Turning, milling, drilling and grinding; machining time

Why it matters

Crankshaft journals are turned and ground, cylinder-head faces milled, oil galleries drilled and gear bores ground – and every one of these operations is planned from the same few relations between cutting speed, spindle speed, feed and depth of cut. Machining time sets cycle time and cost, and material removal rate times specific energy sets the machine power. These calculations appear in almost every manufacturing paper.

Key ideas

Three cutting parameters. Cutting speed V (m/min) is the surface speed of work relative to tool; it is chosen from the tool–work pair (tool life). Feed f is the advance per revolution (mm/rev), per tooth (mm/tooth) or per minute (mm/min); it controls finish and force. Depth of cut d (mm) is the thickness removed in one pass. Spindle speed follows from V and the diameter of whatever rotates.

Turning (lathe). The work rotates; a single-point tool feeds along (straight turning), across (facing), at an angle (taper turning), or forms threads, grooves and bores. In straight turning, the depth of cut is half the diameter reduction. Approach and overtravel are added to the length of cut. Surface roughness depends mainly on feed and nose radius (covered in the surface-finish topic).

Drilling. The twist drill rotates and feeds axially; the standard point angle is 118°, so the drill must travel an extra approach equal to the cone height before the full diameter cuts, and a through hole needs a little overtravel. Related operations: reaming (finishing a drilled hole to size and finish), boring (enlarging and correcting position), counterboring, countersinking, spot-facing and tapping.

Milling. A multi-tooth rotating cutter, with the work fed past it. Each tooth cuts an intermittent, variable-thickness chip.

• Peripheral (slab) milling – cutter axis parallel to the surface. Up (conventional) milling – cutter rotation opposes the feed; chip thickness grows from zero; tends to lift the work; safer on machines with backlash. Down (climb) milling – rotation along the feed; chip starts thick; better finish and tool life, pulls the work into the table; needs a backlash-free feed drive.
• Face milling – cutter axis perpendicular to the surface; most flat surfaces on blocks and heads.
• End milling – slots, pockets, profiles.
• Before full-depth cutting starts, the cutter must travel an approach distance that depends on cutter diameter and depth (slab) or on width of cut (face).

Grinding. A bonded abrasive wheel acts as a huge number of tiny cutting edges with large negative rake. Very small chips, high specific energy (several times that of turning), high surface speed (typically tens of m/s), fine finish and close tolerance, and the ability to cut hardened steel.

• Wheel specification: abrasive type (A = aluminium oxide for steels; C = silicon carbide for cast iron, non-ferrous and non-metallic; CBN and diamond superabrasives), grain size (higher number = finer), grade (hardness of the bond, A soft … Z hard), structure (grain spacing) and bond (V vitrified, B resinoid, R rubber, M metal), e.g. A 46 K 5 V.
• Rule of thumb: soft wheel for hard work (grains break out and expose fresh edges), hard wheel for soft work.
• Glazing (dull grains, wheel too hard) and loading (chips clog pores, soft gummy work) are corrected by dressing; truing restores the wheel's geometry.
• Coolant is essential to avoid grinding burns, tempering of hardened surfaces and residual tensile stress.
• Types: surface, cylindrical (between centres), internal, centreless (crankshaft pins, gudgeon pins, valve stems), creep-feed.

Power. Cutting power = specific cutting energy × MRR; motor power = cutting power/mechanical efficiency. Specific energy depends on the material (take from a data book) and rises at small chip thickness – the "size effect" that makes grinding so energy-hungry.

Formulas

N = 1000·V / (π·D) N = spindle speed (rev/min), V = cutting speed (m/min), D = diameter of the rotating element – work in turning, tool in drilling and milling (mm).

T_m = (L + A + O) / (f·N) Machining time (min) for turning and drilling; L = length of cut (mm), A = approach, O = overtravel (mm), f = feed (mm/rev).

MRR = V·f·d × 1000 (turning, mm³/min, V in m/min) ≈ π·D_avg·d·f·N Using D_avg = mean of initial and final diameters gives the exact value.

