13.1 Module Placement and Routing Guidelines

It is critical to follow the recommendations listed below to achieve the best RF performance:

• The module must be placed on the host board, and the chip antenna area must not overlap with the host board. The portion of the module containing the antenna must not stick out over the edge of the host board. Figure 13-2 shows the best, poor and worst case module placements in the host board.
  Note: Do not place the module in the middle of the host board or far away from the host board edge.
• Follow the mechanical recommendations as shown in Figure 13-1. The antenna is specifically tuned to the mechanical recommendations depicted in Figure 13-1. The host PCB must have a thickness of 1.5mm.
• Follow the module placement and keepout recommendation, as shown in Figure 13-1.
  • Avoid routing any traces in the highlighted region on the top layer of the host board, which will be directly below the module area.
  • Follow the electrical keepout layer recommendation, as shown in Figure 13-1. There must be no copper in all layers of the host board in this region. Avoid placing any components (like mechanical spacers, bumpon, etc.) in the area above the line indicated in the Figure 13-1.
  • Place the GND polygon pour below the module with the recommended boundary in the top layer of the host board, as shown in Figure 13-1. Do not have any breaks in this GND plane. The GND polygon pour in the top layer of the host board must have a minimum area of 20 x 40 mm.
  • Place sufficient GND vias in the highlighted area below the module for better RF performance.
  • Having a 5x5 grid of GND vias solidly connecting the exposed GND paddle of the module to the ground plane on the inner/other layers of the host board is recommended. This will act as a good ground and thermal conduction path for the ATWILC3000-MR110xA module. The GND vias must have a minimum via hole size of 0.2 mm.
  • The antenna on the module must not be placed in direct contact or close proximity to plastic casing/objects. Keep a minimum clearance of > 7 mm in all directions around the chip antenna.
• Do not enclose the antenna within a metal shield.
• Keep any components that may radiate noise or signals within the 2.4 GHz to 2.5 GHz frequency band away from the antenna and, if possible, shield those components. Any noise radiated from the host board in this frequency band will degrade the sensitivity of the module.
• Make sure the width of the traces routed to GND, VDDIO and VBAT rails are sufficiently larger for handling the peak TX current consumption.