Managing Ground Planes in Compact 4-Layer PCB Designs

Design and Layout
1

I’m looking for advice on handling ground planes. Is it better to designate both internal ground planes with the same net (a unified GND), or should I separate them into DGND (Digital Ground) and AGND (Analog Ground) and use a net tie to connect them?

I’m working on a compact 40x30mm PCB with a 4-layer stackup (signal, ground, ground, signal). Digital signals are on the top layer and analog signals on the bottom, with power routed on the signal layers. My main concern is managing ground planes effectively, particularly with a sensitive component like the AD7124 on the bottom of the board.

My main concern is keeping the design straightforward and minimizing the risk of introducing noise due to unnecessary complexity. I’ve have come across information about splitting a single ground plane in the XY direction but haven’t come across much guidance about using different nets for two ground planes in a 4-layer design. Would separating the ground planes be appropriate for my setup, or should I stick with a single GND net for simplicity?

2

To manage ground planes effectively, focus on ensuring that return paths for digital signals and noise-inducing nets, such as switch-mode power supplies, do not intersect with the analog signals feeding into your AD chip. Simply splitting the ground planes and connecting them with a net tie won’t inherently improve or harm the design—it depends on how the return currents are managed.

If the design is well-engineered so that all noisy return currents are isolated from the sensitive analog sections, it won’t matter if the ground planes are unified, as the currents won’t interfere with one another. However, if the return paths are poorly planned, the currents will naturally follow the path of least impedance, potentially crossing into sensitive areas. Stitching GND vias along the boundary of the ground planes can help shorten return paths and reduce noise. Without these stitching vias, introducing a net tie at a single point could force return currents to travel through the analog ground (AGND) to reach the digital ground (DGND), introducing noise into the AGND plane. Using a ferrite bead as a net tie in such a scenario might even worsen the problem by adding impedance to the return path.

For a compact board, isolating noisy digital components from sensitive analog circuits is challenging, particularly if the analog section operates at audio frequencies or lower. Implementing additional filtering may be necessary to mitigate noise.

If digital signals are on the top layer and analog signals are on the bottom, this is a solid starting point. Pay close attention to where the two domains meet, such as at an ADC. For example, at an ADC with SPI on one side and analog inputs on the other, ensure there are stitching GND vias near the signals crossing from L4 to L1. These vias will help maintain a clean return path for digital signals, keeping noise away from sensitive analog areas like power pins and signals.

1 Like
3

I agree with Will. You should focus on the return path. Also keep in mind if you want to pass a signal from layer 1 to layer 4 and give some return path continuity, close to the via you should add one more extra GND via connecting layer 2 and 3.

1 Like
4

As has already been stated in the two earlier replies, it is the return paths that really determine how good the performance is going to be. Putting the low frequency analogue on one layer and high frequency digital on a different layer is a good plan, but the moment you need to make either analogue signals cross over other analogue signals (or similarly digital crossing over digital) you need to route signals on the other layer, and the return plane changes and therefore needs stitching together at every place where this occurs. At this point the two grounds become one, and the intention to keep them separate must be replaced by the greater priority of keeping the integrity of the return current paths. Net result, there is only one ground and it is implemented on two physical layers. No plane splits. No separate analogue / digital grounds.

If you check up the writings of seasoned practitioners of signal integrity like Prof. Eric Bogatin (and others) you will see why the best advice is to just have solid ground planes (no cuts) and no attempt to separate so called analogue and digital grounds. This contradicts the suggestions given on many applications notes, but the bottom line is that many of these application notes that advocate dividing grounds and linking them at just one point are just plain wrong.

The reason why the digital signals, when their return current paths having been designed properly, work well (i.e. don’t interfere) lies in the fact that the displacement currents that are generated in the plane by the passing of the signal in the adjacent layer follow the signal accurately. The amount of energy in the plane that spreads away from the path of the signal is miniscule. Thus it does not come close enough to other signals to interfere. The only time when the displacement current can spread is when it wants to find a path to the other plane because your signal has just gone through a via. This means you must put ground stitching vias next to signal vias. At least one stitching via per signal via, but two is better.

The best way to maximise the intentional coupling between signal and return current is to minimise the separation between them. In your four layer board, make the prepreg thickness separating the top layer (signal) from the adjacent ground plane as thin as possible. Usually this will be in the range 50um to 100um. Obviously the board will be symmetric, so the same is true on the other side. Now the only figure you need is to pick the ground to ground separation to be whatever is necessary to get the overall board thickness where you need it to be. If you want a 1.6mm (1600um) overall thickness, then you want the ground to ground separation to be about 1300um if you have 35um for each copper layer.

If you have multiple analogue signals, don’t forget that they too can interfere with each other. In this situation, increasing the space between them will help, but on a small board such as you describe, this may not be easy. The normal advice is to put guard tracks between them. If you do this, it only works well if the guard tracks are well stitched into the ground planes with vias with a short interval spacing. Leaving out these vias will normally make matters worse than if you had simply left the space open and not put any copper there.

If, during your product testing phase the performance is not as good as you hoped for, don’t immediately blame the PCB. Look at the larger picture and see whether there might be issues with the wider product grounding strategy. Small boards are often intermediates between larger systems and when performance counts, these larger systems cannot be neglected; but this is getting into a far bigger discussion.

1 Like