Question about proper PCB stack-up

Question

I've got some question about stack-up for 4 layer PCB.

My design is rather simple but due to many connections all arround PCB it couldn't be made with 2 layer PCB, this is why I picked 4 layer board.

My PCB is 1.6mm thick, with 1oz copper on all layers (incl. internals).

I'm using 1st layer as a power/signal layer with some locals ground pours that are connected with multiple vias to inner ground plane (which is 2nd layer // and whole 2nd layer is big ground pour without any slots [excl. vias clearance]).

Question is should I use 3rd layer as a power/signal and 4th as a big ground pour? Or should I swap it and make 3rd layer as a GND and 4th as a signal/power.

Due to many connections it's not possible to place power only traces on 3rd layer and signals on 4th because there will be some slots here and there and it will make my current loop alot longer, this is why I combined power and signal to one layer. From mechanical point of view 1st and 2nd layer are adjacent do each other, similiar for 3rd and 4th.

I'm very curious which option could be better for me - I hope some of you might help ;)

PS: all component pads are located at 1st layer, there is no MCU's or any other high speed signals like clocks etc. PCB is mostly occupied with power IC's like supervisors, LDO's and some audio stuff.

Answer 1

I would go with this :

1. Signal - Power
2. Ground
3. Power distribution & ground
4. Signal - power

Signal on top is obvious, it is to avoid vias as much as possible.

Ground on layer 2 is obvious too.

I usually use Layer 3 for power distribution, it helps a ton to keep the signal layer as clean as possible, and allows optimal routing of power traces.

I try to avoid inner signal traces, it makes debugging & rework much harder than needed, so layer 4 is for signal.

Answer 2

Question is should I use 3rd layer as a power/signal and 4th as a big ground pour? Or should I swap it and make 3rd layer as a GND and 4th as a signal/power.

It is usually better to put the a solid GND on one of the inner layers.

1) it facilitates a nice ground plane and creates a small amount of capacitance between the traces on the outer layer, which is nice for high speed signals and transmission lines. 2) A solid ground reduces common mode noise from return currents. If you ran a network of traces the resistance in the traces could create a voltage noise from switching current or large currents. Because of this we use a nice big solid plane that lowers the resistance between all components connected to it.

It's also a good idea to have large traces for power, reducing resistance and inductance. A better idea is to have planes.

It's really up to you how the layers go and what kind of design it is. The best way is to use a PCB trace calculator to give you an idea of what the resistance and inductance is of the PCB copper.

Some designs must use shielding, and use grounds on the outside and power and signal on the inside.

The typical stackup looks like this:

1) signal
2) GND
3) Power\Signal\GND
4) Power\Signal

Answer 3

it's not possible to place power only traces on 3rd layer and signals on 4th because there will be some slots here and there and it will make my current loop alot longer.

Try this:

1 : Components, short traces (10 mm or less, say)

2 : Power

3 : Ground

4 : Any length traces

By using 1 and 4 as trace layers; and 2 and 3 as plane layers you make a symmetric stack-up which is less prone to warping.

By putting your ground on layer 3 and long traces on 4 you avoid routing long traces across the slots in your power plane.

By restricting layer 1 to short traces you avoid routing long traces across the slots in the power plane. In any case it's often difficult to route long traces on layer 1 due to components getting in the way.

In this scheme, "traces" can include both signal and power routing, but of course you'll want to minimize the use of traces for power to keep the inductance low.

Answer 4

I use either

1. Signal
2. GND
3. Power
4. Signal

as that gives me easier access to signal traces for rework and debugging and simplifies the routing, or

1. Signal
2. Power
3. Signal
4. GND

if I either have lots of thermal vias (which are connected to a GND pad on most components) or lots of impedance controlled signals (because I can pack them a tiny bit tighter if they are between two planes).