Machining Science, Machine Tools and Metrology cover
Interactive book · Semester 4-5

Machining Science, Machine Tools and Metrology

Form a chip, draw the Merchant circle, index a dividing head, run G-code and set a sine bar in your browser

Thirteen chapters, 13 interactives, few words. Every chapter is mapped to the Anna University, VTU, SPPU, Mumbai University and KTU units it covers: how a chip forms and what it costs in force and tool life, the lathe, milling, drilling, indexing, grinding and CNC machines that cut it, then the metrology that proves the part is right: errors, gauges, limits and fits, threads, gears and surface finish.

  • AUME3493Manufacturing Technology
  • AUME3592Metrology and Measurements
  • VTUBME402Machining Science and Metrology
  • SPPU302045-BMachining Science and Technology
  • SPPU302053Measurement Laboratory
  • MUMEC303Production Processes
  • KTUPCMET402Machine Tools and Metrology

By Skill-Lync · Updated 16 Nov 2026 · 13 chapters · 13 interactives · free, no sign-up

Chapter 1

Mechanics of metal cutting: how a chip forms

Which syllabus covers thisAU ME3493 Unit IVTU BME402 Module 1SPPU 302045-B Unit 1MU MEC303 4.2KTU PCMET402 Module 1

What is the difference between orthogonal and oblique cutting?

In orthogonal cutting the cutting edge is square to the cutting velocity, so the chip flows straight up the tool face and the problem is two-dimensional: two forces describe it. In oblique cutting the edge is inclined (inclination angle ), the chip curls sideways and three forces act. Most real turning is oblique; theory starts orthogonal.

How do you read a single-point tool signature?

The ASA signature lists seven numbers in a fixed order: back rake, side rake, end relief, side relief, end cutting edge angle, side cutting edge angle (degrees) and nose radius (mm). For example 8-14-6-6-6-15-1. Positive rake makes a sharper wedge with lower forces; relief angles stop the flanks rubbing the work.

What is the shear angle and how do you find it?

Metal ahead of the tool shears along a thin plane inclined at the shear angle to the cut. The chip comes off thicker than the uncut layer; the chip thickness ratio (always below 1) gives . A bigger shear angle means a shorter shear plane, a thinner chip and lower cutting force.

Orthogonal cutting: shear plane, shear angle and chip thickness: interactive loads as you scroll

Which chips form, and when?

Continuous chips come from ductile metals at high speed with a sharp, positive-rake tool and give the best finish. Discontinuous chips come from brittle metals such as cast iron. A continuous chip with built-up edge forms at low speed when work metal welds to the tool tip; it spoils the finish. Chip breakers curl long chips into safe pieces.

Predict, then check

Two cuts, same tool and depth. Cut A gives a chip 2 times the uncut thickness, cut B 3 times. Which has the larger shear angle?

Worked examples

Shear angle and shear strain · Orthogonal cut, = 0.25 mm, chip = 0.625 mm, rake = 10°
  1. = 0.4
  2. → = 22.94°
  3. = 2.59

Answer: = 22.94°, shear strain = 2.59

Chip ratio from chip length · Zero rake tool; 100 mm of uncut chip length comes off as a 40 mm chip
  1. Volume is conserved and width hardly changes, so
  2. = 40/100 = 0.4
  3. = 0: → = 21.8°

Answer: = 0.4, = 21.8°

Chapter 2

Cutting forces: the Merchant circle

Which syllabus covers thisAU ME3493 Unit IVTU BME402 Module 1SPPU 302045-B Unit 1MU not in syllabusKTU PCMET402 Module 1

What does the Merchant circle show?

One resultant force acts between tool and chip. Merchant drew it as the diameter of a circle and split it three ways: cutting force and thrust (what a dynamometer measures), friction and normal on the rake face, and shear force and normal on the shear plane. Every pair closes on the same circle.

Merchant's circle of cutting forces: interactive loads as you scroll

How do you get the shear stress of the work material?

Resolve the measured forces onto the shear plane, then divide by its area. The shear plane is longer than the uncut thickness by , so . The result is close to the shear flow stress of the metal and stays nearly constant across speeds.

What does Merchant's theory predict?

Assuming the chip picks the shear angle that needs the least energy gives . It explains the trends: more rake or less friction gives a larger shear angle. As a number it usually overestimates ; Lee and Shaffer's is another estimate. Measure the chip when you can.

How much power does a cut take?

Only the cutting force moves at cutting speed, so power is ; thrust does almost no work. Dividing power by the metal removal rate gives specific cutting energy, roughly 2–9 J/mm³ for steels and 0.4–1 J/mm³ for aluminium alloys in handbook tables, rising for thin chips (the size effect). About three quarters goes into shear, the rest into rake-face friction.

Predict, then check

The coolant is changed and friction on the rake face drops (β falls). According to Merchant, the shear angle:

Worked examples

Merchant circle from dynamometer readings · = 1200 N, = 500 N, = 10°, = 0.4, = 0.25 mm, = 2.5 mm
  1. = 700.8 N; = 1094.9 N
  2. = 0.640, = 32.62°
  3. = 22.94° (chapter 1): = 910.1 N, = 928.2 N
  4. = 1.603 mm², = 568 MPa

Answer: = 0.64, = 910 N, ≈ 568 MPa

Power and specific energy · Same cut at = 40 m/min
  1. = 1200 × 40/60 = 800 W = 0.8 kW
  2. MRR = = 2.5 × 0.25 × 40,000 = 25,000 mm³/min
  3. = 1200/0.625 = 1,920 N/mm² = 1.92 J/mm³

Answer: 0.8 kW, 1.92 J/mm³

Chip and shear velocities, and Merchant's estimate · Same cut
  1. Chip velocity = 0.4 × 40 = 16 m/min
  2. Shear velocity = 40.42 m/min
  3. Merchant: = 33.7°, against 22.9° measured

Answer: = 16 m/min, = 40.4 m/min; Merchant overestimates here by 11°

Chapter 3

Heat, tool wear, tool life and machinability

Which syllabus covers thisAU ME3493 Unit IVTU BME402 Module 3SPPU 302045-B Unit 1MU MEC303 4.2KTU PCMET402 Module 1

Where does the heat in cutting come from?

Almost all cutting energy becomes heat in three zones: the shear zone, the rake face where the chip rubs, and the flank where the tool rubs the new surface. At normal speeds the chip carries away most of it, but the rake-face zone runs hottest; its temperature, often 600–900 °C for carbide on steel, is what softens and wears the tool.

How does a tool wear out?

Flank wear is a land rubbed on the clearance face; it grows steadily and is the usual tool-life criterion (ISO 3685: average land width = 0.3 mm). Crater wear is a hollow on the rake face from diffusion at high temperature. Mechanisms: abrasion, adhesion, diffusion and oxidation. Chipping and plastic deformation end a tool suddenly.

What is Taylor's tool life equation?

F. W. Taylor (1907) found that tool life falls steeply with cutting speed: . The exponent is about 0.1–0.15 for HSS, 0.2–0.4 for carbide and 0.4–0.6 for ceramics; is the speed for one minute of life. Two tests give both constants. The extended form adds feed and depth.

Taylor tool life and the cutting speed for minimum cost: interactive loads as you scroll

Which cutting speed is the most economical?

Faster cutting saves machine time but uses up tools and tool changes. Minimising cost per piece gives an optimum tool life that depends on , the tool change time , the cost per edge and the machine rate . Ignoring tool cost gives the shorter life for maximum production rate.

Which tool materials, fluids and machinability?

Hot hardness ranks tool materials: high-speed steel, cemented carbide (often TiN, TiCN or Al₂O₃ coated), ceramics, cubic boron nitride for hardened steel, and diamond for non-ferrous metals. Cutting fluids cool and lubricate. Machinability compares how easily a metal cuts (tool life, force, finish); the index rates free-cutting steel AISI 1112 as 100 %.

Predict, then check

Carbide tool, = 0.25. You raise cutting speed by 20 %. Tool life:

Worked examples

Taylor constants from two tests · Tool life 60 min at 100 m/min and 12 min at 150 m/min
  1. = 0.252
  2. = 281 m/min

Answer:

Effect of a 20 % speed increase · = 0.25
  1. = 0.482

Answer: Tool life falls by 51.8 %

Minimum-cost and maximum-production speeds · , machine + labour ₹5/min, ₹40 per edge, tool change 2 min
  1. = 3 × 10 = 30 min → = 128.2 m/min
  2. = 6 min → = 191.7 m/min

Answer: 128 m/min for least cost, 192 m/min for the fastest output

Chapter 4

The lathe: turning, tapers, threads and machining time

Which syllabus covers thisAU ME3493 Unit IIVTU BME402 Module 1SPPU not in syllabusMU MEC303 4.1KTU PCMET402 Module 1

What are the main parts of a centre lathe?

The bed carries the headstock (spindle, speed gearbox), the tailstock (dead centre, drilling) and the carriage, which holds the cross-slide, compound rest and tool post. The feed rod drives the carriage for turning; the lead screw and half-nut drive it for thread cutting. A lathe is specified by swing over the bed and distance between centres.

How do you calculate spindle speed, machining time and MRR?

Spindle speed comes from the cutting speed you want: . The tool advances mm every revolution, so one pass over length (plus approach and over-travel) takes minutes. Metal removal rate is roughly ; power is MRR times specific energy.

One turning pass: speed, time, power and the feed marks the nose leaves: interactive loads as you scroll

How are tapers turned?

