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

[Hardik]

Hi

I am developing 4 layer PCB for the nRF51822 with a power and a ground plane in the inner layers. I will be using a balun from Johanson Technology (2450BM14E0003) with the Johanson Technology (2450AT18A100)chip antenna.
PCB thickness will be 63 mils.

Please help to solve below queries:

1. The product specification of the nRF51822 says that I need to put a keep-out area under the antenna matching circuitry. Is this keep-out also needed when using a balun? Or can I both have a power and a ground layer there?

2. Stack up considered.

    Top layer ( Antenna RF trace )
    Gnd layer
    Power layer
    Bottom layer
50 ohm impedance matching should be coplanar waveguide right?

3. What trace width should i consider in top layer for 50 ohm RF Antenna trace from Balun to Chip antenna.

4. What reference layer should be consider for RF antenna trace, gnd layer or power layer?

5. what should be seperation of gnd plane from RF trace on same top layer? twice of tracewidth or thrice of trace width?

6. If possible share stack of four layer with 63 mils of pcb thickness.

[Andreas]

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