HDI Rigid-Flex PCB Design & Manufacturing

25 September 2026
New

An HDI Rigid-Flex PCB combines rigid multilayer sections, flexible polyimide interconnects, and high-density interconnect features such as laser-drilled microvias, blind/buried vias, via-in-pad, fine lines, and sequential lamination in one integrated circuit. A practical HDI Rigid-Flex PCB may use 50–100 µm laser microvias, 50/50–75/75 µm line/space, 12–35 µm flex copper, 25–50 µm polyimide, and 75–100 µm HDI dielectric layers. Reliable production depends on designing the rigid, flex, and HDI structures as one mechanical-electrical system: microvia geometry, copper type, bend radius, material expansion, desmear chemistry, impedance, and rigid-to-flex transition geometry must be defined before the stackup is released.

HDI Rigid-Flex Characteristics

Structure and HDI Technology

A conventional Rigid-Flex PCB connects rigid component areas through flexible layers that remain permanently integrated into the multilayer construction. HDI technology adds localized interconnect density where fine-pitch BGA or dense routing requires more escape channels.

Typical HDI features include:

Laser microvias: 50–100 µm finished diameter
Capture pads: typically 200–300 µm
Fine line/space: 50/50–75/75 µm
Mechanical PTH: typically ≥0.20–0.25 mm
Via-in-pad plated over structures
Copper-filled microvias
Blind and buried vias
Sequential lamination
Staggered or stacked microvias
Controlled impedance: commonly ±10%, with tighter targets requiring process review

This combination is particularly useful below 0.8 mm BGA pitch. At 0.5 mm and 0.4 mm pitch, conventional through-hole fanout can consume too much routing area, while microvias can transfer signals directly from BGA pads to adjacent routing layers.

The manufacturing consequence is significant: an HDI Rigid-Flex PCB is not simply a flexible PCB board with smaller holes. It combines HDI registration tolerances with flex-specific dimensional movement.

Common Constructions

A typical 10-layer HDI Rigid Flex PCB may be structured as:

L1-L2: laser microvia
L2-L3: optional staggered or stacked microvia
L1-L3: HDI build-up region
L4-L7: flex-layer region
L1-L10: mechanical PTH in rigid areas
Rigid areas: FR-4 or high-speed laminate
Flex core: polyimide with RA copper
External flex protection: polyimide coverlay

Common HDI constructions include:

Construction	HDI structure	Relative process complexity	Typical use
1+N+1	One HDI build-up each side	Moderate	0.8–0.65 mm BGA
2+N+2	Two sequential HDI levels	High	0.5 mm BGA
3+N+3	Three build-up levels	Very high	Dense FPGA/processor routing
Any-layer	Microvia interconnection across multiple layers	Highest	Extreme routing density

Every additional sequential lamination cycle adds registration, plating, thermal, and material-interaction risk.

HDI Rigid-Flex PCB Material

Rigid and Flex Materials

The rigid and flexible regions require different material behavior.

A representative material set includes:

Flexible region

Polyimide: 25–50 µm
RA copper: 12–35 µm
Coverlay polyimide: 12.5–25 µm
Coverlay adhesive: approximately 15–50 µm
Adhesiveless FCCL for dynamic or thin constructions

Rigid region

FR-4 Tg: typically 150–180°C
High-Tg FR-4: ≥170°C for demanding thermal cycles
Low-loss material for high-speed channels where required
HDI build-up dielectric: approximately 50–100 µm after processing
Copper foil: typically 12–35 µm before additional plating

Adhesiveless flex laminate is often preferred in high-density structures because removing the base adhesive reduces thickness and improves dimensional stability.

The material set should be frozen before final impedance routing. Changing a 50 µm dielectric to 75 µm after layout can materially alter both impedance and the required trace geometry.

Material Variations

Rigid and flex materials respond differently to heat, pressure, moisture, plasma, chemistry, and mechanical loading.

That creates a manufacturing issue rarely visible in CAD: one panel contains materials with different dimensional and surface behaviors.

A 0.10% dimensional change across a 300 mm reference length equals 0.30 mm. That is several times larger than the registration window of a 75 µm microvia.

For this reason, the HDI Rigid-Flex PCB manufacturer must control:

Polyimide dimensional movement
Rigid laminate expansion
Copper distribution
Lamination pressure
Resin flow
Flex-zone protection
Laser registration
Coverlay movement

Material selection is therefore directly linked to microvia registration.

HDI Rigid-Flex PCB Stackup

Stackup Design Rules

Stackup development should begin before detailed routing.

