Annular Ring in PCB Design: Minimums, Breakout & IPC Classes

Annular Ring in PCB Design: Minimums, Breakout & IPC Classes: RLX Solutions blog thumbnail

An annular ring is the copper that remains around a finished drilled hole in a PCB pad. Its minimum size must absorb drill and layer-registration error while preserving copper around the plated barrel. Tangency means the hole reaches the pad edge; breakout means part of the copper ring is lost.

RLX Solutions, a contract electronics manufacturer based in Concord (Vaughan), Ontario, checks pad and hole geometry in an engineer-reviewed DFM before fabricating bare boards to annular ring and IPC class requirements. For layout engineers, the practical rule is simple: do not size a pad so that the nominal ring equals the fabricator’s minimum. The nominal geometry also has to leave room for the real manufacturing variation that occurs before and during drilling.

What the copper ring controls in a plated hole

The ring width is the radial copper distance between the edge of a finished hole and the outer edge of its pad or land. For a centred circular hole and circular pad, the nominal value is:

Ring width = (pad diameter – finished hole diameter) / 2

That formula is useful, but it describes ideal geometry. A fabricated printed circuit board is built from imaged copper layers that must register to drilled holes. Lamination movement, artwork scaling, drilling position, hole-size tolerance and etching all influence how much copper remains around the final hole.

The ring matters because a plated through-hole or via is not just a drilled opening. The hole wall is plated, and that plated barrel has to connect reliably to the copper land on each layer where an electrical connection is required. If the hole shifts toward one edge of the land, the ring narrows on that side. If it reaches the edge, the geometry reaches tangency. If it moves farther, breakout occurs.

This is why pad diameter cannot be chosen from electrical connectivity alone. A pad that looks generous in CAD can become marginal after tolerance is applied across the full fabrication process.

For the drill technologies themselves, how mechanical and laser drilling form PCB holes covers how the hole is formed and why the drilling method changes with feature size.

Annular ring minimums in PCB design

A useful design minimum must be tied to the fabricator’s process capability, the layer on which the land sits and the finished hole geometry. Fabricators commonly publish rigid-board minimums of about 0.075 mm (3 mil) on inner layers and 0.1 mm (4 mil) on outer layers, but the governing values are the ones your fabricator states for your stackup.

Those numbers should be treated as fabrication limits, not as a reason to set every CAD pad to the exact same nominal ring. If a 0.30 mm finished hole is placed in a 0.50 mm pad, the nominal ring is:

(0.50 – 0.30) / 2 = 0.10 mm

That appears to meet a 0.10 mm outer-layer minimum when everything is perfectly concentric. But the design has no geometric reserve for positional movement. If the finished hole centre shifts 0.05 mm in one direction, the narrow side becomes approximately 0.05 mm while the opposite side becomes approximately 0.15 mm. The nominal calculation did not change, but the manufactured result did.

Now increase the pad to 0.60 mm around the same hypothetical 0.30 mm finished hole:

(0.60 – 0.30) / 2 = 0.15 mm

With the same hypothetical 0.05 mm centre shift, the narrow side is approximately 0.10 mm. That extra pad diameter gives the process room to move while retaining more copper on the worst side.

The exact allowance should come from the actual stackup, drill plan and fabrication review. What matters is the method: start with the finished hole, add the required retained ring, then add enough allowance for the manufacturing process rather than treating the hole as perfectly centred.

Tangency and breakout are registration outcomes

Tangency occurs when the edge of the drilled hole meets the edge of the copper land, leaving zero ring width at the point of contact. Breakout occurs when the hole extends beyond the land boundary. The difference is geometric, but the engineering consequence depends on where the breakout occurs and what copper must remain connected.

A via with a trace entering from one side is more sensitive if breakout cuts into the trace-to-pad neck. The risk is not simply that the pad looks incomplete. The concern is that registration error can remove copper from the current path between the trace, land and plated barrel.

This is why teardrops are sometimes used at trace-to-pad transitions. A teardrop adds copper where the narrow trace joins the larger pad. It does not correct poor drill registration, and it does not replace a valid pad-to-hole rule, but it can preserve more conductor width at a connection that would otherwise be vulnerable to edge loss.

Fabrication registration and assembly registration should also be kept separate. Breakout around a drilled pad is mainly a relationship between the hole and its copper land inside the bare board process. PCB fiducial marks for placement registration address the optical references used later by assembly equipment, which is a different alignment problem.

IPC Class 2 vs Class 3 changes the acceptance target

IPC Class 2 and Class 3 are not different formulas for pad diameter. They are different acceptance levels that change how tightly the finished board must control features such as retained copper and plated-hole quality. RLX fabricates bare boards to IPC-6012 Class 2 and Class 3, and Class 3 work carries tighter retained-ring, plating and cross-section expectations.

