+91 8866188126 [email protected]

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 quote

What 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

Laser microvias, one or more build-up layers on each side of a core, via-in-pad under fine-pitch parts, thin dielectric layers between build-up copper and narrow traces and spaces on the outer layers.

Signs you may need it

BGAs or CSPs at 0.5 mm pitch or finer, a large pin-count BGA that cannot be escaped with dog-bone vias, a board outline that is fixed and too small for the routing, or a layer count that keeps climbing with through-vias only.

Signs you probably do not

Parts at 0.8 mm pitch or coarser, enough board area to fan out with dog-bone vias, and a design that fits comfortably in 4–8 through-via layers. A conventional multilayer board is usually cheaper and faster in these cases.

Try conventional routing first

A common approach is to check whether a few extra through-via layers or a slightly larger outline would solve the routing problem. HDI is powerful, but every build-up cycle adds cost and time — use it when it genuinely saves space, layers or signal-quality problems.

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.

PropertyMechanically drilled viaLaser microvia
How it is madeDrilled with a rotating carbide bit after laminationAblated with a laser through a thin dielectric layer, then plated
Typical finished sizeRoughly 0.15–0.3 mm and largerCommonly about 0.075–0.15 mm at the top
Layers it spansUsually 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 8:1–10:1Kept 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
ShapeStraight cylinderSlightly tapered cone; may be left open, filled with copper or plugged
Main useGeneral interconnect, through-hole parts, the core of an HDI buildFine-pitch BGA escape, via-in-pad, dense outer-layer routing

Capture and target pads

A microvia lands on a target pad on the layer below and is surrounded by a capture pad on the layer it starts from. A common rule of thumb is a capture pad roughly 0.15–0.25 mm larger than the laser hole, but the right annular ring depends on the fabricator’s registration — ask before you lock the footprint.

Dielectric thickness

Build-up dielectrics are thin — often in the 50–100 µm range — so the microvia stays shallow. Thinner dielectric also changes trace impedance, so plan the stack-up early (see the stack-up section below).

What our online calculator covers

Our online calculator prices mechanically drilled through-vias on FR-4 boards up to 16 layers, with a minimum via setting down to 0.1 mm drill on boards with 4 or more layers (the smallest settings come with board-thickness, material and surface-finish limits). Laser microvias, blind and buried vias are not part of the instant price — those designs are quoted by our team.

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.

StructureWhat it meansLamination cycles (typical)Typical use
1+N+1One 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 cycleEntry-level HDI: 0.65–0.5 mm pitch BGAs, compact modules, many consumer and IoT products
2+N+2Two build-up layers on each side. Microvias reach L1→L2→L3, either stacked or staggered.Core + 2 build-up cyclesDenser BGAs (around 0.4 mm pitch), several large BGAs on one board, more routing channels
3+N+3 and higherThree or more build-up layers per side.Core + 3 or more cyclesVery 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 layerSmartphones and very small, very dense products; the most expensive option
  1. 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. 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. 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. 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 microviasStaggered microvias
ArrangementEach microvia sits directly on the one below; lower ones are copper-filledEach microvia is offset sideways and joined by a short trace or pad
Board spaceSmallest footprint — ideal under a fine-pitch BGAUses more area per connection
ProcessLower microvias must be copper-filled and planarised before the next layerFilling is often not needed; simpler plating
ReliabilityMore sensitive to thermal stress; the interface between stacked vias is a known weak point if filling or plating is not well controlledGenerally more tolerant of thermal cycling and repeated reflow
CostHigherLower

A common rule for reliability

Many designers prefer staggered microvias where space allows, and limit stacks to two levels where they can. Long stacks of three or more microvias have been linked to latent cracks after repeated reflow and thermal cycling, which is why industry guidance (for example in IPC-6012 and related IPC documents) puts extra attention on microvia reliability testing. If your design needs deep stacks, tell us early so the build can be reviewed.

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. 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. 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. 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. 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. 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. 6

    Finish as a normal board

    Final through-holes, solder mask, surface finish, profiling and electrical test follow, as on any multilayer board.

Cost

Each extra build-up cycle adds lamination, drilling, plating and inspection steps, plus a yield risk on every layer. Via filling and planarising add more. The price rises with the number of cycles, not just the layer count.

Time

Steps are sequential — a build-up cannot start until the previous one is finished — so each cycle extends the production time compared with a single-press board.

Material stress

Repeated lamination and later reflows heat the laminate several times. This is why HDI boards usually need materials rated for many thermal cycles (see materials below).

