NOISE IN PCB DESIGN

A Guide for PCB Designers
by Bill Chambers, PE

INTRODUCTION

There are many ways that noise can crop up in circuits, and it is usually harmful. It can be random, but often it results when one circuit picks up another's signal. Radio waves, for instance, are very useful when you tune in your radio -- but they can cause problems in any other circuit. To keep noise to a minimum, you need to reduce the efficiency of both generators and receivers of noise.

Most of the sources of random noise are either resistors or semiconductors and tubes. The thermal energy of electrons produces noise in every resistance, even if it is not connected to anything. Any current flow in a tube includes noise, because each electron strikes the plate at a slightly different moment. Semiconductor junctions have a similar problem. These sources are fundamental to circuitry, and it's difficult to reduce the noise they produce.

You can, however, reduce all types of pick-up. These can affect circuits in many ways. They often seem random, but there is always an underlying cause. If two traces are too close, current can flow directly between them. Two circuits that share a common ground or power supply line can influence each other through the impedance of the line they share. Thermal effects can generate spurious voltages. Electric fields, magnetic fields, and Electro/Magnetic waves (E/M radiation, including radio waves) can affect circuits at a distance and are called EMI.

Nodes are most sensitive to noise currents if they have a high impedance and carry low level or very accurate signals. An electric field may induce the problem current, or it may come from circuitry connected directly to the node. Because trace impedance rises with frequency, this problem is worst at high frequencies. To disturb a low impedance point, a noise source would have to inject a large amount of current.

Loops are sensitive to magnetic fields if they have a low impedance and a large area. Any loop that current can flow around may be affected, even if it is made up of several nodes. Most power supplies are slightly affected. Ground, however, has a lower impedance than the complete supply loop and is often very sensitive to noise.

Other factors which make a node sensitive include the length and layout of its traces. Traces which pass near a noise source will be affected by that source. Long traces act like antennas and are generally more sensitive to all types of noise. (If there are strong radio waves in the circuit or nearby, however, particular trace lengths will cause the most trouble. These lengths are multiples of 1/4 of the wave's length.

REDUCING COUPLING AT THE SOURCE

Careful trace layout is important. Route sensitive traces away from noisy traces and components. Try to keep both types of traces short. (Even if the engineer doesn't say anything, treat any clock signals with care.) Keep your normal traces and spaces as wide as possible. One effective but rather awkward trick is to avoid running problem traces parallel to any others. Consider reserving one layer of a multi-layer board for a few of these traces. Avoid loops, and keep the necessary ones as small as possible. All of these methods reduce cross-talk by keeping capacitive and inductive coupling to a minimum.

Regular, 'pretty' board layout is good for high densities but produces high noise levels. The narrow, cramped, parallel traces that it uses have high cross-talk and relatively high impedances. Always check if there are power levels, high frequencies, or sensitive circuits which may demand special treatment. The faster logic families, including 74F and 74AC, should have wide spaces between ALL traces.

Circuits which share a common trace can interfere with each other. Prevent this by keeping trace impedances low. Otherwise, a voltage drop will occur in each trace. This error is equal to the amount of current flowing multiplied by the impedance. Suppose that you have to use 11 inches of 20 mil trace to bring ground to one part. A similar trace carries power. If you specify one-ounce copper for the board, this trace has a resistance of 1/2 Ohm. Then a direct current of 100 mA will drop 50 mV along the trace. This may be acceptable for digital power and ground, but it is a substantial error. Circuits that are further out along the same trace will be subjected to the full error. Resistance decreases proportionally as you increase trace thickness and width.

Ground and power are the most important connections. Any noise in a circuit's power and ground will appear on every one of its outputs! Ground is usually a little more important than power. One of the most common causes of EMI is an RF voltage on a ground run. This can be eliminated by proper grounding.

While you probably cannot reduce the peak amount of power that the circuit draws, you can provide that power and keep it clean. Use heavy traces to provide both power and ground. Make sure that there is at least one electrolytic capacitor from each supply to ground. These traces and capacitors provide for the power requirements of the circuit from DC up to about 1 MHz.

