Hole-making is a fundamental group of manufacturing operations. Holes may be required for bolts, shafts, bearings, lubrication passages, electrical connections, locating pins, or fluid flow. Although drilling is often the first operation, producing a functional hole usually requires a sequence of processes: drilling creates the opening, boring corrects its location and geometry, reaming improves size and surface finish, and thread production prepares the hole to receive a fastener or form an internal screw thread.

The quality of a hole is determined by more than its nominal diameter. Important characteristics include location, straightness, roundness, cylindricity, perpendicularity, surface roughness, burr formation, and the quality of any thread. The selected machine, cutting tool, workholding method, cutting parameters, coolant, and inspection method must therefore be considered as an integrated system.

This chapter develops the principles required to select and operate equipment for drilling, boring, reaming, and thread production. It also explains the calculation of cutting speed, spindle speed, feed, machining time, drilling forces, and torque, while emphasizing alignment, dimensional control, safety, and defect diagnosis.

Learning Objectives

1. Hole-Making Processes and Their Roles

1.1 Drilling

Drilling produces a cylindrical hole using a rotating, multi-point tool, normally a twist drill, that advances axially into the workpiece. It is usually the fastest and most economical method for producing an initial hole. However, a drilled hole may have limited positional accuracy, a relatively rough surface, a small amount of taper, and a diameter different from the drill’s nominal size.

1.2 Boring

Boring enlarges and corrects an existing hole with a single-point or multi-point tool. Unlike drilling, boring can improve hole location, concentricity, straightness, and diameter control. A boring bar is particularly useful when a hole must be aligned with another datum or when the required diameter is not available as a standard drill size.

Boring may be carried out on a lathe, milling machine, machining centre, jig boring machine, or dedicated boring machine. The workpiece or the boring tool rotates depending on the machine. Single-point boring is flexible because the diameter can be adjusted, but it generally removes material more slowly than drilling.

1.3 Reaming

Reaming is a finishing operation that removes a small, controlled allowance from a previously drilled or bored hole. A reamer has multiple cutting edges and produces improved size, roundness, and surface finish. It does not normally correct a badly misplaced or substantially crooked hole. Reaming should therefore follow an accurately located and adequately sized preliminary hole.

Typical reaming allowances depend on diameter, material, and process capability. An allowance that is too small may cause rubbing and poor finish; an allowance that is too large may overload the reamer and produce an oversize or tapered hole. Manufacturer recommendations should be used for production work.

Hand reamers are operated manually and commonly have a long lead section. Machine reamers are designed for rigid machine feed and generally have a shorter lead. Reamers must rotate in the cutting direction during withdrawal; reversing a reamer while it is engaged can damage cutting edges and the hole.

1.4 Thread Production

Threads may be produced by cutting, forming, milling, rolling, grinding, or additive processes.

The choice depends on material, thread size, tolerance, production quantity, blind or through-hole geometry, machine control, and required strength.

2. Machines, Tools, and Workholding

2.1 Machine selection

A bench or pillar drill is appropriate for general-purpose drilling where positional accuracy is moderate. A radial drilling machine is useful for large or awkward workpieces because the spindle can be positioned over the work. A lathe is preferred when the hole must be concentric with a turned outside diameter. A milling machine or machining centre is selected when hole location is controlled by coordinates and when drilling is combined with milling, boring, tapping, or inspection. A jig boring machine provides very high positional accuracy but is less economical for routine work.

2.2 Cutting tools

The standard twist drill has a point, cutting lips, chisel edge, flutes, body, margin, and shank. The point angle affects cutting force and centring behaviour. A general-purpose point angle near 118° is widely used for steels and many general applications, while larger angles may suit harder materials and smaller angles may suit softer materials. The correct geometry depends on the tool manufacturer and work material.

High-speed steel drills are tough and economical for general work. Carbide drills permit higher cutting speeds and can provide excellent productivity, but they require rigid machines, accurate workholding, and careful handling. Indexable insert drills are effective for larger diameters and production environments.

