Comprehensive Guide to HDI PCBs: Design, Advantages, and Applications
15 min
- Design Tips for HDI PCB:
- The Advantages of HDI PCB:
- Different Types of Vias in HDI PCB:
- HDI PCB Materials Selection:
- Design Considerations for HDI PCBs:
- HDI PCB Manufacturing Process:
- Cost Effective HDI:
- HDI PCB Industries and Applications:
- FAQ about HDI PCBs
Key Takeaways
- Core HDI Limits: Standard HDI uses 3/3 mil trace/space and 0.075–0.15 mm (3–6 mil, 4 mil default) laser microvias across 1st- to 3rd-order stack-ups for optimal yield and density.
- Via-in-Pad Benefits: Copper-filled laser microvias and resin-plugged, plated-over vias (JLCPCB's POFV process) on SMT pads eliminate trace fan-out and prevent solder wicking.
- Symmetrical 1+N+1 or 2+N+2 staggered microvias cut sequential lamination cycles and thermal stress.
High Density Interconnect (HDI) printed circuit boards (PCBs) are circuit boards with a higher wiring density per unit area than traditional PCBs. HDI PCBs have denser interconnections and components, finer lines and spaces, and higher connection pad density. They also have smaller vias and traces, and higher layer counts. A single HDI board can accommodate the functionalities of multiple boards previously used in a device. HDI PCBs are a preferred choice for high-layer and expensive laminated boards. HDI PCBs require different fabrication and assembly processes than typical circuit boards. These circuit boards often involve higher manufacturing costs, more complex design considerations, and tighter manufacturability tolerances. However, with modern advanced fabrication technologies—such as JLCPCB's precision laser drilling and automated optical inspection (AOI)—HDI designs can be produced efficiently and cost-effectively.
Design Tips for HDI PCB:
1- Choose the type of vias to minimize process complexity
Choosing the appropriate via type determines the necessary lamination cycles, drilling operations, and total cost. For high-density BGA designs with fine pitch (e.g., ≤0.5 mm), traditional "dog-bone" routing consumes valuable surface space and increases parasitic inductance. Utilizing JLCPCB’s Plated Over Filled Via (POFV / Via-in-Pad) technology and copper-filled laser microvias allows vias to be placed directly inside component pads without solder wicking issues, significantly increasing routing density and enhancing thermal dissipation.
2- Choose the minimum number of components for HDI applications
Component selection directly dictates the trace widths, clearance, via sizes, and required layer stack-up. To maximize HDI efficiency, prioritize compact surface-mount devices (SMD) and fine-pitch packages (such as 0.4 mm/0.5 mm pitch BGAs, WLCSPs, and 0201/01005 passives) paired with an ENIG surface finish for optimal pad coplanarity. Replacing bulky through-hole components with integrated SMD solutions not only reduces overall board dimensions but also eliminates extra through-hole drilling steps, streamlining JLCPCB's automated SMT assembly process.
3- Minimize stress and EMI when placing components
Asymmetric placement of microvias or uneven distribution of copper planes can lead to mechanical stress, resulting in board warpage during sequential lamination or reflow soldering. Maintain a symmetrical layer stack-up and copper balance across all layers. To mitigate EMI in dense HDI designs, route high-speed differential pairs over continuous ground planes, keep microvias close to decoupling capacitors to minimize loop inductance, and utilize JLCPCB’s controlled impedance capabilities (e.g., 50Ω single-ended / 100Ω differential).
4- Minimize signal integrity issues by optimizing routing
HDI allows narrower trace widths and spaces (e.g., JLCPCB's 3 mil/3 mil standard), enabling higher signal density. However, tighter routing requires strict SI management. Minimize trace lengths, avoid 90-degree sharp turns, and use blind/buried vias to eliminate unused via stubs that cause signal reflections. For ultra-high-speed interfaces (such as PCIe or LPDDR), ensure proper reference plane transitions using ground return vias adjacent to signal microvias.
5- Choose stack-ups to minimize material costs
The layer count and lamination sequence dominate the fabrication cost of HDI PCBs. Complex structures requiring multiple sequential laminations (e.g., 3+N+3 or Any-Layer HDI) significantly increase thermal cycles and lead times. To achieve optimal cost-efficiency, opt for standard 1+N+1 (Type I) or 2+N+2 (Type II with staggered vias) stack-ups using JLCPCB’s standardized Prepreg (such as 1080 or 2116) and High-Tg FR-4 materials.
