Cutting Parameters and Machining Economics

Introduction

CNC programming is not only the preparation of geometrical tool paths. A technically correct program can still produce poor results if cutting speed, feed, depth of cut, tool life, chip control, or machine power is unsuitable. Cutting parameters determine productivity, dimensional accuracy, surface finish, tool consumption, energy use, and manufacturing cost.

The programmer and manufacturing engineer must therefore balance four objectives: remove material rapidly, preserve the required quality, avoid overloading the machine and tool, and achieve an economically justified cost per component. These objectives are interdependent. Increasing cutting speed may reduce machining time but shorten tool life. Increasing feed may improve productivity but increase roughness and cutting force. Increasing depth of cut may reduce the number of passes but exceed available spindle power.

This chapter develops the principal relationships used to select and evaluate machining parameters for turning, milling, and drilling. The equations are idealized engineering models; actual values must be checked against tool manufacturer recommendations, workpiece material data, machine limitations, rigidity, coolant conditions, and shop-floor trials.

Learning Objectives

After studying this chapter, the student should be able to:

1. Define cutting speed, spindle speed, feed, depth of cut, machining time, material-removal rate, and cutting power.
2. Calculate CNC cutting parameters for turning, milling, and drilling.
3. Estimate machining time and material-removal rate using consistent units.
4. Apply Taylor’s tool-life relationship and explain its limitations.
5. Relate feed and tool geometry to chip formation, surface finish, and chip control.
6. Evaluate machine power, torque, and process constraints.
7. Compare alternative parameter choices using machining economics.
8. Select practical parameters that balance cost, quality, productivity, and safety.

1. Fundamental Cutting Parameters

1.1 Cutting speed and spindle speed

Cutting speed is the relative speed between the cutting edge and the workpiece at the cutting zone. In turning, the surface speed depends on workpiece diameter and spindle speed. In milling, it depends primarily on cutter diameter and spindle speed.

For diameter in millimetres and speed in revolutions per minute:

where V_c is cutting speed in m/min, D is diameter in mm, and N is spindle speed in rev/min. Rearranging gives:

These equations assume a conventional constant-diameter calculation. In turning, the diameter changes during facing, tapering, or profiling. The calculated speed is therefore an instantaneous or representative value. CNC controls may use constant surface speed, in which spindle speed changes as diameter changes. A maximum spindle-speed limit must always be programmed or enabled.

1.2 Feed

Feed may be specified in different forms:

• Feed per revolution, f_n, in mm/rev, commonly used in turning and drilling.
• Feed per tooth, f_z, in mm/tooth, commonly used in milling.
• Linear feed rate, F, in mm/min, used by the CNC control.

For turning or drilling:

For milling with z teeth:

The milling equation assumes that each tooth receives the specified feed per tooth and that all programmed teeth are effective. Runout, unequal tooth spacing, tool wear, and interrupted cutting can make the actual chip load different from the nominal value.

1.3 Depth of cut and width of cut

In external turning, radial depth of cut is:

where D₀ and D_f are the initial and final diameters. The factor of two is essential because diameter reduction occurs on two sides of the workpiece.

In milling, a_p usually denotes axial depth of cut and a_e denotes radial width of cut. Their meanings must be confirmed from the tooling documentation because conventions differ between suppliers.

1.4 Cutting direction and engagement

Conventional and climb milling differ in chip thickness, force direction, and tendency to pull the workpiece into the cutter. Modern rigid CNC machines generally prefer climb milling because it often produces better finish and lower rubbing, but backlash, weak workholding, or special machine conditions may require another strategy. Tool engagement angle also affects chip thickness, heat generation, and instantaneous cutting force.

2. Machining-Time and Material-Removal Calculations

2.1 Turning time

For a straight turning pass of length L, with feed per revolution f_n and spindle speed N:

Here t_m is cutting time in minutes if L is in mm, f_n in mm/rev, and N in rev/min. Approach, overtravel, tool change, rapid motion, inspection, and loading time are not included.

For several passes:

The number of roughing passes is approximately:

where a_total is the required radial stock removal and a_p is the selected radial depth per pass. The ceiling function means that a partial final pass is counted as a complete pass.

2.2 Milling time

For a linear milling cut of length L:

where F is in mm/min. The effective programmed length should include approach and exit distances where the cutter must travel before and after full engagement. For pocketing and complex contours, total time is best obtained from verified CAM simulation or machine-control data rather than from a single straight-cut equation.

