nrf52832 4 layers pcb antenna trace design

RE: nrf52832 4 layers pcb antenna trace design

manishmistry — Tue, 17 Dec 2019 11:56:34 GMT

Hi Ketiljo,

I am have same case, in my case I have calculated 50ohm impedance using reference GND layer as inner layer (second layer). So can I remove inner layer keepout area under antenna trace?

or need to keep keepout area under antenna trace in inner layer as per nordic reference design & calculate antenna impedance using bottom layer as reference??

RE: nrf52832 4 layers pcb antenna trace design

ketiljo — Thu, 01 Nov 2018 09:00:49 GMT

Use what's correct for your PCB stackup.

RE: nrf52832 4 layers pcb antenna trace design

Berker — Wed, 31 Oct 2018 21:54:38 GMT

If 0.18mm should be used, the impedance is not 50 ohm. Which one is correct?

50ohm or 0.18mm(not 50ohm)

RE: nrf52832 4 layers pcb antenna trace design

ketiljo — Wed, 31 Oct 2018 09:08:22 GMT

If you remove the inner layers, the thickness will be 1.6 mm. If you keep the second layer as ground, refer to the PCB manufacturers stack up, but 0.18 mm sounds correct.

RE: nrf52832 4 layers pcb antenna trace design

Berker — Wed, 31 Oct 2018 08:15:32 GMT

What should be dielectric thickness? 1.6mm or 0.18mm .

If layer2 reference(solid ground for co-planar waveguide), why we don't use 0.18mm in the formula?

RE: nrf52832 4 layers pcb antenna trace design

ketiljo — Wed, 31 Oct 2018 08:00:24 GMT

Yes, the bottom layer is solid under the RF section:

What happens on the rest of the board doesn't matter here.

RE: nrf52832 4 layers pcb antenna trace design

Berker — Tue, 30 Oct 2018 18:12:46 GMT

Ji ketiljo,

I don't want to take more your time. But I want to understand DK design.

Yes, you need to have a solid ground plane under the waveguide

[quote userid="2125" url="~/f/nordic-q-a/39920/nrf52832-4-layers-pcb-antenna-trace-design/155141"]Yes, you need to have a solid ground plane under the waveguide[/quote]

Layer4 on DK,is not a solid plane.

Layer1:Sİgnal

Layer2:GND

Layer3:PWR+Signal

Layer4:GND+Signal

How is calculated the impedance, although layer4 is not a solid ground?

RE: nrf52832 4 layers pcb antenna trace design

ketiljo — Tue, 30 Oct 2018 13:29:49 GMT

Yes, you need to have a solid ground plane under the waveguide. If you can't use layer 4, use another layer and re-calculate the width.

RE: nrf52832 4 layers pcb antenna trace design

Berker — Tue, 30 Oct 2018 10:06:56 GMT

Hi,

Layer4 is not a continuous ground layer,there's some signals on it. As i know, ground layer under co-planar waveguide should be whole ground.

Why layer2 didn't used instead of layer4? This is a whole ground.

I think if layer2 is used, the calculations should change completely.

Note: I calculated thinner and thicker part impedances. These are about 58ohm and 48ohm respectively.

Thickness of layer2 0.18mm.

RE: nrf52832 4 layers pcb antenna trace design

ketiljo — Tue, 30 Oct 2018 08:29:37 GMT

Technically, you don't need to have the cutout under on the inner layers, the capacitance to ground is low with just the footprint of two components. If you use a transmission line between L1 and the antenna, you need to calculate it using the specification for the board you are using. It's sometimes easier to remove the inner layer because the distance to the inner layers doesn't matter and you don't lock your design to one specific stack up.

The wider track on the DK is the 50 ohm transmission line. It's on the short side so is debatable whether is has an impact or not.

The easiest is to use a co-planar waveguide. You can find on-line calculators or use Appcad to calculate the dimensions. The important parameters are distance to the same side ground plane, distance to the other or inner side ground plane and the track width.