3 Layout Planning and Design
4.1 Design Rules for Analog Circuits
In today’s world, people can easily assume that they live in an all-digital world, yet analog signals are still found within more than 60 per cent of present-day electronic designs. The three important considerations which form the basis for design rules for analog circuit PCBs are:
a Component placement;
a Signal conductors; and
a Supply and ground line conductors.
4.1.1 Component Placement
Component placement plays a crucial role, especially in analog circuits PCB design. The important guidelines to be followed in this regard are:
a Components which need to be accessed from the front panel must be placed exactly according to the requirements of the equipment designer.
a Components for internal adjustments such as potentiometers, trimmers, switches, etc. should be arranged near the board edge and placed in the proper direction for easy operation.
a Components with metal cases should not be placed very near to potentiometers, trimmers and switches etc. otherwise while adjusting, the screwdriver may cause a short-circuit between the component and the equipment chassis.
Copyright © 2006 by The McGraw-Hill Companies, Inc. Click here for terms of use.
a The placing of heat-producing and heat-sensitive components must be carefully planned. Heat- producing components should be placed away from the heat-sensitive components.
a Heat-producing components should be uniformly distributed over the entire board area as far as possible. This will avoid local over-heating of the board.
a Components likely to get heated must be separated from the board surface by suitable spacers.
Provision for space for these spacers should be made on the board.
a Where mounting screws need to be provided, the requisite space for nut and washer must be planned for, and no conductive track should be run underneath.
4.1.2 Signal Conductors
Signal conductors in analog circuit PCBs have to perform a variety of different tasks including input, reference level, feedback, output, etc. Therefore, a signal line for one application has to be optimized in a different manner than for another application. But a common consideration in all analog circuit PCB designs is to keep the signal conductor as short as possible. This is because the magnitude of the undesirable inductive and capacitive coupling effects increases almost proportionally to the length of the signal conductor. It may not always be possible to keep all signal conductors as short as possible. A practical approach in such a case is to identify the most critical signal conductor and to put it first in the layout.
The signal conductor layout has to be made carefully, particularly for the following types of circuits:
a High frequency amplifiers/oscillators;
a Multi-stage amplifiers especially with high power output stage;
a High gain dc amplifiers;
a Low level signal amplifiers; and a Differential amplifiers.
High Gain dc Amplifiers
High gain dc amplifiers are generally used to amplify low level signals. When a device like a transistor or dc amplifier is soldered on to the PCB, a thermocouple junction can be formed between copper and the lead of the device. This will create different voltages, which in turn, will generate a noise signal to the amplifier. In order to minimize the temperature gradient at the input stage of the dc amplifier and to maintain a stable temperature gradient, it is advisable to put the input stage in a separate enclosure which does not allow a free movement of the surrounding air.
Differential Amplifier
A differential amplifier amplifies the voltage difference between two signals and rejects the common voltage on both signals. When the signal level is low, the common voltage will interfere and create small difference signals if the differential amplifier and its PCB are not properly designed. The differential amplifier inputs have high impedance to ground and any unbalance in them will bring
Design Considerations for Special Circuits 157
down the circuit performance to an unacceptable level. Therefore, the physical geometrical symmetry of the amplifier on the PCB must be ensured during layout design.
A finite leakage resistance exists at the input of the differential amplifier, which can cause an unbalanced offset voltage. This problem can be solved by providing guarding at the input circuit.
This arrangement is shown in Figure 4.1. The guard encloses the signal conductors and if it is kept at the same potential as the low line of the two signal conductors, it would result in an increase in the effective resistance. This type of arrangement ensures that the source end and the guard line are at the same potential as the low end of the signal source. Figure 4.2 shows how guarding can be done on a PCB. The guard conductor in the form of a loop encloses the signal conductors from the input connector upto the amplifier input solder joints and is connected with the guard of the equipment.