2.3 Drilling time

For drilling depth L at feed per revolution f_n:

The length should include the required approach and, where relevant, the drill-point distance and breakthrough allowance. Peck drilling introduces retract time and therefore takes longer than the simple cutting-time estimate.

2.4 Material-removal rate

For turning, a useful approximate material-removal rate is:

where Q is in mm³/min, V_c is in m/min, a_p is radial depth in mm, and f is feed in mm/rev. This expression approximates the annular cross-section removed per revolution and is most appropriate for straight turning with modest radial engagement.

For milling, a common planning approximation is:

where a_p and a_e are in mm and F is in mm/min. The result is mm³/min. Actual removal varies with cutter engagement, radial immersion, tool path, entry and exit, and chip thinning.

To express removal rate in cm³/min:

3. Worked Parameter Examples

Example 1: Turning speed, feed, time, and removal rate

A 60 mm diameter bar is turned at a recommended cutting speed of 150 m/min. The feed is 0.20 mm/rev, radial depth of cut is 2 mm, and cutting length is 120 mm.

Spindle speed:

Feed rate:

Cutting time:

Material-removal rate:

The calculation describes one ideal straight pass. If the machine requires a separate finishing pass, its time and removal rate must be added separately.

Example 2: Milling feed and time

A four-tooth cutter of diameter 80 mm operates at 120 m/min. Feed per tooth is 0.08 mm/tooth. The programmed cutting length is 240 mm.

If the axial depth is 3 mm and radial width is 20 mm:

4. Cutting Power, Torque, and Machine Constraints

Cutting power is the rate at which mechanical work is performed. A practical estimate based on specific cutting force is:

when k_c is in N/mm², Q is in mm³/min, and P_c is in kW. The factor 60,000 converts N·mm/min to kW.

Specific cutting force depends on workpiece material, chip thickness, tool geometry, cutting speed, and lubrication. It is not a universal constant. Manufacturers and machining references provide approximate values.

An alternative relation is:

where F_c is cutting force in newtons and V_c is m/min. Both equations estimate cutting power at the cutting zone. The required motor power is greater because of transmission losses:

where η is total mechanical and electrical efficiency, expressed as a decimal.

Spindle torque is related to power and angular speed. With power in kW and speed in rev/min:

where T is torque in N·m. The machine must satisfy both power and torque limits. At low spindle speed, torque may be limiting; at high speed, power or maximum rpm may be limiting.

Example 3: Power check

A milling operation removes material at 9,180 mm³/min. The estimated specific cutting force is 1,800 N/mm² and machine efficiency is 0.80.

A machine rated at 3 kW has adequate power according to this simplified estimate. However, rigidity, cutter engagement, workholding, torque, insert grade, and transient loads must still be checked. A power calculation alone cannot guarantee a stable process.

5. Tool Life and Tool-Wear Mechanisms

Tool life is the usable cutting time before a specified wear criterion or quality limit is reached. Common wear mechanisms include flank wear, crater wear, notch wear, built-up edge, thermal cracking, chipping, and plastic deformation.

The classical Taylor relationship is:

where V_c is cutting speed, T is tool life, n is the tool-life exponent, and C is a constant for a particular tool-workpiece combination, geometry, coolant condition, and wear criterion. The relationship is empirical and applies only over the tested operating range.

For two known cutting conditions:

This shows why a modest increase in speed can cause a substantial reduction in tool life, especially when n is small.

Feed and depth of cut also affect tool life, so an extended empirical model may be written as:

The exponents and constant must be obtained experimentally or from validated technical data. They should not be assumed to be universal.

Example 4: Effect of speed on tool life

A tool lasts 30 minutes at 180 m/min. For the tool-workpiece pair, n = 0.25. Estimate life at 200 m/min.

Since 1/0.25 = 4:

The 11.1% speed increase reduces predicted life from 30 to approximately 19.7 minutes. The result is an estimate, not a guarantee, because actual wear may be dominated by chipping, vibration, or thermal damage.

6. Chip Formation, Chip Control, and Surface Quality

A cutting tool separates a chip from the workpiece through plastic deformation. Chip thickness, shear angle, friction, tool rake angle, cutting speed, feed, and material ductility influence the resulting chip. Continuous chips can wrap around the workpiece or tool and create a safety hazard. Short, controlled chips are generally preferable, but excessively fragmented chips may indicate unstable cutting or excessive brittleness.

Chip breakers alter the chip-flow path and force the chip to curl and break. Their operating range is defined by feed, depth of cut, and workpiece material. A chip breaker selected for heavy roughing may fail at light finishing feeds because the chip is too thin to contact the breaker effectively.

Surface roughness in an ideal turning operation is often approximated by:

where R_a is theoretical arithmetic average roughness in mm, f_n is feed in mm/rev, and r_ε is tool-nose radius in mm. This approximation assumes a sharp tool, ideal kinematics, a rigid setup, and a regular feed-mark profile. Actual roughness is affected by vibration, built-up edge, wear, material tearing, machine error, and tool geometry.

The equation indicates that reducing feed or increasing nose radius can improve theoretical finish. However, an excessively large nose radius increases radial force and may promote chatter in a weak setup. Finishing parameters must therefore be selected with rigidity and deflection in mind.

Chip-control practice includes:

• selecting the correct chip-breaker geometry and grade;
• maintaining the feed range recommended for the chip breaker;
• using adequate coolant or high-pressure coolant where appropriate;
• avoiding excessive nose-radius contact in flexible setups;
• using peck cycles for deep or difficult drilling when chip evacuation requires them;
• stopping the machine before manually removing chips and using appropriate tools rather than bare hands.

7. Machining Economics

Machining economics concerns the cost and time consequences of parameter selection. A faster process is not automatically cheaper if it consumes tools rapidly, causes scrap, or requires rework.

A simplified cost per component can be represented as:

where C_machine is machine and labor cost per minute, t_p is total production time per part, and the other terms represent material, tooling, setup, inspection, and quality-related costs. This is a planning model; actual accounting may allocate overhead differently.

If a tool costs C_t and produces n_p parts before replacement, tooling cost per part is:

Tool-changing time must be included in production time. A high-speed condition may reduce cutting time but increase tool changes. An economically favorable condition minimizes total cost while meeting quality and delivery requirements, not merely cutting time.

Two important theoretical speeds are often distinguished:

• Maximum-production-rate speed: minimizes time per part, usually using a relatively high cutting speed and accepting more frequent tool changes.
• Minimum-cost speed: minimizes cost per part by balancing machining time and tool-change cost.

These speeds depend on tool price, tool-change time, machine rate, batch size, setup time, and the tool-life relationship. They are not fixed material properties.

In practice, economic optimization should be constrained by surface finish, dimensional tolerance, burr formation, spindle power, vibration, chip control, environmental requirements, and tool supplier limits.

8. Integrated Applied Case: Turning a Steel Shaft

Background

An illustrative job requires 500 identical steel shafts. Each shaft must be reduced from 54 mm to 50 mm over a 100 mm length. A carbide insert is available. The machine has a 7.5 kW spindle, a maximum speed of 4,000 rev/min, and an estimated efficiency of 80%. The production team is considering a roughing speed of 160 m/min, feed of 0.22 mm/rev, and radial depth of 2 mm, followed by a finishing pass.

Problem

The team must determine whether the roughing parameters are feasible, estimate time and removal rate, and identify economic and quality issues.

Analysis

The total radial stock is:

Thus, the proposed roughing pass removes the entire radial stock. In production, this may be unsuitable because it leaves no material for a finishing pass. A practical alternative is a 1.5 mm roughing depth followed by a 0.5 mm finishing depth.

At the roughing diameter of 54 mm:

Roughing feed rate:

For a 100 mm cutting length, excluding approach and exit:

Approximate roughing removal rate:

Suppose the estimated specific cutting force is 2,000 N/mm²:

Required motor power, using 80% efficiency:

The estimated power is below the 7.5 kW rating. Nevertheless, the engineer must check torque, insert grade, workholding, deflection, chip control, and actual machine load.

Approach and solution

The roughing pass should leave a controlled finishing allowance. The finishing pass should use a feed and nose radius compatible with the required surface finish. Constant surface speed may be used, but a maximum spindle-speed limit should be specified. Tool wear should be monitored after trial components, and the tool should be changed before dimensional drift or surface deterioration occurs.

If chips become long and hazardous, the team should first verify that feed and depth lie within the chip-breaker range. Increasing speed alone is not a reliable chip-control method. Coolant direction and pressure should also be checked.

