nrf52840 pcb layout

[Stas]

Hello! I'm drawing a circuit with nrf52840 chip and I want to ask some questions:

1. Is it ok to use 2-side pcb (not 4)? what's of these better in part of radio communication?
2. for connecting to inner rows of pins I have to use vias with diameter about 0.15mm for footprint, I ask it because to produce pcb with hole less that 0.2mm much more expensive (more than two times). The central GND PAD (74 pin) is not allow to go through inner room to other layer. Is there any solution to avoid so tiny hole in pcb? Can I use vias with 0.2/0.35 for fanout?
3. I'm gonna use RFX2401 Power amplifier. Are there some advices for use it with this chip? pros and cons use it. Thanks!

[FormerMember]

1) Yes, it should work fine to use a 2-layer PCB instead of a 4-layer PCB. With respect to the radio performance, the only difference will lay in the ground layer. When using 2-layer PCB, the ground plane will not be as large and solid as when using a 4-layer PCB. But other than that, it should be fine.

2) Using 0.2/0.35 vias should be ok, but check with your PCB supplier to verify that they are ok with the reduction in annular ring. Please note that it is recommended to specify capping of the vias to ensure good soldering of the pads.

Both the layers will have to be ground layers, to get proper performance. Therefore, the chip should be grounded via the via holes.

3) I don't have any specific advices for that PA/LNA, just remember to place it in the 50 Ohm reference point, after all the components in the reference layout.

Update March 2nd 2017: Answer to Roger Clark's comment

Yes, the large pad under the nRF52840 is necessary. The pad is the main ground "source" for the chip. VSS and VSS_PA is ground, so they should simply be connected to the center ground pad, see the reference layout.

Since the ground pad under the chip is necessary, there should not be any tracks there. Tracks directly under the chip would in any case also be risky, there is a risk of a short circuit with/to the chip.

Regarding two ground layers: Yes, the ground layer is "one half of the antenna"/a mirror. In addition, ground is the reference for the system. A larger ground plane is more stable than a small one (changes less depending on the surroundings). Since the impedance of the antenna is 50 Ohm with respect to ground, a more stable ground plane will result in a more stable antenna impedance.

Yes, I would recommend you to have a lot of via holes connecting the two ground layers. Separate ground layer pieces in the top layer will need via holes to the bottom ground plane to be the same ground reference as the rest of the ground layer.

[FormerMember]

I have updated my answer to answer your comment.