A_drill = (D / 2) / tan(θ / 2) MRR_drill = (π·D² / 4)·f·N θ = point angle (118° standard ⇒ A ≈ 0.3·D).

f_m = f_z·Z·N Table feed (mm/min) in milling; f_z = feed per tooth (mm), Z = number of teeth.

A_slab = √(d·(D − d)) T_m = (L + A) / f_m Slab-milling approach (mm) and time (min); overtravel added if specified. For face milling with the cutter centred over a work of width w: A = O = 0.5·(D − √(D² − w²)) for a partial-width cut, and A = O = D/2 when the cutter must fully clear the work.

MRR_mill = w·d·f_m w = width of cut (mm), d = depth (mm).

P_c = u·MRR P_motor = P_c / η u = specific cutting energy (J/mm³), MRR in mm³/s, P in W; η = machine efficiency.

Worked examples

Example 1 (standard) – turning a shaft. A 60 mm bar is turned to 56 mm over 250 mm in one pass. V = 90 m/min, f = 0.25 mm/rev, approach + overtravel = 5 mm, u = 2.5 J/mm³.

1. d = (60 − 56)/2 = 2 mm.
2. N = 1000V/(πD) = 90 000/(π × 60) = 477.5 rev/min.
3. T_m = (L + A + O)/(f·N) = 255/(0.25 × 477.5) = 2.14 min.
4. MRR ≈ V·f·d = 90 000 × 0.25 × 2 = 45 000 mm³/min (exact, with D_avg = 58 mm: 43 500 mm³/min).
5. Cutting power = 2.5 × 45 000/60 = 1.88 kW.

Example 2 (GATE level) – slab milling. A plate 200 mm long and 50 mm wide is slab-milled to a depth of 5 mm with an 80 mm diameter, 8-tooth cutter at 300 rev/min and 0.1 mm/tooth. Overtravel is neglected.

1. f_m = f_z·Z·N = 0.1 × 8 × 300 = 240 mm/min.
2. A = √(d(D − d)) = √(5 × 75) = 19.36 mm.
3. T_m = (200 + 19.36)/240 = 0.914 min (54.8 s).
4. MRR = 50 × 5 × 240 = 60 000 mm³/min.

Example 3 – drilling a through hole. A 20 mm drill (118° point) drills a 40 mm deep through hole at V = 25 m/min, f = 0.2 mm/rev. N = 25 000/(π × 20) = 397.9 rev/min; A = 10/tan 59° = 6.01 mm; T_m = (40 + 6.01)/(0.2 × 397.9) = 0.578 min; MRR = (π/4)(20²)(0.2)(397.9) = 25 000 mm³/min.

Common mistakes

• Using the final diameter for spindle speed in turning; the cutting speed acts at the uncut (initial) diameter.
• Taking depth of cut as the diameter reduction instead of half of it.
• Forgetting the factor 1000 when V is in m/min and D in mm.
• Using feed per tooth as table feed in milling (multiply by Z and N).
• Leaving out the approach distance in milling and drilling when the question expects it – read whether approach/overtravel are to be included.
• Choosing a hard grinding wheel for hard work; the rule is the reverse.

For GATE ME

Expect machining-time and MRR calculations for turning, facing, drilling and milling (with approach), power from specific energy, the conversion between cutting speed and spindle speed, and conceptual questions on up vs down milling, grinding-wheel specification, glazing vs loading, dressing vs truing and centreless grinding. Practise approach-distance geometry for slab and face milling.

Quick check

1. Spindle speed for V = 31.4 m/min on a 10 mm drill?
2. Table feed for 6 teeth, 0.05 mm/tooth, 1000 rev/min?
3. In which milling mode does chip thickness start at zero?
4. What does "V" mean at the end of a grinding-wheel specification?
5. Turning time for L = 150 mm, f = 0.25 mm/rev, N = 600 rev/min (no approach)?

Answers: 1. 1000 rev/min; 2. 300 mm/min; 3. Up (conventional) milling; 4. Vitrified bond; 5. 1 min.