CNC hole tolerances — drilling vs reaming vs boring

§ 01 / HOLE-MAKING

Hole-making process capability

Process	Typical tolerance	IT class	Surface finish (Ra)	Relative cost
Twist drill (standard)	+0.1 to +0.3 mm oversize	IT12-13	3.2-6.3 μm	1.0× (baseline)
Twist drill (precision)	+0.05 to +0.15 mm oversize	IT11-12	1.6-3.2 μm	1.2×
Spot drill + drill	Same as drill alone but accurate location	IT11-12	Same	1.3×
Drilled + reamed	±0.025 mm	IT8-9	0.8-1.6 μm	1.5-2×
Drilled + precision reamed	±0.015 mm	IT7	0.4-0.8 μm	2-3×
Bored (single point)	±0.010 mm	IT7	0.8-1.6 μm	3-5×
Bored + honed	±0.005 mm	IT6	0.2-0.4 μm	5-7×
Jig bored	±0.005 mm with ±0.003 mm position	IT6	0.4-0.8 μm	8-12×
Ground	±0.003 mm	IT5	0.1-0.4 μm	10-15×

§ 02 / DRILL

Drill bit sizing reality

A "Ø6.0 mm" drill typically produces a hole that is:

Ø6.0 to Ø6.15 mm (HSS drill, standard conditions)
Ø6.0 to Ø6.05 mm (carbide drill, rigid machine)
Ø6.00 to Ø6.02 mm (carbide drill with coolant, peck cycle, rigid setup)

Drilled hole is always slightly oversize and never undersize. The variation comes from:

Drill wandering entering the workpiece
Drill flex under cutting load
Drill wear as it cuts
Heat expansion

For holes where function is "bolt clearance through this hole," drilled tolerance is usually adequate. For holes where a pin or bushing must press-fit precisely, reaming or boring is required.

§ 03 / WHEN

When to spec reaming vs boring

Reaming:

Uses a pre-existing drilled hole (slightly undersize)
Follows the drill — cannot straighten a drilled-crooked hole
Produces a round, cylindrical hole at the reamer diameter
Fast — 2-5× the time of drilling alone
Best for holes Ø3-25 mm in production volumes

Boring (single-point):

Cuts the hole with a single adjustable tool
Can correct alignment errors from drilling
Provides very precise diameter and position
Slow — 5-10× the time of drilling alone
Best for large holes (>Ø25 mm) or where precision matters more than cycle time

Typical workflow for a precision through-hole:

Spot drill (creates accurate start point)
Undersize drill (forms the bore, slightly undersize of finish)
Ream or bore to final dimension

This three-step process is standard for IT7 or tighter holes.

§ 04 / POSITION

Position vs diameter — two different tolerances

Hole tolerance has two components:

Diameter tolerance: how close the hole is to spec size (e.g., ±0.01 mm on Ø10)
Position tolerance: where the hole center is relative to datums (e.g., Ø0.05 mm true position)

These are independent. A hole can be perfect diameter but 0.2 mm off position; or perfect position but 0.1 mm oversize. Both matter.

Position tolerance is typically specified using GD&T:

⌖ Ø0.2 mm: general mounting holes, bolt clearance
⌖ Ø0.1 mm: precision assembly, dowel clearance
⌖ Ø0.05 mm: bearing bore, press-fit features
⌖ Ø0.025 mm: precision jig bores, measurement fixtures

For precision pin/bushing fits, BOTH diameter and position must be tight. Loose on either defeats the precision.

§ 05 / PRACTICAL

Practical spec guidance

Bolt clearance holes → drilled, ±0.1 mm standard

No need for reaming. Most bolts have 0.5-1 mm clearance anyway. Don't over-tolerance.

Dowel pin holes → reamed, ±0.025 mm

Press-fit dowel pins need reamed hole. Specify H7 tolerance on the hole (H7 = ~+0.021 mm for most pin sizes).

Bearing bores → reamed or bored to H7

Standard fit for most bearing outer races. H7 on the bore + k6 on the shaft = light interference fit.

O-ring grooves → drilled + bored (or form cutter)

Depth tolerance matters as much as diameter. Usually ±0.05 mm on both. Specify Ra 0.8 on sealing surface.

Oil passages → drilled, ±0.2 mm

Size matters less than location. Spec position but let diameter be drill-standard.

READY WHEN YOU ARE

Precision holes on your drawing?

Email [email protected]. We'll review the tolerance stack on each hole — sometimes a ±0.025 mm hole can be ±0.05 mm without functional impact, saving 50% on that feature's cost.

Start a quote →