PCB antenna not scannable

RE: PCB antenna not scannable

Bendik Heiskel — Fri, 14 Nov 2025 09:54:53 GMT

Hi,

There's a couple of changes needed to be the board layout:

There must be a GND layer directly under the SoC. It looks like there is no copper fill on L2:

For 4 layer boards we recommend having a copper fill on L2 but with a cutout under the RF section. This cutout should also be on L3 such that the bottom layer is the reference GND plane for the transmission line. The cutout helps reduce the capacitance of the trace and component pads. Here is some snippets showing how this should be implemented from the nRF52DK which is a 4 layer board:

The nRF52DK hardware files can be downloaded here:
https://www.nordicsemi.com/Products/Development-hardware/nRF52-DK/Download
The via grounding C3 must be removed, this capacitor should instead be grounded to the center GND pad:

This helps increase the attenuation of the 2nd harmonic frequency.

Other than these two points the design looks good.

Best regards,

Bendik

RE: PCB antenna not scannable

Wade Brainerd — Thu, 13 Nov 2025 13:01:52 GMT

Following up, I found several issues with the design:

1. Ground plane under the PCB antenna. I misread the instructions to imply I needed a ground fill on the bottom layer under the entire antenna. This is removed in the latest design. The purple in the image posted is a back side coin cell battery that is locked, and KiCad is shading the locked footprint, but there is also a ground plane.

2. When selecting my parts with JLCPCB, I accidentally allowed a substitute 40Mhz crystal in place of the 32Mhz crystal. Amazingly the device boots and all peripherals work, but this would not allow BLE to function from my understanding.

3. Unrelated, but one of the LEDs is connected to a NC pin. D'oh

I have an updated design, if a Nordic engineer is available to review it, the production files and KiCad sources are here:
github.com/.../production_files

Thanks!

RE: PCB antenna not scannable

Wade Brainerd — Wed, 12 Nov 2025 20:20:55 GMT

Regarding crystal, I hadn't done anything special with the crystal.

The one on the PCB is this: jlcpcb.com/.../8588879124262109184

The description reads 40Mhz but the comment says 32Mhz. How can I tell which one I got?

After this comment I added the following lines to prj.conf, but they had no effect. (I believe because they control the 32Khz crystal, not the 32Mhz one)

CONFIG_CLOCK_CONTROL_NRF=y
CONFIG_CLOCK_CONTROL_NRF_K32SRC_RC=n
CONFIG_CLOCK_CONTROL_NRF_K32SRC_XTAL=y

RE: PCB antenna not scannable

Wade Brainerd — Wed, 12 Nov 2025 16:50:46 GMT

Reading https://devzone.nordicsemi.com/guides/hardware-design-test-and-measuring/b/nrf5x/posts/general-pcb-design-guidelines-for-nrf52-series, it indicates that there is supposed to be a ground plane under this kind of antenna:

Monopole quarter wave, printed PCB antenna: This antenna is easy to make and easy to tune, and it only needs one shunt components for impedance matching in addition to the antenna length. Space: About 23 mm long and needs a minimum of 5 mm clearance to the ground plane.
See the white paper on monopole quarter wave antenna.

RE: PCB antenna not scannable

Turbo J — Wed, 12 Nov 2025 16:30:19 GMT

Layout looks like there is a ground plane below the PCB antenna? That won't work - usually. Most PCB antenna designs require that no metal is anywhere near them AFAIK.

NRF chips are very sensitive for the main crystal as these are constantly turned off and on. If you did not use one of the few specified parts, it probably won't work.