CNC Drilling Cutting Parameters and Formulas

CNC Drilling Cutting Parameters and Formulas: Complete Technical Guide

A Mentor CNC technical guide covering all drilling optimization calculations — from cutting speed, feed, force and power formulas to the Taylor tool-life equation, material-specific parameters and feed calibration.

🇹🇷 Bu rehberi Türkçe okuyun

Introduction: The Critical Importance of Drilling

Drilling is one of the most frequent operations on CNC lathes and mills. Success in this high-efficiency, high-quality, high-precision operation depends on selecting the right cutting parameters. This guide covers drilling parameters through international standards (ISO 513, ISO 3685) and the Mentor CNC engineering approach. For drilling methods and tool systems, see our CNC Drilling Cutting Tools Guide; this article focuses on cutting parameters and formulas.

Automotive: Engine block and cylinder-head holes.
Die and mold: High-precision location holes.
Aerospace: Clean holes in titanium and aluminium alloys.
General mechatronics: Fast production of standard components.

With correct parameters it is possible to increase tool life 2–3× and raise production speed by 30–50%.

1. Cutting Speed (V_c) and Spindle Speed (n)

Cutting Speed / Spindle Speed

V_c = (π × D_c × n) / 1000 ↔ n = (V_c × 1000) / (π × D_c)

V_c: cutting speed (m/min), D_c: drill diameter (mm), n: spindle speed (rpm).

✓ ExampleØ10 mm hole in S235 steel, target V_c = 50 m/min → n = (50 × 1000)/(π × 10) = 1592 rpm. Set ≈ 1600 rpm on the machine.

2. Feed (f)

Feed is selected by hole diameter, tip geometry and material. The values below are a starting reference for standard tools.

Table 1: Recommended Feed by Hole Diameter (mm/rev)

Hole Diameter	Steel	Stainless	Nodular Cast Iron	Aluminium
Ø 3–5 mm	0.05–0.08	0.03–0.06	0.08–0.12	0.10–0.15
Ø 5–10 mm	0.08–0.15	0.06–0.12	0.12–0.18	0.15–0.25
Ø 10–20 mm	0.15–0.25	0.12–0.20	0.18–0.28	0.25–0.40
Ø 20–50 mm	0.25–0.50	0.20–0.40	0.28–0.50	0.40–0.60

3. Calculating Cutting Force and Power

Cutting Force (simplified estimate) and Power

F_c ≈ (f × D_c × k_c) / 2 | P_c = (F_c × V_c) / (60 × 1000) [kW]

f: feed (mm/rev), D_c: diameter (mm), k_c: specific cutting force (N/mm²), V_c: cutting speed (m/min). F_c is an approximation; verify on the machine.

Table 2: Specific Cutting Force (k_c) of Common Materials

Material	k_c (N/mm²)	Property
Steel S235	800–1000	Low carbon, easy to machine
Steel S355	1200–1500	High strength, medium difficulty
Stainless 1.4404 (316L)	1500–1900	Work-hardening, heat issue
Nodular Cast Iron GGG40	600–800	Low plasticity, brittle chip
Aluminium 2024-T4	400–600	Low force, high feed
Titanium Grade 5 (Ti-6Al-4V)	1800–2200	Very high temp, special tools

✓ Worked exampleS235 (k_c ≈ 900), Ø12 mm, f = 0.20 mm/rev, V_c = 60 m/min: F_c = (0.20 × 12 × 900)/2 = 1080 N. n = (60×1000)/(π×12) = 1592 rpm. P_c = (1080 × 60)/(60×1000) = 1.08 kW.

4. Tool Life: The Taylor Equation

Tool life drops rapidly as cutting speed increases. This is expressed by the Taylor tool-life equation:

Taylor Tool-Life Equation

V_c × Tⁿ = C ⇒ T = (C / V_c)^1/n

T: tool life (min), C: material constant, n: exponent (typically 0.15–0.35 for carbide). This is the correct form; writing “T = C/V_cⁿ” is incorrect.