A practical 12-layer HDI Rigid-Flex PCB could use:

L1-L2: 75 µm laser microvia
L2-L3: 75 µm laser microvia
L3-L10: multilayer core structure
L11-L12: symmetrical HDI build-up
L5-L8: flex section
18 µm RA copper in active flex layers
25–50 µm polyimide flex dielectric
60–100 µm HDI dielectric
0.20–0.25 mm minimum mechanical drill
50/50–75/75 µm minimum line/space in HDI areas

Symmetry is important. An asymmetric copper or dielectric structure increases bow, twist, and local stress during lamination.

HDI Stackup Comparison

Parameter	Standard Rigid-Flex PCB	HDI Rigid-Flex PCB
Typical line/space	100/100 µm	50/50–75/75 µm
Smallest common via	0.20–0.30 mm PTH	50–100 µm microvia
Sequential lamination	Often unnecessary	1–3+ cycles
Via-in-pad	Limited need	Common
BGA pitch	≥0.8 mm easier	0.4–0.65 mm practical
Registration demand	Moderate	High
Fabrication complexity	High	Very high

The correct construction is determined by escape routing, not by choosing the largest possible HDI order.

If a 1+N+1 structure can escape the BGA, specifying 3+N+3 adds two unnecessary sequential lamination stages and increases cost and reliability exposure.

HDI Rigid-Flex Design Guidelines

No Vias in Bend Areas

Vias create rigid copper cylinders through an otherwise flexible structure. They become mechanical stress concentrators when placed in an active bend.

Production-oriented starting rules are:

No PTH, blind via, or microvia inside an active bend.
Keep vias approximately 1.0–2.0 mm from static bend transitions where geometry permits.
Use 2.0–3.0 mm or more separation for dynamic flex zones.
Avoid placing a via at the edge of a stiffener.
Use teardrops at trace-to-pad transitions where appropriate.
Keep pad geometry outside the bend tangent region.

Moving a via 2 mm away from a bend can produce more reliability benefit than adding copper to the flex trace because it removes the local strain concentration.

Bend Radius and Routing

Practical starting bend ratios are:

Single-layer static flex: ≥6× flex thickness
Double-layer static flex: ≥10×
Multilayer flex: ≥12×
Dynamic flex: ≥20×, with larger radii preferred for high cycle counts

For a 0.20 mm flexible section, a 20× dynamic design begins at approximately a 4.0 mm radius.

Inside the bend:

Route traces perpendicular to the bend axis.
Avoid 90° corners.
Use smooth curved trace transitions.
Avoid abrupt width changes.
Stagger conductors between adjacent layers.
Avoid solid copper planes in repeatedly flexing regions when electrical requirements allow.
Prefer RA copper for repeated bending.

The mechanical drawing should identify bend radius, bend angle, direction, and cycle requirement. “Flexible area” alone is insufficient for manufacturing qualification.

Benefits of HDI Rigid-Flex

Space Saving and Density

An HDI Rigid-Flex PCB combines two different density improvements.

First, rigid-flex construction eliminates board-to-board cables and connectors. Second, HDI microvias increase routing density around fine-pitch devices.

For example, a 0.4 mm BGA may require 75 µm microvias and approximately 50–75 µm routing features depending on pad geometry and stackup.

The result can be:

Fewer connectors
Reduced assembly volume
Shorter interconnect paths
Higher component density
Fewer discrete cable assemblies

The value is not merely a smaller PCB. The entire electromechanical system can become smaller.

High Reliability

A conventional multi-board assembly may require two rigid PCBs, two connectors, and one cable harness.

A Rigid Flexible PCB can replace these interfaces with one continuous circuit.

Removing connectors eliminates contact interfaces susceptible to:

Fretting
Vibration
Improper mating
Bent pins
Assembly variation

However, rigid-flex only improves system reliability when bend geometry, copper selection, transition zones, and lamination are properly controlled.

Signal Integrity

HDI can shorten routing between a BGA pad and its reference layer.

For high-speed signals, this can reduce:

Via stub length
Parasitic inductance
Layer-transition distance
Connector discontinuities

Typical controlled targets include:

50 Ω single-ended
90 Ω differential USB-class structures
100 Ω differential structures
Manufacturing tolerance commonly ±10%

A controlled-impedance Rigid-Flex PCB requires separate field-solver evaluation for rigid and flex regions because dielectric materials, thickness, coverlay, reference planes, and surrounding air can change along the signal path.

HDI Manufacturing Process

Sequential Lamination

A representative 2+N+2 manufacturing flow is:

Image and etch inner rigid and flex layers.
Apply flex coverlay where required.
Form the initial multilayer substructure.
Perform surface preparation and lamination.
Add first HDI dielectric and copper.
Laser-drill microvias.
Desmear and condition microvia surfaces.
Electroless copper deposition.
Electroplate microvias.
Image and etch the HDI layer.
Repeat build-up for the second HDI stage.
Drill mechanical PTHs.
Desmear and plate through holes.
Form external circuitry.
Apply rigid-area solder mask.
Apply final surface finish.
Route rigid outline and expose flex regions.
Perform electrical and dimensional inspection.

