EMI, EMC, and Shielding PCB EMC Design Informational

What is the proper technique for transitioning a signal between layers on a multilayer PCB to minimize EMI?

Signal transitions between layers on a multilayer PCB must be designed properly to minimize EMI. When a signal trace transitions from one PCB layer to another through a via, the electromagnetic return current path changes. If not handled properly, these layer transitions create impedance discontinuities, return current disruptions, and EMI radiation. Proper technique for transitioning a signal between layers: (1) Maintain the return current path: the signal return current flows on the ground plane directly below (or above) the signal trace. When the signal transitions to a different layer: the return current must also transition to the ground plane adjacent to the new layer. If the reference plane changes (e.g., from L2 GND to L5 GND): place ground stitching vias within 0.5-1 mm of the signal via. These stitching vias connect L2 GND to L5 GND, providing a low-inductance path for the return current transition. Without stitching vias: the return current must find an alternate path (through the nearest existing via connecting the two ground planes). The detour creates a large current loop that radiates EMI and creates a voltage difference between the two ground planes. (2) Via impedance matching: a standard through-hole via has a characteristic impedance of approximately 25-35 ohms (lower than the 50-ohm trace). This creates a capacitive impedance discontinuity. For frequencies below 5 GHz: the via discontinuity is small (VSWR < 1.2:1 for a single via) and can be ignored. For 5-20 GHz: the via should be designed to minimize discontinuity. Use a smaller via antipad (the clearance ring in the ground plane around the via). A smaller antipad reduces the capacitive loading. (3) Via stub: in a through-hole via, the portion of the via that extends beyond the target layer is a stub that resonates at approximately f_res = c/(4×L_stub×sqrt(epsilon_r)). For a 1.2 mm stub on FR-4: f_res = 30.5 GHz. Below 30 GHz: the stub has minimal effect. For thicker boards or higher frequencies: backdrill the stub.

Category: EMI, EMC, and Shielding

Updated: April 2026

Product Tie-In: PCB Materials, Capacitors, Ferrites

PCB Layer Transition Design

Via transitions between layers on a multilayer PCB are one of the most common sources of signal integrity and EMI problems, especially at frequencies above 5 GHz.

Technical Considerations

(1) The critical rule: every signal via must have at least one stitching via (connecting the two reference planes) within 0.5-1 mm. More stitching vias = lower transition inductance = better performance. Best practice: 2-4 stitching vias arranged symmetrically around the signal via. This creates a quasi-coaxial transition through the board stack-up. (2) Stitching via placement: place the stitching vias on the side of the signal via closest to the return current path. If the signal trace approaches from the left on L1 and exits to the right on L3: the return current flows from left to right. The stitching vias should be placed on the left and right sides of the signal via (aligned with the current flow). (3) Via pairs for differential signals: for differential pairs (USB, LVDS, PCIe): transition both traces simultaneously through adjacent vias. Place stitching vias on both sides of the differential pair. The two signal vias and the stitching vias form a "coaxial group" that maintains the differential impedance through the transition.

Performance verification: confirm specifications against the application requirements before finalizing the design
Environmental factors: temperature range, humidity, and vibration affect long-term reliability and parameter drift
Cost vs. performance: evaluate whether the application demands premium components or standard commercial grades
Interface compatibility: verify impedance, connector type, and mechanical form factor match the system architecture

Performance Analysis

(1) Through-hole via stub resonance: for a signal entering on L1 and exiting on L3 in a 6-layer board: the via stub extends from L3 to L6. Stub length: approximately 0.4-1.0 mm (depending on the layer stack-up). The stub resonates at f_res = c/(4×L_stub×sqrt(epsilon_eff)). At the resonant frequency: the via acts as a notch filter (severe insertion loss, potentially > 20 dB). (2) Backdrill: remove the via stub by drilling out the unused portion from the back of the board. Drill depth: controlled to within ±0.1 mm. Stub residual: approximately 0.1-0.2 mm (nearly zero parasitic). Cost: adds $0.50-5 per via (backdrilling is a post-process). (3) Blind/buried vias: formed only between the required layers (no stub). Laser-drilled microvias (0.1 mm drill, connecting only adjacent layers): no stub parasitic. HDI (high-density interconnect) PCB process. Cost: higher than standard through-hole (requires sequential lamination).

Common Questions

Frequently Asked Questions

Do I need stitching vias for every signal transition?

For best practice: yes. Every signal via that transitions between reference planes should have stitching vias. In practice: at frequencies below 1 GHz: the via transition effects are small, and stitching vias are less critical (but still good practice). From 1-10 GHz: stitching vias are recommended for all high-speed signals (clocks, data buses, RF). Above 10 GHz: stitching vias are mandatory for acceptable signal integrity and EMI performance.

How many stitching vias do I need per signal via?

Minimum: 1 stitching via within 1 mm of the signal via. Recommended: 2 stitching vias (one on each side of the signal via). Best: 4 stitching vias arranged symmetrically (forming a cage around the signal via). Each additional stitching via reduces the transition inductance by approximately 30-50%.

What is backdrilling and is it worth the cost?

Backdrilling (also called controlled-depth drilling or stub removal): a drill bit removes the unused via stub from the back side of the PCB after the through-hole via is plated. Cost: $0.50-5 per via (incremental over standard fabrication). Worth it when: the via stub causes measurable signal degradation at the operating frequency (typically above 10-15 GHz). For most designs below 10 GHz: backdrilling is not necessary. For 28+ GHz 5G and 25+ Gbps data: backdrilling or blind vias are standard practice.

Keep Reading