Practical result: a 20% increase in cutting speed can cut tool life by 40–50%. Choose the economical cutting speed that yields the lowest cost.

5. Tool Selection for Drilling

Table 3: Tool Selection by Diameter and Operation

Hole Diameter	Operation	Tool Type	Material	Recommendation
Ø 3–8 mm	Roughing	Twist drill	HSS / carbide	High rpm, low feed
Ø 8–20 mm	Roughing	Solid carbide drill	Carbide (WC)	2–3× longer life
Ø 5–15 mm	Precision	Coated drill	HSS / coated	Reduces thrust force
Ø 10–50 mm	Fine machining	Reamer / boring bar	Carbide + coating	±0.05 mm tolerance
Ø 20–100 mm	Roughing	Indexable-insert drill	Carbide	Solves vibration

6. Material-Specific Cutting Parameters

6.1. Steels

S235 (low carbon): V_c 40–80 m/min, f 0.08–0.20 mm/rev; mineral oil + emulsion.
S355 (high strength): V_c 25–50 m/min (lower), f 0.06–0.15; intensive cooling needed.
Stainless 316L (1.4404): V_c 15–35 m/min (very low!), f 0.05–0.12. Critical issue is work hardening; continuous feed, no vibration, sharp tool and intensive cooling are essential.

6.2. Aluminium Alloys

Al 2024-T4: V_c 100–150 m/min (high), f 0.15–0.40 mm/rev. Fast machining, low force. Chip formation is critical; helical geometry matters for good evacuation.

6.3. Nodular Cast Iron (GGG)

GGG40: V_c 30–60 m/min, f 0.10–0.25 mm/rev. Brittle chip, risk of tool impact; use vibration-dampening holders and low runout (eccentricity).

6.4. Titanium Alloys

⚠ Ti-6Al-4V (Grade 5)V_c 10–25 m/min (very low!), f 0.05–0.10 mm/rev (very small). 900–1000°C in the cutting zone; flood cooling is mandatory and TiAlN-coated tools are required. HSS tools fail — always use carbide/coated tools.

7. Effect of Parameters

Higher cutting speed: (+) machining rate/capacity; (−) tool life and surface quality. An economic optimum is needed.
Higher feed: (+) production rate; (−) thrust force and surface quality. Check the spindle’s axial force capacity.
Coolant: mineral oil → steel/stainless (good lubrication); synthetic emulsion → cast iron (good cooling); air → aluminium (chip evacuation).

8. Precision Drilling (±0.05 mm)

1. Roughing: V_c 70–80% of nominal, normal feed. Goal: remove residual stress and deviation.
2. Semi-finishing: V_c 80–90%, feed 80%. Special reamer (leave 0.05–0.10 mm stock).
3. Fine reaming: V_c 40–50% (very low), feed 50–60%; calibrated reamer, vibration control.

Conditions for tolerance success: spindle vibration < 0.05 mm; holder runout (eccentricity) < 0.02 mm; stable, sufficient clamping pressure; clean, steady coolant flow.

9. Common Problems and Solutions

Table 4: Drilling Problems

Problem	Symptom	Cause	Solution
Hole Deviation	Ø12 hole comes out Ø12.3–12.5.	Low speed, high feed, spindle runout.	Raise speed, reduce feed, spindle maintenance; pilot hole.
Poor Surface Quality	R_a > 3.2 µm.	Dull tool, low cooling, low rpm.	Change tool, increase cooling/rpm.
Tool Breakage	Sudden tip fracture.	High feed, vibration, spindle issue.	Reduce feed, find vibration source, check spindle.
Crater Wear	Cavity on the tip rake face.	High temperature, insufficient cooling.	Reduce speed, increase cooling, check coating match.
Chatter	Chatter noise, high-frequency vibration.	Low holder rigidity, high speed, part deflection.	Change holder, reduce speed, clamp part closer.
Flank Wear	Hole diameter grows, edge degrades.	High temperature, excess feed.	Increase cooling, reduce feed, change tool material.
No Chip Formation (stainless)	Very thin/curled chip, high temperature.	Work hardening, low feed.	Increase feed, slightly reduce speed, sharp tool.

