nRF24L01+ Antenna and Board Design

I would like to tightly integrate a nRF24L01+ with my microcontroller. I have read as much as I could, and copied as closely as I can, but the best layout required moving components from the examples. I tried to move components I thought might be less sensitive to being moved... I would love to get a more experienced opinion before I run boards. Any feedback is appreciated. Thanks!

Instead of multiple via's separating the antenna from circuit would it be better to cut a slot to more thoroughly separate the antenna or do the via's add something?

0402 components throughout. 

FA-20H 16.0000MF12Z-AC3 oscillator

I got the antenna design from: https://www.cypress.com/file/136236/download page 10

I plan to run boards from JLCPCB: JLCPCB specs

  • Hi, 

    could you upload the schematic and gerber files? 

    FYI, this is a public ticket, change to private if you want the information to be confidential. 

    Best regards,
    Kaja

  • Hi Kaja, thanks for looks at this. I attached the Gerber files, the Solidworks PCB files and a PDF of the schematic. thanks, -mike

    nRF24L01+ Antenna and Board Design.zip

  • The tracks between the ANT pins and L1 should be symmetrical. So the best will be to turn the whole 24L01 with the external component 90 degrees CW. You will end up with the matching network near the middle of the board, but you can have the antenna in the same position by using a coplanar waveguide (50 ohm transmission line) between C6 and the antenna feed point. You can calculate the dimensions of the waveguide by either using an online calculator or download Appcad http://www.hp.woodshot.com/ Remember to set the PCB material to FR4.

    You also need a ground plane on the top layer. Just one via pr. ground connection isn't enough and will have too much series inductance to ground. Take a look at the reference layout for the nRF24L01+ and see how it's done there.

    Also note how the ground plane is pulled back around the matching network to reduce capacitance to ground:nRF24LU1P_Reference_Layout_Rev1_0.zip

  • Thank you so much. This was very helpful. 

    One more question: Is there a recommended component list that I can reference?
    I have the component values from the reference materials, but I was hoping there were "suggested components" that I can use to ensure I meet all the required component specifications.

    thanks again, mike

  • The reference design is made with Murata LQP15-series inductors. The capacitors are standard NP0 for the small ones in the RF section. 

    For the crystal, mostly anything goes here, but select one with a low CL value, 6-7 pF, for faster startup and lower current draw. Calculate the load caps, C1 and C2, as follows: 

    Ccap = CL * 2 - C(pin and track), where Cpin and track is 1-2 pF.

    Make sure the total tolerance (initial and temperature) is less than 60 ppm

Related