四层板的电源层需不需要弄成完整的一个平面？

sfcsdc

四层板的电源层需不需要弄成完整的一个平面？ [复制链接]

 

一般四层板的顺序是：信号层-地层-电源层-信号层；

为了保证最小的回路路径，地层需要保持完整的一整块；

那么，电源层是否也需要保持完整呢？

保持完整的电源层可以和地层形成一个很大的分布电容，对每个信号都起到一定的滤波作用，并且也有一定的屏蔽效果。

但是我经常看到别人的参考设计，电源层是直接拉线连接的，并没有搞成完整的一个平面。

如下TI的一个蓝牙参考设计

大家怎么看？

飞鸿浩劫

纠结这个干啥呢

btty038

满足要求  根据自己的需求就行了   散热什么的  和成本

qwqwqw2088

PCB布板多从板子的原理图上分析

看现象不一定看透本质

topwon

电源铺平面有助于利用层间电容效应对高频噪声去耦。不利之处，如果bottom层的高速信号参考第三层的话，需要所参考的电源平面不要被分割，比如不同的电源电压网络，避免跨参考平面，否则不如电源走线而把空余区域也铺地作为高速信号参考层。另外电源走线也有助于控制电源线上的干扰电流流向，避免不同电路区域的干扰。所以是要根据具体设计要求来考虑的。一般我是会选择 高速信号只走top层，电源层铺平面。

sfcsdc

谢谢大家回复

topwon

Some circuits result in large signal currents switching rapidly at the same time. Any inductance in the path of these current swings will result in noise voltages being generated across the inductance. The concept of "ground bounce" relates to this issue. Planes generally provide the lowest inductance paths for these currents. Therefore, planes are used to reduce noise when there are high current flows in power distribution systems. Even if large current swings are not present, small signals in very fast switching circuits can also be affected by noise caused by currents flowing through "stray" inductance. Planes generally provide the lowest inductance paths in these environments also. Properly designed planes will act like very small capacitors. The do not offer enough capacitance to substitute for bypass capacitors in the medium frequency ranges, but they can offer enough capacitance to provide the initial charge required by very fast leading edge switching transients when ordinary bypass capacitors have to much lead inductance to respond. All signals MUST have a return signal. As frequency harmonics get higher, the path for the return signal will want to be directly underneath the signal trace. This can be on EITHER a power or a ground plane. Consider the concept of a loop. The signal trace and the return signal on the plane comprise a loop. If there is no obstruction anywhere on the plane, then the area of this loop will be small. If the return signal must take a circuitous path --- because, perhaps, the plane is not solid and there are voids on the plane --- the loop area will be larger. EMI emissions are directly related to this loop area. Therefore, one reason for designing in planes is for control of EMI emissions. And one reason for avoiding slots and voids in planes is to minimize loop area.

wudayongnb

铺铜一定要距离固定孔要远，隔开足够的距离。

谷峰

对于4层板，如果电源单一可以采用一个平面，但是如果电源有多路，就需要把电源平面切成若干个平面，同时保持临近的信号层尽量不跨moat，不建议直接拉线，建议走整块铜箔

中文用户名

不一定吧看实际情况

54liuyi

topwon 发表于 2019-6-20 11:25 电源铺平面有助于利用层间电容效应对高频噪声去耦。不利之处，如果bottom层的高速信号参考第三层的话，需要 ...

“需要所参考的电源平面不要被分割，比如不同的电源电压网络，避免跨参考平面”，这句话的意思是：不同的电源电压网络不跨参考平面就不算分割电源平面是吗？

topwon

54liuyi 发表于 2022-4-25 17:27 “需要所参考的电源平面不要被分割，比如不同的电源电压网络，避免跨参考平面”，这句话的意思 ...

比如底层的一条高速时钟线，其路径在第三层分别参考了3.3V电源平面和1.8V电源平面，那就是跨参考平面。。。。