Decision factor IPC Class 2 IPC Class 3
Typical intent Dedicated-service electronic products High-performance electronic products where continued performance is required
Retained-ring acceptance More allowance for limited breakout under applicable acceptance criteria Tighter retained-ring expectations
Registration margin in layout Can support a less restrictive acceptance target, but still needs fabricator allowance Should be planned with greater reserve against tangency and breakout
Fabrication control Standard production controls for the specified class Tighter control of retained copper, plating and cross-section evaluation
Procurement instruction State the required class in the fabrication documentation State Class 3 clearly and keep the requirement consistent across drawing, notes and purchase documentation

The key design consequence is that a layout should be built around the required class before the board is released. It is risky to route a dense design around a marginal land geometry and then add a Class 3 note after routing is complete. The class affects the acceptance target, so it can change whether the existing pad and drill relationship gives the fabricator enough room.

The comparison of what changes between the two IPC acceptance classes covers the broader distinction between the two classes beyond drilled-pad geometry.

IPC-6012 fabrication acceptance for rigid PCBs explains how the specification fits into bare-board acceptance and why procurement documentation should state the required class consistently.

Design from finished geometry, not the drill centreline

The most useful ring-width calculation starts from the finished geometry the board must have, then works backward through process allowance. A CAD tool normally shows a hole centred in its pad, but a fabrication drawing is a manufacturing contract. It must describe what is required after drilling, plating and etching, not what an ideal centreline looks like on screen.

A practical design sequence is:

  1. Set the finished hole size. Use the electrical or mechanical requirement that determines the final opening.
  2. Identify whether the hole is plated. Plated through-holes and vias interact with the copper land and barrel; non-plated holes follow a different copper-clearance problem.
  3. Set the required retained ring by layer type. Inner and outer layers may have different fabrication limits.
  4. Add manufacturing allowance. Account for the fabricator’s drill and registration capability rather than assuming zero positional error.
  5. Check the trace entry. A ring may pass a radial rule while the trace neck remains vulnerable if the pad is crowded or necked down.
  6. Run the rule on every relevant layer. A multilayer via can have different land geometry on signal, plane and outer layers.
  7. State the IPC class in the fabrication notes. The acceptance target should not be left for interpretation after fabrication starts.

This sequence also prevents a common CAD mistake: setting one global via style for every location. Dense BGA escape regions, stitching vias, through-hole connectors and mechanical plated holes may have different finished-hole requirements and different room for pad growth.

Inner-layer ring geometry needs separate attention

Inner layers deserve their own review because the land is hidden after lamination and the final relationship depends on layer-to-drill registration. The outer pad can look well centred while an internal land is shifted relative to the same plated barrel.

Typical published minimums are 0.075 mm on inner layers and 0.1 mm on outer layers. That difference does not mean inner layers can be ignored. On a multilayer board, every electrically connected internal land has to survive the actual registration stack.

Consider a hypothetical eight-layer board using a 0.30 mm finished through-hole via. Board A uses 0.60 mm lands on all connected layers, giving a 0.15 mm nominal ring before manufacturing variation. Board B keeps the same eight layers and the same 0.30 mm finished hole but reduces selected internal lands to 0.45 mm, giving only 0.075 mm nominal ring.

Both boards have the same layer count and the same hole diameter, yet Board B places much more pressure on registration because its nominal inner-layer ring already sits at the typical published inner-layer minimum. Board A provides more geometric reserve. This is why layer count alone does not describe the difficulty of a multilayer build.

Drill size, aspect ratio and via architecture interact with the ring

Pad-to-hole geometry should be reviewed with the full via structure, not as an isolated rule. Mechanical drill size, laser-drilled microvia size and the aspect ratio of board thickness to hole diameter all set limits on how small a plated hole can be, so confirm those limits for the actual stackup.

A smaller hole does not automatically solve density. Reducing the hole may permit a smaller land, but it can also change drilling method, plating requirements or the via architecture used to connect layers. Blind, buried and microvia structures can alter the lamination sequence and the number of drilling and plating operations.

For high-density interconnect work, via tenting, plugging and filling options covers the surface treatment choices that become relevant once via location, pad geometry and assembly interaction are fixed.

A useful layout decision is therefore not “How small can the retained ring be?” It is “What hole and pad combination gives the required electrical connection, class acceptance and fabrication margin without forcing a more complicated via structure than the design needs?”