Boring bars may be steel, carbide, or damped designs. Long, slender bars are susceptible to chatter. Reamers may be straight-fluted or helical, fixed or adjustable, and made from high-speed steel or carbide. Tool runout, edge condition, coating, and correct diameter are central to hole quality.

2.3 Workholding and alignment

The workpiece must be supported so that it cannot rotate, shift, or vibrate. A drill press vice, fixture, chuck, collet, faceplate, or modular fixture may be used. Clamping directly on a thin unsupported wall can distort the workpiece and release it when the clamp is removed.

Before cutting, the operator should establish a datum scheme, clean the locating surfaces, verify that the tool is concentric with the spindle, and ensure that the work surface is perpendicular to the spindle when required. A centre punch mark alone is not a substitute for accurate coordinate location. For precision work, spotting, edge finding, probing, or numerical control should be used.

3. Operating Parameters and Calculations

3.1 Cutting speed and spindle speed

Cutting speed is the tangential speed at the outside diameter of the rotating tool. For a tool diameter in millimetres and cutting speed in metres per minute, spindle speed is:

The factor 1000 converts metres to millimetres. This equation assumes that the cutting speed is specified at the tool circumference and that the tool diameter remains constant. The calculated value must be limited by the machine speed range, tool manufacturer’s recommendation, work material, coolant, and rigidity.

Worked example. A 20 mm high-speed steel drill is recommended to operate at 25 m/min. The required spindle speed is:

A practical machine setting would be approximately 400 rev/min, provided that the machine, tool, and workholding permit it.

3.2 Feed rate

where v_f is axial feed rate in mm/min, f_n is feed per revolution in mm/rev, and n is spindle speed in rev/min. If feed per tooth is specified instead:

where f_z is feed per tooth in mm/tooth and z is the number of effective teeth. For a conventional twist drill, feed is commonly specified directly in mm/rev because the chisel edge and cutting lips do not behave like a simple idealized milling cutter.

Feed must be selected from tool data and adjusted for diameter, material, hole depth, rigidity, and coolant. Excessive feed increases thrust and may break the drill; insufficient feed can cause rubbing, work hardening, and poor tool life.

3.3 Machining time

where t_c is cutting time in minutes, L is the axial cutting distance in millimetres, and v_f is feed rate in mm/min. The distance L should include the workpiece thickness and the required point breakthrough or approach distance. For a blind hole it must include the drill-point geometry or an allowance specified by the drawing.

This is cutting time only. Total cycle time may also include rapid approach, tool changes, chip clearing, measurement, peck retracts, and work loading.

Worked example. A 12 mm drill operates at 600 rev/min with a feed of 0.18 mm/rev. It must travel 32 mm. Then:

3.4 Material removal rate

where Q is material removal rate in mm³/min, D is drill diameter in mm, and v_f is feed rate in mm/min. This assumes a full circular cross-section is being removed and neglects the small effects of the drill point and chip compression. It is therefore useful for estimating productivity rather than exact chip volume.

3.5 Torque and power

Cutting torque and power depend strongly on tool geometry, material, diameter, feed, and lubrication. Manufacturer data or validated empirical models should be preferred. Once torque T in N·m and rotational speed n in rev/min are known, spindle power is:

where P is power in watts. The factor 60 converts minutes to seconds. If power is expressed in kilowatts:

The available machine power must exceed the required cutting power after allowing for transmission losses. A machine with adequate power may still be unsuitable if it lacks rigidity or torque at the required speed.

3.6 Thread pitch and tapping speed

For a metric thread, pitch P is the axial distance between corresponding points on adjacent threads, in millimetres. In synchronized tapping, the feed must equal pitch per revolution:

For a 1.5 mm pitch thread at 300 rev/min, the feed is v_f = 1.5 × 300 = 450 mm/min. In rigid tapping, spindle rotation and axial feed are electronically synchronized. In manual or non-synchronized tapping, excessive feed mismatch can damage the tap or thread.

where d_t is the approximate tap-drill diameter, d is the nominal thread diameter, and P is pitch. This is an approximation for a typical thread percentage, not a universal rule. Exact tap-drill selection must use the required thread percentage, material, tolerance class, and tap manufacturer’s data. Forming taps require a different pre-hole size.