The order can vary with construction, but the core principle remains: each sequential HDI level must be built, registered, drilled, metallized, and verified before the next interconnect level is completed.

Specialized Desmearing

Desmear is more complicated in an HDI Rigid-Flex PCB than in a conventional FR-4 multilayer because polyimide and epoxy-based materials respond differently to chemical and plasma processes.

After laser drilling, the microvia bottom must expose clean copper without leaving carbonized polymer or resin residue.

Process options include:

Plasma treatment
Permanganate chemistry for compatible materials
Combined plasma/chemical processes
Material-specific conditioning

Over-processing can attack polyimide or alter the microvia geometry. Under-processing can leave residue at the capture pad and reduce copper adhesion.

For a 75 µm laser microvia, even a thin residue layer at the via bottom can interfere with metallization over a significant percentage of the contact area.

The process recipe must therefore follow the actual dielectric system rather than reusing a standard rigid FR-4 desmear cycle.

Microvia Reliability

Stacked vs Staggered Vias

Stacked microvias maximize routing density but concentrate interfaces vertically.

Staggered microvias offset adjacent via levels and generally provide a larger process window when routing space permits.

Factor	Stacked microvia	Staggered microvia
Routing density	Highest	High
Footprint	Smaller	Larger
Registration sensitivity	Higher	Lower
Copper fill importance	Critical	Less demanding
Process complexity	Higher	Lower
Reliability margin	More structure-dependent	Generally wider

Where maximum density is unnecessary, staggered construction can reduce manufacturing risk.

Microvia Geometry

Microvia reliability is strongly influenced by via diameter, dielectric depth, capture-pad geometry, plating, and copper fill.

A typical HDI target may use:

Via diameter: 75 µm
Dielectric depth: 60 µm
Aspect ratio: 0.8:1
Capture pad: approximately 225 µm
Copper-filled structure for stacked vias

A shallow microvia is generally easier to plate reliably than a deep, narrow feature.

Increasing dielectric thickness from 60 µm to 100 µm while retaining a 75 µm via changes the geometry from 0.8:1 to approximately 1.33:1. That is not a trivial material substitution; it changes the plating process window.

Quality Control

Fabrication Inspection

A professional HDI Rigid-Flex PCB manufacturer should establish inspection around the actual construction rather than applying only generic rigid-board inspection.

Typical controls include:

100% continuity and isolation test
Laser microvia registration inspection
Microsection analysis
Copper-fill inspection
PTH wall inspection
Coverlay registration measurement
Flex thickness measurement
Rigid-to-flex transition inspection
Impedance coupon testing when specified
Finished dimensional inspection
Surface-finish inspection
Ionic cleanliness testing when required
Bend qualification when specified by the application

Microsections should specifically examine microvia bottoms, stacked-via interfaces, copper fill, capture-pad registration, PTH plating, and rigid-flex transition structures.

Applicable IPC Standards

IPC-2221C establishes generic printed-board design requirements, while IPC identifies IPC-2223 as the sectional design standard for flexible and rigid-flexible boards. IPC-6013E is the applicable qualification and performance specification for flexible and rigid-flex printed boards; its scope includes rigid-flex multilayers and permits build-up HDI layers.

Important documents include:

IPC-2221C: Generic Standard on Printed Board Design
IPC-2223E: Sectional Design Standard for Flexible/Rigid-Flexible Printed Boards
IPC-6013E: Qualification and Performance Specification for Flexible/Rigid-Flexible Printed Boards
IPC-4204: Flexible metal-clad dielectric material requirements
IPC-A-600: Printed-board acceptability criteria
IPC-TM-650: Applicable test methods

IPC-6012F addresses rigid printed boards, including rigid HDI technologies such as blind, buried, and microvias. For the completed rigid-flex product, however, IPC-6013 is the primary flex/rigid-flex performance specification rather than substituting IPC-6012 for the whole construction.

IPC currently lists IPC-2223F and IPC-6013F as final drafts for industry review, so IPC-2223E and IPC-6013E remain the released revisions at the time of writing.

Real HDI Rigid-Flex Case

12-Layer 2+N+2 Build

A representative factory case involved a compact control module requiring fine-pitch BGA fanout and a folded connection between two rigid component zones.

The production configuration was:

Layer count: 12
HDI construction: 2+N+2
Flex layers: 4
Flex copper: 18 µm RA
Flex polyimide: 25 µm
Laser microvia: 75 µm
Microvia depth: approximately 60 µm
Minimum line/space: 60/60 µm
Mechanical PTH: 0.20 mm
BGA pitch: 0.5 mm
Differential impedance: 100 Ω ±10%
Single-ended impedance: 50 Ω ±10%
Flex finished thickness: approximately 0.20 mm in the active bend region
Minimum specified bend radius: 4.0 mm

The first engineering lot showed reduced microvia-bottom process margin on one build-up layer and excessive mechanical concentration close to the rigid-flex transition.

