Placement and Routing Considerations for General-purpose Analog Circuit Boards

A “general-purpose” analog circuit board is defined here as one that uses common analog circuitry (op amps, transistors, etc.) that operates at only a few megahertz (MHz) of bandwidth. This type of circuit is fairly forgiving of circuit board placement and routing oversights, but there are a few guidelines still to be followed. Proper ground and power distribution (as described in Chapter Two) is important, as are decoupling capacitors. Beyond that, you should not have many problems.

Placement and Routing Considerations for General-purpose Digital Circuit Boards

“General-purpose” digital circuit boards contain digital circuitry (gates, counters, microcontrollers, etc.) that operates up to about 20 MHz. There is usually not much critical timing in the design. Once again, this board type is fairly forgiving of placement or routing oversights. Since the circuitry on the board is digital, however, there are a few other things to think about when placing and routing your board.

Most modern digital circuitry is CMOS (complementary metal oxide semiconductor) of one type or other, rather than the older TTL (transistor-transistor logic). CMOS logic consumes much less power and switches faster than TTL. The increased speed comes with a price, however; the price is noise! The extremely fast transitions on CMOS logic outputs—1 nanosecond (ns) or less—produce much more power supply noise and crosstalk than TTL logic.

To prevent CMOS logic from corrupting your power supply, be sure to use appropriate decoupling capacitors. As a minimum, you should have one capacitor (0.1 μF ceramic is typical) per CMOS chip. Place the capacitor close to the chip’s power pin, as described in Chapter Two. Devices with more than one power pin need more than one decoupling capacitor; one decoupling capacitor per power pin is sufficient.

Controlling crosstalk on a general purpose digital circuit board is usually not too difficult. Be sure not to route outputs next to inputs, especially if the inputs are to be used when the outputs are switching. This will prevent the sharp transition of the output from coupling onto the input line at just the wrong time. Of course, it is impossible to route the board without getting inputs and outputs close together somewhere; just try to avoid long lines where the coupling might be worse.

One final note about general-purpose digital circuitry involves crystal oscillators. Most microcontrollers use a crystal oscillator as a timing reference. The crystal is used in a positive feedback loop around an amplifier in the microcontroller. The positive feedback makes the amplifier unstable, so it oscillates. If everything goes right, the amplifier oscillates at exactly the frequency of the crystal. Who cares, you ask? Well, you do! If you are faced with a board design containing a crystal oscillator, you must be careful both with placement and with routing. Most crystal circuits require a small capacitor (typically a 15-pF ceramic) to ground on each side of the crystal. In addition, some circuits have a resistor in series with the feedback loop. To insure that your oscillator will work, place it first (right after the microcontroller). Try to place the crystal and resistor in a small loop, right next to the pins of the microcontroller. Place the startup capacitors close by. Route the board with the shortest routes possible, and make sure the ground connections on the capacitors are very short. See Figure 3-1 for a correctly placed and routed crystal oscillator. Notice how X1 (the crystal) is in a small loop of traces starting and ending at U1 (the microcontroller). R2 (the series resistor) is in the loop, while C1 and C2 (startup capacitors) are connected from the two loop nodes to a ground plane (not shown). Notice how the parts are placed as close together as possible, and how the traces form a small, tight loop.

Placement and Routing Considerations for High-performance Analog Circuit Boards

“High-performance” analog circuit boards contain analog circuitry that is either higher in bandwidth (like video circuitry), higher in gain (like sensor amplifiers), lower in noise, or have larger dynamic range (like A/D and D/A converters) than a general-purpose analog circuit board. No matter what type of circuitry is on your board, there are a few useful techniques for placing and routing high-end analog circuitry. By this point, it should go without saying that good grounding, power distribution, and decoupling techniques must be used.

The active devices (op amps and transistors) on a high-performance board tend to have both more gain and operate at higher frequencies. This can yield significant problems if a few guidelines are not followed:

In addition to these guidelines, the performance of analog circuitry can be improved by a technique called ground rings. A ground ring is used to isolate a section of circuitry from the rest of the board. It is most useful for high-end op amps. See Figure 3-2 for an example of a ground ring. See how the ground ring surrounds the sensitive input pins of the amplifier. It connects both to the ground pins of the amplifier and to the ground plane of the board (not shown). Ground rings should be used on low noise or high impedance points in the circuit.

