English is currently available.
Wi-Fi DISCUSSION
I moved from an ESP32 dev board to my own two-layer PCB with the same WROOM module. RSSI at the same spot dropped from about -55 dBm to -75 dBm. The module sits in the middle of the board with ground pour on both layers underneath, and the board is mounted in a plastic case next to a metal bracket.
What are the layout rules for a module with a PCB antenna, and if I later use a module with an external antenna connector or a chip antenna, how do I route the 50 Ω trace?
A loss of that size is what copper under the antenna typically costs. The meander trace at the end of the module is the antenna, and it needs free space: no ground pour, no traces and no components under or immediately around it on any layer. With ground directly beneath, the antenna is detuned away from 2.4 GHz and radiates poorly.
The module datasheet shows the recommended placement: the antenna end at the edge of the board, preferably overhanging it or with the PCB cut out underneath, and otherwise a clearance of about 15 mm around the antenna area. A module in the middle of a board with pour on both sides is the worst case. Twenty decibels is a factor of 100 in power, which corresponds to a tenfold loss of range in free space.
The enclosure matters as much as the board. Metal close to the antenna, such as your bracket, a battery, a display or a shielded cable, reflects the signal and detunes the antenna; keep metal parts a couple of centimetres or more away from the antenna end, and never between the antenna and the outside. Plastic walls should not touch the antenna either: a few millimetres of air gap avoids shifting its resonant frequency, since plastic has a higher dielectric constant than air. Metallised paints and carbon-filled plastics act like metal.
A PCB antenna is also not uniform in all directions, so test the product in its real mounting position rather than lying flat on the bench.
For an external antenna, a chip antenna or a coaxial connector on your own board, the trace from the RF pin must be a 50 Ω transmission line, and its width depends on the stack-up. On a standard 1.6 mm two-layer FR-4 board, a plain microstrip over the bottom ground plane needs a width close to twice the board thickness, about 3 mm, which is impractically wide next to a small pad. The usual solution is a grounded coplanar waveguide: the trace runs between ground pours on the top layer with a small controlled gap and stitching vias along both sides, which allows a much narrower trace.
Calculate it with an impedance calculator using your manufacturer's actual stack-up and dielectric constant rather than copying a number.
Keep the RF trace short and straight, with no stubs, no sharp corners and no layer changes if possible, and keep the ground under it unbroken. Provide footprints for a matching network next to the antenna or connector: a pi arrangement of three small parts, initially fitted with a 0 Ω series resistor and the two shunt positions empty.
Chip antennas in particular depend on the ground plane size and clearance given in their datasheet, and they nearly always need those matching components tuned on the final board in the final enclosure, ideally with a vector network analyser. Keep switching regulators and fast digital lines away from the antenna area, since they raise the noise floor the receiver sees.
To verify a new layout, compare like with like. Place the dev board and your board at the same spot and orientation a few metres from the access point, log RSSI for a minute each and compare the averages; single readings move by several dB. Repeat in two or three orientations and with the enclosure closed.
One regulatory point for a product: modules are certified with their own antenna or with specified antenna types. Using the module's PCB antenna as intended keeps you within that certification, while a different antenna may require new testing, so check the module's certification documents before choosing.
Back to Wi-Fi community
