SigmaDSP PCB Layout Best Practices

Document created by BrettG on Aug 31, 2011Last modified by BrettG on Oct 24, 2011
Version 5Show Document
  • View in full screen mode

Good layout practices are of key importance when designing SigmaDSP system PCBs.


  • First of all, a solid ground plane is a necessity in order to  maintain signal integrity and minimize EMI radiation. If you have two  ground planes, I would recommend using stitching vias spead evenly  throughout the board in order to connect them.


  • Power supply high frequency decoupling capacitors should be placed  as close as possible to the respective power and ground pins, on the  same side of the board as the SigmaDSP IC. There should be no vias  between the pins and the decoupling caps. Please see the following excerpts from the ADAU144x datasheet for more detail.



ScreenHunter_05 Sep. 13 11.09.jpg



ScreenHunter_04 Aug. 31 15.07.jpg


  • Typically, we use a single 100 nF capacitor for each power-ground  pin pair. However, if there is excessive high frequency noise in the  system, an additional 10 nF capacitor can be used in parallel. In that  case, the 10 nF capacitor should be closest, and the thermal connections  should be on the far side of the 100 nF capacitor.



ScreenHunter_06 Aug. 31 15.11.jpg


  • 10 uF capacitors should be used for each named supply (DVDD, AVDD,  IOVDD, etc) in order to provide a current reservoir in case of sudden  current spikes.



ScreenHunter_07 Aug. 31 15.14.jpg


  • If ferrite beads are desired for supply isolation, the beads should always be placed outside of the local high frequency decoupling capacitors, like in the following diagram. If the ferrite beads are instead placed between the supply pin and the decoupling capcitor, high frequency noise will be reflected back into the IC since it does not have a suitable return path to ground, and this will increase EMI and create noisy supplies.


ScreenHunter_02 Oct. 24 14.13.jpg


  • The proximity of components to the IC is important. Here is my  suggested order of priority which should be followed when placing components. The  top of the list begins with the components that should be placed closest to the IC (those in bold have highest priority), and the bottom of the list has the components that can (if absolutely necessary) be placed further away.
    • 10 nF high frequency decoupling capacitors
    • 100 nF high frequency decoupling capacitors
    • PLL filter components
    • Crystal
    • Current reservoir capacitors


  • ICs with exposed thermal paddles require extra attention during PCB design. A copper square matching the geometry of the exposed pad should be placed on all layers the PCB, with thermal vias connecting the layers in order to maximize heat transfer.


ScreenHunter_03 Sep. 13 11.06.jpg


ScreenHunter_04 Sep. 13 11.08.jpg



This FAQ was generated from the following discussion: in case of crash

1 person found this helpful