### Ground

#### Where Good Signals Go When They Die

Introduction

Too many engineers actually believe the simplification that treats "ground" as a perfect current sink with no potential differences, and that any points in a system which can be represented by the triangle or the dangling worms are joined together by an inductance-free superconductor in which the speed of light (and electrical propagation) is infinite. In fact neither room temperature superconductors nor hyperdrives have yet been invented, and real life is much less orderly.

This application note discusses some of the issues that need to be considered in the layout of analog system grounds, and in particular issues of ground impedance, ground configuration, and ground noise.

Basic Law of Engineering - Murphy's Law

#### Figure 1

Murphy's Law is the subject of many engineering jokes, but, in its simplest form, "What can go wrong, will!" it states the simple truth that physical laws do not cease to operate just because we have overlooked or ignored them. In analog design (and most other branches of engineering, too), there are plenty of effects that are easy to overlook, but which will cause chaos if they are not considered.

The most important laws to keep in mind when designing the ground layout of an analog system are Ohm's Law and Kirchoff's Law, and also Lenz's Law and Faraday's Law. We may also need to consider the Seebeck Effect.

When designing any analog circuit (or, indeed any circuit at all), we should ask ourselves what the effects of these laws might be on our circuit layout, and do some simple calculations to determine if the magnitudes involved are large enough to merit more detailed analysis.

Resistance of Copper Conductors

Every engineer is familiar with resistors – little cylinders with wire ends or surface-mounted blocks with tinned ends – although perhaps fewer are aware of all their idiosyncrasies. But how many of us consider that all the wires and PC tracks with which our systems and circuits are assembled are also resistors?

#### Figure 2

Copper is not a room temperature superconductor. At 25°C the resistivity of pure copper is 1.724E-6 Ω cm. The thickness of standard (1 ounce) PCB foil is 0.038 mm (0.0015"). The resistance of standard PCB copper is therefore 0.45 mΩ/square, which implies a resistance for the 0.25 mm track frequently used in computer designed digital circuitry of 18 mΩ/cm, which is quite large. Thus, minimum width tracks cannot be used for analog grounds, or for any other ground where any very substantial current is likely to flow.

Moreover, the temperature coefficient of resistance (TC) for copper is about 0.4%/°C around room temperature, which can be a further inconvenience in precision analog circuitry, although copper's resistance TC is unlikely to cause major issues in ground design.

Skin Effect

At high frequencies, we must consider both the dc resistance of our conductors and the "skin effect", where inductive effects cause currents to flow only on their surface. This has the effect of increasing the resistance of a conductor at high frequencies (note that this effect is separate from the increase in impedance due to the effects of the self-inductance of conductors as frequency is increased--that will be dealt with later). Skin effect is a complex phenomenon, and detailed calculations are beyond the scope of this note. However, a good approximation for copper is that the skin depth in centimeters is 6.6/√f (f in Hz).

#### Figure 3

Assuming that skin effects become important when the skin depth is less than 50% of the thickness of the conductor, this tells us that for normal 0.038 mm PC foil, we must be concerned about skin effects at frequencies above approximately 12 MHz.

Where skin effect is important, the resistance per square for copper is 2.6E-7 √f Ω/square (f in Hz). It is very important to remember that this formula is valid only when the conductor thickness is greater than the skin depth (otherwise the resistance – from this formula – would be zero at dc. And, as I have previously mentioned, copper is not a superconductor).

When calculating skin effect in PCBs, it is important to remember that current may flow in both sides of the PC foil (this is not the case in microstrip lines) so the resistance per square of PC foil may be half the above value.

Signal Return Currents

Kirchoff's Law tells us that at any point in a circuit the algebraic sum of the currents is zero. This tells us that all currents flow in circles and, particularly, that the return current must always be considered when analyzing a circuit.

#### Figure 4

Most people consider the return current when considering a fully differential circuit, but when considering the more usual circuit where a signal is referred to "ground", it is common to assume that all the points on the circuit diagram where the ground symbol is to be found are at the same potential. This is unwise.

Figure 5 shows the ideal and the dismal reality. In real life, the return current flows in the complex impedance that exists between the two "ground" points shown in the ideal, giving rise to a voltage drop in the total signal path. Furtherrmore, external currents may also flow in the same path, generating uncorrelated noise voltages which are also seen by the load.

"Noise" in electronics refers to unwanted signals that corrupt wanted signals. There are two basic types: signals generated by (often unavoidable) physical processes in the signal path of a system, and signals actually wanted (by someone) which find their way into a place where they are not wanted. This ground noise is the second type.

