Solder flow thru via on pad

Been there - done that. Makes a mess on that 2nd reflow process- doesn't it!?!?!?

This is caused by design. If the open via is located in the land area, it will flow thru the via and cause pumps on the opposite side. You can have your vias filled with mask and save yourself some time bumping heads with your design guys. Unless your ICT guy is using this via for test, then you'll have to have a strip of masking placed between your solder paste and the via - if possible.

reply »

Oooo, the solder on the pad and PGA ball is flowing during reflow down the via to the secondary side? Why didn�t you say so?? ;-)

Why would you expect that gravity and capillary action wouldn�t force solder to flow down the solder plated via to the secondary side when the solder is heated to reflow temperatures? Beyond those pesky bumps, there is a more pressing problem. Even though you�re probably partially filling the via with paste during print, the solder that is flowing-out the bottom of your board is probably starving your solder connections, which is possibly reducing the reliability of your product.

Here�s what a production type can do: * Secondary side solder bumps: Learn to love �em. If you really hate them, you could use a temporary solder mask to block the solder from flowing all the way through the via. While cheaper than rework, it�s not something that most would want to start. * Starved solder connections: Increase the amount of paste printed to accommodate the loss of material used to fill the via and make the bumps on the other side. [Ummm, this sounds dicey. Enlarging the stencil aperture could cause bridging between PGA balls. Increasing the stencil thickness � naw can�t do that!!! Maybe just slowing down the print head speed will do it. In real life, all of this is fairly futile and almost always increases reflow oven maintenance to scrape solder splats from the bottom side heaters.]

Here�s what a design type can do: * DON�T DO VIA IN PAD!!!! [We�ve talked about how much we like via in pad previously in the fine SMTnet Archives. ;-(] Many of the design tricks for accommodating VIP don�t work with BGA pads. ;-( * Increase the BGA pad size with a small bubble on one side of the pad you�re using now, put the via in the increased area of the bubble, and specify solder mask over the increased area. Duhh!!! * Specify a plugged and plated-over via. * Specify solder mask cover over the bottom side of the via. [This can be risky, if you�re using a uV cured solder mask, because the mask in the via may not cure properly.] * Specify a minimum via that is not too expensive, but will close during plating. [A guess at what has worked in the past is: 0.013- thou. Don�t bet on that, I can�t remember where to find this and your fab can help more.] [This can be a little risky, because plating is the thickest where the hole meets the board. So, there is some potential of sealing process chemicals in the via, if you let the fab close the via.] * Convert the via to a blind or microvia.

reply »