Swivel the compound rest to the half angle for short steep tapers; offset the tailstock for long gentle tapers between centres; use a taper-turning attachment for accurate tapers of any length; or use a form tool for short ones. The half angle comes from the two diameters and the taper length.

What sets the surface finish of a turned part?

A round-nosed tool leaves a row of arcs, one every feed. Their height is the theoretical peak-to-valley roughness , so halving the feed cuts roughness by four while a bigger nose radius smooths it. Real surfaces are rougher because of built-up edge, vibration and tool wear.

What do capstan and turret lathes add?

They replace the tailstock with a six-station indexing turret, so one setup drills, turns, bores and threads in sequence without changing tools. A capstan lathe's turret slides on a ram (light, bar work); a turret lathe's turret sits on a saddle that moves on the bed (heavier chucking work). Automatics such as Swiss-type lathes run whole cycles unattended.

Predict, then check

You halve the feed on a finishing pass with the same tool. The theoretical roughness:

Worked examples

Machining time, MRR and power for a turning pass · = 50 mm, = 2 mm, = 0.2 mm/rev, = 30 m/min, = 100 mm + 5 mm approach, = 2.5 J/mm³
  1. = 191 rpm
  2. = 2.75 min
  3. MRR = 11,520 mm³/min
  4. = 480 W

Answer: 191 rpm, 2.75 min, 11.52 cm³/min, 0.48 kW

Taper by compound rest and by tailstock offset · Taper from 50 to 40 mm over 60 mm; job 200 mm long between centres
  1. → = 4.76°: swivel the compound rest by this
  2. Tailstock offset = 16.67 mm

Answer: Half angle 4.76°, or offset 16.67 mm

Theoretical finish · = 0.2 mm/rev, nose radius 0.8 mm
  1. = 0.00625 mm = 6.25 µm
  2. = 1.60 µm

Answer: = 6.25 µm, ≈ 1.6 µm (grade N7)

Change gears for a thread · Lead screw pitch 6 mm; cut a 1.5 mm pitch thread
  1. Driver/driven = job pitch/lead screw pitch = 1.5/6 = 1/4
  2. = 20/80: a 20-tooth gear on the spindle drives an 80-tooth gear on the lead screw (with an idler)

Answer: 20 : 80

Chapter 5

Milling, drilling, shaping and broaching

Which syllabus covers thisAU ME3493 Unit IIIVTU BME402 Module 2SPPU not in syllabusMU MEC303 4.1KTU PCMET402 Module 2

Up milling or down milling?

In up (conventional) milling the cutter turns against the feed: each tooth starts at zero chip thickness, rubs before it bites and tends to lift the work. In down (climb) milling it turns with the feed: the tooth enters at full thickness, finish and tool life are better, but the table needs a backlash eliminator or the cutter pulls the work in.

Up and down milling: engagement, approach and chip thickness: interactive loads as you scroll

Which milling machines and cutters are there?

Column-and-knee machines (horizontal, vertical, universal) raise the table on a knee; bed-type and planer mills carry heavier work. Cutters: plain (slab), side-and-face, slitting saws, angle, form, end mills and face mills. Operations include face, slab, slot, gang and straddle milling, plus gear cutting with a dividing head.

How do you find drilling time?

A twist drill (point angle usually 118°) must travel the hole depth plus its own cone length to break through, plus a little clearance. Reaming finishes a drilled hole to size, boring corrects its position, tapping cuts an internal thread. Radial drills move the head over large work.

What do shapers, planers, slotters and broaches do?

A shaper's single-point tool cuts on the forward stroke and returns quickly: the crank and slotted lever make the return faster. A planer moves the work under a fixed tool, for long beds. A slotter cuts vertically, for keyways. A broach is a long multi-tooth tool, each tooth a little taller, that finishes a hole or slot in one pass.

Predict, then check

On an old knee mill with a worn lead screw (backlash), which milling is safer?

Worked examples

Slab milling time · Cutter 80 mm, 10 teeth, 100 rpm, = 0.1 mm, depth 5 mm, width 50 mm, length 200 mm, over-travel 5 mm
  1. = 100 mm/min
  2. Approach = 19.36 mm
  3. = 2.24 min
  4. MRR = 25,000 mm³/min

Answer: 2.24 min, 25 cm³/min

Drilling a through hole · 20 mm drill, 118° point, = 0.2 mm/rev, = 25 m/min, plate 40 mm, clearance 2 mm
  1. = 398 rpm
  2. Cone length = 6.01 mm
  3. = 0.603 min

Answer: 0.60 min ≈ 36 s

Shaper quick-return ratio · Crank radius 100 mm, crank centre 300 mm from the slotted-lever pivot
  1. Return angle = 141.06°
  2. Cutting angle = 360 − 141.06 = 218.94°

Answer: Quick-return ratio = 1.55

Chapter 6

Indexing, gear cutting and thread production

Which syllabus covers thisAU ME3493 Unit IIIVTU BME402 Module 2SPPU 302045-B Unit 2MU MEC303 4.1KTU PCMET402 Module 2

How does simple indexing work?

