PCB Via Hole Guide: Types, Sizes and Aspect Ratio

A via hole is the smallest feature that decides whether a board can be built at all. Diameter, depth, pad size and plating thickness are linked, and pushing one of them past the process window turns a routine multilayer board into a yield problem. This guide covers the four via types, the numbers that matter in each, and the design rules that keep them manufacturable.

The Four Via Types

A through-hole via passes through every layer of the board. Diameters typically run from 0.2 mm to 0.6 mm, and the hole is drilled after lamination and plated in one operation, which makes it the cheapest option per connection.

A blind via starts on an outer layer and ends on an inner layer, so it is drilled before the final press. Blind vias usually measure 0.15 to 0.2 mm and add a lamination cycle. A buried via connects inner layers only and never reaches the surface, which frees routing space on the outer layers at the cost of an extra press cycle. A microvia is laser drilled with a diameter of 0.075 to 0.15 mm and a depth of roughly one dielectric layer, and it is the tool that makes high density interconnect possible.

Diameter and Drill Selection

The drill diameter should be the smallest size the fabricator can plate reliably at the finished board thickness, not the smallest number in a catalogue. Standard through holes sit between 0.2 and 0.4 mm; blind vias between 0.15 and 0.2 mm; microvias between 0.075 and 0.15 mm.

Component leads and connector pins set the lower limit, so each hole must clear the pin with room for the plating. Once the hole size is fixed, every other dimension follows from it.

Aspect Ratio Limits

Aspect ratio is the board thickness divided by the hole diameter. Standard production handles 8:1 to 10:1, advanced lines reach 12:1, and anything beyond that needs a special plating process and a slower, more expensive drill cycle.

The reason is fluid exchange. Plating solution has to circulate through the barrel to deposit copper evenly, and a deep, narrow hole does not allow it. The result is a thin or voided barrel that passes electrical test and fails later during thermal cycling. Microvias run at about 1:1, which is why they are laser drilled and plated in a dedicated line rather than on the mechanical drill.

Pad Size and Annular Ring

The finished pad diameter is normally calculated as the via hole diameter plus 0.4 mm. A 0.3 mm hole therefore takes a 0.7 mm pad. That allowance covers drill registration, plating build-up and the annular ring that must remain after etching.

Keep at least 0.05 mm of annular ring around the finished hole, and prefer 0.1 mm on boards where registration is uncertain. A pad that barely surrounds the hole will break out on one side after a small drill offset, and a broken ring is an open circuit waiting to happen. Where space is tight, reducing the via diameter is usually better than shaving the ring.

Plating Thickness and Barrel Quality

Copper in the barrel is typically 20 to 25 µm on the walls. Thinner deposits reduce current capacity and increase the risk of barrel cracking during thermal cycling, while much thicker deposits take longer to plate and can close small holes.

Back-drilling, where the unused portion of a through-hole stub is removed, improves signal integrity on thick backplanes but adds a process step. On high speed designs, the stub length matters more than the plating thickness, and the two should be evaluated together.

Current Carrying Capacity

A via carries current through a much smaller cross section than the trace that feeds it. A single 0.3 mm via with 25 µm of copper has far less copper area than a 1 mm wide trace, so power nets need several vias in parallel or a larger drill.

The calculation follows the same rules as a trace, described in the guidance on trace width and current calculation. As a rule of thumb, use at least two vias for any net above an ampere, and more where the ambient temperature is high.

Via in Pad and Tented Vias

Placing a via inside a component pad saves routing space but requires the hole to be filled and capped so that paste does not wick into the barrel during reflow. Unfilled via-in-pad is one of the most common causes of voiding under a ball grid array. The trade-offs are set out in the comparison of via in pad and plated through construction.

Tented vias, covered by solder mask, are fine for slow nets and protect the barrel from contamination. They should not be tented on pads or on test points, and a tented via cannot be used as a probe target.

Choosing the Right Structure

Start with through vias and keep them wherever routing allows, because they cost the least and carry the fewest process risks. Move to blind and buried vias only when the layer count or the routing density demands it, and use microvias where the package pitch leaves no other escape. The comparison of blind and buried via stack selection sets out how each structure affects the press schedule and the price.

Every decision should be recorded in the drill schedule, with hole size, plating class, tolerance and via type listed for each entry. Fabricators work from that table, and an ambiguous drill chart is the fastest route to a rebuild.

Placement, Stitching and Thermal Relief

Via placement matters as much as via size. A stitching via that ties two ground planes together should sit close to the edge of the plane and repeat every few millimetres along its length, because plane resonance is driven by the distance between bonds. Ground stitching around a connector field also shortens the return path for signals entering the board.

Vias that connect a pad to an internal plane are usually given thermal relief spokes so the pad does not act as a heat sink during soldering. On a power net the opposite is wanted: a direct connection with several vias gives the lowest impedance and the best heat transfer.

Keep vias out of the solder mask dam around fine pitch pads, and keep them clear of the component courtyard unless they are filled and capped. A via that sits slightly under a package body cannot be inspected or reworked, so placing it a fraction of a millimetre away is worth the small routing cost.

FAQ

What is the smallest practical via hole? Mechanical drilling holds about 0.2 mm in volume production, and laser drilled microvias reach 0.075 mm. Going below those values is possible but the cost rises sharply and the panel becomes harder to plate.

How much annular ring does a via need? Keep at least 0.05 mm after plating and etching, and use 0.1 mm where drill registration is less certain. The pad is normally sized as hole diameter plus 0.4 mm to leave that margin.

Do vias need to be filled? Only when they sit inside a solder pad or under a ball grid array. Vias placed on a trace can stay open, or be tented with solder mask, which is cheaper and perfectly reliable.