A reamer is not designed to remove large amounts of material. It's a finishing tool that skims a few thousandths from the surface of a drilled hole to bring it to a specific diameter, roundness, and surface finish. The drill makes the hole — the reamer perfects it.
If you leave too much stock for the reamer, it behaves like a drill in a hole — it has to cut aggressively, generates heat, deflects from center, and produces a hole that's no more accurate than the drilled hole you started with. In the worst case, too much allowance breaks reamers or causes chatter that ruins the hole finish.
If you leave too little stock, the reamer contacts so little material that it rubs rather than cuts. Rubbing generates heat without removing material cleanly, burnishes the surface instead of cutting it, and dulls the reamer rapidly without improving the hole quality. A reamer that's barely removing material produces a worse finish than one that's cutting properly.
The correct ream allowance is the range where the reamer is cutting consistently — removing enough material to establish true diameter and finish without overloading the flutes.
The traditional rule is to leave 0.010" to 0.015" of stock for reaming in most materials. This gets taught in machinist training and appears in most tooling references. It's a reasonable middle-of-the-road guideline, but it ignores variables that matter significantly in practice.
The rule assumes mild steel, standard HSS reamers, and hand-chucked drill press or lathe work. It breaks down when you're working in harder materials, using carbide reamers, working at CNC spindle speeds, reaming thin-wall parts, or working to very tight tolerances.
A better approach is to understand the factors that shift the allowance range, and use the standard rule as a starting point rather than a constant.
Material hardness. Softer materials like aluminum, brass, and free-machining steels tolerate wider ream allowance ranges — you can leave 0.015" to 0.020" and the reamer handles it cleanly. Harder materials like 4140 HT, 17-4 PH stainless, or titanium require tighter allowances — 0.005" to 0.010" — because the reamer has less cutting ability to spare and excess material causes deflection and chatter.
Hole diameter. Small-diameter reamers (under ¼") are more sensitive to allowance than large-diameter reamers. A small reamer with too much stock will deflect off center. For diameters under ³⁄₁₆", keep allowance at the low end: 0.003" to 0.007". For diameters above ½", the 0.010"–0.015" range is appropriate.
Reamer type. Hand reamers have relatively flexible shanks and work best with lighter cuts — 0.005"–0.010". Machine reamers are more rigid and can handle the full 0.010"–0.015" standard range. Carbide reamers are rigid and sensitive to misalignment — use lighter allowances and precise alignment. Adjustable reamers are designed for a range and can handle slightly more stock than fixed-size equivalents.
Tolerance requirements. For H7 tolerances (common in press-fit and clearance-fit applications), the allowance needs to be consistent from hole to hole. In production, test the allowance on a sample hole first — measure the reamed result and adjust your pre-ream drill size if the diameter or finish isn't meeting spec. For loose tolerances, the allowance matters less because the reamer has more room to produce an acceptable result.
The standard approach:
For a nominal ream diameter, subtract the desired allowance to get the pre-ream drill size. If you're reaming to 0.500" (½") and want 0.012" allowance, your pre-ream drill is nominally 0.488". The closest standard fraction is 31/64" (0.484") — that gives you 0.016" allowance, which is on the upper end but acceptable for mild steel.
In practice, drills don't always hit exactly their nominal size. A ½" drill in a worn chuck on a drill press with any runout can produce a hole from 0.498" to 0.510" depending on conditions. If the hole is already 0.501" and you're reaming to 0.500"... you have a problem. This is why hole condition monitoring matters on precision reaming work — a quick check with a pin gauge or telescoping gauge on a few representative holes before committing to a production run saves scrap.
For CNC work, the solution is to qualify the drill and fixture combination: drill a test hole, measure it, and confirm the allowance before running the batch. A drill that consistently hits 0.496"–0.498" in your material gives you a known 0.002"–0.004" allowance for ½" reaming — you may want more stock, so a 31/64" drill at 0.484" nominal gives you 0.016" allowance.
Blind holes (reamed partway through) require more attention to allowance than through-holes. In a through-hole, chips escape from the exit side and the reamer can complete its cut cleanly. In a blind hole, chips must be evacuated back out through the reamer flutes past the entry, and they accumulate at the bottom.
For blind holes, reduce ream allowance by 10–20% compared to the equivalent through-hole. The reduced chip load helps with evacuation. Also use spiral-flute reamers in blind holes if possible — the spiral flute design is designed to pull chips up and out rather than letting them pack at the bottom.
For very deep blind holes (depth-to-diameter ratio over 3:1), pre-ream with a smaller drill, clear chips thoroughly, then ream. The drilling operation generates the most chips; reaming should be almost a finishing pass at this point.
Too much stock: reamer chatters, hole is oversize or out-of-round, reamer dulls faster than expected, excessive heat at the reamer body, surface finish is rough or torn.
Too little stock: reamer squeaks or squeals, hole diameter doesn't quite reach nominal size, surface finish looks burnished rather than cut, reamer dulls fast from rubbing, hole roundness doesn't improve over the drilled state.
Correct allowance: reamer cuts smoothly with a steady feed, consistent chips form and evacuate, hole diameter hits nominal consistently, surface finish is clean and regular, reamer life is predictable.
If you're getting inconsistent results, start by measuring your pre-ream hole diameter — not the nominal drill size, but the actual hole. The drill is a starting point, not a guarantee. Know what you're actually giving the reamer, and adjust accordingly.
The pre-ream hole quality depends on the drill. A dull drill produces an oversize, out-of-round hole that leaves the reamer fighting to clean up — or can't. Mail in your pre-ream drills and we'll restore them to spec.
Get a Quote →