Another important routing technique involves differential signals. These signals are often used to improve a system’s dynamic range and noise immunity. A differential analog signal is actually a pair of signal lines with opposite DC values. In a typical differential signal application, a pair of differential signal lines is used to move a signal from a driver to a receiver. Note that these parts can be quite a distance from one another. The differential driver (usually built from an op amp) drives each signal line in opposite directions. At the other end, the differential receiver (also usually an op amp) subtracts the two signal lines from each other to produce the output signal. When routing these types of signals, it is important that the two lines be routed completely parallel and close to each other. The reason for this is so that any external noise will be coupled equally onto each line, and thus subtracted out at the receiver. This is one of the only times when long parallel routes can actually work to your advantage.

Placement and Routing Considerations for High-speed Digital Circuit Boards

This type of board has digital circuitry that runs above 20 MHz. Common components in this type of design include microprocessors or digital signal processors, static or dynamic RAM, flash memory, high-speed programmable logic, and complex mixed signal processors. There is often critical timing in the design, where signals must arrive within one nanosecond (ns) of each other. These designs also usually have large (more than eight bits) address and/or data busses which must be connected between chips.

The high-speed operation of these large busses creates tremendous electrical noise. When 16 or 32 CMOS lines change state simultaneously, a large amount of energy is required from the power supply. The supply cannot provide the power fast enough, because of the inherent inductance in even the best-designed distribution system. For this reason, power supply decoupling is even more important. Every pin which connects to the power supply must have a decoupling capacitor (0.1 μF ceramic is typical). This means that, for a microprocessor or DSP chip, there may be as many as 20 decouplers! In addition to the 0.1 μF decouplers on each power pin, you should provide a “bulk” decoupling capacitor for each large digital device. This is usually a larger capacitance (10 μF tantalum is typical) to provide an energy store for this hungry digital chip!

Be careful when you route the decoupling capacitors. In order to prevent the noisy chip from corrupting your power supply, you must make sure that the capacitor is located between the chip and the supply. Figure 3-3 shows a poorly placed and routed decoupling capacitor, while Figure 3-4 shows a correct decoupling design.

In both Figure 3-3 and Figure 3-4, U1 is the active device. It connects to the power supply on pin 14, and the power is provided by connector BT1. C1 is the decoupling capacitor. Notice how in Figure 3-3 the power flows in from BT1 directly into U1, while C1 is way off to the right. In fact, as far as high-frequency noise is concerned, C1 is effectively out of the circuit. The long trace length between U1 pin 14 and C1 will contribute enough stray (parasitic) inductance such that the effective value of C1 is greatly reduced. Now consider the circuit in Figure 3-4. In this case, the power must flow in from BT1, through the input pin of C1, and into U1 pin 14. In this case, C1 will effectively decouple any high frequency noise produced by U1. Note that the idea here still applies no matter how the power is applied to the active devices. In the examples, I used connector BT1, but you might use a trace, or a via, from a backside or inner power layer. No matter how the power gets to the chip, it should have to go through the decoupling capacitor and from there through a short trace directly to the device power pin. You cannot decouple a circuit board too well.

When routing the high-speed digital circuit board, keep all routes as short as possible. If the route lengths get too long, the fast logic transitions may cause signals to bounce back and forth up and down the route, causing ringing on the desired signal. This ringing is also called a transmission line effect. The signal ringing can be reduced by terminating the routes with a resistor. A shunt termination is often used. This is usually a “pullup” (to the power supply) or a “pulldown” (to ground) resistor of approximately 10 kilohms. The shunt termination is placed at the destination of the route. Keep in mind that the shunt termination will dissipate power and load the logic gate that is driving the line.

In some cases, a shunt termination may not be enough to reduce the ringing to acceptable levels. This is often true of high-speed clock lines. In these cases a series termination will usually reduce transmission line effects to tolerable levels. The series termination is usually a small resistor (150 Ω typically) placed at the source of the signal.

