Custom NRF52840 board design review

RE: Custom NRF52840 board design review

Bendik Heiskel — Tue, 21 Mar 2023 10:19:55 GMT

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

RE: Custom NRF52840 board design review

LJBouman — Mon, 20 Mar 2023 13:12:37 GMT

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.

RE: Custom NRF52840 board design review

Bendik Heiskel — Fri, 17 Mar 2023 10:55:50 GMT

[quote user="LJBouman"] I found an example of an pi network, is this what you mean ? How does this setup look on the PCB itself ?[/quote]

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.

[quote user="LJBouman"]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 ? [/quote]

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.

[quote user="LJBouman"]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[/quote]

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.

RE: Custom NRF52840 board design review

LJBouman — Thu, 16 Mar 2023 13:36:43 GMT

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

RE: Custom NRF52840 board design review

Bendik Heiskel — Thu, 16 Mar 2023 12:18:43 GMT

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

RE: Custom NRF52840 board design review

LJBouman — Thu, 16 Mar 2023 08:38:37 GMT

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

RE: Custom NRF52840 board design review

LJBouman — Wed, 15 Mar 2023 15:12:38 GMT

I also have zoomed pictures to view the traces with their names.

RE: Custom NRF52840 board design review

LJBouman — Wed, 15 Mar 2023 15:11:12 GMT

Hi Bendik, thanks voor the review. I updated my PCB design with al the things you mentioned. You think it will be good now ? I left space for the antenna like on the example you sent.

RE: Custom NRF52840 board design review

Bendik Heiskel — Mon, 13 Mar 2023 10:30:28 GMT

Hi Léon,

Sorry for the delay.

The updated schematic looks good. One thing to note is that when you have selected the antenna type you are using you will need to add a antenna matching network between L3 and the antenna. Chip antennas have a recommended matching circuit in the antenna datasheet. The number on matching components needed for a PCB antenna is dependent on the type, monopole antennas with few bends can be tuned with only a shunt component and by varying the length of the antenna. For this type of antenna it is a good idea to make the antenna longer than the theoretical optimal length on the first prototype, its easiest to reduce the length of the antenna when tuning. Antennas with more bends(like the meander antenna used on the nRF52840) should have a pi network, shunt-series-shunt, available when tuning.

[quote user="LJBouman"]Hi Bendik, in the mean time i designed the first version of the PCB itself. I tried to do as much research as possible and process it in the design. If you can review the PCB as well that would be great!
[/quote]

More vias should be added to the center GND pad, we recommend using at least a 3x3 via grid. The SoC needs a good connection to the bottom layer ground to have a stable output from the radio.
C17 should only be grounded to the VSS pin 31 and the center GND pad. In conjunction with the trace impedance this creates a notch filter that helps with attenuating the 2nd harmonic frequency. Here is a snippet from the reference layout showing the correct grounding:
The antenna needs a keep out area on the bottom layer as well, the same size as the one on the top layer.
Both of the crystals must be placed closer to the SoC, its important to minimize the length of the traces between the crystal and the SoC.
The decoupling capacitors on the VDD net must be placed close the VDD pins. The 4.7uF capacitor must be placed close to pin 48, while the two 100nF close to pin 13 and 36.
The decoupling capacitors on the DEC lines must also be placed closer to the SoC.

You can download the design and production files for the reference design here: https://www.nordicsemi.com/Products/nRF52832/Download#infotabs

I recommend you use it as a guide on where the components should be placed.

Best regards,

Bendik

RE: Custom NRF52840 board design review

LJBouman — Fri, 10 Mar 2023 15:56:11 GMT

Comment: The upper section of the PCB is for the antenna

RE: Custom NRF52840 board design review

LJBouman — Fri, 10 Mar 2023 15:48:22 GMT

Hi Bendik, in the mean time i designed the first version of the PCB itself. I tried to do as much research as possible and process it in the design. If you can review the PCB as well that would be great!

RE: Custom NRF52840 board design review

LJBouman — Fri, 10 Mar 2023 10:43:43 GMT

Hi Bendik, again thank you for your usefull answer. I decided to replace the NRF52840 for the NRF52832. It still fits my needs and it might be easier for me. Maybe in the future i can always update to the NRF52840. I updated my schematic (Sheet 1 V2) and have added it in my comment. I also removed the CP2104 and added a header to SWDIO and SWDCLK. I am planning to program my board throug a NRF development board. I still haven't add an antenna but maybe you can review my schematic again ? devzone.nordicsemi.com/.../Sheet-1-V2.pdf

RE: Custom NRF52840 board design review

Bendik Heiskel — Thu, 09 Mar 2023 13:03:03 GMT

It depends on what features you need, the nRF52832 is lacking some of the features of the nRF52840 and it also has less RAM and flash. Here is a list comparing all the nRF52 series devices with each other to help with deciding which device is best for your application:
https://infocenter.nordicsemi.com/topic/struct_nrf52/struct/nrf52.html?cp=5

One feature you might want is the built in USB peripheral in the nRF52840, with this you can get rid of the USB to UART bridge.

[quote user="LJBouman"] LCSC (the component supplier of EASYEDA) has an package of this one available with solder pads on the side instead of the NRF52840 which has it on the underside of the chip. I am planning to solder the first couple of prototypes myself untill i am sure everything works as it should.[/quote]

There is a version of the nRF52840 in a QFN package, nRF52840-QFAA, which is the same package as the nRF52832. This version of the nRF52840 is missing some of the features the other packages have, mainly the high voltage regulator and the USB peripheral.

When you are soldering the chip yourself you have to keep in mind that the center GND pad under the SoC needs a good solder connection to the board. This is important for the radio to function properly.

[quote user="LJBouman"] If i choose for the NRF52832, is my circuitry right and i need to keep the NCP114 right ?[/quote]

Yes, the nRF52832 have a maximum input voltage of 3.6V, keeping the regulator will insure that the supply voltage is within the specifications.

RE: Custom NRF52840 board design review

LJBouman — Wed, 08 Mar 2023 13:25:38 GMT

Thank you Bendik for your review! I am wondering, isn't it easier for me to just choose the NRF52832 for my project ? LCSC (the component supplier of EASYEDA) has an package of this one available with solder pads on the side instead of the NRF52840 which has it on the underside of the chip. I am planning to solder the first couple of prototypes myself untill i am sure everything works as it should. If i choose for the NRF52832, is my circuitry right and i need to keep the NCP114 right ?

RE: Custom NRF52840 board design review

Bendik Heiskel — Wed, 08 Mar 2023 13:03:11 GMT

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.

[quote user=""]- Are my power nets designed the right way ?[/quote]

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.

[quote user=""]USB -> UART: The CP2104 is used to program the NRF52840 by an USB cable.[/quote][quote user=""]- 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 ?[/quote]

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.

[quote user=""]- Is the NRF52840 going to work like this ?[/quote]

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.

[quote user=""]- 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 ?[/quote]

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

RE: Custom NRF52840 board design review

LJBouman — Wed, 08 Mar 2023 10:35:54 GMT

Hi Bendik, you can make it public again.

Kind regards,
Léon

RE: Custom NRF52840 board design review

Bendik Heiskel — Wed, 08 Mar 2023 08:57:05 GMT

Hi,

I have made this case private since you are sharing your schematic files. Let me know if you want the case to be switched back to public.

I'll take a look at the schematic and get back to you with my comments.

Best regards,

Bendik