RF pad version
The RF pad is a soldered antenna connection on the surface-mount device. The RF signal travels from pin 36 on the module to the antenna through a single ended RF transmission line on the PCB. This line should have a controlled impedance of 50 Ω.
For the transmission line, we recommend either a microstrip or coplanar waveguide trace on the PCB. We provide a microstrip example below, because it is simpler to design and generally requires less area on the host PCB than coplanar waveguide.
We do not recommend using a stripline RF trace because that requires routing the RF trace to an inner PCB layer, and via transitions can introduce matching and performance problems.
The following figure shows a layout example of a microstrip connecting an RF pad module to a through-hole RPSMA RF connector.
- The top two layers of the PCB have a controlled thickness dielectric material in between. The second layer has a ground plane which runs underneath the entire RF pad area. This ground plane is a distance d, the thickness of the dielectric, below the top layer.
- The top layer has an RF trace running from pin 36 of the device to the RF pin of the RPSMA connector. The RF trace's width determines the impedance of the transmission line with relation to the ground plane. Many online tools can estimate this value, although you should consult the PCB manufacturer for the exact width. Assuming d = 0.025 in, and that the dielectric has a relative permittivity of 4.4, the width in this example will be approximately 0.045 in for a 50 Ω trace. This trace width is a good fit with the module footprint's 0.060 in pad width.
We do not recommend using a trace wider than the pad width, and using a very narrow trace can cause unwanted RF loss. You can minimize the length of the trace by placing the RPSMA jack close to the module. All of the grounds on the jack and the module are connected to the ground planes directly or through closely placed vias. Space any ground fill on the top layer at least twice the distance d (in this case, at least 0.050 in) from the microstrip to minimize their interaction.
| Number | Description |
|---|---|
| 1 |
XBee |
| 2 | 50 Ω microstrip trace |
| 3 | Back off ground fill at least twice the distance between layers 1 and 2 |
| 4 | RF connector |
| 5 | Stitch vias near the edges of the ground plane |
| 6 | Pour a solid ground plane under the RF trace on the reference layer |
Implementing these design suggestions helps ensure that the RF pad device performs to specifications.
PDF
