• State TI Thinks Resolved
  • Replies 3 replies
  • Answers 1 answer
  • Subscribers 63 subscribers
  • Views 44 views
  • Users 0 members are here
Support feedback
Options
Options
Related

TPSM8287A12: How to design thermal pad & vias on the PCB for TPSM8287AXX/TPS6287X and how to process soldering correctly

Andrew Su
Intellectual 1605 points
Part Number: TPSM8287A12
Other Parts Discussed in Thread: TPS6287B25, TPS62870,

Tool/software:

dears,

Our power modules, such as TPSM8287AXX, always have 3 thermal pads as below picture shows:

I checked the datasheet and EVM user guide, there is no detailed guidance on the PCB design and soldering skills for the PADs,  just find a picture as below:

There are only 2 vias for each PAD-- but I find that the user guide of TPS6287B25 says to use 9 150um vias on the thermal pads, which is correct?  I read some articles on the internet, they recommend multi vias to improve thermal dissipation capacity and  <250um vias to limit the solder leakage,  are they right? Should the customer use blind vias or put solder resist to the vias before soldering?

In addition, as the thermal pads are a bit big, it may cause the difficulty to mount the device on the PCB. How to secure the welding quality to avoid non-firm soldering? Should the 2 GND thermal pads on the PCB top layer need to be separated or prefer to combine them in a bigger plane? 

 Please help to share me the guidance on the PCB thermal pad & vias design and soldering process.

 

Thank you!

  • 0
    TI__Guru**** 150650 points

    Hi Andrew,

    Which customer is this for?

    Every device has a different number of thermal pads.  TPS62870 has 1, TPSM8287A has 3, TPS6287B has 3, TPSM8287B has 3 or 4, etc.  In all cases, the package drawing has a recommended land pattern and stencil design, which should include thermal vias.

    Much more information on vias and board design is given in this app note: https://www.ti.com/lit/an/slua271c/slua271c.pdf

    As the app note explains, the via and board design must be discussed with the CM that assembles the devices onto the PCB and the board shop that makes the raw PCB.  The board technology and capabilities of each are critical to having a good assembly yield.  There is no right or perfect answer for all customers.

    In most cases, it is desirable to prevent solder wicking down into the via.  The app note explains several ways to do this, with a small vias size (like 150um or 250um) being a common solution.

    Thanks,

    Chris

  • 0 in reply to Chris Glaser
    TI__Intellectual 1605 points

    Dear Chris,

    i noticed that the QFN and SON PCB Attachment Application Note recommends NSMD pad style:

    NSMD pads are recommended over SMD pads due to the tighter tolerance on copper etching compared to
    solder masking. In addition, the NSMD pads help to contain the solder paste within the solder mask opening.
    NSDM, by definition, also provides a larger copper pad area and allows the solder to anchor to the edges of the
    copper pads, thus providing an increase in wettable surface area.

    But in the TPSM8287A12 datasheet, SMD is recommended:

    For best manufacturing results, create the pads as solder mask defined (SMD) when some pins (such as VIN, VOUT,
    and GND) are connected to large copper planes. Using SMD pads keeps each pad the same size and avoids
    solder pulling the device during reflow.

    which one should be recommend?

    Should the 2 GND thermal pads need to be separated or prefer to combine them in a bigger single plane? the EVM board separated the GND pads.

    Thank you!

  • 0 in reply to Andrew Su
    TI__Guru**** 150650 points

    Hi Andrew,

    Usually, the customer discusses these details with their CM and does not need TI to inform them.  Is something different for this case?

    The NSMD vs. SMD discussion is one such item.  Power devices are different in that their thermal pads (and other pins) are connected to large planes.  This grows the pad area compared to NSMD pads.  It also does not give exposed copper on the vertical edges of the pad, like for most NSMD pads, since there is no edge present--it continues into a copper plane.

    We do recommend 2 distinct GND pads under the part.  There should be soldermask between them to control where the solder paste flows to.  There is a solid copper GND plane under the IC, but soldermask separates the pads into 2, in order to match the pins on the IC.

    Chris