2.4 RNWF11 Module Routing Guidelines

  • Use the multi-layer host board for routing signals on the inner layer and the bottom layer.
  • The top layer (underneath the module) of the host board must be ground with as many GND vias as possible (see Figure 2-9 and 54-Lead RF Module With Shield (6YX) - 20.5x24.5 mm [MODULE]).
  • Avoid fan-out of the signals under the module or antenna area. Use a via to fan-out signals to the edge of the RNWF11 Module.
  • For better GND connection to the RNWF11 Module, solder the exposed GND pads of the RNWF11 Module on the host board.
  • For the module GND pad, use a GND via of a minimum 10 mil (hole diameter) for good ground to all the layers and thermal conduction path.
  • It is recommended to have a series resistor on the host board for all GPIOs. These resistors must be placed close to the RNWF11 Module. For the placement of the series resistor, see Figure 2-9. Pin 26 through pin 30 on the RNWF11 Module are critical pins to have series resistors. For more details on these pins, see Table 2-1.
  • All Ethernet TX and RX signals trace lengths (RMII interface) are matched on the RNWF11 Module PCB.
  • USB differential pair signals are 90Ω impedance matched on the RNWF11 Module PCB and the same must be followed on the host board.
  • SOSC crystal (32.768 kHz) on the host board must be placed close to the RNWF11 Module and follow the shortest trace routing length with the minimum number of vias (see Figure 2-9 and Figure 2-10).
    Figure 2-9. Example Host Board Top Layer
    Note:

    1. For the recommended RNWF11 Module footprint, see 54-Lead RF Module With Shield (6YX) - 20.5x24.5 mm [MODULE].

    Figure 2-10. Placement and Routing of SOSC Crystal