High-speed digital clocks are among the most difficult signals to route. A common problem is how to distribute a clock from some type of source (an oscillator or gate output) to several different inputs across the board. There are basically two ways to do this: a “starburst” or a “daisy-chain” route. The starburst route places the clock source in the center of a “star,” with each clock load at the end of a route. The problem here is that each arm of the star is a transmission line. If these lines aren’t terminated correctly, the reflections and ringing will all combine at the center of the star, and can ruin the clock signal. If you do terminate each end of the star, the clock source may not have enough power to drive all of the terminations.

The other solution is to route the clock signal in a daisy chain. This is a single, long route from the source, through each load one by one. The line should be terminated at the end to avoid ringing. This is a more difficult way to route the clock, but will often give superior results.

Placement and Routing Considerations for RF Circuit Boards

Radio frequency (RF) circuit boards are generally considered the most difficult boards to place and route. This is due to the characteristics of the circuits and signals found in typical radio designs. Signals on an RF board range in frequency from zero (DC) to tens of gigahertz (10,000,000,000 cycles per second!). In addition, the amplitude (size) of the signals ranges from tens of nanovolts (0.00000001 volt) to tens of volts. Circuits commonly used in RF designs often have very high impedance. This, combined with the high gain commonly found in radio designs (a gain of 100 dB, which is ten billion, is not unusual!), greatly increases the circuits’ susceptibility to interference or pickup. Finally, the component values used in RF circuits are often very small. Capacitors as small as 0.1 pF (0.0000000000001 farad) and inductors as small as 10 nH (0.00000001 henry) are commonly used. All of these factors combine to make an RF circuit board a true placement and routing challenge. A good RF board designer must keep each of these difficulties in mind as he or she places and routes the board. Note that I said “he or she,” not “it.” There is no place for automatic placement or routing software in the design of RF circuit boards. If you think you will save time by using these tools, then think again. You will only force yourself to completely redo the board (by hand) after it doesn’t work!

Special RF Routing Techniques: Microstrip

When routing high-frequency RF signals, the traces themselves become an important part of the circuit. Remember the high-speed digital circuit boards discussed above? The traces on those boards are sometimes called transmission lines, because of the reflections that happen at their ends. The solution there was to terminate the lines with resistors to try to reduce or eliminate these reflections. A different solution is often used on RF transmission lines: the lines themselves are designed to match the terminating impedance inherent in the RF circuitry. Two ways to achieve this are with the use of microstrip or stripline. These are types of controlled-impedance traces. They are easy to design and build, even for the home hobbyist. We will discuss microstrip first and then stripline in the next section.

Which RF traces should be treated as transmission lines? In general, all high frequency or long traces should be considered transmission lines. But how high is high or how long is long? A rule of thumb to use is that any trace that is longer than 1/16 of a wavelength will act as a transmission line. To compute a signal’s wavelength, use the formula:

where λ is the wavelength (in inches) and F is the signal’s frequency (in MHz). This equation includes an approximation to account for the fact that your signal will travel slightly slower on a circuit board than it would in free space.

For example, a 915-MHz signal has a wavelength of about twelve inches, so a transmission line would be any trace longer than about 0.8 inch. Note that this doesn’t mean that you should carefully route a two-inch trace as a transmission line while carelessly routing a 0.7-inch trace. Once you have one controlled impedance transmission line on your board, it is just as easy to make all of your RF traces into transmission lines. See Table 3-1 for a list of frequencies, wavelengths, and transmission line lengths. The table also includes the length of a quarter-wave dipole antenna for each frequency. A quarter-wave dipole is a very common type of antenna; it consists of a quarter-wave conductor mounted over a ground plane. You can see that, at high frequencies, circuit board traces can easily become efficient antennas!

Once you have identified which traces on your board are to be treated as transmission lines, then it is time to decide on the type of transmission line to use. There are many different types to choose from. You are already very familiar with the most common type of transmission line, the coaxial cable. It certainly works well, as millions of cable TV viewer will attest to. Unfortunately, coaxial transmission lines are difficult to fabricate on circuit boards. As previously noted, the two most common types of transmission line used on circuit boards are microstrip and stripline.

