Click to get → [Ground Layer Usage Guide]

Maintaining a low impedance, large area ground plane is important for all current analog circuits. The ground plane not only serves as a low impedance return path for decoupling high frequency currents (originating from fast digital logic), but also minimizes EMI/RFI emissions. Due to the shielding effect of the ground plane, the circuit is also less susceptible to external EMI/RFI.

The ground plane also allows the use of transmission line technologies (microstrip or stripline) to transmit high-speed digital or analog signals, which require controlled impedance.

Since the "bus wire" has impedance at most logic switching equivalent frequencies, it is completely unacceptable to use it as a "ground". For example, #22 standard wire has an inductance of about 20nH/in. A transient current with a slew rate of 10mA/ns generated by a logic signal will form an unnecessary voltage drop of 200mV when flowing through 1 inch of this wire:

For a signal with a 2V peak-to-peak range, this voltage drop translates to an error of about 200mV or 10% (about "3.5 bits of accuracy"). Even in a fully digital circuit, this error can significantly reduce the logic noise margin.

Figure 1 shows the digital return current modulating the analog return current (top). The ground return conductor inductance and resistance are shared by the analog and digital circuits, which can affect each other and ultimately produce errors.

Figure 1. Digital current flowing in the analog return path creates an error voltage.

One possible solution is to have the digital return current path flow directly to GND REF, as shown in the bottom figure. This shows the basic concept of a “star” or single-point ground system. It is difficult to achieve a true single-point ground in a system that contains multiple high-frequency return paths. Because the physical length of each return current conductor will introduce parasitic resistance and inductance, it is difficult to obtain a low-impedance high-frequency ground. In practice, the current return path must be composed of a large area ground plane to obtain low impedance to high-frequency currents. Without a low-impedance ground plane, it is almost impossible to avoid the shared impedance mentioned above, especially at high frequencies.

All integrated circuit ground pins should be soldered directly to a low impedance ground plane to minimize series inductance and resistance. Traditional IC sockets are not recommended for high-speed devices. Even with a "small footprint" socket, additional inductance and capacitance may introduce unwanted shared paths that can degrade device performance. If a socket must be used with a DIP package, such as when prototyping, individual "pin sockets" or "cage sockets" are acceptable. The above pin sockets are available in both covered and uncovered versions. The use of spring-loaded gold contacts ensures good electrical and mechanical connection to the IC pins. However, repeated insertion and removal may degrade their performance.

Low-inductance, surface-mount ceramic capacitors should be used to decouple the power pins directly to the ground plane. If through-hole ceramic capacitors must be used, their lead length should be less than 1 mm. The ceramic capacitors should be placed as close to the IC power pins as possible. Ferrite beads may also be required for noise filtering.

A ground plane solves many ground impedance problems, but not all. Even a continuous copper foil has residual resistance and inductance that, in certain circumstances, can be enough to prevent a circuit from functioning properly. Figure 2 illustrates this problem and shows how to solve it.

Figure 2. Splitting the ground plane can change the direction of current flow, thereby improving accuracy.

Due to practical mechanical design reasons, the power input connector is at one end of the board, while the power output section, which needs to be close to the heat sink, is at the other end. The board has a 100 mm wide ground plane, and there is a power amplifier with a current of 15 A. If the ground plane is 0.038 mm thick, 15 A of current will produce a voltage drop of 68 μV/mm when flowing through it. This voltage drop will cause serious problems for any precision analog circuits that share this PCB and use ground as a reference. The ground plane can be split to prevent the large current from flowing into the precision circuit area and force it to flow around the split. This will prevent the grounding problem (which exists in this case), but the voltage gradient will be increased in the part of the ground plane where the current flows.

In a multiple ground plane system, be sure to avoid overlapping ground planes, especially analog and digital layers. This problem will result in capacitive coupling from one layer (probably digital ground) to another. Remember that a capacitor is made up of two conductors (the two ground planes) separated by an insulator (the PC board material).

If there is a break in the ground plane beneath the conductor, the ground plane return current must flow around the break. This causes the circuit inductance to increase, and the circuit is more susceptible to external fields. Figure 3 shows this situation, where conductors A and B must pass through each other.

Figure 3. A split ground plane increases circuit inductance and makes the circuit more susceptible to external fields.

When the split is to cross two vertical wires, it is better to connect the second signal line across the first signal line and the ground plane through a flying lead. In this case, the ground plane acts as a natural shield between the two signal lines, and due to the skin effect, the two ground return currents will flow on the upper and lower surfaces of the ground plane respectively without interfering with each other.

Multilayer boards can support both signal line crossing and continuous ground planes without having to consider line link issues. Although multilayer boards are more expensive and not as easy to debug as simple double-sided boards, they provide better shielding and signal routing. The principles remain the same, but there are more layout and routing options.

Using a double-sided or multi-layer PCB with at least one continuous ground plane is undoubtedly one of the most successful design methods for high-performance mixed-signal circuits. Usually, the impedance of such a ground plane is low enough to allow the analog and digital parts of the system to share a single ground plane. However, whether this can be achieved depends on the resolution and bandwidth requirements and the amount of digital noise in the system.

Other examples illustrate this point. High frequency current feedback amplifiers are very sensitive to capacitance around their inverting inputs. An input trace next to a ground plane can have the type of capacitance that can cause problems. Remember that a capacitor is made up of two conductors (the trace and the ground plane) separated by an insulator (the board and possibly solder mask). In this regard, the ground plane should be separated from the input pins, as shown in Figure 4, which is an evaluation board for the AD8001 high speed current feedback amplifier. The effect of a small capacitor on a current feedback amplifier is shown in Figure 5. Note the ringing on the output.

Figure 4. AD8001AR evaluation board—top view (a) and bottom view (b)

Figure 5. Effect of 10pF inverting input stray capacitance on the pulse response of an amplifier (AD8001).