An 8.5 mm drill may be a suitable starting selection for many conventional applications, but the engineering drawing, thread class, material, and tap data must be checked before production.

4. Controlling Accuracy and Surface Quality

4.1 Positional accuracy

Hole position errors arise from inaccurate layout, poor datum selection, drill wandering, workpiece movement, spindle runout, and fixture errors. A spot drill or centre-cutting tool creates a stable starting surface. The spot diameter should be sufficient to guide the drill without producing an excessively deep conical cavity.

On CNC machines, coordinate accuracy depends on machine calibration, thermal condition, tool offsets, probing, and correct work coordinate systems. A hole may have the correct diameter but still fail if its axis is displaced from the specified position.

4.2 Size and form

Drill diameter alone does not guarantee hole diameter. Lip imbalance, runout, uneven sharpening, material springback, and tool deflection commonly produce oversize holes. Reaming or boring should be used when the required tolerance exceeds reliable drilling capability.

Inspection may involve plug gauges, pin gauges, internal micrometers, telescoping gauges, bore gauges, coordinate measuring machines, or air gauges. A go gauge checks acceptance at the maximum material condition, while a no-go gauge checks the opposite limit; the exact interpretation depends on the dimensioning standard and gauge design.

4.3 Straightness, perpendicularity, and cylindricity

A hole can be accurately located at its entrance but deviate internally because of workpiece distortion, drill deflection, interrupted cutting, or inadequate support. Long holes are especially sensitive. Peck cycles, pilot holes, gun drills, guide bushes, boring operations, or specialized deep-hole drilling may be required.

Perpendicularity errors occur when the work surface is not square to the spindle, the fixture is incorrectly seated, or the tool deflects. A drill point may initially enter at an angle and then cut a curved path. A rigid setup and a short, accurately guided tool are the primary controls.

4.4 Surface finish and burrs

Surface finish depends on tool geometry, feed, speed, edge condition, material, coolant, vibration, and chip evacuation. Reaming usually improves finish, but a reamer cannot remove severe chatter marks or correct major form errors. Exit burrs are reduced by backing material, using a sacrificial support, reducing feed near breakthrough, applying a countersink, or using a dedicated deburring tool.

Burr removal is not merely cosmetic. Burrs can interfere with assembly, damage seals, alter dimensions, create stress raisers, and injure operators. Deburring should be specified, controlled, and inspected rather than treated as an informal final activity.

5. Thread Production Practice

5.1 Tapping

Cut taps have flutes that remove material. Taper, plug, and bottoming taps differ in the length of their chamfer and are selected according to whether the hole is through or blind. Spiral-point taps push chips forward and are effective in through holes. Spiral-flute taps pull chips out of blind holes. Form taps require ductile material and produce no cutting chips, but they demand suitable lubrication and a controlled pre-hole.

Before tapping, the hole must have adequate depth and the entrance should be chamfered. The tap must be aligned with the hole axis. For manual tapping, forward rotation should be steady and the tap should be periodically reversed as appropriate for the tool and material to break chips. Excessive force indicates misalignment, an undersized or blocked hole, inadequate lubrication, or an unsuitable tap.

5.2 Thread milling and single-point threading

Thread milling permits internal threads in materials that are difficult to tap and allows one cutter to produce several diameters of the same pitch. It also permits correction or removal of a thread without using a rigidly fixed tap. The operation requires accurate interpolation and careful control of tool engagement.

Single-point threading on a lathe provides excellent control of pitch and profile. The tool advances one pitch per spindle revolution, and multiple passes are used to reach full depth. It is slower than tapping for many small holes but is flexible and appropriate for large or unusual threads.

5.3 Thread quality

Thread inspection may involve thread plug gauges, optical measurement, functional assembly, pitch-diameter measurement, or coordinate measurement. A thread can have acceptable major and minor diameters yet fail because of incorrect pitch, flank angle, lead, crest condition, or pitch diameter. Functional gauging is valuable because it evaluates assembly behaviour, but it should be supported by dimensional controls where traceability is required.

