Coupons
Help
  • FAQ
    browse most common questions
  • Live Chat
    talk with our online service
  • Email
    contact your dedicated sales:

Mixed-Signal IC Grounding and Decoupling: AGND, DGND, and Clock Jitter

Author : Daniel Li | PCB Assembly & Electronics Application Engineer

November 16, 2026


Mixed-Signal IC Grounding and High-Frequency Layout

Mixed-signal converters sit at the boundary between two very different electrical worlds. On one side is the analog domain, where microvolt-level signals and reference levels must be preserved with extreme care. On the other side is the digital domain, where fast edges and switching currents are the norm. Every ADC and DAC therefore has to answer a deceptively simple question: which ground plane should its ground pins return to, and where should its supply pins be decoupled? Getting this wrong does not usually destroy the converter outright. Instead it quietly degrades noise, distortion, and effective resolution, often in ways that are difficult to trace back to the layout.

This article works through the practical rules for grounding and decoupling mixed-signal ICs that carry only small internal digital currents, explains why the "DGND" pin label does not automatically mean "connect to the system digital ground," and shows how a small series resistor and a nearby buffer can keep fast output edges from corrupting converter performance. It then extends the same reasoning to the sampling clock, where phase jitter converts directly into lost signal-to-noise ratio. The thread running through all of it is a single idea: keep the fast, high-current digital return currents in the smallest possible loop, and never let them share a conductor with the analog reference.

Highlights:

  • Converters with low internal digital current should be treated as analog components: AGND and DGND are tied together externally with the shortest possible lead and connected to the analog ground plane, while the DGND pin is connected to the digital ground plane under no circumstances.
  • About 0.2 pF of stray capacitance exists between every adjacent pair of pins in an IC package, and fast digital currents on the die will couple through stray capacitance into the analog circuitry unless the return path is confined to a small loop by a local decoupling capacitor of 0.01 μF to 0.1 μF.
  • An unisolated CMOS output driving roughly 10 pF of trace and register capacitance at a 1 V/ns slew rate produces about 10 mA of transient current; a series resistor turns that edge into a filtered, slowed transition and protects converter performance.

Grounding and Decoupling Mixed-Signal ICs with Low Digital Current

Sensitive analog components such as amplifiers and voltage references must be referenced to, and decoupled to, the analog ground plane. This is uncontroversial. The less obvious case is the ADC and DAC, along with other mixed-signal ICs that draw only small digital currents. These devices should generally be treated as analog components as well, and grounded and decoupled to the analog ground plane in exactly the same way.

At first glance this requirement looks self-contradictory. A converter has both an analog interface and a digital interface, and it typically provides pins explicitly labeled as analog ground (AGND) and digital ground (DGND). If the part hands you two grounds, the instinct is to connect each one to its matching plane. That instinct is wrong for this class of device, and the reason becomes clear once the internal structure of the converter is examined.

Inside an IC that contains both analog and digital circuitry, such as an ADC or a DAC, the grounds are usually kept separate on the die so that digital signals are not coupled into the analog section. This is the simple converter model, and it is a reasonable one. The connection from the chip pad to the package pin inevitably brings bond wire inductance and resistance, and the IC designer can do nothing about that; it simply has to be accepted as part of the problem. Fast-changing digital currents develop a voltage at node B, and that voltage will inevitably couple through stray capacitance CSTRAY into node A of the analog circuitry. On top of this, each pair of adjacent pins in an IC package contributes roughly 0.2 pF of stray capacitance, and that cannot be avoided either. The IC designer's job is to make the chip work despite these effects. The board designer's job is to prevent further coupling.

The way to do that is to join AGND and DGND externally through the shortest possible lead and connect that junction to the analog ground plane. Any additional impedance in the DGND connection will develop more digital noise at node B, and more of that noise will then couple through the stray capacitance into the analog circuitry. The failure mode to avoid is connecting DGND to the digital ground plane: doing so applies VNOISE directly across the AGND and DGND pins, which is a serious problem rather than a minor layout imperfection.

The label "DGND" indicates that the pin connects to the digital ground of the IC. It does not mean that the pin must be connected to the digital ground of the system. A more accurate name would be the IC's internal "digital return."

This arrangement does inject a small amount of digital noise into the analog ground plane, but the currents involved are very small. They are kept to a minimum simply by ensuring that the converter outputs do not drive a large fanout, which is not how such parts are designed to be used in the first place. Minimizing the fanout on the converter's digital port also means lower current, which in turn means the logic transition waveforms at the converter are less affected by ringing, digital switching currents are as small as possible, and coupling into the converter's analog ports is reduced accordingly.

