PCB Via Structures: Through, Blind, Buried and Microvia

A Hole Is Not Just a Hole

Almost every net on a multi layer board changes layers at least once, and every one of those transitions is a hole. The shape of that hole decides how much routing space it consumes, how much it disturbs a high speed signal, how many process steps the board needs and what the panel costs to drill. Getting the structure right at the design stage is far cheaper than discovering at the shop that the requested aspect ratio cannot be plated.

This guide walks through the standard structures from a plain through hole to a laser drilled microvia, with the numbers that appear on fabrication drawings.

Two Jobs: Connection and Mounting

Holes are either plated or not, and the distinction is important because it changes both the artwork and the process.

A plated through hole, or PTH, has copper on the barrel after drilling and plating. It carries current between layers. Typical barrel copper is 20 to 25 micron. A non plated through hole, or NPTH, is drilled but never plated. It exists for a screw, a standoff, a locating pin or a connector body. Mixing them up is one of the classic first article findings: a mounting hole that was drawn as a pad on the copper layer will come back plated, with a smaller clearance than the screw needs, and the panel will short to the chassis.

Mechanical holes also do thermal work. A field of small vias under a power device, often called thermal vias, moves heat from the component pad into inner copper planes. That is a copper and layout decision more than a drilling one, and it belongs with the rest of the thermal management strategy rather than being added late.

Through, Blind and Buried

• Through hole via. Drilled from the top of the stack to the bottom. Simple, strong and cheap. It blocks routing on every layer it passes through, which is why a dense board runs out of space long before it runs out of layers.
• Blind via. Connects an outer layer to one or more inner layers but does not pass through the board. Requires sequential lamination or controlled depth drilling, so it costs more and increases lead time.
• Buried via. Connects inner layers only and is invisible from outside. It frees the outer layers completely but needs a separate lamination cycle for each set.
• Microvia. A laser drilled hole of 50 to 150 micron that connects an outer layer to the next layer down. This is the building block of HDI PCB construction, and it is what makes fine pitch BGA escape routing possible.

The trade is always the same: the more of the stack a hole passes through, the cheaper it is to make and the more routing space it costs. Designers move to blind, buried and microvia structures only when the layer count or the escape routing demands it.

Hole Sizes That Match the Job

• 0.10 to 0.30 mm: microvia range, laser drilled, one layer deep per step.
• 0.30 to 0.50 mm: signal vias in standard multilayer construction.
• 0.60 to 1.00 mm: through hole component leads, connectors and transformers.
• Above 1.00 mm: mounting holes, standoffs and hardware clearance.

Two secondary dimensions matter as much as the drill size. The annular ring is the copper pad width around the hole, and the usual minimum is 0.10 to 0.15 mm; below that a small registration error breaks the connection. Drill tolerance is typically plus or minus 0.05 to 0.075 mm, and a hole that is drawn too close to the minimum may end up too tight for the component lead or too loose for a reliable solder joint.

Panel thickness relative to drill size gives the aspect ratio, and that number decides whether plating is feasible. Most shops plate comfortably to 8:1 and will attempt 10:1 with care. A 0.3 mm hole in a 3 mm board is 10:1. Push further and the copper thins toward the middle of the barrel, which is exactly the failure mode a microsection is looking for.

How the Holes Are Made

Mechanical drilling with a CNC router handles everything from 0.15 mm upward. The drill bit is a consumable, the entry and exit materials control burring, and the panel is stacked under controlled pressure so the bit does not wander. Bit wear is the main cause of rough barrel walls, and rough walls plate unevenly.

Laser drilling handles the microvia range, because a mechanical bit that small would break under the load. The laser removes dielectric down to the target copper pad, which is why microvias are formed as a controlled depth hole with a copper bottom rather than a through hole. A stack of microvias, one per layer, is how an HDI board climbs through the stack without drilling through it.

After drilling comes plating, and the sequence is fixed: clean the hole, deposit a thin electroless copper seed over the resin and glass, electroplate copper to the specified barrel thickness with a bath chemistry that throws metal into the middle of the hole, then apply the surface finish. Everything after that, including the soldermask and the silkscreen, sits on top of that finished barrel. The plating details and how they are verified are covered under PCB manufacturing.

Design Rules Worth Following

• Keep enough annular ring. 0.10 to 0.15 mm is the floor. More is better on anything that will see thermal cycling.
• Watch the aspect ratio. Stay at or below 8:1 for routine work, and discuss anything above 10:1 with the fabricator before release.
• Space the holes. Too small a gap between walls lets the drill break into the neighbouring hole, and it leaves no room for the return current path.
• Use via in pad with care. It saves routing space under a BGA, but the via must be filled and capped, and the fill must be flat enough for the paste deposit. This is a process requirement, not just a layout one.
• Treat high speed transitions as electrical, not mechanical. A long stub reflects energy, and every layer change without a nearby return via adds inductance.
• Count the holes. Drill cost scales with the number of hits, and a design with thousands of unnecessary vias pays for them on every unit.

Common Drilling Defects

Four problems account for most hole related scrap. Drill wander moves the hole off centre, which eats the annular ring on one side. A rough barrel wall from a worn bit or the wrong feed rate plates unevenly and can trap voids. Plating voids leave a gap in the copper that fails electrically after thermal cycling rather than immediately. Layer to layer misregistration shifts the pad relative to the hole, and it is caught mostly by the coupon rather than by the finished board.

All four are process control problems rather than design problems, which is why the incoming inspection step matters: the first article coupon and the microsection report are the evidence that the drilling and plating steps stayed in control. That check belongs in the standard PCBA testing flow for any program where field reliability matters.

What Drilling Costs

Drilling is one of the larger items in the fabrication price, and it scales with the number and size of the hits.

• Standard mechanical drill: roughly 0.0008 to 0.003 US dollars per hole.
• Small via drill: 0.002 to 0.006 per hole, because the bits are fragile and the feeds are slower.
• Laser microvia: 0.01 to 0.05 per hole, reflecting the equipment and the lamination steps around it.

On an HDI board the drilling and microvia steps can account for 15 to 30 percent of the total manufacturing cost. The practical consequence is that removing a few hundred unnecessary vias, or consolidating a stack of layer changes, is worth real money at volume. It also shortens the drill program, which helps lead time.

FAQ

What is the smallest via a fabricator can make? Around 0.10 to 0.15 mm in HDI construction, using laser drilling for the smallest sizes.

Do all holes need plating? No. PTH holes carry signals and current; NPTH holes exist for mounting and alignment and are deliberately not plated.

What is a reasonable aspect ratio? 8:1 is routine, 10:1 is achievable with care, and anything higher needs an explicit conversation.

How many vias can a board have? From a few hundred on a simple control board to tens of thousands on a dense HDI design. The count drives drill cost directly.

Summary

Via structure is a routing decision with a manufacturing price attached. Through holes are cheap and strong but block layers, blind and buried vias buy routing space at the cost of extra lamination, and microvias make fine pitch HDI possible. Keep the annular ring above 0.10 mm, keep the aspect ratio at or below 8:1 unless there is a reason not to, fill and cap any via that sits in a pad, and give every high speed transition a return path. Confirming the drill and plating results on a coupon through PCB design and layout review and incoming inspection closes the loop.