Several rules for power supply design of RF circuits

Aguilera

Several rules for power supply design of RF circuits [Copy link]

(1) The power line is an important way for EMI to enter and exit the circuit. Through the power line, external interference can be transmitted to the internal circuit and affect the RF circuit indicators. In order to reduce electromagnetic radiation and coupling, the primary, secondary and load side loop areas of the DC-DC module are required to be minimized. No matter how complex the power circuit is, its large current loop must be as small as possible. The power line and ground line should always be placed very close.
　　(2) If a switching power supply is used in the circuit, the layout of the peripheral components of the switching power supply must comply with the principle of the shortest power return path. The filter capacitor should be close to the relevant pins of the switching power supply. Use common-mode inductors and close to the switching power supply module.
　　(3) Long-distance power lines on a single board cannot be close to or pass through the output and input terminals of the cascade amplifier (gain greater than 45dB) at the same time. Avoid the power line from becoming an RF signal transmission path, which may cause self-excitation or reduce sector isolation. High-frequency filter capacitors need to be added to both ends of the long-distance power line, and even in the middle.
　　(4) Three filter capacitors are combined in parallel at the power input of the RF PCB, and the respective advantages of these three capacitors are used to filter out the low, medium and high frequencies on the power line respectively. For example: 10uf, 0.1uf, 100pf. And in order from large to small, they should be close to the input pin of the power supply.
　　(5) When using the same set of power supplies to feed the small signal cascade amplifier, it should start from the last stage and then supply power to the previous stage in turn, so that the EMI generated by the last stage circuit has less impact on the previous stage. And each stage of the power supply filter has at least two capacitors: 0.1uf, 100pf. When the signal frequency is higher than 1GHz, a 10pf filter capacitor should be added.
　　(6) Small power electronic filters are often used. The filter capacitor should be close to the transistor pins, and the high-frequency filter capacitor should be closer to the pins. The transistor should be selected with a lower cutoff frequency. If the transistor in the electronic filter is a high-frequency tube, it works in the amplification area, and the layout of the peripheral devices is unreasonable, it is easy to generate high-frequency oscillation at the power output end.
　　The linear voltage regulator module may also have the same problem because there is a feedback loop in the chip and the internal transistor works in the amplification area. When laying out, the high-frequency filter capacitor is required to be close to the pins to reduce the distributed inductance and destroy the oscillation conditions.
　　(7) The copper foil size of the POWER part of the PCB should meet the maximum current flowing through it, and the margin should be considered (generally referred to as 1A/mm line width).
　　(8) The input and output of the power line cannot cross.
　　(9) Pay attention to power decoupling and filtering to prevent interference between different units through the power line. The power lines should be isolated from each other during power wiring. The power line is isolated from other strong interference lines (such as CLK) by ground wire.
　　(10) The power wiring of the small signal amplifier needs to be isolated by ground copper foil and ground vias to prevent other EMI interference from intruding, thereby deteriorating the signal quality of this level.
　　(11) Different power layers should avoid overlapping in space. The main purpose is to reduce the interference between different power supplies, especially between some power supplies with large voltage differences. The overlap of power planes must be avoided. If it is difficult to avoid, consider using a ground layer in the middle.
　　(12) PCB layer allocation facilitates the subsequent wiring process. For a four-layer PCB board (commonly used in WLAN), in most applications, the top layer of the circuit board is used to place components and RF leads, the second layer is used as the system ground, the power part is placed on the third layer, and any signal line can be distributed on the fourth layer.
　　The use of a continuous ground plane layout on the second layer is essential for establishing an impedance-controlled RF signal path. It also facilitates the shortest possible ground loop, provides a high degree of electrical isolation between the first and third layers, and minimizes coupling between the two layers. Of course, other board layer definitions can also be used (especially when the circuit board has different numbers of layers), but the above structure is a proven successful example.
　　(13) A large power layer can make Vcc wiring easier, but this structure is often the fuse that causes system performance to deteriorate. Connecting all power leads together on a large plane will not avoid noise transmission between pins. On the contrary, if a star topology is used, the coupling between different power pins will be reduced.
　　Good power decoupling technology combined with rigorous PCB layout and Vcc leads (star topology) can lay a solid foundation for any RF system design. Although there will be other factors that reduce system performance indicators in actual design, having a "noise-free" power supply is a basic element to optimize system performance.

张玲莉

I have learned it. I am currently drawing an RF board. It is very useful.