#### Figure 5

It is evident, of course, that other currents can only flow in the ground impedance if there is a current path for them. Figure 5 shows such a path at "ground" potential, which is the notorious "Ground Loop", but equally severe problems will arise if a circuit shares an unlooped ground return with another circuit generating too much current (ac or dc) for the common ground impedance, as in Figure 6.

#### Figure 6

It is evident from Figure 7 that if a ground network contains loops, there is a greater danger of it being vulnerable to EMFs induced by external magnetic fields, and of ground current "escaping" from high current areas to cause noise in sensitive regions. For these reasons ground loops are best avoided.

#### Figure 7

However, there are situations where looped grounds are unlikely to cause unacceptable noise, and the configuration may actually offer benefits in the form of safety or reduced impedance. In such circumstances, the optimum ground arrangement may contain loops. Sensible engineers should not allow the almost superstitious dread inspired by the term "ground loop" to prevent the adoption of such designs, if careful analysis and experiment has shown that they actually are optimum.

There are a number of possible ways of attacking the problem of ground noise, apart from the (presently) impractical one of using superconducting grounds. It is rare for a single method to be used to the exclusion of all others, and systems generally contain a mixture of approaches. For the purposes of description, however, it is better to describe each approach separately.

Star Grounds

The "star" ground philosophy builds on the theory that there is a single point in a circuit to which all voltages are referred. This is known as the "star" point.

This philosophy is reasonable, but frequently encounters practical difficulties. For example, if we design a system with a star ground, drawing all the signal paths to minimize signal interaction and the effects of high impedance signal or ground paths, we frequently find, when the power supplies are added to the circuit diagram, that they either add unwanted ground paths or that supply currents, flowing in existing ground paths, are sufficiently large, or noisy, or both, as to corrupt the signal transmission. This problem may often be avoided by having separate power supplies for different parts of the circuit. Separate analog and digital supplies, and separate analog and digital grounds, joined at the star point, are common in mixed signal applications.

Separate Analog and Digital Grounds

Digital circuitry is noisy. Most saturating logic draws large, fast current spikes from its supply during switching and, having noise immunity of hundreds of millivolts or more, has little need of very high levels of supply decoupling. (4000 series CMOS is a welcome, if rather slow, exception to the "high current spike" problem and despite being over 30 years old is still valuable where low noise, rather than high speed or high density, "glue" logic is required.)

Analog circuitry, on the other hand, is very vulnerable to noise in supplies or grounds. It is therefore sensible to separate analog and digital circuitry to prevent digital noise from corrupting analog performance. This will involve separation of both grounds and power supplies, which may be inconvenient in a mixed signal system. Nevertheless, if a system is to give the full performance of which it is capable, it is often essential to have separate analog and digital grounds and power supplies. The fact that much modern analog circuitry will operate from a single positive low-voltage supply does NOT mean that it may be operated satisfactorily from the same noisy supply as the microprocessor and dynamic RAM, the electric fan, the buzzer, and the solenoid jackhammer!

Not all analog circuitry is noise-free, of course. If there are noisy analog circuits in a system they may well also need separate grounds from the high-precision or low-noise analog circuits. In either case, all the grounds – analog and digital – in a system must be joined at some point to allow signals to be referred to a common potential. This star point, or analog/digital common point, is chosen so that it does not introduce noise currents into the ground of the sensitive analog part of the system – it is usually most convenient to make the connection at the power supplies. (In extremely noisy systems the need for a common star point may be avoided by the use of galvanic isolation – digital, or analog, or both. This will not be covered in this article but read the data on the AD202, AD210 and similar analog isolators, and the ADuM family of iCoupler® digital isolators.)

Many ADCs and DACs have separate "analog ground" (AGND) and "digital ground" (DGND) pins, and users are advised, on the data sheets, to connect these pins together at the device package. This seems to conflict with the advice to connect analog and digital ground at the power supplies, and, in systems with more than one converter, with the advice to join the analog and digital ground at a single point.

There is, in fact, no conflict. The labels AGND and DGND on these pins refer to the parts of the converter where the pins are connected, and not to the system grounds to which they must go. These two pins should be joined together with the lowest possible impedance (short lead, no resistor, no inductor, no ferrite bead) and to the analog ground of the system. Converters only have separate AGND and DGND pins when it is not possible to join the two pins within the IC package because the analog part of the converter cannot tolerate the voltage resulting from the digital current flowing in the bond wire impedance – many ADCs and DACs do not have this problem and have a single ground pin.

