PCB design guide
HDI PCB design: microvias, build-up layers and sequential lamination
High-density interconnect (HDI) boards use tiny laser-drilled vias and extra thin layers laminated in stages, so very fine-pitch parts can be routed in a small area. This guide explains how HDI works, which build-up to choose, where the reliability traps are and what to send us so our engineers can quote your HDI design.
Get an instant quoteWhat makes a board HDI — and when you really need it
There is no single switch that turns a board into HDI. In general use, a board is called HDI when it relies on microvias (very small, usually laser-drilled vias that join only neighbouring layers) and on fine lines and spaces to reach a wiring density that ordinary through-hole vias cannot give. IPC-2226 is the design standard most often referred to for HDI boards.
Typical HDI features
Signs you may need it
Signs you probably do not
Try conventional routing first
Laser microvias vs mechanically drilled vias
Both are plated holes that join copper layers; they differ in how they are made, how small they can be and which layers they can reach. For the basics of through, blind and buried vias, see vias and special holes.
| Property | Mechanically drilled via | Laser microvia |
|---|---|---|
| How it is made | Drilled with a rotating carbide bit after lamination | Ablated with a laser through a thin dielectric layer, then plated |
| Typical finished size | Roughly 0.15–0.3 mm and larger | Commonly about 0.075–0.15 mm at the top |
| Layers it spans | Usually through the whole board (or a blind/buried range in a sub-stack) | Usually one dielectric layer — from one copper layer to the next |
| Aspect ratio (depth : diameter) | Through-vias commonly up to about 8:1–10:1 | Kept low — a common rule is 1:1 or less (often about 0.6:1–0.8:1) so plating reaches the bottom of the hole reliably |
| Shape | Straight cylinder | Slightly tapered cone; may be left open, filled with copper or plugged |
| Main use | General interconnect, through-hole parts, the core of an HDI build | Fine-pitch BGA escape, via-in-pad, dense outer-layer routing |
Capture and target pads
Dielectric thickness
What our online calculator covers
Build-up structures: 1+N+1, 2+N+2 and any-layer
HDI boards are described by how many microvia build-up layers sit on each side of a conventional core. "N" is the core: an ordinary laminated stack with mechanically drilled (often buried) vias.
| Structure | What it means | Lamination cycles (typical) | Typical use |
|---|---|---|---|
| 1+N+1 | One microvia build-up layer on each side of the core. Microvias go from L1 to L2 and from the bottom layer to the one above it. | Core + 1 build-up cycle | Entry-level HDI: 0.65–0.5 mm pitch BGAs, compact modules, many consumer and IoT products |
| 2+N+2 | Two build-up layers on each side. Microvias reach L1→L2→L3, either stacked or staggered. | Core + 2 build-up cycles | Denser BGAs (around 0.4 mm pitch), several large BGAs on one board, more routing channels |
| 3+N+3 and higher | Three or more build-up layers per side. | Core + 3 or more cycles | Very dense processors and memory, where routing cannot close otherwise |
| Any-layer (ELIC) | Every layer is a build-up layer, so a microvia can connect any neighbouring pair of layers anywhere. | Many cycles — roughly one per added layer | Smartphones and very small, very dense products; the most expensive option |
- 1
List the finest-pitch parts
Write down every BGA/CSP pitch and ball count. The finest pitch and the number of ball rows you must escape usually decide how many build-up layers you need. - 2
Count escape rows
As a rough rule, each routing layer escapes about one to two rows of balls at fine pitch. A BGA with many rows needs more layers reachable by microvias — that pushes you from 1+N+1 towards 2+N+2.Tip: Placing power and ground balls on dedicated plane layers frees routing channels for signals.
- 3
Pick the simplest structure that closes
Choose the lowest build-up count that routes the board. Moving from 1+N+1 to 2+N+2 adds a full lamination cycle. - 4
Agree the stack-up before routing
Confirm dielectric thicknesses, copper weights and impedance targets with the fabricator before detailed routing. See stack-up and impedance for the general approach.
