PCB Blog - Three special routing techniques in PCB board design and wiring

The quality of PCB boarddesign and wiring will directly affect the performance of the entire system, and most high-speed design theories will eventually be realized and verified through Layout. It can be seen that wiring is very important in high-speed PCB design. The following will analyze the rationality of some situations that may be encountered in actual wiring, and give some optimized routing strategies. It is mainly explained from three aspects: right-angle routing, differential routing, and serpentine routing.

1. Right angle trace
Right-angle wiring is generally a situation that needs to be avoided as much as possible in PCB wiring, and it has almost become one of the standards for measuring the quality of wiring. So how much impact does right-angle wiring have on signal transmission? In principle, right-angle traces will change the line width of the transmission line, resulting in discontinuities in impedance. In fact, not only right-angle traces, but also sharp-angle traces may cause impedance changes.
The impact of the right-angle trace on the signal is mainly reflected in three aspects:
(1) The corner can be equivalent to a capacitive load on the transmission line to slow down the rise time;
(2) Impedance discontinuity will cause signal reflection;
(3) EMI generated at right angles.
The parasitic capacitance caused by the right angle of the transmission line can be calculated by the following empirical formula:
C=61W(Er)1/2/Z0, in the above formula, C refers to the equivalent capacitance of the corner (unit: pF), W refers to the width of the trace (unit: inch), εr refers to the dielectric constant of the medium, Z0 is the characteristic impedance of the transmission line. For example, for a 4Mils 50 ohm transmission line (εr is 4.3), the capacitance brought by a right angle is about 0.0101pF, and the resulting rise time change can be estimated: T10-90%=2.2* C*Z0/2 = 2.2*0.0101*50/2 = 0.556ps. It can be seen from the calculation that the capacitive effect caused by the right-angle trace is extremely small. As the line width of the right-angle trace increases, the impedance there will decrease, so a certain signal reflection phenomenon will occur. We can calculate the equivalent impedance after the line width is increased according to the impedance calculation formula mentioned in the transmission line chapter, and then Calculate the reflection coefficient according to the empirical formula: ρ=(Zs-Z0)/(Zs+Z0). Generally, the impedance change caused by right-angle wiring is between 7% and 20%, so the reflection coefficient is about 0.1. Moreover, as can be seen from the figure below, the impedance of the transmission line changes to 100% during the W/2 line, and then returns to the normal impedance after the W/2 time. The entire impedance change occurs in a very short time, often within 10ps., such a fast and small change is almost negligible for general signal transmission. Many people have such an understanding of right-angle wiring, thinking that it is easy to emit or receive electromagnetic waves and generate EMI, which is also one of the reasons why many people think that right-angle wiring is not possible. However, the results of many practical tests show that right-angle traces do not produce significant EMI than straight lines. Perhaps the current instrument performance and test level restrict the testability, but at least it shows a problem, the radiation of right-angle traces is already smaller than the measurement error of the instrument itself. In general, right-angle routing is not as scary as you might imagine. At least in applications below GHz, any effects such as capacitance, reflection, EMI, etc. produced by it are hardly reflected in TDR testing. The focus of high-speed PCB board design engineers should still be on layout, power/ground design, and trace design., vias and other aspects. Of course, although the impact of right-angle wiring is not very serious, it does not mean that we can all walk right-angle lines in the future. Attention to details is a basic quality that every engineer must have. Moreover, with the rapid development of digital circuits, PCB boards The frequency of the signals that engineers deal with will continue to increase, and in the field of RF design above 10GHz, these small right angles may become the focus of high-speed problems.

2. Differential trace
Differential signals are more and more widely used in high-speed circuit board design. The key signals in the circuit are often designed with differential structure. Why is it so popular? How to ensure its good performance in PCB board design? With these two questions, we proceed to the next part of the discussion. What is differential signaling? In layman's terms, the driving end sends two signals of equal value and opposite phase, and the receiving end judges the logical state "0" or "1" by comparing the difference between the two voltages. The pair of traces that carry the differential signal is called a differential trace.