10. Insert Coating Strategy

Modern tips are made of coated carbide or ceramic. The right coating can increase tool life 2–3×.

Table 5: Common Coating Types

Coating	Color	Temperature	Application
TiN (titanium nitride)	Gold	< 600°C	Steel, aluminium; good lubricity
TiAlN (titanium aluminium nitride)	Purple/grey	< 900°C	High temp, stainless; high hardness
CrN (chromium nitride)	Silver	< 700°C	Cast iron, aluminium; low adhesion
PVD multilayer	Mixed	< 1000°C	Precision work; long life, stable heat

Selection: S235 → TiN is enough; S355 + stainless → TiAlN needed; titanium → TiAlN + intensive cooling; aluminium → the key is feed and chip evacuation.

11. Feed Calibration

The actual feed can differ from the programmed value by 10–20%. It can be verified with a simple test hole:

Actual Feed (calibration)

f_actual = L / (n × t) [mm/rev]

L: hole length (mm), n: spindle speed (rpm), t: measured time (minutes). If using seconds: f = L × 60 / (n × t_sec).

⚠ Corrected exampleProgrammed f = 0.15 mm/rev, n = 2000 rpm, L = 20 mm. Theoretical time: 20/(0.15×2000) = 0.0667 min ≈ 4 s. Measured: 5 s. Actual feed: 20 × 60 / (2000 × 5) = 0.12 mm/rev — i.e. the machine feeds ~20% slower than programmed (0.12 vs 0.15). Note: the source text mistakenly gave “2.0 mm/rev”, which is physically impossible — if the time increased, the actual feed decreases.

Conclusion: Optimal Drilling Strategy

Table 6: Job Start Checklist

Check	Method	Failure Criterion
Spindle vibration	Vibration meter, Ø10 test hole	> 0.05 mm
Holder runout (eccentricity)	Dial indicator, rotate tool	> 0.02 mm
Workpiece clamping	Clamp, deflection test	Deflection > 0.1 mm
Coolant	Color, consistency, pH	Dark color, oil separation
Tip condition	Visual / microscope	Chip, wear, notch
Parameter accuracy	Program check, test cut	Wrong F, S values

Table 7: Optimum Parameters by Material Group (Ø5–20 mm)

Material	V_c (m/min)	f (mm/rev)	Expected Life	Cooling
Low-carbon steel	50–80	0.12–0.20	100–150 holes	Mineral oil
High-strength steel	25–50	0.08–0.15	50–100 holes	Intensive emulsion
Stainless steel	15–35	0.05–0.12	20–50 holes	Flood
Nodular cast iron	30–60	0.10–0.25	80–120 holes	Air / oil
Aluminium alloy	100–150	0.15–0.40	200–300 holes	Air / emulsion
Titanium alloy	10–25	0.05–0.10	30–80 holes	Flood (mandatory)

Efficiency Tips

Feed first: optimize feed for output first; tool choice second.
Combine operations: do roughing + precision in one setup; reduce tool changes.
Coolant management: dirty fluid cuts life 20–30%; check filters weekly.
Planned tool change: replace before breakage, monitoring thrust force.
Program order: drilling small to large balances forces.
Pilot hole: reduces wander by 50–60% where needed.

Quick Reference Formulas

n = V_c×1000/(π×D_c) | V_c = π×D_c×n/1000 | P_c = F_c×V_c/60000 | F_c ≈ f×D_c×k_c/2 | T_mach = L/(f×n)

T_mach: machining time (min), L: hole length (mm). V_c×Tⁿ=C (Taylor).

Success in drilling depends not on a single parameter but on the whole system: correct tool/coating, formula-based parameters, solid clamping, regular cooling and pilot testing. This guide summarizes Mentor CNC’s knowledge in light of the ISO 513 and ISO 3685 international standards and industrial practice; always verify parameters against your own material and machine conditions. Continue with the CNC Drilling Cutting Tools Guide and the Cutting Tools category.

CNC Drilling Cutting Parameters and Formulas: Complete Technical Guide