RF PCB Design Guide

RF PCB design operates under a different set of rules than standard digital board layout. At frequencies above approximately 100 MHz, every trace becomes a transmission line, every via introduces an impedance discontinuity, and every ground plane gap creates an unintended slot antenna. This guide covers the practical layout decisions that determine whether an RF PCB performs to specification or fails on the bench — focusing on the choices that matter most during the transition from schematic to manufactured board.

Transmission line geometry

At RF frequencies, signal traces must be designed as controlled-impedance transmission lines. The characteristic impedance of a trace depends on its width, the dielectric thickness to the reference plane, the dielectric constant of the laminate, and the copper thickness. Microstrip (trace on the outer layer with a ground plane below) is the most common RF transmission line type because it is easy to probe and tune. Stripline (trace between two ground planes) provides better shielding and lower radiation but is harder to access for tuning.

For a 50-ohm microstrip on Rogers 4350B (Dk 3.48, 10 mil dielectric), the trace width is approximately 22 mil. On standard FR-4 (Dk 4.2, 10 mil dielectric), the same 50-ohm target requires approximately 18 mil trace width. The specific geometry must be calculated using a field solver (not the simplified formulas found in textbooks) because edge effects, copper roughness and solder mask loading all influence the actual impedance.

Ground plane strategy

A continuous, unbroken ground plane directly beneath the RF signal layer is the single most important requirement for good RF PCB design. Every gap, slot, split or routing channel in the ground plane creates an impedance discontinuity and a potential radiation source. Even a narrow slot cut by a trace on the ground layer can shift the resonant frequency of a filter, increase the insertion loss of a transmission line, or couple energy between circuits that should be isolated.

When a ground plane must accommodate vias, route them outside the RF signal path footprint. When power planes must cross beneath RF traces, place stitching capacitors at the boundary to maintain AC ground continuity. For mixed-signal boards with separate analog and digital ground regions, merge the grounds at a single point beneath the ADC/DAC rather than splitting the ground plane into isolated islands.

Via design for RF

Vias at RF frequencies are not just electrical connections — they are inductors. A standard 10-mil via through a 62-mil board presents approximately 0.5 to 1 nH of inductance, which becomes significant impedance at frequencies above 1 GHz. For RF grounding vias (connecting component ground pads to the ground plane), use multiple vias in parallel to reduce the effective inductance. Place grounding vias as close to the component pad as physically possible.

Via fencing — a row of ground vias along both sides of an RF trace — reduces radiation from microstrip lines and improves isolation between adjacent RF channels. The via spacing should be less than one-quarter wavelength at the highest operating frequency to prevent waveguide-mode propagation between the vias.

Material selection for RF

Standard FR-4 is usable for RF designs up to approximately 1-2 GHz, depending on loss budget and trace length. Above 2 GHz, the increasing dissipation factor of FR-4 causes unacceptable insertion loss in longer traces. Rogers 4350B and 4003C are the most common RF laminates for designs from 1 GHz to 10 GHz. For frequencies above 10 GHz and through millimeter-wave, PTFE-based laminates (Rogers RT/duroid, Taconic) provide the lowest loss but require specialized processing during fabrication.

Hybrid stackups — RF layers on Rogers or PTFE with digital layers on FR-4 — offer a practical compromise for mixed-signal designs. The RF section gets the low-loss laminate it needs while the digital section uses cost-effective FR-4. AstroPCB manufactures hybrid stackup RF boards with impedance control across both material types.

Component placement for RF

RF component placement follows signal flow: input at one side of the board, output at the other, with gain stages, filters and frequency conversion blocks arranged in the signal path sequence. This linear flow minimizes the risk of output-to-input coupling that causes oscillation or gain flatness problems. Keep high-gain amplifier stages physically separated from sensitive receiver front-end circuits. Use shielding cans or board-level compartmentalization when isolation requirements exceed what layout separation alone can provide.

Manufacturing considerations

RF PCB design decisions that look correct in the EDA tool can become manufacturing problems if fabrication tolerances are not considered. Trace width tolerance affects impedance. Dielectric thickness variation affects impedance. Copper roughness affects insertion loss at high frequencies. Solder mask thickness and coverage affect microstrip impedance. Discuss these tolerances with the fabricator during design — not after the boards fail RF testing.

AstroPCB provides impedance-controlled RF PCB fabrication on Rogers, PTFE and hybrid stackups with manufacturing tolerance to ±8% on controlled impedance traces. The engineering team reviews RF layouts for manufacturability before fabrication begins.

Request an RF PCB Quote →