Reamer Allowance & Hole-Prep Chart
Recommended pre-drill undersize for hand and machine reaming, plus grinding, honing, and lapping stock allowances. Imperial and metric tables with speeds-and-feeds for common reamer operations.
Reference
Reamers finish a drilled hole to a precise size and smooth surface. The pre-drill must be undersize by the reamer allowance so the reamer peels a small, consistent chip on each tooth. Too little stock → the reamer burnishes and chatters; too much → it deflects and cuts oversize. Use hand-reamer allowances for hand-tapping through brass and light-gauge stock; machine-reamer allowances for lathe / mill / CNC work where the reamer is rigidly held and spinning.
Hand reamer — imperial
| Reamer Ø | Pre-drill (undersize by) | Pre-drill size | Notes |
|---|---|---|---|
| Up to 1/8" | 0.003 - 0.005" | Just under nominal | Very little stock — brass preferred |
| 1/8 to 1/4" | 0.004 - 0.006" | E.g. #4 drill before 1/4 reamer | Use cutting oil; clear chips every 2-3 turns |
| 1/4 to 1/2" | 0.005 - 0.010" | E.g. 15/32 before 1/2" | Check alignment — hand reamers wander on hard spots |
| 1/2 to 3/4" | 0.008 - 0.012" | E.g. 23/32 before 3/4" | Torque can be high — clamp work securely |
| 3/4 to 1" | 0.010 - 0.015" | E.g. 63/64 before 1" | Very slow rotation; use both hands on the T-handle |
| 1 to 2" | 0.012 - 0.020" | E.g. 1-61/64 before 2" | Reamers this size are hard to hand-ream — prefer machine |
Machine reamer — imperial
| Reamer Ø | Pre-drill (undersize by) | Typical pre-drill | RPM factor |
|---|---|---|---|
| Up to 1/8" | 0.005 - 0.008" | e.g. 3/32 before 7/64 | ~2/3 of drill RPM |
| 1/8 to 1/4" | 0.008 - 0.012" | e.g. 15/64 before 1/4 | ~2/3 of drill RPM |
| 1/4 to 1/2" | 0.012 - 0.016" | e.g. 15/32 before 1/2 | ~2/3 of drill RPM |
| 1/2 to 3/4" | 0.016 - 0.020" | e.g. 45/64 before 3/4 | ~1/2 of drill RPM |
| 3/4 to 1" | 0.020 - 0.025" | e.g. 31/32 before 1" | ~1/2 of drill RPM |
| 1 to 1-1/2" | 0.025 - 0.031" | e.g. 1-29/32 before 2" | ~1/3 of drill RPM |
| Over 1-1/2" | 0.031 - 0.040" | — | ~1/3 of drill RPM |
Metric reaming allowance
| Reamer Ø (mm) | Hand allowance | Machine allowance |
|---|---|---|
| Up to 3 mm | 0.08 - 0.15 mm | 0.10 - 0.20 mm |
| 3 to 6 mm | 0.10 - 0.20 mm | 0.15 - 0.30 mm |
| 6 to 13 mm | 0.15 - 0.30 mm | 0.20 - 0.40 mm |
| 13 to 25 mm | 0.25 - 0.50 mm | 0.40 - 0.60 mm |
| 25 to 50 mm | 0.40 - 0.80 mm | 0.60 - 1.00 mm |
| Over 50 mm | 0.80 - 1.20 mm | 1.00 - 1.50 mm |
Reaming speeds (starting SFM, HSS reamer)
| Material | SFM | % of drill SFM | Feed per rev |
|---|---|---|---|
| Aluminum | 150 - 300 | 60-80% | 0.004 - 0.012" |
| Brass / bronze | 100 - 200 | 60-80% | 0.004 - 0.012" |
| Cast iron | 40 - 60 | 60-70% | 0.004 - 0.012" |
| Mild steel | 40 - 80 | 60-70% | 0.004 - 0.012" |
| Alloy steel | 30 - 60 | 50-70% | 0.003 - 0.010" |
| Tool steel | 15 - 40 | 50-60% | 0.003 - 0.008" |
| Stainless | 15 - 30 | 40-60% | 0.002 - 0.008" |
| Titanium | 10 - 25 | 40-60% | 0.002 - 0.006" |
| Plastic | 100 - 250 | 50-70% | 0.005 - 0.015" |
Finish allowance — grinding, honing, lapping
| Process | Typical stock / side | Resulting tolerance | Resulting Ra |
|---|---|---|---|
| Rough grinding | 0.005 - 0.020" | ±0.0005" | 32-125 μin |
| Finish grinding | 0.002 - 0.005" | ±0.0001" | 8-32 μin |
| Precision grinding | 0.0005 - 0.002" | ±0.00005" | 4-16 μin |
| Honing | 0.001 - 0.010" | ±0.0001" | 4-32 μin |
| Lapping | 0.0001 - 0.001" | ±0.00002" | 0.5-8 μin |
| Superfinishing | 0.0001 - 0.0005" | ±0.00001" | 0.5-4 μin |
| Electropolishing | 0.0002 - 0.001" | loss of size | 4-32 μin |
Operating tips
- Rigidity is everything: a reamer that can wobble will cut oversize. Use the shortest possible reamer for the depth; hold in a solid-mount chuck, not a floating holder unless necessary.
- Run reamers at half to two-thirds the SFM of an equivalent drill; feed at 2-3× the drill feed rate. Light pressure + aggressive feed = clean shearing chip.
- Never back a reamer out while rotating forward under power — the flutes pick up material and score the hole. Stop the spindle, then reverse or retract.
- Use flood coolant or cutting oil — reamers generate heat quickly and work-hardening materials (stainless, Inconel) will "glaze" the flutes in seconds if dry.
- For close-tolerance holes (< 0.0005" tolerance), rough with a drill two sizes undersize, bore to within 0.005" of final, then ream.
- Through-holes: retract reamer at full feed to avoid the heel rubbing. Blind holes: use a bottoming / end-cutting reamer.
- Chatter marks are almost always a tool-holder issue, not the reamer. Check spindle runout and collet chuck grip before re-grinding.
Reamer types
- Chucking (machine) reamer
- Straight shank with 45° bevel lead, flutes helical or straight. Most common in the shop.
- Hand reamer
- Long taper lead (1-2") at the front so it self-aligns when turned by hand. Requires more allowance than machine reamer.
- Taper-pin reamer
- 1/4" per foot taper. For taper pin holes (drive pins, alignment dowels).
- Shell reamer
- Hollow reamer that mounts on an arbor — cheap way to stock large sizes.
- Adjustable reamer
- Blades are moved radially to hit any size in a small range. Handy for repair; slow to set.
- Expansion reamer
- Single-size reamer with a hollow body + plug to expand diameter 0.005-0.015" for hand-fitting.
- Carbide-tipped
- Brazed carbide tips on each cutter. 3-5× life of HSS on abrasive materials; more expensive.
- Solid carbide
- Whole body is carbide; 10× life of HSS on hardened materials. Brittle — no chatter tolerated.
- PCD (polycrystalline diamond)
- Diamond-tipped for aluminium and composites. Up to 20× life of carbide on Al-Si alloys.
Last updated: