3.4 RF Traces and Components

This section describes the recommended layout guidelines with respect to RF trace routing:

  1. The RF trace routed from pins LPA_OUT (18) of the PIC32CX1012BZ24032 device must be designed for a 50Ω impedance-controlled trace.
  2. Be sure to isolate the RF trace from LPA_OUT until the junction of series-matching components are as they are in the reference layout design illustrated in Figure 3-9. A GND polygon pour with a GND via must be added in between the RF traces from LPA_OUT.
  3. In this specific reference layout, RF traces are routed with a thickness of 0.302 mm with spacing to GND polygon pour at 0.158 mm. The following figure illustrates the recommended PCB stack-up details.
    Figure 3-9. RF Front-end Trace Routing Overlaid with Top Assembly
  4. Place guard ground vias along the RF trace on either side of the trace. The PCB layer directly below the RF trace must have a ground polygon pour.
  5. Do not route any signal traces below the RF trace on all the other layers. Also, do not route any signal traces adjacent to the RF trace. The following figure illustrates the locations within inner layer 2 and all the signal traces that are routed away from the RF traces.
    Figure 3-10. Inner Layer 1 – RF Section
    Figure 3-11. Inner Layer 2 – RF Section
    Figure 3-12. Bottom Layer – RF Section
  6. Do not use thermal relief pads for the ground pads of all components in the RF front-end. These pads must be completely connected to the ground copper polygon pour using the direct connect style. Place dedicated vias to ground for all these individual shunt components.
    Figure 3-13. Reference Placement of Guard Ground Vias
  7. Keep any components that may radiate in the 2.4 to 2.5 GHz frequency band away from the antenna and the RF traces, and, if possible, shield these components. Any noise radiated from the board in this frequency band degrades the RF performance of the module.
  8. Adding the RF test point as shown in the following figure is recommended. The circular ring around the RF test point is for the GND contact for the probe from the socket. This test point must be designed based on the recommendation of the probe structure in the test socket design. The purpose of this test point is for the measurement of RF parameters in the production test. In the production test fixture, ensure the antenna is detuned sufficiently so that the maximum RF power is coupled to the RF test point instead of the antenna.
    Figure 3-14. RF Test Point in Bottom Layer with Bottom Solder Mask and Top Assembly Overlaid