The logic supply pin, labeled VD, can be further isolated from the analog supply by inserting a small lossy ferrite bead. With that bead in place, the converter's internal transient digital currents flow in a small local loop: from VD through the decoupling capacitor to DGND, following the red path in the diagram. The transient digital currents therefore never appear on the external analog ground plane; they stay confined within that loop. The VD pin decoupling capacitor should be mounted as close to the converter as possible to minimize parasitic inductance. It should be a low-inductance ceramic type, typically between 0.01 μF (10 nF) and 0.1 μF (100 nF).

It is worth repeating that no single grounding scheme is correct for every application. What can be done is to understand the available options and apply the rules up front, which reduces problems to the minimum achievable level.

Handling ADC Digital Outputs with Care

Placing a data buffer next to the converter is a good practice. It isolates the digital outputs from noise on the data bus, and it also helps minimize the load presented to the converter's digital outputs while providing a Faraday shield between those outputs and the data bus. Many converters already include three-state output or input capability, but those registers still sit on the chip: they allow the signal on the data pins to couple into sensitive areas, so an external isolation buffer remains a good design choice. In some cases an additional data buffer is required on the analog ground plane, placed right next to the converter outputs, to achieve sufficient isolation.

A series resistor between the ADC output and the input of the buffer register, marked "R" in the grounding diagram, helps reduce the digital transient currents that can affect converter performance. The resistor isolates the digital output driver from the capacitance of the buffer register input. The resistor and the register input capacitance together form an RC network that acts as a low-pass filter and slows the fast edge.

A typical CMOS gate, combined with PCB trace and via capacitance, presents a load of approximately 10 pF. Without an isolation resistor, a logic output slew rate of 1 V/ns will produce a dynamic current of 10 mA:

Δi = C × (Δv / Δt) = 10 pF × (1 V / ns) = 10 mA

When driving a 10 pF register input capacitance, a 500 Ω series resistor minimizes the transient output current and produces rise and fall times of approximately 11 ns:

tr = 2.2 × τ = 2.2 × R × C = 2.2 × 500 Ω × 10 pF = 11 ns

TTL registers have a relatively high input capacitance and can noticeably increase the dynamic switching current, so they should be avoided. Buffer registers and other digital circuitry should be grounded and decoupled to the digital ground plane of the board.

Note that any noise between the analog and digital ground planes reduces the noise margin on the converter's digital interface. Because digital noise immunity is measured in hundreds or thousands of millivolts, this is generally unlikely to cause trouble. Noise on the analog ground plane is normally low, but if the noise on the digital ground plane, referred to the analog ground plane, exceeds a few hundred millivolts, steps should be taken to reduce the digital ground plane impedance so that digital noise margin stays at an acceptable level. In no case should the voltage between the two ground planes exceed 300 mV, or the IC may be damaged.

It is best to provide separate supplies for the analog and digital circuitry. The analog supply should be used to power the converter. If the converter has a dedicated digital supply pin (VD), it should be powered from the separate analog supply, or filtered as shown in the supply decoupling diagram. All converter supply pins should be decoupled to the analog ground plane, and all logic circuit supply pins should be decoupled to the digital ground plane. If the digital supply is relatively quiet, it can be used to power analog circuitry, but only with particular care.

In some situations it is not possible to connect VD to the analog supply. Certain high-speed ICs may use a +5 V supply for their analog portion in order to interface with external logic. In that case the IC's +3.3 V pin should be decoupled directly to the analog ground plane. It is also recommended to place a ferrite bead in series with the supply trace that connects the pin to the +3.3 V digital logic supply.

The circuit that generates the sampling clock deserves the same treatment as the analog circuitry: it should be grounded and heavily decoupled to the analog ground plane. Phase noise on the sampling clock degrades the system signal-to-noise ratio (SNR), a point examined in the next section.

Sampling Clock Considerations

In a high-performance sampled data system, the ADC or DAC sampling clock should be generated by a low phase noise crystal oscillator, because sampling clock jitter modulates the analog input or output signal and raises the noise and distortion floor. The clock generator should be isolated from noisy digital circuitry and, like the operational amplifiers and the ADC itself, grounded and decoupled to the analog ground plane.