If AGND and DGND are connected in this way, the digital noise immunity of the converter is diminished by the amount of common-mode noise between the digital and analog system grounds. Since digital noise immunity is of the order of hundreds or thousands of millivolts, this is unlikely to matter very much.

The analog noise immunity is diminished only by the external digital currents of the converter itself flowing in the analog ground. These currents should be quite small, and can be minimized by ensuring that the converter outputs do not drive large fanouts. If the logic supply to the converter is isolated with a small resistance and decoupled to analog ground with a 0.1ΩF capacitor located as close to the converter as possible, all the internal digital currents of the converter will return to ground through the capacitor and will not appear in the external ground circuit. If the analog ground impedance is as low as it should be for adequate analog performance, the additional noise due to the external digital ground current should rarely present a problem.

Ground Planes

Related to the star ground system is the use of a ground plane. One side of a double-sided PCB, or one layer of a multi-layer one, is made of continuous metal, used as ground. The theory behind this is that the large amount of metal will have low resistance, and as low inductance as is possible.

It is sometimes argued that ground planes should not be used because they are liable to introduce problems in manufacture and assembly. Such an argument may have had a limited validity in the past when PCB adhesives were less well developed, wave-soldering less reliable, and solder resist techniques less well understood, but today it should not be tolerated – get a new PCB facility if they will not make ground planes!

Ground planes solve many ground impedance problems, but not all. Even a continuous sheet of copper foil has residual resistance and inductance; in some circumstances, they can be enough to prevent proper circuit function. Figure 8 shows such a problem and a possible solution.

#### Figure 8

Consider a ground-plane PCB 100 mm wide with a ground connection at one end and a power amplifier at the other drawing 15 A. If the ground plane is 0.038 mm thick and 15 A flows in it, there will be a voltage drop of 68 ΩV/mm. This voltage drop would cause quite serious problems to any ground-referenced precision circuitry sharing the PCB. However, if we slit the ground plane so that high current does not flow in the region of the precision circuitry, we can possibly solve the problem – even though the voltage gradient will increase in those parts of the ground plane where the current does flow.

Transmission Lines

A break in a ground plane is not always a good thing. If outward and return signal paths are close together inductance is minimized, so a break in the ground under a ground-referred signal will increase inductance in the signal path. As mentioned in Figure 3, when an HF signal flows in a PC track running over a ground plane the arrangement functions as a microstrip transmission line, and the majority of the return current flows in the ground plane underneath the line.

#### Figure 9

The characteristic impedance of the line will depend upon the width of the track, the thickness of the PCB, and the dielectric constant, Er, of the material. For most lower frequency applications, the characteristic impedance will be unimportant, as the line will not be correctly terminated, but at UHF and higher it is possible to use PCB tracks as microstrip transmission lines in properly terminated systems. If losses in such systems are to be minimized, the PCB material must be chosen for low loss at high frequency, which usually means the use of expensive Teflon substrate material.

Where there is a break in the ground plane under a conductor, the return current must flow around the break, and both the inductance and the vulnerability of the circuit to external fields are increased.

Where such a break is made to allow a crossover of two perpendicular conductors, it is far better if the second signal is carried across both the first and the other side of the ground plane by means of a piece of insulated wire than by breaking the ground plane and making a crossover in the copper of the ground plane layer of the board. The ground plane then acts as a shield between the two signal conductors, and the two ground return currents, flowing in opposite sides of the ground plane as a result of skin effects, do not interact.

#### Figure 10

With a multi-layer board, both the crossover and the continuous ground plane can be accommodated without the need for a wire link. Multi-layer PCBs are expensive and harder to trouble-shoot than simple double-sided boards, but do offer even better shielding and signal routing. The principles involved remain unchanged but the range of layout options is increased.

Use of double-sided or multi-layer board with at least one continuous ground plane is undoubtedly one of the most successful approaches to the design of high performance mixed signal circuitry. Often the impedance of the ground plane is sufficiently low to permit the use of a single ground plane for both analog and digital parts of the system, but this does depend upon the resolution and bandwidth required, and the amount of digital noise in the system.

System Grounds

In systems where there are several PCBs, grounding may be more of a problem. At first sight, it would appear that the problem is similar to that of a single PCB, where particular subsystems must be positioned so that large ground currents do not flow where ground noise must be minimized. In a multicard system, the grounds of individual PCBs must be interconnected so that such harmful interactions are minimized.