A dividing head has a 40:1 worm, so 40 crank turns rotate the work once. For divisions the crank turns : whole turns plus a fraction, made up as holes on an index plate circle whose hole count is a multiple of the fraction's denominator. Sector arms are set to span the holes so you can't miscount.

Dividing head: simple and differential indexing on index plates: interactive loads as you scroll

What if no plate has the right circle?

Differential indexing: index for a nearby number that the plates can do, and let change gears turn the plate slowly to correct the error. Gear ratio driver/driven = . If is bigger than the plate turns the same way as the crank; if smaller, the opposite way. Compound indexing uses two circles instead.

How are gears cut?

Form milling uses a cutter shaped like the tooth space and indexes tooth by tooth; one cutter covers a range of tooth numbers, so it is approximate. Generating methods are exact and faster: hobbing (a worm-like hob rolls with the blank, for spur and helical gears) and gear shaping (a pinion cutter reciprocates, for internal and cluster gears). Shaving and grinding finish them.

How are threads produced?

Single-point cutting on a lathe, dies and taps for small sizes, thread milling, thread grinding for precision, and thread rolling, which forms the thread between hardened dies without cutting. Rolled threads are stronger because the grain flows around the root and the surface is cold-worked; most fasteners are rolled.

Predict, then check

40:1 dividing head with Brown & Sharpe plates. For 35 divisions the crank moves:

Worked examples

Simple indexing for 27 divisions · Brown & Sharpe plates, 40:1 head
  1. 40/27 = 1 13/27
  2. Plate 2 has a 27-hole circle

Answer: 1 full turn + 13 holes on the 27-hole circle

Simple indexing for 35 divisions · Brown & Sharpe plates
  1. 40/35 = 1 5/35 = 1 1/7
  2. 1/7 = 3/21: plate 2 has a 21-hole circle (7/49 on plate 3 also works)

Answer: 1 turn + 3 holes on the 21-hole circle

Differential indexing for 97 divisions · 97 is prime and no plate has 97 holes; choose = 100
  1. Index for 100: 40/100 = 6/15 → 6 holes on the 15-hole circle
  2. Gear ratio = 1.2 = 48/40
  3. 48-tooth driver on the spindle, 40-tooth driven on the plate shaft
  4. : the plate must turn the same way as the crank

Answer: 6 holes on 15, gears 48/40, plate turns with the crank

Chapter 7

Grinding and super-finishing

Which syllabus covers thisAU ME3493 Unit IIIVTU BME402 Module 2SPPU 302045-B Unit 3MU MEC303 4.1KTU PCMET402 Module 2

How do you read a grinding wheel marking?

The marking (IS 551, like ISO 525) gives, in order: abrasive (A aluminium oxide, C silicon carbide), grain size (10–24 coarse to 220–600 very fine), grade (A–H soft, I–P medium, Q–Z hard: how firmly the bond holds the grains), structure (1–8 dense, 9 and above open) and bond (V vitrified, B resinoid, R rubber, E shellac, S silicate, M metal). 51 A 46 K 5 V 23 is an example.

Grinding wheel marking builder: abrasive, grit, grade, structure and bond: interactive loads as you scroll

How do you choose a wheel?

Aluminium oxide for steels, silicon carbide for cast iron, non-ferrous metals and carbide; CBN and diamond for hardened steel and carbide. Use a soft grade for hard work (blunt grains break out and expose sharp ones) and a hard grade for soft work. Coarse grain for fast removal, fine grain for finish; open structure for large contact areas.

Which grinding processes are there?

Surface grinding (flat faces, reciprocating or rotary table), cylindrical grinding between centres, internal grinding of bores and centreless grinding, where a regulating wheel turns and feeds the work against the grinding wheel without centres: ideal for pins and rollers in high volume. Creep-feed grinding takes deep cuts at very slow feed.

What are glazing, loading, dressing and truing?

A glazed wheel has blunt grains polished flat (grade too hard); a loaded wheel has its pores clogged with metal (often soft metals). Dressing removes the dull layer to expose sharp grains. Truing makes the wheel round and concentric with its spindle again. Wheels are also balanced before use to avoid vibration and chatter marks.

What are honing, lapping, buffing and burnishing?

Honing rotates and reciprocates abrasive stones inside a bore, leaving a crosshatch that holds oil (engine cylinders). Lapping rubs the part against a lap with loose abrasive slurry for flatness and Ra below 0.1 µm (gauge blocks, valve seats). Buffing polishes with soft wheels and compound. Burnishing rolls the surface smooth without removing metal.

