CNC Reaming Calculator

Calculate recommended spindle speed (RPM), feed rate (IPM), stock allowance per side, and cycle time for precision reaming. Covers HSS and carbide reamers across 14 common workpiece materials with hole tolerance guidance.

Free Tool · RPM & Feed · Stock Allowance · HSS & Carbide · H6/H7/H8 Tolerance · Inch & Metric

Units

Reamer & Material

Reamer Diameter

⌀ in

Workpiece Material

MAT

Reamer Type

Operation Details

Hole Depth

Number of Holes

# holes

Tolerance Class Target

ISO

H7 is most common for shaft/bearing fits. H6 requires more care with stock allowance and coolant.

Results

Spindle Speed

—

RPM

Feed Rate

—

IPM

Stock / Side

—

Pre-Drill Size vs. Reamer Size

Reamer ⌀

0.5000 in

Pre-drill ⌀

0.4840 in

Stock / side

0.0080 in

RPM

—

from SFM

Feed Rate

—

IPM

Feed per Rev

—

in/rev

Cutting Speed

—

SFM

Pre-Drill Dia

—

before reaming

Cycle Time (all holes)

—

total cut time

Ready Select reamer diameter and material, then click Calculate.

Detailed Summary

Reamer Parameters
Reamer diameter	—
Reamer type	—
Workpiece material	—
Tolerance class	—
Speeds & Feeds
Cutting speed (SFM)	—
Spindle speed (RPM)	—
Feed per revolution	—
Feed rate	—
Stock Allowance
Stock allowance per side	—
Total stock on diameter	—
Pre-drill / bore diameter	—
Cycle
Hole depth	—
Number of holes	—
Cycle time per hole	—
Total cycle time	—

Reaming Cross-Section — Stock Allowance & Reamer Geometry

Reaming removes a small amount of stock (allowance per side) left from the pre-drill or boring operation. Too little stock causes chatter and poor finish; too much stock overloads the reamer and produces oversized holes.

How CNC Reaming Parameters Are Calculated

Reaming is a precision sizing operation — not a material removal operation. The reamer follows the existing hole geometry and removes only a thin layer of stock to bring the hole to final diameter with tight tolerance (H6–H8) and good surface finish (Ra 32–125 µin). Getting the stock allowance, speed, and feed right is critical: too little stock causes the reamer to rub and chatter; too much overloads the cutting edges and produces oversized, tapered holes.

1 Cutting Speed (SFM)

Reamers run at much lower speeds than drills or endmills — typically 25–40% of the drilling speed for the same material. Higher speeds cause the reamer to generate heat, which expands the tool and produces oversized holes. HSS reamers run slower; carbide reamers can run 2–3× faster.

Spindle Speed: RPM = (SFM × 3.82) / D [inch] RPM = (Vc × 1000) / (π × D) [metric] D = reamer diameter SFM typical ranges (HSS): Aluminum: 150–250 SFM Mild steel: 40–60 SFM Stainless: 25–40 SFM Cast iron: 50–70 SFM Titanium: 15–25 SFM Carbide factor: multiply SFM × 2.5–3×

2 Feed Rate

Reamers use a feed per revolution (IPR) that is much higher than drills — typically 3–5× the drilling feed for the same diameter. High feed rate prevents the reamer from "spinning in place" and rubbing. The IPM feed rate is IPR × RPM.

Feed per Revolution (IPR): fpr = D × feed_factor feed_factor typical (HSS): Aluminum: 0.012–0.018 /in of D Steel: 0.004–0.007 /in of D Stainless: 0.003–0.005 /in of D Cast iron: 0.005–0.008 /in of D Feed Rate (IPM): IPM = fpr × RPM Example (D=0.5", steel, 50 SFM): RPM = (50 × 3.82) / 0.5 = 382 fpr = 0.5 × 0.005 = 0.0025 in/rev IPM = 0.0025 × 382 = 0.955 IPM

3 Stock Allowance

Stock allowance (per side) is the material left by the pre-drill or bore for the reamer to remove. It must be enough to allow all cutting edges to engage, but not so much that cutting forces exceed the reamer's design limits.

Stock Allowance per Side: stock = D × material_factor Typical factors: Aluminum: 0.010–0.020 per inch D Steel: 0.004–0.007 per inch D Stainless: 0.003–0.005 per inch D Cast iron: 0.005–0.008 per inch D Pre-drill diameter: D_predrill = D_reamer − 2 × stock Example (D=0.500", steel): stock = 0.500 × 0.006 = 0.003" D_predrill = 0.500 − 2×0.003 = 0.494" → use 31/64" drill

4 Tolerance Classes

ISO hole tolerance classes define the allowable deviation from nominal diameter. H7 is the most common — it fits standard bearing and shaft fits. H6 requires tighter process control. H8 is used for general clearance fits where some variation is acceptable.

