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.

[Roger Clark]

I have the same sort problems as @stas

I need to use a 2 layer PCB, and I'm not sure the PCB factory can produce "Via in pad"

Is the large pad under the nRF52840 necessary? If I put tracks and vias under the MCU, I will be able to do a cooper pour, to link VSS_PA and the VSS's, but it won't be a solid area

For heat extraction, multiple larger diameter vias will be needed to join the layers for thermal conduction. However I think these can be larger as they are all connected to GND

Also....

Just to confirm, that you recommend both top and bottom layers as GND for best performance. I presume this is for best RF performance, as it is effectively one half of the antenna ?

As the top of my board is where most of the tracks are located, I presume you are recommending using multiple via's to link the bottom layer (which should mostly be solid copper) to areas on the top layer

[FormerMember]

I have updated my answer to answer your comment.

[Roger Clark]

@kristin

Thanks for the update.

Edit. (removed my previous text)

I've looked under at my nRF52832 samples and I can see the large metal pad under them, so I presume you mean the nRF52840 when you said

"Yes, the large pad under the nRF52832 is necessary"

I'll redraw my PCB symbol to include that central metal pad.

Not being able to route tracks under the device, means that either I'd need very thin tracks from the inner pads or that "via in pad" will be needed.

Actually, I'd need to change the design rules, as currently its impossible for me to route between the pads, and I suspect its not manufacturable in that way, as I'd need 0.1 or 0.15mm tracks

Image of PCB track sizes / problems

I'll need to speak to the manufacturer to find out what is possible for them

[FormerMember]

Yes, it should be nRF52840, not nRF52832. (The same will apply for nRF52832; no routing in the center pad.)