# PCB antenna placement for small connected devices

> Getting PCB antenna placement right matters more than the radio chip: edge position, keep-out, matching networks and tuning inside the real enclosure.

- Author: Milo Perović, Founder & lead engineer
- Published: 2026-10-21
- Topic: Hardware

Most range complaints we see on small connected devices are not radio problems. They are PCB antenna placement problems, decided months earlier by someone squeezing a battery connector into the last free corner of the board. This post is for founders, product managers and engineers who are about to lay out a board with a chip antenna, a printed trace antenna or a module, and want it to work inside the real enclosure.

The radio silicon is rarely the weak link. A modern BLE or Wi-Fi chip will happily deliver its datasheet output power into 50 ohms. What happens across the next few centimetres of copper, plastic and battery decides the range.

## Why the antenna is part of the board, not a part on it

A chip antenna or a printed inverted-F antenna is only half an antenna. The other half is the ground plane it works against. The vendor's datasheet figures for gain and efficiency are measured on a specific evaluation board, with a specific ground size, in free air. Change the ground, and you have a different antenna.

For 2.4 GHz, the free-space wavelength is about 122 mm, so a quarter wave is roughly 30 mm. Ground planes much shorter than that along the antenna axis start to cost efficiency and shift resonance. At 868 MHz the quarter wave is around 86 mm, which is why sub-GHz LoRa devices on a matchbox-sized board are hard: the ground plane is simply too small to be a good counterpoise, and losing several dB is normal unless the layout is planned around it. We cover the radio choice itself in [picking between BLE and LoRa before picking the chip](https://miloperovic.com/journal/ble-or-lora-picking-the-radio-before-picking-the-chip/); this post assumes that decision is made.

## PCB antenna placement rules we start every layout with

These are the rules we apply before routing a single signal. Nearly all of them are in the antenna or module datasheet, and they are still broken on most boards we review.

- **Edge, ideally a corner.** The antenna sits on the board edge with the feed pointing inwards, so that radiation is not shadowed by ground on three sides. Many chip antennas are specified for a corner or short-edge position only.

- **Keep-out on every layer.** No copper, no ground pour, no traces and no components under or around the antenna on any layer, for the full clearance area the datasheet specifies. A single inner-layer ground pour under the antenna can wreck it.

- **Module antennas overhang or get clearance.** Modules such as the ESP32-WROOM family recommend that the antenna section extends past the carrier board edge, or that a generous copper-free area is left beneath and beside it. Check the exact figure in the module's hardware design guidelines rather than copying a footprint from an old project.

- **Nothing tall or metallic nearby.** Batteries, coin cell holders, USB connectors, shielding cans, buzzers, displays and screws all detune and absorb. Keep them well away from the antenna, and never behind it.

- **Solid, stitched ground.** The ground plane next to the antenna should be continuous and stitched with vias along its edge, so the return current sees one clean plane rather than a patchwork of islands.

## The feed line and matching network

Between the radio pin and the antenna there should be a short, controlled-impedance 50 ohm line and a footprint for a matching network. On two- and four-layer boards that line is usually a grounded coplanar waveguide, with a row of ground vias either side. Ask the fabricator for their stack-up before you calculate the trace width; a guessed dielectric thickness is a guessed impedance.

We always place a pi network (series element plus a shunt to ground on each side) even when the vendor says none is needed. Populated with a 0 ohm resistor and two unfitted shunts, it costs almost nothing. Without it, the only way to fix a detuned antenna after the enclosure arrives is a board respin.

Keep the feed line short and straight, avoid vias in it where possible, and keep switching regulators, crystals and fast digital lines away from both the line and the antenna. Noise coupled here shows up as reduced sensitivity, not an obvious fault. The same discipline helps later with [EMC pre-compliance testing](https://miloperovic.com/journal/emc-pre-compliance-testing-before-you-book-a-lab/).

## What the enclosure does to your antenna

Plastic is not transparent to an antenna in the near field. Any dielectric close to the antenna lowers its resonant frequency, and the effect grows quickly as the wall gets closer. A board that measures beautifully on the bench can be shifted noticeably lower once it is screwed into an ABS or polycarbonate housing a millimetre or two away.

Other enclosure decisions matter just as much:

- **Metallic paints, plating and fillers.** Metallic-effect finishes, vacuum metallisation and some conductive or glass-filled grades can attenuate badly. Ask for the exact grade and finish before signing off CMF.

- **Metal parts and inserts.** Brass heat-set inserts, screws, a metal bracket or an aluminium face plate near the antenna will all detune it.

- **Mounting surface.** A device that will sit on a metal shelf, a wall or a pipe needs testing in that position. Its ground and pattern change with what it is attached to.

- **Hands and bodies.** Wearables and handheld devices are detuned by the user. Tune with a hand or a body phantom in place, or at least check the margin.

## Tuning and verifying on the bench

Tuning is done on the assembled board, in the real enclosure, with the battery and every other part fitted. We measure the antenna's reflection coefficient (S11) with a vector network analyser through a short pigtail, soldered to the feed after disconnecting the radio. The usual target is better than about -10 dB across the band of interest, which corresponds to a VSWR of roughly 2:1. Then we adjust the pi network components until the resonance sits centred in the band with margin on both sides.

A good S11 does not prove a good antenna; it only proves that power goes in. A lossy antenna buried behind a battery can match well and still radiate poorly. So we follow up with radiated checks:

- Compare received signal strength against a reference device, such as the vendor evaluation board, at a fixed distance and orientation.

- Rotate the device through several orientations to find nulls, especially for products whose mounting position is fixed.

- Run a range walk in a realistic environment with the firmware's actual transmit power, data rate and packet size.

- Where the budget allows, book a short slot in an anechoic chamber for total radiated power and sensitivity. It is far cheaper before certification than after.

## Chip antenna, PCB trace or external

The right antenna type depends on board size, enclosure and cost target.

OptionStrengthsWatch out for

Printed trace (inverted-F, meander)Near-zero part cost, repeatable, well documented reference designsNeeds board area and a correct stack-up; hard at sub-GHz on small boards

Ceramic chip antennaSmall, flexible placement, vendor tuning supportVery sensitive to ground size and keep-out; needs a matching network

Certified module with integrated antennaShortest path to certification and a known layoutStrict keep-out and overhang rules; placement dictates board shape

External or flex antenna on u.FLBest performance, can be placed away from noise and metalExtra part and assembly step, cable routing, connector reliability

## What we would do before committing to a layout

If we were about to release a board for its first prototype run, this is the short checklist we would walk through:

- Antenna position fixed first, at an edge or corner, before any other component is placed.

- Datasheet keep-out applied on every copper layer, including inner layers.

- Pi matching footprint placed close to the antenna feed, with a 50 ohm line calculated from the fabricator's real stack-up.

- Battery, connectors, inserts and metal parts kept clear of the antenna in the 3D model, not just in the 2D layout.

- Enclosure material and finish confirmed as RF-friendly, with wall distance to the antenna known.

- A tuning session with a VNA booked for the first assembled boards in the real housing, followed by a reference-device range test.

Getting PCB antenna placement right costs a few hours of planning. Getting it wrong usually costs a respin, a delayed certification slot and a product that quietly underperforms in the field.