The electrical CAD data was valid. The problems came from interaction between materials and manufacturing geometry.

Cross-section review showed that the selected dielectric thickness increased the microvia depth beyond the preferred process window. The design also placed copper features too close to the rigid-to-flex transition.

The corrective build used:

Reduced HDI dielectric thickness
Improved laser parameters for the actual dielectric
Material-specific desmear
Increased copper keep-back from the flex transition
Rebalanced copper around the transition zone
Revalidated impedance geometry after dielectric adjustment

The revised structure reduced the microvia aspect ratio and created a more uniform transition into the flexible section without changing the 0.5 mm BGA footprint.

The production lesson is straightforward: HDI density, flex mechanics, and material processing cannot be optimized independently.

Common Design Errors

HDI Layout Errors

Frequent production problems include:

Specifying stacked microvias when staggered vias have sufficient routing space.
Using a 100 µm dielectric with a 75 µm microvia without reviewing aspect ratio.
Placing laser vias too close to the rigid-flex transition.
Routing fine-pitch BGA escapes before confirming stackup.
Using the same impedance geometry in rigid and flex regions.
Designing 50/50 µm traces where 75/75 µm would complete the routing.
Adding unnecessary sequential lamination stages.

A smaller feature is not automatically a better HDI design. The preferred feature is the largest geometry that still solves the routing requirement.

Flex Layout Errors

Mechanical mistakes include:

Vias inside active bend areas
Stiffener edges on bend tangents
Thick ED copper in repeated-flex regions
Abrupt trace-width changes
Sharp corners inside bends
Solid copper directly through dynamic bends
Undefined bend radius
Undefined bend-cycle requirement

A fabrication drawing should identify each flexible region as installation-only or dynamic and specify bend radius, direction, angle, and cycle requirement where applicable.

HDI Rigid-Flex Manufacturer

Engineering Before Fabrication

A capable HDI Rigid-Flex PCB manufacturer should review the design before production tooling is generated.

The engineering review should confirm:

HDI order and sequential lamination count.
Microvia diameter and dielectric depth.
Stacked versus staggered microvia architecture.
Copper-fill requirement.
Rigid and flexible laminate compatibility.
Flex copper type and thickness.
Bend radius and bend zones.
Via-to-bend and via-to-transition distance.
Controlled-impedance structures.
Coverlay and stiffener geometry.
Material-specific desmear process.
Electrical test and reliability requirements.

The objective is not to manufacture the smallest possible features. It is to establish enough density for the component package while maintaining a repeatable fabrication window.

FAQ

What Is an HDI Rigid-Flex PCB?

Question: What is the difference between an HDI Rigid-Flex PCB and a standard Rigid-Flex PCB?

Answer: An HDI Rigid-Flex PCB adds high-density features such as 50–100 µm laser microvias, blind/buried vias, via-in-pad, copper-filled microvias, 50/50–75/75 µm routing, and sequential lamination to an integrated rigid-flex structure. Standard rigid-flex designs can often use conventional PTH technology and 100/100 µm or larger routing.

What Microvia Size Is Practical?

Question: What microvia diameter should be used for an HDI Rigid Flex PCB?

Answer: A 75–100 µm laser microvia is a practical production range for many HDI constructions, while approximately 50 µm requires tighter material, imaging, laser, and plating controls. Diameter cannot be selected independently of dielectric depth. A 75 µm via through a 60 µm dielectric has an aspect ratio of about 0.8:1, while the same via through 100 µm dielectric reaches approximately 1.33:1 and requires a substantially different process review.

Can Vias Be Put in a Bend?

Question: Can an HDI Rigid-Flex PCB use microvias inside the flexible bend area?

Answer: Microvias, PTHs, and other rigid plated structures should be kept outside active bend areas. A practical starting separation is approximately 1–2 mm from static bend transitions and 2–3 mm or more for dynamic regions, depending on thickness and mechanical geometry. The bend radius should also be defined numerically rather than leaving the manufacturer to infer it.

Which IPC Standard Applies?

Question: Which IPC standards apply to HDI Rigid Flexible PCB manufacturing?

Answer: IPC-2221C provides generic PCB design requirements, IPC-2223E addresses flexible and rigid-flex design, and IPC-6013E establishes qualification and performance requirements for flexible and rigid-flex printed boards, including constructions containing build-up HDI layers. IPC-6012F applies specifically to rigid printed boards and remains relevant to rigid-board HDI technology, but it should not replace IPC-6013 as the primary performance specification for the finished rigid-flex construction.