2.3 RF Traces and Components

It is mandatory to follow the recommendations as listed:

• The RF traces from RTX and PA1OP pins of the IS2083BM to the antenna must be 50 Ohm controlled impedance trace.
• Copy exact routing and placement for the RF section layout design (RTX and PA1OP connections) from the reference design module layout. These controlled impedance traces must reference a ground plane on a lower layer and to be adjusted, depending on the dielectric and copper weight used.
• Do not route any other traces in the RF area on any layer. This ground reference plane must extend entirely under the tuner.
• Be sure to add as many ground Vias as possible.
• Connect all the ground layers together (ground stitching) along the RF traces and throughout the area, where the RF traces are routed.
• Add at least two ground Vias for every ground pad around the RF components. Place all the ground Vias along the RF traces on either side.
• Connect the center ground pad of the IS2083BM to the inner ground layer, using a grid of Vias (as suggested in the BM83 module reference design). The ground path going from the ground pad down to the ground plane must be absolutely as low impedance as possible.
• Do not use thermal relief pads for the ground pads of all components in the RF path. These component pads must be filled with the ground copper.
• Ensure that the route from the antenna to IS2083BM is as short as possible and is completely isolated from all other signals on the board. No signals must route under this trace on any layer of the board.
• Ensure that when IS2083BM is active, all the digital signals which are toggled are placed away from the antenna. The digital signals must not be placed near the antenna. All the digital components and switching regulators on the board must be shielded to avoid the noise generated by the antenna.