A via in a PCB is a small plated hole that connects copper on one layer to copper on another. A circuit board via is sometimes just called a via hole. The hole is drilled, its wall is coated with copper, and the resulting barrel carries a signal, power, or ground from one layer to the next. Vias are what make a multilayer circuit board possible: without them, every trace would have to stay on the layer where it started.
Most boards only need plain through-hole vias. Blind, buried, micro, and via-in-pad structures exist to solve specific density problems, and each one adds drilling, lamination, or plating steps that you pay for. The useful question is not "which via is best" but "what is the cheapest via structure that still lets this layout route?"
This guide explains what vias are, the main types of vias, how via size and aspect ratio limit your choices, and how to call vias out so the fabricator quotes the board you designed.
Key takeaways
- A PCB via is a plated hole that joins copper on two or more layers. A component hole holds a lead; a via only carries current between layers.
- Through vias are the default and the cheapest. Blind, buried, and microvias trade cost for routing space.
- Aspect ratio helps flag deep, narrow holes for fabrication review; the ratio alone does not establish plating quality or reliability.
- Every additional lamination cycle, laser step, or fill-and-cap operation shows up in price and lead time. Count them before you commit to a structure.
- Put vias on the fabrication drawing as a drill table by layer pair, with fill, cap, and protection requirements stated, rather than leaving them to CAM interpretation.
What is a via in a PCB?
The word comes from the Latin for "path", and some engineers expand it as vertical interconnect access. On a circuit board, a via has three parts:
| Part | What it is | Why it matters |
|---|---|---|
| Barrel | The plated copper wall inside the drilled hole | Carries the current; its plating thickness and integrity decide reliability |
| Pad (land) | The copper ring around the hole on each connected layer | Gives the drill a target and the barrel a place to join the trace |
| Antipad (clearance) | The copper-free gap around the barrel on planes it must not touch | Prevents shorts to planes it passes through and affects impedance |
The ring of copper left between the hole edge and the pad edge is the annular ring. If the drill lands off-center, the ring thins out on one side, which is why drill registration matters as much as hole size.
Vias versus through-holes for components
Both are plated holes, and on a drill file they look alike. The difference is what goes in them. A component hole is sized for a lead or press-fit pin, so its finished diameter and tolerance are set by the part. A via carries no lead, so it can be much smaller, and its job is purely electrical or thermal. Some boards also use non-plated holes for mounting, which are neither.
Which via type does your BGA need: through, blind, micro, or via-in-pad?
There are four basic via types, plus a few variants built from them. The table summarizes how APT's drilling page describes each structure and how it is produced.
| Via type | What it connects | How it is made | Typical reason to use it |
|---|---|---|---|
| Through via (PTH) | Top layer to bottom layer, passing every layer | Mechanical CNC drilling after the final lamination | Standard signal and power routing |
| Blind via | An outer layer to one or more inner layers, not through the board | Mechanical controlled-depth or laser drilling | Fan-out from dense parts, recovering routing space on other layers |
| Buried via | Inner layers only; invisible from the outside | Mechanical drilling on an inner sub-lamination | Crossing dense inner routing channels |
| Microvia | One build-up layer to the next | Laser ablation on a thin dielectric | HDI structures and fine-pitch BGA escape |
| Stacked microvia | Several microvias directly on top of one another | Laser ablation with each lower via filled and plated flat | The densest routing, very fine BGA pitch |
| Staggered microvia | Microvias offset from layer to layer | Laser ablation | Density with less stacking, often preferred for thermal cycling |
| Via-in-pad (VIPPO) | A via placed inside an SMD pad, filled and plated over | Drilling plus fill, planarization, and cap plating | Fine-pitch BGA breakout without dog-bone traces |
| Backdrilled via | A through via with the unused copper stub drilled away | Controlled-depth counter-drilling | Reducing stub reflections on fast serial links |
| Thermal via array | A grid of plated holes under a thermal pad | Mechanical drilling | Moving heat from a power device into planes |
Through vias, blind vias, and buried vias are the core vocabulary. Microvias and via-in-pad are where HDI begins. For how blind and buried spans are planned layer by layer, see the blind and buried via planning guide.
