CNC Drilling Cutting Tools: Methods, Cutting Conditions and Optimization Guide
A Mentor CNC technical guide — from solid carbide and indexable-insert drills to step, chamfer, adjustable-bar and peck drilling — with cutting-condition formulas, material strategies and worked engineering scenarios.
🇹🇷 Bu rehberi Türkçe okuyun
Introduction: The Industrial Importance of Drilling
Drilling is one of the most frequent operations on CNC lathes and machining centers. Correct choice of material grade, tool geometry and cutting conditions directly affects the final part’s tolerance and surface quality. This guide covers every stage of drilling with a Mentor CNC engineering approach, grounded in international standards such as ISO 513 (cutting-tool classification) and ISO 3685 (tool-life testing). Formulas and practical tips are given so you can adapt them to your own machine and material.
1. Drilling Methods
1.1. Classic Drilling (Twist Drill / Solid Drill)
The most basic and common method. A twist drill with two cutting edges forms the hole through rotation and axial feed.
- Advantages: Simple standard tools, easy sourcing, low cost and wide material compatibility.
- Disadvantages: Chip evacuation is harder at high L/D; tight-tolerance holes may need extra reaming/boring.
- Application: General-purpose holes and pilot-hole operations.
1.2. Stepped Drilling
A single tool with cutting edges of different diameters opens several diameter steps in one operation (e.g. hole + chamfer, or hole + widening in one plunge). Achievable tolerances are typically IT8–IT10; solid carbide precision drills improve this to IT7–IT8.
| Hole Diameter (mm) | Depth (× Dc) | Typical Achievable Tolerance |
|---|---|---|
| 3.00 – 6.00 | 2 – 7 × Dc | IT8 (≈ ±0.02 mm) |
| 6.01 – 10.00 | 2 – 5 × Dc | IT8 (≈ ±0.02 mm) |
| 10.01 – 14.00 | 2 – 5 × Dc | IT9 (≈ ±0.03 mm) |
| 14.01 – 17.00 | 2 – 5 × Dc | IT9 (≈ ±0.03 mm) |
| Material | Cutting Speed Vc (m/min) | Feed f (mm/rev) | Coolant |
|---|---|---|---|
| Steel (P) | 70 – 130 | 0.14 – 0.31 | Emulsion |
| Stainless (M) | 40 – 110 | 0.07 – 0.20 | Emulsion |
| Cast Iron (K) | 80 – 120 | 0.15 – 0.25 | Dry / air |
| Aluminium (N) | 250 – 400 | 0.12 – 0.22 | Emulsion |
| Titanium (S) | 25 – 30 | 0.08 – 0.16 | High pressure |
1.3. Chamfering / Countersinking
Creates an angled chamfer/countersink at the hole mouth for recessing bolt heads, easing assembly and removing burrs. It can be done in the same cycle as drilling in a single pass (drill → position countersink tool → cut chamfer).
| Material | Vc (m/min) | f (mm/rev) | Angle |
|---|---|---|---|
| Steel | 20 – 60 | 0.10 | 45° |
| Stainless | 15 – 40 | 0.08 – 0.10 | 45° |
| Aluminium | 50 – 100 | 0.10 – 0.20 | 45° |
| Titanium | 10 – 20 | 0.05 – 0.10 | 45° |
1.4. Adjustable / Eccentric Hole Enlargement (Adjustable Bar)
Radially adjustable systems let the hole diameter be set to micron precision and enlarged beyond the drill diameter. Used for tight tolerances (H7/H8), die and tool making, and automotive precision work.
| Drill Diameter (mm) | Vc (m/min) | f (mm/rev) | Material |
|---|---|---|---|
| 12.00 – 63.50 | 100 – 150 | 0.18 | Steel, stainless |
| 14.00 – 63.50 | 70 – 180 | 0.20 – 0.30 | Steel, cast iron |
| 12.00 – 63.50 | 100 – 150 | 0.10 – 0.20 | Titanium, light alloy |
1.5. Peck and Spot Drilling
Spot drilling: A shallow pilot/center hole to minimize tool deflection at start. Peck drilling: Retracting the tool in steps in deep holes to break and evacuate chips; prevents jamming and tool breakage.
| Coolant | Peck Frequency | Chip Evacuation |
|---|---|---|
| Dry | Every 1–3 mm | Manual |
| Emulsion | Every 2–5 mm | Automatic |
| High pressure | Every 5–10 mm | Automatic |
1.6. Coolant Management
| Material | Coolant | Concentration | Flow |
|---|---|---|---|
| Steel (P) | Oil emulsion | 5–15% | 5–10 L/min |
| Stainless (M) | Precision cutting oil | 5–15% | 8–15 L/min |
| Cast Iron (K) | Dry or air | — | Variable |
| Aluminium (N) | Kerosene/oil mix or emulsion | 10–20% | 10–20 L/min |
| Titanium (S) | High-performance oil | 8–12% | 15–25 L/min |
Selection criteria: effective chip evacuation, tool life, surface quality and cutting-speed stability.
