Optimal Grounding Strategies for High-Speed Signals in Two-Layer PCBs

[Charles]

I’m working on a two-layer PCB that includes high-speed signals with rise and fall times as short as 3ns.

Research suggests that effective grounding is crucial for improving signal integrity and minimizing EMI. To reduce the impact of displacement current and crosstalk, it’s recommended to route a ground element alongside each high-speed trace. This could be a ground plane beneath the trace or a ground trace adjacent to it (please correct if this understanding is incorrect).

Would it be more effective to have both layers serve as ground planes? A ground plane ensures a nearby return path for most signals, and incorporating stitching vias can further enhance these return paths.

Are there additional benefits to having both power and ground planes? This approach can increase decoupling capacitance.

When referring to having two ground planes, the meaning is Signal-Ground/Signal-Ground. When mentioning one power and one ground plane, it means Signal-Power/Signal-Ground.

[Sophia]

A 2-layer PCB might not be suitable for high-speed signals when dealing with complex designs that utilize modern, small surface-mount chips. With a 2-layer PCB, it can be challenging to dedicate separate planes for power and ground unless the design is quite simple. The distance between the ground plane and signal traces is significantly greater than on a 4-layer PCB, which can negatively impact signal integrity.

In your design, you will likely need to use series termination resistors at least on the source end of the signal traces to minimize ringing. This will require precise measurements on a prototype board to manually optimize the component values.

Having two reference planes is always beneficial, whether that’s a ground and a power plane or even multiple ground planes in a multi-layer design. The key strategy is to “short” these planes together at AC by distributing small coupling capacitors across the board. Think of it as adding a few capacitors on the boards. These capacitors would be placed between the power and ground planes, independent of any decoupling caps next to the chips. These capacitors provide the distributed capacitance needed to ensure the power and ground planes effectively route the return currents of high-speed signals.

[eduardo.mateos]

I agree with Sophia. If you can afford a 4 layers PCB everything is easier and much better. Keep in mind that the 50 ohms tracks can be quite wide if you use a typical 1.6 mm thick PCB. For example using a 1.6 mm thick FR4 PCB (standard), tracks have to be 3mm wide to get 50 ohms. This is too much. IC pads are much more thin and you will need some artefacts to adjust a 3mm track on a 0.5 mm pad.
If for any reason you muss use a two layers PCB then the correct stack up is: Signal/power-GND.
A power plane is not a muss but routing is much easier.

[jonathan.lloyd.riley]

Two layer PCBs for signals with fast edge rates are always tricky, but can be done. With 3ns rise and fall times, EMI is usually the biggest problem; when they’re faster than 1ns signal integrity tends to dominate your list of worries.

At least one layer needs to be reserved for a ground plane. It might be useful to mention that displacement currents are those currents that flow in the part of the ground plane that is immediately underneath the signal traces. They match the current flowing in the signal path except that the direction of flow of current is the opposite of that in the signal itself.

Your biggest concern is that you know where the displacement currents are because spreading displacement currents are one of the key things that give rise to both EMI and signal integrity problems. The first factor is the separation between signal and plane, the closer they are, the better defined the location of the displacement current is. When you have a 2-layer PCB with a 1.6mm separation, typical thin PCB traces will be much more narrow than this separation and so the displacement current will spread over a wide area relative to the trace width. The best plan here is to make the board thinner. As long as the board is not very big, there is enough mechanical strength in a 0.5mm thickness board for most applications. It represents a change from 16:1 (height to width) down to 5:1 which is a big step in the right direction. Thinner would be better, but it soon gets to be too delicate.

The second issue, and really it is this one that is the killer, is when you have splits in the ground plane, because now the displacement current has got to work out a way round the obstruction, and this is the main thing to worry about from an EMI point of view. The bottom line is don’t put splits in the plane, you’ll regret it when you do the EMC testing.

Putting ground traces on both sides of the signal trace is done to try to reduce crosstalk. But it only works if you stitch the ground traces into the planes at regular intervals (usually 2-3mm apart). Failure to do this simply means that the aggressor pumps energy into the supposed ground trace and excites it to resonance and it becomes a very good radiator of certain frequencies (+ harmonics).

The question about trying to make the signal side double up as another ground or power layer in the spaces that are unused for tracking is a good one. The benefit of filling empty space with power in the hope of getting capacitance from the PCB sounds good, but tends to be underwhelming. When we have buried capacitance in multi-layer PCBs these normally have a separation of between 50um to 100um. A 1.6mm two-layer board has a separation of 1600um, so it can only give somewhere between 1/16th to 1/32nd or so of the capacitance a multi-layer board provides. This makes it not worth the bother. For once, if you want an extra 200pF of capacitance at your power pin, just buy a small ceramic capacitor. Filling the space with GND does help if you remember to space out the traces allowing room for the stitched-GND traces in between (note that if these had been power not GND, you couldn’t stitch with just vias, you’d have to add capacitors as well, because the voltages would not be the same).

Finally, having explained why you want routed power and a solid ground plane, we come to the options listed at the end: signal/GND - signal/GND, or signal/Power - signal/GND. The second of these two is a non-starter. But in fairness, the first option is not much better. The best option is signal/GND - GND.

The reason for this is obvious - do not split the GND plane with tracks. Unless there is a very compelling reason, this ruins the EMI performance of your design. One fast-edge signal crossing whose displacement current path has been broken will radiate in a big way.

Where does this leave us?

1. Golden rule for two-layer boards - one layer is a plane, resist the temptation to route signals in it.
2. Treat power as though these are just more signals (but the trace can be a bit wider).
3. Keep all signals on one layer.
4. If you must cross over signals, consider using resistors rather than trashing the ground plane.
5. Make the board thin. Forget 1.6mm, try 0.5mm (this was the defacto standard thickness for PCMCIA cards, so it is well known technology).
6. Even a 0.5mm board is too thick for controlled impedance traces without them becoming very wide. All the impedances will work out on the high side, so trying to do Ethernet or USB on a 2-layer PCB is practically impossible. There comes a time when 4-layer boards become the only sensible answer to problems.