Stats

  • Replies 5
  • Subscribers 160
  • Views 4876
  • Members are here 0
More Content

How Should I Implement Vias in Pad?

John T

Having reviewed many PCBs for Manufacturability/Assembly, I wanted to highlight two mistakes that I keep seeing in designs regarding thermal vias in diepads. If you are familiar with this area, please feel free to add to the conversation, or to contradict, based on your experience. All thoughts, opinions, and questions are welcome.

 

For clarity, I am referring to vias placed within smd pads in order to improve the thermal performance of certain components.

There is plenty of information online explaining why these are used, but I don’t find much information explaining how to implement this.

 

Mistake 1 is regarding component placement. Normally, these via pads are completely exposed by the soldermask layers. The via pads themselves are not visibly distinguishable from the copper surface; only the array of holes are visible in the diepad. Therefore, the solder paste can flow freely down the holes during reflow.

This is not an issue as long as you have designed your PCB with DFM in mind. And we are talking about automated production, assuming no hand-soldering or rework is planned. To get all of your components to solder correctly the first time in an automated process, you should ensure that such surface components are placed on “reflow side 2” of the board. This ensures that any paste protruding through the via holes does not cause obstruction to the stencil on the second reflow side.

The reason is Gasketing: This is the seal that a stencil has with the surface when placed on the PCB. The thickness of the stencil normally dictates the volume of paste deposited for a given aperture. “Poor gasketing” is caused by protruding solder bumps, which elevate the stencil and place additional unwanted paste. As per the QFN image above, this can have detrimental effects on the small components placed on the opposite side. An unpredictable amount of paste will be deposited due to the elevation of the stencil, leading to a number of possible soldering defects such as shorts or tombstoning.

 

Mistake 2: Suppose you already have fully open vias, with soldermask openings that result in full exposure of the via pads on both the top &  bottom side. Opening these vias individually is not advised. Designers should instead create a larger exposed metal shape on the opposite side of the board. This in known as a wetting area.

 

 

This helps lower the profile of through-solder and reduce any potential effects that may occur because of too much solder accumulation down one hole. Solder accumulation patterns are random, as the solder flux boils and bubbles its way off the pad. It is best that an exposed copper surface is provided on the opposite side as a large wetting area. This will enable any solder flowing through to flow freer and flatter on the opposite side. This solder-management technique is best for the overall quality and reduction of solder balls.

 

So, which side is the first reflow side of your board? Do you know, and how do you decide?

There may be a lot more to discuss here, but for now, please consider the points presented above. Any further comments or opinions are welcome.  

Parents

  • In my experience, problem 1 & 2 are easily solved by sizing the drills of the via in the thermal pad accordingly. We typically use a 0.25 mm diameter finished hole size which serves the purpose of connecting the vias to an internal layer for thermal purposes, but is too small to allow paste to readily flow through the hole and created solder bumps on the secondary side. We've yet to see ANY protrusion of solder on the opposite side of a QFN or any other SMT part when doing it this way. We then add enough vias in the pad to achieve the thermal connectivity we need (typically quite a few. If the drill size is to large the problems detailed above most definitely happen.

    As for which side is the first reflow side of the board, it's typically the side with the decoupling caps and small mass parts that sit opposite the large or greater mass parts. Reflow profile by the CM controls those parts staying on the board when doing the secondary reflow of the larger mass parts.

  • in reply to Byron365

    Great insight thanks Byron! I think your experience with via size should be very useful; all users should take note!

    I would query if the paste type could impact this process stability.  A finer ball size may encourage solder protrusion, what do you think? 

    In past projects we were encouraged to stick with a single via hole size, or at least minimal variation. This was to achieve lowest possible board cost. Larger vias can enable Fabricators to drill multiple boards at once. But to me, it sounds like your suggestion is money well spent.

Reply
  • in reply to Byron365

    Great insight thanks Byron! I think your experience with via size should be very useful; all users should take note!

    I would query if the paste type could impact this process stability.  A finer ball size may encourage solder protrusion, what do you think? 

    In past projects we were encouraged to stick with a single via hole size, or at least minimal variation. This was to achieve lowest possible board cost. Larger vias can enable Fabricators to drill multiple boards at once. But to me, it sounds like your suggestion is money well spent.

Children
No Data
Cadence Guidelines

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.