Predict, then check

You grind hardened tool steel and the wheel glazes. Next wheel should be:

Worked examples

Decoding a wheel · 51 A 46 K 5 V 23
  1. 51: maker's abrasive prefix; A: aluminium oxide
  2. 46: medium grain
  3. K: medium grade (I–P)
  4. 5: dense structure
  5. V: vitrified bond; 23: maker's record

Answer: Medium-grain, medium-grade vitrified aluminium oxide wheel: general steel grinding

Wheel surface speed · 300 mm vitrified wheel at 1,900 rpm; maximum safe speed 33 m/s
  1. = 29.8 m/s
  2. Below the 33 m/s limit printed on the wheel

Answer: 29.8 m/s: safe

Grinding ratio · 2,000 mm³ of steel removed while the wheel loses 40 mm³
  1. = volume of work removed / volume of wheel worn = 2000/40

Answer: = 50

Chapter 8

CNC machines and part programming

Which syllabus covers thisAU ME3493 Units IV and VVTU not in syllabusSPPU 302045-B Unit 6MU MEC404 Module 4KTU not in syllabus

What makes a machine CNC?

A computer reads the program and drives each axis through servo motors and recirculating ball screws (rolling balls instead of sliding threads: little friction, no backlash when preloaded). Encoders feed position back (closed loop). Automatic tool changers, coolant systems and enclosures complete turning centres and machining centres. Control can be point-to-point (drilling) or continuous path (contouring).

How are CNC axes named?

Right-hand rule, ISO 841: Z is the spindle axis, positive away from the work; X is the longest horizontal travel; Y completes the right-handed set. A, B and C are rotations about X, Y and Z. Programs are written from the part zero (work offset, G54), not the machine zero.

Which G and M codes do you need first?

G00 rapid move, G01 straight feed, G02 clockwise and G03 counter-clockwise arcs (centre by I, J offsets from the start point, or radius R), G90 absolute and G91 incremental coordinates, G17 XY plane, G21 millimetres, G41/G42 cutter radius compensation. M03 spindle on clockwise, M05 stop, M06 tool change, M08 coolant on, M30 end of program.

Step through CNC G-code: absolute and incremental moves, G02/G03 arcs: interactive loads as you scroll

What are canned cycles and subroutines?

A canned cycle packs a repetitive motion into one block: G81 drilling, G83 peck drilling, G84 tapping on machining centres; G71 rough turning and G76 threading on Fanuc-type lathes. Subroutines (M98 call, M99 return) and loops repeat a pattern, such as the same pocket at several places, so the program stays short and readable.

Predict, then check

The tool is at X40 Y0. Which block cuts a quarter circle of radius 10 ending at X50 Y10, curving up like the corner of a box traced counter-clockwise?

Worked examples

Absolute and incremental blocks · Path (0,0) → (40,0) → (40,30) → (0,30)
  1. G90: G01 X40 Y0, X40 Y30, X0 Y30
  2. G91: G01 X40 Y0, X0 Y30, X-40 Y0

Answer: Absolute gives positions from zero; incremental gives each move from the last point

Ball screw resolution · Ball screw lead 5 mm, encoder 2,000 counts/rev, feed 500 mm/min
  1. Basic length unit = 5/2000 = 0.0025 mm
  2. Screw speed = 500/5 = 100 rpm

Answer: 2.5 µm per count, 100 rpm

An arc block and its time · From X40 Y0, G03 X50 Y10 I0 J10 F200
  1. Centre = (40 + 0, 0 + 10) = (40, 10); start and end are both 10 mm from it
  2. Quarter circle length = = 15.71 mm
  3. Time = 15.71/200 min = 4.7 s

Answer: R10 counter-clockwise arc, 4.7 s

Chapter 9

Jigs, fixtures and process planning

Which syllabus covers thisAU ME3493 Unit IVVTU not in syllabusSPPU 302045-B Units 4 and 5MU MEC303 4.2KTU PCMET402 Module 2

What is the difference between a jig and a fixture?

Both locate and hold the work so every part is machined in the same place without marking out. A jig also guides the tool, usually through hardened drill bushes, and is used for drilling, reaming and tapping. A fixture only holds the work; the tool is set to it with setting blocks or feeler gauges: milling, turning, welding and inspection fixtures.

What is the 3-2-1 principle?

A free block has 12 degrees of freedom: move or turn either way along and about three axes. Three locators under the base, two on a side face and one on the end fix it in one position, locking 9 of them; clamps pressed towards the locators lock the last 3. Extra locators on the same face over-constrain the part and make it rock.

3-2-1 location: pins and clamps stopping a block's 12 freedoms: interactive loads as you scroll

What are the rules of good fixture design?

Locate on machined, stable faces, as far apart as possible; clamp onto solid parts, directly over locators, never against the cutting force; make loading foolproof so a part can't go in the wrong way; leave room for chips and coolant; keep it rigid and quick to load. Common jigs: template, plate, channel, box, leaf and turnover jigs.

What does a process plan contain?