Compared with ordinary single-ended signal traces, differential signals have obvious advantages in the following three aspects:
a. Strong anti-interference ability, because the coupling between the two differential traces is very good. When there is noise interference in the outside world, they are almost coupled to the two wires at the same time, and the receiving end only cares about the difference between the two signals. So the external common mode noise can be completely canceled.
b. It can effectively suppress EMI. In the same way, because the polarities of the two signals are opposite, the electromagnetic fields radiated by them can cancel each other. The tighter the coupling, the less electromagnetic energy is released to the outside world.
c. Timing positioning, because the switching change of the differential signal is located at the intersection of the two signals, unlike ordinary single-ended signals that rely on two threshold voltages, high and low, so it is less affected by process and temperature, and can reduce timing errors. It is also more suitable for circuits with low amplitude signals. The current popular LVDS refers to this small-amplitude differential signaling technology. For PCB board engineers, the concern is how to ensure that these advantages of differential routing can be fully utilized in actual routing. Maybe anyone who has been in contact with stackup will understand the general requirement for differential traces, which is "equal length, equal spacing". Equal length is to ensure that the two differential signals maintain opposite polarities at all times and reduce common mode components; equal distance is mainly to ensure that the differential impedance of the two is consistent and reduce reflection. The "as close as possible principle" is sometimes one of the requirements for differential routing. But all of these rules are not meant to be rhetorical, and many engineers don't seem to understand the nature of high-speed differential signaling. The following focuses on several common misunderstandings in PCB differential signal design.

Misunderstanding 1: Think that the differential signal does not need a ground plane as a return path, or think that the differential traces provide a return path for each other. This misunderstanding is caused by being confused by superficial phenomena, or the understanding of the mechanism of high-speed signal transmission is not deep enough. It can be seen from the structure of the receiving end that the emitter currents of the transistors Q3 and Q4 are equal and opposite, and their currents at the ground just cancel each other (I1=0), so the differential circuit is suitable for similar bounces and other possible existences. It is insensitive to noise signals on the power and ground planes. The partial return cancellation of the ground plane does not mean that the differential circuit does not use the reference plane as the signal return path. In fact, in the analysis of signal return, the mechanism of differential routing and ordinary single-ended routing is the same, that is, high-frequency signals are always The difference between the return flow along the loop of the inductor is that in addition to the coupling to the ground, the differential line also has mutual coupling. Whichever coupling is strong will become the main return path.
In PCB circuit design, the coupling between differential traces is generally small, often only accounting for 10~20% of the coupling degree, and more is the coupling to the ground, so the main return path of the differential trace still exists in the ground. flat. When the ground plane is discontinuous, the coupling between the differential traces in the area without the reference plane will provide the main return path. Although the discontinuity of the reference plane does not affect the differential trace as seriously as the ordinary single-ended trace, it will still reduce the quality of the differential signal and increase the EMI, which should be avoided as much as possible. Some designers also believe that the reference plane under the differential trace can be removed to suppress some common-mode signals in differential transmission, but this approach is theoretically undesirable. How to control the impedance? Not providing a ground impedance loop for the common mode signal will inevitably cause EMI radiation, which does more harm than good.

Myth 2: Thinking that maintaining equal spacing is more important than matching line lengths. In the actual PCB board layout, it is often impossible to meet the requirements of differential design at the same time. Due to factors such as pin distribution, vias, and routing space, the purpose of matching the line length must be achieved through appropriate routing, but the result must be that some areas of the differential pair cannot be parallel. What should we do at this time? What about trade-offs? Before drawing conclusions, let's take a look at the following simulation results. From the above simulation results, the waveforms of scheme 1 and scheme 2 are almost coincident, that is to say, the impact caused by the unequal spacing is minimal. In comparison, the impact of line length mismatch on the timing is much greater (Option 3). From the theoretical analysis, although the inconsistency of the spacing will cause the differential impedance to change, because the coupling between the differential pairs itself is not significant, the impedance variation range is also very small, usually within 10%, which is only equivalent to a single pass. reflections caused by holes, which do not significantly affect signal transmission. Once the line length does not match, in addition to the timing offset, a common mode component is introduced into the differential signal, which reduces the quality of the signal and increases EMI. It can be said that the important rule in the design of differential traces on the PCB is to match the length of the lines, and other rules can be flexibly handled according to the design requirements and practical applications.

