Multi-layer layout and return currents of high-speed signals

I am planning to use the following layer stackup for my 10-layer PCB:

Layer 1 - Components / Short traces / GND
Layer 2 - GND
Layer 3 - Signals (vertical)
Layer 4 - Signals (horizontal)
Layer 5 - PWR / GND
Layer 6 - PWR / GND
Layer 7 - Signals (horizontal)
Layer 8 - Signals (vertical)
Layer 9 - GND
Layer 10 - Components / Short traces / GND


The distances between the layers are not symmetrical and the thicknesses of 142.1 um and 124 um are alternated (this is given by the PCB manufacturer).

What has troubled me is what the reference planes for the return currents for high speed traces in layers 3, 4, 7 and 8 will be.

Let's take for example layers 3 and 4. They are between a GND plane on layer 2 and a Power plane on layer 5.

As it is well known, high speed signals will have their return currents on the trace's reference plane, following the route of the trace.

So in this particular case, will the return currents use layer 2 or 5 or both? Is the distance between the signal and the reference layers of any importance at all?

The background of the question is my concern regarding the power planes of layers 5 and 6. Since, naturally, there are many different power supplies, there is no such thing as continuous reference plane on these layers. So the question in the context of the return currents is, should I try to bridge the gaps with capacitors or I shouldn't care so much about it?

• What specific high speed signals do you have? Reflections may or may not be an issue (for small values of reflection). – Peter Smith Jan 16 '18 at 9:17

1 Answer

What edge rates are we looking at here?

Return currents will flow in both 2 & 5, split in direct relation to how close the signal layer is, so you will want to bridge gaps with caps, but remember that a via typically has a 1nH inductance, before you consider the added loop area, this is very much inferior to a solid plane.

I would note that asymmetric stripline is something that layout tools sometimes have trouble computing impedances for, you may have to do this manually.

I normally work on the basis that anything with fast edge rates runs close to a plane on at least one side, and if I must have a signal layer without an adjacent plane (or with one that is chopped up) it is only used for low speed stuff.

Further it is worth defining the stackup such that internal high speed signals are very much closer to the reference plane then they are to any plane that is cut up, custom stackups are a very standard sort of thing by the time you are looking at a 10 layer board.