Optimal Ground Plane Connection Methodd

[gigio]

What’s the most effective method for connecting ground planes together on a PCB?

I’m aware that connecting ground planes at various points helps maintain a low impedance ground across the entire board and establishes a return path for signals. However, I’ve come across different approaches:

• Adding vias close to every decoupling capacitor.
• Implementing a grid pattern of vias with a spacing of 1/20th of the maximum wavelength on the board.
• Placing vias along the traces.
• Scattering vias randomly across the ground planes.
• I’ve also seen a combination of these methods: vias along the lines along with randomly scattered vias on the ground planes.

What’s the recommended practice or the most efficient approach for achieving low radiation, good signal integrity, and power supply decoupling?

[allank]

I’d go for all of them (within reason). Each one of these techniques was created to solve a specific problem (more or less). As such, each will contribute to the best performance of your board. You want to step back, look at your design, and see where you think problems might occur. You don’t want to place vias randomly or saturate the board with them, especially on a small PCB. But if you see parts of the circuit where a clear path to ground is not obvious, these are the tools to fix that.

[JimJJewett]

@gigio

• Adding vias close to every decoupling capacitor.
• Implementing a grid pattern of vias with a spacing of 1/20th of the maximum wavelength on the board.
• Placing vias along the traces.
• Scattering vias randomly across the ground planes.
• I’ve also seen a combination of these methods: vias along the lines along with randomly scattered vias on the ground planes.

What’s the recommended practice or the most efficient approach for achieving low radiation, good signal integrity, and power supply decoupling?

What is your alternative that you think of as a default?

My assumption (feel free to correct me, or point out counterexamples) is that if you have enough layers for multiple ground planes, you have to tie them together somehow, and it might as well be near decoupling capacitors. You have to get the ground up to them somehow, and it would be strange if you had room for a long ground trace, but not room for a via. (Tying them together at only a single via to maintain “single point of connection” is maybe also an option, but it sounds like you’re assuming multiple connections.)

When you talk about “along the traces”, if you really mean “beside signal traces” rather than just “inside a ground trace”, then I assume that is a waveguide. Like the 1/20th grid, it should reduce interference in or out. I’ve seen it mostly on antenna feeds, and am guessing you don’t need it elsewhere until you’re working with very high speeds or very sensitive signals. But it shouldn’t hurt, either, unless you need controlled impedance, and forget to recalculate for the waveguide. Or if it eats through needed routing space on other layers.

I’m not sure what the point of “randomly scattered” is, except maybe “gotta connect it somewhere; plenty of room here.”

[gigio]

Yes, that’s perfect. I have often "scattered them where I had room. It is usually done for LF boards, just to keep a low impedance to gnd.

The important thing is to start with the obviously needed methods, then choose what efforts would get the best results with the least cost/effort

[myrtlee]

There isn’t a one-size-fits-all approach to grounding on a PCB. However, here are some insights that I would like to share. The approach to ground planes largely depends on your objectives. You might be aiming for low impedance paths, isolating different areas, or managing EMI. Doing it wrong can indeed lead to performance issues, but unless you’re working with high-frequency circuits or precision analog work, the impact may not be significant. You can gauge how well your grounding works by observing the number of fluctuating bits in an ADC reading with grounded inputs or the spectral purity of an RF signal measured by a spectrum analyzer. Achieving perfect grounding (as per datasheet specifications) is often impractical unless your system is as simple as the test circuits.

The most complex ground connection challenges arise with RF frequencies and signals that are either weak or susceptible to EMI coupling at those frequencies. At microwave frequencies, even a centimeter can act as an effective antenna and cause interference. I recall a professor mentioning that in the industry, they would leave several points where grounds could be shorted together and test each to find the best performance, particularly in high-frequency (microwave) circuits.

Typically, there are three kinds of ground plane elements you’d want to connect:

1. Real Ground Planes: You might have multiple ground planes and need to connect them. This is common in standard circuits.
2. Ground/Guard Traces: These run along signal lines, providing a return path or guarding a high-frequency signal, especially for signals to/from high-impedance sources or sinks. This helps prevent signal leakage or EMI coupling.
3. Multiple Ground Planes: Sometimes, different ground planes are actually the same ground.

For real ground planes, It’s essential to understand that there isn’t a universal ground. Different grounds in the same circuit can serve different purposes. For example, ADC datasheets often differentiate between analog and digital grounds to prevent noisy digital circuits from interfering with high-resolution ADCs. Digital circuits tend to generate noise at the clock frequency and its harmonics due to sudden current spikes, while analog circuits are generally quieter. Bypassing capacitors help, but they may not be enough to achieve the millivolt or microvolt resolution an ADC can provide.

Similarly, power grounds tend to be noisy due to loads like motors and solenoids, which can introduce noise from commutation or PWM effects. High currents and the finite resistance of even a copper ground plane can cause significant transients on the power ground, potentially disrupting sensitive measurements like encoder signals in motor control applications.

The goal, then, is to isolate these grounds as much as possible. Ensure that analog and digital grounds do not overlap. All analog components should connect to the analog ground, and all digital components to the digital ground, in separate PCB areas. When isolation is the objective, connect the planes together at a single point to prevent current loops that can cause EMI issues and create unintended antennas. This single connection point is often referred to as the star ground and serves as a central ground reference. Ideally, these grounds should be shorted near where the analog and digital circuits interact, such as at an ADC or DAC. In less ideal designs, they may be shorted near the power supply, though this can lead to problems.

For guard traces, if the trace is at ground, EMI is usually the concern. In cases of leakage, the guard should be driven at a voltage close to the signal level. Regardless, the guard should offer a low-impedance path to the source, which may involve multiple vias to the ground plane if the trace is grounded.

The third type of grounding involves ensuring uniformity within each ground plane after isolation. For instance, you don’t want a measurable potential difference between different areas of an analog ground plane. This requires a low-impedance path to the star ground, with each pin or pad connecting to the plane for a direct route to the star ground point. Ground planes also provide return paths for signal traces, minimizing current loops that could act as antennas. If the ground plane must be broken but a return path is necessary, consider using another layer. When multiple planes share the same ground, periodic vias can help reduce impedance.