Please note as of Wednesday, August 15th, 2018 this wiki has been set to read only. If you are a TI Employee and require Edit ability please contact x0211426 from the company directory.
CC26xx HW Checklist
HW Design checklist for CC26xx
For proper operation of the CC26xx and for best RF performance it is paramount to follow the reference designs. There might be several application specific reference designs, but the main reference will always be the CC2650EM designs (applies to CC2640R2F as well). Make sure you are using the latest revision by downloading it from the wiki page.
- Verify that all component values are correct. For the RF components and the DCDC-inductor it is also recommended to use the same part numbers.
- Verify that the Exposed Ground Pad (EGP) is connected to ground.
- Check that the crystals are within the required spec. (see CC26xx datasheet and CC26xx Crystals article)
- Note that CC26xx has an internal load cap array on the 24 MHz crystal pins. The cap array supports load cap values from 0 to 10 pF (default setting is CL = 9 pF)
- Note that using crystals with lower CL will decrease start-up time and power consumption. The same is true for lower Lm (motional inductance)
- Are antenna matching components included?
- Ensure that all IO connections are correct (analog functionality, 8 mA capability and sensor controller connection is limited to certain pins).
- Do you need to support Over-the-Air Download (OAD) for updating BLE firmware? If so, consider adding provisions for external serial EEPROM (i.e., SPI flash) to your board if your application size is not able to meet the code size limitations for on chip OAD which is dependent on the product and SDK release. Use the CC2640R2F LaunchPad design files as a reference for adding external SPI flash (applies to all CC26xx BLE designs).
- Ensure that the substrate height (thickness of the dielectric layer between the layout pattern and the undelying ground plane) corresponds to the reference design being copied. For the CC2650EM-XXX reference designs, which are all 2-layer boards, the value is 0.7 mm or 30 mils. For multilayer boards, you can achieve this by placing the ground plane on the layer that most closely corresponds to this height.
- Ensure that the layout of the RF components closely follows the reference design.
- All RF components connected to ground should have multiple ground vias close to their ground pads to minimize ground impedance.
- There must be an uninterrupted and solid ground plane under all the RF components, stretching from the antenna and all the way back to the ground vias in the EGP. There must not be any traces under the RF path.
- The balun and/or RF filter must be placed as close to the CC26xx as possible.
- The antenna matching components should be placed as close to the antenna as possible.
- Ensure that decoupling capacitors are placed as close to the respective VDD pins as possible. It is also important the the ground return path from the decoupling caps and back to the EGP is as short and direct as possible.
- The DCDC components (10 uH inductor and 10 uF capacitor) must be placed close to the DCDC_SW pin. Equally important is the ground connection from the DCDC-cap to the CC26xx EGP. This should be as short and direct as possible to avoid ground switching noise.