There are three problems with this. First of all, there is far less opportunity to rearrange the physical layout of a system consisting of a few cards connected to a common backplane. Secondly, many multicard systems are designed to be reconfigured in a "mix 'n' match" arrangement to allow a large number of system options. It can be impossible to predict what systems are going to be required and to ensure that all of them are noise free. Finally, multicard systems are likely to have higher ground currents than occur on single, relatively simple, PCBs, but these currents must flow in the higher impedances associated with intercard connectors, even when multiple ground pins are used.

Multiple ground pins in PCB connectors are very important (multiple power pins are a good idea, too). The connector of a PCB should not have one, or even two, ground pins – it should have many. Possibly as many as 20% of all the pins should be ground pins. These multiple pins serve two functions: minimizing ground impedance and providing shielding between signal conductors. If we measure the resistance of a single pin on a new connector it will be quite low, a few mΩ with luck, but it will be far higher if we measure it after a decade of service in a dirty, humid, high vibration environment. If we want our equipment to continue to work we must consider this and design for worst case end of life high contact resistance. Ground pins in a connector also minimize crosstalk by acting as electrostatic shields between signal pins. If the connector leads are long, it makes sense to separate signal leads with ground leads. This arrangement acts as a transmission line, minimizing mutual inductance and capacitive coupling between circuits.

The basic principles still apply: ground impedance must be as low as possible, high level and low level signals must be separated so that they do not interfere with each other, and capacitance and mutual inductance coupling must be avoided. Nevertheless, it must be accepted that situations can arise where it is not possible to transfer a high speed, high-accuracy signal from one PCB to another in a noisy system without unacceptable signal degradation.

A good way of minimizing ground impedance in a multicard system is to use another PCB as a backplane and have a ground plane (or even two—one analog, one digital) on that mother card. If there are multiple ground pins this arrangement is capable of excellent performance. Where there are several card cages (racks for PCBs), the ground planes of the several mother boards must be tied together and, probably, to the metal chassis holding the card cages – the exact layout of the interconnections will depend on the overall system architecture.

If a mother board with a ground plane is not possible, then the ground pins of the PCB sockets must be wired together – with due attention to probable current flows and common ground impedances – with heavy, multi-strand wire, having as low resistance as possible. In many cases, the resulting ground screen will be tied to chassis ground at a number of points, but it will sometimes be better to join them at a single star point.

It is not just the ground layout that is important in high performance mixed signal systems, the location of different subsystems and the routing of signals is most important in determining overall system performance.

Signal Routing

It is evident that we can minimize noise by paying attention to the system layout and preventing different signals from interfering with each other, possibly by using ground plane as a screen. High level analog signals should be separated from low level analog signals, and both should be kept away from digital signals. We have seen elsewhere that in waveform sampling and reconstruction systems, the sampling clock (which is a digital signal), is as vulnerable to noise as any analog signal, but it is as liable to cause noise as any digital signal, and so must be kept isolated from both analog and digital signals.

#### Figure 11

Figure 11 shows a good layout for a data acquisition system where all sensitive areas are isolated from each other, and signal paths are kept as short as possible. While real life is rarely as tidy as this, the principle remains a valid one.

Modern high performance mixed signal systems handle signals with very high resolution, 12-bits or more, at sampling rates of hundreds of MHz. Preserving signal integrity between cards in a multi-card system is extremely difficult at such performance levels, and may be impossible.

#### Figure 12

Differential signal transmission is very useful in such cases but it is not a panacea. In the past differential amplifiers with high common-mode rejection ratios (CMRR) were mostly low-frequency devices and high-frequency differential amplifier were either unavailable as ICs or not very high performance. Modern high-speed bipolar processes have changed this and in the last few years very high performance differential amplifiers, with high CMRR and working at frequencies in the low GHz range, have become readily available. (See the Analog Devices AD813x series.) Nevertheless where inter-card ground noise is high the optimum solution is to partition the system so that the most critical analog signals are not transferred between boards.

Conclusion

We have seen that inadequate ground design can seriously degrade the performance of analog systems, and have reviewed a number of techniques for addressing the issues involved. But while poor ground design is undoubtedly the commonest cause of poor analog performance it is not the only one. System performance can also be degraded by poor choice of passive components and by noise coupled into the system by e-fields, m-fields, e-m fields, conduction through power lines, and by optical coupling where glass diodes respond to modulated light. Such issues are outside the scope of this article but should never be overlooked.

James M. Bryant
23 January 2006