Drilling, Reaming and Boring: Hole Tolerance by Process
Standard twist drilling holds roughly ±0.1 mm, reaming takes a hole to H7, and boring reaches H6 or tighter — and the process you choose sets not just the size tolerance but the roundness, straightness, and surface finish inside the hole. Match the process to the fit class on the drawing, because no tool change fixes a hole that was drilled when it should have been bored.
Holes are the most common feature on machined parts and the most common source of assembly failure. A hole that is oversized, undersized, oval, bellmouthed, or wandering off axis turns a simple pin fit or bearing seat into a rework. The drawing's fit callout — H7, H8, or a plain ± dimension — should dictate the process, and each process has a cost and capability that is well understood. This guide covers the four hole-making processes on a CNC machine, the tolerance each one realistically holds, and how to spec holes so the machinist uses the cheapest process that still meets the fit.
The Four Processes and What Each One Holds
Twist drilling is the baseline: a rotating fluted tool cuts the hole in one pass, fast and cheap, but with a tolerance band of roughly ±0.1 mm or looser depending on size and depth, plus a tendency to wander on entry and produce slightly bellmouthed mouths. Reaming follows a drilled hole with a multi-flute reamer that removes a small amount of stock (typically 0.1–0.3 mm) and brings size to H7 or better with a fine finish. Boring uses a single-point tool to enlarge an existing hole to a precise size — the most controllable process, capable of H6 or tighter, but the slowest. The fourth option, for very small or very deep holes, is specialized: gun drilling for deep straight holes, or EDM for holes no rotating tool can reach.
| Process | Typical size tolerance (ISO) | Roundness | Surface finish (Ra) | Relative cost per hole |
|---|---|---|---|---|
| Twist drilling | ±0.1 mm or looser (H12–H13 range) | Fair — can be oval on entry | 1.6–6.3 µm | Lowest |
| Drilling + reaming | H7 typical (H8 easy, H6 with care) | Good | 0.4–1.6 µm | Low–moderate |
| Boring (single point) | H6–H7, adjustable | Excellent | 0.4–1.6 µm | Moderate–high |
| Gun drilling (deep) | ±0.05–0.1 mm on diameter | Good along depth | 0.8–3.2 µm | High, depth-driven |
| Internal grinding | H5–H6 possible | Excellent | 0.1–0.4 µm | Highest |
The tolerance classes deserve a moment. An H7 hole of 10 mm diameter has a tolerance band of about +0.015 mm above nominal; H8 spreads to about +0.022 mm; H6 tightens to about +0.009 mm. Reaming holds H7 routinely because the reamer is sized to the hole and the machine is rigid. Boring holds H6 because the tool can be adjusted to the measured size and corrected. Drilling cannot reliably hold either — it is a roughing process that happens to make holes.
When Drilling Is the Right Answer
Most holes on a machined part do not need H7. Clearance holes for fasteners, cable pass-throughs, vent holes, and any hole with a plain ±0.1 mm or ±0.2 mm callout are drilled and done. A clearance hole for an M6 screw, for example, is typically 6.6–7.0 mm with generous tolerance — no reamer needed. Drilling is also the right first step for holes that will be reamed or bored: the drill removes the bulk of the material and the finishing process only cleans up the last fraction of a millimeter. Specifying drilling where drilling is enough is a real cost saving, because reaming and boring add tooling, cycle time, and inspection.
The depth-to-diameter ratio changes the drilling math. Up to about 3× diameter, a standard drill is fine. From 3× to 10×, peck drilling or a good coolant-through drill keeps chips from packing and the hole from wandering. Beyond 10× diameter, gun drilling or a specialized deep-hole cycle becomes necessary, and cost climbs with depth. Our threading guide covers the same logic one step further — the hole drilled for a tapped thread is itself a tolerance decision, because tap drill size sets thread engagement.
When to Ream Instead
Reaming is the default answer for a hole that must mate with a pin, dowel, shaft, or bearing seat — anything calling H7, or an interference fit like a press-fit dowel hole. The process is simple: drill undersize by 0.1–0.3 mm (reaming removes stock evenly rather than cutting deep), then run the reamer once through. The result is a round, straight, accurately sized hole with a fine finish, at a cost only slightly above drilling. Reaming is also forgiving in production: a reamer held in a floating holder follows the drilled hole's axis, which is why reamed holes are usually straight even when the drilled pilot wandered slightly.
| Fit class on drawing | Process that achieves it | Typical example |
|---|---|---|
| Clearance, ±0.1 mm or looser | Drill only | Screw clearance, cable holes |
| H11–H12 | Drill, or drill + light ream | Sliding fits, low precision |
| H8 | Drill + ream (or bore) | General engineering fits |
| H7 | Drill + ream, or bore | Dowel pins, bearing seats, shaft fits |
| H6 and tighter | Bore (or grind for finest) | Precision bearing journals, valve guides |
The reamer choice matters: machine reamers with a short lead and solid construction hold size better than hand reamers, and the hole should be drilled with the reamer's recommended stock allowance — too much stock makes the reamer chatter, too little makes it rub and wear. Reaming also cannot fix a badly drilled pilot: if the drill wandered off position, the reamer follows it, so positional tolerance on reamed holes is set by the drilling step, and position-critical holes may need the pilot drilled with a spot drill or center drill first.
