CNC drilling vs reaming vs boring: what is the difference?

The short answer

Three jobs, three tools

The three operations are separated by what each one is allowed to change. A twist drill creates a hole in solid stock and removes the bulk of the material quickly, but it follows its own deflection: the hole it leaves is usually slightly oversize, slightly tapered and not perfectly round, and its position depends on the entry. A boring bar is a single-point tool mounted on a rigid bar, so its diameter can be adjusted on the machine and it is aligned to the intended centreline; that means boring can correct the position and straightness of a hole that drilling has already produced. A reamer is a multi-flute finishing tool of fixed diameter that removes a small, even allowance and produces a very consistent round hole; what it cannot do is change where the hole is. Understanding that one distinction, boring changes geometry and reaming only changes size, prevents most of the arguments between a designer and a machine shop.

Tolerances and surface finish side by side

Drilling alone is a clearance-grade process. It lands somewhere in the IT12 to IT14 range with surface finish around Ra 3.2 to 12.5 micrometres depending on the feed, the drill quality and whether the chips cleared; that is perfectly adequate for a fastener hole, a cable route or a drain. Boring takes the same hole to IT7 to IT9 and Ra 0.8 to 3.2 micrometres, and because the size is set by the operator rather than by the tool it also handles diameters for which no standard reamer exists. Reaming holds IT6 to IT7 with Ra 0.4 to 1.6 micrometres and is the standard answer for a dowel hole, a bearing seat or an H7 press fit. The weakest common specification is an H7 callout on a hole that only ever sees a bolt pass through it: forcing a reaming operation onto every hole on a bracket adds roughly 1.5 to 2 times the machining cost for no functional benefit at all.

Why boring can fix a hole and reaming cannot

A reamer has no independent way to find the centre of the hole it is entering: it follows the path the drill left behind, so if the hole is off position or tapered, the finished hole is off position and round but off position. A boring bar is set on the machine's own axis, so the first pass removes the high side of an eccentric hole and the hole moves towards the true centreline. That is why the practical sequence for a tight bore is drill, then bore to correct and roughly size, then ream or fine-bore to the final figure. It is also why reamers are a poor choice for interrupted cuts such as a cross-drilled hole, and why they must not be asked to remove a heavy allowance: reaming more than about 0.3 mm on diameter overloads the flutes and produces the bell-mouthed hole that everyone then blames on the operator.

Stock allowance, entry and blind holes

Leave the sizing tool a predictable amount of material rather than a generous one. For reaming, 0.10 to 0.30 mm on diameter is the normal allowance, and the pre-drill should be about 0.2 to 0.3 mm under the reamer size; for boring, aim to come within 0.05 to 0.10 mm of the final diameter. A reamer needs a chamfered lead-in at the entry and either a through exit or an undercut at the bottom, so a genuinely blind precision hole is usually bored rather than reamed. Where a blind hole must be reamed, the drill depth has to be set deeper than the reamed depth to leave room for the chips and the tool nose. Standardising on the sizes your shop already stocks for drills and reamers avoids the lead time and cost of special tooling, and if a non-standard diameter has to hold a tight tolerance, boring is the cheaper route.

Deep holes change the rules

Up to about five times the diameter, a standard drill behaves acceptably. Beyond that, drill deflection grows, chips have a long way to travel and heat builds up, so the hole drifts, tapers and comes out rough; peck drilling cycles and high-pressure through-coolant flushing are the minimum counter-measures above a depth-to-diameter ratio of about four to one. Where both depth and accuracy are needed, gun drilling with a single-flute tool and internal coolant delivery holds roughly twenty times diameter or more and reaches tolerance bands well under what standard drilling can manage. Deep-hole work is also where the sequence matters most, because a defect created at the entry is amplified all the way to the bottom and no later operation can bring a curved hole back to a straight line.

What to put on the drawing

Specify the tolerance and the finish you actually need, and specify them on the hole diameter only where it matters. Give the depth with a clear reference face, because hole depth measured from a rough casting face is a different hole from one measured from a machined datum. State whether the hole must be round, straight or concentric, since reaming will satisfy the first and boring is required for the others, and name the inspection method: a plug gauge, a bore gauge and a CMM can differ by more than a fine tolerance, and the difference is discovered at goods-in rather than in the drawing office. Wall thickness and hole-to-edge distance matter too, because a hole placed within about two material thicknesses of an edge will bulge or tear the edge during machining. Finally, say how many holes are involved, because the cost of a finer process is multiplied by every hole on the part.

See CNC machining services for drilled, bored and reamed holes quoted from your drawing, metal stamping for punched holes at production volume, and die casting for holes that are cast in and then finished by machining.