SPRAA99C March   2008  – May 2021 AM3351 , AM3352 , AM3354 , AM3356 , AM3357 , AM3358 , AM3359 , AM4372 , AM4376 , AM4377 , AM4378 , AM4379 , OMAPL138B-EP , TMUX646

 

  1.   Trademarks
  2. 1Introduction
  3. 2PCB Design Considerations
    1. 2.1 Solder Land Areas
    2. 2.2 Conductor Width/Spacing
    3. 2.3 High-Density Routing Techniques
    4. 2.4 Via Density
    5. 2.5 Conventional PCB Design
    6. 2.6 Advanced Design Methods
  4. 3Reliability
    1. 3.1 Reliability Calculations
    2. 3.2 Package Characteristics
    3. 3.3 Thermal Modeling
  5. 4Surface-Mounting nFBGA Packages
    1. 4.1 Design for Manufacturability (DFM)
    2. 4.2 Solder Paste
    3. 4.3 Solder Ball Collapse
    4. 4.4 Reflow
    5. 4.5 Inspection
  6. 5Packing and Shipping
    1. 5.1 Tray Packing Method
    2. 5.2 Tape-and-Reel Packing Method
    3. 5.3 Tape Format
    4. 5.4 Device Insertion
    5. 5.5 Packaging Method
  7. 6Sockets
    1. 6.1 The Design Challenge
    2. 6.2 Contacting the Ball
    3. 6.3 Pinch Contact
    4. 6.4 Micro Tuning Fork Contact
    5. 6.5 Texas Instruments Sockets
  8. 7Summary
  9.   A Frequently Asked Questions
    1.     A.1 Package Questions
    2.     A.2 Assembly Questions
    3.     A.3 Small Body nFBGA Package Questions
  10.   B Package Data Sheets
  11.   C Thermal Modeling Results
  12.   Revision History

2.1 Solder Land Areas

Designs of both the nFBGA package itself and the printed circuit board (PCB) are important in achieving good manufacturability and optimum reliability. In particular, the diameters of the package vias and the board lands are critical. While the actual sizes of these dimensions are important, their ratio is more critical. Figure 2-1 illustrates the package via-to-PCB configuration and Figure 2-2 illustrates why this ratio is critical.

GUID-166816E5-3B48-4229-8376-E4F1CB5F505A-low.gif Figure 2-1 Package Via to Board Land Area Configuration
GUID-EAEA2F7B-2C7C-43C8-BEEC-D4474B50DC1A-low.gif Figure 2-2 Effects of Via-to-Land Ratios

In the top view of Figure 2-2, the package via is larger than the PCB via, and the solder ball is prone to crack prematurely at the PCB interface. In the middle view, the PCB via is larger than the package via, which leads to cracks at the package surface. In the bottom view, where the ratio is almost 1:1, the stresses are equalized and neither site is more susceptible to cracking than the other.

Solder lands on the PCB are generally simple round pads. Solder lands are either solder-mask-defined or non-solder-mask-defined.

  • Solder-mask-defined (SMD) land. With this method, the copper pad is made larger than the desired land area, and the opening size is defined by the opening in the solder mask material. The advantages normally associated with this technique include more closely controlled size and better copper adhesion to the laminate. Better size control is the result of photo imaging the stencils for masks. The chief disadvantage of this method is that the larger copper spot can make routing more difficult.
  • Non-solder-mask-defined (NSMD) land. Here, the land area is etched inside the solder mask area. While the size control is dependent on copper etching and is not as accurate as the solder mask method, the overall pattern registration is dependent on copper artwork, which is quite accurate. The tradeoff is between accurate dot placement and accurate dot size.

For an example of optimum land diameters and configurations for a common nFBGA pitch, see Table 2-1.

GUID-D616BF6A-52C8-4E95-83FB-79495DA95E89-low.gif
GUID-EF150858-EFF8-4D5D-9C4D-066963D736C5-low.gif It is not recommended to use "U" shape PCB land because of trapping void during reflow.
Figure 2-3 Optimum Land Configurations
Table 2-1 Optimum Land Configurations
All Measurements in mm Ball Size, SMO, Pad Size and Apertures are Shown in Diameters
Ball Pitch Solder Mask Type PCB Design Stencil Design Area Aspect Ratio
SMO Pad Size Thickness Aperture
0.4 SMD 0.225 0.300 0.076 0.250 0.82
NSMD 0.300 0.225
0.5 SMD 0.300 0.400 0.100 0.300 0.75
NSMD 0.400 0.300
0.65 SMD 0.350 0.450 0.127 0.350 0.69
NSMD 0.450 0.350
0.8 SMD 0.400 0.500 0.152 0.400 0.66
NSMD 0.500 0.400
1 SMD 0.450 0.550 0.152 0.450 0.74
NSMD 0.550 0.450
  • Area Ratio = Area of Aperture / Area of Aperture Wall
  • For optimal release of solder paste, Area Ratio ≥ 0.66 is recommended.