How do RF circuits and digital circuits work in harmony on the same PCB?

- Dec 04, 2019-

How do RF circuits and digital circuits work in harmony on the same PCB?

Summary of content: The single-chip RF device greatly facilitates the application in the wireless communication field in a certain range. A complete wireless communication link can be formed by using a suitable microcontroller and antenna and combining this transceiver device. They can be integrated on a small circuit board and used in many fields such as wireless digital audio, digital video data transmission systems, wireless remote control and telemetry systems, wireless data acquisition systems, wireless networks, and wireless security systems.

1 Potential contradictions between digital circuits and analog circuits

If the analog circuit (RF) and the digital circuit (microcontroller) work separately, they may work well, but once the two are placed on the same circuit board and run on the same power supply, the entire system is likely to be unstable. . This is mainly because the digital signal swings frequently between the ground and the positive power supply (3V in size), and the period is particularly short, often ns level. Due to the large amplitude and small switching time, these digital signals contain a large number of high-frequency components that are independent of the switching frequency. In the analog part, the signal transmitted from the antenna tuning loop to the wireless device receiving part is generally less than 1 μV. Therefore, the difference between digital signals and RF signals will reach 10-6 (120dB). Obviously, if the digital signal and the RF signal cannot be separated well, the weak RF signal may be damaged. In this way, the working performance of the wireless device will be deteriorated, or even it will not work at all.

2 Frequently Asked Questions of RF Circuit and Digital Circuit on the Same PCB

It is a common problem to fail to fully isolate sensitive and noisy signal lines. As mentioned above, digital signals have high swings and contain a lot of high-frequency harmonics. If the digital signal routing on the PCB is close to sensitive analog signals, high frequency harmonics may be coupled in. The most sensitive nodes of RF devices are usually phase-locked loop (PLL) loop filter circuits, external voltage-controlled oscillator (VCO) inductors, crystal reference signals, and antenna terminals. These parts of the circuit should be handled with special care.

(1) Power supply noise

Because the input / output signal has a swing of several V, digital circuits are generally acceptable for power supply noise (less than 50mV). However, analog circuits are quite sensitive to power supply noise, especially to glitch voltages and other high-frequency harmonics. Therefore, the routing of power lines on PCBs containing RF (or other analog) circuits must be done more carefully than on ordinary digital circuit boards, and automatic routing should be avoided. It should also be noted that the microcontroller (or other digital circuit) will suddenly draw most of the current within a short period of time within each internal clock cycle. This is because modern microcontrollers are designed using CMOS processes. Therefore, assuming that a microcontroller is running at an internal clock frequency of 1 MHz, it will draw (pulse) current from the power source at this frequency. Without proper power supply decoupling, it will inevitably cause voltage glitches on the power supply line. If these voltage glitches reach the power pin of the RF part of the circuit, it may seriously cause work failure, so it must be ensured that the analog power line is separated from the digital circuit area.

(2) Unreasonable ground

The RF circuit board should always have a ground layer connected to the negative pole of the power supply. If it is not handled properly, some strange phenomena may occur. This may be difficult for a digital circuit designer to understand because most digital circuit functions perform well even without a ground plane. In the RF band, even a very short wire acts as an inductor. Roughly calculated, the inductance per mm length is about 1nH, and the inductive reactance of a 10mm PCB line at 434MHz is about 27Ω. Without a ground plane, most ground wires will be longer and the circuit will not guarantee the design characteristics.

(3) Radiation of antenna to other analog parts

This is often overlooked in circuits that include radio frequency and other parts. In addition to the RF part, there are usually other analog circuits on the board. For example, many microcontrollers have built-in analog-to-digital converters (ADCs) for measuring analog inputs as well as battery voltage or other parameters. If the RF transmitter's antenna is located near this PCB (or just on this PCB), the high-frequency signal emitted may reach the analog input of the ADC. Don't forget that any circuit line can send or receive RF signals like an antenna. If the input of the ADC is not processed properly, the RF signal may self-excite in the ESD diode of the ADC input, which may cause ADC deviation.

3 RF and digital circuit solutions on the same PCB

Here are some common design and wiring strategies in most RF applications. However, it is more important to follow the RF device layout recommendations for practical applications.

(1) A reliable ground plane

When designing a PCB with RF components, a reliable ground plane should always be used. The purpose is to establish a valid 0V potential point in the circuit, so that all devices are easily decoupled. The 0V terminal of the power supply should be connected directly to this ground plane. Due to the low impedance of the ground plane, no signal coupling will occur between the two nodes that have been decoupled. It is very important for the amplitude of multiple signals on the board to differ by 120dB. On a surface mount PCB, all signals are routed on the same side of the component mounting surface, while the ground plane is on the opposite side. The ideal ground plane should cover the entire PCB (except under the antenna PCB). If more than two layers of PCB are used, the ground layer should be placed on the layer adjacent to the signal layer (such as the next layer on the component side). Another good method is to fill the remaining part of the signal wiring layer with the ground plane. These ground planes must be connected to the main ground plane through multiple vias. It should be noted that the existence of the ground point will cause the inductance characteristics nearby to change, so the selection of the inductance value and the layout of the inductance must be carefully considered.