This method facilitates an efficient technique of handling low level differential signals. In addition, the PCB base material used for low level differential amplifiers should preferably be of glass epoxy type, which aids in reducing leakage currents.
Amplifier
VCM
Guard
Chassis (box) Guard (box)
High High
Low Low
Guard R1 R2
Source (Thermocouple)
Fig. 4.1 Guarding a differential amplifier. At the source end, guard line is at the same potential as low end
+ – High
Low
Guard Connector end
AmplifierIC (8 pin pack)
Fig. 4.2 Guarding signal conductors on a PCB (after Bosshart, 1983)
Low-level Signal Amplifiers: The amplifiers handling low-level signals are of two types.
High-impedance (low current) Amplifier: In these amplifiers, the capacitive coupling between two neighbouring signal conductors can seriously affect the circuit perform- ance, even leading to masking of the low level signal.
Capacitive coupling between the two conductors in high impedance circuit is shown in Figure 4.3. In order to minimize the coupling, it is advisable to provide a sufficient
distance between the high impedance conductors and the other interfering signal. As a rule of thumb, the separation distance may be kept at least 40 times the signal conductor width.
However, the capacitance of low level signal conductors to ground should be high so that the coupled voltage is low. This implies that low level signal conductors should be close to ground conductors. If a wide separation is not possible, the coupling can be reduced by putting a ground conductor in between as shown in Figure 4.4.
GND
Ca–b Cb–GND Ca–GND
Ca–GND Ca–b
a b a GND b
Cb–GND
Laminate
Ca–b > Cb–GND > Ca–GND Ca–GND = Cb–GND >> Ca–b
Criticalconfiguration Improvedversion
Fig. 4.4 Cross-talk reduction in parallel running signal lines by having a ground conductor between them (after Bosshart, 1983)
When amplifying signals from photocells and electrochemical cells, source impedance may be many millions or billions of ohms. If PCBs are inadequately cleaned after etching, the residual electrolytes on the board surface may result in comparable resistances between nearby conductors.
Even with properly cleaned boards, leakage resistances of no more than 1012 ohms can be expected.
These resistances, moreover, are unlikely to be isotropic so that the resistance between two adjacent tracks may be higher than that between two tracks separated by a much larger gap. For this reason,
Ca–GND
Cb–GND
Ca–b
R
High-impedance signal b
a
Va
Fig. 4.3 Capacitive coupling between two conductors in high impedance circuits (after Bosshart, 1983)
Design Considerations for Special Circuits 159
the inputs to low-level I/V converters should be protected by guard rings on both sides of the PCB (Figure 4.5) connected to a point at the same potential as the summing junction. If this is done, the exact value of the leakage resistance is unimportant since the potential difference across it will be small.
R1
R2
RL
Surfaceleakage on aPCB is unpredictable.R is not necessarily less than R
1 2
If avulnerable conductoris surrounded bya guard ring (on both sides of the board) whichis at the same potential as the conductoritis guarding, the effects ofleakage resistance willbe minimized
Fig. 4.5 Reduction of leakage resistance on printed circuit boards by using a guard ring
In applications of this type, the use of plated through-holes (PTH) is inadvisable. The bulk resistivity of PCB material is much lower than the sheet resistivity of its surface and it is very difficult to fabricate a guard ring in the bulk of a board. The best approach is to connect such high impedance amplifier terminals to a Teflon insulator rather than a PCB track. This is shown in Figure 4.6.
Low-impedance (low voltage) Amplifier: In case of low impedance circuits, there is a likelihood of having induced voltages due to inductive coupling or magnetic fields. This interference can be reduced to some extent by
a Placing conductors carrying higher level ac signals sufficient away from low-level signal conductors;
a Providing ground conductors near the signal conductors; and
Teflon PCB
I.C.
Fig. 4.6 Use of a Teflon stand-off insulator which has a much lower leakage than a PCB track
a Avoiding ground loops to disable the external magnetic field from disturbing low level signals.