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 pitchCommon fan-out approach (general guidance)
1.0 mm and 0.8 mmUsually dog-bone fan-out with through-vias between the balls; HDI is rarely required.
0.65 mmDog-bone is tight; small through-vias or via-in-pad, depending on the ball count and trace width.
0.5 mmTypically via-in-pad with laser microvias (1+N+1 or 2+N+2).
0.4 mm and finerMicrovia-in-pad with stacked or staggered microvias; often 2+N+2 or more.

Why the via must be filled and capped

An open via in a solder pad wicks solder paste away from the joint during reflow, leaving voids or an incomplete joint. Filling the via (with conductive or non-conductive epoxy, or with copper for microvias) and plating a flat copper cap over it gives a solid, flat pad. IPC-4761 describes this as a filled and capped via type.

What to put in your drawing

Mark which vias are in pad, state the fill type (non-conductive epoxy, conductive epoxy or copper fill) and say they must be capped and planarised. Leaving this out is one of the most common causes of HDI quote questions.

Filled & capped vias in our online calculator

For rigid FR-4 boards with through-vias, our online calculator offers Epoxy filled & capped and Copper paste filled & capped via options, suitable for via-in-pad with mechanically drilled vias. Microvia-in-pad on HDI builds is reviewed and quoted by our team.

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

A common choice is a high-Tg FR-4-class laminate (Tg around 170 °C or above) with a high decomposition temperature (Td), so the board tolerates repeated lamination and lead-free reflow.

Low Z-axis expansion

Lower through-thickness expansion (CTE) reduces stress on plated holes and microvia joints during heating, which helps with stacked microvias.

Laser-friendly dielectrics

Thin prepregs with fine, evenly spread glass weaves — or resin-coated copper with no glass at all — let the laser make clean, round holes.

Low-loss materials for high speed

For fast serial links, low-loss laminates reduce signal attenuation. They usually cost more and may affect lead time, so ask before you specify one.

Flat surface finish

Fine-pitch pads need a flat finish. ENIG and OSP are flat; HASL leaves an uneven surface and is generally avoided on HDI. See choosing a surface finish.

Moisture handling for assembly

Thin, dense boards can absorb moisture. A common practice is to bake bare boards when needed (IPC-1601 gives general guidance) and to handle moisture-sensitive components according to J-STD-033 before reflow.

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.

ItemWhat to include
Gerber or ODB++ filesAll copper, mask, silkscreen and outline layers, with clear layer names and order.
Drill files per spanA 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 drawingLayer order, copper weights, dielectric thicknesses, build-up structure (1+N+1, 2+N+2 …) and any material preference.
Via detailsMicrovia sizes and capture/target pads, stacked or staggered, which vias are in pad, fill type (epoxy or copper) and capping.
Impedance targetsTrace widths, reference layers and target impedances with tolerance, if the board has controlled-impedance nets.
Fabrication notesSurface finish, solder mask colour, board thickness and tolerance, and any standard or class the board must meet (for example IPC-6012 class).
QuantityHow many boards you need (minimum 5 PCBs) and whether you also need assembly.
  1. 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. 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. 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

Our PCBA instant price is calculated from solder pads, but designs with BGA, LGA or 0201 parts go to engineering review. Assembly is done in panels and components are quoted from your BOM. See assembly services and the assembly quote FAQ.

HDI FAQ

No. Our instant price covers FR-4 and flex boards up to 16 layers with through-vias. Boards with laser microvias, blind or buried vias are quoted by our engineering team — upload your files and use Send for quote.

A blind via is any via that starts on an outer layer and stops inside the board. A microvia is a very small, usually laser-drilled via that typically spans just one dielectric layer. Many microvias are blind, but a mechanically drilled blind via that spans several layers is not a microvia.

It often is for 0.5–0.65 mm pitch BGAs with a moderate number of ball rows. Very fine pitch (around 0.4 mm), several large BGAs or very high pin counts usually need 2+N+2 or more. Send us the design and our team can suggest the simplest structure that works.

Staggered microvias are generally more robust and cheaper; stacked microvias save space under fine-pitch parts. A common rule is to stagger where you can and keep stacks short.

In practice, almost always. An open via inside an SMD solder pad can draw solder away from the joint during reflow and cause voids. The usual rule is to specify filled and capped (or, for microvias, copper-filled) vias for every via-in-pad.

A flat finish such as ENIG or OSP is generally preferred for fine-pitch pads. See choosing a surface finish for the trade-offs.

Each build-up layer needs its own lamination, laser drilling, plating and inspection, done one after another. The number of build-up cycles, via filling and stacked vias all add cost and time. See what drives PCB cost.

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.

For More Details Contact Us