Custom NRF52840 board design review

[LJBouman]

Hello,

I have designed my own custom NRF52840 board for my own apllication. I tried to gather as much information about the NRF as possible and put it in an schematic. I am building the PCB in EASYEDA but first i want to make sure the schematics are right. The purpose of the PCB is to control an laser diode by an smartphone app using the BLE network of the SoC. The schematic consist of 2 sheets and i will try to explain everything as good as possible. 

Sheet 1: (Power supply)

4237.Sheet 2.pdf 

USB-C Connector: The board is going to be charged and programmed by an USB-C cable.

Battery Charging: The PCB is powered by an 3.7V LiPo battery which is charged via the TP4056 IC.

Battery Protection: The LiPo is protected by the DW01 and FS8205.

Vin -> 3.3V: The battery voltage is converted to 3.3V (VDD) for the NRF52840 by the NCP114.

Laser Diode: The laser diode is powered by an constant current circuit.

Battery: Solder pads for the battery.

Sheet 2 (Controller): 

2654.Sheet 1.pdf

USB -> UART: The CP2104 is used to program the NRF52840 by an USB cable.

Crystals: The crystals for the NRF52840

NRF52840: The SoC itself. 

I have a couple questions about this project:

- Are my power nets designed the right way ?

- Is the NRF52840 going to work like this ?

- I connected the ANT pin untill the antenna itself. I need to look further into this which antenna is good for this project but maybe somebody can already help me with this ?

- Maybe my biggest question of this whole project. This PCB is eventually going to be mass produced after the prototypes are tested and fully working. What is the best way to program a board like this when its going to be mass produced. I saw somebody do it this way and i liked it because it uses the USB port. But i also saw that they use the SWDIO and SWDCLK pins but i dont know a lot about this. Can somebody help me with this ?

- Final question. Are there any other upgrades i can make for this schematic ?

[LJBouman]

Hi Bendik, you can make it public again.

Kind regards,
Léon

[Bendik Heiskel]

Hi again Léon,

No problem, most customers want the design files to be private, so I made it private just in case it was mistakenly made public.

You mention that you are using the nRF52840, but the SoC used in the schematic does not match up with any of the versions of the nRF52840. Based on the pin numbering  it looks like the nRF52832 have been used:

There are differences in the required external components between the nRF52840 and the nRF52832 so this part of the schematic must changed  to match the nRF52840 reference schematic. The nRF52840 comes in 3 different packages, which all have different external component requirements.

- Are my power nets designed the right way ?

The aQFN73 and the WLCSP versions of the nRF52840 can be used in high voltage mode which accepts a input voltage range of 5.5V to 2.5V. This means that you can remove the NCP114 and supply the nRF52840 directly from the battery.

USB -> UART: The CP2104 is used to program the NRF52840 by an USB cable.

- Maybe my biggest question of this whole project. This PCB is eventually going to be mass produced after the prototypes are tested and fully working. What is the best way to program a board like this when its going to be mass produced. I saw somebody do it this way and i liked it because it uses the USB port. But i also saw that they use the SWDIO and SWDCLK pins but i dont know a lot about this. Can somebody help me with this ?

To program the device over UART you must first flash a bootloader to the nRF52840,  for this you have to use the SWD interface and a external programmer or nRF52840DK. So the SWDIO and SWDCLK pins must be available to connect the programmer.

- Is the NRF52840 going to work like this ?

The current schematic wont work with the nRF52840, i recommend you copy the reference design for the version of  the nRF52840 you are planning on using. You can upload  the updated schematic for me to do a second review.

- I connected the ANT pin untill the antenna itself. I need to look further into this which antenna is good for this project but maybe somebody can already help me with this ?

There is multiple types of antennas you can use,  the main categories are PCB and chip  antennas. PCB antennas are very cheap, as the are made from PCB traces. Chip antennas are easy to use, as you just need to copy the antenna footprint from the antenna datasheet. Both types of antennas needs to be tuned,  which is something we can help with, if you don't have the equipment to do  it yourself.

We have a paper on designing a monopole PCB antenna,  available here:  https://infocenter.nordicsemi.com/pdf/nwp_008.pdf?cp=18_19

The design and production files for the nRF52840DK and the nRF52840 dongle are also available for download,  the nRF52840DK  uses a monopole PCB antenna, while the nRF52840 dongle uses a meandering PCB antenna.
https://www.nordicsemi.com/Products/Development-hardware/nRF52840-Dongle/Download?lang=en#infotabs

https://www.nordicsemi.com/Products/Development-hardware/nRF52840-DK/Download#infotabs

 

Best regards,

Bendik

[LJBouman]

Is an simple antenna layout like this going to work ? I found some other projects with the NRF52832 where this setup worked. I don't need long range for Bluetooth, max like 5 meters

[Bendik Heiskel]

This looks better, but there are still a couple of points that needs to change:

• No traces can be routed under RF path, these 3 traces must be moved:
  
• A antenna matching network is needed to match the antenna impedance, and tune the resonance frequency. For this type of antenna I recommend using a pi network(shunt-series-shunt). The values of the components must be determined by measuring the antenna impedance and SWR, so as a starting point the shunt components can be NC, and the series component a 0 Ohm resistor.

Other than this the layout looks good.

 

Best regards,

Bendik

[LJBouman]

I change the 3 traces under the RF path, that is fixed now. Can you maybe explain a little bit more about the antenna matching network ? I am really unexperienced about that part.. Or can you give me an example matching my PCB ? I found an example of an pi network, is this what you mean ? How does this setup look on the PCB itself ?

Isn't it better for me to copy the monopole antenna from the DK board ? Maybe it is an easier solution for this board because i dont need that long range anyway

[Bendik Heiskel]

LJBouman said:

I found an example of an pi network, is this what you mean ? How does this setup look on the PCB itself ?

Yes, this is what I meant. The nRF52840 dongle uses a Pi network for the antenna matching, here is a snippet from the layout showing how the components are placed:

The most important part, is that the matching network is placed close to the antenna.

LJBouman said:

an you maybe explain a little bit more about the antenna matching network ? I am really unexperienced about that part.. Or can you give me an example matching my PCB ?

We have a paper outlining the antenna matching process: https://infocenter.nordicsemi.com/pdf/nwp_017.pdf?cp=18_15,

Since not all of our customers have the required equipment for tuning the antenna, we offer tuning antenna tuning free of charge for designs using our SoCs. When the prototypes are produced you can create a private ticket requesting tuning. At the same time we will also measure the output from the radio, and tune the radio matching network. This will make sure the harmonic distortion is not causing spurious emissions above the regulatory limits.

LJBouman said:

Isn't it better for me to copy the monopole antenna from the DK board ? Maybe it is an easier solution for this board because i dont need that long range anyway

The monopole antenna will still required tuning. They only require one shunt capacitor as the matching network, but the length of the antenna will also be adjusted during tuning. This means that a second revision of the PCB must be made after the antenna have been tuned, with the new antenna length.

[LJBouman]

I choosed a monopole antenna and added one shunt capacitor (C4) of 1.2pF to the schematic. I calculated the antenna matched network for my PCB (picture of the AppCAD calculation is added). I also designed my own antenna with an appx length of 25.8mm so it can always be trimmed to the required length. I added the new version of the PCB.

[Bendik Heiskel]

I recommend avoiding the sharp corner in the antenna, a more rounded bend would be better.

Other than this the antenna looks good.

 

Best regards,

Bendik