RE: Four layer PCB stack up for NRF51822. RF antenna trace width.

Andreas — Mon, 05 Nov 2018 15:32:03 GMT

Hi,

1. The keepout is not crucial with a balun. You should still have a ground plane underneath though, but it is fine to use the internal ground layer for this with a balun. With lumped matching components we see that using the internal ground layer as ground plane raises the harmonics quite a bit due to the increased parasittics (thin substrate thickness between top and ground plane), resulting in loosing some output power when tuning the matching network to the the harmonics down. It will work fine, even so, you will just not get all the output power you pay for, and it is thus not recommended.

2. Coplanar waveguide is recommended, yes. If you use the internal ground layer, the thickness will be lower, and thus you have to adjust the width and gap of the trace.

3. Depends on the substrate thickness and material and the gap between the center conductor and ground. Use a calculator for this, e.g. AppCAD.

4. Whichever layer makes up the ground plane you have underneath the RF part. Our reference design uses 1.6mm thickness, using a keepout in internal layers in >2 layer boards.

5. Depends on trace width and substrate again. Suggestion with typical FR-4, 1.6mm thickness: W/G = 1mm/0.2mm, 0.18mm thickness: W/G = 0.3mm/0.2mm

6. See the nRF51-DK HW files.

Best regards,

Andreas