• State Resolved
  • Locked Locked
  • Replies 8 replies
  • Subscribers 81 subscribers
  • Views 718 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.

Tombstone shaped PCB pads for the MSP430F5528IRGC

oldViking
Expert 1160 points

The MSP430 package I am using specifies a PCB pad with a tombstone shape (a rectangle capped with a semicrcle). 

The problem is that my PCB layout package (Eagle) does not support a pad of this geometry.

Is it OK to substitute a pad with a rectangular shape ?

If so,  should the rectangular pad be the full height of the tombstone or should I shorten the height of the rectangle by cutting off  the semicircle ?

Thank you for your assistance.

Roy Nordstrom

 

  • 0
    Guru 58965 points

    I think your question can be better answered by the vender that you use to solder the chip.

  • 0 in reply to old_cow_yellow
    Expert 1160 points

    Hi,  

    These were the first people I asked.   They were not willing to offer any advice other than saying that I should follow the recommendations of the data sheet.

    So I am still without a definitive answer.

    Roy

  • 0 in reply to oldViking
    Genius 3330 points

    I use rectangular pads with good results. I ignore the little semi-circle.

  • 0 in reply to eltury
    Expert 1160 points

    Thank you.

    I will do that.

     

    Roy

  • 0
    Guru 25210 points

    Roy Nordstrom1 said:
    he MSP430 package I am using specifies a PCB pad with a tombstone shape (a rectangle capped with a semicrcle). 

    Which document do you see this in? The RGC package drawing document http://www.ti.com/lit/ml/mpqf125e/mpqf125e.pdf shows the shape of the pin/pad on the part, but does not give a recommended PWB land pattern.

    Roy Nordstrom1 said:
    Is it OK to substitute a pad with a rectangular shape ?

    You should use a rectangular pad. Your manufacturing partner should give you guidance on paste aperture.

    Roy Nordstrom1 said:
    If so,  should the rectangular pad be the full height of the tombstone or should I shorten the height of the rectangle by cutting off  the semicircle ?

    It should be bigger than the pad on the device. The QFN pads wrap up the side of the package. You want the PWB pad to extend outside of the package slightly to allow for a good solder fillet. This has the side benefit of allowing tacking a wire or scope probe on for debug.

  • 0 in reply to Brian Boorman
    Expert 1160 points

    Hi Brian,

    I got the PCB layout from page 119 of this document. This is the RGC package.

    http://www.ti.com/lit/ds/symlink/msp430f5529.pdf

    I followed this very closely, except for the semi-circle at the top of the pad, which I cut  off to make a rectangular pad.

    So the pad is 0.28 x 0.71 mm.  I do get the fillet you mentioned, because the pad peaks out from under the part, just as the drawing on page 119 specifies.

    I am questioning whether I would be better off to use a full height rectangular pad (0.28 x 0.85 mm)  or just stay with the short one.

    Thank you

    Roy

     

  • 0 in reply to oldViking
    Guru 25210 points

    I think you are fine with the short one.

  • 0
    Guru 227245 points

    I too use rectangular pads without any problems. I’m surprised you didn’t get a guide from the people who shall do the soldering. They should be able to give you minimum specs regarding pad size and paste mask size for a given pin geometry.

    Usually, I make the pads a bit longer to the outside, and small enough to have a small stripe of soldering resist between them. It makes manual soldering much easier and has never negatively affected automatic soldering (except for a little bit more tin on the pads due to the larger length).

    However, V6 of Eagle supports adding copper to a pad, so you can add the semi-circle to the pads now, if you want (don’t forget to adjust the glue and paste layers). On 4x version, we had to add layer 60/61 for additional copper like this (required for half-circle solder jumpers, or cooling copper in a device package). And explicitly tell the PCB manufacturer about this anomaly.

**Attention** This is a public forum