MixedSignal PCBs: How to Deal with Analog and Digital Grounding
Reto B. Keller studied electrical engineering at Fachhochschule OST in Rapperswil SG, Switzerland. He works as Principal Electronics Development Engineer at Roche Diagnostics International Ltd., Rotkreuz Switzerland. He is a member of the IEC TC65 and is actively involved in developing EMC standards. As president of the Academy of EMC, and author of the openaccess book "Design for Electromagnetic Compatibility  In a Nutshell", he publishes free knowledge about EMC for professional engineers.
About the Author:
Reto B. Keller studied electrical engineering at Fachhochschule OST in Rapperswil SG, Switzerland. He is a Principal Electronics Development Engineer at Roche Diagnostics International Ltd., Rotkreuz, Switzerland. He is a member of IEC TC65 and is actively involved in developing EMC standards. As president of the Academy of EMC and author of the openaccess book Design for Electromagnetic Compatibility – In a Nutshell, he makes important knowledge about EMC freely available to professional engineers.
Introduction
A mixedsignal design consists of analog and digital circuits on a single printed circuit board (PCB).
Every electronics design engineer is familiar with this question: Should we split the ground of our mixedsignal PCB into analog and digital ground? And if so, how should we connect them? A good grounding strategy for a mixedsignal PCB design is essential to minimizing noise and interference, improving power integrity and signal integrity, and eliminating electromagnetic compatibility (EMC) issues. This article explains grounding for mixedsignal PCB designs and discusses some pitfalls.
Grounding Conductors
In electronic circuits, ground conductors are the conductors through which the power supply return currents and the signal return currents flow. Ground planes on a PCB or grounding conductors in a system are often meant to be equipotential. However, this is not the case, as there is a voltage drop across the ground plane or along a ground conductor as soon as there is a current flowing because ground planes and ground conductors have an impedance Z_{g} [Ω] that is greater than zero:
Figure 1: Zg [Ω] is the impedance of the return current signal ground, which is not shown in any circuit schematic but is present in every circuit [1].
It is practical to model the ground (plane or connector) as a series connection of a resistance R_{g} [Ω] and an inductance L_{g} [H]. This is a massive simplification. However, it is in many cases sufficient. The ground (plane or conductor) impedance can then be written as [1]:
𝑍_{𝑔} = 𝑅_{𝑔} + 𝑗𝜔𝐿_{𝑔} (2)
where R_{g} [Ω] is the ground resistance, L_{g} [H] is the ground inductance, and ω = 2𝜋f [rad/sec] is the angular frequency of a sinusoidal harmonic of the signal. Equation (2) shows us that the ground impedance is frequency dependent. For lowfrequency signals, where the frequency f [Hz] is low (let’s say <100 kHz), the dominant part in Z_{g} [Ω] is the resistance R_{g} [Ω]. However, once the frequency exceeds a certain limit (e.g., >1 MHz), the reactance X_{g} = ωL_{g} is going to become dominant.
Figure 2 shows the frequencydependent impedance Z(f) [Ω] of two ideal single round copper wires with length L = 0.1 m and diameters D = 1 mm and D = 0.1 mm.
The two graphs in Figure 2 show that the dimensions of an interconnection determine when the reactance starts to be dominant. Even if we consider the skin effect of the wire, the reactance dominates at high frequency, because the reactance X = ωL increases by 20 dB/decade and the resistance due to the skin effect by 10 dB/decade.
Please bear in mind that the graphs in Figure 2 represent a massive oversimplification and that things are much more complicated in real electronic designs. However, it gives an idea of the behavior of a (ground) conductor impedance at high frequencies.
Ground conductors play an important role for the following design topics:
 Power and signal integrity
 Electromagnetic compatibility
Therefore, the next two sections will present a deeper understanding of why grounding is important for power/signal integrity and electromagnetic compatibility.
Figure 2: Impedance Z = R + jωL of a round wire with length L = 0.1 m and
diameter D = 1 mm (see above) or D = 0.1 mm (see below).
Sources: R calculation, equation 10.8 [1],
L calculation, equation 6.2.1.1 [3].
Return Current through Ground Planes
On a PCB, ground is the name for the return current conductor: signal currents of analog and digital circuits flow through the ground plane back to their sources.
As shown in Equation (2) and Figure 2, the ground impedance is dominated by the resistance R_{g} [Ω] for low frequencies and by the inductance L_{g} [H] for high frequencies. This means:
 At low frequencies (around f < 100 kHz), the signal return current path in the solid ground plane flows straight (see the return current in Figure 3 for low frequencies).
This is because the resistance R_{g} [Ω] is the lowest for the direct connection form Via 1 to Via 2 in Figure 3.
 At high frequencies (around f > 1 MHz), the signal return current in the solid ground plane flows directly below the respective PCB trace (see the return current in Figure 3 for high frequencies).
This is because the highfrequency return currents take the path that minimizes the energy stored in the magnetic field, and that is when the area between the forward and return current is minimized.
Figure 3: Signal return currents in a solid PCB ground plane.
Left Image: At low frequencies (around f < 100 kHz).
Right Image: At high frequencies (around f > 1 MHz).
PCB Grounding and Power/Signal Integrity
Good grounding provides a lowimpedance path for the return currents in a circuit. Here's why grounding is important and how improper grounding practices can worsen power and signal integrity:

Common Impedance Coupling (Ground Bounce):
Improper grounding can lead to ground bounce, which is the fluctuation in the ground reference voltage caused by switching signals. Ground bounce can result in voltage noise on power or signal lines, affecting the stability and functionality of the circuit. As soon as multiple power supplies or signal lines share a common ground plane or ground conductor, there is the possibility of a problematic noise voltage along the ground connection being introduced by alternating currents. 
