Cutting Tool Technology and Geometry

Introduction

Cutting tool technology is one of the fundamental pillars of the machinist trade. To succeed on the Red Seal exam, you must master not only tool nomenclature, but also the physical principles governing metal cutting, basic geometries, manufacturing materials, and cutting parameters. This chapter covers all the knowledge required according to the National Occupational Analysis (NOA) for the machinist trade.

2.1 Fundamental Principles of Metal Cutting

2.1.1 The Chip Formation Mechanism

Metal cutting is a process of localized plastic deformation. When the tool penetrates the workpiece, the metal is compressed and then sheared along a plane called the shear plane. The chip formed slides along the rake face of the tool.

Three types of chips can form:

Chip Type	Formation Condition	Characteristics
Continuous chip	Ductile material, high cutting speed, positive rake angle	Good surface finish, long and regular chip
Discontinuous (segmented) chip	Brittle material (cast iron), low speed, small rake angle	Short chips, better evacuation, risk of vibration
Chip with built-up edge (BUE)	Low speed, ductile material, high friction	Rough surface, tool deterioration, dimensional instability

> Exam Tip: The built-up edge forms mainly at low cutting speeds on ductile materials like aluminum and mild steel. To eliminate it, increase the cutting speed or use an appropriate cutting fluid.

2.1.2 The Three Fundamental Angles

The geometry of a cutting tool is defined by three main angles measured in different planes:

Relief angle (clearance angle): angle between the flank face and the machined surface. It prevents friction between the tool and the workpiece. Typical value: 6° to 12°.

Wedge angle (cutting edge angle): angle formed between the rake face and the flank face. It determines the strength of the cutting edge.

Rake angle: angle between the rake face and the normal to the machined surface. It influences chip formation and cutting force.

The sum of these three angles is always equal to 90°:

Relief angle + Wedge angle + Rake angle = 90°

2.1.3 The Rake Angle and Its Influence

The rake angle is the most critical parameter for tool performance:

Positive rake angle: facilitates cutting, reduces required force, but weakens the cutting edge. Used for soft materials (aluminum, plastics).

Negative rake angle: strengthens the cutting edge, increases impact resistance, but requires more power. Used for hard materials (hardened steels) and carbide tools.

Neutral rake angle: a compromise between the two, used for certain specialized tools.

> Rule of thumb: For every 5° increase in positive rake angle, the cutting force decreases by approximately 1%. However, too positive an angle weakens the edge and can cause chipping.

2.2 Cutting Tool Materials

2.2.1 Classification of Materials

The choice of tool material depends on hot hardness, toughness, wear resistance, and cost. Here are the main materials used:

Material	Hardness (HRC)	Max. Operating Temperature	Relative Cutting Speed	Typical Application
High-Speed Steel (HSS)	60-65	600 °C	1×	Drills, end mills, form tools
Cobalt HSS (M42)	65-67	650 °C	1.2×	Resistant materials, stainless steels
Cemented Carbide (ISO K, P, M)	78-82	900-1000 °C	3-5×	Turning, high-speed milling
Cermet	90-93	900 °C	4-6×	Finishing, hardened steels
Cubic Boron Nitride (CBN)	95	1200 °C	8-10×	Hardened steels (>45 HRC)
Polycrystalline Diamond (PCD)	100	800 °C	10-15×	Aluminum, non-ferrous alloys, composites

2.2.2 ISO Carbide Classifications

The ISO system (ISO 513) classifies carbides into three main categories:

Class P: for machining steels (long chips). Grades P10 to P50 — the lower the number, the harder and more wear-resistant the tool; the higher the number, the tougher the tool.

Class M: for machining stainless steels and difficult-to-cut alloy steels.

Class K: for machining cast irons and non-ferrous materials (short chips).

2.2.3 Tool Coatings

Coatings significantly increase tool life:

TiN (Titanium Nitride): gold color, reduces friction, increases surface hardness. Max. temperature: 600 °C.

