CC3000 PCB Design Guidelines

From Texas Instruments Wiki
Jump to: navigation, search

Return to CC3000 Main page

Introduction

This page will walk an engineer through the recommended guidelines for designing a PCB around TI's CC3000 module. It is recommended that a designer follow TI's CC3000 Evaluation Module User's Guide alongside this wiki page.

*NEW* You can now check your design with the CC3000 Checklist. The checklist enables you to verify your design in a series of easy-to-follow steps. The link to the checklist is below.

File:CC3000 Checklist.zip

PCB Design Resources

Reference design files such as schematics, PCB files and gerber files are available from the download page.
Please locate the files for either the evaluation module or the booster pack within that page.


Layout Guidelines Specific to CC3000

PCB Stack

  • The PCB can be two layers, but 4 layers are used in CC3000MOD reference
  • The PCB should be made of standard FR4 material
  • If two-layer PCB, both layers should be used for signal routing.


Module

  • The proximity of ground vias must be close to the pad.
  • Signal traces must not be run underneath the module on the layer where the module is mounted.
  • Have a complete ground pour in layer 2 for thermal dissipation.
  • Have a solid ground plane and ground vias under the module for stable system and thermal dissipation.
  • Increase the ground pour in the first layer and have all of the traces from the first layer on the inner layers, if possible.
  • Signal traces can be run on a third layer under the solid ground layer, which is below the module mounting layer.

 Antenna and RF 


Antenna Considerations

  • Antenna should be located on far side of board, and should be pointing away from any ground plane
  • The trace to the RF antenna should be as short as possible beyond the ground reference to avoid excess creating excess radiation.
  • There should be no traces or ground plane underneath the antenna

RF Trace Considerations

  • A 50-ohm trace impedance match is recommended on the trace to the antenna.
  • RF traces should be as short as possible and located near the edge of the PCB. Consider the enclosure material and proximity when designing.
  • RF traces should have via stiching on ground plane (both sides of trace).
  • RF traces should have constant impedance.
  • The RF trace bends must be gradual with an approximate maximum bend of 45 degrees with trace mitered. RF traces must not have sharp corners.
  • The PCB designer must understand the microstrip model used and the scale line width according to the microstrip model.
  • For best results, the RF trace ground layer must be the ground layer immediately below the RF trace. The ground layer must be solid.


Power

  • The power trace for VBAT should be 40 mil wide.
  • The VIO_HOST trace should be 18 mil wide.
  • Make VBAT traces as wide as possible to reduce inductance and trace resitance.
  • Shield VBAT traces with ground above, below and beside VBAT traces if possible.


Useful Test Points

  • Add points for RS232, this includes RESERVED_1 and RESERVED_2.


Additional PCB Design Resources

For the curious, below are some useful NON-TI resources for designing RF PCB boards:

From EEWeb : Basic Concepts of Designing an RF PCB Board

From Jefferson Lab : RF/Microwave PC Board Design and Layout