• State
  • Locked Locked
  • Replies 2 replies
  • Subscribers 99 subscribers
  • Views 145 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

AM62P: Ball pad discrepancy

Tom Schultz
Expert 4140 points
Part Number: AM62P

Tool/software:

Team,

Posting on behalf of my customer.

The data sheet for the AM62P gives a ball pad of 0.35mm (13.78mil).  In the SK-AM62P-LP reference design, the pad is 13mil.  A mismatch of the pad diameter to the part diameter will cause reliability issues from what I understand.  Is the pad diameter mismatch from an error in the data sheet or reference design?   Is it enough to cause reliability issues if we were to use a 13 mil copper pad following the reference design?

Please see PROC164E1 within https://www.ti.com/document-viewer/lit/html/SPRT780

Thanks,

Tom

  • 0
    TI__Guru**** 192809 points

    Hello Tom, 

    Thank you for the query.

    Let me check with the team internally and update you.

    Regards,

    Sreenivasa

  • 0
    TI__Mastermind 30140 points

    Hello Tom,

    Matching solder mask opening (SMO) or pad size of the PCB to SMO/pad size of SOC package is ideal to avoid solder ball cracking.
    Refer to SPRAA99 2.1 Solder Land Areas... https://www.ti.com/lit/pdf/spraa99
     - With equal sizes, the stresses are equalized and neither site is more susceptible to cracking than the other.
     - AM62P AMH package is solder mask defined with SMO of 0.35mm diameter

    In that regard the pad diameter on the PCB is in error (not the datasheet).

    However, I suspect tradeoffs were made and I am following up with the PCB designer.
    If the pad diameter is simply increased to 0.35mm (13.78 Mil), spacing constraints between pad and adjacent VIAs are violated:
      Constraint value: 3.08 MIL
      Actual value:     2.72 MIL

    VIAs were already optimized to 17D8 (17 mil pad, 8 mil drill) instead of 18D8 typical of a ~1.6mm board thickness.
    These constraint violations can be resolved by using 16D8 VIAs but then VIA quality may be compromised (with yield impacts).

    I will confirm the constraints are reflective of the capabilities of the PCB fab used.

    Customers need to evaluate their end product classification, IPC requirements, and work with their PCB fab to design for manufacture and board-level reliability.

    Refer also to these helpful websites
    https://www.epiccolo.com/articles/pcb-vias-guide
    https://www.protoexpress.com/blog/dont-let-annular-rings-drive-you-crazy/