The Advantages of HDI PCB:
Improved Reliability: Due to their smaller depth-to-diameter aspect ratio (typically ≤1:1 compared to up to 16:1 for deep mechanical through-holes), laser microvias experience significantly lower Z-axis thermal expansion stress during lead-free reflow cycles. Combined with High-Tg FR-4 (Tg 170°C) laminates, microvias resist barrel cracking and deliver superior long-term interconnect reliability.
Enhanced Signal Integrity: HDI technology incorporates POFV (via-in-pad) and blind-via techniques that allow decoupling capacitors and high-speed ICs to be placed closer together, shortening critical signal paths. By terminating vias precisely on target inner layers, blind microvias eliminate the unused copper via stubs common in through-hole boards, dramatically reducing signal reflections, parasitic capacitance, and crosstalk at multi-gigabit speeds.
Cost-effectiveness: With proper DFM planning, HDI technology can reduce total system costs compared to conventional multilayer PCBs. By leveraging finer 3/3 mil routing and microvias, designers can often compress an 8-layer through-hole board into a 6-layer (1+N+1) HDI stack-up, cutting raw laminate area, layer counts, and overall enclosure size.
Compact Form Factor: Combining blind and buried vias frees up inner and outer routing channels that would otherwise be blocked by full-board through-hole barrels, enabling higher I/O pin density within ultra-compact footprints.
Overall, by using HDI technology, designers have the flexibility to place more fine-pitch components on both sides of the PCB. Laser microvias and via-in-pad processes unlock valuable PCB real estate, enabling shorter interconnects, faster signal transmission, and lower power loss.
Different Types of Vias in HDI PCB:
A via is a small conductive hole that connects multiple layers of an HDI PCB, allowing signals to pass between them. Depending on stack-up complexity and routing density, HDI designs utilize several specialized via structures:

● Through-hole via: These mechanically drilled vias extend from the top to the bottom layer of the PCB. In JLCPCB's HDI process, through-holes support diameters ≥0.15 mm with a maximum aspect ratio of 16:1.
● Blind via: These laser-drilled vias connect an outer surface layer to one adjacent inner layer without penetrating the entire board. JLCPCB supports 1st-, 2nd-, and 3rd-order blind microvias (0.075–0.15 mm diameter) that are electroplated with solid copper and planarized.
● Buried via: These mechanically drilled vias connect two or more inner layers and remain completely hidden inside the board. At JLCPCB (0.15–0.55 mm diameter, across a ≥0.30 mm inner core), buried vias are plugged with non-conductive resin and copper-capped.
● Microvia (Staggered, Stacked & Skip Vias): Laser-drilled holes with diameters ≤0.15 mm (6 mil) and an aspect ratio ≤1:1. Across multi-step HDI builds, microvias can be arranged as staggered vias (offset horizontally across sequential layers for lower cost and higher reliability), stacked vias (aligned vertically on the same axis via copper-filled planarization to save maximum space), or skip vias (spanning two layers, manufactured as stacked blind/buried structures).
HDI PCB Materials Selection:
The choice of dielectric material and glass-weave construction is pivotal in the design and manufacturing of HDI PCBs. Because HDI boards undergo multiple sequential lamination cycles and precision laser ablation, substrates must maintain dimensional stability, resist conductive anodic filament (CAF) growth, and match laser drilling requirements:
● Copper Clad Laminate (CCL): Copper-clad laminate materials involve the lamination of copper foil to one or both sides of a cured (C-stage) dielectric. For multi-layer HDI production, JLCPCB utilizes High-Tg FR-4 laminates (Tg 170°C, such as Shengyi or Nan Ya) with Anti-CAF performance and low Z-axis thermal expansion, ensuring layer-to-layer registration stability across repeated lamination and reflow cycles.
● Resin Coated Copper (RCC): Resin-coated copper materials consist of thin copper foil coated with a B-stage resin dielectric layer, which can be directly laminated onto the inner sub-composite. Because RCC lacks woven glass reinforcement, it enables ultra-clean UV or CO2 laser ablation for microvias in ultra-thin, high-density build-ups.
