How to Choose the Reamer Feed and Speed in a Machining Center

• 1
  Key takeaways
• 2
  What Actually Controls Reamer Feed and Speed
• 3
  Stock Allowance: The Number You Set Before Any Cutting
• 4
  How to Set Reamer Feed per Tooth and per Revolution
• 5
  Spindle Speed and Surface Speed for Reaming
• 6
  When the Hole Comes Out Wrong
• 7
  Step-by-Step Setup on the Machining Center
• 8
  Reaming Parameters by Material

A reamer is a multi-edge finishing tool. It follows an existing hole and shaves a thin layer off the wall. Because the radial depth of cut is tiny, the cutting edge spends most of its time rubbing rather than shearing. That is why reaming numbers look so different from drilling or milling numbers.

Two variables decide whether the hole comes out round, on size and smooth. The first is feed per tooth, which sets chip thickness. The second is surface speed, which sets edge temperature. Get the chip thin enough and the edge stays sharp. Push it too thin and the tool burnishes the wall instead of cutting it.

There is a third factor most operators ignore. Reamer feed and speed only work if the pre-drill is straight and leaves the right stock. A reamer cannot correct a bell-mouthed or tapered hole. It will follow the error and reproduce it with a better finish.

Our shop runs 127 high-precision CNC machines, including 16 simultaneous 5-axis centers and 27 three-axis machines. Reaming jobs on parts from Ø2 mm to Ø50 mm follow the same logic: control the stock, control the chip, control the coolant. Everything below builds on those three.

The radial stock left for the reamer (called the reaming allowance) is the single largest source of scrap on reamed holes. Too much stock overloads the flutes, raises cutting pressure and tears the wall. Too little stock lets the reamer skate over the surface without cutting cleanly.

For rough reaming with a standard HSS or carbide reamer, leave 0.1–0.3 mm on diameter. For finishing reaming where you need H7, tighten that to 0.03–0.1 mm on diameter. Never go below 0.02 mm. Below that the edge rubs and the hole burns out fast.

The pre-drill matters as much as the number. Drill to roughly 0.2 mm under the finished size for a standard allowance, and hold the pre-drill concentric. A drill that wanders by 0.05 mm will hand the reamer a curved hole, and the reamer will keep that curve.

If the pre-drilled hole is larger than expected, do not simply run the reamer anyway. Check the drill diameter, check runout, and check whether the material spring-back is opening the hole. Cutting air with half the flutes is how holes come out oval.

• 1
  Rough reaming0.1–0.3 mm on diameter of stock left for the reamer.
• 2
  Finishing / H70.03–0.1 mm on diameter. Below 0.02 mm the edge rubs.
• 3
  Pre-drill targetAbout 0.2 mm under final size, held concentric within 0.02 mm TIR.
• 4
  Split when neededFor tight sizes, rough ream then finish ream to hold the tolerance.

Feed is expressed two ways: feed per tooth and feed per revolution. Most shop manuals and CAM posts use feed per revolution (mm/rev), because that is what the machine code carries. A typical reamer has 4 to 8 teeth, so the two numbers move together.

A safe starting band for feed per revolution is 0.1–0.3 mm/rev in aluminium and mild steel, dropping to 0.05–0.15 mm/rev in stainless and titanium. Multiply by the tooth count to get the chip load per edge. If the chip load drops below about 0.02 mm per tooth, the reamer starts to rub instead of cut.

The most common mistake is running too slow on feed to chase a better finish. That backfires. A thin chip does not shear off cleanly; it smears along the wall, raises the surface roughness, and work-hardens stainless in particular. If the finish is poor, increase feed first, then check coolant.

Another mistake is running the reamer at the same feed as the drill that made the hole. A drill has two edges and needs a much heavier chip. Copying that number onto a 6-flute reamer gives a chip load that is far too small and a hole that will not clean up.

• 1
  Aluminium / mild steel0.1–0.3 mm/rev starting band.
• 2
  Stainless / titanium0.05–0.15 mm/rev, do not go under 0.02 mm per tooth.
• 3
  Never copy drill feedA multi-flute reamer needs a very different chip load.
• 4
  Poor finish first fixIncrease feed before you touch spindle speed.

Reamers run at low surface speed compared with end mills. In carbon and alloy steel, use 6–15 m/min. In aluminium and brass, 10–20 m/min. Stainless, titanium and Inconel sit at 4–8 m/min. These numbers keep the edge cool and stop built-up edge from forming on the margin.

Convert surface speed to rpm with the standard formula: rpm = (1000 × surface speed) / (π × reamer diameter). For a Ø10 mm reamer in mild steel at 10 m/min, that gives about 318 rpm. Round to a clean value the controller will accept, then verify the actual feed per tooth.

The margin of a reamer is the cylindrical land just behind the cutting edge. It rubs the hole wall by design, which is what gives the size and finish. If the surface speed is too high, the margin heats up, the hole grows, and the finish degrades. If it is too low, the reamer burnishes and the wall work-hardens.

When in doubt, start low and step up in small increments. Run one or two holes, measure the diameter, then raise rpm by 10–15 percent and run again. Stop increasing once the size starts to drift or the surface roughness turns patchy. That is the practical ceiling for that tool and material.

• 1
  Carbon / alloy steel6–15 m/min surface speed.
• 2
  Aluminium / brass10–20 m/min.
• 3
  Stainless / titanium / Inconel4–8 m/min.
• 4
  Formularpm = (1000 × surface speed) / (π × diameter).

Oversize holes usually trace back to runout or too much stock. Check the holder TIR first, then confirm the allowance. If both are correct, the reamer may be cutting on the margin because the surface speed is too high. Reduce rpm and re-measure.

Undersize holes are less common and often come from spring-back in stainless or from a worn reamer. Measure the reamer diameter with a micrometer before blaming the program. A tool that has lost 0.01 mm will never hold a tight H7 fit.

Poor surface finish with an on-size hole points at feed that is too light, coolant that is not reaching the cutting edge, or a retract that is too fast. Increase feed slightly, confirm flood coverage, and make sure the pull-out uses the programmed feed rate.

Chatter shows up as a spiral pattern on the wall. It comes from a long reamer, a weak holder, or a spindle speed that matches a natural frequency of the setup. Shorten the gauge length, switch to a stiffer holder, and shift rpm by 10 percent to break the resonance.

• 1
  OversizeCheck runout, allowance and surface speed, in that order.
• 2
  UndersizeMeasure the reamer, then check spring-back in stainless.
• 3
  Rough wallFeed too light, coolant starved, or retract too fast.
• 4
  ChatterShorten overhang, stiffen the holder, shift rpm by 10 percent.