TechnoService

Remember to maintain proper spacing of conductive components and milling line, which will secure the circuits against breakdown to cover or other components on the PCB edge. Maintaining proper spacing will provide insulation of conductive components.
To determine the spacing, allow for the minimum values:
a) minimum ground - PCB edge spacing (milling line) is 0.20 mm (8 mils),
a) minimum track - PCB edge spacing (milling line) is 0.25 mm (10 mils),
a) minimum ground, track and pad - PCB edge spacing in inner layers is 0.20 mm (8 mils).
Minimum ground and track - scoring line spacing, depending on laminate thickness are shown in the table below:

PCB plating method is specified by the Client, although it is not arbitrary, since the plating methods have some limitations. Tin plating is more cost-effective, although the quality compared to gold plating is lower. It can easily be made for less complicated printed boards. For more complex designs, gold plating is recommended. In many cases, there is no choice, for technical reasons some of the printed boards cannot be tin plated.
Gold plating is made for circuits with:
a) BGA,
b) clearance or track width 100 µm (4 mils),
c) pads ≤ 200 µm (8 mils) for one-sided SMD,
d) pads ≤ 300 µm (10 mils) for two-sided SMD,
f) blind vias.
The limitations apply to circuits made of <0.8 mm thick laminate.
Gold plating shall be used if necessary (technical considerations) and if high resistance to external factors, even pad surface and perfect soldering capabilities are required. By selecting this plating method, we make sure that the nickel layer protects copper plating against dissolving during installation, which must be adapted to gold, and allowed for during design calculations.

Position and size of gaps and holes depends on the design, although some limitations apply. Remember:
a) maximum depth of blind via is max. 75 % of the drill diameter for holes 0.3 mm to 1.0 mm in diameter,
b) for holes with >1.0 mm diameter, the maximum blind via depth equals the drill diameter.
Other values will not provide suitable plating and will cause issues with electric connection between layers.

Proper hole design must allow for all limitations. A minimum hole diameter for selected laminate thickness and pad size must be maintained. Minimum hole diameters are specified in table below:
Laminate thickness (mm)
Minimum allowable PTH diameter (mm)

For printed boards with blind vias, maximum blind via depth may not exceed 75% of drill diameter.
Plated through hole diameter is reduced by 0.1 mm after the copper layer is applied. Standard tolerance of hole diameter is +/- 0.1 mm. Specific tolerances shall be detailed at placing an order. It is not possible to fabricate circuits with hole dimension tolerance +/- 0.00 mm.
Plating method does not affect hole diameters. Printed boards with blind vias cannot be tin plated. Gold plating is required.

Printed boards with blind vias have additional holes, connecting selected layers of a multi-layer PCB. The holes do not go through the PCB, hence the name - blind via. By drilling holes to the depth of a copper layer inside the printed board, an electrical connection between specific layers is obtained after plating. It improves printed board capabilities and applicability. A printed board of this type is presented below:

When preparing a design with blind vias, remember that the printed boards with blind vias must be gold plated (not tin plated), and the maximum depth of blind vias may not exceed 75% of a drill diameter. For 0.4 mm drill, the maximum blind via depth is 0.3 mm. The printed boards designed in accordance with those requirements may be fabricated without limitations.

Standard minimum pad size (annular ring) for multi-layer printed boards:

Method for calculation of a correct AR size:

(a)

Hole, pad (a) and anti-pad (b) diameters

For 4-layer PCB, minimum distance D-d = 0.4 mm (16 mils), i.e. annular ring size is 8 mils. For 6 and 8-layer PCB, minimum distance D-d = 0.5 mm (20 mils), i.e. annular ring size is 10 mils.
Printed boards with 6-mils ring for 4-layer PCB and 8-mils rings for 6-layer PCB are also available. The solution requires special, non-standard design, and the resulting PCB is much more intricate.