What is the annular ring formula?
Annular ring = (pad diameter − hole diameter) ÷ 2. A 1.4 mm pad on a 0.8 mm hole is 0.3 mm as drawn. The worst case subtracts half the upper hole tolerance and the full registration error: with +0.08 mm and 0.075 mm that leaves 0.185 mm. IPC-6012 Class 3 needs at least 0.05 mm on external layers.
Annular ring formula
Start from the ring you drew, then remove what the fab is allowed to take away. External rings use the finished hole, internal rings use the drilled hole.
AR = (D − H) ÷ 2 ARworst = (D − H − T⁺) ÷ 2 − E
- AR
- annular ring as drawn
- D
- pad diameter
- H
- hole diameter (finished for external, drilled for internal)
- T⁺
- upper tolerance of the hole diameter
- E
- registration: largest offset of the hole center from the pad center
The smallest pad that leaves a required ring b follows directly:
When breakout is allowed the limit is an angle rather than a ring. With r the largest hole radius and α the allowed breakout, the pad radius comes from the triangle of pad center, hole center and the point where the edges cross:
R = √(r² + E² − 2 r E cos(180° − α ÷ 2))
IPC-2221 uses a simpler land formula, with a fabrication allowance c in place of the tolerance stack:
L = a + 2b + c c = 0.4 mm (Level A), 0.25 mm (Level B), 0.2 mm (Level C)
Worked examples
Example 1: a 1.4 mm pad on a 0.8 mm hole
Drawn ring: (1.4 − 0.8) ÷ 2 = 0.3 mm. With +0.08 mm hole tolerance and 0.075 mm registration the worst case is 0.185 mm (7.28 mil), comfortably above the 0.05 mm Class 3 external limit.
Example 2: a 0.3 mm via with a 0.45 mm pad
Drawn ring: 0.075 mm. Vias are often specified with no upper hole tolerance, so the worst case is 0.075 mm − 0.075 mm = 0 mm, exactly tangent. That passes Class 2 but fails Class 3, which needs a pad of 0.55 mm at the same registration.
Example 3: the pad each class needs at JLCPCB tolerances
For a 0.8 mm hole at +0.13 mm and 0.075 mm registration, Class 2 at its 90° limit needs 1.04 mm, no breakout needs 1.08 mm, and Class 3 needs 1.18 mm. JLCPCB's own 2-layer rule asks for 1.3 mm for this hole, so its rule is the one that decides here.
Minimum via pad size by hole and IPC class
Worst-case stack with +0.08 mm hole tolerance and 0.075 mm registration. Internal uses a 0.1 mm drill oversize. Sizes in mm. Vias are often specified with no upper hole tolerance, as in Example 2, which makes the pad smaller.
| Finished hole | Class 1 ext | Class 2 ext | No breakout | Class 3 ext | Class 3 int |
|---|
| 0.20 | 0.318 | 0.400 | 0.430 | 0.530 | 0.580 |
| 0.30 | 0.409 | 0.498 | 0.530 | 0.630 | 0.680 |
| 0.40 | 0.503 | 0.596 | 0.630 | 0.730 | 0.780 |
| 0.50 | 0.599 | 0.694 | 0.730 | 0.830 | 0.880 |
| 0.60 | 0.696 | 0.793 | 0.830 | 0.930 | 0.980 |
| 0.80 | 0.893 | 0.992 | 1.030 | 1.130 | 1.180 |
| 1.00 | 1.090 | 1.191 | 1.230 | 1.330 | 1.380 |
| 1.20 | 1.289 | 1.390 | 1.430 | 1.530 | 1.580 |
Minimum annular ring at JLCPCB and PCBWay
What two common fabs state for plated through holes in 1 oz copper. These pages change, so check them before you order.
| Fab | Minimum ring | Recommended | Hole tolerance | Hole position |
|---|
| JLCPCB, 2 layers | 0.18 mm | 0.25 mm | +0.13 / −0.08 mm | ±0.075 mm |
| JLCPCB, multilayer | 0.15 mm | 0.2 mm | +0.13 / −0.08 mm | ±0.075 mm |
| PCBWay, standard | 0.15 mm | not stated | +0.08 / −0.08 mm | ±0.075 mm |
The PCBWay position tolerance is the normal-process figure from the Advanced PCB table on its capabilities page. Ask your fab for its real figure if you are designing close to the limit.
