SPRAAV1C May   2009  – March 2020 AM3703 , AM3715 , OMAP3503 , OMAP3515 , OMAP3525 , OMAP3530

 

  1.   PCB Design Guidelines for 0.4mm Package-On-Package (PoP) Packages, Part I
    1.     Trademarks
    2. 1  Using This Guide
    3. 2  A Word of Caution
    4. 3  A Team Sport
    5. 4  Be Wary of Quotes
    6. 5  Don’t Forget Your CAD Tools
    7. 6  Metric Vs English
    8. 7  PCB Fab Limits
    9. 8  Routing and Layer Stackup
    10. 9  OMAP35x 0.4mm Pitch
    11. 10 Pad Type
    12. 11 PCB Pad Dimensions for 0.4mm BGA Package
    13. 12 Multiple BGA Packages
    14. 13 Etch Traps and Heat Sinks
    15. 14 Vias and VIP
    16. 15 Laser Blind Vias
    17. 16 Filled Vias
    18. 17 Know Your Tools
    19. 18 BeagleBoard
    20. 19 BeagleBoard Views
      1. 19.1 Top Layer – Signal - Area Underneath the OMAP35x
      2. 19.2 Layer 2 – Ground
      3. 19.3 Layer 3 – Signal
      4. 19.4 Layer 4 – Signal
      5. 19.5 Layer 5 – Power (VDD2)
      6. 19.6 Layer 6 – Signal – Bottom Copper – Bottom Component Outlines
    21. 20 OMAP35x Decoupling
    22. 21 PCB Finishes for High Density Interconnect (HDI)
    23. 22 Real World Second Opinion
    24. 23 Acknowledgments
    25. 24 References
  2.   Revision History

11 PCB Pad Dimensions for 0.4mm BGA Package

Through several meetings with both board fabricators and board assembly houses, the following recommendation has been created for the circuit board BGA footprint for the OMAP35x having 0.4mm or 400 μm, pitch solder balls. Figure 8 shows the top layer with vias down to layer 2.

At the 0.4mm pitch, there is insufficient space between pads to allow a 3mil trace to run between pads without incurring solder bridging. Therefore, except for the outside perimeter balls, all connections are routed to the lower layers through VIP technology. With this technology, only six layers were needed for the BeagleBoard.

For the BeagleBoard design, the desired finished pad size is equal to the solder ball diameter. Since no traces run between the pads, the copper pad is enlarged to 280 μm (11mils). The solder mask opening is set to 254 μm (10 mils).

With this arrangement, there is plenty of solder webbing between pads which helps prevent adjacent ball solder bridging. For more information regarding additional parameters that impact the assembly of this package, see PCB Assembly Guidelines for 0.4mm Package-On-Package (PoP) Packages, Part II.

Pad Type Solder Mask Defined
Pad Pitch A 400 μm (0.4mm)
Mask Opening B 254 μm (10 mils)
Pad Size C 280 μm (11 mils)
Mask Shape Round
Mask Web D 150 μm
Pad to Pad Clearance E 120 μm
Trace Allowed Between No
pad_dim_praav1.gifFigure 8. Recommendations for 0.4mm Pitch Packages - Top Layer