At DC, a trace's impedance is only resistance (R.) At high frequencies, the trace inductance (L) is more important and the impedance is approximately 6.28 x f x L. Keep inductance low by using wide, short, straight traces. 45 degree angle turns are better than sharper ones, but they still add inductance. Radio frequency circuits use smooth curves whenever a trace must change direction.

Digital circuits use much of their current in high frequency pulses. A good deal of it is in the range of 10 to 200 MHz. Here, inductance is much more important than resistance. In the previous example, the trace has a resistance of 1/2 Ohm. The same trace has an inductance of at least 0.41 uHenry. At 10 MHz, this inductance is equivalent to an impedance of 26 Ohms -- making the trace all but useless. Wider copper is helpful, but to halve the inductance you need 10 times the width. Trace inductance increases a little more than proportionally with length.(1)

This is the reason that each IC power supply pin should have its own ceramic decoupling capacitor. 0.1 uFd is usually enough, but the data sheets of large digital parts (28 pins and larger) often call for larger values. Connect this capacitor between the IC's power and ground pins with the shortest, heaviest possible traces. Do not connect it between two IC's unless you're certain that this will provide the shortest return path for current.(2) These capacitors are more effective than the electrolytic parts at 1 MHz and beyond.

Electrolytic capacitors and long traces have too much inductance to be useful at high frequencies. Ceramic capacitors have a low inductance, so they can supply the pulses of current that the IC's require. The short connections keep the impedance low, and keep the high frequency currents flowing in as small a loop as possible. The impedance of each 0.1 uFd capacitor at 10 MHz is under 0.2 Ohms. If you have to use 1.2" of 100 mil trace to connect it, however, the trace inductance adds 1.4 Ohms to that!

Adding a ground plane to the board greatly reduces this impedance. It also limits the loop area and fields for every trace. High frequency currents try to minimize loop area. In an unbroken plane, the return current for each trace will flow directly under (or over) that trace. A plane with lots of small breaks in it, such as a component-side plane, is still helpful but has much less effect at high frequencies. If you cannot use a plane, use a regular ground grid in which each IC connects to all of its neighbors.

A board with both power and ground planes has both small loops and very low impedances. It does not need as many decoupling capacitors for the power plane net as a double-sided board would. For the lowest possible impedance at high frequencies, some designers add one 0.001 uFd surface mount capacitor between the two planes.

Remember that other nodes besides power and ground can have trouble with circuits connected to a common trace. Any high current or high accuracy node may have the same problem. If a plane layer is not available, the best way to avoid interference is to run a separate trace for each sensitive circuit. Even if an added trace has to be narrower, it will reduce noise.

After you've run separate traces back to the power connector, you may want to add more connector pins for the same reason. This is most useful if one part of the circuitry is for gross power and another is more sensitive. Displays, motor controllers, and other parts often have at least two separate grounds for these functions.

Thermocouple effects will induce small DC errors when a component's leads aren't all at the same temperature. When laying out accurate analog circuits, keep all components away from sources of heat. If a resistor must be near something hot, both ends should be equally close. Be sure that resistors have equal lead lengths and trace widths -- especially those that dissipate as much as 1/10 of their rated power. Note that this means a hot resistor should not connect directly to a ground plane in one of these circuits.

MITIGATION

So far this article has focused on stopping noise at the source. If you still have problems after reducing the sources as much as possible, you will need to work on containing the noise.

Remember those sensitive, high-impedance nodes. Even when they are as small as you can make them, current from nearby signals or power may still leak into them. One way to reduce this problem is to clean the finished PCB assembly and apply a conformal coating of plastic. This keeps moisture and contamination out, reducing leakage, but it's more difficult to service a coated board.

A guard etch is a much cleaner solution to the same problem. A guard is a piece of etch which surrounds the sensitive node on both sides of the board, and shunts away any leakage currents. The guard must connect to a low impedance point which is at the same voltage as the node it is protecting. Ideally, the guard should surround the node completely. (Often, the guard connects to ground and surrounds the inverting input node of an op amp.) Ask the engineer if there are any points that need to be guarded, and how to drive the guards.

