Should You Use Star Point Grounding in a PCB?By ZM Peterson • Sep 27, 2021
One of the longstanding design guidelines surrounding mixed signal PCB design is the use of split ground planes and star grounding. It’s difficult to tell where this all came from, but it continues to persist to this day, even though such guidelines are known causes of EMC test failures. Perhaps more interesting is the mis-application of terminology here: star grounding was never meant to refer to something in PCB layout, yet I often see it applied in such a way by novice designers.
In this article, I want to look at star point grounding in the way it is often applied in PCB design. I’ve discussed this in several other articles on Altium’s site, technical papers, videos, and in some courses. However, it deserves another look here as companies may have incorrect expectations as to what they want or should have in their PCB layouts. Let’s jump right in and take a look at outdated grounding guidelines and how they can affect EMI.
What is Star Point Grounding?
Conceptually, star grounding involves constructing an electrical system with all modules or equipment in the system connected to ground at a single point. The simplest way to think about this is with a power supply, where the negative terminal (and thus the positive terminal) are branched off into different modules, basically connecting them in parallel in a circuit diagram. The idea here is to prevent ground loops by separating out grounds from each other. In this way, ground offsets might exist, but any potential for high DC current to flow between different systems is effectively eliminated.
If you also had a PE wire, you could also wire this up to each subsystem; this is basically what is done in residential wiring when receptacles and switches aren’t daisy chained. In a PCB that supports a modern electronic device, I would shy away from star point grounding for several reasons. I would note that there are some cases where you need to split ground regions in very specific ways, but this is sometimes ignored by newer designers and is used to justify bad routing practices when they aren’t needed.
Star Ground in a PCB
A star point grounding strategy in a PCB is intended to provide a single point where all ground return paths connect. This single point is generally the negative power supply terminal (either GND or the DC common terminal on a typical power supply). For a low-power AC system, this could be a connection to the neutral wire, although this might be bridged to earth in non-residential systems.
This type of grounding strategy in a PCB layout is shown below. This particular layout is for an audio board, but I would argue grounding is improperly implemented and will not provide any protection against radiated EMI from external sources.
The ground net in this PCB is shown in blue. Image credit: User Tomasz Kowalczyk on stackexchange.com.
In terms of noise suppression and defining ground in a system, the idea behind star point grounding on a PCB is that the space between these planes or ground rails, which are only connected at a single point, will prevent currents from traveling between different sections of the board. In effect, each section is largely isolated because return currents from one section (e.g., the digital section) can’t flow into a different section (e.g., the analog section). Because these paths for return currents would be blocked, you would have no mixed-signal interference.
I would argue that, at least in terms of electrical functionality, this was not the intent of star point grounding as it is classically implemented in, say, an industrial system. By tying all the grounds together at the same point, you would be intending to ensure that all the ground potentials are set to the same reference (i.e., earth in the case of an AC input, or the DC PSU ground plane in an isolated DC-DC converter, which might be floating w.r.t. its AC input). This might not work out in reality; any system that receives power from a central power source might apply its own regulation. The PCBs in different devices could then have different ground potentials or floating grounds, which is not normally a problem in PCB design unless you start routing single-ended signals between these devices.
If instead, we were to place all these “devices” onto the same PCB with overlapping GND planes at different potentials, these planes would couple capacitively. This would cause noise to appear superimposed on any signal that is read out with respect to one of the ground planes due to capacitive coupling, particularly at higher frequencies. The constant charging and discharging of the plane pair could also act as a source of radiated EMI. We've still eliminated the ground loop problem, but we've replaced it with a radiated EMI problem.
The major problem with EMI in mixed-signal systems, both in terms of emission and reception, comes from the routing constraints imposed in star point grounding. This is the major reason to not use star point grounding in mixed-signal systems that include digital components and, instead, use the proven method of placing ground planes.
The Routing Problem in Star Point Grounding
On the PCB, this forces a design to implement two bad grounding practices: cutting a plane up into sections (regardless if they are connected at one point) and routing over an open split between two planes. These practices must be avoided in the following types of mixed-signal designs:
- HS/HF mixed-signal designs: High speed PCB design with a high frequency analog section or wireless section does not need split planes.
- Mixed frequency analog designs: The only exception that might apply here is when one analog frequency is very low (less than 1 kHz) and is being implemented on the same board as a high frequency signal (e.g., for wireless).
The reason digital designs with split planes often fail is not because the planes are split, it’s because the people want to have their cake and eat it too. They want the isolation provided by split planes or by no planes at all, meaning ground is provided entirely by traces, but they don’t want to obey the routing rules this imposes. Just because you have split planes that ensure return path isolation, it doesn’t mean you can route wherever you want on the board. It’s a standard routing guideline for digital and analog systems that traces should only be routed over continuous ground planes.
Star point grounding with split planes creates potential for EMI whenever a trace is routed over a gap. In a star point ground arrangement with traces as ground connections, there will be huge gaps with strong radiation if traces are carrying digital signals or high frequency analog signals.
This design and routing will fail EMC if it is used to try and isolate digital signals, even at 5-10 ns rise times, from analog signals of any frequency. The second you route over the gap in the ground plane, you have a high impedance return path or a large loop inductance return path. As a result, you have just created a very large loop antenna that emits radiation on the rising and falling edges of your digital signal. The same applies with analog signals, which can radiate strongly at a single frequency, particularly when the capacitively coupled analog signal in the ground loop corresponds to a resonance in the embedded loop antenna structure.
The irony is that this bad routing and grounding practice is often implemented in high speed/high frequency PCBs by newer designers. The reality is that these higher speed/higher frequency signals are easier to isolate than slower signals because they will more easily couple to the adjacent ground plane via substrate capacitance. Because of this, you won’t need split planes or star grounding to isolate these signals; you’ll have much more control and shielding effectiveness with an appropriately constructed ground region on the adjacent layer and some grounded copper judiciously placed around traces.
When Star Point Grounding is Appropriate
There are a few cases in mixed-signal PCB design and in power system design where split planes or routing with traces in a star point grounding arrangement are preferred. Some of these cases include:
- Boards that will only run at DC. Although this type of board won’t radiate, it will easily receive radiated EMI from external sources.
- Audio systems that include a digital controller because return paths for the 20 kHz and lower signals can be difficult to control
- Systems with multiple analog frequencies at multiple levels, although shielding is much more effective for protecting low SNR analog lines than splitting planes
- Isolated power systems, including systems with multiple rails, where splits in planes are implemented for galvanic isolation rather than noise control
- Systems where two devices, operating at different frequencies/speeds, need to sit on the same substrate but will have absolutely no interaction or signals sent between them
There are other instances where splitting is appropriate, but these should be treated as corner cases or very specialized applications, rather than as a standard design practice. I’ll discuss these instances, particularly the case of splitting up multiple power grounds, in an upcoming article. I’ve discussed this extensively in a recent Altium article, which you can find here.
Whether you’re designing high-speed digital systems or high frequency analog systems, it pays to understand the drawbacks of star point grounding in PCBs. NWES is an experienced design firm that develops advanced IoT platforms, RF power supply designs, data center products, aerospace systems, and much more. NWES helps aerospace OEMs, defense primes, and private companies in multiple industries design modern PCBs and create cutting-edge embedded technology. We've also partnered directly with EDA companies and advanced ITAR-compliant PCB manufacturers, and we'll make sure your next high speed digital system is fully manufacturable at scale. Contact NWES for a consultation.