Vias formed with mechanical drills are described as through-hole, blind, and buried based on the layers that they start and stop on. Through-hole vias go through all layers of a board, blind vias start on an outer layer and stop on an inner layer, and buried vias start and stop on interior layers. All of these vias are formed in the exact same way. All that changes is whether or not additional layers of copper are later laminated to the board after through-hole via formation.
Microvias are used in very-high density board design. These vias are cut with lasers that usually penetrate a single layer at a time. Then copper is deposited into the via hole through electroplating. To gain greater depth for microvias, additional layers of copper foil and dielectric are added to the outer-layer of a board. Microvias can be stacked to almost any depth, but staggered microvias are generally considered more reliable than stacked microvias, but a good fabricator can make stacked microvias that are as reliable as staggered microvias.
Mechanical vias are made with twist drills, and the minimum drill diameter is 5.9 mils. Drills smaller than 5.9 mils are not practical in a production setting due to their short wear life, high rotational speed requirements, and tendency to break and wander off target.
The basic process involves taking either a 2-layer core or a laminated multi-layer stack and carefully drilling holes where the vias will eventually be formed. Next, a layer of photo-imageable mask is laminated to the outer layers of the circuit board — this prevents electrodeposition on parts of the copper that will be later chemically etched away. The mask is exposed to the negative image of the circuit board traces and copper pours. The parts of the mask that were not exposed to light, and are therefore not polymerized are washed away, exposing bare copper and via holes.
Next, the entire board is placed in a tank and hooked up to the cathode of a power supply. Copper ingots that are also in the tank are connected to an anode. Copper ions leave the ingots and deposit themselves on the surface of the board and in the via holes, thickening the board, and forming the vias. After the copper has been deposited to the proper thickness, the mask is washed away and the board is submerged in a tank of ferric-chloride — which etches away the parts of the board that were not electroplated.
The minimum via diameter is determined by a fabrication shop aspect ratio and the minimum drill diameter. The industry standard limitation is currently around 10:1. That means your minimum via drill diameters are:
|0.8 mm (32 mil)
||0.15 mm (5.9 mil)
|1.6 mm (63 mil)
||0.16 mm (6.3 mil)
|2.4 mm (95 mil)
||0.24 mm (9.5 mil)
Your fab shop might have their own rules — but at Royal Circuits, one of our fabrication partners – small vias are drilled oversize and plated to finished size. If you can allow some amount of variation in barrel-wall thickness, your project will have a higher yield and therefore cost less.
Vias are drilled into copper pads. And those pads are not always perfectly aligned. So a minimum pad diameter is required to prevent breakout. The manufacturing minimum is to add at least a 0.13 mm (5 mils) annular ring surrounding your drilled hole. That is a pad diameter = drill diameter + a minimum of 0.25 mm (10 mils). For our project, we will add an 8 mil annular ring. This will provide the greatest chance of inexpensive manufacture across a variety of board houses.
The amount of air-space that surrounds a pad and the nearest copper depends on the copper weight. So use your manufacturer’s trace and space guidelines, along with your copper weight to determine that.
If a problem is solvable, an engineer will find a solution, and that engineer can be you. Yes, there are geniuses out there, but they are few and far between. The rest of us mere mortals get to where we want to be through hard work and perhaps a little luck. So push yourself to learn something new this week. Ask questions.
For 0.5 oz copper, the minimum manufactuing space that separates two bits of copper is 0.1 mm (4 mils and 3.5 mils if we push it). Anti-pad diameter = pad diameter + 0.2 mm (8 mils) For our project we will increase that to 8 mils of clearance or 16 mils additional diameter. This large margin increases the chance that we can inexpensively manufacture our board almost anywhere.
Microvias are formed by using a UV laser to drill a hole through one layer of copper and partway into the layer below. The hole is cleaned and treated with an electroless copper solution that plates a ~10 micron thick layer of copper in the hole. That makes the entire board conductive and ready for an electroplating bath. Copper is then deposited into the via cavity and fills the hole.
Microvias can be made down to 1 mil diameter. But the limiting factor is the aspect ratio. Microvias never exceed the ratio of 1:1 diameter to depth. Look at your layer stack and determine the distance between layers.
In the example above, and focusing on layer-thickness only, microvias between layers 3 and 4 could be smaller than microvias between layers 1 and 2. But that’s an awful lot to keep track of, and bigger is better, so use the thickest layer for your 1:1 aspect ratio determination.
Laser microvia drills use computer vision systems to align the drill in the center of the pad — which means the pad can be a bit smaller than a mechanically drilled via. Lasers are perfectly aligned and never wander. The minimum annular ring is 2 mils. Minimum pad diameter = drill diameter + 4 mils.
The minimum antipad diameters are determined by the copper thickness, just like a mechanical via. Determine the anti-pad annulus width from the trace and space charts for your manufacturer.