TiCN (Titanium Carbonitride): blue-grey color, harder than TiN, better wear resistance.

TiAlN (Titanium Aluminum Nitride): violet-black color, excellent heat resistance (up to 800 °C), ideal for dry machining.

AlCrN (Aluminum Chromium Nitride): for highly abrasive materials and extreme temperatures.

> Exam Tip: The TiAlN coating is best suited for high-speed dry machining because it forms an alumina (Al₂O₃) layer at high temperatures that acts as a thermal barrier.

2.3 Turning Tool Geometry

2.3.1 Turning Tool Nomenclature

A turning tool consists of:

The shank (body): the part held in the tool holder.

The rake face: the surface on which the chip slides.

The major flank face: the surface facing the workpiece.

The minor flank face: the surface facing the end of the workpiece.

The major cutting edge: the intersection of the rake face and the major flank face.

The minor cutting edge: the intersection of the rake face and the minor flank face.

The nose (tool point): the junction point of the two cutting edges.

2.3.2 Turning Tool Angles

Angle	Definition	Typical Value	Effect
Cutting edge angle (χ)	Angle between the major cutting edge and the workpiece axis	45°-95°	Influences chip thickness and radial force
Nose angle (ε)	Angle between the two cutting edges	55°-100°	Larger = stronger, but more vibration
Inclination angle (λ)	Angle between the cutting edge and the horizontal plane	-6° to +6°	Controls chip flow direction
Relief angle (α)	Angle between the flank face and the machined surface	6°-12°	Prevents friction, influences finish
Rake angle (γ)	Angle between the rake face and the normal	-6° to +15°	Controls chip formation

2.3.3 Nose Radius

The nose radius is the radius of curvature at the tool point:

Small nose radius (0.2-0.4 mm): fine finish, low cutting force, but fragile edge.

Medium nose radius (0.8-1.2 mm): standard compromise for most operations.

Large nose radius (1.6-2.4 mm): high strength, good heat dissipation, but risk of vibration.

> Important Relationship: The theoretical surface roughness (Ra) is related to the nose radius and the feed rate:

> Ra ≈ (feed²) / (8 × nose radius) × 1000 (in µm)

> Example: feed = 0.2 mm/rev, nose radius = 0.8 mm

> Ra = (0.2²) / (8 × 0.8) × 1000 = 0.04 / 6.4 × 1000 = 6.25 µm

2.4 Milling Cutter Geometry

2.4.1 Types of Milling Cutters

Cutter Type	Application	Characteristics
Cylindrical mill (2-flute)	Shoulders, slots	Peripheral and face cutting
Face mill	Flat surfaces	Large diameter, indexable inserts
Slitting saw	Slots, parting	Variable thickness, peripheral teeth
End mill	Slots, profiles	Various shapes (square, ball, radius)
Side-and-face cutter	Deep slots	Three cutting faces
Thread mill	Internal and external threads	Tooth profile matching the thread

2.4.2 Milling Cutter Angles

High-speed steel cutters generally have:

Helix angle (λ): 30° standard, 45° for soft materials, 15° for hard materials.

Right-hand helix: cuts when rotating clockwise (viewed from the shank).

Left-hand helix: cuts when rotating counter-clockwise.

Relief angle: 6°-10° for HSS cutters, 8°-12° for carbide cutters.

Radial rake angle: positive for soft materials, negative for hard materials.

2.4.3 Tooth Pitch

The pitch is the distance between two consecutive teeth:

Fine pitch: more teeth, better finish, but limited chip evacuation.

Medium pitch: standard for general machining.

Coarse pitch: fewer teeth, better chip evacuation, for gummy materials or large depths of cut.

> Engagement Rule: For a carbide cutter, radial engagement should not exceed 50% of the cutter diameter to avoid vibration. For an HSS cutter, engagement can reach 70-80%.