2. Cutting Tool Selection and Geometry
The tool families below are Mentor CNC’s generic drilling systems, organized by ISO 513 application classes (P, M, K, N, S). They can be adapted to your own machine.
| Mentor CNC Tool Series | Purpose | Diameter Range | Depth |
|---|---|---|---|
| MD Series (indexable-insert drill) | General drilling, all material groups | 12.00 – 63.50 mm | 2 – 5 × Dc |
| SC Series (solid carbide drill) | Precision-diameter holes (IT6–IT8) | 0.30 – 20.00 mm | 2 – 7 × Dc |
| BD Series (large-diameter insert drill) | Large-diameter holes, stable cutting | 25.00 – 65.00 mm | 7 – 15 × Dc |
| TR Series (trepanning) | Large diameter, minimum chip volume | 60.00 – 110.00 mm | 2.5 × Dc and above |
| CS Series (countersink/chamfer) | Drill + chamfer in one cycle | 9.50 – 30.40 mm | 3.5 – 5 × Dc |
2.1. Geometry and Grade Selection (ISO 513)
- Long-chip geometry (L): Good chip flow in long/ductile-chipping steels.
- Anti-adhesion geometry (M): Reduces built-up edge (BUE) in stainless.
- Wide corner-radius geometry (R): Fine cutting, good surface quality.
- Wide-angle finishing geometry (T): Low force, fine machining.
- P class (steel): CVD-coated universal carbide — first choice for steel and cast iron.
- M class (stainless): Tough, free-cutting grade — high speed and hardening resistance.
- N class (aluminium): Uncoated/thin-coated sharp grade; alloys up to 12% silicon.
- K class (cast iron): Wear-resistant thick CVD-coated grade.
3. Calculating Cutting Conditions
4. Method Selection: Decision Matrix
| Diameter (mm) | Depth | Recommended Method | Tool System |
|---|---|---|---|
| < 3 | < 10 mm | Classic solid drill | SC Series |
| 3 – 10 | 10 – 50 mm | Stepped / solid carbide | SC Series |
| 10 – 25 | 50 – 150 mm | Indexable insert + chamfer | MD Series |
| 25 – 65 | 150 mm+ | Large-diameter / adjustable bar | BD Series |
| > 65 | 200 mm+ | Trepanning | TR Series |
| Material | Vc (m/min) | f (mm/rev) | Coolant |
|---|---|---|---|
| Steel (P) | 100 – 200 | 0.15 – 0.30 | Emulsion |
| Stainless (M) | 50 – 120 | 0.10 – 0.20 | High concentration |
| Cast Iron (K) | 80 – 150 | 0.15 – 0.25 | Dry / air |
| Aluminium (N) | 300 – 400 | 0.20 – 0.40 | Emulsion |
| Titanium (S) | 25 – 50 | 0.08 – 0.15 | High pressure |
5. Common Problems and Solutions
| Problem | Symptom | Solution |
|---|---|---|
| Built-Up Edge (BUE) | Surface degradation, shorter life, frequent breakage. | Raise cutting speed (+15–20%); change coolant; switch to a sharp/anti-adhesion geometry; reduce feed slightly. |
| Excessive Tool Wear | Fast breakage, rising chip heat. | Reduce cutting speed (−15–20%); check coolant circulation; distinguish wear type (flank / crater). |
| Poor Chip Breaking | Vibration, long/wrapping chips. | Increase peck frequency; balance speed; check holder rigidity and machine axis alignment. |
| Poor Surface Quality | Ra > 1.6 µm, marked surface. | Reduce feed (−20–30%); choose wide-angle finishing geometry (T); check coolant supply. |
6. Engineering Scenarios (Worked Examples)
Scenario 1: Ø16 mm Hole in SAE 1045 Steel
Parameters: SAE 1045 steel, Ø16 mm (H7), depth 40 mm (2.5 × Dc), MD-Series indexable drill (P-class grade), CNC lathe (max 15 kW).
Recommendation: Vc 120 m/min, f 0.20 mm/rev, n 2387 rpm, 10% oil emulsion. Expected Ra ≈ 1.2 µm (suits H7). Note: if a larger diameter or harder material pushes power near the limit, reduce feed first, then cutting speed.
Scenario 2: Chamfered Ø8 mm Hole in 304 Stainless
Parameters: 304 stainless, Ø8 mm (f7), 45° / 3 mm chamfer, MD-Series + CS-Series countersink, kc ≈ 2700 N/mm².
Recommendation: hole Vc 80, chamfer Vc 50 m/min, 10% precision cutting oil; tool check every 50 parts. Expected Ra ≈ 0.8 µm.
7. Advanced Applications
7.1. Demanding Materials (Titanium, Nickel Alloys)
| Material | Vc (m/min) | f (mm/rev) | Cooling |
|---|---|---|---|
| Ti-6Al-4V | 25 – 40 | 0.08 – 0.12 | High pressure (70–100 bar) |
| Hastelloy X | 15 – 30 | 0.06 – 0.10 | High pressure |
| Inconel 718 | 20 – 35 | 0.07 – 0.11 | High pressure |
Tips: reduce vibration at the holder; deliver coolant at 70–100 bar straight to the cutting point; peck every 3–5 mm; monitor tool contact temperature.
7.2. Large-Diameter Holes (Trepanning)
Conclusion: Optimal Drilling Strategy
Drilling is one of the most critical CNC operations. For success: know the material and pick speed/feed/coolant accordingly; select the tool and grade to suit diameter, depth and tolerance; use the formulas to compute parameters within machine capacity; recognize common problems as symptom-solution pairs; and monitor surface quality, tolerance and tool life.
This guide summarizes Mentor CNC’s drilling knowledge in light of the ISO 513 and ISO 3685 international standards. Always verify parameters against your own material and machine conditions. For the other machining guides in the series, explore the Cutting Tools category and our CNC calculators.