When to Bore Instead
Boring takes over where reaming cannot go: holes larger than standard reamer sizes, holes needing H6 or adjustable size control, interrupted holes (a bore crossing a slot or oil gallery), and holes where the reamer's tendency to follow the pilot would propagate an error. Because a boring bar is a single-point tool on adjustable center, the machinist can measure the hole and correct the next pass — which is why boring is the process for the tightest classes and for matching two holes to a specific mating size rather than a nominal class.
Boring is slower and demands more skill. Cycle time is higher, the setup is more involved, and the result depends on the bar's rigidity — a long small-diameter boring bar deflects and cuts taper. The classic boring problems are taper (bar deflection), chatter (insufficient rigidity), and size drift (tool wear on long runs), all of which show up in the roundness and straightness of the finished hole. For a hole that is round but tapered, or straight but oval, the geometry discussion in our roundness and concentricity guide explains what to measure and how to catch it before assembly.
Choosing by Depth, Size, and Callout
The practical selection sequence goes like this. Read the hole callout: if it is a plain ± tolerance of ±0.1 mm or looser, drill it. If it is H8–H7, drill and ream. If it is H6, tighter, larger than reamer range, or needs adjustable size, bore it. Then check the geometry: depth-to-diameter beyond 3× needs pecking or coolant-through tooling; beyond 10× needs gun drilling or a deep-hole specialist. Interrupted holes and angled entries push the choice toward boring or toward a spot-faced entry. And if the hole carries a positional tolerance relative to other features, remember that the finishing process only fixes size — position is set by the first operation and by the fixture.
| Hole situation | Recommended process |
|---|---|
| Clearance hole, any size, plain tolerance | Drill |
| Dowel or pin hole, H7 | Spot drill + drill + ream |
| Bearing seat, H6, larger diameter | Drill + bore, measure and correct |
| Deep hole, 10×+ diameter | Gun drill or peck cycle with coolant-through |
| Interrupted bore crossing a slot | Bore with rigid bar |
| Threaded hole | Drill to tap-drill size, then tap or thread mill |
Cost follows capability in a straight line: drilling is a few seconds and one tool; reaming adds a second tool and a pass; boring adds setup, measurement, and slower feeds. The cheapest correct process is the one that meets the callout with margin — no more, no less. That is how we route holes through CNC milling and turning work: the drawing's fit class decides the process, and critical holes are verified on the first article and sampled through the batch on the precision components line.
Email sc@bquq.com or WhatsApp +86 137 1315 7787 with your PDF/DXF/STEP file. An engineer reviews it and replies with price, lead time and DFM notes on working days.
Frequently Asked Questions
Q: What tolerance does a standard drill hold?
A: A twist drill typically holds ±0.1 mm or looser on diameter — roughly an H12–H13 range — with fair roundness. Drilling is a roughing process; holes needing H8 or better are drilled undersize and finished with a reamer or boring bar.
Q: What is the difference between reaming and boring?
A: Reaming enlarges a drilled pilot by 0.1–0.3 mm with a multi-flute tool that follows the existing hole, reaching H7 quickly and cheaply. Boring uses a single-point adjustable tool that can correct size pass by pass, reaching H6 and tighter and handling larger or interrupted holes.
Q: How much stock should be left for reaming?
A: Typically 0.1–0.3 mm on diameter, depending on hole size and material. Too much stock makes the reamer chatter and oversize the hole; too little makes it rub, wear quickly, and lose size control. Follow the reamer manufacturer's recommended allowance.
Q: When do I need to bore instead of ream?
A: Bore when the hole is larger than reamer range, needs H6 or adjustable size, crosses an interruption like a slot, or must not inherit the pilot hole's error. Boring is slower but is the most controllable hole-finishing process on a CNC machine.
Q: Why are my reamed holes sometimes out of round?
A: Usually from insufficient reaming stock, a worn reamer, or a non-rigid setup that lets the tool deflect or the part move. Roundness is set by tool condition and rigidity — a fresh reamer with correct stock in a rigid holder produces round, straight holes.
Authored by the BQUQ Engineering Team. BQUQ is an ISO9001-certified source factory in Dongguan, China, running CNC machining, metal stamping, custom springs, heat sink and collet lines under one roof. Send drawings to sc@bquq.com or WhatsApp +86 13713157787 for a quote within 12 working hours. www.bquq.com