2.5 Cutting Parameters and Calculations

2.5.1 Cutting Speed

The cutting speed (Vc) is the relative speed between the tool and the workpiece, expressed in meters per minute (m/min).

Formula for turning:

Vc = (π × D × N) / 1000

Where:

Vc = cutting speed (m/min)

D = workpiece diameter (mm)

N = rotational speed (RPM)

π ≈ 3.1416

Formula for milling:

Vc = (π × D × N) / 1000

Where D = cutter diameter (mm)

Rotational speed (RPM):

N = (Vc × 1000) / (π × D)

2.5.2 Recommended Cutting Speeds

Workpiece Material	HSS Tool (m/min)	Carbide Tool (m/min)
Mild steel (1018)	25-35	150-250
Alloy steel (4140)	15-25	100-180
Stainless steel (304)	10-18	80-150
Grey cast iron	15-25	100-200
Aluminum	60-100	300-600
Brass	60-90	200-400
Bronze	40-60	150-250
Titanium	8-12	40-80

> Exam Tip: These values are starting points. Adjust according to machine rigidity, depth of cut, and cutting fluid used. Cutting speed should be reduced by 20-30% for roughing operations and can be increased by 10-20% for finishing.

2.5.3 Feed Rate

The feed rate (f) is the displacement of the tool per workpiece revolution (turning) or per tooth (milling).

Feed per revolution (turning): f = 0.05 to 0.5 mm/rev depending on the operation.

Feed per tooth (milling):

fz = feed per tooth (mm/tooth)

Vf = fz × Z × N

Where:

Vf = feed speed (mm/min)

Z = number of cutter teeth

N = rotational speed (RPM)

2.5.4 Depth of Cut

The depth of cut (ap) is the thickness of material removed in one pass:

Roughing: ap = 2-6 mm (turning), 1-3 mm (milling)

Finishing: ap = 0.2-0.5 mm (turning), 0.2-1 mm (milling)

2.5.5 Machining Time

Turning time:

T = L / (f × N)

Where:

T = time (min)

L = machining length (mm)

f = feed rate (mm/rev)

N = rotational speed (RPM)

Milling time:

T = L / Vf

Where L = total length including approach and overtravel.

2.5.6 Complete Calculation Example

Problem: You need to turn a 4140 steel workpiece with a diameter of 50 mm over a length of 100 mm. Use a carbide tool, a depth of cut of 2 mm, and a feed rate of 0.3 mm/rev.

Step 1: Choose the cutting speed. For 4140 steel with carbide: Vc = 150 m/min.

Step 2: Calculate the rotational speed.

N = (150 × 1000) / (π × 50) = 150000 / 157.08 = 955 RPM

Step 3: Calculate the machining time.

T = 100 / (0.3 × 955) = 100 / 286.5 = 0.349 min ≈ 21 seconds

2.6 Cutting Fluids

2.6.1 Functions of Cutting Fluids

Cutting fluids perform four main functions:

136.Cooling: remove heat generated by cutting (up to 80% of the heat).

137.Lubrication: reduce friction between the tool and the chip.

138.Chip evacuation: remove chips from the cutting zone.

139.Corrosion protection: protect the workpiece and the machine.

2.6.2 Types of Fluids

Type	Composition	Application	Advantages	Disadvantages
Neat oil	Mineral or vegetable oil	Threading, tapping, broaching	Excellent lubrication	Poor cooling, fire risk
Emulsion (soluble oil)	5-10% oil in water	General machining	Good cooling, economical	Requires maintenance (bacteria)
Semi-synthetic fluid	5-20% oil + additives	Turning, milling	Good compromise	Higher cost
Synthetic fluid	Chemical solution without oil	Grinding, high-speed machining	Excellent cooling	Limited lubrication
Oil mist	Atomized oil in air	High-speed machining	Low consumption	Health risk (inhalation)

> Exam Tip: For machining aluminum, use a 5-8% emulsion or a light oil. For machining stainless steels, use a high-pressure cutting oil or a 10% emulsion.

