# Four layer PCB with dual supply (12V and 5V) and signals

I'm designing a PCB which controls 4 motors (400mA peak) with H-bridges, a Bill-Validator (using UART to communication) and drives 4 LEDs using 12V dc.

On my 5V power I have a microcontroller, 4 current sensor analog signal (for the motors). I have 1 UART RS-232 (9600 baud), 1 UART TTL (9600 baud), 2 I2C (100 kHz), 8 I/O for free use (only with pull-ups), and 8 inputs with pull-ups and bypass for switches.

I've just decided to use a 4-layer PCB using the following stack-up:

1. Signal
2. GND
3. POWER
4. Signal

The components are located only on the Top Layer.

However I'm not sure about the POWER plane and how I can layout the signals, so I have some questions:

• Shall I use the same POWER plane for 12V and 5V? How can I divide the power plane? 12V and 5V come from different power supplies but they have the same ground.

• How can I separate the signals? Shall I use the top layer for communication signals and analog signals, and use the bottom layer for inputs, I/O signals and H-bridge signals? I don't know how I can separate the signals in 2 layers.

• It sounds to me like you don't need more than two layers. Why complicate things? Commented Oct 28, 2016 at 5:02
• With a 4-layer I can have a better grounding. Commented Oct 28, 2016 at 5:20
• Your English is fine. What are the the board dimensions?
– Rev
Commented Oct 28, 2016 at 6:28

First, the signals

It doesn't make much sense to try to segregate the signals by assigning them layers depending on their kind. The fact you have two layers for the signals allows you to make crossings. If you have a lot of digital signals, for example, you need two layers to route them efficiently. So, use both signal layers for all kind of signals.

What makes sense, however, is to separate the circuit in blocks of different type (high power, digital, analog, ...) and put them on different areas of the PCB, to minimize intererences between sensitive blocks (e.g. put noise-sensitive analog signals far from switching regulators, ...). Also choose the locations of all these blocks so that you minimize the trace lengths between blocks.

Now, the power planes

Whether you use the same layer for 5V and 12V (with a split plane), or use one of the signal layer to have them on different layers is not that important. There is one big rule to follow, however: avoid signals that cross a split plane (especially high-speed signals): that would create unwanted EMI.

Check what makes sense in your specific case: if the 12V is used only in circuit parts that do not use the 5V, use a split plane. If the 12V is used only on a few nodes, but in circuit parts that also use 5V extensively, use the whole power plane for the 5V and route the additional required 12V traces on a signal layer (you don't even need to use a plane, actually).

The only thing is that, if you use the whole power layer as a 5V plane and have a large portion of the signal layer on top of it with an additional 12V plane, there will be capacitance between them. So if there is noise on one of the supplies, it may couple on the other one. So maybe avoid that.

My feeling

Your design doesn't seem to be very sensitive. I don't see very high-speed signals, you didn't mention switching regulators, ... So actually, anything will do. Just follow you gut feelings and logic to make choices (minimize trace lengths, organize blocks efficiently, ...), and it will be fine. And probably Roger Rowland is right in his comment: two layers would most certainly be enough. You suggested that 4 layers allows for "better grounding", but there is no point in making the ground "better" (whatever that means) than required, especially if it costs 4 times the price. Careful layout with gridding the planes on the two layers would for sure provide a good enough ground in you case.

Here is a document from TI giving good advices (and in particular the ground gridding explanations in chapter 2.2.3).