What this model leaves out
The worst case stacks both tolerances in the same direction, which is pessimistic but is the only bound a fab actually commits to. Breakout limits in IPC-6012 come with a second condition this page cannot compute: where a trace enters the pad, the junction has to keep a minimum width, so a teardrop or a wider neck is cheap insurance when you design close to the limit. For internal layers, a 2011 IPC APEX EXPO paper by Dudek and Hart gives 180° of breakout for Class 1 and 90° for Class 2. Altium's summary of IPC-6012 also allows 90° in Class 2, but lists a limit on pad-to-trace width reduction for Class 1, and it still recommends sizing those pads for no breakout. The calculator follows that advice, which is conservative; IPC-6012 is a paid document we did not read directly, so check your revision if the margin matters. Large holes also want more ring than the formula gives, since the pad has to hold solder and survive rework.
Glossary
- Annular ring (PCB)
- The band of copper around a plated hole, from the hole wall to the outer edge of the pad.
- Finished hole
- The hole diameter after plating, which is smaller than the drill bit.
- Registration
- How far the drilled hole can land from the center of the pad.
- Breakout
- A drilled hole that is partly outside its pad, measured as an angle of the hole edge.
- Tangency
- The limit where the hole just touches the pad edge, leaving a ring of zero at that point.
- IPC class
- The reliability grade of the board in IPC-6012: 1 general, 2 dedicated service, 3 high reliability.
Frequently asked questions
What is an annular ring in PCB design?
An annular ring is the band of copper around a plated hole, from the hole wall to the outer edge of the pad. The hole can land off center and come out at its upper tolerance, so the ring you can count on is smaller than the one you draw.
How do you calculate annular ring size?
Annular ring = (pad diameter − hole diameter) / 2. A 1.4 mm pad on a 0.8 mm hole has a 0.3 mm ring as drawn. Subtract half the upper hole tolerance and the full registration error to get the ring you can count on: 0.185 mm here.
What is the minimum annular ring for IPC Class 2 and Class 3?
An IPC Class 3 annular ring must be at least 50 µm (2 mil) on external layers and 25 µm (1 mil) on internal layers, per IPC-6012. Class 2 allows up to 90° of breakout on external layers, and Class 1 up to 180°, provided the junction with the conductor keeps its width.
What is annular ring breakout?
Breakout is when the drilled hole is not fully inside the pad, so part of the hole edge has no copper around it. It is measured as the angle of the hole edge outside the pad. Tangency is the point where the hole just touches the pad edge, and the remaining ring there is zero.
Is the annular ring measured from the drill or the finished hole?
External rings are measured from the finished (plated) hole wall, internal rings from the drilled hole. Internal rings are therefore computed with a larger hole, which is why the calculator asks for the drill oversize.
What via pad size do I need?
Size it for your class and your fab's tolerances. A 0.3 mm via held to a 0.075 mm position tolerance needs a pad of 0.55 mm for a Class 3 external ring, while JLCPCB's preferred 0.45 mm pad leaves a 0 mm worst-case ring, which is tangency.
Why does my fab ask for a bigger annular ring than IPC?
The fab rule is about the pad you draw, and it has room built in for its own tolerances, while the IPC limits apply to the finished board. JLCPCB recommends at least 0.25 mm on 2-layer boards, far above the 0.05 mm Class 3 limit, because it applies to the drawing before drill wander and plating.
What is the IPC-2221 minimum land formula?
L = a + 2b + c, where a is the largest hole, b the minimum ring and c the fabrication allowance. For a 0.8 mm hole with a 0.08 mm upper tolerance it gives 1.38 mm at Level A, 1.23 mm at Level B and 1.18 mm at Level C.
More free PCB tools
See all free electronics tools →
- PCB trace resistance calculatorResistance, voltage drop and power loss of a PCB trace from its width, length, copper weight and temperature.
- Online Gerber viewerDrop a Gerber zip to see every layer and a rendered board, and check the files are ready to order. Files never leave your browser.
- Online KiCad design checkerUpload a KiCad project to run KiCad 10 DRC, ERC and schematic parity, plus JLCPCB or PCBWay rules. Every finding links to its fix.
- PCB via current calculatorHow much current a plated via carries, plus its resistance and voltage drop, from drill size and plating.
- PCB trace width calculatorIPC-2221 trace width for a given current and temperature rise, with resistance, voltage drop and power loss.
- PCB impedance calculatorSingle-ended and differential impedance for microstrip and stripline traces from your stackup.
Design the whole board, not one number
ProtoFlow is free AI PCB design software: describe a circuit and get a schematic with real parts, PCB layout with an autorouter, SPICE simulation and Gerber files. Native KiCad, Altium and EAGLE import and export. Free on macOS, Windows and Linux.