Ground planes have a similar shunting effect on capacitively coupled noise. They are most effective if placed directly between the source and the sensitive node. Separate sheets of metal have the same effect, and also will block radio waves and high frequency magnetic fields. Magnetic fields are hard to shield below about 10 kHz. Shields are most effective when they completely enclose the sensitive circuit.

Wires can carry noise in and out of a system, but adding the right filters will stop it. Placing an impedance in series with the wire will reduce the noise current, and adding a capacitor to ground will keep that current from producing a large voltage. Even the power supply lines often need small series impedances. Small resistors, ferrite beads, and coils are all suitable in some cases. Many EMI filters are available off the shelf.

To protect against large surges coming from outside the board, there may be spark gaps, varistors, or high power zener diodes. These function somewhat like decoupling capacitors: they limit the current flow to a small area, and keep it away from the rest of the board. To be effective, they need short connections. The trace between the input connector and the protective device (or devices) must not have any branches leading to the rest of the board, so there is no way around the protector. The device's leads should be soldered into the middle of both the signal (or power) and return tracks.

In extreme cases, it may be worthwhile trying to spoil the efficiency of traces that are acting as antennas. This may be possible by changing trace length and orientation. It may also be necessary to rotate the position of the finished PCB in the system. Antennas couple most efficiently when they are parallel to each other.

PITFALLS

There are a few common mistakes to avoid.

The biggest mistake is using the wrong ground. Earth ground would be ideal, but usually the connection is many feet long. Then the best available ground is chassis ground. All noise filters, including decoupling capacitors, should connect to the chassis as directly as possible. All grounds must be connected together unless isolation is important.

Don't break up your ground plane unless it's really necessary. Remember that any high frequency currents will try to flow through the plane close to each trace. If there's a break in the way, the current will have to follow a longer path: it will see a higher impedance and will radiate more noise.

In ground planes, keep areas of high current flow away from sensitive circuitry and its ground connections. Although the plane has a low impedance, a large current will cause small errors. Sometimes you need to split the plane, or make a slit in it, to keep the current in its place. Slit all plane layers at the same location.

If you use shielded wires, connect the shield at only one point. (This point should be at the signal or sensor end of the cable.) Otherwise, even a tiny difference in the 'ground' potentials between the two ends of the cable will cause a current to flow through the shield. This current is right next to the conductor you are trying to protect, and will couple noise into it. It will also radiate the ground noise. There may be enough current flow to blow fuses or cause damage.

(There are two reasons that it may be necessary to ground the shield several places. If there could be an extreme difference in ground potentials, (over 24 Volts,) it would be a safety hazard. But be sure that the ground current isn't also a hazard. The best way to protect against external EMI is to use a shielded, twisted pair. The twisted pair will tend to reject any fields from the shield or outside. If external EMI is severe, sometimes grounding the shield more than once will help.)

Pull-up resistors are often driven by several digital outputs which are far apart, giving a long current path. Small-valued resistors pass more current, contributing to the problem. If possible, move the outputs closer together and place the resistor near to the middle output.

NOTES:

(1) Formulas and data from the Mixed Signal Design Seminar book, page XI-25. Analog Devices, (617) 329-4700, Norwood, MA, c 1991.
(2) This may be necessary for high accuracy analog circuits. It is NOT possible with devices that drive several similar loads, as on a digital bus. For details, see "Analog Signal-Handling for High Speed and Accuracy," by A. Paul Brokaw, Analog Dialogue, 11- 2 1977. Analog Devices.

Copyright Notice:

Copyright 1997 by William Chambers. Feel free to distribute this article and notice for non-commercial purposes. All World Wide Web links are welcome. No changes may be made without permission of the author.

Bill Chambers runs Acquisition & Control Electronics, a Boston area consulting firm doing analog circuit review and design. If you have questions, feel free to contact him at KILLspamA at @spam@D2A.com.

To continue:

For a short resume ...
For a more detailed resume ...
Or a brochure about my services ...
For links to other Web sites ...
For more tutorials on analog design and more links ...
Back to Acquisition & Control Electronics' Home Page ...

The address of this page is http://www.channel1.com/users/analog/noise.html