Main Navigation
Blind and Buried Vias
Introduction - When are blind vias necessary
As component pitches get tighter on QFP and BGA type footprints, there comes a point where there is very limited space to fan out interconnect from the component to the remaining board circuitry. There are two approaches which the designer can take to get round this issue:
- Reduce the track and gap
- Use blind via techniques.
Reducing the track and gap is usually the first option, but there are limits to which most fabricators would wish to go. Although it is possible to go finer, the current industry standard is 4 thou (100micron) track and gap.
If there is no practical remaining reduction in track/gap, or the design is such that the interconnect simply cannot fan out on the surface layer, then blind vias are the answer.
What are blind vias ?
Blind vias are via holes which are formed to connect the outer circuit with inner layers, but DO NOT go through the entire board. Blind vias fall into three categories:
- Vias formed by using z axis controlled mechanical drilling.
- Vias formed by multiple lamination of micobonded portions of the final board.
- Vias formed by laser drilling.
Via formation and Design Criteria
Z axis - mechanically formed
These vias are formed by bonding the multilayer board in the usual fashion. When the panels are drilled , the blind vias are formed by only drilling part way through the board and stopping. This is the most cost effective means of forming a blind via hole.
Design limitations of this type of via:
The aspect ratio (via depth divided by via diameter) of the via must be less than or equal to 1 or the blind via cannot be plated. This is a universally accepted limitation due to the fluid dynamics involved. This obviously limits the number of layers that can be connected to the outer circuit. The smallest drilled hole is 0.20 (0.15 finished).
Microbond - multiple lamination
The microbond technique involves making a number of inner layers and then bonding them together to form part of a multilayer board called a microbond. This is then drilled, plated, etched etc as though it were a multilayer board in its own right.
Typically 2 microbonds are then laminated together (some times with additional print and etch layers in between). When laminated together, the holes which were "through holes" at the microbond stage, form the blind vias.
This allows interconnect much deeper into the board as the aspect ratio on a microbond via can be up to approx 7 because the hole is not blind when it is plated.
Design limitations of this type of via :
Because the holes have to be mechanically drilled, the drilled hole size must be greater than or equal to 0.2mm (0.15 finished).
Laser drilled microvias
When the drilled hole size required is 0.15mm (0.10mm finished hole) or below, lasers are used to drill the blind via holes.
Lasers are used to cut through the copper foil and the dielectric below, stopping at a "stop pad" on the layer 2. ( Ideally the stop pad should have a diameter 0.2mm greater than the drilled hole). The blind hole which is formed is then plated to form the blind via in a similar method to "1" above.
Design limitations of this type of via :
The aspect ratio of the blind hole can only be up to 1, ie the dielectric spacing plus the copper foil thickness between layers 1 & 2 can be no greater than the drilled hole diameter. Typically dielectric spacing are approx 60 - 70 microns, thus being suitable for drilled holes down 75 microns (assuming a half oz or thinner outer circuit foil).
