Ground in PCB 4 layers

Question

I'm designing a PCB with 4 layers, but I've seen different recommendations about layer distribution. I'm considering that:

Top layer - Signal + short traces of VCC
2nd layer - Signal
3rd layer - VCC
4th layer - GND

Can I fill all area around with ground in each plane and place several vias to connect grounds across the layers? Can I have the VCC layer filled with ground plane?

The circuit has a nordic + lora radio in one module castellation. Output antenna has a connector over the module already, so no need to design microstrip lines.

What is the minimum recommended power trace width for a 3.3 V and 150 mA maximum? Shall I have very large traces in 3rd layer and not filled with ground around?

Answer 1

Your stackup is a poor choice in most cases.

Most 4 layer stackups are like

Top
thin insulator
Mid 1
Thick insulator
Mid 2
Thin insulator
Bottom.

So your stackup places your signal traces far away from any reference plane.

The most common arrangement would be to use mid1 for ground and mid 2 for power, this means that all signal traces are close to a reference plane, but it has the downside that you can't just couple the two reference planes directly with a via, but instead they can only be coupled through a capacitor. This impacts signal integrity when a signal changes planes.

Another option would be to use both mid1 and mid2 for ground. This would allow better signal integrity on reference plane changes, but would mean your power would need to be routed on a signal layer.

It can make sense to swap the layers around, for example if you want EMI shielding on the bottom then you might put the ground on the bottom, ground or power on mid1 and signals on top and mid2 but you should generally always have one signal layer and one power/ground layer in each pair.

Answer 2

Here's a good starting point:

1. Top layer - signal, components. The radio communication components should go on this layer.
2. Inner layer - ground plane
3. Inner layer - power plane
4. Bottom layer - signal, components

It may be possible [or even necessary] to deviate from that arrangement. That would depend on the purpose and schematic design of your device.

Answer 3

You need to put the signal layers on the prepregs and the power planes on the core. Otherwise you cannot reach the most common impedances of 90Ω and 100Ω for your differential pairs, and those for your antenna most likely neither.

Answer 4

Signal, Ground, Power, Signal is the most common 4 layer board stack up. In many cases when this is used the power plane acts like a return plane for the signals on the bottom layer.

Ideally not all the layers are equally spaced depending on what you are trying to accomplish. Remember engineering is always a trade of something for something else.

Something to ask yourself is how important is the decoupling of your 3.3V to Ground? Is it most important to protect your wireless signal from radiation?

See the link below for some 4 layer board combinations and the trade offs. http://www.hottconsultants.com/techtips/pcb-stack-up-2.html