PCB antenna desing nRF52832 with accelerometer

[davidesteban13]

Hello,

 

I am trying to fabricate a board based on the Thingy design, including the accelerometer.

 

I positioned the components, traces, vias and pads following some recommendations found in this forum, used the same components found in the Thingy BOM and I will do the assembly by hand because I need to have it working ASAP.

 

Following is the link of my board: easyeda.com/editor shape is because I need to match the space available in the housing…I have these questions:

 1. I added more vias to have more contact between the ground planes (following one recommendation), I tried to do it locating them in the empty space of my board. Are they correctly positioned?

 2. However, in Altium I see that the vias are 0.305 mm and my local PCB manufacturer only handles vias minimum of 0.4 mm…could this be a problem for the performance of the ground planes?

 3. In the Thingy design the antenna is in the border of the PCB, and at least on two sides there are no components. In my design I had to put part of the  ground plane close to one of the antenna sides, leaving only one side with nothing around. Do you think this could cause a problem?

I sincerely appreciate if you see something that I am not taking into consideration on the design.

[Andreas]

Hi,

 

The link does not direct to your design, but to the start page of the tool you've used. You need to link to your design specifically. I am not familiar with this tool so not sure how/if that is possible, if not just export some images or something of the design.

 

1. Not able to answer until I see the design
2. No this will not be a problem.
3. Potentially, depending on the specific antenna part you used. Exactly how much is hard to say, but you should probably be able to establish at communication if you place the devices right next to each other(it should not kill the communication entirely, just limit the max range).

 

Best regards,
Andreas

[davidesteban13]

hello Andreas, thanks for answer, this is the correct link https://easyeda.com/editor#id=89cadac81a994c709d8385a8e9b905d2|e96e4c6f2e414b9288230fb4b0801b6a 

[davidesteban13]

I'm sorry, the PCB appears only when you copy and paste the link...

[Andreas]

Hi,

 

The design looks good. C22 and C24 is not needed, but it does not seem you've moved forward to your layout with them, so this is fine. One thing I really recommend you fix is the keepout for the antenna, similar to what is shown in the datasheet(making a 'corner') or as I attempted to illustrate here:

Lastly, you might also want to remove the connection between C25 and the ground pour to the right, only ground it into the center pad through pin 31. This will improve spurious rejection of the filter.

 

Best regards,

Andreas

[davidesteban13]

Hi Andreas, Thank you very much for your suggestions, i will fix my PCB design and make it, when i finish i will tell you how it work.

[Andreas]

Hi,

 

Happy to help, looking forward to hear how it works.

 

Best regards,

Andreas

[davidesteban13]

Hello,

I tested the PCB with the two designs (with and without changes), and the difference is big; I'm using a PCA10031  as a sniffer with the nRF Connect  (BLE). In the boards I programmed a beacon with +4 dbm. The first PCB works with -65 to -70 dbm at ~10 cm of the PCA10031 and the other  between -46 to -50 dbm. After that I tested a distance of 6 meters with a wall between those, i can´t see the first PCB and the second have -75 to -80 dbm. So the changes works very good.

Thank you very much.