Blind & Buried Vias

Due to the increasing complexity of design structures blind vias and buried vias are increasingly used in high-density circuit boards (HDI).

A blind Via connects exactly one outer layer with one or more inner layers.

A buried via is a via between at least two inner layers, which is not visible from the outer layers. This technology allows more functionality in less board space (packing density).

For cost reasons, we recommend avoiding an overlap of blind and buried vias in the layer build-up! For example, avoid blind vias from L1 - L3 and simultaneously buried vias from L2 - L4.

Blind Via

Microsection of a blind via

Blind vias are used to connect one outer layer with at least one inner layer.

The holes for each connection level must be defined as a separate drill file.

The ratio of hole depth to drill diameter (aspect ratio) must be ≤ 1.

The smallest hole determines the depth and thus the max. distance between the
outer layer and the corresponding inner layers.

Your advantage: Whether laser or mechanically drilled, we always use the best / cheapest technology suitable for the job!


Design Parameters

Design parameters for printed circuit board blind vias.
Type Ø min. Ø max Via Pad Restring* Aspect Ratio
TypeBlind Via (mecanical)Ø min.100µmØ max0,4mmVia Pad400µmRestring*150µmAspect Ratio1:1 (rfq 1:1,2)
TypeBlind Via (laser)Ø min.75µmØ max0,4mmVia Pad225µmRestring* 75µmAspect Ratio1:1

*  circular


Optional: Via-in-Pad

Copper filled via

You can also place your blind vias within pads (via-in-pad).

The following applies:

  • Ø ≤ 100µm - copper filled (galvanic)
  • Ø ≤ 400µm - filled with non-conductive paste and overplated
  • Production according to IPC 4761 Type VII
  • Aspect Ratio 1:1

See also Via-in Pad: Via Filling.

Type Ø min. Pad size min. SS-clearance min. SS-bridge min.
TypeVia-in-Pad (standard)Ø min.200µmPad size min.400µmSS-clearance min.50µmSS-bridge min.100µm
TypeVia-in-Pad (extreme)*Ø min.100µmPad size min.300µmSS-clearance min.50µmSS-bridge min.100µm

* Note: Most economical are via-in-pad solutions with Ø ≥ 200 microns!

SS = solder-stop

Buried Via

Microsection of a circuit board buried via.

Buried vias are used to create connections of the inner layers, which have no contact with the outer layers.

The holes for each connection level must be defined as a separate drill file.

The ratio of hole depth to drill diameter (aspect ratio) must be ≤ 12.

The smallest hole determines the depth and thus the max. distance between the respective inner layers.

Generally: The larger you choose the annular rings on the inner layers, the more stable the connection.


Design Parameters

Design parameters for printed circuit board buried vias.
Type Ø min. Ø max Via Pad Restring* Aspect Ratio
TypeBuried ViaØ min.100µmØ max0,4mmVia Pad300µmRestring*150µmAspect Ratio1:10
TypeBuried Via (extreme**)Ø min.75µmØ max0,4mmVia Pad225µmRestring*75µmAspect Ratio1:12

* circular

** attention: higher costs