How Does Reaming Improve Hole Accuracy and Surface Finish?

What Is Reaming?

Reaming is a hole-finishing process in which a reamer removes a very thin layer of metal from the hole wall to improve dimensional accuracy and reduce surface roughness. It is commonly used to finish moderate-diameter holes in materials that are not excessively hard and can also serve as preparation before honing or lapping. Machine reaming offers high productivity and low labor demand, making it suitable for mass production.

Reaming can achieve IT9 to IT7 accuracy and a typical surface roughness of Ra 1.6 to 0.8 µm. This performance results from the reamer’s specialized geometry, the small machining allowance, and the low cutting speed.

For example, six equally spaced Ø20H7 holes with a required Ra 1.6 surface finish are suitable candidates for reaming.

An IT8 hole can generally be completed in one reaming pass. An IT7 hole should be reamed twice: first with a reamer 0.05 to 0.2 mm below the hole size, then with a finishing reamer that meets the hole tolerance. An IT6 hole should be reamed three times.

Reaming has limited ability to correct positional error, so the preceding operations must establish the required location. A hole with demanding coaxiality or positional tolerance may be spot-drilled, drilled, rough-bored, and then reamed. Before reaming, the hole surface roughness should be below Ra 3.2 µm.

Coolant helps produce a better surface and remove chips. Reaming does not generate a large amount of heat, so a standard coolant is normally sufficient.

Reamer Construction and Selection

Reamer Structure

Machining centers generally use standard machine reamers. Common forms include straight-shank, taper-shank, and shell reamers. Typical diameter ranges are Ø6 to Ø20 mm for straight-shank tools, Ø10 to Ø32 mm for taper-shank tools, and Ø25 to Ø80 mm for shell reamers. Reamers are commonly available in H7, H8, and H9 accuracy grades.

The initial portion of the head is the entry chamfer or lead, which helps the tool enter an unchamfered hole. Some reamers include a tapered cutting section that performs most of the cutting. Its small half-angle, generally 1° to 15°, improves centering and produces thin chips.

The sizing section corrects hole diameter, finishes the wall, and guides the tool. Its cylindrical portion maintains the reamer diameter and provides a measuring surface. A slight back taper on the rear portion reduces friction against the hole wall.

Determining Reamer Diameter

Hole accuracy depends primarily on reamer dimensional accuracy. A new standard cylindrical reamer often includes grinding allowance and may have insufficient surface finish. Before producing holes more accurate than IT8, its diameter should therefore be ground to the required size.

A reamed hole may expand or contract, and there is no single universal allowance for this behavior. A practical sizing method is:

• Reamer basic diameter = hole basic diameter.
• Upper deviation = two-thirds of the hole diameter tolerance.
• Lower deviation = one-third of the hole diameter tolerance.

For an Ø20H7 hole with a tolerance of +0.021/-0 mm, the reamer basic diameter is Ø20 mm, the upper deviation is 2/3 × 0.021 = 0.014 mm, and the lower deviation is 1/3 × 0.021 = 0.007 mm. The selected reamer diameter is therefore Ø20 mm with deviations of +0.014/+0.007 mm.

Selecting the Number of Teeth

A reamer is a multi-edge tool, and tooth count depends on hole diameter and accuracy. Standard reamers have 4 to 12 teeth. Too many teeth make manufacturing and sharpening difficult, reduce tooth strength at a fixed diameter, restrict chip space, and can cause chip packing, wall scratches, or edge chipping. Too few teeth reduce stability, increase load per tooth, and make geometric error more likely.

Reamers may have straight or helical teeth. A helical reamer with left-hand flutes is suitable for through holes because the helix forces chips toward the bottom and into the open space beyond the hole. It is not suitable for blind holes.

Selecting Reaming Parameters

Reaming Allowance

Reaming allowance is the depth of material reserved for the reaming operation. It is normally smaller than the allowance for counterboring or boring. Excessive allowance increases cutting pressure, can damage the reamer, and produces poor surface finish. When the allowance is large, separate rough- and finish-reaming passes should be used.

Insufficient allowance can cause premature tool wear, prevent normal cutting, and also degrade the finish. A typical allowance is 0.1 to 0.25 mm and should not exceed 0.3 mm on larger holes. A general recommendation is to reserve 1% to 3% of the reamer diameter as diametral stock.

Feed Rate

Reaming feed is usually two to three times the drilling feed. The higher feed encourages the reamer to cut rather than rub, although surface roughness Ra increases as feed increases.

If feed is too low, radial rubbing increases. The reamer then wears quickly, may chatter, and can leave a rough hole surface.

Spindle Speed

All cutting parameters influence reamed surface roughness, but cutting speed has the greatest effect. To obtain approximately Ra 0.63 with a high-speed steel reamer in medium-carbon steel, cutting speed should not exceed 5 m/min so that a built-up edge is unlikely to form. Cast-iron chips break into particles and do not readily form a built-up edge, so speed can be increased to 8 to 10 m/min.

A common starting point is a reaming spindle speed equal to two-thirds of the drilling speed in the same material. If drilling uses 500 r/min, for example, a reasonable reaming speed is 500 × 0.660 = 330 r/min.

Using a Canned Cycle for Reaming

The sequence for reaming resembles other hole-making operations. For a blind hole, drilling is followed by reaming, but drilling chips left in the hole may disrupt the reamer. An M00 program stop should therefore be used before reaming so the operator can remove all chips.

Reaming programs also use canned cycles. FANUC controls do not define a dedicated reaming cycle, but G85 is appropriate because it feeds into and out of the hole at the same feed rate.