2.7 Tool Wear and Tool Life

2.7.1 Wear Modes

Wear Mode	Description	Cause	Remedy
Crater wear	Depression on the rake face	High temperature, diffusion	Reduce speed, change grade
Flank wear	Wear band on the flank face	Abrasion, friction	Reduce speed, increase relief angle
Chipping	Removal of small fragments from the edge	Shocks, vibration	Increase rake angle, use a tougher grade
Fracture	Complete tool breakage	Overload, thermal shock	Reduce feed, check clamping
Built-up edge	Material accumulation on the edge	Low speed, ductile material	Increase speed, use a fluid

2.7.2 Sharpening Criteria

The tool should be sharpened or replaced when:

Flank wear reaches 0.3 mm (finishing) or 0.6 mm (roughing).

Crater wear reaches 0.1 mm in depth.

The surface roughness of the workpiece visibly deteriorates.

Abnormal vibrations or noises appear.

Power consumption increases significantly.

2.7.3 Taylor's Law

Taylor's law relates tool life to cutting speed:

Vc × Tⁿ = C

Where:

Vc = cutting speed (m/min)

T = tool life (min)

n = exponent characteristic of the tool material (0.1-0.2 for HSS, 0.2-0.3 for carbide)

C = constant

> Practical Application: If you double the cutting speed, tool life is divided by 2^(1/n). For a carbide tool (n = 0.25), doubling the speed reduces tool life by a factor of 2⁴ = 16 times.

2.8 Applicable Canadian Standards and Codes

2.8.1 CSA Standards

CSA Group standards govern certain aspects of machining:

CSA B149.1: Natural Gas and Propane Installation Code — applicable if you work on systems using these gases.

CSA B149.2: Propane Storage and Handling Code — for propane installations.

CSA W47.1: Certification of Companies for Fusion Welding — if you perform related welding operations.

> Important Note: For the Red Seal exam in machining, knowledge of CSA standards is primarily required for safety and workplace environment aspects. The Canadian Electrical Code, Part I (CE Code) (C22.1) applies to electrical installations in workshops but is not a direct exam topic for the machinist.

2.8.2 Workplace Safety

The Occupational Health and Safety Act (OHSA) and corresponding provincial regulations require:

Wearing personal protective equipment (PPE): safety glasses, steel-toed boots, hearing protection.

Using machine guards that comply with CSA standards.

Periodic inspection of lifting equipment (CSA B167 standards for overhead cranes).

Safe management of cutting fluids (WHMIS — Workplace Hazardous Materials Information System).

2.8.3 WHMIS

WHMIS is mandatory in all Canadian workplaces. Requirements include:

Safety Data Sheets (SDS) available for all chemical products.

Compliant labeling of containers.

Worker training on hazards and protective measures.

> Exam Tip: Cutting fluids are classified as hazardous materials. You must know the hazard pictograms and associated risk statements.

2.9 Practical Procedures and Best Practices

2.9.1 Tool Mounting

186.Clean the tool holder and insert before mounting.

187.Verify that the insert is correctly positioned in its seat.

188.Tighten the clamping screw to the recommended torque (generally 2-6 N·m depending on size).

189.Align the tool point with the workpiece axis (turning) or with the spindle center (milling).

190.Check the cutter runout after clamping (max. 0.02 mm).

2.9.2 Tool Height Adjustment

Turning: the tool point must be exactly at the height of the workpiece center. A tool that is too high or too low changes the actual cutting angles and can cause problems.

Milling: the cutter must be centered relative to the workpiece. A lateral offset changes the effective rake angle.

2.9.3 Quality Control

Surface roughness: measured with a profilometer (Ra, Rz). Typical values: roughing 3.2-6.3 µm, finishing 0.8-1.6 µm, grinding 0.2-0.4 µm.

Dimensional tolerances: checked with micrometers, limit gauges, or coordinate measuring machines (CMM).

