Noise and Grounding:Audio Ampliﬁer Printed Circuit Board Design

Audio Ampliﬁer Printed Circuit Board Design

This section addresses the special printed circuit board (PCB) design problems presented by power ampliﬁers, particularly those operating in Class-B. All power ampliﬁer systems contain the power-amp stages themselves, and usually associated control and protection circuitry; most also contain small-signal audio sections such as balanced input ampliﬁers, subsonic ﬁlters, output meters, and so on.

Other topics related to PCB design, such as grounding, safety, and reliability, are also dealt with.

The performance of an audio power ampliﬁer depends on many factors, but in all cases the detailed design of the PCB is critical because of the risk of inductive distortion due to cross talk between the supply rails and the signal circuitry; this can very easily be the ultimate limitation on ampliﬁer linearity, and it is hard to overemphasize its importance. The PCB design will, to a great extent, deﬁne both the distortion and the cross talk performance of the ampliﬁer.

Apart from these performance considerations, the PCB design can have considerable inﬂuence on ease of manufacture, ease of testing and repair, and reliability. All of these issues are addressed here.

Successful audio PCB layout requires enough electronic knowledge to fully appreciate the points set out here so that layout can proceed smoothly and effectively. It is common in many electronic ﬁelds for PCB design to be handed over to draftspersons, who, while very skilled in the use of CAD, have little or no understanding of the details of circuit operation. In some ﬁelds this works ﬁne; in power ampliﬁer design it will not because basic parameters such as cross talk and distortion are so strongly layout dependent. At the very least the PCB designer should understand the points that follow.

Cross Talk

All cross talk has a transmitting end (which can be at any impedance) and a receiving end, usually either at high impedance or at virtual earth. Either way, it is sensitive to the injection of small currents. When interchannel cross talk is being discussed, the transmitting and receiving channels are usually called speaking and nonspeaking channels, respectively.

Cross talk comes in various forms:

● Capacitative cross talk is a consequence of the physical proximity of different circuits and may be represented by a small notional capacitor joining the two circuits. It usually increases at the rate of 6 dB/octave, although higher dB/octave rates are possible. Screening with any conductive material is a complete cure, but physical distance is usually less expensive.

● Resistive cross talk usually occurs simply because ground tracks have a nonzero resistance. Copper is not a room-temperature superconductor. Resistive cross talk is constant with frequency.

● Inductive cross talk is rarely a problem in general audio design; it might occur if you have to mount two uncanned audio transformers close together, but otherwise you can usually forget it. The notable exception to this rule is the Class-B audio power ampliﬁer, where the rail currents are halfwave sines that seriously degrade the distortion performance if allowed to couple into the input, feedback, or output circuitry.

In most line-level audio circuitry the primary cause of cross talk is unwanted capacitative coupling between different parts of a circuit, and in most cases this is deﬁned solely by the PCB layout. Class-B power ampliﬁers, in contrast, should suffer very low or negligible levels of cross talk from capacitative effects, as circuit impedances tend to be low and the physical separation large; a much greater problem is inductive coupling between the supply-rail currents and the signal circuitry. If coupling occurs to the same channel, it manifests itself as distortion and can dominate ampliﬁer nonlinearity. If it occurs to the other (nonspeaking) channel it will appear as cross talk of a distorted signal. In either case it is thoroughly undesirable, and precautions must be taken to prevent it.

The PCB layout is only one component of this, as cross talk must be both emitted and received. In general, the emission is greatest from internal wiring due to its length and extent; wiring layout will probably be critical for best performance and needs to be ﬁxed by cable ties, etc. The receiving end is probably the input and feedback circuitry of the ampliﬁer, which will be ﬁxed on the PCB. Designing these sections for maximum immunity is critical to good performance.

Rail Induction Distortion

The supply rails of a Class-B power-amp carry large and very distorted currents. As outlined previously, if these are allowed to cross talk into the audio path by induction, the distortion performance will be severely degraded. This applies to PCB conductors just as much as cabling, and it is sadly true that it is easy to produce an ampliﬁer PCB that is absolutely satisfactory in every respect but this one, and the only solution is another board iteration. The effect can be completely prevented, but in the present state of knowledge I cannot give detailed guidelines to suit every constructional topology. The best approach is to minimize radiation from the supply rails by running the V+ and V– rails as close together as possible. Keep them away from the input stages of the ampliﬁer and the output connections; the best method is to bring the rails up to the output stage from one side, with the rest of the ampliﬁer on the other side. Then run tracks from the output to power the rest of the amp; these carry no halfwave currents and should cause no problems.

