Reaming Techniques: Pre-Drilled Hole, Spindle Speed, Feed and Cycle Time Calculation
Reaming is a finishing operation that brings a previously drilled hole to a precise size, better roundness and a smoother surface. A successful result depends not only on the reamer diameter, but on evaluating the stock allowance left in the pre-drilled hole, tool runout, hole type, cutting speed, feed, coolant and clamping rigidity together.
The calculator at the end of the page takes a few basic inputs and computes the recommended pre-drilled hole range, cutting speed, machine spindle speed, feed per revolution or per tooth, feed per minute, metal removal rate and approximate time.
What reaming can and cannot correct
A reamer removes a small, balanced amount of stock to bring the hole to its final size. It is not designed to straighten from scratch a hole that is seriously off-axis, bent or cut with excessive taper. The position and accuracy of the pre-drilled hole are the foundation of the reaming result.
How the reamer affects size and surface
Brings the hole to final diameter
The multi-flute cutting geometry removes the small stock allowance left by the drilling or boring operation. The reamer diameter, cutting edge condition and tool runout determine the actual hole size.
Improves roundness and cylindricity
Geometries such as unequal flute spacing can reduce vibration marks. However, if the pre-drilled hole has a large axis error, the reamer may follow that error or deflect under side load.
Produces a fine finished surface
Correct stock allowance and feed create a true cut. Too little stock or an unnecessarily low feed can lead to rubbing instead of cutting, causing built-up edge and rapid wear.
IT7 and H7 are not the same thing
IT7 denotes the tolerance grade; H7 combines the hole's tolerance zone with the IT7 grade. A catalog stating "IT7 or H7 achievable" does not mean H7 will be obtained automatically on every part. The Hole Tolerances: IT Grades Calculator shows how many microns an IT grade is at a given diameter.
- Tool runout and holder cleanliness
- Actual diameter and accuracy of the pre-drilled hole
- Workholding and wall rigidity
- Cutting fluid reaching the cutting zone
- Tool wear and measurement temperature
Choose the reamer type based on hole, material and production style
Flexible and general purpose
Usable in low- and medium-speed applications, on less rigid machines and in small-batch production. Because cutting data varies greatly with the tool's coating, cobalt content and geometry, entering catalog values in the calculator is recommended.
Precision and high productivity
With rigid clamping and low runout, it delivers high cutting speed and consistent hole quality. Both standard multi-purpose and material-optimized geometries are available.
Large diameters and high feed
Special head geometries can suit high feed rates, cross holes and angled surfaces in steel and some cast irons. Since feed per tooth is used, the flute count must be known.
System with size compensation
Small diameter adjustments can be made for wear and target size. The adjustment amount, equal loading of the cutting edges and the manufacturer's procedure must be followed precisely.
Special hole form and finish
Special geometries such as the K10 gun reamer must not be calculated with the standard solid-carbide reamer table. Cutting data, stock allowance and toolpath must come only from the tool's own manufacturer data.
Compensates small axis misalignment
Especially in lathe and transfer-machine applications, it can reduce small alignment errors. However, it is not used to correct a poorly drilled pre-hole or large misalignment.
Flute logic for through, blind and interrupted holes
General selection logic
Through hole: A flute geometry that carries chips toward the exit is preferred. In some catalog examples, spiral/helical flutes are used for this purpose.
Blind hole: A geometry that carries chips back toward the hole mouth and effective internal coolant are required. Chip packing at the bottom and unnecessary dwell must not be allowed.
Cross or interrupted hole: The cutting edge takes impact loading. Only a robust geometry designed for this application should be used; the same values must not be applied automatically to a standard reamer.
Why the reaming allowance must be neither too small nor too large
The pre-drilled hole diameter determines whether the reamer actually cuts. With too little stock allowance, the cutting edge may burnish and rub the surface. With too much stock allowance, force, heat, hole oversizing and breakage risk all increase.
| Final reamer diameter | General starting diametral stock | Pre-drilled hole example | Note |
|---|---|---|---|
| 3–6 mm | 0.10–0.20 mm | About Ø4.85 for Ø5 | At small diameters, runout and edge sharpness become more critical. |
| 6–12 mm | 0.15–0.30 mm | About Ø9.80 for Ø10 | The common general starting range. |
| 12–20 mm | 0.20–0.40 mm | About Ø15.70 for Ø16 | Hole accuracy and part wall thickness should be checked. |
| 20–32 mm | 0.25–0.50 mm | About Ø24.60 for Ø25 | Tool type, power and radial load become more significant. |
| Special high-feed head | 0.20–0.60 mm diametral | 0.10–0.30 mm radial ap | Only for geometries that explicitly support this range. |
How to select Vc, fn and fz by material
Reamer catalogs usually do not state spindle speed directly. They give cutting speed Vc and feed per revolution fn or feed per tooth fz. The calculator converts this data into machine spindle speed and feed per minute.