● PP (Prepreg): Often referred to as B-stage or bonding sheet, Prepreg comprises fiberglass fabric impregnated with partially cured resin. During the heating and pressing phase of PCB lamination, the resin in PP flows, adheres, and bonds the core with copper foil. In HDI stack-ups, fine glass-weave Prepregs (such as 1080, 2116, or 106/3313, with pressed thicknesses of 50–127 μm) are preferred over heavy weaves (like 7628) to prevent laser beam scattering and maintain a blind-via aspect ratio ≤1:1.
● Surface Finish Compatibility: Electroless Nickel Immersion Gold (ENIG) is the standard surface finish for HDI PCBs, providing a flat, oxidation-resistant surface essential for fine-pitch BGA soldering and reliable wire bonding.
Design Considerations for HDI PCBs:
The processes involved in the production of HDI PCBs are often different from those used with other PCB types. Here is what you need to know about HDI board production and key design considerations to keep in mind throughout the manufacturing process:
Sequential Lamination: In the lamination process, the PCB core is bonded with copper foil and prepreg layers under controlled heat and pressure, followed by drilling and plating. Unlike standard multilayer PCBs laminated in a single cycle, HDI boards undergo sequential lamination—1 cycle for 1st-order (1+N+1), 2 cycles for 2nd-order (2+N+2), and 3 cycles for 3rd-order (3+N+3) HDI—to build outer interconnection layers step by step. Because repeated thermal cycles challenge layer-to-layer registration, maintaining a symmetrical stack-up and using X-ray/CCD target alignment are critical to prevent board warpage.
Via Fill Types: Via fill types should always match your specific application and PCB requirements. Common industry via fill materials include electroplated copper, silver-filled paste, conductive epoxy, and non-conductive epoxy. In JLCPCB's HDI manufacturing, laser blind microvias are filled with solid electroplated copper to ensure high thermal and electrical conductivity, while mechanically drilled buried vias and via-in-pad through-holes are filled with non-conductive epoxy resin.
Via-in-Pad Process: The via-in-pad production process allows you to place vias directly inside flat SMT component pads by plating the via, filling it with copper or non-conductive resin, capping it, and finally planarizing and plating over it (known as POFV at JLCPCB). Via-in-pad is typically a 10- to 12-step process that requires specialized equipment and skilled technicians to guarantee a smooth, dimple-free solderable surface (with fill recess ≤25.4 μm).
Laser Drill Technology: Multi-layer HDI designs rely on high-precision UV or CO2 laser systems to form microvias, replacing conventional mechanical drills that cannot reliably execute holes below 0.15 mm (6 mil). Modern industrial laser production, such as JLCPCB’s standard HDI process, reliably produces microvias with finished diameters down to 0.075–0.10 mm (3–4 mil) and capture pads of 0.225–0.25 mm (9–10 mil), while maintaining a maximum depth-to-diameter aspect ratio of 1:1 to expose inner copper targets without thermal damage to underlying layers.
HDI PCB Manufacturing Process:
Successfully manufacturing an HDI PCB requires maintaining high dimensional control and precise chemical etching:
Line Width and Spacing: Broadly in chip packaging (such as mSAP or IC substrates), line width/spacing can shrink below 1 mil. However, for standard printed circuit board fabrication using subtractive copper processes, maintaining 3 mil / 3 mil (0.075 mm / 0.075 mm) represents the optimal balance between high routing density and robust manufacturing yield. Designing within these 3 mil constraints allows fine-pitch BGAs (e.g., 0.4 mm or 0.5 mm) to break out smoothly without triggering micro-shorting risks during fabrication—a standard tolerance naturally supported in JLCPCB’s HDI production line.
Via Size and Placement: According to IPC standards, microvias are defined as blind structures with an aspect ratio typically not exceeding 1:1, with diameters ≤0.15 mm (6 mil). In practical HDI applications, utilizing 0.075–0.10 mm (3–4 mil) copper-filled laser microvias paired with Via-in-Pad technology (such as JLCPCB's Plated Over Filled Via process, POFV) allows engineers to place vias directly on SMT pads, preventing solder wicking while completely eliminating trace fan-outs.
Layer Stack-up: HDI boards require sequential lamination to build dielectric and copper layers sequentially over a core. Standardized build-ups, such as symmetrical 1+N+1 or 2+N+2 (staggered microvias) using High-Tg FR-4 (Tg170) and universal Prepregs (e.g., 1080 or 2116), provide stable thermal performance and minimize board warpage during reflow.