Microstrip is the most common type of transmission line. It simply consists of a copper trace of a known width a certain distance above an infinite ground plane. A dielectric (insulating) material is between the trace and the ground plane, and nothing is above the trace. Figure 3-6 shows a cross-section drawing of a microstrip.

Note that any trace on a printed circuit board can be viewed as a microstrip. In fact, all circuit board traces are microstrips, but only some are designed that way. The complete analysis of a microstrip is a bit complex but a few approximations will help. The first approximation is that the ground plane is finite in size, since it cannot really be infinite, but it must be much larger in all directions than the transmission line. Another approximation concerns the free space above the trace. Most circuit boards are used in an enclosure of some type; if a microstrip is used on the circuit board then any metal cover must be kept far above the traces. This will keep the electric field lines above the microstrip from becoming distorted by the presence of a cover.

These approximations allow one to write a simple formula for the characteristic impedance of the microstrip. This equation is:

where w is the width of the microstrip trace (in mils, which are 0.001 of an inch), d is the distance to the ground plane (again, in mils), t is the thickness of the trace (in mils) and _r is the relative dielectric constant of the dielectric material used in the circuit board. The result is Z₀, which is the characteristic impedance of the transmission line in ohms. The term characteristic impedance is simply a way of describing the effects the transmission line will have on the signals it carries. For the purposes of nearly all circuit boards, your goal as a board designer is to produce transmission lines of a known characteristic impedance. This will allow the circuit board to “match” to the components on it, resulting in a minimum of transmission line reflections.

What is the dielectric constant (_r), you ask? It is a material property of the circuit board you have chosen to use, and it is usually outside of the board designer’s control. Nearly all (99%) of circuit boards are built on “FR-4” woven fiberglass circuit boards, including the ones used in this manual. Exotic high frequency, high power, or low-loss circuit boards are sometimes built on more advanced (and much more expensive) materials. Table 3-2 lists material properties for common circuit board materials. Air is listed for reference only (it’s very hard to build circuit boards in air!).

In addition to dielectric constant, the loss tangent is also given for each circuit board type. This is related to the loss an RF signal will experience when it passes through circuit boards made with each dielectric. A lower loss tangent means less loss. Notice how the least expensive material (FR-4) has the highest loss tangent, while the more exotic materials have lower loss tangents.

The process of computing the loss on a transmission line from the loss tangent is even more complex than the computations for characteristic impedance, as it involves the frequency of the signal. Table 3-3 lists a few representative losses of different types of microstrip traces. Notice how the microstrip width is the same for any signal frequency; only the RF loss rate changes with frequency.

You can see that the RF loss of FR-4 greatly increases at signal frequencies above 1000 MHz. The advanced materials are used exclusively for these high frequencies.

The RF loss rate is specified in units of decibels per inch (dB/inch). To compute the actual loss of a stripline, multiply the loss rate by the length of the microstrip. While these losses may seem small, remember that a total loss of only 3 decibels (dB) means that half an RF signal’s power is lost in the microstrip, and only the remaining half may be delivered to the load.

Once you have determined what board material and dielectric thickness you are going to use, it is time to compute the microstrip line width to use to design a microstrip of a given characteristic impedance. The impedance you are shooting for will nearly always be 50OΩ this has become the industry standard for RF controlled impedance circuitry. The only significant exception would be for cable television (CATV) designs, which are typically 75Ω. If you re-arrange the formula given above to solve for the microstrip line width, you get:

where w is the microstrip width (in mils), d is the dielectric thickness (in mils), t is the trace thickness (in mils), _r. is the dielectric constant, and Z₀ is the desired characteristic impedance. Table 3-4 lists microstrip line widths for the most common applications likely to be used. Note that a few mils of error on your board will not dramatically shift the impedance; a ten percent tolerance on characteristic impedance is usually “close enough.”

There are a few last details to discuss about microstrips. In addition to the approximations discussed above (infinite ground and nothing above the line), there are two design guidelines to keep in mind. The first is to keep other traces, either on the same or other layers, as far from the microstrip as possible. A good rule of thumb is to keep all other traces and vias at least five line widths from the microstrip. This will not always be possible, but it is a good goal. Another design guideline is to try to make all of your RF traces into microstrips. This can be as easy as setting your default routing width to your desired microstrip width. In this way, every RF trace you route (no matter how short) will automatically have the proper impedance.