ISO Hole Tolerance (approx. for ½"): H6: +0.000 / +0.0004" (±0.0002") H7: +0.000 / +0.0008" (±0.0004") H8: +0.000 / +0.0014" (±0.0007") H7 rules of thumb: - Stock allowance: 0.5–1.5% of D - Coolant required: yes (steel/SS) - Floating holder: recommended - Reamer quality: premium ground H6 adds: - Tighter stock control (bore, don't drill) - Temperature-controlled shop preferred - Measure with air gauge or bore gauge

Never Reverse a Reamer — The #1 Reaming Mistake

Reversing a reamer (running it back out of the hole in reverse rotation) is the fastest way to destroy a precision reamer. The cutting edges are designed to cut in one direction only. Reversing causes them to drag across the newly finished bore surface, creating built-up edge, chipping the flutes, and ruining the hole finish. Always retract the reamer in the forward (cutting) direction — program G85 (boring/reaming cycle) rather than G73 (peck drill cycle). On manual machines, keep the spindle rotating forward while retracting by hand or use the quill.

Worked Examples

🔵 ½" H7 in Mild Steel

Dia: 0.500" (HSS reamer) Material: Mild Steel 1018 Target: H7 tolerance SFM: 50 feed factor: 0.005 Depth: 1.5", 4 holes

RPM = 382 IPM = 0.96
Stock/side = 0.0025"
Pre-drill = 0.4950"

Pre-drill with 31/64" (0.4844") or spot bore to 0.4950". Use flood coolant. Cycle time ≈ 9.4 sec per hole.

🔵 12mm H7 in Aluminum

Dia: 12mm (carbide reamer) Material: Aluminum 6061 Target: H7 tolerance Vc: 500 m/min (carbide) Depth: 25mm, 6 holes

RPM = 13,263 mmpm = 2,387
Stock/side = 0.18mm
Pre-drill = 11.64mm

Carbide reamer runs 2.5× faster than HSS. High feed essential — never "nibble" aluminum with a reamer. Pre-drill with 11.5mm twist drill.

🔵 ¾" H7 in Stainless 304

Dia: 0.750" (HSS reamer) Material: Stainless 304 Target: H7 tolerance SFM: 35 feed factor: 0.004 Depth: 2.0", 2 holes

RPM = 178 IPM = 0.53
Stock/side = 0.0030"
Pre-drill = 0.7440"

Stainless requires slow speed, adequate feed, and heavy flood coolant. Never dwell — keep the reamer moving or it will work-harden the bore wall.

Reaming Speed & Feed Reference Table

Material	HSS SFM	Carbide SFM	Feed Factor (/in D)	Stock/Side Factor	Coolant
Aluminum 6061/7075	150–250	400–600	0.012–0.018	1.0–2.0%	Flood or air blast
Aluminum Cast	100–180	300–500	0.010–0.015	0.8–1.5%	Flood or dry
Mild Steel 1018	40–60	120–180	0.004–0.007	0.4–0.7%	Flood (soluble oil)
Alloy Steel 4140	30–50	90–150	0.003–0.006	0.3–0.6%	Flood (sulfurized)
Free-Machining 12L14	60–80	180–240	0.006–0.009	0.5–0.8%	Flood
Stainless 304/316	25–40	75–120	0.003–0.005	0.3–0.5%	Heavy flood
Gray Cast Iron	50–70	150–210	0.005–0.008	0.4–0.7%	Dry or air blast
Titanium Ti-6Al-4V	15–25	45–75	0.002–0.004	0.2–0.4%	High-pressure flood
Inconel 718	10–20	30–60	0.0015–0.003	0.15–0.3%	Heavy flood
Copper / Brass	70–100	210–300	0.007–0.010	0.6–1.0%	Dry or light oil

Frequently Asked Questions

For H7 and tighter tolerances, a floating (self-aligning) reamer holder is strongly recommended. A floating holder compensates for minor misalignment between the machine spindle and the pre-drilled hole center — even a few thousandths of runout in a rigid holder will cause the reamer to cut oversize or produce a bell-mouthed hole. For H8 tolerance work, rigid holders are acceptable if spindle runout is under 0.0002". On CNC machining centers with well-maintained spindles and accurate toolholding (shrink fit, hydraulic chuck), rigid holding can work for H7 if the pre-drill was made in the same setup and runout is controlled.

Common causes of oversized reamed holes: (1) Cutting speed too high — heat expands the reamer and the hole springs back after cooling, reading oversize; (2) Too much stock allowance — excessive material forces the reamer outward; (3) Spindle runout or tool runout — a reamer running with even 0.001" TIR will cut 0.002" oversize; (4) Wrong coolant or no coolant — especially in steel and stainless, thermal expansion is significant; (5) Worn reamer — a worn reamer tends to "plow" and cut oversize due to rubbing; (6) The part or fixture is not fully clamped — vibration causes the hole to open up. Measure the reamer's actual diameter with a micrometer before blaming the process — new reamers from questionable suppliers are sometimes already undersize or have excessive runout.

Yes — and for H6 and tight H7 work, boring before reaming is preferred over drilling. A boring bar produces a better-located, more accurately sized, and rounder pre-hole than a drill. This means the reamer has less work to do, removes more uniform stock around the circumference, and produces a more consistent result. The bored pre-hole should be left with 0.003–0.008" stock on diameter (not per side) for final reaming. Drilling directly followed by reaming is acceptable for H8 and general H7 work in softer materials like aluminum, but boring + reaming is the correct process for high-precision fits in steel and stainless.