• State Suggested Answer
  • Replies 8 replies
  • Answers 1 answer
  • Subscribers 87 subscribers
  • Views 1569 views
  • Users 0 members are here
Attachments (0)
Nordic Case Info
  • Case ID: 349558
Options

nRF52810 Antenna review

Positron

Hello!

I'm preparing a second revision of my first BLE PCB with nRF52810 MCU.

The first iteration worked ok, but BLE range was worse than a ready-made module with PCB antenna. The project is a PCB to control tiny RC models, so PCB size is 10x14mm.

I used a chip antenna that can be mounted in the corner of PCB with a radiating element PCB trace. I chose it for minimal footprint required (5x3mm). Antenna impedance is stated to be 50 ohm.

RF matching part is taken from MCU datasheet.

PCB is 4 layers with GND below RF path (and another GND below that). Width of the wires inside Pi network up to antenna footprint is impedance-matched (I just used JLCPCB calculator)

schematic (relevant part)

top

inner 1

Antenna datasheet, for reference. 1-10nH inductor is required for other variants of placement (and is missing from this edge-mounted variant).

Please suggest what can be improved here. Are there any low-hanging fruits? Considering that: 

1) I don't have a vector analyzer

2) PCB space is very limited, so no space for another full Pi network (in addition to existing one that matches MCU pin to 50 Ohm from datasheet). And I have no way of tuning it anyway due to p1. I added a DNP capacitor though, can place a 1.5pF capacitor from antenna datasheet there.

3) I want to stick to minimum components size of 0402.

  • 0 in reply to Bendik Heiskel

    Ok, thank you! I'll study the document!

    Meanwhile, I've tried to fit 2nd matching network as you suggested, and found ways to add this without stubs (or with 1 stub, or with 2), at the cost of a bit more bendy antenna trace and a capacitor sticking out into decoupling area. 

       

    Which do you think is preferrable? Should I prioritize removing stubs or it's not a big deal because they are small? 

    On a similar note, considering traces between components are about 1mm long, much less than quarter wavelength, how important is impedance-matching them? I can't even decide whether to treat them as microstrip or coplanar waveguide as there is not much ground around them.

  • 0 in reply to Positron
    Positron said:

       

    Which do you think is preferrable? Should I prioritize removing stubs or it's not a big deal because they are small? 

    Either option should be OK. I would go for the layout with the one stub, as this allows for GND vias to be added between the RF section and the 32MHz crystal, improving the shielding between them:

    Positron said:
    On a similar note, considering traces between components are about 1mm long, much less than quarter wavelength, how important is impedance-matching them? I can't even decide whether to treat them as microstrip or coplanar waveguide as there is not much ground around them.

    There's no need to make the RF traces impedance controlled. The only part of the circuit that would be matched to an 50 ohm impedance is the trace between the radio and antenna matching circuit. Since there is no significant length of transmission line between the matching networks there won't be any losses to to impedance missmatch.

Related
Terms of service