The effect of sampling clock jitter on ADC signal-to-noise ratio can be approximated with the following relationship:

SNR = 20 log10 [ 1 / (2π f tj) ]

Here f is the analog input frequency, and SNR is the signal-to-noise ratio of a perfect ADC of infinite resolution in which the only noise source is the rms sampling clock jitter tj. A simple example makes the magnitude of the effect clear: with tj = 50 ps (rms) and f = 100 kHz, the resulting SNR is 90 dB, equivalent to a dynamic range of about 15 bits.

It should be noted that tj in this example is actually the root-sum-square (rss) value of the external clock jitter and the internal ADC clock jitter, which is usually called aperture jitter. In most high-performance ADCs, however, the internal aperture jitter is negligible compared with the jitter on the sampling clock.

Because the loss of signal-to-noise ratio is primarily caused by external clock jitter, steps must be taken to make the sampling clock as noise-free as possible, with the lowest phase jitter achievable. This is what makes a crystal oscillator mandatory. Several manufacturers offer small crystal oscillators that produce low jitter (less than 5 ps rms) CMOS-compatible outputs.

Ideally, the sampling clock crystal oscillator should be referenced to the analog ground plane in a separated ground system. System constraints, however, may make that impossible. In many cases the sampling clock must be derived from a higher-frequency, multi-purpose system clock generated on the digital ground plane, and must then be transferred from its origin on the digital ground plane to the ADC on the analog ground plane. Ground noise between the two planes adds directly to the clock signal and produces excessive jitter. That jitter degrades the signal-to-noise ratio and also generates interfering harmonics.

The sampling clock distribution diagram illustrates this situation. The clock originates in the digital domain, where the system clock is available, and must reach the converter located in the analog domain. Every point at which the clock path crosses from one ground reference to the other is a point where ground noise is injected into the timing of the sampling edges, so the crossing must be planned deliberately rather than left to the routing.

The Root of the Confusion in Mixed-Signal Grounding

Most ADC, DAC, and other mixed-signal device data sheets discuss grounding in the context of a single PCB, usually the manufacturer's own evaluation board. Trying to apply those principles to a multi-card or multi-ADC/DAC system is where designers start to feel lost. The usual recommendation is to divide the PCB ground plane into an analog plane and a digital plane, tie the converter's AGND and DGND pins together, and connect the analog ground plane to the digital ground plane at that same point. In effect this creates a system "star" ground right at the mixed-signal device. All of the high-noise digital current flows out of the digital supply into the digital ground plane and back to the digital supply, isolated from the sensitive analog portion of the board. The system star point appears exactly where the analog and digital ground planes are joined at the mixed-signal device.

This approach is generally used in simple systems with a single PCB and a single ADC/DAC, and it is not suitable for multi-card mixed-signal systems. In a system with several ADCs or DACs on different PCBs, or even several on the same PCB, the analog and digital ground planes end up connected at multiple points, which makes ground loops possible; a single-point star ground system cannot do that. For these reasons the method is not applicable to multi-card systems, and the approach described above should be reserved for mixed-signal ICs that carry low digital currents.

 

Grounding of a mixed-signal IC: single PCB (typical evaluation/test board).

 

Grounding for High-Frequency Operation

It is widely recommended that supply and signal currents return through a ground plane, and that the same plane also serve as the reference node for converters, voltage references, and other subcircuits. However, even the extensive use of a ground plane does not by itself guarantee a high-quality AC ground reference. The geometry of the plane, and the way the return current is allowed to flow within it, matter just as much as the presence of the plane.

On the top layer there is an AC/DC current source with one end connected to via 1 and the other end routed through a U-shaped copper trace to via 2. Both vias pass through the board and connect to the ground plane. Ideally, the impedance of the top connector and of the ground return loop between via 1 and via 2 is zero, so the voltage across the current source is zero.

Schematic and layout of a current source with a U-shaped trace on the PCB, returning through the ground plane.

This simple schematic barely reveals the subtleties involved, but understanding how the current actually travels through the ground plane from via 1 to via 2 helps us see where the real problem lies and how to eliminate high-frequency layout ground noise.

DC current flow in the PCB

The DC current takes the path of least resistance through the ground plane from via 1 to via 2. Some current spreading does occur, but essentially no current deviates in a meaningful way from that path. AC current behaves differently: it takes the path of least impedance, and that path is governed by inductance.

 

Magnetic field lines and inductive loop (right-hand rule).

