Annular ring and drill tolerances: what PCB fabs guarantee
What the annular ring is, and where fabs measure it
The annular ring is the copper left between the edge of a drilled hole and the edge of its pad. On paper it is simple: pad diameter minus hole diameter, divided by two. On a real board the drill wanders, the layers shift a little during lamination, and the ring ends up thinner on one side than the ring you drew.
The first trap is which hole diameter goes into the formula. Eurocircuits calculates the annular ring from the production tool size, not from the finished hole size in your data. For plated holes its tool is the finished size plus 0.10 mm, which leaves room for the copper plated onto the barrel wall. Non-plated holes are drilled at the finished size.
So a 0.30 mm via in a 0.60 mm pad has a 0.15 mm ring in your CAD tool and a 0.10 mm ring in Eurocircuits' check. The two numbers describe the same pad.
What IPC-6012 accepts on the finished board
IPC-6012 is the acceptance specification for rigid boards. For Class 2 it does not ask for a minimum ring width at all: it limits how far the hole may break out of the pad. Altium's summary of the standard gives these values:
| Class | External layers | Internal layers |
|---|---|---|
| Class 1 | Breakout up to 180° allowed | See the standard |
| Class 2 | Breakout up to 90° allowed | Breakout up to 90° allowed |
| Class 3 | 0.050 mm (2 mil) minimum ring | 0.025 mm (1 mil) minimum ring |
On external layers the ring is measured from the plating on the hole wall, on internal layers from the edge of the drilled hole. Minimum wall plating is 0.8 mil (about 20 µm) for Class 1 and 2 and 1 mil for Class 3.
These are acceptance numbers, what may be left after the process has eaten into the pad. The number you draw has to be larger. IPC-2221 builds the land size as L = a + 2b + c: hole diameter, twice the minimum ring, plus a fabrication allowance for drill wander and registration. Altium uses 0.20 mm (8 mil) for the allowance at IPC-2221 producibility Level C. For a 0.30 mm finished hole on an outer layer at Class 3 that gives 0.30 + 2 × 0.05 + 0.20 = 0.60 mm.
The design minimums the fabs publish
Each fab turns its own drill and registration accuracy into a minimum ring. From their pages, checked today:
| Fab | Minimum annular ring | Measured from | Other limits |
|---|---|---|---|
| EU Eurocircuits | Outer layers: 0.150 mm at pattern class 5, 0.125 mm at class 6 and 7, 0.100 mm at class 8 and 9 | Tool size (finished + 0.10 mm for PTH) | Inner layers 0.125 mm from class 6 up. Connected NPTH: 0.30 mm recommended |
| CN JLCPCB | 0.13 mm with 1 oz copper, 0.2 mm with 2 oz | Not stated | PTH pads: hole + 0.5 mm, minimum pad 1.0 mm. Via diameter 0.5 mm minimum on 1 and 2 layer boards, 0.45 mm on multilayer |
| CN PCBWay | 0.15 mm (6 mil), vias included | Not stated | Normal ring per side with 1 oz: 0.20 mm on PTH pads, 0.15 mm on via pads, plus 0.01 mm for each extra ounce |
The Eurocircuits values come from its classification table (2019 edition, PDF). The fab says it may reduce via holes by up to 0.30 mm to solve annular ring problems, and gives vias a maximum negative tolerance of 0.30 mm. A via that is too tight for its pad can therefore come back with a smaller hole instead of a stopped order. For oblong plated holes Eurocircuits asks for at least 0.30 mm of ring on the long sides and no breakout on the short sides.
The JLCPCB capabilities page lists several ring figures. Beside the 0.13 mm table value it says the ring of PTH holes is enlarged to 0.15 mm in production, and that the minimum ring around plated through hole pads is 0.25 mm. The safe reading is 0.25 mm for component pads and 0.13 mm as the lower limit for vias.
Hole size tolerance: the other half
The ring deals with where the hole lands. The size tolerance deals with how big it comes out. The three fabs publish:
- Eurocircuits: PTH ±0.10 mm up to 4.00 mm finished size and ±0.20 mm above. NPTH ±0.05 mm up to 4.00 mm and ±0.10 mm above.