Table: Standard HDI Manufacturing Capabilities and JLCPCB Specifications
| Parameter | Industry Baseline / IPC Standard | JLCPCB Standard Capability | Engineering Impact & Application |
|---|---|---|---|
| Microvia Hole Size | ≤0.15 mm (6 mil) | 0.10 mm (4 mil) | Supports tight breakout routing for 0.4 mm / 0.5 mm fine-pitch BGAs. |
| Microvia Capture Pad | 0.25 - 0.30 mm (10 - 12 mil) | 0.25 mm (10 mil) | Frees up surface real estate for higher routing density. |
| Min Trace Width / Space | 0.075 - 0.10 mm (3 - 4 mil) | 3 mil / 3mil (0.075 mm) | Enables precise impedance control and fine-line routing for high-speed signals. |
| Via-in-Pad Process | Resin Fill & Cap (VIPPO / POFV) | FPOV (Fully Plated Over Via) | Prevents solder wicking on SMT pads and enhances thermal dissipation. |
| HDI Stack-up Types | 1+N+1, 2+N+2, Any-Layer | 1+N+1, 2+N+2 (Stacked / Staggered) | Utilizes High-Tg FR-4 (Tg170) to balance thermal reliability and production efficiency. |
Cost Effective HDI:
While some consumer products shrink down in size, quality remains the most important factor for the consumer second to price. By leveraging HDI technology, designers can often transition an 8-layer conventional through-hole PCB into a 6-layer or 4-layer HDI PCB (such as a 1+N+1 structure) without compromising routing density or performance. Although HDI involves laser drilling and resin filling steps, the overall cost savings achieved through reduced raw laminate area, fewer layer counts, and improved signal integrity frequently offset the fabrication add-ons.
Stacked vs. Staggered Microvias Cost Efficiency: Staggered vias require fewer complex plating operations compared to stacked microvias. For optimal cost-efficiency at JLCPCB, selecting staggered microvia placement in 2+N+2 stackups is recommended unless board area constraints strictly enforce stacked vias.
To manage your HDI PCB costs effectively, consider the following factors:
1) Vias and Holes: Smaller vias require more precision and cost more. More vias also increase costs.
2) Stackup and Layers: Complex stack-ups and additional layers raise costs; aim for the most efficient number.
3) Materials: The choice of core materials (like FR4, metal) and surface finishes (like ENIG) affects costs.
4) Laminations: More laminations improve performance but increase cost and processing time.
5) Stacked vs. Staggered: Stacked vias cost more due to additional materials and time required.
6) Pad Size: Optimize pad size early to reduce costs.
7) Turnaround Time: Rush orders cost more; plan ahead for savings.
8) Supplier: Choose a supplier offering high-quality products at competitive prices to avoid future expenses.
HDI PCB Industries and Applications:
HDI technology is essential for modern electronics, enabling smaller, cost-effective devices without compromising performance. Key industries using HDI PCBs include:
Consumer Electronics: HDI PCBs are found in smartphones, laptops, wearables, smart home devices, and IoT gadgets, allowing for miniaturized yet powerful consumer tech.
Communications: Essential in devices like routers, switches, and semiconductors, HDI boards support electronic communication, digital media, and network infrastructure.
Automotive and Aerospace: HDI PCBs enable compact, lightweight components for cars and aircraft, supporting features like WiFi, GPS, cameras, and sensors, contributing to more efficient operation.
Medical Devices: Used in advanced monitoring, imaging, and surgical equipment, HDI technology enhances performance and reduces device size.
Industrial Applications: HDI boards power IoT devices and smart sensors in manufacturing, warehousing, and industrial operations, optimizing performance and connectivity.
FAQ about HDI PCBs
Q: What is the difference between 1st-order, 2nd-order, and 3rd-order HDI PCBs?
The HDI order corresponds to the number of sequential lamination and laser-drilling cycles used to build outer microvia layers. 1st-order HDI (1+N+1) features one laser microvia layer on each side of the core; 2nd-order HDI (2+N+2) adds two sequential microvia layers per side (staggered or stacked); and 3rd-order HDI (3+N+3) includes three sequential microvia layers per side. JLCPCB supports 1st-, 2nd-, and 3rd-order HDI across 4 to 24 layers.