Read the drawing, check the material and stock, then list operations in order (datums first, roughing before finishing, holes after faces), with the machine, the work holding, tools, speeds, feeds and the inspection method for each. The route sheet and operation sheets carry this to the shop floor; time and cost estimates come from the same data.

Predict, then check

A long round bar sits in a long V-block with an end stop. How many of its 12 freedoms are still free?

Worked examples

Counting freedoms for a prismatic block · 3 base locators, 2 side locators, 1 end locator, 3 clamps
  1. Base 3: −Z, ± rotation about X and Y → 5
  2. Side 2: −Y, ± rotation about Z → 3
  3. End 1: −X → 1
  4. Locators: 9 of 12; clamps add +X, +Y, +Z → 12

Answer: Fully constrained with 6 locators and 3 clamps

Order of operations for a flanged bush · Bush with a bored hole, a flange face and four bolt holes
  1. Face and rough-turn the flange side in a chuck
  2. Bore the hole and face the flange in the same setup (square to each other)
  3. Turn the outside on a mandrel located in the bore
  4. Drill the bolt holes in a plate jig located on the bore and flange face
  5. Inspect the bore with a plug gauge

Answer: Datums (bore + face) first, then everything located from them

Chapter 10

Measurement, errors, standards and uncertainty

Which syllabus covers thisAU ME3592 Unit IVTU BME402 Module 4SPPU 302053 term work 1-2MU not in syllabusKTU PCMET402 Module 3

What is the difference between accuracy and precision?

Accuracy is how close the average reading is to the true value; precision is how close repeated readings are to each other. A micrometer with a zero error is precise but inaccurate: correct it and it becomes accurate. Resolution is the smallest change the instrument shows, which says nothing about either.

Accuracy vs precision: systematic and random error in repeated readings: interactive loads as you scroll

Which errors affect a measurement?

Systematic errors repeat in size and sign: zero error, a worn or wrongly calibrated instrument, temperature away from 20 °C (steel grows 11.5 µm per metre per °C), Abbe offset. Random errors scatter both ways and are reduced by averaging. SWIPE lists the sources: Standard, Workpiece, Instrument, Person, Environment.

How is the metre defined and passed down?

Since 1983 the metre is the distance light travels in vacuum in 1/299,792,458 of a second, realised with stabilised lasers. Line standards (scales) carry length between engraved lines; end standards (gauge blocks, length bars) between flat faces. A traceable chain of calibrations runs from the national laboratory, CSIR-NPL in India, down to your shop gauge.

How do you state measurement uncertainty?

Type A comes from repeat readings: the standard uncertainty of the mean is . Type B comes from other information: the calibration certificate, resolution (divide by ), temperature. Combine them as the root of the sum of squares and multiply by = 2 for about 95 % confidence (ISO GUM).

Predict, then check

You take 4 times as many readings with the same micrometer. The uncertainty of the mean (type A):

Worked examples

Mean, standard deviation and uncertainty · Five readings of a 25 mm gauge block: 25.012, 25.008, 25.011, 25.009, 25.010 mm
  1. Mean = 25.010 mm; deviations +2, −2, +1, −1, 0 µm
  2. = 1.58 µm
  3. = 0.71 µm
  4. Block certified 25.000 mm: systematic error = +10 µm, subtract it from future readings

Answer: 25.010 mm, = 1.58 µm, = 0.71 µm, bias +10 µm

Temperature error · 100 mm steel part measured at 30 °C (reference 20 °C), = 11.5 × 10⁻⁶ /°C
  1. = 11.5 × 10⁻⁶ × 100 × 10 mm

Answer: 11.5 µm too long, five times a 2 µm tolerance budget

Combined and expanded uncertainty · = 0.71 µm; certificate ±2 µm at = 2; resolution 1 µm
  1. Certificate: 2/2 = 1.00 µm
  2. Resolution: = 0.29 µm
  3. = 1.26 µm

Answer: = 2.5 µm (about 95 % confidence)

Chapter 11

Linear and angular measurement, gauge blocks and comparators

Which syllabus covers thisAU ME3592 Unit IIVTU BME402 Modules 4 and 5SPPU 302053 term work 2, 5, 6MU not in syllabusKTU PCMET402 Module 3

How do vernier calipers and micrometers read so fine?

A vernier scale has divisions spanning main-scale divisions, so the least count is one main division divided by : 50 divisions over 49 mm give 0.02 mm. A micrometer turns a screw: 0.5 mm pitch and 50 thimble divisions give 0.01 mm. Always check and subtract zero error.

How do you build a size with slip gauges?

Gauge blocks are hardened, lapped steel or ceramic blocks that wring together (a film of a few hundredths of a micron) to build any size. With the 87-piece set, clear the last decimal place first, then the next, then the 0.5 mm steps and the tens: 41.125 = 1.005 + 1.12 + 9 + 30. Fewer blocks mean less accumulated error.

