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.

TPS22924CYZPR PWB Footprint with Microvia-in-Pad

We’ve had very high fallout with these parts on our manufacturing floor. We recently had to hand replace every single part of the 21 used on each of our cards as we were having widespread opens and shorts—some latent, but many not. We returned many samples to TI for failure analysis and the conclusion was that either our PWB footprints were wrong, or something in our manufacturing process was wrong.

 

We received and reviewed TI’s Strategies for handling WCSP parts presentation (TI_WCSP_Handling_SK_2012_Nov.pdf) and TI Wafer Chip Scale Package SMT Guidelines, June 2011. We’re in the process of designing a test card that will have some of our old footprints, and many new footprints that are based on TI’s guidance. We’ll use this test vehicle to hopefully replicate our failures with the old footprints, and prove that with the TI-recommended footprints, we can use these parts without high failure rates.

 

In our application, the device pins are typically connected on the PWB in 1 of 2 ways. They are either enveloped in copper pour (for the VIN and VOUT pins), or they are connected by a Microvia-in-pad (for the ON and GND pins). We rarely find ourselves escaping the pins using traces in an HDI design (i.e. blind and buried vias) which is where these parts are typically used. Both of the aforementioned TI documents were silent on the use of Microvias in the pads for these parts.

 

Q1. Please provide any applicable guidance and/or cautions related to the use of Microvia-in-Pad for these parts.

 

At this writing, we are assuming that if the Microvia pad is larger than the TI-recommended pad size for the pin, then we would apply soldermask to create a soldermask defined pad based on TI’s guidance in the TI Wafer Chip Scale Package SMT Guidelines document (pages 6-7). If the Microvia pad is smaller than the TI-recommended pad size for the pin, then we’d just use the TI-recommended pad size.

 

Q2. Please advise if our assumptions regarding TPS22924CYZPR pad size with an embedded Microvia above are incorrect.

 

In either case, we assume the use of a Microvia (i.e. laser drilled hole that’s ~5 mils in diameter, and ~2-5 mils tall, connects the outer layer to the next layer in, and is typically 100% filled with copper) is acceptable for these parts.  We include a PWB drawing note that requires our fabricator to ensure the Microvia dimple does not dip down more than 1 mil into the pad.  We don't specify a limit for a dimple that would protrude from the pad (i.e. if the Microvia plating were to produce an outward dimple); we rely on applicable IPC specifications to limit these, but in practice, we don't see many outward dimples.  They typically are dimples that extend down into the pad.

 

Q3. Please advise if our assumption that it's acceptable to embed a Microvia (as described above) in the pad for the TPS22924CYZPR is incorrect.

  • Hi Bob,

    Sorry to hear you have been having issues.  I will check with our packaging experts on the use of microvia-in-pad.

    Regards,

    Adam

  • Adam,
    I should mention that we downloaded the recommended Allegro footprint from the TI website, and it had 12 mil pads???
    Per the WCSP guidelines we received from TI late last year, 9 mils was the right pad size for non-soldermask defined pads, and for soldermask defined pads, the pad gets bigger, but the soldermask opening is then reduced to 9 mils (to ensure the same exposed, solderable pad size regardless of whether soldermask defined or not).
    We will use mostly soldermask defined pads, as we'll envelop some pins (VIN and VOUT) in external copper pour, and our Microvia-in-pad will likely have a pad that is bigger than the 9-mil recommended pad for this load switch, so we will end up with a soldermask defined pad as well (for GND and ON). That is assuming TI says Microvia-in-Pad is OK for these packages.
    Thanks.Bob K
  • Bob,

    It certainly is OK to use solder mask defined pads on DSBGA (WCSP) devices, as a matter of fact we would encourage you to do so in cases where copper pours would expand the effective pad size beyond the 0.225mm recommendations.

    What is important for DSBGA assembly is that the amount of metal exposed for soldering be the same for *all* device balls, otherwise the device will tilt towards the pads that have a larger exposed metal content.

    A potential problem with microVia on pad is that the dimple could trap air under the paste which expands during reflow, either introducing voids or in extreme cases blowing the ball off. But that occurs only if the via is centered on the pad and hence "capped" by the solder ball on assembly.

    To prevent this of course flat-pad technology is an option. However we have on all our internal designs avoided this extra expense by offsetting the microVia pad away from the center of the component pad.

    In this case (6-bump) all vias can be placed away from the soldering pads, for larger 0.5mm pitch arrays the pitch is wide enough that the dimple can be offset totally off the pad. If you do not have the PCB space to do this, a partial (0.1mm) offset will do. This (x=y=) 0.1mm offset is what we routinely use for 0.4mm pitch devices. It offsets the dimple just enough that any trapped air or organics will not force excessive voids into the solder joint.

    Any further questions, please do not hesitate to let us know. Best regards.

  • Thanks Ernesto.  I do have a follow-on question.  Based on what you said above, and our soldermask registration tolerances, I came up with a rectangular pad that allows us to offset the Microvia hole by 4 mils.  The rectangular pad is large enough that if the soldermask is mis-registered by up to 1 mil, the exposed portion will remain 100% copper (i.e. it won’t fall off the edge of the metal pad if soldermask moves by up to 1 mil).  I’ve attached a PDF that shows the Microvia-in-pad centered (which you indicated is a bad plan).  It also shows the rectangular pad I came up with to solve the problem.  Please review and let me know if you see any issues with adopting this approach.  Thanks.  Bob K.  Harris Corp.Switch Layout rev0.pdf

  • Bob,

    The rectangular pad with horizontal or vertical offset you propose should work for the device you are using since the bumps are on a 2x3 array and the SMD metal pads can be extended outwards away from the device. The x=y=0.1mm diagonal offset we suggested offsets the microVia by about 0.14mm (0.0055"), which is a bit more than what you have, but because it is a shallow dimple it should not matter.

    With a diagonal offset, this solution can be extended to larger arrays in which the rectangle approach cannot be used. Please see attached illustration of the approach we recommend for 0.5mm pitch arrays, using x=y=0.2mm offset, 0.1mm microVias on 0.2mm microVia pads. By offsetting radially away from the center of the device, routing channels on layer 2 are much wider. This may be useful for this project as well as for future projects with larger devices.

    Any further questions, please let us know.

    Best regards,  Ernesto.

    P.S.- I'm impressed, 0.001" soldermask registration tolerance is not common unless you are using LDI process.

    microVia Radial Offset.pdf

  • Thanks Ernesto. And yes, we'd be using LDI with a 1 mil registration. I think we can close this one out now. We appreciate your support. Bob K. Harris Corp.