HDI PCB Guide: Microvias, Stackups, and Manufacturing Choices

Six-layer HDI PCB cross-section with a blind microvia and a plated through-hole

An HDI PCB, or high-density interconnect printed circuit board, uses microvias with short layer spans and smaller connection pads. It also pairs these structures with fine-line geometry to create more routing space for dense components. When choosing HDI, first check whether component pins can fan out and which layers the signals must reach. Then compare via structures and the added manufacturing steps. Two boards with the same layer count can still use different connection structures.

How does an HDI PCB differ from a conventional multilayer PCB?

The first difference is the space used by each local connection. A multilayer PCB has several copper layers. Higher local connection density also requires vias, pads, and traces to fit in limited space and connect to the needed copper layers. For this reason, microvias and buildup structures can limit a layer transition to the span the connection needs instead of using a via that passes through the entire board.

For example, on a six-layer board, a signal that only needs to connect L1 to L2 can use either a through via or an L1 to L2 blind microvia. The through via still passes through L1 to L6, so routing on later layers must avoid that via and its required pads or clearances. The blind microvia ends at L2 and does not pass through L3 to L6. This compares two via structures for the same connection task, not boards with different total layer counts.

A via passing through a layer is not necessarily electrically connected to that layer's copper. Connected layers use pads. Nonconnected copper layers need clearance around the via. To assess the space it uses, check the opening and pads as well as the copper layers it crosses. The visible hole diameter alone does not show the limits on internal routing.

For a general view of how copper layers, cores, and prepreg form a multilayer stackup, see the multilayer PCB structure guide. HDI adds denser layer connections to these base structures. The choice still needs to preserve the required reference planes, dielectric thickness, and electrical connections.

When do you need HDI, and when can a conventional structure work?

Compare blind vias, microvias, or other stackup options when the component pad pitch and through-via pads leave no route for the required trace width and spacing. Fanout carries a component package pad to a point where routing can continue. It depends on the package pad array and the via and trace geometry.

Device fanout, pad pitch, and stackup jointly determine via selection. A BGA package can be evaluated with both through-via and blind-via options. If there is room to route between pads for through vias and an escape path remains for pads in the inner rows, a conventional structure may work. If vias and pads block connections to the inner rows, shorter layer spans or smaller microvias may free routing space. A BGA alone does not mean the whole board needs one HDI structure.

When evaluating an HDI PCB, compare the layer count and manufacturing steps together. Adding conventional signal layers may help routing, but it does not reduce the space occupied by existing through vias. Buildup microvias may free routing channels, but they change the sequence for hole formation, metallization, and lamination. The selected structure must complete the required connections and match the project's manufacturing requirements.

How do blind, buried, and microvias connect copper layers?

Through vias, blind vias, and buried vias are classified by their start and stop layers in the finished board and by whether the hole is visible from the outside. Microvias describe short-span hole structures and their formation method, so the terms can overlap. An L1 to L2 microvia can also be a blind via. The terms blind via and microvia do not describe mutually exclusive choices.

Six-layer cross-sections comparing a through via, mechanical blind via, buried via, and L1 to L2 blind microvia spans

Figure 1. A conceptual six-layer cross-section showing a through via, mechanical blind via, mechanical buried via, and outer-layer blind microvia. Layer numbers show the connection spans. The microvia is drawn in a thinner outer buildup dielectric. The diagram is not to scale.

Table 1. Connection spans and manufacturing implications of the via structures in Figure 1

Structure shownConnection spanRouting and manufacturing meaning
Through viaL1 to L6Passes through the board. Pads on connected layers and clearances on nonconnected copper layers must both be planned.
Mechanical blind via exampleL1 to L3Starts at an outer layer and stops at an inner layer. The span must match the process stage that forms the via.
Mechanical buried via exampleL2 to L5Has no opening on the finished board surface. It must be completed before later layers cover the core that contains it.
Outer-layer blind microvia exampleL1 to L2Spans only the outer buildup dielectric. The via bottom connects to the target pad on L2.

The target pad is the copper pad that receives a microvia at its bottom. The via must land accurately on that copper and form the required connection along its wall and at its bottom. To continue to deeper layers, microvias can be staggered or stacked at matching connection points. A staggered structure needs connection space on the intermediate layer. In a stacked structure, each upper via lands on the connection point below. The lower via fill and the flatness of its copper landing surface must be confirmed for the upper via design.

The layer spans of blind and buried via connections across layers can be compared pair by pair. The relevant microvia options include single, stacked, and staggered microvia structures. Both questions can arise within one stackup, but a general count of via stages cannot replace a precise via map.

What do via-in-pad, hole filling, and copper capping do?

Via-in-pad describes a location. It places a via inside a component pad instead of beside it, reducing the space needed by nearby routing. If that pad is also on a soldering surface, the pad surface and opening must be addressed. Moving a via to the center of a pad in the layout does not complete the design.

