mother card. To complete the overall system grounding scheme there are two possibilities:
The backplane ground plane can be connected to chassis ground at numerous points, thereby diffusing the various ground current return paths. This is commonly referred to as a “multipoint” grounding system and is shown in Figure C.9 below. The ground plane can be connected to a single system “star ground” point (generally at the power supply).
Figure C.9: Multipoint ground concept.
The first approach is most often used in all-digital systems but can be used in mixed-signal systems, provided that the ground currents due to digital circuits are sufficiently low and diffused over a large area. The low ground impedance is maintained all the way through the PC boards, the backplane, and ultimately the chassis.
However, it is critical that good electrical contact be made where the grounds are connected to the sheet-metal chassis. This requires self-tapping sheet-metal screws or “biting” washers. Special care must be taken where anodized aluminum is used for the chassis material, since its surface acts as an insulator.
The second approach (“star ground”) is often used in high-speed, mixed-signal systems having separate analog and digital ground systems and warrants further discussion.
Separating Analog and Digital Grounds
In mixed-signal systems with large amounts of digital circuitry, it is highly desirable to physically separate sensitive analog components from noisy digital components. It may also be beneficial to use separate ground planes for the analog and the digital circuitry.
These planes should not overlap in order to minimize capacitive coupling between the two. The separate analog and digital ground planes are continued on the backplane using either motherboard ground planes or “ground screens,” which are made up of a series of wired interconnections between the connector ground pins.
The arrangement shown in Figure C.10 below illustrates that the two planes are kept separate all the way back to a common system “star” ground, generally located at the power supplies.
Figure C.10: Separating analog and digital ground planes.
The connections between the ground planes, the power supplies, and the “star” should be made up of multiple bus bars or wide copper braids for minimum resistance and inductance. The back-to-back Schottky diodes on each PCB are inserted to prevent accidental DC voltage from developing between the two ground systems when cards are plugged and unplugged.
This voltage should be kept less than 300 mV to prevent damage to ICs that have connections to both the analog and digital ground planes. Schottky diodes are preferable because of their low capacitance and low forward voltage drop. The low capacitance prevents AC coupling between the analog and digital ground planes.
Schottky diodes begin to conduct at about 300 mV, and several parallel diodes in parallel may be required if high currents are expected. In some cases, ferrite beads can be used instead of Schottky diodes, but they introduce DC ground loops, which can be troublesome in precision systems.
It is mandatory that the impedance of the ground planes be kept as low as possible, all the way back to the system star ground. DC or AC voltages of more than 300 mV between the two ground planes not only can damage ICs, but they can cause false triggering of logic gates and possible latchup.
Loading comments... Write a comment