nRF24L01+ Antenna and Board Design

[mej7000]

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

[mej7000]

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

[ketiljo]

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

[mej7000]

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

[ketiljo]

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

[mej7000]

Awesome! Thanks!

[mej7000]

choose ​​Murata Crystal​ XRCGB16M000FXN00R0 ​​, which I think meets the specs, however when I calculate C1/C2 I get a value of about 10pF. I expected to get a value closer to the reference Cap value: 22pF. I think the lower Cap value is because the 6pF Crystal CL is  relatively low, but I want to make sure I've got it right.

Did I do something wrong here or does this look ok?​   -Thanks!

​Ccap = 6pf * 2 - (~1.5pf)​ = 10.5pf

XRCGB16M000FXN00R0
Manufacturer:​ ​​​Murata
Load Capacitance:​ ​6 pF
Frequency:​ ​16 MHz
Tolerance:​ ​40 PPM
Frequency Stability:​ ​25 PPM, 30 PPM
ESR:​ ​200 Ohms
Drive Level:​ ​100 uW

p79e-806516.pdf

[ketiljo]

The value of the load capacitors are dependent only of the CL value of the crystal. 22 pF caps are for a 12 pF crystal. 

You can find the crystal spec in the datasheet: 

Note that ESR should be less than 100 ohm. And min CL is 8 pF, sorry for saying 6 - 7 pF earlier. 

This excludes the smallest packages as ESR will increase when the crystal gets physically smaller.