Milling Calculator

Compute spindle speed, feed rate, metal removal rate, and optimize cutting parameters for milling operations.

Alu: 200–600, Steel: 80–200
Aluminium (7075)
Carbon steel (P20)
Stainless 316
Titanium Ti6Al4V
Cast iron (rough)
Calculating...

Understanding Milling Parameters

Milling is a fundamental machining process where a rotating multi-tooth cutter removes material. Correct cutting parameters ensure productivity, surface quality, and tool life. Below we explain each variable and its practical significance.

Core equations (ideal conditions):

n (rpm) = (Vc × 1000) / (π × D)

Vf (mm/min) = fz × Z × n

Q (cm³/min) = (ap × ae × Vf) / 1000

where D = tool diameter (mm), Vc = cutting speed (m/min), fz = feed per tooth (mm), Z = number of teeth, ap = axial depth (mm), ae = radial depth (mm).

Cutting Speed (Vc)

Cutting speed is the relative velocity between the tool periphery and the workpiece. It primarily affects tool wear and thermal load. Recommended Vc depends on tool material (HSS, carbide, ceramic) and workpiece material. Higher Vc increases productivity but accelerates flank wear. For carbide tools in aluminium, Vc can reach 600 m/min; in heat-resistant alloys, it may drop below 40 m/min.

Feed per Tooth (fz) and Chip Load

fz determines the chip thickness. Too low fz causes rubbing and work hardening (especially in stainless steels); too high leads to excessive cutting forces or tool breakage. Typical fz for carbide end mills ranges from 0.02 to 0.2 mm/tooth, depending on tool diameter, material, and operation (roughing vs. finishing).

Axial (ap) and Radial (ae) Depth of Cut

ap is the depth in the tool axis direction, ae is the width of cut perpendicular to the tool axis. The product ap×ae defines the engagement area. Together with Vf they determine the metal removal rate Q. In high-performance milling (HPC), large ap and moderate ae are used; in high-speed machining (HSM), small ae and high Vc & Vf are common.

Material-specific Recommendations

Values below are typical for carbide tools (coated/uncoated) and may vary with tool geometry, coating, and machine rigidity. Always consult tool manufacturer's catalogue.

Material group Vc carbide (m/min) fz (mm/tooth) for D=12mm Example alloys
Aluminium (wrought) 300–800 0.10–0.25 6061, 7075
Carbon steel (<300 HB) 120–250 0.08–0.18 A36, 1045
Alloy steel (300–400 HB) 70–150 0.05–0.12 4140, 4340
Stainless steel (austenitic) 60–120 0.04–0.10 304, 316
Titanium alloys 30–60 0.02–0.08 Ti6Al4V
Cast iron (grey) 150–300 0.12–0.30 GJL250

Data compiled from Sandvik Coromant, Seco Tools, and Machinery's Handbook (31st ed.).

Metal Removal Rate (MRR) & Power

MRR (Q) directly correlates with machining time. However, it is limited by available spindle power and cutting forces. A rough estimate of net power required at the spindle: Pc (kW) = (Q × kc) / 60, where kc is specific cutting force (N/mm²). For aluminium kc ≈ 800, for steels 2000–3000. The calculator uses a typical kc = 2500 for steel/alloy approximation; actual values may differ.

Case Study: Pocket Milling in 7075 Aluminium

Operation: Rough pocketing with 16 mm carbide end mill (Z=4). Target: maximum MRR while respecting 10 kW spindle power.
Initial guess: Vc=500 m/min, fz=0.15 mm, ap=8 mm, ae=12 mm.
Calculation: n = (500×1000)/(π×16) ≈ 9947 rpm, Vf = 0.15×4×9947 ≈ 5968 mm/min, Q = (8×12×5968)/1000 ≈ 573 cm³/min. Power ≈ 573×800/60 ≈ 7.6 kW → within limit.
Result: Efficient roughing. Adjust ae if chatter occurs.

Relation to Other Process Parameters

  • Surface finish: Higher fz leaves rougher finish; finishing passes use reduced fz and ae.
  • Tool wear: Vc has strongest influence on tool life (Taylor's equation).
  • Chatter: Stability depends on ae, n, and system dynamics; sometimes reduce ae to avoid vibrations.

Common Mistakes & How to Avoid Them

  • Ignoring tool runout: Can increase effective fz on one tooth; reduce fz to compensate.
  • Using too low Vc for HSS tools: HSS requires lower Vc (20–60 m/min).
  • Not adjusting for radial engagement: For small ae ( < 0.5×D ), chip thinning occurs; may need to increase fz to maintain chip load. This calculator uses nominal fz; advanced users should apply chip thinning correction.

Historical Note & Standards

The fundamental relationships have been used since the early 20th century. The International Organization for Standardization (ISO) defines symbols in ISO 3002 (cutting geometry). Modern CNC controls use these formulas in their cycles. Machinery's Handbook (31st edition) provides extensive tables.

Frequently Asked Questions

Start from tool manufacturer's recommendations. General ranges: carbide in aluminium 300–600 m/min, in steel 100–250 m/min. Reduce for harder materials or when tool overhang is large.

Feed per revolution f = fz × Z. It is the distance the table moves in one spindle revolution. Feed per tooth is more fundamental because each tooth produces a chip. For milling, fz is used to calculate chip thickness.

When ae < 0.5×D, the maximum chip thickness (hex) becomes less than the programmed fz due to chip thinning. To maintain constant hex, fz should be increased proportionally. For simplicity, this calculator does not apply chip thinning; for critical applications use adjusted feed.

In aluminium, 50–150 cm³/min is achievable; in steel, 10–40 cm³/min. It depends on machine power, tool holder, and stability.

If required n exceeds machine limit, you must reduce Vc or increase D. Alternatively, use a tool with more teeth to keep Vf high while lowering n.

The specific cutting force kc varies with material, tool wear, and chip thickness. The value 2500 N/mm² is a typical average for medium steel. For better accuracy, use kc from your tool catalogue.
References: Oberg et al. "Machinery's Handbook" 31st ed.; Sandvik Coromant "Metal Cutting Technology Training"; ISO 3002-1. Values from Seco Tools and Kennametal technical data (2025). All recommendations are for guidance; actual results may vary.