Radio frequency circuit (RF) is called “black art” because of many uncertain factors. However, through practice and exploration, we will find that there are rules to follow. Based on our many years’ working practice and previous experience, we will discuss the circuit board design of RF circuit around these aspects: layout, impedance, lamination, design considerations, edge wrapping, power supply treatment and surface treatment.
1 about layout
The principle of RF circuit layout is that the RF signal should be as short as possible, and the input should be far away from the output. The RF circuit should be arranged in a word, followed by an L-shaped arrangement, or an obtuse angle greater than 90 degrees (such as an angle of 135 degrees). There is also a U-shaped layout, which mainly depends on the space and wiring requirements. The U-shaped layout is used when conditions are really limited, and the distance between two parallel lines should be controlled to be at least 2mm. High-sensitive devices such as filters need to be equipped with metal shields, and slots should be provided where microstrip lines enter and exit the shields. RF area and other areas (such as voltage stabilizing block area and numerical control area) should be laid out separately; High-power amplifier, low-noise amplifier, frequency synthesizer, etc. all need to be laid out separately, and they should be separated by retaining walls.
2 About impedance
Factors related to impedance include line width, thickness of dielectric plate, dielectric constant of dielectric plate, thickness of copper skin, etc. In RF, 50 ohms is often used as the impedance matching standard, and Rogers series plates, such as Rogers 4350 plates, are usually used for the selection of RF dielectric plates. Assuming that we choose 0.254mm thickness, then according to the simulation, the line width is 0.55mm, and the copper thickness is 0.5OZ. At this time, the impedance can be controlled to 50 ohms. For other models, plates with other thicknesses can be simulated according to their dielectric constant and thickness. It is recommended that you use Polar SI8000 impedance calculation tool for calculation, which is simple and convenient.
3 About laminated structure
Generally, devices and microstrip lines are placed on the top layer of RF board, the second layer should be paved with network copper in a large area, and the bottom layer should be completely paved with copper to directly contact the cavity plane, and the middle layer should be routed with signal lines. If the circuit is complex and there are multiple signal lines in the middle, then the ground plane should be added between the adjacent signal lines, and the two signal lines should be routed vertically, that is, one line is mainly horizontal and the other is mainly vertical. Because the RF circuit board cannot use non-ground network through holes, Therefore, the blind hole design should be used for other networks except ground holes. If there are eight-layer boards, in order to make effective use of the laminate, the seventh layer should be the signal line layer, which will lead to a large number of 1 to 7 blind holes. In actual processing, such blind hole design will cause serious warpage of the circuit board. The solution is to use a back drill, that is, make the blind holes according to the through holes, and then cut out the copper of this metallized hole from the bottom up to the seventh and eighth layers, not to the seventh layer, in order to make the performance more stable.
4 matters needing attention in circuit board design
1) Duplexer, mixer and IF amplifier always have multiple RF and IF signals interfering with each other, so the interference must be minimized. The RF and IF traces should be crossed as much as possible, and a grounding copper skin should be placed between them as much as possible, and more grounding vias should be made.
2) The non-ground vias should be placed as little as possible within the range of 2 times the line width of the microstrip line of the RF board, and the size of the vias should be as small as possible, which can not only reduce the path inductance, so that the copper laying on the main ground plane will be as complete as possible, and the RF signal energy should be placed to pass through the vias, resulting in leakage.
3) The microstrip line of RF board should be windowed, that is, no green oil solder resist. The actual measurement shows that it can improve the performance of RF circuit.
4) A row of ground holes should be placed on both sides of the edge of the RF signal at a distance of 1.5 times the line width parallel to the RF line. This distance should not be too close. Simulation shows that if the ground is too close to the microstrip line, a part of RF energy will be coupled to the ground, which will cause a certain loss. The ground holes should be small and dense, with a diameter of 0.2mm to 0.3mm and a distance of 0.6mm to 1mm. This ground hole can inhibit the crosstalk between microstrip lines. In actual wiring, Because there are signal lines in the inner layer of some circuit boards, and the lines are complicated, there are often many places where isolation holes cannot be placed. Then the solution is to change the grounding holes that will encounter the signal lines into one or two blind holes, thus greatly preserving the integrity of the ground holes and effectively suppressing the crosstalk.
5 About wrapping
The circuit board edge wrapping treatment and the network metallization edge wrapping treatment around the radio frequency circuit board can reduce the loss of radio frequency signals. Because the circuit board is made of spliced boards in the actual manufacturing process, and the metallization of the board edge requires that the shape of the metal-clad edge should be cut before the via hole is copper-deposited. At this time, the circuit board has not been finished yet, so the boards must be connected with each other through some connecting belts, so they cannot be cut completely. Generally, we will place these connecting strips in the area far away from RF, and make them as short as possible. Generally, the board factory will require two connecting strips on each side, which are not shorter than 5mm. Generally, the microstrip lines at the input and output of RF will be pushed to the edge of the board. In this position, we will require the board factory to have a complete edge covering. Since the edge covering is in the same network as the earth, it will be short-circuited with the microstrip lines. Then, it is required that our circuit board should be gently scraped with a scalpel after returning to the process assembly department of our company.
6 About the treatment of RF circuit power supply
As we all know, the power supply of the circuit needs decoupling capacitors to filter the power supply and remove the interference. RF chips are more sensitive to the power supply, so decoupling capacitors and isolation inductors are needed to filter the noise interference of the power supply part. The power supply of the RF circuit should be filtered immediately after being introduced into the circuit board, and distributed to all parts of the circuit through voltage stabilizing blocks. In order to reduce the current loss and generate voltage drop, the power supply is best transmitted to the required devices through blind holes through the inner layer. Generally, the power supply of the RF circuit does not need to be divided into planes, and the whole power supply plane will interfere with the RF signal, so it is only necessary to supply power in the form of wires in the inner layer to meet the current requirements. However, in order to avoid voltage drop, the power supply line should be as short as possible, and it should not overlap with the microstrip line, and the loop should be avoided. In addition, the decoupling power supply around the chip and the via holes on the grounding pad should be placed as close as possible to the capacitor pad, and the grounding pad of the capacitor should be laid with a large area of copper skin. Here, attention should be paid.
7 About surface treatment
RF boards often need gold wire bonding, which can’t be met by ordinary surface treatment. Generally, electroplating thick gold should be used, and the gold thickness should be controlled above 2um, so that the adhesion requirement of gold wire bonding can be met, and it has a great relationship with the purity of gold. Due to the requirement of gold plating process, the pads must be physically connected, so all the pads can be plated with gold by electroplating. Therefore, there is a thin process line between the two pads in our designed circuit board that should not be connected together. It needs to be manually removed before the circuit board is soldered, which not only takes time, but also destroys the smoothness and integrity of the circuit. It is not realistic to leave the process line for complex multilayer boards. In the actual gold plating process, aluminum wires are usually pressed on the copper skin and then plated with gold, and then the aluminum wires are removed after gold plating. The chemical nickel-palladium-gold deposition process has been proved by practice to achieve perfect bonding effect, and it can be achieved by controlling the thickness of metal nickel, palladium and gold without any process line. Generally, nickel does not need special control according to the conventional thickness, and the thickness of palladium and gold is generally controlled at 3 microinches.
