How to distinguish between pads and vias_Differences between vias and pads
[Copy link]
Pad and via designComponents are fixed on the printed circuit board by soldering the leads to the pads. The function of vias is to connect electrical connections at different levels. (1) Pad size The pad size is related to factors such as the lead hole and the minimum hole ring width. The pad size should be increased as much as possible, but the wiring density should also be considered. In order to ensure the reliability of the connection between the pad and the substrate, the lead hole is drilled in the center of the pad, and the hole diameter should be slightly larger than the diameter of the lead of the soldered component. The diameter of the lead hole of the component is preferably 0.5 mm, 0.8 mm, and 1.2 mm. The pad ring width is selected within the range of 0.5 to 1.0 mm. Generally, the pad diameter size for dual in-line integrated circuits is 1.5 to 1.6 mm, and 0.3 to 0.4 mm wide printed wires can pass through adjacent pads. Generally, the pad ring width is not less than 0.3 mm, and the pad diameter is not less than 1.3 mm. The actual pad size uses the parameters recommended in Table 8-1. （2）Pad shape Different pad shapes can be selected according to different requirements. Common pad shapes include round, square, oval, island and special shapes. This content is originally created by EEWORLD forum user luoxiao1116. If you need to reprint or use it for commercial purposes, you must obtain the author's consent and indicate the source Circular pad: The outer diameter is generally 2 to 3 times the aperture diameter, and the aperture is 0.2 to 0.3 mm larger than the lead. Island pad: The connection between the pads is integrated into one, like an island on the water, so it is called an island pad. It is often used in irregular arrangement of components, which is conducive to dense fixing of components and can greatly reduce the length and number of printed wires. Therefore, it is often used in high-frequency circuits. Other forms of pads are made by deforming the circular pads in order to allow the printed wires to pass between adjacent pads. When using it, it should be used flexibly according to the actual situation. （3）Via selection The hole diameter should be as small as possible to less than 0.2 mm, which can improve the connection quality of the pads on both sides of the metallized via. The difference between vias and through-hole pads in PCBIn PCB design, vias VIA and pads PAD can achieve similar functions. They can all be inserted into component pins, especially for DIP packaged devices, they are almost the same. However! In PCB manufacturing, their processing methods are different. 1. The number of holes in the VIA is indicated in the design, and the number of holes is the same. Then it has to go through copper deposition and other process steps, and the actual hole diameter will be about 0.1mm smaller than the designed hole diameter. For example, if the via is set to 0.5mm, the actual hole diameter after completion is only 0.4mm. 2. The aperture of PAD will increase by 0.15mm when drilling. After copper deposition, the aperture is slightly larger than the designed aperture, about 0.05mm. For example, if the designed aperture is 0.5mm, the drilling will be 0.65mm, and the completed aperture is 0.55mm. 3. VIA will be covered with green oil in some default PCB processes. It may be blocked by the green oil and cannot be soldered. Test points cannot be made either. 4. The minimum width of the VIA solder ring is 0.15mm (under general process conditions) to ensure reliable copper plating. 5. The minimum width of the PAD solder ring is 0.20mm (under general process conditions) to ensure the adhesion of the pad. Can vias be punched on pads in PCB design? When designing a PCB board, sometimes due to the limitation of the board area or the complexity of the routing, it is considered to punch vias on the pads of the SMD components. There have always been two opinions: support and opposition. But in general, based on the author's many years of practical experience, it is felt that the method of punching vias on the pads is likely to cause cold soldering of SMD components. It should be used with caution when it is absolutely necessary. The two viewpoints are briefly described as follows. Support: Generally, the purpose of drilling vias on the pads is to enhance the overcurrent capability or heat dissipation. Therefore, the back side is mainly copper for connecting the power supply or ground, and SMD components are rarely placed. In order to prevent tin leakage during reflow soldering, green oil can be added to the back side of the vias, and the problem is solved. The power supply parts of the server motherboards I have come into contact with are all handled in this way. Oppose: Generally, SMD components can be processed by reflow soldering or wave soldering. Wave soldering requires that the pad density should not be too high. Too dense pads are prone to cause tin short circuits. SMD IC feet are relatively dense, so reflow soldering is the preferred solution. Insertion files can only be processed by wave soldering. There are many introductions about wave soldering and reflow soldering on the Internet. Engineers who are engaged in PCB design should first understand these production processes before knowing how to design. There is a Fanout rule in Protel, which prohibits punching vias on pads. Traditional processes prohibit this because solder will flow into the vias. Now there are two processes, micro vias and plug vias, which allow vias to be placed on pads, but they are very expensive. Consult the PCB factory. It is best not to punch vias on PADs, which is easy to cause cold soldering. After sorting out the layout, the position of a small via should still be found. However, for SMD components, the solder will flow away through the vias during reflow. So use with caution.
PCB设计应用教材.rar
(13.93 MB, downloads: 219)
| 
提升卡
变色卡
千斤顶
京公网安备 11010802033920号
