1.3 RF Traces and Components

It is mandatory to follow the recommendations as listed:

• The RF traces from RF_TX and RF_RX pins of the IS1870/IS1871 to the antenna must be 50Ω controlled impedance trace.
• Copy exact routing and placement for the RF section layout design (RF_TX and RF_RX connections) from the reference design module layout. These controlled impedance traces must reference a ground plane on a lower layer and adjust 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 IS1870/IS1871 to the inner ground layer using a grid of Vias (as suggested in the BM70/BM71 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. Fill these component pads with the ground copper.
• Ensure that the route from the antenna to IS1870/IS1871 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 IS1870/IS1871 is active, place all the toggled digital signals away from the antenna. Do not place the digital signals near the antenna. Shield all the digital components and switching regulators on the board to avoid the noise generated by the antenna.