Suggestion for NRF52832 custom PCB

[Sweety]

Hi,

I have designed a custom PCB using NRF52832 IC.I have followed Sparkfun NRF52832 breakout board for placement of NRF52832 IC core part(including antenna) which is similar to the recommended reference design in the datasheet. SparkFun board link: learn.sparkfun.com/.../nrf52832-breakout-board-hookup-guide

My board dimensions: 100x50 mm.

Is this design OK? Need improvements/suggestions for my design. .

Layout:

Ground planes:

Layout after adding polygon cut-outs around matching circuit elements:

[Jørn]

Hello Sweety

I had your previous case, and I apologize for the lack of response. I was out travelling and just got back today.

You have 3 lines running under your RF section, P22, P23 and P24. The ground plane under the RF section should be whole and unbroken. Any holes in the ground plane will affect the characteristic impedance of the segments, and will affect the matching of the matching network, as well as cause unwanted emissions. I would advise you to route these lines away from your RF network, and keep the ground plane underneath the RF section whole. You should also ensure that the line leading from the nRF52 matching network to the antenna matching has a characteristic impedance of 50 Ohm.

Unfortunately I cannot comment too much on the antenna as we do not have any guidelines for meandered inverse F antennas, and their analysis is not straightforward. Additionally, antennas are very dependent on environment. The layout of your board, product casing etc. will affect its impedance. Optimally you should do measurements of an antenna prototype while it is in an environment that closely matches the one it will be used in, and tune the match based on that.

Considering the antenna was used for an nRF52832 it should work fine if followed exactly and if it is properly matched, granted it was working properly on the reference design. When following the reference designs you should consider substrate type and thickness. Nordic Semiconductor's reference designs are all made for FR4 substrate, with 1.6mm thickness from top to bottom layer. If a different substrate and/or thickness is used the matching networks may need tuning.

If you want to do your own antenna design you would want an EM solver in which you can define your antenna structure and surrounding environment. With this, you could then find the input impedance of your design and simulate the far-field of the antenna. What design parameters to consider will depend greatly on the antenna type. Alternatively you can use reference designs and then use a vector network analyzer to measure S11 of your antenna, and then tune the antenna/adjust the matching based on that.

Nordic Semiconductor also offers tuning services for your design. Go to nordicsemi.com and create a MyPage case stating you would like help to tune the antenna and include your design files.

Best regards

Jørn Frøysa

[Jørn]

I don't think your board dimensions and shape should matter too much, however as previously stated the antenna is always sensitive to its surroundings. Be sure to have a good ground for your antenna. Via fences can be used to limit radiation in the board, to better shield sensitive components. Top and bottom ground planes should be well connected with Vias, and be sure not to leave any floating islands. As for the RF section you should keep your traces as short as possible, to ensure low loss and impedance transformation. Lumped components used in matching should preferably be kept small to reduce parasitics.