How does a sine bar set an angle?

A sine bar is a hardened bar with two rollers a known distance apart (100 or 200 mm). Raising one roller on slip gauges of height tilts it to . Errors in matter more as the angle grows, so above about 45° use angle gauges or a sine centre instead.

Sine bar on slip gauges: building h = L sin θ from an M87 set: interactive loads as you scroll

What are comparators and angular instruments?

A comparator magnifies the difference between the part and a master set to size: mechanical (dial indicator, Sigma, reed), optical (Zeiss ultra-optimeter), pneumatic (Solex air gauge, flow or back-pressure) and electrical (LVDT). Angles are measured with bevel protractors, angle gauges, clinometers, and autocollimators or angle dekkors, which read tiny tilts from a reflected image.

Predict, then check

A 100 mm sine bar. A 1 µm error in the slip stack causes the larger angle error at:

Worked examples

Reading a vernier caliper · 50 vernier divisions = 49 mm; main scale shows 32 mm, vernier line 23 coincides
  1. LC = 1 − 49/50 = 0.02 mm
  2. Reading = 32 + 23 × 0.02

Answer: 32.46 mm

Micrometer with zero error · Pitch 0.5 mm, 50 thimble divisions; sleeve 7.5 mm, thimble 28; zero error +0.02 mm
  1. LC = 0.5/50 = 0.01 mm
  2. Reading = 7.5 + 28 × 0.01 = 7.78 mm
  3. Correct reading = 7.78 − 0.02

Answer: 7.76 mm

Building 41.125 mm · M87 slip gauge set
  1. Last decimal 0.005: take 1.005 → remainder 40.120
  2. Hundredths: take 1.12 → 39.000
  3. Take 9 → 30; take 30 → 0

Answer: 1.005 + 1.12 + 9 + 30 (four blocks)

Setting 23.5° on a sine bar · 100 mm sine bar, M87 set
  1. = 39.8749 mm → build 39.875
  2. 39.875 = 1.005 + 1.37 + 7.5 + 30
  3. Angle actually set = = 23.5001°

Answer: Slip stack 39.875 mm (4 blocks), angle within 0.2″

Chapter 12

Limits, fits, tolerances and limit gauges

Which syllabus covers thisAU ME3592 Unit IIIVTU BME402 Modules 4 and 5SPPU 302053 term work 3MU not in syllabusKTU PCMET402 Module 3

What do basic size, deviation and tolerance mean?

Basic size is the drawing size. Upper and lower deviations say how far the largest and smallest allowed sizes sit from it; tolerance is their difference. Interchangeability means any hole fits any shaft without selection; selective assembly instead sorts parts into groups to get close fits from wider tolerances. Tighter tolerance always costs more.

How does the ISO system set tolerances?

IS 919 (ISO 286) splits sizes into steps and uses the step's geometric mean to compute the tolerance unit in microns. Grades IT5 to IT11 multiply it by 7, 10, 16, 25, 40, 64 and 100. A letter places the zone: H holes and h shafts start at the basic size, a–g shafts sit below it, k–zc above.

Limits and fits: hole and shaft tolerance zones from the IS 919 formulae: interactive loads as you scroll

Clearance, transition or interference fit?

Clearance: the smallest hole is bigger than the largest shaft (running fits such as H7/g6, H8/f7). Interference: the largest hole is smaller than the smallest shaft (press fits such as H7/p6, H7/s6). Transition: either can happen (locating fits such as H7/k6, H7/n6). Hole basis keeps the hole H and varies the shaft; it is preferred because reamers and plug gauges come in fixed sizes.

How are GO and NO-GO gauges designed?

Taylor's principle: the GO gauge checks the maximum-material limit and the whole form (full length), the NO-GO gauge checks the other limit at one point. Gauge maker's tolerance is usually 10 % of the work tolerance, and the GO gauge, which wears, gets a wear allowance (about 10 % of the gauge tolerance) inside the work limits.

Predict, then check

Hole basis system. Which shaft letter gives a transition fit with an H7 hole?

Worked examples

25 H8/f7 from the IS 919 formulae · Basic size 25 mm (step 18–30 mm)
  1. = 23.24 mm, = 1.307 µm
  2. IT8 = 25 = 32.7 → 33 µm; IT7 = 16 = 20.9 → 21 µm
  3. f shaft: = -20.0 → −20 µm, = −20 − 21 = −41 µm
  4. Hole 25.000 / 25.033; shaft 24.980 / 24.959

Answer: Clearance fit: 20 µm minimum, 74 µm maximum

60 H7/g6 · Basic size 60 mm (step 50–80 mm)
  1. = 63.25 mm, = 1.856 µm
  2. IT7 = 30 µm, IT6 = 19 µm
  3. g: = −10 µm, = −29 µm
  4. Hole 60.000 / 60.030; shaft 59.990 / 59.971

