• State Resolved
  • Locked Locked
  • Replies 3 replies
  • Subscribers 64 subscribers
  • Views 4809 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

bq51013 YFF package layout guidelines and PCB manufacturing design rules

Pentleman
Intellectual 970 points
Other Parts Discussed in Thread: BQ51013

I have a prototype with the bq51013 in the YFF package.   I followed the layout guidelines as shown in the documentation for the BQ51013EVM-725 - Evaluation Module for bq51013

There are six pads that required vias and I took my best shot at the layout.    We are struggling with putting the bq51013 YFF package down on the first board as it looks like the board house grew the pads with the vias.   I should have asked this before having the board fabbed, so here are my PCB layout questions:

1) What is the recommended pad size for the YFF package?   (I used 0.20 mm which is approx. 8 mil for 1oz copper pcb)

2) What is the recommended via and hole size for the 6 signals that need routing from the center of the part?  (I used 0.228 mm/ 9 mil via with 5 mil hole size)

3) What is the recommended finish for the PCB?  Can you have a leaded (non-ROHS) finish?

4) The ball material under the column "Lead/Ball Finish" says 'Call TI' in the device data sheet under Package Option Addendum.   Which phone number?

5) What is the melting temperature of the ball material?   Is there a recommended temperature (we are guessing 255 C)?

Thanks,

Thom

  • 0
    TI__Guru 65716 points

     

     

      1.) Recommended pad—See attached PDF file---Also the bq51013 (YFF) footprint on the EVM (HPA725) used a Non-Solder Mask Defined Pad size is 10mil / 0.254mm, with mask clearance of at 12mil / 0.305mm

      2.) We have used 6 mil drill hole in pad then plated over for flatness. See below table for pins that use Via on EVM (HPA725).

      3.) Finish can be Emersion Gold, ENIG or Emersion Silver, we have used both.

      4.) YFF Ball material is Tin/Silver/Copper

      5.) Melting Temp—see attached PDF file which includes solder profile.

     

    EVM (HPA725) Pin with Via:

    A1-PGND

    A2-PGND

    A3-PGND

    A4-PGND

    E2-Clamp2

    E3-Clamp1

    F2-VTSB

    F3-AD_EN

    Gerber files for the bq51013 (YEE) EVM can be found in the EVM Product Folder under Technical Documents – TI Software

    www.ti.com/tool/bq51013evm-725

    Bill

     

    WCSP_PCB_Design_Application_Note.pdf
  • 0 in reply to Bill Johns
    Prodigy 10 points

    Bill:

    From the gerbers for the EVM it appears that the pad size is 10mil with a solder mask diameter at 14mil.   Is the 12 mil solder mask  figure in your reply in error or is that the preferred diameter?

    Matt

  • 0 in reply to Matt Kahn
    TI__Guru 65716 points

    Matt

    For a non-solder mask defined pad and Bump Diameter of 0.250mm (9.84mil) the recommend copper pad is 0.230mm (9.05mil) and solder mask opening 0.310mm (12.2mil).  This is based on slide 4 of the attached presentation.

    But consult you PCB manufacturing house regarding their capability and experience with this package. 

    We are using a 10mil pad and 14mil opening and have had good results.

    Bill