XBee®/XBee‐PRO® ZB SMT RF Modules
Design Notes for RF Pad Modules
The RF Pad is a soldered antenna connection. The RF signal travels from pin 36 on the module to the
antenna through an RF trace transmission line on the PCB. Please note that any additional components
between the module and antenna will violate modular certification. The RF trace should have a
controlled impedance of 50 ohms. We recommend using a microstrip trace, although coplanar
waveguide may also be used if more isolation is needed. Microstrip generally requires less area on the
PCB than coplanar waveguide. Stripline is not recommended because sending the signal to different PCB
layers can introduce matching and performance problems.
It is essential to follow good design practices when implementing the RF trace on a PCB. The following
figures show a layout example of a host PCB that connects an RF Pad module to a right angle, through
hole RPSMA jack. 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 module 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 the PCB manufacturer should be consulted for the exact width.
Assuming d=0.025", and that the dielectric has a relative permittivity of 4.4, the width in this example
will be approximately 0.045" for a 50 ohm trace. This trace width is a good fit with the module
footprint's 0.060" pad width. Using a trace wider than the pad width is not recommended, and using a
very narrow trace (under 0.010") can cause unwanted RF loss. The length of the trace is minimized 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. Any ground fill on the top layer
should be spaced at least twice the distance d (in this case, at least 0.050") from the microstrip to
minimize their interaction.
Implementing these design suggestions will help ensure that the RF Pad module performs to its
specifications.
PCB Layer 1 of RF Layout Example
© 2010 Digi International, Inc.
15
DCD [ DIGITAL CORE DESIGN ]
