{"id":355,"date":"2026-09-09T09:00:00","date_gmt":"2026-09-09T09:00:00","guid":{"rendered":"https:\/\/rlxsolutions.com\/blog\/blind-buried-microvias\/"},"modified":"2026-09-09T09:00:00","modified_gmt":"2026-09-09T09:00:00","slug":"blind-buried-microvias","status":"publish","type":"post","link":"https:\/\/rlxsolutions.com\/blog\/blind-buried-microvias\/","title":{"rendered":"Blind, Buried & Microvias: Types, Uses & Manufacturing Cost"},"content":{"rendered":"

Blind vias connect an outer layer to one or more inner layers, buried vias connect only internal layers, and microvias are small laser-drilled connections used for dense interconnects. Each changes the PCB fabrication<\/a> sequence and therefore cost. RLX Solutions<\/a>, a contract electronics manufacturer in Concord, Ontario, reviews via architecture against the proposed stackup before a board is quoted.<\/p>\n

For an engineer, the useful question is not simply which via occupies the least board area. It is which interconnect structure provides the routing access you need without adding unnecessary lamination, drilling, filling or plating operations. For the full picture, see our PCB Manufacturing Guide<\/a>.<\/p>\n

Blind, buried and microvias solve different routing problems<\/h2>\n

A conventional plated through-hole (PTH) via passes through the complete printed circuit board stack. It is mechanically drilled, plated and electrically available across the board thickness. That simplicity makes it a useful baseline for understanding the alternatives.<\/p>\n

A blind via starts on an outer layer but stops at an internal layer. A buried via starts and ends between internal layers, so neither end is visible on the finished board surface. Both structures free routing space that a full-depth via would otherwise consume.<\/p>\n

A microvia describes a small laser-drilled interconnect rather than simply another layer-access category. Microvias can form blind structures, and multiple microvias can be stacked or staggered to reach farther through a high-density interconnect<\/a> (HDI) stackup.<\/p>\n\n\n\n\n\n\n\n\n\n
Decision factor<\/th>\nBlind via<\/th>\nBuried via<\/th>\nMicrovia<\/th>\n<\/tr>\n<\/thead>\n
Layer access<\/td>\nOuter to inner<\/td>\nInner to inner<\/td>\nTypically short layer transitions<\/td>\n<\/tr>\n
Primary routing benefit<\/td>\nFrees deeper layers from a full-depth via<\/td>\nPreserves outer-layer routing area<\/td>\nSupports dense component escape and fine routing<\/td>\n<\/tr>\n
Drilling method<\/td>\nDepends on geometry and build<\/td>\nBuilt into internal subassembly<\/td>\nLaser drilled<\/td>\n<\/tr>\n
Stackup consequence<\/td>\nSequential lamination<\/td>\nInternal drilling and plating before final lamination<\/td>\nHDI build sequence, potentially repeated<\/td>\n<\/tr>\n
Typical cost pressure<\/td>\nAdded process stages<\/td>\nAdded internal processing<\/td>\nLaser drilling, fill\/cap and repeated HDI cycles where required<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

The distinction matters because two vias that look similar in a CAD view can require very different fabrication sequences.<\/p>\n

Blind vias trade fabrication steps for routing area<\/h2>\n

Blind vias are useful when a signal must leave an outer-layer component pad but does not need electrical access through the complete PCB thickness.<\/p>\n

Consider an 8-layer board where a component on Layer 1 needs to connect to a signal route on Layer 3. A through via would pass from Layer 1 through Layer 8 even though Layers 4 through 8 do not need that connection. Its barrel and clearance requirements can consume routing space on every intervening layer.<\/p>\n

A Layer 1 to Layer 3 blind via terminates at Layer 3. The deeper layers remain available for routing, planes or other structures.<\/p>\n

The manufacturing consequence is more significant than the CAD geometry suggests. Blind vias on multilayer stackups require sequential lamination. The relevant layers must be drilled and plated at the appropriate point in the build before later portions of the stack are completed.<\/p>\n

That sequence creates an important design rule: specify blind vias as part of the stackup architecture, not as a late routing fix.<\/p>\n

Aspect ratio still matters<\/h3>\n

A blind hole has both diameter and depth. The relationship between them affects whether plating can form reliably along the hole wall.<\/p>\n

Suppose a proposed blind via has a 0.20 mm finished hole through a 0.40 mm dielectric structure. Its nominal depth-to-diameter ratio is 2:1. Change the same hole to a 0.60 mm depth and the ratio becomes 3:1.<\/p>\n

That change may look minor on the layout. Fabrication sees a substantially deeper feature relative to its opening.<\/p>\n

For mechanically drilled structures, the complete board stack also matters. A 0.20 mm hole through a 2.0 mm board represents a 10:1 aspect ratio. Via diameter, finished board thickness and the actual layer span therefore belong in the same design conversation.<\/p>\n

Buried vias move interconnect density inside the board<\/h2>\n

Buried vias are useful when internal signal layers need to connect without consuming pad and clearance area on the outer surfaces.<\/p>\n

Imagine a 10-layer circuit board with a connection required only between Layer 3 and Layer 6. A through via could make that connection, but it would also occupy space on Layers 1, 2, 7, 8, 9 and 10.<\/p>\n

A Layer 3 to Layer 6 buried via confines the structure to the layers that need it.<\/p>\n

The trade-off is process sequence. Those internal layers must be processed as a subassembly, drilled and plated before they are incorporated into the final laminated stack. Registration through subsequent lamination stages becomes part of the manufacturing problem.<\/p>\n

This is why buried vias should earn their place in a design. They can solve genuine routing constraints, but using them where an ordinary through via would work adds manufacturing operations without creating electrical value.<\/p>\n

One practical use is preserving surface area under dense packages. Another is keeping internal interconnections away from surface routing channels needed for component escape.<\/p>\n

Microvias change the routing strategy under fine-pitch components<\/h2>\n

A microvia is a laser-drilled interconnect used for short layer transitions. It becomes particularly useful when mechanical drilling and conventional capture pads consume too much area around a dense ball grid array (BGA) or similar package.<\/p>\n

Laser drilling supports smaller hole geometry because material removal is performed differently from mechanical drilling. The hole is then metallized to create the electrical connection.<\/p>\n

For example, consider a 0.5 mm-pitch BGA on Layer 1. If the escape strategy cannot fit a conventional through-via pad between neighbouring lands while maintaining the required copper geometry, a Layer 1 to Layer 2 microvia can move the signal to the next routing layer without sending a large drilled barrel through the full stack.<\/p>\n

A 0.10 mm laser-drilled microvia is one available fabrication geometry for this type of HDI structure. Stacked and staggered configurations can extend the connection across additional layers when the stackup requires it.<\/p>\n

Stacked and staggered microvias are not equivalent<\/h3>\n

A staggered structure offsets successive microvias. For example:<\/p>\n