Optimal Distribution of Vcc in a 4-Layer PCB Design

[George]

I’m currently in the process of designing a 4-layer PCB for a GPS tracker. I’ve allocated the 2nd layer for ground and the 3rd layer for Vcc. While I understand the benefits of having a dedicated ground layer, I’m uncertain about the best approach for distributing the positive supply on the 3rd layer. Should I cover the entire layer with the supply? Or would it be better to pour Vcc only underneath the Vcc pins? Any insights or recommendations would be greatly appreciated.

[allank]

If you can you almost always want to create as close to a full plane as you can. The easiest way to look at it is to think of the ground plane as a sheet of metal; then think of your power plain as a sheet of metal, then think of your dielectric as an insulator. 2 sheets of metal separated by an insulator is the definition of a capacitor. Larger area equals more capacitance, larger capacitance means tighter coupling, less noise, lower loss - I think you see where I’m going here.

[myrtlee]

It’s contingent upon the noise level of your power plane. If your power plane isn’t excessively noisy and isn’t carrying high-current voltage, covering the entire layer with Vcc could be feasible. Additionally, employing adjacent ground and Vcc planes on consecutive layers is advantageous. This configuration fosters capacitance between layers, effectively serving as a decoupling capacitor.

[jonathan.lloyd.riley]

You might find it useful to see the comments I made in this thread and the explanation for them as this relates directly to the concerns raised here. Follow the link and look for my reply.

Ground Pours considerations

If EMC matters, it is much better to make both of the two inner layers to be GND, and route the power on the signal layers. When you use copper pours on the signal layers they will now be to lower the impedance of the Power tracks. The reason why you want the two planes to be GND is because this is where the displacement currents from your signals flow. If your signals never change layer (top to bottom, or vice versa) it makes no difference what voltage is present on the plane, but the moment yo…

[BerndKruger]

It mainly depends on what you connect to the VCC. If noise travels backward from the circuit to the VCC plane, it’s preferable for that noise to be directed toward the VCC regulator than other circuits. Consider a scenario where a 5V layer is connected to a 3.3V switch regulator and 5V logic. In the event of noise generated by the 3.3V regulator, it’s undesirable for this noise to affect the 5V logic circuits. However, the optimal solution involves addressing the noise source and implementing individual decoupling for each integrated circuit supply.

[realke]

Planes are commonly employed to ensure the availability of return paths for fast signal transitions, EMI control, and to achieve clean signal waveforms. When fast signal transitions occur, particularly with logic UP edges, the logic VDD experiences high currents, necessitating the provision of return paths.
To address this, you can utilize small ceramic capacitors positioned locally from the VDD pin of the integrated circuit (IC) to the ground plane. In my opinion, this eliminates the need for a dedicated VDD plane. However, it requires some thoughtful consideration and the plotting of return paths. By investing effort into this process, you liberate the “VDD plane” for numerous other valuable purposes.