CNC Drilling vs. CNC Boring: When to Add a Finishing Pass

Drilling opens the hole; boring cuts its existing wall

A conventional drill feeds along the hole axis and cuts across the end of its tool. Its diameter establishes the nominal opening, subject to the actual drill, holder, workpiece, entry and depth conditions. Some drill designs can enlarge a prepared opening, but their axial cutting method is still drilling. Sandvik Coromant lists hole diameter, depth and required quality as the first drilling considerations. [1]

A boring tool cuts material from the wall of an existing hole. That opening might have been drilled, milled, cast or forged; a solid blank needs an opening before an ordinary boring tool can work inside it. Rough boring removes more of the wall to prepare it for a final pass. Fine boring then works the remaining wall to the required size and surface condition when the setup and tool can support it. [2] [3]

On a machining center, a rotating boring head can work on a stationary clamped housing. On a lathe, a boring bar can cut the inside of a rotating component. Those machine arrangements differ, but both require a pre-existing opening and enough access for the tool. The broader machining process guide covers the neighboring process families; the choice here is specifically what should happen to one hole after it has been opened.

A drilled hole can already be the finished feature

Begin with what the hole does in the assembly. A bolt clearance hole must let the specified fastener pass and let the parts assemble in the intended position. A fluid passage must meet its flow, wall and cleanliness requirements. Neither automatically needs a fine-bored wall. A pin or bearing seat asks a different question: the mating component may depend on the internal diameter and its relationship to other part features, not merely on the existence of an opening.

For each hole, compare the actual drilled result with the drawing’s complete requirement. A drill-only route is reasonable when the result passes the specified diameter limits, location, usable depth, surface and edge condition. It is not enough to say “the drill is nominally the right size”; a nominal drill diameter is a tool designation, while an accepted hole is a measured part feature. The entry and exit surfaces, chip removal and unsupported tool reach can affect what the drill leaves. Sandvik’s drilling guidance distinguishes bolt-clearance holes from good-fit holes and other functions for this reason. [1]

The opposite shortcut is to bore every hole on a “precision” drawing. That adds a second cutting and verification step without improving a clearance feature whose existing result already meets its own requirement. If position relative to a datum is the issue, first find out whether the drilled hole actually fails that location requirement; do not substitute a surface-finish operation for a location decision. The CNC drilling machine guide addresses machine and hole-pattern choices; the present decision is whether each produced hole needs further work.

Choose the route by the unfinished characteristic

The following routes share the same comparison basis: what opening exists, which finished feature matters, and what the proposed extra operation can actually change. They are alternatives for a stated condition, not a ranking from cheap to expensive or rough to precise.

The table does not imply that a reamer, boring head or milling cutter is the only possible tool for every geometry. It identifies which operation merits evaluation once the functional requirement is known. A tool supplier’s specific application data and the part’s actual acceptance criteria then narrow the selection. [2] [4] [5]

Boring needs an opening, material to cut and full-depth access

A planned finish bore has a center axis and final diameter. The starter hole must be smaller at every relevant section, with enough remaining wall at its thinnest side for the intended rough and finish passes. Its entrance also has to admit the tool body, and the tool must reach the full functional bore length without colliding with shoulders or adjacent features. A nominally adequate opening at the mouth is not proof of adequate stock deeper in the part.

Suppose a housing has a rough opening for a bearing seat. If the wall is irregular or the amount of material to remove is substantial, a rough-boring operation can establish a more uniform pre-finish opening before fine boring. If the opening is already suitable for the finishing tool, a separate rough pass may add no value. Sandvik’s boring guidance separates rough removal from the final small-cut operation; it also asks designers to consider depth, tolerance, position, straightness, interrupted walls, fixture stability and tool extension. [2] [3]

Long reach and a flexible tool can compromise the very diameter or finish the second operation is intended to improve. The bore can also contain a cross-hole or step that interrupts the cut. Those are tool-selection and setup questions, not reasons to write “bore to size” on a drawing and assume the shop can achieve it. Conversely, a solid starter hole is not always necessary: a cast core or previously milled opening can supply the entry, provided its condition and position leave a machinable wall.

An off-center starter hole can leave too little wall to correct

Boring can establish a new finished axis relative to the chosen setup only by removing material. It cannot fill a region where the initial opening already lies outside the intended finished cylinder. This is the practical limit behind the vague instruction to “bore out” a misplaced hole. Measure or otherwise characterize the existing opening against the intended datum-related axis before deciding that a finish pass can correct it.

For two ideal, straight circular holes with parallel axes, let D_f be the required final diameter, D_s the starter diameter and e the offset between their centers at one section. The least radial material available there is (D_f − D_s)/2 − e. This is a geometric check, not a recommended cutting allowance. With a 30 mm final bore, 28 mm starter hole and 0.6 mm offset, the least stock is (30 − 28)/2 − 0.6 = 0.4 mm. Change only the offset to 1.2 mm and the result becomes −0.2 mm: the starter opening crosses the proposed final boundary on one side, so no boring pass can leave a complete 30 mm cylindrical wall on that target axis.

A positive result answers only “is there material everywhere in this ideal section?” It does not prove that the tool can make a stable cut, that enough finish allowance remains, or that the hole is straight along its depth. A rough cast or drilled opening may vary in size and center down the part. Evaluate the worst relevant section, the selected tool’s minimum workable cut, final wall thickness and the actual locating datums. If those do not work, the design or blank may need revision; simply adding another finish pass cannot replace absent stock.

