A small PCB Stack Up for High Speed

Question

I design 2 PCB's. They are connected with a connector.

First one is PCB1, has the size of 50cmX10cm , the other one is PCB2 and has the size 2x5 cm.

Through this pcbs and connectors some communication channels are travelling, which operates around 300Mhz.

Therefore, I have selected for the longer one a 6-Layer pcb stack up, in order to keep communication stable enough. For the 6-Layer PCB1 I have the following stack up:

In PCB2, I have basically only the connector and all the signals are travelling through. I want to still keep same 6-Layer stack up. But within this size+connector I can not take communication channels inside the Layer, so they stay on top. As far as I know, 6 layer brings the advantage , since we encapsulate the signals with ground references from top and bottom.

Therefore, I could basically live even with 2 layers for PCB2.

But, should I now worry about the communication reliability ?

Answer 1

TL:DR 300MHz isn't really that fast. Signal integrity will be fine, but EMC may be an issue.

Your looking at 300MHz, which isn't that fast. Assuming you're looking at single ended signals, rather than LVDS, and you have some reasonable checks in place on the communication, I can't see why you need to worry about a 6 layer for that, a four layer would do the job (for SI, clearly you may want 6 or more layers for routing).

You talk about putting ground references top and bottom on the signal. There is no need to do that, only one layer will be the reference. With good design you should be able to work out which it is, and so reduce layer count to 4.

The wording of your question makes me think you are looking at this purely from a SI point of view. While SI is important, the main reason to consider the reference plane is EMC. Without considering your reference planes it's easy to design even a slow(ish) PCB which radiates massive amounts of EMI, and thus becomes unsalable in many markets (different areas have different radiated emissions limits). If you are doing this for a home project, EMC issues can be ignored, or at least left alone for now. If you are making a product to sell, then it IS a problem.

Don't forget that the signals will still be using a reference plane when they go through the connector, and that can completely muck up your plan.

Second "don't forget": if the distances on these signals on the PCB are short (relative to their frequencies) then any kind of reference planes is irrelevant.

You are worrying about this more than you need to from the sound of things. I would recommend an EMC design course to clarify these points (I've been on a couple in the UK, both were useful).

Answer 2

But, should I now worry about the communication reliability ?

If the signals are less than ~50Mhz, then no, since yours are faster than than, you may want to worry about it.

If the PCB design has impedance controlled transmission lines in it, then they most likely need a reference plane. The reference plane can have larger spacing (between the middle layer if you want to run a two layer design, but this will affect the trace size. Use a PCB trace width calculator

If there isn't transmission lines on the PCB, then it probably doesn't matter, with the exception of a few more 0.1pF's of capacitance between layers. The last thing to think about is noise. If the design needs to pass FCC testing or equivalent (like unintentional radiators) then it may be good to have shield planes for electromagnetic control.

In your case, I would probably stick with more than a two layer design, since the design most likely has impedance controlled lines. I would also consider the size of the board since you could also be creating an antenna with PCB2, which would depend on the size of the PCB.