Through vias
A through via is drilled after all layers are laminated, so it costs one drilling and one plating pass. It passes every layer, which means it also blocks routing on every layer, even the ones it does not need to connect. On a board with two or three dense packages, that blocking is usually what pushes a design toward blind or buried vias.
Blind and buried vias
A blind via starts on an outer layer and stops inside the board. A buried via starts and stops inside. Buried vias are drilled and plated on an inner core or sub-stack before it is laminated with the rest of the board, so each buried span normally adds a lamination cycle. Blind vias can be made by controlled-depth mechanical drilling or by laser, depending on depth and diameter.
Microvias
A microvia is a small via, commonly laser-formed, that connects adjacent layers in a build-up structure. Its geometry and feasibility depend on the construction and manufacturing process. Microvias are the building blocks of HDI notation such as 1+N+1 (one build-up layer on each side of a core) and 2+N+2 (two build-up layers per side). See the microvia guide for a closer look at their construction and review.
Via drill and aspect ratio: what limits the smallest via you can actually order?
For a mechanically drilled through-hole, aspect ratio compares board thickness with hole diameter. A deeper, narrower hole can be more difficult to drill, prepare and plate. The ratio is a screening tool, not proof that a hole will meet its copper requirements or withstand the product's thermal history.
For hole-wall preparation after drilling, see PCB desmear and inspection.
Check which dimensions are used before comparing a calculation with a fabricator's capability. A drawing can specify a finished hole, while a manufacturing assessment may use a production drill diameter and the thickness at drilling. These dimensions are not interchangeable.
For example, a 1.60 mm finished board thickness divided by a 0.20 mm specified finished hole gives an 8:1 finished-hole screening ratio. If a fabricator hypothetically used a 0.30 mm drill and the same 1.60 mm thickness for its assessment, the result would be approximately 5.33:1. The two ratios use different diameters; the hypothetical drill is not a recommended tool or plating allowance and does not establish the resulting finished hole size. Confirm the supplier's thickness, diameter and tolerance convention for the actual build.
Review the drill table
- Identify each hole's location, quantity, plated or non-plated status, and function as a via or component hole. Keep the drill files and drawing consistent.
- Specify the finished hole diameter, tolerance and measurement condition. For component holes, check lead fit and assembly requirements.
- Provide the stackup, materials, finished thickness and tolerance, and applicable copper and surface finish requirements. Ask the fabricator which thickness and diameter it uses for the assessment.
- Check the affected pad and annular ring, copper clearances and routing on each layer. Mark holes that cannot be changed without approval.
- Agree on the inspection or test evidence needed for the order. A microsection shows a local plane in a sampled hole, not every hole or lifetime performance; see PCB test coupons.
The smallest finished hole is a useful starting point for review, but component fit, clearances and the full construction also matter. Copper deposition and other processing can change the finished opening, so do not add an assumed plating allowance to design files unless the supplier agrees to that convention.
How to size a through via
- Start with the required board thickness and finished hole size, then check the calculation basis with the fabricator.
- If the hole is flagged, consider a larger finished hole or a thinner board. Recheck the pad, routing, component fit, stiffness, impedance and stackup before changing either.
- Where a through via cannot meet the layout requirements, discuss a different layer path or via structure. Compare its manufacturing sequence, cost and inspection requirements before revising the design.
Via-in-pad and filled vias
Via-in-pad places the via inside the component pad instead of beside it. Open holes in a pad would wick solder away from the joint during reflow, so the via is filled, planarized, and plated over. APT's drilling page lists VIPPO for fine-pitch BGA breakout and solder-wicking prevention, and as the base that lets one microvia be stacked on another.
Filling is not only for via-in-pad. Fill may be specified to keep solder mask or flux out of holes, to give a flat surface for assembly, or to support a stacked microvia. Fill material can be conductive or non-conductive, and the choice should be recorded on the drawing. For the process controls and acceptance points, see the via-in-pad manufacturing guide and the article on void control for VIPPO under BGAs.
Via protection (tenting, plugging, or filling with or without a cap) is classified in IPC-4761. Name the protection method you want on the drawing. "Tented" alone leaves room for interpretation.
Choosing a via structure: cost and lamination count
This is the decision table. Start in the top row and move down only when the layout forces you to. Relative cost is a ranking for the same board size and layer count, not a price.
| Via structure | Drilling steps | Extra lamination cycles | Relative cost | Move to it when |
|---|---|---|---|---|
| Through vias only | One mechanical pass | None | Lowest | Default; every net can escape with through vias |
| Through + mechanical blind (controlled depth) | Mechanical plus depth-controlled pass | Usually none | Low to moderate | A few outer-to-inner connections free up a congested layer |
| Through + buried | Mechanical on sub-stack, then final | One per buried span | Moderate | Inner channels are blocked, but outer layers are not |
| 1+N+1 HDI (one microvia layer per side) | Laser plus mechanical | One build-up cycle | Moderate to high | BGA pitch is too fine for through-via fan-out |
| 2+N+2 HDI (staggered or stacked) | Two laser steps per side plus mechanical | Two build-up cycles | High | One microvia layer still does not escape the package |
| Via-in-pad (filled and capped) | Adds fill, planarization, cap plating | None by itself | Adds to any of the above | Dog-bone fan-out does not fit between pads |
| Backdrill | Adds controlled-depth counter-drill | None | Adds to any of the above | Stub length hurts a fast channel |
Two rules keep this table honest:
- Count lamination cycles. Each one adds pressing, drilling registration, and inspection time. APT's HDI pages note that a 2+N+2 build adds lamination, registration, plating, inspection, cost, and schedule compared with 1+N+1.
- Do not mix structures casually. A board with buried vias, stacked microvias, and backdrilling has three separate process risks. If one structure can solve the routing alone, use one.
APT's rigid PCB capability page notes that fine-pitch BGAs around 0.4 mm or 0.5 mm, tight routing channels, or high-speed layer transitions that cannot be achieved with through vias are the usual triggers for an HDI build. When that is your situation, the HDI PCB manufacturing team can review whether a 1+N+1 structure is enough before you design for 2+N+2.
When vias affect signal integrity
At high data rates the via is part of the transmission line. The unused part of a through via below the last connected layer, the stub, can reflect energy. Options are to route the fast signal to a layer near the bottom, use a blind via, or backdrill the stub. APT publishes a backdrill depth accuracy of ±50 μm. The backdrill planning guide covers how to define depth and stub targets.
Thermal vias
Thermal via arrays move heat from an exposed pad into internal planes. They are ordinary through vias in a grid, but they create a solder-wicking problem under bottom-terminated packages. Decide early whether they will be filled, plugged, or left open with a paste-reduction pattern on the stencil.
How vias drive PCB cost
Beyond the structure itself, three via choices move the quote: total drill count (machine time), the smallest mechanical drill (tool wear and drill stack height), and aspect ratio near the top of the supplier's range (slower plating or extra cross-section checks). Microsection coupons for via structures add inspection scope when the order calls for them.
If the quote is higher than expected, ask the fabricator which via feature is driving it. Often one package forced the whole board into HDI, and moving or swapping that part removes a lamination cycle.
Via callouts on the fab drawing
A clear callout is the cheapest way to avoid a wrong build. Include:
- A drill table by layer pair, for example L1–L2 laser, L2–L7 buried, L1–L8 through, with finished or drilled sizes stated and which one is which
- Plated versus non-plated holes, separated in the NC drill files
- Via fill requirement and material (conductive or non-conductive), and whether a cap is required
- Via protection method by IPC-4761 type where used, and on which side
- Via-in-pad locations, if any, and the flatness or dimple expectation for those pads
- Backdrill locations, the layer that must stay connected, and the allowed stub
- The acceptance class for the board, for example IPC-6012 Class 2 or Class 3
APT's HDI capability page asks for the proposed stackup, a layer-to-layer via map, stacked or staggered callouts, buried vias, and via-in-pad locations with the RFQ. Sending those with Gerber X2, ODB++, or IPC-2581 data lets CAM confirm the structure instead of guessing it.