Note that all of the transmission line calculations and tables given in this manual are approximations. When you have an RF circuit board manufactured professionally, be sure to ask for and follow the recommendations of the fabrication house. They should be able to provide you with recommended microstrip width and dielectric thickness for transmission lines of a given characteristic impedance. These recommendations will take into account all of the details of their fabrication process, and should almost always result in properly designed transmission lines. Note also that you, as the board designer, can request the fabrication house to test the impedance of their boards. These tests are usually performed with a TDR (time-domain reflectometer), an instrument which measures reflections on transmission lines. The usual procedure is that the fabrication house will design a test coupon that is built along with your circuit board. The test coupon will allow the fabrication house to quickly and easily measure the characteristic impedance of the microstrips on your board.

Special RF Routing Techniques: Stripline

Stripline is another type of transmission line that can be easily built on a circuit board. It is identical to microstrip, but with ground planes both above and below the trace. Figure 3-7 shows a cross-sectional diagram of stripline. Stripline offers much improved isolation over microstrip, but at the cost of increased RF loss. Striplines are most often used for either high- or low-level RF signals requiring isolation from surrounding circuitry.

As with microstrip, several simplifying approximations allow one to write a simple formula for the characteristic impedance of the stripline. This equation is:

where w is the width of the stripline trace (in mils, which are 0.001 of an inch), t is the thickness of the trace (in mils), d is the total distance between ground planes (again, in mils), and _r is the dielectric constant of the dielectric material used in the circuit board.

Once again, this equation can be re-written to solve for the stripline width, given a desired characteristic impedance:

Striplines behave identically to microstrip, but with the added benefit that the RF signal is surrounded top and bottom by ground. The ground planes provide a high degree of isolation, so external signals are less likely to interfere with the RF signal on the stripline. The reverse is also true; RF signals on the stripline will radiate much less energy due to the shielding effect of the ground planes. The downside to stripline is increased RF loss. This is due to the fact that the dielectric (insulating) material is now on both sides of the trace, and tends to absorb more of the RF. Table 3-5 lists stripline widths and decibel loss rates for a few stripline designs.

Table 3-6 lists stripline line widths for the most common applications. As with microstrips, you should discuss your stripline requirement with your fabrication house for the most accurate line width to use for a given characteristic impedance.

Striplines are most easily constructed on the inner layers of multi-layer printed circuit boards. If you are making a multi-layer board, then building a stripline layer is easy. First define two ground layers (one on either side of your stripline layer), and then define your stripline layer in the middle. Remember to set the default routing width on the stripline layer to the stripline’s design width. You will have to use vias or through-hole device pins to connect to and from the stripline layer.

Note that the stripline layer can also be used to route other (non-stripline) signals. Just remember to keep all signals far from the striplines. In fact, it is best to place copper (ground) areas around your striplines, right on the stripline layer. This will enclose the RF trace in ground on all sides, and will provide the highest degree of isolation available. The resultant stripline trace is very similar to a coaxial cable, with the signal in the center, completely surrounded by ground. Remember when placing the ground areas to keep them at least five line widths away from the stripline. Use plated-through vias to “tie” the ground areas to the ground planes above and below the stripline layer. Figure 3-8 shows an example stripline layer with ground isolation around each stripline. Notice in the figure how the RF striplines are completely protected by ground areas which are kept far from the stripline trace. Also note that there are other ground areas which are around non-RF traces. These ground areas are allowed to come much closer to the traces, because they are not controlled impedance transmission lines. The circles represent vias, in which signals are crossing through this layer from other layers.

Just because you are building your own two-layer circuit boards does not mean that you cannot use striplines. Simply etch the stripline onto one side of a board, with a ground plane on the other side. Then use another single-sided board (of the same thickness) as the ground plane for the other side of the stripline. Place the two boards together, with the stripline traces touching the empty (non-copper) side of the single-sided board. Drill many holes through the boards in the ground areas (don’t drill through your striplines!), and then use press-in vias or small wires to solder the two ground planes together. Finally, wrap copper tape around the outer edges of the circuit board and solder the tape to both ground planes. Now you’ve made your own stripline circuit board!