Should You Ever Separate Analog and Digital Ground Planes?

Key Takeaways

• Separating analog and digital ground planes is a contentious design practice that can create power integrity and signal integrity problems.

• Separating the ground planes is less important than routing over the gap between two ground plane regions.

• There is a limited case where creating physically separated ground planes is acceptable, but this amounts to a trivial design practice that does not create any advantages for system function.

The exposed copper on this board can be tied back to a ground system, but should the various grounds be separated?

There are three PCB design guidelines that everyone loves to hate:

1. Never route at 90-degree angles.

2. Most “rules of thumb” involving distances and clearances between copper.

3. Never separate analog and digital ground planes.

Only the last of these design guidelines has any level of legitimacy, and it is something of a necessity in modern PCBs. However, it is often extremely poorly communicated.

When many designers use the term “split ground plane,” they may be talking about different ways of defining grounds in a system. Then, there is how you route in those different systems—another area that is extremely poorly communicated, yet a clear understanding of what routing looks like in these systems is vital. If routing isn’t done correctly in any system with a ground plane (even split ground planes), you’ll create a new EMI problem that is worse than the problem the split ground planes were supposed to solve.

To better see why separate analog and digital ground planes are so contentious, let’s clear the air and define exactly what the term “split ground planes” actually means and what best routing practices look like on these boards.

What Are Separate Analog and Digital Ground Planes?

The phrases “split ground planes” or “separate analog and digital ground planes” could mean two totally different things within mixed-signal PCB design:

1. A ground plane that is totally uniform, but has one “section” where we try to place only digital components and another section where we try to place only analog components.

2. Two totally separate, completely disconnected ground regions, one for analog components and another for digital components.

These two grounding methods are shown below.

Two ways to “split” analog and digital ground planes

In the left image, we have two physically disconnected ground planes, one dedicated to analog components and the other dedicated to digital components. In the right image, the board has a single ground plane that has some copper removed to define an analog section and a distinct digital section.

Before the more experienced designers in the PCB design community become concerned about EMI problems, let’s clarify something:

The above two grounding methods are unnecessary and are even bad practice in modern PCBs, regardless of the frequencies they use. If you understand how to properly layout a board and follow return paths, you don’t need to use split ground planes, and you won’t have to cut out sections from a ground plane. This applies to all-digital, all-analog, and mixed-signal systems.

With that out of the way, this brings up the question: why would anyone do this to begin with, especially if it is such bad practice?

Why Would You Use Totally Separate Ground Planes?

The entire idea behind separating ground planes is to keep digital signals and analog signals separate. For example, if the return current from a digital signal travels near an analog interconnect, the changing edge of the digital signal generates a magnetic field that can create inductive crosstalk in an analog interconnect, and vice versa. By splitting the ground plane into two totally different sections, you’ve created very high isolation between the analog and digital sections, so the two types of signals will never interfere!

The Only Time You Should Use Separate Ground Planes

So, what’s wrong with a totally split plane arrangement? It would seem like each section has a nice uniform ground plane, so why would this be a problem? This is where we need to be extremely specific with the following guideline:

This means there are two devices that are completely isolated from each other (one analog and one digital), they just happen to be on the same substrate.

If no traces are routed between these two regions, then you have totally isolated devices

If you think about this, it’s a pretty pointless exercise. In fact, if you do this and you now bring in a chassis ground or some other floating conductor, all of which are at different reference potentials, you now have the possibility of inducing common mode currents between board sections. By trying to solve one EMI problem, you’ve created a new EMI problem that can be much more difficult to solve.

A Sectioned Ground Plane is Okay If...

If you use a “sectioned” ground plane, the situation is a bit different. Now, because there is some grounded copper that connects the analog and digital sections, return currents from one section can travel near the other section. As a result, there is a chance for crosstalk between the two sections if you don’t keep track of your return paths.

With today’s digital signals, this is a moot point. Even slow digital buses operate with bandwidths stretching well into the 100’s of MHz, so the return path of these digital signals stays close to the trace that defines them. As a result, it’s quite easy to guide your digital return paths around the board without using physically separated analog and digital ground planes.

If, for some reason, you must use the H-shaped ground plane shown below, and you must route a trace between the analog and digital sections, only route that trace over a solid copper ground region. Do not route over the gap between the two ground regions. The copper connection will provide the clear return path you need to ensure low loop inductance. The second you route over the gap, you’ve got a radiated EMI problem.

If you must use separated ground regions with a ground cutout, do not route over the gap in the ground plane

Uniform Copper Provides Clear Return Paths

Remember, a ground plane in a PCB is supposed to provide a clear low reactance path for return current. The second you route a high speed digital trace over a region without any grounded copper beneath it, you’ve created a return current path that may have very large loop inductance, which could create a radiated EMI problem. This loop may act like a big antenna and radiate strongly whenever the digital signal switches between states. The same applies to an analog signal sent across the gap between the ground regions; it just radiates continuously.

Note that “high speed” here can refer to a digital signal with rise time as slow as 20-30 ns. This is a rise time value you might see in clock signals on an SPI bus, but even this can cause a board to fail EMC testing if return paths are not clearly defined and you route over a gap in a ground plane. For this reason, take some time to learn what carries return currents in your PCB layout, and you’ll be able to control return currents in your ground plane without the need for gridding.

Stop the Silliness and Use Uniform Ground Planes

If you want to make your design process easier, prevent power integrity problems in a high speed digital system, and provide high isolation between layers and board surfaces, just cut out all the split ground plane silliness and use uniform ground planes. If you’re designing a board with multiple ground planes and grounded copper pour, tie all those regions together with vias. It’s easier to design like this and, in some cases, it’s the best way to ensure you don’t create EMI disasters.

The truth is, if you understand how to layout a board to prevent interference between digital and analog return paths, then you won’t need to use a sectioned ground plane! This means practicing sectioning, but use a complete ground plane below your components regardless. High frequency analog signals and high speed digital signals will naturally form tight return paths around their traces, so you mostly need to worry about tracking return paths with low-frequency analog signals (less than ~100 kHz).

If you want to use best practices and avoid separating analog and digital ground planes, use PCB design and analysis software for professional design teams. OrCAD PCB designer has the necessary tools for component placement and ground plane pour to implement an ideal grounding strategy.