6. Defect Diagnosis

Defect	Likely causes	Corrective action
Hole oversize	Runout, unequal lips, worn drill, excessive speed, flexible setup	Check spindle and tool runout; sharpen or replace tool; improve rigidity
Hole undersize	Dull tool, insufficient feed, work hardening, springback	Use correct feed; replace tool; avoid rubbing; finish by reaming if appropriate
Hole taper	Deflection, poor support, worn reamer, misalignment	Shorten tool overhang; improve support; align tool; inspect reamer
Hole wandering	No spot operation, poor point geometry, angled surface, interrupted entry	Spot accurately; use correct point; support or machine the entry surface
Chatter or poor finish	Low rigidity, excessive overhang, unsuitable speed, worn tool	Increase rigidity; reduce overhang; alter speed/feed; use suitable geometry
Bellmouth at entrance	Reamer deflection, excessive entrance pressure, worn lead	Align reamer; reduce pressure; inspect lead and allowance
Burr at exit	Excessive breakthrough feed, unsupported material, dull tool	Support exit; reduce feed near breakthrough; deburr deliberately
Broken drill	Excessive torque, chip packing, poor coolant, misalignment	Withdraw for chip clearing; use coolant; verify speed/feed and alignment
Broken tap	Undersized hole, blind-hole packing, misalignment, excessive torque	Verify tap drill; use correct tap style and depth; improve synchronization
Poor thread fit	Wrong tap size, incorrect pitch, worn tap, wrong thread standard	Confirm drawing and standard; inspect tap and gauge; control pre-hole

Diagnosis should begin with evidence rather than adjustment by trial and error. Measure the defect, inspect the tool, verify the setup, review the programmed or selected parameters, and then change one major variable at a time.

7. Safety, Quality, and Sustainability

Loose clothing, gloves near rotating tools, jewellery, and unsecured workpieces create serious hazards. Eye protection is essential, and long chips must never be removed by hand. The machine should be stopped before measuring, clearing chips, changing tools, or adjusting the fixture. A brush, hook, or suitable chip tool should be used for chip removal.

Coolants reduce temperature and assist chip evacuation, but they may cause skin irritation, mist exposure, microbial growth, and disposal concerns. Concentration should be monitored, leaks controlled, and waste managed according to local environmental requirements. Dry machining may be suitable for some materials and coated carbide tools, whereas through-tool coolant or minimum-quantity lubrication may be necessary for deep or difficult drilling.

Quality systems should identify critical hole characteristics, define inspection frequency, control tool life, and maintain traceability of gauges and measuring equipment. Statistical process control can be applied to hole diameter or position when repeated production data are available. A stable process should be improved through tool-life studies, condition monitoring, and preventive maintenance rather than relying solely on final inspection.

8. Applied Case: Precision Mounting Plate

Background

A steel mounting plate requires four 12 mm through holes for locating pins. The holes must be positioned within ±0.05 mm relative to two datum edges, have a diameter tolerance of 0.018 mm, and be perpendicular to the plate within the specified drawing limit. Direct drilling on a pillar drill produced acceptable diameters but inconsistent positions.

Problem analysis

Inspection showed that the principal error was positional rather than dimensional. The operator used layout marks and a centre punch, and the plate was clamped in a vice without a dedicated datum stop. The drill also had measurable runout. The process therefore contained several independent sources of error: manual location, workpiece movement, tool runout, and uncertain perpendicularity.

Approach and solution

The plate was moved to a vertical machining centre. The fixture incorporated hardened datum stops and clamps positioned to prevent lifting. The work coordinate system was established by probing the two datum edges. Each hole location was spot-drilled, followed by drilling 11.7 mm and reaming to 12.000–12.018 mm. The reamer was held in a precision tool holder, with a short overhang and suitable coolant.

The machine was set near 600 rev/min. With a feed of 0.14 mm/rev, the feed rate was:

The reaming allowance was selected from the tool manufacturer’s data rather than from a universal rule.

