EMI, EMC, and Shielding Shielding and Enclosure Design Informational

How does grounding strategy affect EMI performance in a mixed signal PCB with RF and digital circuits?

Q: What about star grounding?

Star grounding (all ground connections radiate from a single point) is an audio/low-frequency technique. At RF: star grounding is impractical because the long ground traces (from each circuit to the star point) have high inductance at RF. The ground impedance becomes significant (ohms) at just 10 MHz. For RF PCBs: use a ground plane (distributed ground), not star wiring. The ground plane provides a low-inductance ground return at all frequencies. Star grounding is only used for: bench-level interconnection of separate instruments (to avoid ground loops between equipment), and some precision DC measurement setups.

Q: Do I need a guard ring around sensitive RF traces?

A guard ring is a grounded copper pour or ring around a sensitive trace or component connected to the ground plane with vias. Benefits: reduces the electric field coupling from nearby aggressors by providing a grounded shield. Improves the effective isolation by 10-20 dB for microstrip traces. Provides a controlled impedance environment for the trace (coplanar waveguide structure). When to use: around VCO traces and components, around LNA input traces, around crystal oscillator traces, and around any high-impedance trace (bias lines, DC control lines that carry sensitive analog information). The guard ring vias should be spaced < lambda/20 at the highest frequency of concern to prevent the ring from acting as a slot antenna.

The grounding strategy is the single most important factor in controlling EMI on a mixed-signal PCB with RF and digital circuits. The ground plane provides the return current path for all signals, and its design determines the coupling between circuits. Key principles: (1) Solid ground plane is preferred: a continuous, unbroken copper plane on the layer immediately adjacent to the signal layers provides the lowest-impedance return path. At RF frequencies: the return current follows the path of minimum impedance, which is directly under the signal trace (within approximately 3× the trace height). This happens naturally on a solid ground plane; the RF return current stays under the RF traces and the digital return current stays under the digital traces. No physical barrier (split) is needed to separate them. (2) Split ground creates problems: a split ground plane forces return currents to detour around the split gap. If a signal trace crosses the split: its return current must travel around the split to complete the loop. This creates a large current loop that: radiates EMI (the loop acts as a loop antenna), picks up external interference, and creates a high-impedance ground path at frequencies where the detour is comparable to a wavelength. A 2 cm detour at 1 GHz: the detour is lambda/15, creating significant impedance (10-20 ohms of inductive impedance vs milliohms for a direct path). (3) When splits are necessary: in some extreme cases (e.g., a high-power transmitter sharing a board with a sensitive receiver), separate ground regions connected at a single point may be used. In this case: NO signal traces may cross the split boundary. All inter-region signals must be routed through the single connection point. The connection point should have good filtering (ferrite beads for CM rejection).

Category: EMI, EMC, and Shielding

Updated: April 2026

Product Tie-In: Enclosures, Gaskets, Absorbers, Filters

Grounding for EMI Control

Ground plane design is the foundation of EMC performance. A well-designed ground eliminates most common EMI problems; a poorly designed ground creates problems that are extremely difficult to fix with filtering or shielding after the fact.

Return Current Physics

(1) At DC and low frequencies (< 1 kHz): the return current spreads across the entire ground plane, following the path of least resistance. This can create ground voltage drops if the ground plane has significant resistance (thin copper, long paths). (2) At RF frequencies (> 1 MHz): the return current concentrates directly under the signal trace, following the path of least inductance (not least resistance). The distribution is approximately Gaussian, with most current within ±3H of the trace centerline (H = distance between the trace and the ground plane). This concentration effect means that on a solid ground plane: RF signals are naturally isolated from each other. Two parallel traces separated by > 3H have separate, non-overlapping return current paths. They do not share ground current and do not couple through the ground. (3) Ground plane slots and gaps: if there is a slot (opening) in the ground plane under a signal trace: the return current must detour around the slot. The detour increases the loop area by the slot area, increasing radiation by 20-40 dB. A common cause: accidental slots created by running too many signal traces on the layer adjacent to the ground (consuming the ground copper with trace clearances). Rule: maintain at least 60% ground fill on any layer used as a ground return reference.