Outcome

The selected roughing condition is feasible from the simplified power perspective and gives a cutting time of approximately 29 seconds per roughing pass. The revised two-pass strategy improves dimensional control and finish capability, although it adds finishing time. The final choice should be validated by a controlled trial and measured using actual cycle time, tool life, surface roughness, dimensional capability, and scrap rate.

Learning points

1. Radial depth in turning is half the diameter reduction.
2. A power check is necessary but not sufficient.
3. A finishing allowance must be deliberately planned.
4. Economic performance includes tool changes, inspection, and quality losses.
5. Tool-life and chip-control data should be verified experimentally for the actual setup.

9. Constraints, Best Practices, and Contemporary Developments

Important constraints include machine maximum rpm, spindle power and torque, tool-holder overhang, workpiece stiffness, fixture capacity, coolant capability, thermal expansion, insert geometry, and operator safety. Thin walls and slender shafts may require lower depth of cut, lighter feed, support devices, or alternative tool paths even when the machine has ample power.

Best practice is to begin with validated supplier data, calculate the resulting rpm and feed, check machine limits, simulate the tool path, conduct a controlled first-off trial, and record actual load, tool life, cycle time, and quality. Parameter changes should be made systematically rather than changing speed, feed, and depth simultaneously.

Modern CNC controls may provide adaptive feed control, spindle-load monitoring, constant surface speed, tool-wear compensation, and in-process probing. CAM systems can estimate cycle time and material removal, but estimates may omit acceleration, deceleration, tool changes, machine behavior, and operator actions. Artificial intelligence and machine-learning systems are increasingly used to predict tool wear and detect abnormal spindle-load patterns. Such systems should support, not replace, engineering judgment and verified measurement. Data quality, explainability, cybersecurity, and safe machine integration remain important governance issues.

Environmental decisions also matter. Higher productivity can reduce energy per component, but excessive speed may increase coolant demand, tool waste, noise, and scrap. Dry machining, minimum-quantity lubrication, high-pressure coolant, and optimized tool paths should be evaluated according to material, tooling, machine capability, health requirements, and total environmental impact.

Chapter Summary

Cutting parameters provide the quantitative link between CNC code and machining performance. Cutting speed determines spindle speed through tool or workpiece diameter; feed per revolution and feed per tooth determine linear feed rate; depth and width of cut determine engagement and material removal. Machining time follows from cutting distance divided by feed rate, while material-removal rate estimates productivity.

Cutting power can be estimated from specific cutting force and removal rate, but machine torque, rigidity, workholding, and transient loads must also be considered. Taylor’s relationship explains the strong effect of cutting speed on tool life, although it is empirical and limited to its validated range. Feed, nose radius, chip-breaker geometry, and coolant influence chip control and surface finish.

Machining economics requires more than minimizing cutting time. Tool cost, tool-change time, machine rate, quality, scrap, setup, energy, and delivery requirements must be considered together. Professional parameter selection is therefore a constrained optimization activity supported by calculations, supplier data, simulation, measurement, and safe shop-floor experimentation.

Key Terms

Cutting speed: Relative speed between the cutting edge and workpiece at the cutting zone.

Spindle speed: Rotational speed of the spindle, usually in rev/min.

Feed per revolution: Tool advance during one spindle revolution, in mm/rev.

Feed per tooth: Cutter advance assigned to each milling tooth, in mm/tooth.

Feed rate: Linear tool movement rate, usually in mm/min.

Depth of cut: Thickness of material removed in the cutting direction.

Width of cut: Radial engagement of a milling cutter.

Machining time: Time during which the tool performs the specified cutting travel.

Material-removal rate: Volume of material removed per unit time.

Specific cutting force: Approximate cutting force required per unit uncut chip area.

Cutting power: Mechanical power delivered to the cutting process.

Spindle torque: Rotational moment available at the spindle.

Tool life: Usable cutting time before a defined wear or quality limit.

Taylor tool-life equation: Empirical relationship between cutting speed and tool life.

Flank wear: Wear occurring on the relief face of a cutting tool.

Chip breaker: Tool feature designed to curl and break chips.

Surface roughness: Small-scale irregularity of a machined surface.

Minimum-cost speed: Cutting speed that minimizes total cost per component under stated assumptions.

