What a Drill Bit Actually Does to a Hole
A drill bit is a roughing tool. Its job is to remove material efficiently, not to produce a hole to a precise diameter. Understanding this changes how you think about tolerances and when to introduce a reamer.
A standard jobber drill in good condition typically produces a hole 0.001 to 0.003 inches over nominal diameter. A 1/2 inch drill produces a hole of roughly 0.501 to 0.503 inches. The oversize comes from several sources: slight lip height inequality means one lip cuts more than the other, which causes the drill to orbit slightly rather than track true; any runout in the spindle or chuck adds to this; and the material itself can spring back slightly after the drill passes through.
In soft aluminum on a rigid machine with a fresh, accurately sharpened drill, you might achieve closer to +0.001 inches. In stainless or cast iron with a drill that has seen some use, +0.004 to +0.005 inches over nominal is not unusual. The point is: if your drawing calls for a hole to plus or minus 0.001 inches, a drill alone cannot reliably get you there.
Reamers work differently. A reamer has multiple cutting flutes and a straight or slightly helical cutting geometry designed to remove a small, controlled amount of material and leave a precise diameter with a good surface finish. The reamer follows the existing hole axis rather than generating its own path, which means it corrects size but does not fully correct position. If your drilled hole is in the wrong location, a reamer will not fix that — you need to correct position before reaming, not after.
Tolerance Thresholds: When to Ream
The practical threshold for introducing a reamer is a tolerance of plus or minus 0.001 inches or tighter on hole diameter. Above that — plus or minus 0.003 inches or more — a carefully selected drill and good technique can often hold the tolerance without reaming. Below it, reaming is the standard approach in manual and CNC machining alike.
Common applications that routinely require reaming:
- Press-fit and slip-fit holes for shafts and pins, where the fit class requires a specific diameter range
- Hydraulic and pneumatic component bores where internal leakage depends on hole diameter
- Bearing bores in housings where the bearing OD is the mating dimension
- Dowel pin holes in tooling and fixtures where location repeatability matters
- Any H7 or tighter tolerance hole call-out on a print
Surface finish is the other reason to ream. A drilled hole has a surface finish in the range of 125 to 250 microinches Ra. A reamed hole comes in at 32 to 63 microinches Ra or better. For any application involving sealing, bearing surfaces, or close sliding fits, that finish difference matters functionally, not just cosmetically.
Pre-Ream Undersizing
Reamers require a specific amount of material to remove to work correctly. Too much material and the reamer deflects, chatters, or overheats. Too little and it rubs rather than cuts, generating heat and leaving a poor finish while also dulling the reamer prematurely.
Standard reaming allowances by diameter:
- Up to 1/4 inch: leave 0.005 to 0.008 inches for the reamer
- 1/4 to 1/2 inch: leave 0.008 to 0.015 inches for the reamer
- 1/2 to 1 inch: leave 0.015 to 0.025 inches for the reamer
This means the drill you choose for a reamed hole is deliberately undersized by these amounts. For a 0.500 inch reamed hole using a 0.500 inch reamer, you would drill the hole to roughly 0.480 to 0.490 inches, then ream to final size. Most machining references publish pre-drill sizes for standard reamed holes — consult the Machinery's Handbook table for your specific diameter if you are not sure.
The drill's actual condition affects this calculation. A worn or freehand-sharpened drill that runs oversize by 0.004 inches throws off your pre-ream dimension. This is one practical reason why drill geometry consistency matters even in operations that will be reamed — if you cannot predict what size the drill will produce, you cannot reliably control your pre-ream stock.
Hand vs Machine Reamers
Hand reamers have a long, gradual lead-in taper and are designed to be turned with a tap wrench at low speed. They are for fitting work, repair, and situations where you need to size a hole in place on an assembled component. Hand reamers are not interchangeable with machine reamers — they are meant for low-speed, hand-guided work.
Machine reamers have a shorter, steeper chamfer lead-in and are designed to run in a drill press, lathe, or mill. They need rigid, aligned toolholding. Running a machine reamer at the correct speed — typically one-quarter to one-third the speed you would drill the same material — and with sufficient cutting fluid produces consistent, accurate holes.
The most common reaming mistake on a drill press is running too fast. Reamers are slow tools. A 1/2 inch reamer in steel should run at around 50 to 100 RPM on most drill presses — far slower than the drilling speed for the same material. High-speed reaming generates heat that causes the reamer to cut oversize, defeating the purpose of reaming in the first place.
Floating reamer holders improve results on drill presses and mills by allowing the reamer to self-align with the existing hole rather than being rigidly held to the machine spindle axis. If your reamed holes are coming out slightly bell-mouthed or oversize, a floating holder often cures the problem by letting the reamer follow the hole rather than forcing the hole to follow the spindle.
Reamer Geometry Maintenance
Reamers are more geometry-sensitive than drills. A drill with slightly unequal lips still cuts — it just produces an oversized hole. A reamer with any significant geometry variation produces a hole that is both oversized and out-of-round, which is worse than a drilled hole and defeats the entire point of the operation.
Reamers wear at the chamfer lead-in and at the first millimeter or two of the cutting lands. This wear is often not visible to the eye but shows up as hole diameter drift — holes that were on the high side of tolerance start going over, or finish quality deteriorates before diameter changes. Measuring your reamed holes over time is how you catch reamer wear before it becomes a quality problem.
Carbide reamers hold geometry longer than HSS in abrasive materials but are more expensive to resharpen correctly. HSS reamers are the standard for general shop use and the better economic choice unless you are running high volumes in abrasive materials.
The Connection to Drill Resharpening Programs
Production shops running reamed holes in significant volume have a strong economic interest in consistent pre-drill geometry. Every drill that runs oversize shortens the reamer life by presenting too little stock for the reamer to remove cleanly. Every drill that runs significantly undersize leaves too much stock and causes the reamer to deflect.
The MachinistPost resharpen program returns drills to consistent, documented geometry — the same geometry every time, which is what you need when the drill's output size feeds directly into a reaming operation. Shops with high reaming volume and unpredictable pre-drill diameters often trace the problem back to inconsistent drill geometry from freehand resharpening. Machine resharpening eliminates that variable from the equation.
If you are running a lot of reamed holes and your reamer life is shorter than it should be, or your reamed hole sizes are drifting, look at your pre-drill quality before you replace the reamer. The reamer is often the symptom; the drill is the cause.