How to configure 4 layer pcb

[seyyah]

4 layer pcb

I will route a 4 layer pcb. It is not an rf pcb it contains mixed signals and small analog signals. I could not decide how to configure the layers; what should be on each layer? Can you advise me?

 

[obinobi]

internal layer gnd vcc frequency

Hello
Below is my proposal

Top layer - routing for high speed signal
First internal - solid ground plane
Second internal - power supply layer
Bottom layer - ground plane + routing

Advantage of these solution is good power decoupling. Disadvantage is that high speed signals are not shielded by two ground planes.

What is the biggest frequency of in your circuit. Are you able to determine rise and fall time of digital signals.

Best regards

 

[seyyah]

pcb supply 4-layer design rules

10 MHz is the biggest frequency.

 

[obinobi]

4-layer pcb layout gnd signal

Hello
So I think that you may use configuration proposed above. If you think that you will have problems with radiated emission (in case of plastic housing) you may route noisy traces on third layer. But remember about having a proper distance from noisy tracks to power planes. Distance should be bigger than distance to neighbouring layers (first internal and bottom layer).

Best regards

 

[Gundam001]

pcb power plane 4-layer

Don't forget to add a ground sheild on the noisy signal, so that it will minimized the emission.


-----------------------------------

https://pcb1001.blogspot.com/

 

[pcbdesigner34]

routing power pcb 4 layer

This is a good reference for you.

http://referencedesigner.com/tutorials/si/si_04.php

 

[Evel]

power signal layer mixed pcb

top
L2GND or L2VCC
L3VCC or L3GND
Bottom

high speed signal can routing in top(when L2GND) or bottom(when L3GND).just reference to GND plan,

For EMI, you need keep 20h rule. the power plan need smaller 20h than the GND.

For Mixed singal, you need use the moat for different signal's isolation

some time we need use the EMI cap to across the moat, and analog signals need come out from one gap area.

For impedance control, you need device to singal ended and differencial pair, and the pair signal should be refer to GND plan.

10 MHz is not so high, so you can make sure the power plan is a GND around the power, and all GND is better.clock signal need to routing in a reference to GND plan too.

that's my experience for these year's PCB layout,any other good idea will be given by next friend,hope wish you a whole success on your project process.

 

[obinobi]

4 layer pcb recommendation

Hello
I just want to share with you some information about 20-H rule. You may find in the internet some documentation which describes 20-H rule and impact on radiated emission. Some simulation and measurements show that in some cases such power plane topology may increase radiated emission.

Some examples below

**broken link removed**

But it doesn't mean that using 20-H rule is something wrong.

Best regards

 

[gasper]

analog digital 4 layer pcb

4layer is not difficult to route, only two standard types.
1, Signal, VCC, GND, Signal
2, Signal, GND, VCC, Signal

But if you have any BGAs, I think you must use second layout to route signals.

 

[Tanticle]

gnd vcc layer order 4 layer

Hello,

i accompany obinobi's proposal.
Locate the ground plane next to the component side of the board.
One important aspect is to minimize the ground bounce on any of the signal traces, equal if analog or digital.
In upmost cases GND / 0V is the reference level for analog and logic signals.
Therefore all gnd-referenced components should have an optimum contact to this potential.
To avoid unwanted impedance, this means as short as possible vias to the GND plane.
One can imagine, that a via with a length of 0.3mm/12mil (L1->L2) has much less impedance than that one with a length of 1.3mm/51mil (L1->L3), thus leading to less voltage drop when charged with "high" (but slow) currents or fast rising currents.

As practice has shown, ground bounce problems occure more frequently than estimated.

Good luck with your design!