Skip to content
MechDatum

Reaming tolerances and parameters

What is reaming?

Section titled “What is reaming?”

Reaming is a precision machining process that slightly enlarges a previously drilled or bored hole, improving its diameter, roundness, and surface finish to tight tolerances (IT8‑IT9). A reamer, a rotary cutting tool with multiple cutting edges, removes a small allowance of material (typically 0.1–0.2 mm / 0.004–0.008 in) to leave a dimensionally accurate hole with controlled roughness. It is performed on drilling machines, lathes, machining centers, and even manually.

Operating principle

Section titled “Operating principle”

The reamer is inserted into the existing hole with a slight taper at the entry that self-centers it. The cutting edges, straight or helical, machine the excess material by guiding on the surface of the previous hole, so it does not correct the position or alignment of the center. Chips are evacuated through the flutes and the bottom of the hole requires space for chip accumulation. The cutting action is smooth and steady, achieving very repeatable dimensional and form tolerances if the correct allowance and cutting parameters are respected.

Operating parameters

Section titled “Operating parameters”

Cutting parameters depend on the workpiece material and the type of reamer (generally HSS or carbide). Typical recommendations are shown below:

Material Cutting speed – HSS Cutting speed – Solid carbide Feed per revolution Cutting fluid
Wrought aluminum 60–100 m/min / 200–330 ft/min 120–200 m/min / 400–660 ft/min 0.10–0.20 mm / 0.004–0.008 in Emulsion (10 %) or soluble oil
Carbon steel (<0.3 % C) 15–25 m/min / 50–80 ft/min 40–60 m/min / 130–200 ft/min 0.08–0.15 mm / 0.003–0.006 in Active cutting oil
Austenitic stainless steel 8–15 m/min / 25–50 ft/min 20–30 m/min / 65–100 ft/min 0.05–0.10 mm / 0.002–0.004 in Chlorinated or additized mineral oil
Gray cast iron (GG-25) 20–30 m/min / 65–100 ft/min 40–70 m/min / 130–230 ft/min 0.10–0.20 mm / 0.004–0.008 in Dry or light mist
Brass / Bronze 30–50 m/min / 100–165 ft/min 60–100 m/min / 200–330 ft/min 0.10–0.25 mm / 0.004–0.010 in Soluble oil or dry

Recommended allowance:

  • Soft materials (aluminum, brass, mild steel): 0.1–0.2 mm / 0.004–0.008 in.
  • Hard materials (hardened steels, cast iron): 0.05–0.13 mm / 0.002–0.005 in.
  • Do not exceed 5 % of the previous hole diameter to avoid overloading and premature reamer wear.

Tolerances and surface quality

Section titled “Tolerances and surface quality”

Reaming can maintain dimensional tolerance grades IT8 to IT9 according to ISO 286. In industrial practice, this translates to tolerances of ±0.025 mm / ±0.001 in for diameters up to 25 mm. Roundness and cylindricity improve noticeably compared to drilling, although the hole retains the positional deviation of the previous machining. Typical surface roughness is Ra 0.8–3.2 µm (32–125 µin), reaching values close to Ra 0.4 µm / 16 µin with carbide tools and optimized parameters.

Applicable materials

Section titled “Applicable materials”

Reaming is used on practically any metallic material that produces short chips and is not excessively abrasive, among them:

  • Carbon, alloy, and stainless steels.
  • Gray and nodular cast irons.
  • Aluminum, magnesium, and copper alloys.
  • Brass and bronzes.
  • Titanium and superalloys (with reduced speeds and carbide tools). It is not suitable for highly abrasive fibrous composites, materials with hard inclusions, or thermosetting plastics that tend to dull the cutting edges.

Advantages and limitations

Section titled “Advantages and limitations”

Advantages:

  • Obtaining precise diameters (IT8‑IT9) and good surface finish in a single finishing pass.
  • Fast process and easy to automate in medium and high production.
  • Competitive cost per hole compared to precision boring or honing.

Limitations:

  • Does not correct the position or perpendicularity of the hole; inherits the error of the previous hole.
  • Requires a pilot hole prepared with a controlled allowance; damage or lack of roundness in the drilling is reflected in the result.
  • Limited chip evacuation in blind holes; a chamfer or greater depth must be provided to accommodate chips.
  • Reamer wear can change the diameter in long series, requiring periodic checks or the use of expandable reamers.

Reamer selection guide

Section titled “Reamer selection guide”
  • Chucking reamers: general use in drilling machines, lathes, or milling machines. Straight or Morse taper shank. Straight or helical flutes.
  • Adjustable hand reamers: cover a small diameter range with interchangeable blades. Only for through holes and light reaming; risk of vibration if not used correctly.
  • Taper reamers: for taper pin seats, tapered according to standard (1:50, 1:48, etc.).
  • Roughing and finishing reamers: pairs that split the allowance; the roughing reamer prepares the diameter and the finishing reamer provides final size and surface.
  • Helix criteria: left-hand spiral with right-hand cut for through holes (promotes chip evacuation); straight flute or right-hand spiral for blind holes (pushes chips outward).

Frequently Asked Questions (FAQ)

Section titled “Frequently Asked Questions (FAQ)”

What tolerance can reaming achieve?

Section titled “What tolerance can reaming achieve?”

Reaming typically achieves tolerance grades IT8 to IT9, equivalent to ±0.025 mm (±0.001 in) for diameters up to 25 mm.

What material allowance is left for reaming?

Section titled “What material allowance is left for reaming?”

An allowance of 0.1 to 0.2 mm (0.004–0.008 in) is recommended for soft materials and 0.05 to 0.13 mm (0.002–0.005 in) for hard materials, without exceeding 5 % of the drilled diameter.

What is the typical surface finish after reaming?

Section titled “What is the typical surface finish after reaming?”

Surface finish ranges between 0.8 and 3.2 µm Ra (32–125 µin), and can reach 0.4 µm Ra (16 µin) with carbide tools and adequate cooling.

Section titled “What cutting speed is recommended for reaming aluminum?”

For wrought aluminum, speeds of 60–100 m/min (200–330 ft/min) are used with HSS reamers and up to 200 m/min (660 ft/min) with solid carbide.

Can reaming correct the position of a hole?

Section titled “Can reaming correct the position of a hole?”

No. Reaming only calibrates the diameter and improves roundness; it inherits the positional deviation of the previous hole.

What type of reamer is suitable for through holes in production?

Section titled “What type of reamer is suitable for through holes in production?”

Chucking reamers with left-hand spiral and right-hand cut are preferred, as they evacuate chips forward and reduce the risk of jamming.

References

Section titled “References”