Q: Can I use a 0.075 mm (3 mil) laser blind via through a 0.10 mm dielectric layer?
No. To ensure reliable copper plating inside the microvia, JLCPCB enforces a maximum blind-via depth-to-diameter aspect ratio of 1:1 (with supported blind-via dielectric thicknesses ranging from 0.05 to 0.127 mm). A 0.10 mm dielectric layer requires a laser blind via of at least 0.10 mm (4 mil) in diameter.
Q: How are blind and buried vias filled in JLCPCB's HDI process?
JLCPCB uses two distinct filling methods tailored to via geometry: laser-drilled blind microvias (0.075–0.15 mm) are solid copper-filled via electroplating and planarized, while mechanically drilled buried vias (0.15–0.55 mm) and via-in-pad through-holes are plugged with non-conductive resin and copper-capped (POFV).
Q: Which surface finish is recommended for HDI PCBs?
ENIG (Electroless Nickel Immersion Gold) is strongly recommended for HDI PCBs. Unlike HASL, ENIG provides an ultra-flat, uniform pad surface required for fine-pitch BGAs (≤0.5 mm), 0201/01005 components, and planarized via-in-pad structures.
Keep Learning
Comprehensive Guide to HDI PCBs: Design, Advantages, and Applications
Key Takeaways Core HDI Limits: Standard HDI uses 3/3 mil trace/space and 0.075–0.15 mm (3–6 mil, 4 mil default) laser microvias across 1st- to 3rd-order stack-ups for optimal yield and density. Via-in-Pad Benefits: Copper-filled laser microvias and resin-plugged, plated-over vias (JLCPCB's POFV process) on SMT pads eliminate trace fan-out and prevent solder wicking. Symmetrical 1+N+1 or 2+N+2 staggered microvias cut sequential lamination cycles and thermal stress. High Density Interconnect (HDI) print......
Blind vs Buried Vias: A Comprehensive Guide for PCB Design
A printed circuit board (PCB) is made up of layers of copper foil circuits stacked on top of each other, and the connections between different circuit layers rely on vias. If the holes drilled by a drilling machine or laser are left as is, they will not conduct electricity, because the surface of the original drilled hole is only resin, which is not conductive. Therefore, a layer of conductive material (usually copper) must be plated on the surface of the drilled hole. In this way, current propagates ......
Comparing High-Density PCB Stack-Up With Normal PCB
High-density printed circuit boards (PCBs)are not the same as simple PCBs. Do you know what the difference is? PCBs with a larger number of layers and a higher density of traces are known as HDIs. These are not as common because they are not used in small prototypes or hobby work, but for more professional application. One of the best examples of an HDI board with a complex stack-up that you can see—or might have—is the motherboard of your PC. HDI changes the story completely when it comes into the pi......
How to Optimize Layer Stack-Up in HDI PCB Boards
With the introduction of the HDI stackup, a cutting-edge technique in multilayer PCB design, PCB designers should be able to create increasingly complex, smaller boards in the years to come. Establishing your project's needs precisely is the first step in designing a PCB stackup. Determining the number of layers required is the first stage; this depends on the circuit's complexity, signal density, power distribution requirements, and if the design calls for RF or high-speed signals. In the late 1980s,......
Stack-Up Strategies for Effective HDI PCB Design
Whether you believe Moore's Law is dead or alive, the strong economic incentive to pack more processing power into ever smaller form factors is unlikely to abate any time soon. With the entry of the HDI stackup—a technology at the cutting edge of multilayer PCB design that promises to help PCB designers make smaller complex boards for years to come. The stack-up in a printed circuit board (PCB) design is a critical element that influences the board's performance, manufacturability, and reliability. In......
How Stacked Vias Enable Higher Density and Better Performance in HDI PCBs
Key Takeaways Stacked vias are a critical technology that enables higher routing density and superior performance in HDI PCBs. By vertically aligning microvias in a single column, often combined with via-in-pad designs, they dramatically reduce breakout area, shorten signal paths, lower parasitic inductance, and improve thermal conductivity compared to traditional staggered vias. While requiring precise sequential lamination, via filling, and strict design rules, stacked vias help designers reduce lay......