Mixed-Signal Grounding Best Practices

(1) Unified ground plane: use a single, solid ground plane for the entire PCB. This is the modern best practice endorsed by virtually all component manufacturers (Analog Devices, Texas Instruments, Keysight). The old "split ground" approach has been superseded by better understanding of return current behavior. (2) Component placement isolation: separate RF, digital, and power sections physically on the PCB. The ground beneath each section carries the return current for that section only (because the return current follows the signal trace, not the ground plane shape). No ground plane cuts are needed. (3) Layer stack-up: put the ground plane on Layer 2 (immediately below the top signal layer). This creates the tightest coupling (smallest loop area) and the best EMC. The dielectric between Layer 1 and Layer 2 should be thin (4-8 mil) for maximum coupling. (4) No traces crossing between regions: do not route digital signals under RF components, or RF signals under digital components. The routing should respect the physical partitioning. (5) Decoupling: place decoupling capacitors at each IC power pin, connected to the ground plane with short, wide vias. The decoupling capacitor provides a local ground return for the switching current, keeping it out of the global ground plane. (6) Ground stitching: use via stitching (ground vias connecting multiple ground planes) throughout the board. This prevents the ground planes from resonating as patch antennas and provides vertical connectivity for return currents transitioning between layers.

Common Mistakes

(1) Routing digital clock traces across a ground split: the clock return current detours around the split, creating a massive radiating loop. This is the #1 cause of radiated emissions failures in mixed-signal boards. (2) Splitting the ground under an ADC or DAC: mixed-signal ICs (ADCs, DACs) have analog and digital pins on the same chip. The return currents for both analog and digital signals flow through the IC ground pins. If the ground plane is split under the IC: the return current must flow through the IC from one ground region to the other, creating noise coupling inside the IC. Solution: always use a solid ground under mixed-signal ICs. Connect the AGND and DGND pins to the same solid ground plane. Any ground split must be AWAY from the mixed-signal ICs. (3) Using ferrite beads between ground regions: some designs connect split grounds through a ferrite bead. This creates a high-impedance ground connection at RF, which is the opposite of what a ground should be (low impedance). The ferrite bead ground forces the return current through the bead, becoming a source of common-mode noise.

Ground Return Current Rules

Return current width ≈ ±3H from trace center
Loop area ∝ trace height × trace length
Radiation ∝ I × f × loop_area
Ground impedance: Z_ground ≪ Z_signal
Slot detour: radiation increase 20-40 dB

Common Questions

Frequently Asked Questions

When should I split the ground?

Almost never. The only legitimate case: extremely high-power TX (> 10 W) sharing a PCB with a very sensitive receiver (< -100 dBm). The TX return current (amps) flowing through the shared ground creates a voltage drop that can desensitize the receiver. In this case: separate analog and digital ground regions connected at a single star point. But: all signal routing between regions must go through the star point. This is complex to design. For ALL other cases: use a solid, unified ground. The natural return current containment on a solid ground provides adequate isolation for most mixed-signal designs.

What about star grounding?

Star grounding (all ground connections radiate from a single point) is an audio/low-frequency technique. At RF: star grounding is impractical because the long ground traces (from each circuit to the star point) have high inductance at RF. The ground impedance becomes significant (ohms) at just 10 MHz. For RF PCBs: use a ground plane (distributed ground), not star wiring. The ground plane provides a low-inductance ground return at all frequencies. Star grounding is only used for: bench-level interconnection of separate instruments (to avoid ground loops between equipment), and some precision DC measurement setups.

Do I need a guard ring around sensitive RF traces?

A guard ring is a grounded copper pour or ring around a sensitive trace or component connected to the ground plane with vias. Benefits: reduces the electric field coupling from nearby aggressors by providing a grounded shield. Improves the effective isolation by 10-20 dB for microstrip traces. Provides a controlled impedance environment for the trace (coplanar waveguide structure). When to use: around VCO traces and components, around LNA input traces, around crystal oscillator traces, and around any high-impedance trace (bias lines, DC control lines that carry sensitive analog information). The guard ring vias should be spaced < lambda/20 at the highest frequency of concern to prevent the ring from acting as a slot antenna.

Keep Reading