Misunderstanding 3: Thinking that the differential traces must be very close. Keeping the differential traces close is nothing more than to enhance their coupling, which can not only improve immunity to noise, but also make full use of the opposite polarity of the magnetic field to offset electromagnetic interference to the outside world. Although this approach is very beneficial in most cases, it is not. If we can ensure that they are fully shielded from external interference, then we do not need to achieve anti-interference and anti-interference through strong coupling with each other. the purpose of suppressing EMI. How can we ensure that the differential traces have good isolation and shielding? Increasing the distance with other signal traces is one of the basic ways. The energy of the electromagnetic field decreases with the square relationship of the distance. Generally, when the distance between the lines exceeds 4 times the line width, the interference between them is extremely weak, which is basically OK. neglect. In addition, the isolation of the ground plane can also play a good shielding role. This structure is often used in the design of high-frequency (above 10G) IC package PCB boards. It is called the CPW structure, which can ensure strict differential Impedance Control (2Z0). Differential traces can also be run in different signal layers, but this method is generally not recommended, because the differences in impedance and vias generated by different layers will destroy the effect of differential mode transmission and introduce common mode noise. In addition, if the two adjacent layers are not tightly coupled, it will reduce the ability of the differential trace to resist noise, but if the proper spacing from the surrounding traces can be maintained, crosstalk is not a problem. At general frequencies (below GHz), EMI is not a serious problem. Experiments show that the radiated energy attenuation at a distance of 3 meters has reached 60dB for differential traces separated by 500Mils, which is enough to meet the FCC's electromagnetic radiation standards, so The designer does not have to worry too much about the electromagnetic incompatibility caused by insufficient differential line coupling.

3. serpentine
Serpentine line is a type of routing method often used in Layout. Its main purpose is to adjust the delay to meet the system timing design requirements. The designer must first have this understanding: the serpentine line will destroy the signal quality, change the transmission delay, and try to avoid using it when wiring. However, in actual design, in order to ensure that the signal has sufficient holding time, or to reduce the time offset between the signals in the same group, it is often necessary to deliberately perform wiring. So, what effect does the serpentine wire have on signal transmission? What should I pay attention to when routing? The two key parameters are the parallel coupling length and the coupling distance. Obviously, when the signal is transmitted on the serpentine trace, coupling will occur between the parallel line segments, in the form of differential mode, the smaller the S, the larger the Lp, the greater the coupling degree. It may lead to the reduction of transmission delay and greatly reduce the quality of the signal due to crosstalk. For the mechanism, please refer to the analysis of common mode and differential mode crosstalk in Chapter 3.

A few tips when dealing with serpentine lines:
(1) Try to increase the distance of parallel line segments, at least greater than 3H, where H refers to the distance from the signal trace to the reference plane. In layman's terms, it is to route around a big bend. As long as S is large enough, the mutual coupling effect can be almost completely avoided.
(2) Decrease the coupling length Lp. When the double Lp delay approaches or exceeds the signal rise time, the generated crosstalk will reach saturation.
(3) The signal transmission delay caused by the serpentine line of the strip line or the buried microstrip line is smaller than that of the microstrip line. Theoretically, the stripline will not affect the transmission rate due to differential mode crosstalk.
(4) For high-speed and signal lines with strict timing requirements, try not to take serpentine lines, especially do not meander in a small area.
(5) Serpentine traces with any angle can often be used, which can effectively reduce mutual coupling.
(6) In the design of high-speed PCB board, the serpentine line has no so-called filtering or anti-interference ability, which can only reduce the signal quality, so it is only used for timing matching and no other purposes.
(7) Sometimes the spiral routing method can be considered for winding. The simulation shows that the effect is better than the normal PCB boarddesign serpentine routing.