Stacked vs staggered microvias
When a connection must go deeper than one build-up layer, microvias can either sit directly on top of each other (stacked) or be offset from each other (staggered).
| Stacked microvias | Staggered microvias | |
|---|---|---|
| Arrangement | Each microvia sits directly on the one below; lower ones are copper-filled | Each microvia is offset sideways and joined by a short trace or pad |
| Board space | Smallest footprint — ideal under a fine-pitch BGA | Uses more area per connection |
| Process | Lower microvias must be copper-filled and planarised before the next layer | Filling is often not needed; simpler plating |
| Reliability | More sensitive to thermal stress; the interface between stacked vias is a known weak point if filling or plating is not well controlled | Generally more tolerant of thermal cycling and repeated reflow |
| Cost | Higher | Lower |
A common rule for reliability
Sequential lamination — why each build-up adds cost and time
A conventional multilayer board is pressed once. An HDI board is built in stages: the core is laminated, drilled and plated, then each build-up layer is added and processed in turn.
- 1
Build the core
Inner layers are imaged, etched and laminated into the core. Buried vias in the core are mechanically drilled, plated and usually filled so the surface is flat for the next layer. - 2
Add a build-up dielectric and copper
A thin dielectric (prepreg or resin-coated copper) is laminated onto each side of the core. - 3
Laser drill the microvias
The laser opens holes down to the target pads. The holes are cleaned so plating bonds to the copper underneath. - 4
Plate, fill and image
Microvias are plated (and copper-filled if another microvia will stack on top). The new outer copper is imaged and etched. - 5
Repeat for each extra build-up
Every further build-up layer repeats lamination, laser drilling, plating and imaging — and puts the board through another heat-and-pressure cycle. - 6
Finish as a normal board
Final through-holes, solder mask, surface finish, profiling and electrical test follow, as on any multilayer board.
Cost
Time
Material stress
Fanning out fine-pitch BGAs with via-in-pad
With fine-pitch BGAs there is often no room for a dog-bone (a short trace from the ball pad to a nearby via). Placing the via directly in the ball pad solves the space problem — but only if the via is filled and capped.
| BGA pitch | Common fan-out approach (general guidance) |
|---|---|
| 1.0 mm and 0.8 mm | Usually dog-bone fan-out with through-vias between the balls; HDI is rarely required. |
| 0.65 mm | Dog-bone is tight; small through-vias or via-in-pad, depending on the ball count and trace width. |
| 0.5 mm | Typically via-in-pad with laser microvias (1+N+1 or 2+N+2). |
| 0.4 mm and finer | Microvia-in-pad with stacked or staggered microvias; often 2+N+2 or more. |
Why the via must be filled and capped
What to put in your drawing
Filled & capped vias in our online calculator
Material and surface-finish choices that suit HDI
HDI boards see more heat cycles than ordinary boards — several laminations, then reflow and possibly rework — and their thin dielectrics must be laser-drillable.
High Tg and high decomposition temperature
Low Z-axis expansion
Laser-friendly dielectrics
Low-loss materials for high speed
Flat surface finish
Moisture handling for assembly
What to send us and how HDI boards are quoted
HDI boards are not part of our instant price. Our online calculator prices FR-4 and flex boards up to 16 layers with through-vias; HDI designs are reviewed and quoted by our engineering team.
| Item | What to include |
|---|---|
| Gerber or ODB++ files | All copper, mask, silkscreen and outline layers, with clear layer names and order. |
| Drill files per span | A separate drill file for each via span (for example L1–L2, L2–L3, L3–L6, L1–L8 on an 8-layer 2+N+2 board), each marked laser or mechanical. |
| Stack-up drawing | Layer order, copper weights, dielectric thicknesses, build-up structure (1+N+1, 2+N+2 …) and any material preference. |
| Via details | Microvia sizes and capture/target pads, stacked or staggered, which vias are in pad, fill type (epoxy or copper) and capping. |
| Impedance targets | Trace widths, reference layers and target impedances with tolerance, if the board has controlled-impedance nets. |
| Fabrication notes | Surface finish, solder mask colour, board thickness and tolerance, and any standard or class the board must meet (for example IPC-6012 class). |
| Quantity | How many boards you need (minimum 5 PCBs) and whether you also need assembly. |
- 1
Upload files and use Send for quote
Upload your design with the notes above. Our engineers check your files before production, and production notes inside your files are read and compared with the options we can offer. - 2
Engineering review
Our team reviews the stack-up, via structure and any special requirements, and comes back with questions if something is unclear or could be simplified. - 3
Quotation
You receive a quotation for the reviewed build. As with all orders, payment is made at order time, by online payment or bank transfer.
Assembling an HDI board
HDI FAQ
Related guides
Still have a question?
Send us your files or call us — our engineers will help you choose the right options for your boards and assembly.
Streamline your innovation with
seamless PCB ordering.