Minimize pick-up of rail radiation by keeping the area of the input and feedback circuits to a minimum. These form loops with the audio ground and these loops must be as small in area as possible. This can often best be done by straddling the feedback and input networks across the audio ground track, which is taken across the center of the PCB from input ground to output ground.

Induction of distortion can also occur into the output and output-ground cabling, and even the output inductor. The latter presents a problem as it is usually difﬁcult to change its orientation without a PCB update.

Mounting of Output Devices

The most important decision is whether to mount the power output devices directly on the main ampliﬁer PCB. There are strong arguments for doing so, but it is not always the best choice.

Advantages

● The ampliﬁer PCB can be constructed so as to form a complete operational unit that can be tested thoroughly before being ﬁxed into the chassis. This makes testing much easier, as there is access from all sides; it also minimizes the possibility of cosmetic damage (scratches, etc.) to the metalwork during testing.

● It is impossible to connect the power devices wrongly, providing you get the right devices in the right positions. This is important for such errors usually destroy both output devices and cause other domino-effect faults that are very time- consuming to correct.

● The output device connections can be very short. This seems to help stability of the output stage against HF parasitic oscillations.

Disadvantages

● If the output devices require frequent changing (which obviously indicates something very wrong somewhere) then repeated resoldering will damage the PCB tracks. However, if the worst happens, the damaged track can usually be bridged out with short sections of wire so that the PCB need not be scrapped; make sure this is possible.

● The output devices will probably get fairly hot, even if run well within their ratings; a case temperature of 90°C is not unusual for a TO3 device. If the mounting method does not have a degree of resilience, then thermal expansion may set up stresses that push the pads off the PCB.

● Because the heat sink will be heavy, there must be a solid structural ﬁxing between this and the PCB. Otherwise the assembly will ﬂex when handled, putting stress on soldered connections.

Single- and Double-Sided Printed Circuit Boards

Because of their lower cost, single-sided PCBs are the usual choice for power ampliﬁers; however, the price differential between single- and double-sided plated-through-hole (PTH) PCBs is much less than it used to be. It is not usually necessary to go double-sided for reason of space or convoluted connectivity, as power ampliﬁer components tend to be physically large, determining the PCB size, and in typical circuitry there are a large number of discrete resistors, etc., that can be used for jumping tracks.

Bear in mind that single-sided boards need thicker tracks to ensure adhesion in case desoldering is necessary. Adding one or more ears to pads with only one track leading to them gives much better adhesion and is highly recommended for pads that may need resoldering during maintenance; unfortunately, it is a very tedious task with most CAD systems.

The advantages of double-sided PTH for power ampliﬁers are as follow:

● No links are required.

● Double-sided PCBs may allow one side to be used primarily as a ground plane, minimizing cross talk and EMC problems.

● Much better pad adhesion on resoldering as the pads are retained by the through- hole plating.

● There is more total room for tracks so they can be wider, giving less volt drop and PCB heating.

● The extra cost is small.

Power Supply Printed Circuit Board Layout

Power supply subsystems have special requirements due to the very high capacitor- charging currents involved.

● Tracks carrying the full supply-rail current must have generous widths. The board material used should have not less than 2-oz copper. Four-ounce copper can be obtained but it is expensive and has long lead times; it is not really recommended.

● Reservoir capacitors must have the incoming tracks going directly to the capacitor terminals; likewise the outgoing tracks to the regulator must leave from these terminals. In other words, do not run a tee off to the cap. Failure to observe this puts sharp pulses on the DC and tends to worsen the hum level.

● The tracks to and from the rectiﬁers carry charging pulses that have a considerably higher peak value than the DC output current. Conductor heating is therefore much greater due to the higher value of I2R. Heating is likely to be especially severe at PC-mount fuse holders. Wire links may also heat up and consideration should be given to two links in parallel; this sounds crude but actually works very effectively.

