When you design a multilayer board, you almost always need to route traces from one side of the board to the other. This is done through a via, which is a hole drilled through matching copper pads on the top and bottom of your board that gets plated with a conductive material. The ring of copper left surrounding the via on both the top and bottom of the board is called the annular ring. See, definitely a donut:
In a perfect world, the drill bit would hit the right mark flawlessly every time and there would be no need for an annular ring bigger than a mil or two. However, the drills used by PCB manufacturers are subject to the same variables as the rest of the world and are only guaranteed to strike within a certain tolerance. The tolerance is remarkably tight considering the process, typically about 0.005” (5 mil), but must be taken into account if your design cannot tolerate tangency (the drill is against one edge of the pad) or breakout (the drill completely breaks the boundary of the pad).
The exception would be connecting copper planes. If you are using a multitude of vias to connect two large pours of copper, the annular rings are just a formality.
Determining via annular ring size
If you cannot tolerate tangency or breakout, how much copper do you need in your annular rings? When space is tight, the last thing you want are giant PCB annular rings hogging room. If you have to put your board on a diet, check with your PCB manufacturer for their recommendations. They may be able to slim down their tolerance for a fee. If you want to accept their standard tolerances but not risk a poor connection, a good rule of thumb is to make the annular rings the width of your manufacturer’s tolerance plus one mil. For example, if they can only guarantee 5 mil accuracy on drill hits, make sure your annular rings are a minimum of 6 mil. There is no fancy math here, just the difference between the diameter of the pad and the diameter of the drill divided by two. If you have a 10 mil drill through the center of a 20 mil diameter pad, your annular ring width is (20-10)/2 = 5 mil. If the tolerance you expect is 5 mil, you put yourself at risk for tangency. It would be better to make the pad at least 22 mil in diameter.
The surface area of annular rings
What if you are on the opposite end of the spectrum? You have room to spare and current to move. Vias can only be plated to a certain thickness, so you may need a larger via to get the surface area required for high-current traces. To actually use all that surface area, current must be able to flow all the way around the annular ring and therefore through the entire via. To ensure you do not create a thermal hot spot if the drill does not hit the center, add 1/8 of the connecting trace width to the manufacturer’s tolerance. If you are approaching a via with a 40 mil trace, add 5 mil to the tolerance of 5 mil to get a total annular ring width of 10 mil. If you do not have room for large rings on your PCB, consider using multiple smaller vias to connect the traces.
If you are creating vias to use as mounting holes for through-hole components like a header or through-hole LED, keep in mind that it is difficult to properly hand-solder to an annular ring of less than 10 Mil. Go ahead, use the giant, deep-fried PCB donut (PCB annular ring).
PCB annual ring soldering
As a board designer, we take pride in efficiency. An organized board is a more compact board, which is a cheaper board. It can be tempting to eye the large amounts of exposed copper the donuts of the PCB provide and get ideas. As tempting as it is, do not try to anchor sprinkles of components like tiny resistors to the board using the annular rings. The solder paste flows differently on a ring than it does on a standard pad and will not form a good connection on small components. Larger elements are a different story – the annular rings of thermal vias under a component with a thermal slug do an excellent job of anchoring that part to the board.
Sprinkles are not recommended, but there is nothing wrong with giving your annular rings in a PCB a solder paste glaze. The paste will melt into the vias during reflow and increase conductivity. This is not a good idea for vias that you intend to use to hold components since the reflowed solder will decrease the hole diameter and the component leads might not fit.
There is a lot to keep track of in PCB design, and details like annular ring width can fall through the cracks. Check the settings of your default DRC tool and make sure your PCB annular rings match your design lifestyle.
