Case diagram of several key points of RF PCB design

btty038

Case diagram of several key points of RF PCB design [Copy link]

In electronic products and equipment, the circuit board is an indispensable component, which plays the role of electrical and mechanical connection of the circuit system. How to arrange and combine the components in the circuit on the PCB according to certain requirements is one of the main tasks of the PCB designer. Layout design is not simply to arrange the components on the PCB, or to connect the circuit. Practice has proved that a good circuit design must have a reasonable layout of components to enable the circuit system to achieve stable and reliable operation after physical combination. On the contrary, if the layout of components is unreasonable, it will affect the working performance of the circuit board and even fail to work. Especially today when integrated devices are widely used, if the integrated circuit is still installed in the form of a wiring board, then not only the volume of the circuit is huge, but also it cannot work stably. Therefore, in the product design process, layout design and circuit design have the same important position.

The following is a brief introduction to the considerations in RF PCB design.

1. Layout considerations

(1) Structural design requirements

Before PCB layout, it is necessary to understand the structure of the product. The structure needs to be reflected on the PCB board (the part where the structure contacts the PCB, that is, the position and shape of the cavity shell). For example, the thickness of the outer edge of the cavity shell, the thickness of the middle partition, the chamfer radius, and the size of the screws on the partition, etc. (In other words, the structural design is specifically designed according to the outline (structural part) drawn on the completed PCB (if the structure has been molded in batches, it is another matter)) (the screw types are M2\M2.5\M3\M4, etc.). Generally, the thickness of the outer cavity is 4mm; the width of the inner cavity is 3mm (2mm for the dispensing process); the chamfer radius is 2.5mm. Taking the lower left corner of the PCB board as the origin, the position of the partition on the PCB must be on an integer multiple of 0.5 of the grid point, and at least the grid point must be an integer multiple of 0.1. This is conducive to structural processing and the error control is more accurate. Of course, this needs to be designed according to the specific product type. As shown in the figure below: (Structural outline after PCB design is completed)

(2) Layout requirements

Prioritize the layout of the RF link and then other circuits.

① RF link layout precautions: Layout should be carried out according to the sequence of the schematic diagram (from input to output, including the sequence of each component and the spacing between components. The distance between some components should not be too large, such as π network.), and the layout should be in the shape of "I" or "L". The details are shown in the following figure:

In the actual RF link layout, due to the space limitation of the product, it is impossible to completely realize the "one" shape layout, which forces us to layout it in a "U" shape. It is not impossible to layout in a U shape, but it is necessary to add a partition in the middle to isolate the left and right sides and do a good job of shielding. As for why shielding is needed, I will not say more. As shown in the following figure:

There is also a need to add a partition in the horizontal direction. That is, use a partition to isolate the left and right sides of the straight line. This is mainly because the part that needs to be isolated is very sensitive or easy to interfere with other circuits; in addition, there is another possibility that the gain of the circuit from the input end to the output end of the straight line is too large, and a partition is also needed to separate it (if the gain is too large, the cavity is too large, it may cause self-excitation). As shown in the following figure:

② Chip peripheral circuit layout

The layout of the peripheral circuits of RF devices is strictly based on the requirements on the datasheet. Adjustments can be made due to space limitations (placed as close to the chip as possible while ensuring process requirements). I will not go into detail about the layout of the peripheral circuits of digital chips.

If the structure has a metal base plate, try not to place components on the contact surface between the PCB and the base plate, and avoid cutting grooves on the metal base plate.

2. Cabling considerations

Perform routing according to the 50 ohm impedance line width (generally, a layer reference is required), try to route from the center of the pad, route in a straight line, and try to route on the surface. Make a 45-degree angle or arc routing where a turn is required. It is recommended to use the pads on both sides of the capacitor or resistor as the turning point. If you encounter device routing matching requirements, please strictly follow the reference value length and shape routing on the datasheet. For example, the routing length between an amplifier and a capacitor (or the routing length between an inductor) is required, etc. As shown in the figure below:

When designing PCB, in order to make the design of high-frequency circuit boards more reasonable and have better anti-interference performance, the following aspects should be considered (general practice):

(1) Choose the number of layers appropriately

When routing high-frequency circuit boards in PCB design, using the middle inner plane as the power and ground layers can play a shielding role, effectively reducing parasitic inductance, shortening signal line length, and reducing cross-interference between signals.

(2) Wiring method

The routing must turn at a 45° angle or in a circular arc to reduce the emission of high-frequency signals, mutual coupling, and signal reflection.

(3) Trace length

The shorter the trace length, the better, and the shorter the parallel distance between the two wires, the better.

(4) Number of vias

The more vias the better.

(5) Interlayer wiring direction

The inter-layer wiring direction should be vertical, that is, the top layer is horizontal and the bottom layer is vertical, which can reduce interference between signals.

(6) Copper coating

Increasing the ground copper can reduce interference between signals.

(7) Land lease

Grounding important signal lines can significantly improve the signal's anti-interference capability. Of course, you can also ground the interference source to prevent it from interfering with other signals.

(8) Signal line

Signal routing cannot be looped and needs to be wired in a daisy chain manner.

3. Grounding

(1) RF link grounding

The RF part is grounded using a multi-point grounding method. The RF link copper plating gap is generally 20mil to 40mil. Grounding holes need to be drilled on both sides, and the spacing should be kept as consistent as possible. The grounding pads of the capacitors and resistors on the RF path should be drilled as close as possible. The grounding pads on the device need to be drilled with ground vias. As shown in the following figure:

(2) Cavity shell grounding hole

In order to make better contact between the cavity shell and the PCB board, two rows of grounding holes are usually drilled and placed in a staggered manner, as shown in the figure below.

A window needs to be opened at the contact position between the PCB and the compartment, as shown in the following figure:

The places where the PCB bottom ground copper sheet contacts the base plate need to be opened (windows are not allowed for the signal line layer) to make them contact better. As shown in the following figure (the upper part of the PCB board contacts the base):

(3) Screw placement (structural knowledge required)

In order to make the PCB have a closer contact with the base and cavity shell (better shielding and heat dissipation), it is necessary to place screw hole positions on the PCB board.

The method of placing screws between PCB and cavity shell is: place a screw at each intersection of the cavity. In actual design, it is difficult to achieve, and it can be adjusted appropriately according to the module circuit function. But in any case, there must be screws on the four corners of the cavity shell. As shown in the following figure:

How to place screws between the PCB and the base: Each small cavity in the cavity shell needs to have screws, and the number of screws depends on the size of the cavity (the larger the cavity, the more screws are placed). The general principle is to place screws on the diagonal of the cavity. Screws must be placed next to the SMA head or other connector. The SMA head or connector will not deform the PCB during the plug-in and unplug process. As shown in the figure below (screws in the cavity):

alan000345

The layout of the board is indeed very important. If it is not done properly, the signal reception will be very poor.

青鸟飞鱼

I learned a lot. It's very good.