Design notes for RF pad devices

The RF pad is a soldered antenna connection. The RF signal travels from pin 33 on the device to the antenna through an RF trace transmission line on the PCB. Any additional components between the device and antenna violates modular certification. The controlled impedance for the RF trace is 50 Ω.

We recommend using a microstrip trace, although you can also use a coplanar waveguide if you need more isolation. A microstrip generally requires less area on the PCB than a coplanar waveguide. We do not recommend using a stripline because sending the signal to different PCB layers can introduce matching and performance problems.

Following good design practices is essential when implementing the RF trace on a PCB. Consider the following points:

• Minimize the length of the trace by placing the RPSMA jack close to the device.
• Connect all of the grounds on the jack and the device 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 0.028") from the microstrip to minimize their interaction.

Additional considerations:

• 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 33 of the device to the RF pin of the RPSMA connector.
• The RF trace 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.

Implementing these design suggestions helps ensure that the RF pad device performs to its specifications.

The following figures show a layout example of a host PCB that connects an RF pad device to a right angle, through-hole RPSMA jack.

Number	Description
1	Maintain a distance of at least 2 d between microstrip and ground fill.
2	Device pin 33.
2	RF pad pin.
3	50 Ω microstrip trace.
4	RF connection of RPSMA jack.

The width in this example is approximately 0.025 in for a 50 Ω trace, assuming d = 0.014 in, and that the dielectric has a relative permittivity of 4.4. This trace width is a good fit with the device footprint's 0.335" pad width.

Note We do not recommend using a trace wider than the pad width, and using a very narrow trace (under 0.010") can cause unwanted RF loss.

The following illustration shows PCB layer 2 of an example RF layout.

Number	Description
1	Use multiple vias to help eliminate ground variations.
2	Put a solid ground plane under RF trace to achieve the desired impedance.