Reaming and circular milling solve different hole problems

Reaming is a finishing choice when a prepared hole has a satisfactory axis and enough suitable stock for the selected reamer. It can improve size and finish under the right setup, but Sandvik Coromant explicitly says reaming should not be expected to correct position or straightness errors in the pre-machined hole. The offset between that hole and the reamer should be kept small to avoid vibration. If locating the final bore axis relative to the housing datums is the decisive problem, a reamer following the existing opening is not a substitute for a properly planned boring or milling route. [4]

Circular or helical milling uses a smaller rotating cutter traveling around the intended hole boundary. That can be useful when the cutter can enter, clear the center and reach the wall with a workable path; it can also be a way to widen an accessible opening. Its programmed path offers flexibility in diameter, but the finished result still depends on cutter deflection, setup and verification. The drilling versus hole milling guide covers the entry and toolpath mechanics in detail. This article only needs the boundary: a circular-milled opening may replace or precede a boring pass, but calling either operation “more precise” without the finished requirement and process conditions is not a decision. [5]

A spotface is more localized. If the bolt head needs a flat land on a rough or angled exterior surface, cut that seating land around the hole; do not enlarge and finish the whole cylindrical wall solely for this need. A counterbore or stepped hole may instead require its own diameter and depth, and a true bearing seat may require continuous controlled wall geometry. These features can appear together, but their acceptance is different. BIG DAISHOWA’s back-spotfacing tooling illustrates a bolt-seat operation distinct from full-length hole-wall finishing. [6]

A housing with clearance holes and a bearing seat

Consider a housing that bolts to a plate and supports a bearing. Its four bolt holes primarily provide passage and assembly clearance. If drilling leaves accepted sizes and positions, they are finished without boring. If a bolt head must sit flat on a local cast surface, a spotface can prepare that land while the drilled clearance wall stays as it is. The need for a flat seat does not turn the hole into a close-fit bore.

The central bearing seat has a different job. Its diameter and form affect the bearing fit, while its axis may need a defined relationship to the mounting face and other locating features. A drilled or cast opening can provide access. Boring is worth adding if the initial opening leaves continuous stock and the setup can establish the required finished axis and wall. If the initial opening is too far off-center, the geometry check above can rule that route out before any finish-boring promise is made. A larger finished diameter might restore the missing stock geometrically only if the resulting fit and outside wall remain acceptable. Otherwise, the blank or an approved bore-axis and datum design must change.

This example does not imply that every bearing seat must be bored. A correctly prepared hole might be reamed where its existing axis is adequate and the tool/application suit it. A larger, accessible seat might be milled. The choice is made from the finished fit and geometry, not from the label “bearing housing.”

Inspect size, form and position as separate results

A finishing operation should be verified against the characteristic that justified it. For a bearing seat, record the specified internal diameter where the bearing actually engages. If roundness, straightness or taper matters, the inspection method needs enough sections and orientations to reveal the relevant form, rather than one reading at the entrance. Mitutoyo’s bore-gage guidance explains that an internal gage measures diameter and can reveal ovalness and taper when applied appropriately; an individual gage reading does not establish every aspect of the cylinder. [8]

Size alone does not locate the axis. If the bore’s position or orientation relative to the mounting face controls assembly, set up and inspect those datum relationships as the drawing specifies. ASME Y14.5 provides the language for dimensions, datums, position and form, but its public scope does not assign a tolerance to this housing. The drawing must do that. A bore can be within diameter yet misplaced; a correctly located axis can still have an unacceptable diameter or wall form. The CNC machining tolerances guide goes deeper into those controls. [7]

Specify the shortest route that delivers the accepted hole

1. Define the finished feature. State the hole’s function, finished diameter and depth, and any form, surface, edge or datum relationship that affects assembly. A clearance hole and bearing seat need different answers.
2. Assess the actual starting state. Establish whether the part starts solid, predrilled, milled or cast. For a planned finish bore, check the least remaining stock around the intended axis and the tool’s full-depth access.
3. Choose creation and finishing separately. Drill alone where it passes; add boring where a controllable finished wall or axis is needed and feasible. Use reaming only with an acceptable pre-hole axis; evaluate circular milling or a local spotface where they address the actual geometry.
4. Verify the specified outcomes. Check diameter and relevant form at the functional length, then check datum-related location or orientation separately. Do not add an operation whose result is neither required nor inspected.

The cost comparison then becomes concrete: compare two routes that both make accepted holes, including any extra cutting pass, tool change, setup and inspection. A bore pass may be indispensable on the bearing seat and wasteful on the neighboring clearance holes. There is no defensible universal “drilling is cheaper” or “boring is more accurate” rule without the same material, geometry, quantity and acceptance basis.

Technical sources

1. Sandvik Coromant. Drilling a hole. Hole functions, diameter, depth, quality and setup considerations.
2. Sandvik Coromant. Boring holes. Existing-hole definition, rough and finish operations, tool reach and stability considerations.
3. Sandvik Coromant. Finish boring. Finishing an existing opening for size, position and surface; tool deflection and application constraints.
4. Sandvik Coromant. How to ream a hole. Prepared-hole stock and the limit on correcting its position or straightness.
5. Sandvik Coromant. Milling formulas and definitions. Circular milling and helical ramping as distinct programmed hole-making paths.
6. BIG DAISHOWA. BF-CUTTER Back Spot Facer. Local fastener seating-face operation.
7. ASME. Y14.5-2018 (R2024): Dimensioning and Tolerancing. Public scope for dimensions, datum references, position and form.
8. Mitutoyo. Bore Gage-Standard-8mm with Indicator, Series 511. Inside-diameter measurement and two-contact detection of ovalness and taper.