Rule for 4-layer routing

Layout
1

Hello,
I’m a beginner, how do you route in 4 layers ? Can I reserve layers 2 and 3 for power supplies and ground? What is the general use of layers 2 (In1.Cu) and 3 (In2.Cu) ?

image
image880×372 100 KB

2

With 2 layers I use one layer 100% for GND.

When I can’t connect everything at one layer (with GND at second) I use 4 layers. But I have both inside layers as GND.

If you have In1 as GND and In2 as VCC then when fast signal track jumps trom top to bottom the return current jumps from GND to VCC. Because of this near each via on your signal track you should have capacitor blocking VCC to GND layers, while having both them GND you need only a GND via.
If you don’t have fast signals then it is not a problem.

1 Like
3

I like the Sig/PWR - GND - GND - Sig/PWR stackup as well with 4-layer boards. One additional benefit is the PWR/GND spacing is generally much closer than if PWR - GND are on layers 2 & 3, so it makes a better high frequency capacitor.

If you:

  • route traces mostly in one direction on the top and the other direction on the bottom layer
  • pour PWR on top and bottom
  • pound some vias to connect top/bottom PWR pour

You can reach most areas that need power pretty easily with a copper PWR pour on top and bottom because the cuts caused by the traces are in opposite directions. KiCad will tell you if you if anything is not connected.

image
image926×845 90.1 KB

In case it is not obvious, to create a GND plane on a layer, simply draw a copper pour that fills the layer, and attach it to GND.

I’ve collected some notes here:

4

Sorry, I don’t quite understand what you mean ? Is the return current annoying ?

5

Not sure exactly what your KiCad related question is ? can you explain please ?

6

It can be. The best thing I learn was to concentrate on the return path/current than on the real net.
DC and Audio type AC will flow “as the crow flies” with regards to the return current. However, faster edges (ie digital edges) will want to have the return current under the trace (ie Vcc or GND). This makes sense as this will be where the inductance is the lowest. The return current will look like a gausian curve under the trace and this is also where the rule of thumb of 3W comes from to minimise cross-talk.

When it comes to stackups like this, H.Ott is the GOAT
https://hott.shielddigitaldesign.com/techtips/pcb-stack-up-2.html

if you are concerned about EMI you cannot go wrong with this as a 1st pass consideration

2 Likes
7

Not annoying, but it is a key parameter in PCB design. You could say that PCB design is about optimizing return current paths.
Every current flows in a circuit. The emission from the circuit and its sensitivity are determined by its surface. When the return current flows exactly under the track, the surface is determined by the distance between the track and the GND layer (which is why In1 is better as return path than bottom). In times when everyone carries a mobile phone, even circuits with audio signals must be designed as RF circuits.

1 Like
8

Thank you for this for this explanation, I understand better but I don’t master everything but I think that it will come with time…

9

Thank you, I’ll watch this video later

10

Thanks for the link!

11

In 2020 I have linked here articles that I believe are worth printing and reading with marker in your hand: