[Home](https://www.chinasuqi.com/)
/
[Blog](https://www.chinasuqi.com/en/blog/)
/
Via Types Explained: Through, Blind, Buried and Microvia
GUIDE / PCBELEC
# Via Types Explained: Through, Blind, Buried and Microvia
Through, blind, buried and microvia compared by span, drill method, aspect ratio and cost, plus via fill types per IPC-4761 and the DFM checks that decide the price.
[Discuss your requirements ↗](https://www.chinasuqi.com/en/request-a-quote/)
## The short answer
A via is a plated hole that connects copper on two or more layers. There are four types, and the difference is which layers the hole touches and when it is drilled.
A through via passes through the whole board. A blind via starts on an outer layer and stops at an inner layer. A buried via connects two inner layers and never reaches the surface. A microvia is a laser-drilled hole of 150 µm or less, normally connecting one layer to the next.
Everything else — backdrilling, via-in-pad, filled and capped vias — is a variation on those four, not a fifth type.
## The four types side by side
Cost index is relative to a plain through via on the same board and same layer count. It moves with layer count, aspect ratio and how many sequential lamination cycles the build needs.
| Type | Connects | Drilled | Cost index | Used for |
| --- | --- | --- | --- | --- |
| Through | Every layer | After lamination, mechanically | 1.0 | Default routing, connectors, through-hole parts |
| Blind | Outer to one inner | After first lamination, depth controlled | 1.3–1.6 | BGA escape, dense outer routing |
| Buried | Two inner layers | Before final lamination | 1.5–2.0 | Internal routing in sequential builds |
| Microvia | Layer to adjacent layer | Laser, ≤150 µm | 1.8–3.0 per cycle | HDI, fine-pitch BGA, phone-class density |
| Backdrill | Removes unused stub | After plating, mechanically | +0.2–0.4 | High-speed differential pairs |
## Through vias: the default, and its limit
A through via is drilled after the board is laminated and plated in one pass. It is the cheapest option because it uses one drill program and one plating cycle, and it is the most reliable because the barrel is supported by the full stack.
Its cost is real estate. A through via occupies a pad on every layer it crosses, so on a 12-layer board a via that only needs to reach layer 3 blocks routing on nine layers it never uses. On dense boards that alone forces a redesign.
The other limit is aspect ratio: board thickness divided by drill diameter. Standard processes handle about 8:1 comfortably, 10:1 with attention, and beyond 20:1 only with special plating and a supplier who builds backplanes. A 3.2 mm board with a 0.2 mm drill is 16:1, which is not a standard build.
## Blind and buried vias: buying layers back
A blind via reaches an inner layer from one side. It frees the layers below from its pad, which is what lets a BGA escape on a board that would otherwise need two more layers.
A buried via connects two inner layers and is invisible after lamination. Both are made by drilling before the layers are bonded, which means the board is built in stages — a sequential lamination. Each stage is a separate drill, plate and bond cycle, and each cycle adds cost, lead time and yield risk.
The practical consequence is that blind and buried vias are chosen per layer pair, not per board. A design that needs one buried via between layers 3 and 4 is a different quotation from one that needs buried vias on every inner pair, because the second needs more cycles.
Depth-controlled drilling is the other constraint. A blind via that must stop at layer 2 has a tolerance on how deep it goes, and a drill that overshoots breaks the connection. The tolerance is a process parameter that has to be stated on the drawing.
## Microvias: laser, and one layer at a time
A microvia is a laser-drilled hole of 150 µm or less with an aspect ratio near 1:1, connecting one layer to the adjacent layer. IPC-2226 defines the structure; the practical rule is that a microvia goes through one dielectric layer, not two.
Two arrangements exist. Staggered microvias step sideways from layer to layer, so each one lands on a separate pad. Stacked microvias sit directly on top of each other, which saves the most space and is the hardest to build, because the stack has to be filled and planarised before the next laser hit.
That filling step is where most microvia failures originate: an incompletely filled via leaves a void, and the next lamination collapses it. Via-in-pad makes this worse, because the pad also has to be flat enough for a solder joint.
## Via protection: IPC-4761
How a via is sealed matters as much as how it is drilled, and it is specified separately. IPC-4761 defines seven protection types, from tented (Type I) through plugged, filled and capped, to filled and capped with plating over the pad (Type VII).
A via-in-pad that is only tented will wick solder during reflow, leaving a void under the ball. This is the single most common via-related defect we see in DFM review, and it is a specification gap rather than a manufacturing fault.
| Protection | What it does | Where it is required |
| --- | --- | --- |
| Tented | Mask covers the hole | Default on non-functional vias |
| Plugged | Mask or plug material in the barrel | Vias near pads that must not wick |
| Filled and capped | Epoxy fill, planarised, capped | Via-in-pad under BGA |
| Filled, capped and plated | Fill plus copper over the pad | Via-in-pad that also carries a solder joint |
## Backdrilling
On thick boards carrying high-speed signals, the unused part of a through via — the stub — acts as a resonator and degrades the signal at multi-gigabit rates. Backdrilling removes that stub from the far side after plating.
It is a mechanical operation with its own tolerance, and it adds a process step. It is worth it above roughly 5 Gb/s on thick boards, and rarely worth it on a 1.6 mm board with short vias.
## The DFM checks that decide the price
Before a via-heavy design is quoted, five things get checked, and each one can change the number.
The layer arrangement itself is the other variable, and
[the stackup reference builds ↗](https://www.chinasuqi.com/en/blog/pcb-layer-stackup-design-reference-builds-for-4-6-and-8-layers/)
show what a sequential build looks like in practice.
[The HDI fabrication page ↗](https://www.chinasuqi.com/en/pcb-technologies/hdi/)
covers buildup structures from 1+N+1 upward, and
[the Gerber DFM check list ↗](https://www.chinasuqi.com/en/blog/gerber-dfm-check-twelve-errors-that-stop-a-file/)
includes the via errors that stop a file before it reaches the drill.
A via is a process decision disguised as a geometry decision. The moment a design leaves through vias behind, the board is built in stages, and the quotation follows the stages.
| Check | Why it matters |
| --- | --- |
| Annular ring | A blind via with 0.05 mm ring is a yield problem, not a design choice |
| Drill-to-copper | Too close and the drill breaks into the neighbouring pad |
| Aspect ratio per via type | Above 10:1, plating uniformity and reliability both drop |
| Via count per net class | Thousands of microvias cost more than a few hundred blind vias |
| Fill requirement on via-in-pad | Type VII adds fill, planing and plating steps |
## What to send with the RFQ
A via map that states, for each type: the layers connected, the drill diameter, the aspect ratio and whether it is filled. Plus the stackup, the layer count and the finish. If the design is HDI, say which layers are microvia layers and whether they are stacked or staggered.
The fastest way to get a firm number is a Gerber set plus a via table. A drawing that shows via types on the artwork but not in a table is where the second quotation round starts, which is the same problem described in
[the PCBA quotation inputs ↗](https://www.chinasuqi.com/en/blog/pcba-quotation-inputs-the-9-things-we-need-to-quote-accurately/)
.
Send the via table with the Gerber set and we will return a DFM report that names the vias which drive cost, before the quotation is built on assumptions.
Questions, answered
## Before your next build
What is the difference between a blind via and a buried via?
A blind via is visible from one surface and ends at an inner layer. A buried via connects two inner layers and is fully enclosed after lamination, so it cannot be seen or probed from outside.
How small can a microvia be?
The usual definition is 150 µm or less with an aspect ratio near 1:1, drilled by laser. Below about 75 µm the pad and the capture land become the limiting factor rather than the drill.
Why do blind and buried vias cost more?
Because they require sequential lamination. Each stage means an extra drill, plate and bond cycle, and the panel is handled more times, so both labour and yield loss rise with the number of cycles.
Can I put a via in a BGA pad?
Yes, if it is filled and capped and preferably plated over, which is IPC-4761 Type VII. A tented via in a pad will wick solder and produce voids under the ball.
CONTINUE YOUR REVIEW
## Related manufacturing resources
Explore
### [DFM and Design Rules ↗](https://www.chinasuqi.com/en/blog/dfm-design-rules/)
An index to the design decisions that set the price of a board before anyone quotes it: stackup, hole size, annular ring, clearance, surface finish and panelisation, in the order they should be decided.
technology
### [HDI PCB fabrication ↗](https://www.chinasuqi.com/en/pcb-technologies/hdi/)
HDI PCB fabrication uses fine circuit features and defined via structures for high-density interconnection. Buildup sequence and layer spans set the process.
guide
### [PCB Layer Stackup Design: Reference Builds for 4, 6 and 8 Layers ↗](https://www.chinasuqi.com/en/blog/pcb-layer-stackup-design-reference-builds-for-4-6-and-8-layers/)
Four working stackups you can hand to a fabricator, what each one costs, and the three constraints that override any drawing: impedance target, finished thickness and copper weight.
guide
### [Gerber DFM Check: Twelve Errors That Stop a File at Review ↗](https://www.chinasuqi.com/en/blog/gerber-dfm-check-twelve-errors-that-stop-a-file/)
Twelve defects that show up in a Gerber package before fabrication starts, what each one costs if it survives to the drill, and which of them only the designer can fix.
YOUR NEXT PCB PROJECT
## Let’s define your next build.
Start with your files, requirements and target date.
[Prepare a PCB inquiry ↗](https://www.chinasuqi.com/en/request-a-quote/)

Canonical page: https://www.chinasuqi.com/en/blog/via-types-explained-through-blind-buried-microvia/