Why involve APTPCB in via planning?
APT reviews via structures as part of the engineering check before fabrication release. The review compares the via map with the stackup, finished thickness, drill sizes, and aspect ratio, then flags combinations that sit at the edge of the HDI capability range or that could be simplified. Final via diameter, aspect ratio, capture pad, and sequential-lamination feasibility are confirmed only after that review, because they depend on the complete material, stackup, panel, and quantity.
Relevant standards and references may include:
- IPC-2221: generic standard on printed board design
- IPC-2226: sectional design standard for HDI printed boards
- IPC-6012: qualification and performance of rigid printed boards
- IPC-4761: design guide for protection of printed board via structures
- IPC-A-600: acceptability of printed boards
Frequently asked questions
What are vias in a PCB used for?
Vias in a PCB carry a signal, power, or ground connection from one copper layer to another through a plated hole. It lets traces change layers, ties planes together, and in arrays it can move heat from a component into internal copper.
What are the main types of vias?
The main types of vias are through vias, blind vias, buried vias, and microvias. Variants built on these include stacked and staggered microvias, via-in-pad (filled and capped), backdrilled vias, and thermal via arrays.
What is the smallest via size a PCB can have?
The usable size depends on the hole structure, drilling method, board thickness, stackup, pad size and applicable requirements. Ask the fabricator to review the complete construction and state whether its dimensions refer to a drill or a finished hole.
How do you calculate a through-hole aspect ratio?
Divide the relevant board thickness by the hole diameter using the same units. State whether the diameter is a specified finished hole or a production drill, and confirm which dimensions and tolerances the fabricator uses for its review.
What is the difference between a blind via and a buried via?
A blind via starts on an outer layer and ends on an inner layer, so you can see it from one side. A buried via connects inner layers only and is not visible from either surface. Buried vias usually add a lamination cycle because they are drilled before the final press.
Do vias increase PCB cost?
Through vias add little beyond drill time. Blind, buried, laser, filled, capped, and backdrilled vias each add process steps, and HDI build-up layers add lamination cycles. The structure matters more than the number of holes.
Can you put a via in a pad?
Yes, but an open via in a pad will draw solder away from the joint. For BGA and fine-pitch pads, the via is normally filled, planarized, and plated over (VIPPO) so the pad is flat and solderable.
What is a PCB via?
A via is a conductive connection between board layers, commonly formed by plating a drilled or laser-formed hole. Through, blind, buried, and microvia structures differ in their layer spans and manufacturing requirements.
Via RFQ checklist
- Minimum mechanical drill size required
- Minimum laser drill size and type: CO2 or UV laser
- Aspect ratio (AR) of the deepest through via
- Via type by layer pair: through, blind, buried, microvia, via-in-pad
- Via fill requirement: conductive, non-conductive, or copper overfilled
- Via protection method: tented, plugged, or filled by IPC-4761 type
- Backdrill required: Y/N; target depth and depth tolerance ( ±50 µm)
- Interference-fit press-fit pin hole size and tolerance if applicable
- HDI structure: 1+N+1, 2+N+2, or other sequential lamination
- IPC-6012 acceptance class for the board
- Impedance-controlled nets with target impedance and tolerance
- Backdrill drill table: layer pair, stub length target, allowed residual
Use this checklist when you request a quote and discuss the proposed construction with the fabricator.
Picking the simplest via that routes
Start with through vias and a sensible drill size for your board thickness. Add a structure only when a specific package or channel cannot route without it, and count the lamination cycles each step adds. Then put the result on the drawing as a drill table and a via map. That gives the fabricator what it needs to quote the board you designed, and it gives you a clear place to cut cost if the first quote comes back high.
