Four Layer PCB Stack up with both inner ground layers

Thread Starter

rockgro

Joined Sep 7, 2021
19
In a 4-layer PCB, when to use both inner layers as ground planes? How do you decide if the inner layers should be power and ground, or both as ground?
 

Thread Starter

rockgro

Joined Sep 7, 2021
19
The main reason for going to 4 layers is to have two planes for traces that do not have to contend with power an GND routing.
I used to watch a lot of Phil's Lab videos. And as far as I understood, the power and ground as inner layers are not good for signal integrity.
Here is one of the videos which talk about this:
 

Thread Starter

rockgro

Joined Sep 7, 2021
19
What advantage would there be to have two ground planes?
It improves signal integrity. Because when the signal switches layers, the reference plane changes from ground to power and this can cause several issues.
Here is one of the videos which talk about this:
 

nsaspook

Joined Aug 27, 2009
10,675
The EM energy of the signals are in the PCB dielectric as it moves from point to point. I usually alternate signal/power and ground layers in a PCB to provide a conductive wave-guide for digital signals that act like RF in transmission lines as they move from place to place.
1669180613591.png
https://www.ednasia.com/design-pcbs-for-emi-part-1-how-signals-move/

If you think electromagnetically instead of using static trace wire current flows the layered design is very intuitive.
https://www.nwengineeringllc.com/article/how-to-design-your-pcb-return-current-path.php
 
Last edited:

Thread Starter

rockgro

Joined Sep 7, 2021
19
The EM energy of the signals are in the PCB dielectric as it moves from point to point. I usually alternate signal/power and ground layers in a PCB to provide a conductive wave-guide for digital signals that act like RF in transmission lines as they move from place to place.
View attachment 281246
https://www.ednasia.com/design-pcbs-for-emi-part-1-how-signals-move/

If you think electromagnetically instead of using static trace wire current flows the layered design is very intuitive.
https://www.nwengineeringllc.com/article/how-to-design-your-pcb-return-current-path.php
So basically you are saying, for a 4-layer PCB stack up should be as shown below?

SIGNAL/POWER
GND
GND
SIGNAL/POWER
 

nsaspook

Joined Aug 27, 2009
10,675
https://www.allaboutcircuits.com/technical-articles/common-layer-stack-ups-for-a-four-layer-board/

Stack-ups with Both Power and Ground Planes
1669222939655.png
Drawbacks to the Conventional Four-Layer Stack-ups
1669222979922.png
The first problem with the stack-ups in Figures 1 and 2 arises when a trace changes layer from layer 1 to 4 or vice versa. This is shown in Figure 3.

Two Improved Stack-ups

1669223079920.png
1669223063260.png


Although these two stack-ups don’t have solid power planes, the power pours are in close proximity to the ground planes. As a result, the power pours and the ground planes will create a relatively large capacitance that can act as a decoupling structure at high frequencies. Rick Hartley, a well-respected PCB designer, presents measured data confirming that the decoupling between the power pours and planes of Figures 6 and 7 outperforms the decoupling provided by the ground and power planes of a conventional four-layer board (Figures 1 and 2). Using the decoupling structure of the improved stack-ups along with the usual decoupling capacitors, we can more easily provide transient power for high-speed digital ICs.

Finally, with the improved stack-ups of Figures 6 and 7, high-speed signals can change layers because all the signals are referenced to ground planes (in the conventional stack-ups, the signals were referenced to either a ground plane or a power plane). As a result, we can place a plane-to-plane via close to a transition via to provide a low-impedance path for the return current.
 
Top