Ground Loops:
Incorrect grounding practices can lead to ground loops, which are unintended current paths resulting from multiple ground connections. Ground loops introduce unintended currents that can cause noise and interference and degrade signal quality.
PCB Grounding and Electromagnetic Compatibility
In addition to powerintegrityrelated topics like common impedance coupling and ground loops, EMC design engineers must be mindful of the circuit loop areas A [m^{2}] of highspeed signals (>1 MHz).
The reason for this is that highfrequency signals potentially radiate at unacceptably high levels. Let’s assume an electrically small current loop (circumference < λ/4), so that the current distribution (magnitude, phase) is constant along the current loop, and a measurement point of the Efield [V/m] in the farfield. The maximum root mean square (RMS) value of the electric field E_{DM,max} [V/m] caused by a differentialmode current I_{DM} [A] can be approximated as [2]:
Equation (3)
Where I_{DM} [A] is the RMS differential current through the small current loop, f [Hz] is the frequency of the sinusoidal current signal, A [m^{2}] is the area of the current loop, and d [m] is the distance from the center of the current loop to where the E_{DM,max} [V/m] is measured.
Figure 4: A small current loop (small with respect to the wavelength λ [m] of the signal) as an unintended antenna.
Equation (3) shows that the field strength is proportional to the signal frequency f [Hz] squared (f^{2}). Therefore, unintended radiated emissions are primarily an issue for highfrequency signals (e.g., >1 MHz) rather than lowfrequency signals (e.g., <100 kHz).
Split Ground Planes vs. a Single Ground Plane
In a mixedsignal PCB design with analog circuits and digital circuits, there is often a discussion within design teams about whether the ground should be split into analog ground (AGND) and digital ground (DGND or simply GND). From my own experience, a PCB design with split ground planes does not perform better—with regard to unintended radiated emissions—than a PCB design with a single solid ground plane. In addition, a PCB with a split ground plane makes it much more difficult to route the analog and digital signals.
Dr. Todd Hubing—former president of the IEEE Electromagnetic Compatibility Society and an outstanding EMC expert—offers a clear recommendation [4]: “Don’t gap your ground plane, there's never really a good reason to do that.”
One problem with split ground planes is that they can lead to high radiated emissions when signals are routed over the gap between the ground planes. This is especially true if the signal is a highfrequency signal, such as a serial peripheral interface (SPI) clock. When a signal is routed over a ground plane gap and the return current flows through the common connection point of the grounds, a large current loop may be the result (see Figure 5). From Equation (3), we know that the strength of radiated emissions is approximately proportional to the current loop area and proportional to the square of the frequency.
A solution to this problem would be to route the signal over the connection of the ground planes (i.e., where AGND and GND are connected together).
Figure 5: Forward signal (solidline arrow) and its return current (dashedline arrow).
However, today's PCB designs are getting incredibly dense, and routing of signals is getting more complex. Therefore, it may not be practical to route all highspeed signals over the GND–AGND connection point.
This is one of the reasons why it is best practice to go with one single solid GND.
Another reason to avoid splitting GND planes is related to the issue of where AGND and GND should be connected. Should it be at the analogtodigital converter? Or at the power supply? What if there are multiple ADCs and power supplies on a board: should AGND and GND be connected at every ADC or power supply? Or if only at one of them, which one? Or should you implement a separate AGND for every ADC? These are all questions that arise, once you decide to split the ground planes. These questions are not easy to answer, and what works in one case may not work for the next design.
And then there is another issue when splitting the ground planes: stray capacitive coupling between the split planes. Even if you decide to split the planes, there is always coupling between the planes, and highfrequency signals can move from one plane to the other. Why make the effort of splitting the planes if the gap between them does not provide 100% electrical separation?
Common Impedance Coupling
Figure 6 shows the principle of common impedance coupling. Common impedance coupling can lead to high noise in sensitive analog circuits (ground bounce), where a couple of millivolts is already an unacceptably high noise level.
Figure 6: Common impedance coupling.
Figure 7 shows an example of common impedance coupling with a highpower circuit and a sensitive analog circuit.
The current from the highpower circuit I_{hp} [A] introduces a noise voltage V_{n} [V] in the analog circuit:
𝑉_{𝑛} = 𝑍_{𝑐𝑜𝑚 }∙ 𝐼_{ℎ𝑝} (4)
where Z_{com} [Ω] is the common impedance of the sensitive analog circuit and the highpower circuit.
Figure 7: Common impedance coupling and how to minimize it.
Top: High noise levels in analog circuit. Bottom: Lower noise in analog circuit.
One way to reduce the noise voltage V_{n} [V] is to reduce the common impedance Z_{com} [Ω] by not placing the sensitive analog circuit between the power supply and the highpower circuit. Instead, the sensitive analog circuit is placed so that the noise current has little effect on the analog circuit (see Figure 7).
Conclusion
The ground of a mixedsignal PCB design should not be split into an analog and a digital ground plane. Splitting ground planes increases the complexity of the PCB design and could lead to high radiated emissions. Instead, go with a single solid ground plane and arrange circuits so that common impedance coupling is minimized.
Sources:
[1] Reto B. Keller. Design for Electromagnetic Compatibility – In a Nutshell: Theory and Practice. Springer, 2023.
[2] Clayton R. Paul. Introduction to Electromagnetic Compatibility. 2nd edition. John Wiley & Sons, 2008.
[3] Brian C. Wadell. Transmission Line Design Handbook. Artech House, 1991.
[4] "Four Commonly Held Myths of EMC Design." Altium YouTube channel. Interview with Dr. Todd Hubing. https://www.youtube.com/watch?v=TUS21J5RPE0&t=1313s (24 June 2023).