General questions about 4 layer pcb design

Thread Starter

tesla000

Joined Jun 12, 2021
9
So i made a few 2 layer pcb's and now i wanna try a 4 layer one, i searched on the internet, but i found some conflicting information, so signal traces are on the top and bottom, power traces on the inner layers, is this correct?
So one inner layer can be a ground plane, and the vcc one also better to use a plane or just traces?, harder if there are different voltages.
Also what are useful tips to avoid emi and other interferences, because almost every pcb i made had a noise problem
Decoupling caps on signal traces?, Shortest possible trace lenght and short current return path?, adequate distance between traces?, rc/lc filters?
 

MrChips

Joined Oct 2, 2009
24,222
It depends on the requirements of the board and design.
Frequency? Mixed signal? Current? ADC?

Power plane and ground planes on inside.
Separate ground planes for analog and digital.
No decoupling capacitors on signal traces.
Pay attention to byte/word sized buses and drivers.

We cannot provide more advice without seeing the schematics.
 

ronsimpson

Joined Oct 7, 2019
1,472
You can do almost anything you want with 4 layers.
On boards that must not emit RF into the air, I put ground and power on the outside two layers and hide the signal trances on the inside to form a shield around the traces. More often I have power and ground on the inside.

My last board I have three different grounds. There is a small area for +3.3V, a large 5.0V and a large 1500V on one layer. The 3.3V and 5V share a common ground. The 1500V has it's round under the supply.

There must 100s of ways to do this and every one will tell you their idea.
 

Thread Starter

tesla000

Joined Jun 12, 2021
9
For the pcb i am trying to reroute as a 4 layer it's an electronic load i made, it's made for around 15A max current, it has 4 mosfets controlled by an opamp which is connected to a 62.5kHz pwm pin that passes through a rc filter, rotary encoder, oled display, thermistor and ch340 chip for uart communication, so separate ground planes for digital/analog and for different voltages, why no decoupling capacitors on signal traces?, aren't they usually used(10nF or less)?
 

Thread Starter

tesla000

Joined Jun 12, 2021
9
And at approx. what frequency is this slowdown noticable?, so what is recommended to decouple noise from signal traces?
 

eetech00

Joined Jun 8, 2013
2,576
And at approx. what frequency is this slowdown noticable?, so what is recommended to decouple noise from signal traces?
The idea of decoupling (bypass) capacitors is to stiffen the supply voltages to keep the voltages stable.

Your board doesn't sound like is has high component density. Why do you want a four layer board?

You can reduce noise on a two layer board design by:
1. route +V supply(s) on top layer.
2. route signal traces on top layer.
3. route "less critical" signal traces on bottom layer only if absolutely necessary.
4. use ground planes on both top and bottom layers.

parasitics between the gound plane(s) and V+/signal traces help reduce noise.
 
Last edited:

Thread Starter

tesla000

Joined Jun 12, 2021
9
Well it has 79 components so i barely made in in 2 layers, i also want to make it in 4 layers to learn for future projects, by power plane you meant like this, this is the +12V plane?, don't mind the component layout because this is just a practice pcbexample.png
 

eetech00

Joined Jun 8, 2013
2,576
Well it has 79 components so i barely made in in 2 layers, i also want to make it in 4 layers to learn for future projects, by power plane you meant like this, this is the +12V plane?, don't mind the component layout because this is just a practice pcb
If you mean the "green" plane, yes. The remainder of the top would be used for signal traces. Then apply a top ground plane for remaining ground connections. Also ground plane on bottom with a small number of manually placed vias to connect the ground planes. The bottom ground plane and top signal/power layered above and below each other creates a parasitic capacitance that helps reduce noise.
 

ronsimpson

Joined Oct 7, 2019
1,472
Like the power layer. Ground looks good.
Right side there are two high current traces. You can add traces in the top layer in parallel. I have some 100A traces and I use all 4 layers for that.

Does the voltage regulator get hot? Copper is a heat sink. You can increase the copper area to reduce the heat. Also add more VIAs to the ground to connect the regulator ground to ground layer better. Also pulls heat away batter.
1626352634351.png
I noticed you lined up the parts in nice rows. I deal with high frequencies and need short traces. I moved a component to get rid of the trace length. (makes the board easy to layout) Also the IC need to get power from the bypass capacitors to run so I connect directly from pin-16 to the capacitors. Leave the VIAs. (don't change these now, just for next time)
1626352981899.png
The board looks good. Nice job.
Looks like you have a USB IC. Usually, in the data sheet, there is a guide on layout. USB signal traces should be like a transmission line. (if there is any length) I keep those two traces very short. I turn the IC 90 and push the IC up against the connector so the length is very small. What you did is ok, just saying to read the data sheet on the ICs. There are USB layout examples and often examples of how to do the ( capacitor + crystal + capacitor ). On the USB and the micro the crystal and caps and the ground pin should be a small loop.

Every person has a different way and don't worry to much.
Ron S.
 

Thread Starter

tesla000

Joined Jun 12, 2021
9
Thanks for the detailed reply, what about let's say 10 layer pcb how are the layers devided there, just more signal and power planes in between? or does it depend on the application?
 
Top