| ISO / material | Multi-purpose solid carbide Vc | Material-specific high-performance Vc | Replaceable high-feed Vc |
|---|---|---|---|
| P · Mild/medium steel | 24–36 m/min | 148–222 m/min | 150–200 m/min |
| P · Medium-hard/alloy steel | 16–30 m/min | 112–192 m/min | 70–180 m/min |
| M · Austenitic stainless | Dedicated geometry instead of general table | 32–48 m/min | Application approval required |
| M · Duplex stainless | Dedicated geometry instead of general table | 24–36 m/min | Application approval required |
| K · Gray cast iron | 24–48 m/min | 72–222 m/min | 150–200 m/min |
| K · Ductile/malleable iron | 24–36 m/min | 72–108 m/min | 110–190 m/min |
| N · Aluminum/copper | 64–96 m/min | Verify by geometry | No general automatic value |
| S / H · Heat-resistant or hardened material | Enter current tool-specific catalog values; no automatic value is used. | ||
The wide ranges in the table show that different reamer geometries have very different productivity levels. The value for a multi-purpose reamer must not be transferred to a special high-feed geometry.
Example feed series by diameter
| Feed type | Ø3 | Ø5 | Ø8 | Ø10 | Ø12 | Ø16 | Ø20 |
|---|---|---|---|---|---|---|---|
| Standard fn, mm/rev | 0.16 | 0.20 | 0.27 | 0.32 | 0.36 | 0.41 | 0.47 |
| Hard/unstable condition fn | 0.11 | 0.15 | 0.18 | 0.21 | 0.24 | 0.28 | 0.31 |
| Aluminum/copper fn | 0.18 | 0.25 | 0.35 | 0.39 | 0.43 | 0.50 | 0.53 |
| Special high-feed fn | 0.30 | 0.70 | 1.00 | 1.00 | 1.50 | 1.50 | 1.50 |
| Replaceable head fz | 0.10–0.25 mm/tooth · fn = fz × flute count | ||||||
How to calculate reamer speed, feed and time
Reamer pre-drilled hole, speed, feed and time calculation
Enter only the required values on the main screen. If your tool catalog gives Vc, fn or fz, enter them under "Advanced values" to override the automatic starting value.
Calculate the reaming operation
Generates speed and feed from final diameter, pre-drilled hole, tool type and material; the time calculation is optional.
General G85 training example
The program template appears here once the calculation is complete.
Control warning: The entry, bottom, feed-rate retract and G98/G99 behavior of the G85 cycle can vary between control units. The program must not be run on a part before verification with graphics, a dry run, single block and reduced feed.
Reaming checklist for the operator
Prepare the pre-drilled hole
Measure the actual pre-drilled hole diameter. Do not try to force-correct axis, taper or surface errors with the reamer. Leave a suitable chamfer at the entry.
Clean the tool and holder
Clean the collet, hydraulic holder, clamping surfaces and spindle taper. Clamp the tool as short as possible and measure the runout.
Deliver the cutting fluid
Direct a high-lubricity fluid straight into the cutting zone. In blind holes, prevent chips from staying at the bottom and being re-cut.
Measure and optimize
Machine the first part with controlled values. Measure hole diameter, taper, roundness and surface, and change only one parameter at a time in small steps.
Quick troubleshooting
| Symptom | Probable causes | Checking order |
|---|---|---|
| Hole comes out oversize | Tool runout, built-up edge, high Vc, axis misalignment, edge damage | Clean the holder, measure runout, inspect the edges; then review Vc and lubrication. |
| Hole undersize or tapered | Worn tool, excessive stock allowance, part springback, insufficient cutting fluid | Measure the pre-drilled hole and stock allowance; check tool wear and wall rigidity. |
| Scratched surface | Chip re-cutting, poor lubrication, dwell at bottom, wrong flute direction | Check chip evacuation and coolant outlet; remove unnecessary dwell. |
| Tool chatters | Long overhang, rubbing at low feed, weak clamping, uneven load | Reduce the overhang, correct the runout and move the feed into the manufacturer's range in small steps. |
| Reamer breaks | Chip packing in blind holes, excessive stock, wrong geometry for interrupted holes, misaligned pre-hole | Stop the operation; re-verify the hole type, stock, tool application limits and coolant. |