- JLCPCB: PTH +0.13/-0.08 mm. NPTH ±0.2 mm.
- PCBWay: ±0.08 mm on the finished size of CNC drilled holes, with no separate PTH and NPTH figure on that page.
The pattern flips between fabs. At Eurocircuits the non-plated holes are the tight ones. At JLCPCB they are the loose ones: a 3.20 mm mounting hole can arrive anywhere from 3.00 to 3.40 mm. If a part depends on an exact mechanical hole, such as a press-fit pin or a locating peg, check that line of the capabilities page first.
Rounding adds a little more. Eurocircuits drills in 0.05 mm steps and rounds every size in your files to the nearest step, so a 31 mil hole (0.7874 mm) becomes 0.80 mm.
Hole position: the number nobody publishes
None of the three pages gives a hole position or layer registration tolerance. PCBWay refers you to customer service for it. That missing number is exactly what the ring has to absorb, and the fab has already built it into its ring minimum. Treat the published ring as the guarantee and leave a margin on top of it. Eurocircuits recommends not designing right at its classification limits, because of rounding and unit conversions in CAD output.
One via, three fabs
Take a tight via: 0.30 mm finished hole in a 0.55 mm pad. The CAD ring is 0.125 mm.
- Eurocircuits measures from the 0.40 mm tool, so the ring is 0.075 mm. That is below the 0.100 mm of pattern class 8 and 9.
- JLCPCB accepts the 0.55 mm diameter on any layer count, but 0.125 mm is under its 0.13 mm figure.
- PCBWay asks for 0.15 mm, so the pad is too small.
A 0.60 mm pad fixes all three: 0.15 mm of ring for JLCPCB and PCBWay, 0.10 mm (class 8) at Eurocircuits, and it matches the IPC-2221 Class 3 example above.
The free pad size and annular ring calculator runs the same check for any hole, pad and allowance, and gives the minimum pad for the hole.
Setting the rule in KiCad
KiCad custom design rules have an annular_width constraint (min, opt, max) and a hole_size constraint. A rule file for a fab that asks for 0.15 mm could look like this, where the second rule is taken from KiCad's own examples:
(version 1)
(rule "Fab minimum annular ring"
(constraint annular_width (min 0.15mm)))
(rule "Plated through-hole size"
(constraint hole_size (min 0.2mm) (max 6.35mm))
(condition "A.isPlated() && A.Hole_Size_X == A.Hole_Size_Y"))
DRC can only work with the hole size in your design, which Eurocircuits treats as the finished size. To make KiCad match a check done on the tool size, add half of the 0.10 mm oversize to the limit: 0.125 mm becomes 0.175 mm in the rule.
Look at the drill layer before you order
Off-centre holes in the output usually mean a drill file problem, not a fab problem: wrong units, a different origin or a missing file. Open the ZIP in the PCB Tools Gerber viewer, hide everything except the top copper and the drill layer, and click the drill layer to draw it on top. Then zoom in on the smallest vias.
Every hole should sit in the middle of its pad, and the ring on the vias should still be visible at this zoom. The guide to Excellon drill files explains how plated and non-plated holes are split, the via tenting and filling article covers the hole size limits for filled vias, and the Gerber checklist before ordering lists the rest of the checks.
Sources
- Eurocircuits, PCB design guidelines: drilled holes
- Eurocircuits, What is the production hole diameter?
- Eurocircuits, PCB design guidelines: classification
- Eurocircuits, Classification table (PDF, 2019 edition)
- JLCPCB, PCB manufacturing capabilities
- PCBWay, PCB manufacturing tolerances
- PCBWay, Annular rings
- Altium, Meeting standards: IPC-6012 Class 3 via sizes and annular rings
- KiCad, Custom rules help (constraints and examples)
Information in this article comes from the public documentation of manufacturers, standards bodies and software vendors as of the publication date and may have changed. Check current conditions with the company concerned before you order. Company and product names are trademarks of their owners; mentions are editorial, with no sponsorship or affiliate relationship. See the terms of use.
Check your Gerbers before you order
Load the ZIP or RAR your EDA tool exported and inspect every layer, drill and outline in the browser. Free, no account.
Open the Gerber viewer