• State Verified Answer
  • Replies 3 replies
  • Subscribers 70 subscribers
  • Views 1012 views
  • Users 0 members are here
Attachments (2) Download All
Nordic Case Info
  • Case ID: 295507
Options

PCB Hardware Review - nRF52832 pre-certified module (FSC-BT630)

builder01

nRF52832_PCB_module_v2.zipcustom_symbols_footprints.zip

Hi,

I'd like to have a HW review.
I have designed a PCB around the FSC-BT630 module which includes the nRF52832.

I have included all the files necessary for your to check it out in KiCAD v6.

Goals:

  • Have a low-power buzzer module that I can turn on/off from a distance (10-20m).
  • A regular smartphone will be the intended client.
  • Flexibility for testing different settings:
    • CR2032 or CR2450 battery
    • Self-driving H-bridge for buzzer or differential driving from 2 module PWM pins.
    • Coarse estimation of battery capacity
    • Test whether an LDO is needed or not (either use jumper or LDO, but not both)

Details:

  • The size of the PCB was designed for a Candemboss CBRS01V enclosure.
  • Programming pin-header w/ VDD2V7, RESET, SWD_CLK, SWD_IO and GND
  • Grounded holes for enclosure
  • 2-layer board with signal and ground layers.
  • FSC-BT630 module

Here are some of the relevant screenshots of my design:

Questions:

  • For via shielding around antenna, I assumed 5GHz as the highest frequency (2x2.55GHz). Using the lambda/20 rule-of-thumb, it came out to be 1.4mm. Is this overkill (i.e. should've just used 2.5GHz or is it a safe assumption?
  • Is it possible to program this board from a nRF52832 or nRF52840 DK board?
  • Should I add more via stitching around the board?

Please, let me know if you need anything else.

Thanks in advance! Slight smile

  • +1

    Hi,

    The PCB looks mostly OK, the only changes I recommend is to add a ground fill to the top layer, and extend the keepout area around the antenna upwards since there is room on the PCB.

    For via shielding around antenna, I assumed 5GHz as the highest frequency (2x2.55GHz). Using the lambda/20 rule-of-thumb, it came out to be 1.4mm. Is this overkill (i.e. should've just used 2.5GHz or is it a safe assumption?

    Are you referring to the spacing between the vias?

    This spacing is not critical, as long as there are vias connecting the edges of the ground planes together. For reference the spacing between the vias on the DK is 5mm.

    Is it possible to program this board from a nRF52832 or nRF52840 DK board?

    Yes, but there may be some problems if the board is powered by 2.7V during the programing. The debugger on the DKs does only support 3V VDD. As a workaround during programming the batteries can be removed and the board powered by the 3V VDD from the DK.

    Should I add more via stitching around the board?

    The vias around the edges of the board is plenty, no need to add any more here. If you add a ground fill to the top layer, adding addition vias tying the ground fills together is recommended. Having vias every 5-10mm should enough.

     

    Best regards,

    Bendik

  • 0 in reply to Bendik Heiskel

    Hi Bendik,

    Many thanks for your reply.

    By "extend the area round the antenna upwards" do you mean the following:


    Extend the keepout area up north of the PCB and shift the current bordering vias to surround the extended keepout area?

Related
Terms of service