Outcome

The revised process met the positional and diameter requirements on the first article and remained stable over the controlled tool-life interval. The main improvement did not come from increasing cutting speed; it came from datum control, rigid workholding, accurate spotting, reduced runout, and a separate finishing operation.

Learning points

9. Contemporary Developments and Professional Practice

Modern machining centres combine drilling, boring, reaming, tapping, probing, and in-process measurement. Tool monitoring systems can detect abnormal torque, spindle load, vibration, or acoustic emission, helping prevent broken drills and taps. Digital tool management records tool life and offsets, while adaptive control modifies feed in response to cutting load.

High-pressure through-tool coolant, advanced carbide grades, multilayer coatings, solid carbide drills, and indexable systems have increased productivity. Additive-manufactured components may require post-process drilling or reaming because printed holes can contain rough surfaces, distortion, or residual material. Automated inspection and machine vision can support burr detection and dimensional verification, but measurement systems must be calibrated and their uncertainty understood.

Artificial intelligence is relevant when it assists with tool-wear prediction, anomaly detection, parameter optimization, or inspection classification. It should not replace engineering judgment without validation. Training data may be biased toward particular materials or machines, and an apparently accurate prediction may fail after a tool change or process modification. Human approval, traceability, cybersecurity, and safe fallback procedures remain necessary.

Chapter Summary

Drilling is the primary hole-generation process, but it does not automatically provide high positional or dimensional accuracy. Boring enlarges and corrects existing holes; reaming provides controlled finishing; and threads may be produced by tapping, single-point threading, milling, forming, or rolling. Machine and tool selection must account for material, hole geometry, tolerance, production volume, rigidity, coolant, and inspection requirements.

The central operating relationships are cutting speed and spindle speed, feed per revolution and feed rate, machining distance and cutting time, and pitch and synchronized tapping feed. These equations are useful only when their units, assumptions, machine limits, and tool recommendations are respected. Hole quality depends strongly on datum control, workholding, spindle runout, tool geometry, chip evacuation, and process stability. Defect diagnosis should be evidence-based, and safety requires secure workholding, guarding, eye protection, controlled chip removal, and responsible coolant management.

Key Terms

Boring: Enlarging and correcting an existing hole with a single-point or multi-point tool.

Burr: Unwanted raised material remaining after cutting, often at a hole exit.

Centre drilling: Producing a short starting feature to improve hole location and guidance.

Cutting speed: Tangential speed at the circumference of a rotating cutting tool.

Feed per revolution: Axial distance advanced by a tool during one spindle revolution.

Form tap: A tap that produces threads by plastic deformation rather than chip removal.

Peck drilling: Intermittent drilling with tool withdrawal for chip evacuation and cooling.

Reamer: A multi-edge finishing tool used to improve hole size, form, and surface finish.

Runout: Radial or axial deviation of a rotating tool or spindle from its ideal position.

Spiral-point tap: A tap that pushes chips forward, commonly used in through holes.

Thread milling: Producing a thread by interpolating a rotating multi-tooth cutter.

Review Questions

Short Answer Questions

Long Answer Questions

Analytical / Application Questions

Multiple Choice Questions with Answers

Question 1

Which operation is primarily used to improve the size, roundness, and surface finish of an existing hole?

Question 2

A 20 mm drill operates at a cutting speed of 25 m/min. What spindle speed is approximately required?

Question 3

Question 4

For synchronized tapping of a 1.5 mm pitch thread at 300 rev/min, what feed rate is required?

Question 5

Which tap type is generally suitable for pushing chips forward in a through hole?

Question 6

Question 7

If feed per revolution is 0.18 mm/rev and spindle speed is 600 rev/min, what is the feed rate?

Question 8

Which operation is most suitable for producing a flat-bottomed recess for a cylindrical-head screw?

Question 9

Using the approximation d_t ≈ d - P, what preliminary drill diameter is estimated for an M10 × 1.5 cut thread?

Question 10

Which factor is especially important when diagnosing a hole that is correctly sized but incorrectly located?

Chapter 6 Drilling, Boring, Reaming, and Thread Production

Drilling, Boring, Reaming, and Thread Production

Introduction and Context