12.2 Routing Guidelines

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

  • Follow the RF trace design as highlighted in RF Trace Layout Design Instructions for leveraging the ATSAMR30M18A certifications.
  • In a four or higher layer PCB design, dedicate the layer immediately below the layer containing the ATSAMR30M18A module for GND.
  • Avoid routing any traces in the region on the top layer of the host board which will be directly below the module area.
  • Place GND polygon pour below the module covering the entire area. Do not have any breaks in this GND plane. Place sufficient GND vias in this polygon pour for better RF performance.
    For optimal performance, the GND plane of the host board must have an minimum area of:
    • 30 mm x 35 mm (for chip antenna - 0900AT43A0070)
    • 70 mm x 50 mm (for external antenna - W1910)
    • 101 mm x 101 mm (for external antenna - ANT-916-CW-QW-SMA)
  • Place at least one GND via next to the GND module pinout.
  • The RF trace from RF OUT of the ATSAMR30M18A module to the antenna feed point must be 50Ω single ended controlled impedance trace.
  • Place guard GND vias along the RF trace running from module to feed point of the antenna, in the host PCB. The area directly below the RF trace must have a GND polygon pour, at least in the immediate layer below Top layer.
  • Do not have any signal traces below/adjacent to the RF trace in the host PCB. This is applicable to all layers below the highlighted region in the following image.
  • Do not use thermal relief pads for the GND pads of all components in the RF path. These component pads must be completely filled with GND copper polygon. Place individual vias to the GND pads of these components.
  • It is recommended that the antenna in the host board 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 antenna.
  • Do not enclose the antenna in the host board within a metal shield.
  • Keep any components which may radiate noise or signals within the 850-950 MHz frequency band away from the antenna and if possible, shield those components. Any noise radiated from the host board in this frequency band degrades the sensitivity of the module.
  • Make sure the width of the traces routed to GND and VCC rails are larger for handling the peak TX current consumption.
Figure 12-14. Top Layer Routing