Inductance is proportional to the area of the current loop, and the relationship can be illustrated with the right-hand rule and the magnetic field. Inside the loop, the magnetic fields generated by the current flowing along every part of the loop reinforce one another. Outside the loop, the fields generated by the different parts cancel one another. As a result, the magnetic field is in principle confined within the loop. A larger loop means greater inductance, which in turn means that, for a given current level, more magnetic energy is stored (Li2) and the impedance is higher (XL = jωL), so a larger voltage is developed at a given frequency.

AC current path in a ground plane without resistance (left) and with resistance (right).

So which path will the current choose in the PCB ground plane? Naturally, the path of lowest impedance. Consider the loop formed by the U-shaped surface trace and the ground plane, and ignore resistance: the high-frequency AC current will flow along the path of lowest impedance, which is the path enclosing the smallest area.

In the example shown, the smallest loop is clearly the one formed by the top U-shaped trace and the portion of the ground plane directly beneath it. In practice, the resistance of the ground plane causes low- and mid-frequency currents to flow somewhere between the direct return path and the region directly beneath the top trace.

Even at frequencies as low as 1 MHz or 2 MHz, however, the return path stays close to the region directly beneath the top trace.

 

Beware of Splits in the Ground Plane

If the ground plane beneath a trace is split, the return current in the plane has to flow around the gap. This raises the inductance of the circuit and makes it more susceptible to external fields. 

When the split exists so that two perpendicular traces can cross, a better solution is to jump the second signal trace over the first signal trace and over the ground plane using a fly wire. In that arrangement the ground plane acts as a natural shield between the two signal traces, and thanks to the skin effect the two ground return currents flow on the top and bottom surfaces of the plane respectively without interfering with each other.

A multilayer board supports both signal crossings and a continuous ground plane without any need to worry about wire jumpers. Multilayer boards cost more and are less convenient to debug than a simple double-sided board, but they deliver better shielding and better signal routing. The relevant principles remain unchanged; there are simply more layout and routing options available.

For high-performance mixed-signal circuits, a double-sided or multilayer PCB with at least one continuous ground plane is undoubtedly one of the most successful design approaches. Usually the impedance of such a plane is low enough that the analog and digital portions of the system can share a single ground plane. Whether that is achievable depends on the resolution and bandwidth requirements of the system and on the amount of digital noise present.

Other examples make the same point. A high-frequency current-feedback amplifier is very sensitive to capacitance around its inverting input. An input trace routed alongside a ground plane can present exactly that kind of capacitance. Remember that a capacitor consists of two conductors, the trace and the plane, separated by an insulator, namely the board material and possibly the solder mask. For this reason the ground plane should be kept away from the input pin, which is the evaluation board for the AD8001 high-speed current-feedback amplifier. 

 

Effect of 10 pF of inverting-input stray capacitance on the pulse response of the AD8001 amplifier.

Grounding Summary

No single grounding method can always guarantee optimum performance. Several possible options have been described here, based on the characteristics of the particular mixed-signal device under consideration. When implementing the initial PC board layout, it helps to build in as many of those options as possible.

The PC board must have at least one layer dedicated entirely to the ground plane. The initial board layout should provide non-overlapping analog and digital ground planes, with pads and vias at several locations if needed so that back-to-back Schottky diodes or ferrite beads can be installed. In addition, jumpers can be used to connect the analog and digital ground planes together when required.

In general, the AGND pin of a mixed-signal device should always be connected to the analog ground plane. One exception is a DSP with an internal phase-locked loop (PLL), such as the ADSP-21160 SHARC- processor. The ground pin of the PLL is labeled AGND, but it is connected directly to the digital ground plane of the DSP.

Related Reading:

Printed Circuit History and PCB Classification Guide

Grounding Principles, Star Ground, and Ground Planes in PCB Design

High-Speed ADC PCB Layout Rules: Grounding, Power, E-Pad

High-Speed ADC PCB Layout and Routing Best Practices

Non-Isolated Switching Power Supply PCB Layout: Hot Loops and Shielding

Daniel Li | PCB Assembly & Electronics Application Engineer Daniel Li | PCB Assembly & Electronics Application Engineer

Daniel Li is an experienced PCB assembly and application engineer with over 10 years of experience in SMT and DIP processes. He focuses on soldering quality, stencil design, and defect analysis, as well as real-world PCB applications across industries such as automotive, industrial, and consumer electronics. At AIVON, he reviews and improves content related to assembly techniques and application scenarios, helping bridge the gap between design and manufacturing.

Related Tags


2026 AIVON.COM All Rights Reserved
Intellectual Property Rights | Terms of Service | Privacy Policy | Refund Policy