The following issues need to be considered for vias in PCB design

The following issues need to be considered for vias in PCB design

Via is one of the important components of multi-layer PCB, and the cost of drilling usually accounts for 30% to 40% of the cost of PCB board. From the design point of view, a via is mainly composed of two parts, one is the drill hole in the middle, and the other is the pad area around the drill hole. The size of these two parts determines the size of the via. . Obviously, when designing high-speed and high-density PCBs, designers always want the vias to be as small as possible, so that more wiring space can be left on the board. In addition, the smaller the vias, the smaller the parasitic capacitance. The smaller it is, the more suitable it is for high-speed circuits. However, the reduction in hole size also brings an increase in cost, and the size of the via hole cannot be reduced indefinitely. It is limited by process technologies such as drilling and plating: the smaller the hole, the more drilling The longer the hole takes, the easier it is to deviate from the center; and when the depth of the hole exceeds 6 times the diameter of the drilled hole, it is not guaranteed that the hole wall will be uniformly plated with copper.

Therefore, for comprehensive design and production, we need to consider the following issues:

1. In principle, the inner diameter of the full through hole is required to be 0.2mm (8mil) and above, and the outer diameter is 0.4mm (16mil) or above, and the outer diameter must be controlled to 0.35mm (14mil) in difficult places;

Reminder assistant: According to experience, the size of the inner diameter and outer diameter of the commonly used PCB vias generally follows X*2±2mil (X represents the inner diameter). For example, 8mil inner diameter vias can be designed as 8/14mil, 8/16mil or 8/18mil; for example, 12mil vias can be designed as 12/22mil, 12/24mil, 12/26mil;

2. It is recommended not to use buried blind vias for BGA designs of 0.65mm and above, and the cost will increase significantly. When buried blind vias are used, first-order blind vias (TOP layer-L2 layer or BOTTOM-negative L2) are generally used. The inner diameter of the via hole is generally 0.1mm (4mil), and the outer diameter is 0.25mm (10mil).

3. The vias cannot be placed on the pads smaller than the size of the 0402 resistor-capacitor pads; theoretically, the lead inductance is small when placed on the pads, but during production, the solder paste is easy to enter the vias, causing uneven solder paste and causing the device to stand. The phenomenon of getting up ('tombstone' phenomenon). The general recommended spacing is 4-8mil

4. The spacing between vias and vias should not be too close. Drilling is easy to cause hole breakage. Generally, the spacing between holes is required to be 0.5mm and above, and 0.35mm-0.4mm should be avoided as much as possible, and 0.3mm and below are prohibited.

5. In addition to the heat dissipation vias, the vias of ≤0.5mm need to be plugged with oil (the inner diameter is 0.4mm and the hole needs to be plugged).

1) Especially for devices with metal casings, in principle, no through holes are drilled under the body, and certain plug holes are covered with oil to avoid short circuit between the casing and the through holes.

2) According to the production feedback of the board factory, it is often mentioned that the vias under the BGA are too close to the pads, and the vias need to be moved. This situation is caused by the fact that the vias are not equidistant from the BGA pads. Since it is a normal state that the positions of the vias and test holes under the BAG are not equidistant from the BGA pads, the PCB designers do not pay attention to this. , resulting in continuous engineering problems and a hidden danger to the welding quality. Therefore, we directly recommend punching the hole to the center of the two pads, especially in the BGA, due to the small pitch spacing, it is necessary to cover the via hole under the BGA after punching, so as to avoid short circuit between the BGA ball and the tin. .

6. The fixed pads such as headphone terminals, buttons, and FPC are used to prevent the copper from falling off the pads. When conditions permit, the pads are punched with 1-2 vias (the vias are placed evenly), which can effectively improve the "fixation".

7. Fan hole

The fan-out of vias is very important in PCB design. The way of fan-holes will affect signal integrity, plane integrity, and difficulty of wiring, so as to affect the cost of production.

1) The fan hole recommendation and defect method of conventional CHIP devices, it can be seen that the recommended method can pass the line between the two holes in the inner layer, and the reference plane will not be split. On the contrary, the unrecommended method increases the difficulty of routing. The plane is split and the plane integrity is destroyed.

Comparison of fan-out methods of conventional CHIP devices

Similarly, this kind of device fan hole method is suitable for the situation of punching and changing layers.

2) BGA fan hole method

The BGA fan hole is also not suitable to be punched on the pad. It is recommended to punch the hole in the middle of the two pads. Many engineers move the position of the via hole in the BGA at will or even punch it on the pad in order to facilitate the exit of the wire, resulting in the irregularity of the via hole in the BGA area, which may easily lead to the problem of soldering in the later stage, and may damage the plane integrity