Proper pad-to-via clearance can improve solder joint strength.
Design for assembly consists of more than simply placing components at a safe distance apart. Today’s small pitch components push the limits of fabrication tolerances.
Vias are a major factor in testability and DfA. Vias too close to a pin do not permit solder mask webbing. The absence of the webbing will starve solder from the pin. Paste will travel through the via and short components on the opposite board.
Vias should be exposed for testability. Adequate clearance from pins permits test probes to reach the via and permits a solder mask web. Following is a guide for which via type to use based on different needs and methods.
Via-in-pad. From a design perspective, this comes into play on very tight designs where we are not able to fan out as usual. BGAs with a pitch of 0.65mm and below basically require this, as do some other fine-pitch devices. Other components such as QFNs have thermal pads that require via-in-pad. The difference between a via-in-pad on a thermal pad, as opposed to a BGA, is that the vias in the thermal pad may not need to be filled and polished flat, provided they are a small enough drill size. BGAs or other fine-pitch devices will need to have their vias filled and polished flat, making them suitable for soldering.
Cover my vias, or don’t. There are two reasons to cover vias, and both have to do with the tightness of the design. If there is insufficient pad-to-via clearance, it will be difficult to achieve solder mask webbing between the pad and via. This can cause solder to wick down the barrel of the via, making the connection weaker than it should be. The other reason is attributed to silkscreen; tenting the vias will permit more room for any required silk. Tenting vias lowers the overall testability of the design because fewer vias can be accessed.
Fill material. There are two approaches to filling vias: nonconductive epoxy or plating them closed. Nonconductive epoxy is not recommended for designs that will have multiple thermal cycles because via plugs can expand at different rates, possibly causing board material to pop out of the via.
Plating vias shut with copper during plating has its own set of challenges. Pockets of air can get trapped in the barrel and not let the copper fill the entire via barrel. For either option, consult with the board shop for the best approach for a given design.
Blind/buried vias. Blind vias are holes that extend to only one surface of the board, while buried vias do not extend to either side of the board. Both via types are used in tight areas, such as fine-pitch BGAs.
When choosing a blind/buried via structure, keep in mind how many lamination cycles will be needed. Keeping the lamination cycles to a minimum is important to keep down costs. Take, for example, an eight-layer design where both sides of the board are covered with surface mount components and a through via will not work. There could be a via extending from layer 1 to 2, one extending from layer 1 to 3, one extending from layer 3 to 6, one extending from 6 to 8, and another extending from 7 to 8. This would permit fan out of both sides to layers 3 and 6, respectively. From there, find a spot for the blind via (the 3 to 6) to get through the board to the other side. A stackup like that would require three lamination cycles. Removing the blind vias connecting layers 1 to 2 and 7 to 8, however, would reduce this to two lamination cycles.
This is a simple example, and most board shops have their own methods for blind and buried via structures. Work with the shop to find the method that they prefer, if possible, because this will help keep down costs on these types of high-technology designs.
Vias are important in the DfA process. Knowing which types and methods to use can be the difference between the success of a tight design or not. Close communication with the board shop is key to determining the best, most efficient approach for specific designs, and for keeping costs as low as possible on high-technology designs.
W. Scott Fillebrown is president and CEO of ACD (acdusa.com); This email address is being protected from spambots. You need JavaScript enabled to view it.. His column runs bimonthly.