High Frequency Amplifiers/Oscillators
An improper PCB layout of a high frequency amplifier results in a reduced bandwidth of the amplifier.
Such a situation is shown in Figure 4.7. This is because the proximity of the ground conductors and signal conductors results in a high capacitance, which, along with the output resistance, acts as a low pass filter.
C
C
in out
Amplifier 1 Amplifier 2
C Input
Output
Fig. 4.7 High-frequency amplifier configuration
This action degrades the bandwidth of the amplifier. Also, if the input and output conductors are close to each other, there can be a feedback resulting in oscillations. In order to solve this problem, sufficient spacing must be provided between such conductors to avoid this effect (Lindsey, 1985).
It is a common experience of electronic circuit designers that at high frequencies (>10 MHz), that you design an amplifier, but in practice, it oscillates. Similar problems are encountered in designing the layout of an oscillator; it does not oscillate at the desired frequency. Such problems arise due to the presence of a capacitive coupling effect between the signal lines. One important precaution while making the PCB layout in such cases is to reduce the capacitive coupling between signal lines.
Multi-stage Amplifiers with High Power Output Stage
Multi-stage amplifiers are prone to low frequency oscillations, if supply and ground conductors are too long. The large current drawn by the high power stage will flow through the conductors with their own resistivity. This problem can be solved by de-coupling of the power supply conductors with sufficient large capacitors between supply and ground (Figure 4.8). Alternatively, separate power supply and ground conductors can be provided for the two different stages so that there is no common supply or ground path.
Design Considerations for Special Circuits 161
Input driver/amplifier
High-power output stage VCC
Input
GND
R
R
i+ 1
i+ 1
i I
I
Fig. 4.8 Multi-stage amplifier with high-power output stage: providing separate power supply and ground conductors to avoid common supply guard path
4.1.3 Supply and Ground Conductors
Power supply lines should be of sufficient width to keep the resistance and inductance to a low value. However, the capacitive coupling to ground increases with more width.
Analog and digital circuits on the same PCB should strictly have independent ground network conductors. Similarly, reference voltage circuits, which are normally sensitive to ground potential fluctuations, should tap the supply lines directly at the input to the PCB and its ground line should be connected separately to the stable ground reference point of the equipment. Such an arrangement is shown in Figure 4.9.
GND
VRef
Digital circuit part Analog circuit part Referencevoltages circuit part
Fig. 4.9 Provision of separate ground conductors for reference, analog and digital circuit parts
In real life, ground conductors have both resistance and inductance, and may also be carrying unpredictable currents, which will have voltage drops when they flow in the ground impedances.
CAD PCB programs are particularly bad at ground design because they tend to keep all conductors
as thin as possible to conserve copper and the board area, and this, of course, results in high ground resistance. There is an obvious alternative to thin ground leads — a continuous “ground plane” of copper covering one side of a PCB to which all ground connections are made. The resistance of 0.001" (0.025 mm) copper is approximately 0.67 mW/square inch so that this solution is frequently adequate — but not always.
4.1.4 General Rules for Design of Analog PCBs
A few general rules concerning design of PCBs for analog circuits are:
a Keep the signal path as short as possible. This will help to minimize both voltage drops through the conductors as well as electromagnetic interference by controlling loop areas.
a Provide separate analog and digital grounds and tie the two together only once.
a Provide one connection from the system ground to the actual earth ground.
a Connect capacitive shields once to provide a return path to the noise source.
a Magnetic shields must be made out of a highly permeable material to be effective.
a Metal should not be left electrically floating.
a Maintain the balance of a system to prevent common mode signals from becoming differential.
a Limit the bandwidth of the system to the required signal bandwidth.
a Keep loop areas small and always think as to where the currents will flow.
a Between the two PCBs, use twisted pair cable to improve the noise rejection of a system.
The use of software packages for the design of high speed analog PCBs, typically containing through-hole and SMT components, shielding and signals running at 2 GHz are illustrated by Meyer et. al., (1991)