2.10 Pitfalls to Avoid

199.Confusing cutting speed and rotational speed: cutting speed is in m/min, rotational speed is in RPM. Do not use them interchangeably.

200.Forgetting to convert units: the diameter is in mm, the cutting speed is in m/min. The formula N = (Vc × 1000) / (π × D) includes the factor 1000 for this conversion.

201.Ignoring the negative rake angle: for carbide tools, a negative rake angle is often necessary to strengthen the edge. Do not systematically replace it with a positive angle.

202.Choosing the wrong ISO class: a Class P insert for machining cast iron (Class K) will wear out quickly. Always check the workpiece material.

203.Neglecting the nose radius: a nose radius too small for the feed rate used produces a poor surface finish.

204.Forgetting the safety factor: recommended cutting speeds are starting points. Adjust according to actual conditions (rigidity, clamping, fluid).

205.Confusing crater wear and flank wear: crater wear occurs on the rake face, flank wear on the flank face.

206.Not accounting for Taylor's law: a small increase in cutting speed can significantly reduce tool life.

207.Using the wrong cutting fluid: neat oil for a high-speed turning operation will cause overheating. Use an emulsion.

208.Ignoring safety standards: failure to comply with WHMIS or machine guarding rules is a cause of failure on the practical exam.

2.11 Exam Tips

Memorize the formulas: Vc = (π × D × N) / 1000 and N = (Vc × 1000) / (π × D) are essential.

Learn the typical values: relief angles (6-12°), rake angles (positive for soft materials, negative for hard materials).

Know the ISO classes: P for steel, M for stainless steel, K for cast iron.

Understand the relationships: roughness = f² / (8 × r), Taylor's law Vc × Tⁿ = C.

Practice the calculations: machining time, rotational speed, feed rate.

Review the wear modes: be able to identify each mode on an image and propose a remedy.

2.12 Summary

Metal cutting is based on chip formation through plastic deformation along a shear plane.

The three fundamental angles (relief, wedge, rake) are related by: sum = 90°.

Tool materials range from high-speed steel (HSS) to polycrystalline diamond (PCD), with increasing performance and cost.

Carbides are classified into three ISO categories: P (steels), M (stainless steels), K (cast irons and non-ferrous materials).

Coatings (TiN, TiCN, TiAlN) improve tool life and performance.

Turning tool geometry includes the cutting edge angle, nose angle, inclination angle, relief angle, and rake angle.

The nose radius directly influences surface roughness: Ra ≈ f² / (8 × r).

Cutting parameters (speed, feed, depth) must be calculated and adjusted according to the material, tool, and operation.

Cutting fluids provide cooling, lubrication, chip evacuation, and corrosion protection.

Tool wear manifests in several forms (crater, flank, chipping, fracture) and must be monitored.

Taylor's law (Vc × Tⁿ = C) quantifies the relationship between cutting speed and tool life.

CSA standards and WHMIS govern safety in Canadian machining workshops.

2.13 Pitfalls to Avoid (Summary Table)

Pitfall	Consequence	Solution
Confusing Vc and N	Erroneous calculations, incorrect speed	Always check the units
Wrong ISO class choice	Premature tool wear	Identify the workpiece material
Inappropriate rake angle	Breakage or poor finish	Adapt the angle to the material
Nose radius too small	Excessive roughness	Use r ≥ 0.8 mm for finishing
Speed too high	Tool breakage	Respect recommended values
Unsuitable cutting fluid	Overheating, poor evacuation	Choose according to the operation
Neglecting safety	Accident, non-compliance	Wear PPE, comply with WHMIS

This chapter covers all the essential knowledge in cutting tool technology and geometry for the Red Seal exam. Review the reference tables regularly and practice the calculations until they become automatic. Mastering these concepts will allow you not only to pass the exam, but also to perform quality work in your career as a machinist.

Cutting Tool Technology and Geometry