Answer: Clearance 10 to 59 µm (matches the ISO 286 table)

A press fit from the table · 25 H7/p6, ISO 286-2 table values: H7 = +21/0 µm, p6 = +35/+22 µm
  1. Minimum interference = 22 − 21 = 1 µm
  2. Maximum interference = 35 − 0 = 35 µm

Answer: Interference fit, 1 to 35 µm

Plug gauge for a 25 H8 hole · Hole 25.000 to 25.033 mm
  1. Work tolerance 0.033; gauge tolerance 10 % = 0.0033; wear allowance 10 % of that = 0.00033
  2. GO: 25.00033 to 25.00363 mm
  3. NO-GO: 25.0297 to 25.0330 mm

Answer: GO 25.0003–25.0036 mm, NO-GO 25.0297–25.0330 mm

Chapter 13

Threads, gears, surface finish, form and CMM

Which syllabus covers thisAU ME3592 Units II, IV and VVTU not in syllabusSPPU 302053 term work 4MU not in syllabusKTU PCMET402 Modules 3 and 4

How is the effective diameter of a thread measured?

Three equal wires sit in the thread grooves and a micrometer reads over them. The best wire size touches the flanks at the pitch line, so flank angle errors cancel: , which is 0.577 for 60° metric threads. The effective diameter then follows from the reading .

How are gear teeth checked?

A gear tooth vernier sets its depth slide to the chordal addendum and reads the chordal tooth thickness at the pitch circle. Other checks: base tangent span over several teeth, runout, pitch error, profile and lead on a gear tester, and the rolling (Parkinson) test against a master gear for composite error.

What do Ra, Rq and Rz mean?

A stylus traces the surface; filters split roughness from waviness. is the average distance from the mean line, the root mean square, the average peak-to-valley height over five sampling lengths. Typical : turning 1.6–6.3 µm, grinding 0.2–1.6 µm, lapping 0.05–0.2 µm. Drawings may give N grades: N7 = 1.6 µm.

Surface roughness profile: Ra, Rq, Rz and N grade by process: interactive loads as you scroll

How are straightness, flatness and roundness measured?

Straightness with a straight edge, a level or an autocollimator; flatness with an optical flat, where each interference fringe means half a wavelength of height (about 0.29 µm with sodium light); roundness on a rotating-spindle instrument as the radial gap between two concentric circles. GD&T states these as form tolerances in a feature control frame.

What do CMMs, lasers and machine vision add?

A coordinate measuring machine touches or scans points with a probe and fits geometry to them in software: bridge, cantilever, gantry and horizontal-arm types. Laser interferometers check machine-tool positioning and straightness; ball bars check circular interpolation. Machine vision, white-light scanners and CT inspect parts online and inside, without contact.

Predict, then check

Two surfaces have the same Ra. One has sharp peaks, the other sharp valleys. Ra will:

Worked examples

Three-wire measurement of M20 × 2.5 · Effective diameter ; best wire
  1. = 18.376 mm
  2. Best wire = 1.443 mm
  3. = 18.376 + 4.330 − 2.165

Answer: Expected reading over wires = 20.541 mm

Gear tooth vernier setting · Spur gear, module 5, 32 teeth
  1. = 7.851 mm
  2. = 5.096 mm

Answer: Set the depth slide to 5.096 mm; tooth should read 7.851 mm

Roughness grade of a turned face · = 0.2 mm/rev, 0.8 mm nose radius (chapter 4): ≈ 1.6 µm
  1. N grades double from N1 = 0.025 µm
  2. = 7

Answer: N7

Flatness with an optical flat · 4 straight-curved fringes under sodium light, = 0.5893 µm
  1. Each fringe = = 0.295 µm
  2. 4 × 0.295

Answer: Flatness error ≈ 1.18 µm

Keep going

Recommended reading

  • Manufacturing Technology, Vol. II: Metal Cutting and Machine Tools, P. N. Rao
  • Fundamentals of Machining and Machine Tools, G. Boothroyd and W. A. Knight
  • Metal Cutting Principles, M. C. Shaw
  • Production Technology, HMT Bangalore
  • Manufacturing Engineering and Technology, S. Kalpakjian and S. R. Schmid
  • CNC Machines, B. S. Pabla and M. Adithan
  • Engineering Metrology and Measurements, N. V. Raghavendra and L. Krishnamurthy
  • Engineering Metrology, R. K. Jain

How this book was made

Chapters follow the official syllabi listed above. Every interactive's formulas and every worked-example number were checked by script. Explanations, animations and examples are original to Skill-Lync.

From the exam to a core job

Talk to a counsellor.

Ask how design and manufacturing engineers use machining science, machine tools and metrology on real projects, and what the Geometric Dimensioning and Tolerancing course covers.

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.

Talk to a career counsellor

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.