Plane layers and trace entries can fail differently

A signal land usually has a visible trace entering or leaving it. A plane connection may use a thermal pattern or a direct connection to a larger copper area. Both still depend on the plated barrel, but the geometry around the land differs.

On a signal layer, breakout toward the trace neck can remove part of the conductor path. Breakout on the opposite side may look less severe, but it still indicates that the hole-to-land registration has moved away from the intended geometry. On a plane layer, the concern shifts to whether the barrel maintains the required copper connection and whether the antipad and surrounding clearances remain valid.

This is why a single screenshot of an outer via cannot prove the whole multilayer structure is acceptable. The internal relationship has to be verified against the actual layer stack and the required acceptance class.

For layout review, check the smallest land on every connected layer, the direction and width of trace entry, plane connection geometry, and any layer-specific pad-stack overrides. Pad-stack edits made late in routing are a common place for one layer to end up smaller than the designer intended.

Do not use the fabrication minimum as the CAD default

A fabrication minimum is a boundary of process capability. A CAD default is a design choice that may be repeated hundreds or thousands of times across the board. Treating those two values as interchangeable can create a design that passes a rule check while leaving no room for normal process movement.

A better default is one that gives reasonable reserve for the board technology. Then use smaller lands only where density requires them and review those locations deliberately.

This matters most in areas such as:

  • dense BGA escape channels where pad diameter competes with routing space;
  • via fields with many repeated holes, where a marginal rule is multiplied across the design;
  • connector footprints where hole size is driven by the terminal but pad size is editable;
  • high-layer-count boards where internal registration has more interfaces to control;
  • mixed via architectures where through vias, blind vias and microvias are present on the same design.

If density forces the retained ring near a fabrication boundary, that is a design-for-manufacturing decision, not a cosmetic CAD cleanup.

Document the requirement so fabrication and procurement match

Pad-and-hole intent can be lost when the layout database, fabrication drawing and purchasing documentation do not state the same requirement. The manufacturer needs the hole data, copper data, stackup and class requirement to evaluate the finished geometry correctly.

For a bare PCB release, the useful package includes the manufacturing data, NC drill information, stackup documentation and fabrication notes. Common data formats are Gerber RS-274X, ODB++ or IPC-2581, supplied with NC drill files, a stackup document and fabrication notes.

Keep the documentation internally consistent. If the drawing states Class 3 but a procurement note requests Class 2, the acceptance basis becomes unclear. If the drill file and drawing disagree on finished size, the ring calculation can be wrong before fabrication review begins.

The same applies to pad-stack exceptions. If a small ring is intentional in a constrained area, make sure it is visible in the released data and reviewed against the actual process rather than assumed acceptable because the rest of the board uses larger pads.

Send Your Fabrication Files

Send your Gerbers or ODB++, drill files and fabrication drawing. Every board gets an engineer-reviewed DFM check before fabrication starts, under an ISO 9001:2015 certified quality system. Request a quote or send your files to sales@rlxsolutions.com.

Frequently Asked Questions

How do you calculate annular ring on a PCB?

For a centred circular pad and hole, subtract the finished-hole diameter from the pad diameter and divide by two. A 0.60 mm pad around a 0.30 mm finished hole gives a 0.15 mm nominal ring. That value is only the ideal CAD geometry. Manufacturing allowance still has to cover registration, drilling and other process variation.

What is annular ring breakout?

Breakout occurs when a drilled hole extends beyond the edge of its copper land, so part of the ring is missing. The engineering concern is greatest when the breakout reduces copper at a trace-to-pad connection or conflicts with the required acceptance class. Tangency is the boundary case where the hole reaches the pad edge without extending beyond it.

Is tangency acceptable for IPC Class 2?

Class 2 permits more retained-ring latitude than Class 3 under the applicable PCB acceptance criteria, but the allowed condition depends on the finished feature and the governing fabrication specification. Do not design by assuming tangency is always acceptable. State the required class and let the fabricator review the actual pad, hole, layer and connection geometry.

Does IPC Class 3 require a larger annular ring?

Class 3 applies tighter retained-ring acceptance than Class 2, so the layout generally needs more retained copper margin around plated holes. The exact pad size should not be chosen from a single generic number. It should be based on finished-hole size, layer type, fabrication capability, registration allowance and the Class 3 acceptance target for the finished board.

Should inner and outer annular rings use the same design rule?

Not necessarily. A fabricator may specify different minimums for inner and outer layers, and the manufacturing mechanisms are not identical. Published minimums are often around 0.075 mm on inner layers and 0.1 mm on outer layers. Your CAD rules should reflect the fabricator’s capability while still adding enough design reserve for the specific board.

Leave a Comment

Your email address will not be published. Required fields are marked *

Scroll to Top