For an open mechanical through via inside a pad, solder may enter the hole during reflow and change the amount of solder available at the joint and the surface shape. VIPPO means via-in-pad plated over. It uses filling and copper capping to create a usable pad surface. Via filling, copper capping, and planarization have different roles. Filling treats the hole cavity. The copper cap covers the opening. Planarization reduces the local surface height difference.

The fill material and the electrical connection are separate questions. A resin-filled plated via can still conduct through its via-wall copper. A copper-filled microvia fills the hole cavity with copper. These structures have different purposes. For a stacked connection with another microvia above, the lower landing surface must work with the next via. For a via inside a component pad, the solderable surface requirements must also be specified.

Choosing between via-in-pad and VIPPO starts with the via location and soldering surface. The differences between resin filling, copper filling, and copper capping determine the required treatment. This article covers bare-board connections and surface conditions. Package pad requirements from assembly should be treated as design inputs.

How do buildup and via structures affect manufacturing steps and cost?

HDI manufacturing tradeoffs depend on which vias the structure uses, when they are formed, and how many buildup cycles it requires. A sequential buildup process adds dielectric and copper to a core in stages, then forms the corresponding layer connections. Therefore, even with six copper layers, a through-via multilayer design and a buildup microvia design can follow different manufacturing routes.

Figure 2 uses a 1+4+1 concept to show the sequence. First make the L2 to L5 four-layer core and its core vias. Then add the dielectric and copper for L1 and L6 on both sides. Form the outer microvias and complete metallization and the outer-layer pattern. Repeat stages only if the design calls for further buildup. The 1+4+1 notation describes the layer construction, not the full manufacturing sequence, which also includes making the core.

Illustrative sequential buildup from a four-layer core to a six-layer structure

Figure 2. A sequential buildup concept for a 1+4+1 construction. The core build, buildup, outer-layer hole formation, and metallization are shown in separate stages. Filling or copper capping depends on the selected structure.

This sequence explains why HDI should not be priced by total layer count alone. Buildup connections can add lamination, hole formation, and metallization steps. A stacked structure may also require lower-via filling. A via-in-pad structure may require filling and copper capping. These choices add specific processing steps and surface requirements. If a microvia structure reduces the number of other routing layers needed, it can also change the cost composition of the full board. Compare alternatives for the same connection task and acceptance conditions. Do not apply a fixed price multiplier.

Table 2. Manufacturing differences to compare when evaluating HDI candidates

Structure requirementManufacturing or control involvedWhat to compare
Add buildup connectionsRelated dielectric and copper layers, via formation, and metallization stepsAre these connections needed for the required fanout and layer transitions?
Use stacked microviasLower-via filling, copper landing surface, and flatness requirements for the selected structureAre the stack positions, layer spans, and fill requirements clear?
Use a mechanical via in a pad with resin filling and copper cappingResin filling and curing, followed by the required planarization and copper cappingDo the treatment area, soldering surface, and acceptance conditions match?

The buildup and via processing in HDI sequential lamination are a separate topic from the general multilayer manufacturing sequence. The overall sequence of inner-layer imaging, pattern transfer, and bare-board inspection is covered in the multilayer PCB manufacturing process. Keep these topics separate so a general multilayer process list does not stand in for HDI buildup steps.

How should you confirm stackup, via structures, and manufacturing requirements before release?

Before release, align the thickness and connection details for the same structure. Finished board thickness describes the full board. Individual dielectric thickness affects microvia depth. Whether a core thickness includes copper changes how that field should be read. These values can appear in the same stackup, but they are not interchangeable.

One local six-layer HDI project record specifies a 0.6 mm finished board thickness and a 0.17 mm copper-clad core. The first is a requirement for the finished board. The second describes a specific core component that includes copper. The 0.17 mm value is not the pure dielectric thickness inside the core. The 0.6 mm board thickness is not the drilling depth for an outer-layer microvia.

For each via type, confirm the depth and diameter definitions for via aspect ratio. A mechanical through via spans a different depth from a local outer-layer microvia. Drill diameter and finished hole diameter are also different inputs. After mapping these fields, check the manufacturing package in this order.

  1. List each via’s start and stop layers by copper-layer number. Distinguish mechanical vias from laser microvias, and mark staggered or stacked connections on the relevant layer pairs.
  2. Check the dielectric, core copper basis, hole diameter, and target pad in the same stackup revision. Confirm impedance requirements against the related cross-section.
  3. Specify which vias need filling, the fill material, and whether copper capping is required. State the surface conditions needed for soldering or for a connection above.
  4. Align the approved stackup, drill files, and manufacturing requirements to the same file revision. If the structure changes, update the affected layer pairs and dimensions.

Use the PCB DFM checklist before manufacturing to check file completeness and approval status. For a specific bare-board review, see HDI bare-board manufacturing and review. Submit the stackup and via requirements through the HDI project quote request.

Table of Contents

You Might Also Like