Track heating can usually be detected simply by examining the state of the solder mask after several hours of full-load operation; the green mask materials currently in use discolor to brown on heating. If this occurs then as a very rough rule the track is too hot. If the discoloration tends to dark brown or black then the heating is serious and must deﬁnitely be reduced.

● If there are PCB tracks on the primary side of the mains transformer, and this has multiple taps for multicountry operation, then remember that some of these tracks will carry much greater currents at low voltage tappings; mains current drawn on 90 V input will be nearly three times that at 240 V.

Be sure to observe the standard safety spacing of 60 thou between mains tracks and other conductors for creepage and clearance. (This applies to all track-track, track-PCB edge, and track-metal-ﬁxings spacings.)

In general, PCB tracks carrying mains voltages should be avoided, as presenting an unacceptable safety risk to service personnel. If it must be done, then warnings must be displayed very clearly on both sides of the PCB. Mains-carrying tracks are unacceptable in equipment intended to meet UL regulations in the United States, unless they are fully covered with insulating material that is nonﬂammable and can withstand at least 120°C (e.g., polycarbonate).

Power Ampliﬁer Printed Circuit Board Layout Details

A simple unregulated supply is assumed.

● Power ampliﬁers have heavy currents ﬂowing through the circuitry, and all of the requirements for power supply design also apply here. Thick tracks are essential, and 2-oz copper is highly desirable, especially if the layout is cramped.

If attempting to thicken tracks by laying solder on top, remember that ordinary 60:40 solder has a resistivity of about six times that of copper, so even a thick layer may not be very effective.

● The positive and negative rail reservoir caps will be joined together by a thick earth connection; this is called reservoir ground (RG). Do not attempt to use any

point on this track as the audio-ground starpoint, as it carries heavy charging pulses and will induce ripple into the signal. Instead, take a thick tee from the center of this track (through which the charging pulses will not ﬂow) and use the end of this as the starpoint.

● Low-value resistors in the output stage are likely to get very hot in operation— possibly up to 200°C. They must be spaced out as much as possible and kept from contact with components such as electrolytic capacitors. Keep them away from sensitive devices such as the driver transistors and the bias-generator transistor.

● Vertical power resistors. The use of these in power ampliﬁers appears attractive at ﬁrst because of the small amount of PCB area they take up. However, the vertical construction means that any impact on the component, such as might be received in normal handling, puts a very great strain on the PCB pads, which are likely to be forced off the board. This may result in it being scrapped. Single-sided boards are particularly vulnerable, having much lower pad adhesion due to the absence of vias.

● Solderable metal clips to strengthen the vertical resistors are available in some ranges (e.g., Vitrohm) but this is not a complete solution, and the conclusion must be that horizontal-format power resistors are preferable.

● Rail decoupler capacitors must have a separate ground return to the reservoir ground. This ground must not share any part of the audio ground system, and must not be returned to the starpoint.

● The exact layout of the feedback takeoff point is criticial for proper operation.

Usually the output stage has an output rail that connects the emitter power resistors together. This carries the full output current and must be substantial. Take a tee from this track for the output connection and attach the feedback takeoff point to somewhere along this tee. Do not attach it to the track joining the emitter resistors.

● The input stages (usually a differential pair) should be at the other end of the circuitry from the output stage. Never run input tracks close to the output stage. Input stage ground and the ground at the bottom of the feedback network must be the same track running back to the starpoint. No decoupling capacitors may

be connected to this track, but it seems to be permissible to connect input bias resistors that pass only very small DC currents.

● Put the input transistors close together. The closer the temperature match, the less the ampliﬁer output DC offset due to VBE mismatching. If they can both be

hidden from seeing the infra-red radiation from the heat sink (e.g., by hiding them behind a large electrolytic), then DC drift is reduced.

● Most power ampliﬁers will have additional control circuitry for muting relays, thermal protection, etc. Grounds from this must take a separate path back to the reservoir ground, and not the audio starpoint.

● Unlike most audio boards, power amps will contain a mixture of sensitive circuitry and a high-current power supply. Be careful to keep bridge rectiﬁer connections and so on away from input circuitry.

● Mains/chassis ground will need to be connected to the power ampliﬁer at some point. Do not do this at the transformer center tap as this is spaced away from the input ground voltage by the return charging pulses and will create severe ground- loop hum when the input ground is connected to mains ground through another piece of equipment.

