Precision PCB Fabrication, High-Frequency PCB, High-Speed PCB, Standard PCB, Multilayer PCB and PCB Assembly.
The most reliable PCB & PCBA custom service factory.
1. Via
Vias are one of the important components of multi-layer PCB board, and the cost of drilling usually accounts for 30% to 40% of the cost of PCB board production. Simply put, every hole on a PCB can be called a via. From the perspective of function, vias can be divided into two categories: one is used for electrical connection between layers; the other is used for device fixation or positioning. In terms of process, these vias are generally divided into three categories, namely blind vias, buried vias, and through vias. Blind holes are located on the top and bottom surfaces of the printed circuit board, with a certain depth, for the connection of the surface circuit and the underlying inner circuit, and the depth of the hole usually does not exceed a certain ratio (diameter). Buried vias refer to connection holes located in the inner layer of the printed circuit board, which do not extend to the surface of the circuit board. The above two types of holes are located in the inner layer of the circuit board and are completed by the through hole forming process before lamination. During the formation of the via hole, several inner layers may be overlapped. The third type is called through-hole, which penetrates the entire circuit board and can be used for internal interconnection or as a mounting location hole for components. Because the through hole is easier to realize in the process and the cost is lower, most of the printed circuit boards use it instead of the other two kinds of through holes. The via holes mentioned below are considered as through holes unless otherwise specified. From a design point of view, a via is mainly composed of two parts, one is the middle hole, and the other is the pad area around the hole, as shown in the figure below. The size of these two parts determines the size of the via. Obviously, in the design of high-speed and high-density PCB boards, designers always hope that the smaller the via hole, the better, so that more wiring space can be left on the board. In addition, the smaller the via hole, the more parasitic capacitance of its own The smaller it is, the more suitable it is for high-speed circuits. However, the reduction of hole size also brings an increase in cost, and the size of vias cannot be reduced indefinitely. It is limited by process technologies such as drilling and electroplating: the smaller the hole, the more time it takes to drill. The longer it is, the easier it is to deviate from the center position; and when the depth of the hole exceeds 6 times the diameter of the drilled hole, it cannot be guaranteed that the hole wall can be uniformly plated with copper. For example, the thickness of a normal 6-layer PCB board (through hole depth) is about 50Mil, so the diameter of the hole provided by the PCB board manufacturer is very small and can only reach 8Mil.
2. Parasitic capacitance of vias
The hole itself has parasitic capacitance to the ground. If it is known that the diameter of the isolation hole of the via on the ground layer is D2, the diameter of the via pad is D1, the thickness of the PCB board is T, and the dielectric constant of the board substrate is ε, then the parasitic capacitance of the via hole is similar to: C=1.41εTD1/(D2-D1) The main effect of the parasitic capacitance of the via hole on the circuit is to prolong the rise time of the signal and reduce the speed of the circuit. For example, for a PCB board with a thickness of 50Mil, if a via hole with an inner diameter of 10Mil and a pad diameter of 20Mil is used, and the distance between the pad and the ground copper area is 32Mil, we can approximate the via hole through the above formula. The parasitic capacitance is roughly: C=1.41x4.4x0.050x0.020/(0.032-0.020)=0.517pF, the rise time change caused by this part of the capacitance is: T10-90=2.2C(Z0/2)=2.2 x0.517x(55/2)=31.28ps. From these values, it can be seen that although the effect of slowing rise caused by the parasitic capacitance of a single via is not very obvious, the designer should consider carefully if the via is used for switching between layers in the trace multiple times.
3. Parasitic inductance of vias
Similarly, parasitic inductance exists along with parasitic capacitance of vias. In the design of high-speed digital circuits, the harm caused by the parasitic inductance of vias is often greater than the influence of parasitic capacitance. Its parasitic series inductance will weaken the contribution of the bypass capacitor and reduce the filtering effect of the entire power system. The diameter of the via has little effect on the inductance, while the length of the via has a large effect on the inductance. Still using the above example, the inductance of the via can be calculated as: L=5.08x0.050[ln(4x0.050/0.010) 1]=1.015nH. If the rise time of the signal is 1ns, then its equivalent impedance is XL=πL/T10-90=3.19Ω. Such impedance can no longer be ignored when high-frequency currents pass through. Special attention should be paid to the fact that the bypass capacitor needs to pass through two vias when connecting the power supply layer and the ground layer so that the parasitic inductance of the vias will be multiplied.
4. Via design on a high-speed PCB board
Through the above analysis of the parasitic characteristics of vias, we can see that in the design of high-speed PCB boards, seemingly simple vias often bring great negative effects to circuit design. In order to reduce the adverse effects caused by the parasitic effects of vias, you can try to do as much as possible in the design:
1) Considering both cost and signal quality, select a via the size of a reasonable size. For example, for a 6-10 layer memory module PCB board design, it is better to use 10/20Mil (drilling/pad) vias. For some high-density small-sized boards, you can also try to use 8/18Mil. vias. Under current technical conditions, it is difficult to use smaller vias. For power or ground vias, consider using larger sizes to reduce impedance.
2) From the two formulas discussed above, it can be concluded that using a thinner PCB board is beneficial to reduce the two parasitic parameters of the via.
3) Try not to change the layers of the signal traces on the PCB, that is to say, try not to use unnecessary vias.
4) The pins of the power supply and ground should be drilled as close as possible. The shorter the lead between the via and the pin, the better, because they will increase the inductance. At the same time, the leads of power and ground should be as thick as possible to reduce impedance.
5) Place some grounded vias near the vias where the signal changes layers to provide a close return path for the signal. It is even possible to place a few redundant ground vias on the PCB board in large numbers. Of course, flexibility is also required in the design. The via model discussed earlier is the case where each layer has pads, and sometimes, we can reduce or even remove the pads of some layers. Especially in the case of a very high density of vias, it may lead to the formation of a circuit breaker on the copper layer. To solve this problem, in addition to moving the position of the via, we can also consider placing the PCB board via on the copper layer. The pad size is reduced.
