• State
  • Locked Locked
  • Replies 7 replies
  • Subscribers 82 subscribers
  • Views 956 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.

TMS320F28377DZWTS Default footprint

Francisco Amoros
Prodigy 80 points

Other Parts Discussed in Thread: TMS320F28377D

I downloaded the footprint of TMS320F28377DZWTS microcontroller from Texas official website and i want to know if is ready for via-in-pad design or I need to resize smd pads?. I have added a 6 mil via between pads to consider the scale.

Thanks in advance,

Fran.

  • 0
    TI__Expert 8105 points
    Fran,

    The actual dimensions of pads/vias are affected by board house process parameters and cost. Using 6 mil drill diameter may prove to be expensive. A good starting point for this type of package (.8mm pitch) would be:
    1) ball pad diameter = 15.7 mils
    2) via pad diameter = 15 mils
    3) via hole = 7.5 mils

    Regards,
    PEter
  • 0 in reply to Peter Galicki
    Prodigy 80 points
    are you suggesting that I have to use via-in-pad?

    Regards,
    Fran
  • 0 in reply to Francisco Amoros
    TI__Expert 8105 points

    Fran,

    No, definitely not - vias in pad are not recommended as they will wick solder away from the pads during assembly. Please see attached slides for explanation how the vias are placed in between the pads. These slides refer to another C2000 device but are directly applicable here because the package is similar (0.8mm pitch BGA). The dimension provided should give you a good starting point - the actual dimensions will depend on the process requirements of the board house that you are using.

    Regards,
    PEterconcerto_144_BGA_layout.zip

  • 0 in reply to Peter Galicki
    Prodigy 80 points
    In previous designs we have already taken into account, and had used a pad of 13,5 mil with a via hole of 6 or 7 mil.

    The problem has been that when I downloaded the footprint of this new microcontroller (from official website) the pads are 21 mil (not 14 as you said), and hence have asked.

    Why this packagin this way? That's wrong?

    Thank you,
    Fran
  • 0 in reply to Francisco Amoros
    Prodigy 80 points
    webench.ti.com/.../cad.cgi

    and then: TMS320F28377D_ZWT_337.bxl

    Here it is where I downloaded-
  • 0 in reply to Francisco Amoros
    TI__Expert 8105 points
    Fran,

    According to page 6 of SPRAA9 document the recommended BGA pad size ranges between 0.35mm and 0.40mm (13.8mils - 15.7mils) for a 0.8mm pitch BGA packages. We are currently reviewing the webbench generated footprint, but based on the above I would go with the 14 mil pad instead of 21 mil pad. Will keep you posted if there are any changes that come out of this review.

    Regarding the vias, using common 5 mil trace/space design rules puts the maximum via pad diameter at 16.5 mils. This will allow you to route one signal trace between two adjacent vias. Depending on the board house process used and corresponding drill tolerance values, the size of the via hole may vary. But based on our own experience a 7.5 mill hole is a good place to start.

    REgards,
    Peter
  • 0 in reply to Peter Galicki
    TI__Expert 8105 points

    Fran,

    Just to follow up on your BGA footprint question I am attaching a portion of a new document that we are currently sourcing that may be of help to you. This doc discusses IC package mounting consideration for 0.8-mm BGAs.

    Regards,
    PeterBGA_preliminary_15.zip