(2) shorten the connection distance with the ground layer

All connections to the ground plane must be as short as possible, and ground vias should be placed at (or very close to) the component pads. Never allow two ground signals to share a ground via. This may cause crosstalk between the two pads due to the via connection impedance.

(3) RF decoupling

Decoupling capacitors should be placed as close to the pins as possible, and capacitors should be used for each pin that needs to be decoupled. Using high-quality ceramic capacitors, the dielectric type is preferably "NPO", and "X7R" also works well in most applications. Ideally, the capacitor value should be chosen such that its series resonance is equal to the signal frequency. For example, at 434MHz, the 100pF capacitor mounted by SMD will work well. At this frequency, the capacitive reactance of the capacitor is about 4Ω, and the inductive reactance of the via is also in the same range. The capacitors and vias in series form a notch filter for the signal frequency, enabling it to be effectively decoupled. At 868MHz, a 33pF capacitor is an ideal choice. In addition to RF decoupling of small value capacitors, a large value capacitor should also be placed on the power line to decouple low frequencies. A 2.2μF ceramic or 10μF tantalum capacitor can be selected.

(4) Star wiring of power supply

Star wiring is a well-known technique in analog circuit design (see Figure 1). Star wiring-each module on the circuit board has its own power line from a common power supply point. In this case, the star wiring means that the digital part and the RF part of the circuit should have their own power lines, and these power lines should be decoupled separately near the IC. This is an effective way to isolate the power supply noise from the digital section and from the RF section. If the module with severe noise is placed on the same circuit board, an inductor (bead) or a small resistance (10Ω) can be connected in series between the power line and the module, and a tantalum capacitor of at least 10 μF must be used for these modules. Power supply decoupling. Such modules are RS 232 drivers or switching power regulators.

image 

(5) Reasonably arrange PCB layout

In order to reduce interference from noise modules and surrounding analog parts, the layout of each circuit module on the board is important. Always keep sensitive modules (RF part   and antenna) away from noisy modules (microcontroller and RS 232 driver) to avoid interference.

(6) the effect of shielding RF signal on other analog parts

As mentioned above, the RF signal will cause interference to other sensitive analog circuit modules such as ADCs when transmitting. Most problems occur in lower operating frequency bands (such as 27MHz) and high power output levels. It is a good design practice to use RF decoupling capacitors (100pF) to ground to decouple sensitive points.

(7) Special considerations on plate loop antennas

The antenna can be made on the PCB as a whole. Compared with the traditional whip antenna, it not only saves space and production costs, it is also more stable and reliable. Traditionally, loop antenna designs have been applied to relatively narrow bandwidths, which helps to suppress unwanted strong signals so as not to interfere with the receiver. It should be noted that loop antennas (like all other antennas) may receive noise capacitively coupled by nearby noisy signal lines. It can interfere with the receiver and may also affect the modulation of the transmitter. Therefore, do not run digital signal lines near the antenna, and it is recommended to maintain free space around the antenna. Any object close to the antenna will form part of the tuning network, which will cause the antenna tuning to deviate from the expected frequency point, which will reduce the transmission and reception radiation range (distance). This fact must be noted for all types of antennas, and the housing of the circuit board (outer packaging) may also affect antenna tuning. At the same time, it is necessary to remove the ground plane at the antenna area, otherwise the antenna cannot work effectively.

(8) Connection of circuit board

If the RF circuit board is connected to an external digital circuit with a cable, a twisted pair cable should be used. Each signal line must be twisted with the GND line (DIN / GND, DOUT / GND, CS / GND, PWR_UP / GND). Remember to connect the RF circuit board and the digital application circuit board with the GND wire of the twisted pair cable, and the cable length should be as short as possible. The lines that power the RF board must also be twisted with GND (VDD / GND).

    4 Conclusion

The rapid development of radio frequency integrated circuits provides engineers and technicians engaged in the design of wireless digital audio and video data transmission systems, wireless remote control, telemetry systems, wireless data acquisition systems, wireless networks, and wireless security systems to solve the bottlenecks of wireless applications. may. At the same time, the design of RF circuits requires designers to have certain practical experience and engineering design capabilities. This article is the author's experience in actual development. I hope that it can help many RF IC developers to shorten the development cycle, avoid unnecessary detours, and save manpower and financial resources.


Previous:Features of PCB board micro-hole mechanical drilling Next:No PCB, no electronics, a little advice for electronics beginners