Issue link: https://iconnect007.uberflip.com/i/1040234
44 DESIGN007 MAGAZINE I OCTOBER 2018 did not add to the cost of manufacturing. The solution translates well to similar IC packages. We were back up and running again, but what was the problem in the first place? Problem: Uncontrollable, Unpredictable Solder At first, we used the standard, manufacturer- recommended method for heat sinking. We placed large copper pads on both sides of the board under the chip, connected them with vias to conduct heat, and applied full solder paste coverage for the best thermal contact. As straightforward and intuitive as the standard approach is, it obviously has some problems. In this case, the culprit is solder's unpredict- able behavior once melted, which puts every board at risk of a poor heat sink connection. We've all seen the result of bad solder connec- tions: Failures in quality assurance or worse— shortened life and failure in the field. The problem is so pervasive you might be tempted to accept it as the unavoidable cost of doing business. But if we look at the causes of the chaos, we can find ways to offset them. There are two main mechanisms that cause these failures: Solder wicking through vias and sol- der movement under large pads. Failure 1: Solder Wicking Through Vias This failure mode is the most obvious. If the landing pad is covered in tiny holes, molten solder can run through them to the back of the board. This leads to less solder connecting the pad and the solder that is in place distrib- utes unevenly. Even worse, the wicking will vary from board to board. Common vias are not precision components, and the amount of copper plated onto them varies. Some may be wider than intended, and others plated par- tially or fully shut. Identically designed boards that went through the same manufacturing process may now have significantly different thermal responses. Failure 2: Solder Movement Under Large Pads Again, we have to consider the unpredict- ability of solder movement during reflow. If there is not enough solder under the slug or the board is warped, capillary action can pull the solder to one side of the chip. Attempt to cor- rect this by applying more solder, and the chip might float right off the signal pins. Excess sol- der can overflow the pad and send solder balls out to short or bridge other areas of the board. The varying amount of solder pulled through the vias only exacerbates the problem and hin- ders attempts to correct for it by adjusting the amount of paste used. Solution Fortunately, the solution is as straightfor- ward as the problems themselves. We simply must prevent the solder from wicking through the vias or moving past its area of application. There are two elements to this solution. First, apply solder mask over the landing pad and open circular "islands" for paste applica- tion. If the solder won't behave over a large area, we can break that area up into an array of smaller, better-behaved areas because sol- der mask restricts the paste to its area of appli- cation. While this reduces the amount of sol- der connecting the chip to the board, it also increases the consistency. The circular solder paste apertures release the solder more reliably than those with sharp corners, which helps prevent loose solder balls. Second, surround the "islands" with small (~12 mils or smaller) tented vias (covered with solder mask). Removing the vias from the immediate area being soldered and tenting them prevents any stray solder from wicking down to the other side of the board while still providing good thermal transfer to the pads underneath. You should add these vias as close as possible (nearly tangentially) to the islands. The solder mask tenting will block any solder that wicks onto an exposed via due to manu- facturing tolerances. Keep in mind these few key rules when implementing: • Make sure the pad under the chip is a solid copper plane to spread out the heat • Use a hexagonal packing pattern for the solder islands to give the heat slug maximum coverage