Connecting mains ground to starpoint is better, as the charging pulses are excluded, but the track resistance between input ground and star will carry any ground-loop currents and induce a buzz.

Connecting mains ground to the input ground gives maximal immunity against ground loops.

● If capacitors are installed the wrong way round the results are likely to be explosive. Make every possible effort to put all capacitors in the same orientation to allow efﬁcient visual checking. Mark polarity clearly on the PCB, positioned so it is still visible when the component is ﬁtted.

● Drivers and the bias generator are likely to be ﬁtted to small vertical heat sinks.

Try to position them so that the transistor numbers are visible.

● All transistor positions should have emitter, base, and collector or whatever marked on the top print to aid fault ﬁnding. TO3 devices also need to be identiﬁed on the copper side, as any screen printing is covered up when the devices are installed.

● Any wire links should be numbered to make it easier to check that they have all been ﬁtted.

Audio Printed Circuit Board Layout Sequence

PCB layout must be considered from an early stage of ampliﬁer design. For example, if a front-facial layout shows the volume control immediately adjacent to a loudspeaker routing switch, then a satisfactory cross talk performance will be difﬁcult to obtain because of the relatively high impedance of the volume control wipers. Shielding metalwork may be required for satisfactory performance, which adds cost. In many cases the detailed electronic design has an effect on cross talk quite independently from physical layout.

a. Consider implications of facia layout for PCB layout.

b. Circuitry designed to minimize cross talk. At this stage, try to look ahead to see how op-amp halves, switch sections, and so on should be allocated to keep signals away from sensitive areas. Consider cross talk at above-PCB level; for

example, when designing a module made up of two parallel double-sided PCBs, it is desirable to place signal circuitry on the inside faces of the boards, and power and grounds on the outside, to minimize cross talk and maximize RF immunity.

c. Facia components (pots, switches, etc.) placed to partly deﬁne available board area.

d. Other ﬁxed components, such as power devices, driver heat sinks, input and output connectors, and mounting holes placed. The area left remains for the purely electronic parts of the circuitry that do not have to align with metalwork and so may be moved about fairly freely.

e. Detailed layout of components in each circuit block, with consideration toward manufacturability.

f. Make efﬁcient use of any spare PCB area to fatten grounds and high-current tracks as much as possible. It is not wise to ﬁll in every spare corner of a prototype board with copper as this can be time-consuming (depending on the facilities of your PCB CAD system) and some of it will probably have to be undone to allow modiﬁcations.

Ground tracks should always be as thick as practicable. Copper is free.

Miscellaneous Points

● On double-sided PCBs, copper areas should be solid on the component side for minimum resistance and maximum screening, but will need to be cross-hatched on the solder side to prevent distortion if the PCB is ﬂow soldered. A common standard is 10 thou wide noncopper areas, that is, mostly copper with small square holes; this is determined in the CAD package. If in doubt, consult those doing the ﬂow soldering.

● Do not bury component pads in large areas of copper, as this causes soldering difﬁculties.

● There is often a choice between running two tracks into a pad or taking off a tee so that only one track reaches it. The former is better because it holds the pad more ﬁrmly to the board if desoldering is necessary. This is particularly important for components such as transistors that are relatively likely to be replaced; for single-sided PCBs it is absolutely vital.

● If two parallel tracks are likely to cross talk, then it is beneﬁcial to run a grounded screening track between them. However, the improvement is likely to be disappointing, as electrostatic lines of force will curve over the top of the screen track.

● Jumper options must always be clearly labeled. Assume that everyone loses the manual the moment they get it.

● Label pots and switches with their function on the screen-print layer, as this is a great help when testing. If possible, also label circuit blocks, for example, DC offset detect. The labels must be bigger than component ident text to be clearly readable.

Measurement:Conventional Practice

Troubleshooting variable speed drives:The need for VSDs

LEARNING ABOUT ELECTRONICS FOR YOUR OWN GOOD:THE BIG PICTURE

CONTROL FUNDAMENTALS

OBJECTIVE TEST On Armature reaction and commutation

Measurement:The Tempered Scale And Measuring Distortion

Limit switches:Subminiature Micro Switches and Limit Switch Application

Cables and Cable Termination:Method of Fixing into Wood

Ladder Diagrams part2

Power and Energy:Work and Force

Appendix part1

Teeth defluxing by slots