# Ground in PCB 4 layers

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?

• don't waste a layer on VCC Sep 9, 2020 at 21:02
• The selection of your layers is unconventional and does not provide any info why such unconventional selection is made. Usually VCC and GND layers are the two center layers. Sep 9, 2020 at 21:03

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.

• What do you do in case where you need to have different voltages on the board? For an example 5V and 3V3 power and DGND for digital stuff and separate 5V and 12V power and AGND for a analog stuff? Sep 9, 2020 at 23:11
• It gets messy, you end up with some combination of splitting planes and/or routing power on signal layers, but you have to be really careful about current return loops. You generally don't want to route a signal across a gap in it's corresponding reference plane unless that gap is bridged by a capacitor or it's a very slow signal. Sep 9, 2020 at 23:14
• If possible, split the plane into 5 and 3v3 regions. If everything needs all voltages you might be forced to add more layers or route power on the signal layer. Sep 9, 2020 at 23:16
• @PeterGreen, the OP also asked if it was advisable to fill the unused areas on top layer with GND plane? Sep 10, 2020 at 9:22
• Is there any particular reason why you wouldn't have the signals on the inside? Ease of debugging? Extra isolation between the two signal layers? Sep 10, 2020 at 10:47

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.

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.

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

• Guys: Thanks for the help but seems that there are several options to design and no "cookbook". The thing that makes me quite confusing is : 1- Can I use the power plane and fill with ground ? 2 - Also if you have a complex circuit that you need to route in more than two layers, what can I do if there is not enough room to separte things ? Increase the number of layers ? Sep 17, 2020 at 19:34