Maximum-production-rate speed: Cutting speed that minimizes production time under stated assumptions.

Constant surface speed: CNC control mode that adjusts spindle speed as diameter changes.

Review Questions

Short Answer Questions

1. Distinguish cutting speed from spindle speed.
2. Why is the diameter reduction divided by two when calculating radial depth of cut in turning?
3. State two factors that affect actual tool life besides cutting speed.
4. What is the purpose of a chip breaker?
5. Why must torque be checked in addition to spindle power?

Long Answer Questions

1. Explain the relationships among cutting speed, spindle speed, feed rate, and machining time for turning and milling.
2. Describe the assumptions and limitations of the Taylor tool-life equation.
3. Explain how feed, nose radius, rigidity, and vibration influence surface finish.
4. Discuss the difference between minimum-cost speed and maximum-production-rate speed.
5. Describe a systematic procedure for selecting and validating CNC cutting parameters.

Analytical / Application Questions

1. A 75 mm diameter workpiece is turned at 180 m/min with a feed of 0.25 mm/rev over a 150 mm length. Calculate spindle speed, feed rate, and ideal cutting time.
2. A milling cutter has six teeth and operates at 100 m/min on a 50 mm diameter cutter with 0.06 mm/tooth feed. Calculate spindle speed and table feed. If the cut is 4 mm deep and 12 mm wide, calculate the approximate removal rate.
3. A tool lasts 25 minutes at 150 m/min, with Taylor exponent n = 0.20. Estimate life at 165 m/min and discuss whether the speed increase is economically justified without additional cost and quality data.

Multiple Choice Questions with Answers

Question 1

A 50 mm diameter turning operation uses a cutting speed of 100 m/min. What spindle speed is required?

A. 318 rev/min

B. 637 rev/min

C. 1,273 rev/min

D. 3,183 rev/min

Correct Answer: B. 637 rev/min

Question 2

A milling cutter has 4 teeth, runs at 500 rev/min, and uses 0.10 mm/tooth. What is the feed rate?

A. 50 mm/min

B. 125 mm/min

C. 200 mm/min

D. 2,000 mm/min

Correct Answer: C. 200 mm/min

Question 3

In turning, a diameter reduction from 60 mm to 56 mm corresponds to what radial depth of cut?

A. 1 mm

B. 2 mm

C. 4 mm

D. 8 mm

Correct Answer: B. 2 mm

Question 4

Which equation estimates straight-turning machining time when length is in millimetres?

A. t = L × fN

B. t = L ÷ (fN)

C. t = f ÷ (LN)

D. t = N ÷ (Lf)

Correct Answer: B. t = L ÷ (fN)

Question 5

What is the approximate milling material-removal rate when axial depth is 5 mm, radial width is 10 mm, and feed rate is 200 mm/min?

A. 1 cm³/min

B. 5 cm³/min

C. 10 cm³/min

D. 100 cm³/min

Correct Answer: C. 10 cm³/min

Question 6

In the Taylor relationship V_cTⁿ = C, what generally happens to tool life when cutting speed increases?

A. Tool life increases

B. Tool life remains constant

C. Tool life decreases

D. Tool life becomes independent of wear

Correct Answer: C. Tool life decreases

Question 7

Which factor is included in a realistic machining-cost calculation?

A. Only cutting speed

B. Only material-removal rate

C. Tool-change cost and production time

D. Workpiece colour

Correct Answer: C. Tool-change cost and production time

Question 8

The approximate turning surface-finish relationship R_a ≈ f_n² ÷ (32r_ε) indicates that, under its assumptions, increasing feed generally:

A. Decreases theoretical roughness linearly

B. Increases theoretical roughness approximately with feed squared

C. Has no effect on theoretical roughness

D. Eliminates tool wear

Correct Answer: B. Increases theoretical roughness approximately with feed squared

Question 9

If cutting power at the tool is 2 kW and machine efficiency is 0.80, what motor power is approximately required?

A. 0.8 kW

B. 1.6 kW

C. 2.0 kW

D. 2.5 kW

Correct Answer: D. 2.5 kW

Question 10

Why should a finishing allowance commonly be left after roughing?

A. To eliminate the need for inspection

B. To provide controlled material for achieving final size and finish

C. To increase spindle speed automatically

D. To prevent all chip formation

Correct Answer: B. To provide controlled material for achieving final size and finish