Annular Ring
Specification for designed hole/pad ratio:
The pad diameter is calculated as: Drilled hole dia. + production tolerance + (2 x annular ring) Drilled hole is at GPV Printca defined as: minimum hole + 0.2mm (except pressfit holes).
is defined as; twice the misalignment between any hole and the corresponding pad on the PCB. The misalignment is depending on construction type, panel size, material type, etc..
GPV Printca prod. tol. for 21" panels; price optimum
| Inner Layer | Outer Layers | |
| Double sided PCBs Multilayer, drilled through holes Buried vias, two-layers Blind vias, two-layers Blind or buried vias between several layers Multilayer with flexible inner layers Micro vias capture pad size |
NA +0.30 mm +0.40 mm +0.40 mm +0.50 mm +0.50 mm 0.35 mm |
+0.20 mm +0.20 mm NA +0.30 mm +0.30 mm +0.20 mm 0.35 mm |
GPV Printca prod. tol. for 18" panels
| Inner Layer | Outer Layers | |
| Double sided PCBs Multilayer, drilled through holes Buried vias, two-layers Blind vias, two-layers Blind or buried vias between several layers Multilayer with flexible inner layers Micro vias capture pad size |
NA +0.25 mm +0.35 mm +0.35 mm +0.45 mm +0.45 mm 0.30 mm |
+0.17 mm +0.17 mm NA +0.27 mm +0.27 mm +0.17 mm 0.30 mm |
Calculation of pad sizes, examples;
Pad size = drilled hole + GPV prod.tol. + (2 x annular ring)
Example 1:
Pad size for ESA PSS-01-710 spec. PCB, for a 0.9mm ±0.1mm Component hole, designed for minimum pad sizes (higher costs):
Prod. tol. are 0.2mm on outer layers.
(drilled hole will be min. hole + 0.2mm = 0.8 + 0.2 =1.0mm)
Annular ring demand for C-side is 250µ, S-side is 400µ.
C-side:
1.0 + 0.20 + (2 x 0.25) = 1.70mm
S-side:
1.0 + 0.20 + (2 x 0.40) = 2.00mm
Example 2:
Pad size for a MIL-P-55110D spec. PCB, to a 0.9mm ±0.1mm component hole, designed for price optimum production. Prod. tol. are 0.4mm on inner layers and 0.3mm on outer layers acc. To above fig. (drilled hole will be min. hole + 0.2mm = 0.8 + 0.2 =1.0mm) Annular ring demand for outer layers are 130µ, inner layers 51µ.
Pad size, outer layers:
1.0 + 0.30 + (2 x 0.130) = 1.56mm
Pad size, inner layers:
1.0 + 0.40 + (2 x 0.051) = 1.52mm
Example 3:
Pad size for a industrial std. spec. PCB, (e.g. the danish Perfag3) for a 0.9mm ±0.1mm component hole, designed for price optimum production. Prod. tol. are 0.4mm on inner layers and 0.3mm on outer layers acc. To above fig. (drilled hole will be min. hole + 0.2mm = 0.8 + 0.2 =1.0mm) Annular ring demand for outer layers are 50µ, inner layers 10µ.
Pad size, outer layers:
1.0 + 0.30 + (2 x 0.05) = 1.40mm
Pad size, inner layers:
1.0 + 0.40 + (2 x 0.01) = 1.42mm
Power- & ground-planes
On ground and power planes the clearance pads are the inner layer areas free of copper surrounding the finished hole diameters. It is calculated by measuring the difference between the specified drill diameter and the corresponding clearance pad diameter.
When designing planes without non-functional pads, the openings in the planes must be as follows: Opening = required pad size + (2 x demand for isolation) Ex: Openings in planes with conditions from example 2 above. Inner layer required pad size was 1.52mm. If demand for isolation is 6 mils (0.15mm) from holewall to plane, the openings must be designed: 1.52mm + ( 2 x 0.15mm) = 1.82mm
If the plane layer design leaves strips of copper between clearance pads, a minimum of 0.1mm is required between clearance pads to avoid causing shorts due to resist lifting and redepositing.
Remove copper from planes, minimum 0.4mm inside contour, and please remove copper 2.6mm outside contour. (Then our router lasts longer and the edge quality would be optimised)
If planes are designed with 70µ copper we do not recommend to remove non-functional pads on the plane layers.
ASPECT RATIO
The maximum board thickness divided by the smallest selected drill diameter. The maximum board thickness is the calculated thickness over copper before plating. Additional thickness caused by plating, hot air levelling, or soldermask has no impact on aspect ratio.
 |
1:6 ratio is std. From 0.4mm dia. holes, ratio 1:8 can be processed. For depth drilled holes and micro vias, the ratio is 1:1. |
TENTING OF UNPLATED HOLES
For improved locational accuracy of unplated holes, it is preferred to drill them during the initial plated through hole drilling set-up. In order to avoid plating of etch resist into these holes., it is required that the unplated holes be tented with dry film during the outer layer imaging process, overlapping the hole edge for a minimum distance. Before the etching process, this tent is removed. This allows the removal of copper from the hole walls during the consequent etching process. Maximum hole diameter to be tented is 5mm, tenting dia. is hole dia. + 0.8mm. For holes below 3mm, the tenting dia. is hole + 0.5mm.