CNC machining and CAM

In short

Computer Numerical Control (CNC) is machine-tool control in which a stored program of coded instructions drives servo-powered axes and the spindle instead of a human turning handwheels. CAM (computer-aided manufacturing) is the software step that converts CAD geometry into tool paths and then into that program through a post processor. Together they govern practically all modern Indian production machining - automotive components at Bosch, Sundram Fasteners, Bharat Forge and Rane, aerospace parts at HAL and Godrej Aerospace, and tooling at Pune, Rajkot, Coimbatore and Faridabad clusters. The topic carries steady marks in university Manufacturing/CAD-CAM papers and in GATE (part programming, interpolation, speed-feed-time calculations), and it is the single most asked practical area in production-engineering interviews and NSQF/ITI trade tests.

Explained

From NC to CNC, DNC and the elements of a CNC machine

• NC (numerical control): instructions on punched tape read block by block by hard-wired control logic; no memory, no editing, no calculation. Developed at MIT around 1952 for Parsons' helicopter rotor work.
• CNC: a dedicated computer (microprocessor control) holds the program in memory, so editing, scaling, mirroring, canned cycles, interpolation, diagnostics and tool management are possible on the machine.
• DNC (direct/distributed numerical control): one host computer serves several machines over a network, downloading programs and collecting shop-floor data; drip-feeding is used for large 3D programs that exceed machine memory.
• Adaptive control: sensors measure cutting force, power or vibration and the control alters feed or speed in real time - used for forgings and castings with varying allowance.
• Main elements: MCU (machine control unit, split into DPU - data processing unit, and CLU - control loop unit), drive motors (AC servo), ball screws or linear motors, slideways (LM guideways, hydrostatic on heavy machines), feedback devices (rotary encoder, resolver, linear scale), ATC (automatic tool changer) with tool magazine, APC (automatic pallet changer), coolant and chip conveyor, sheet-metal enclosure with interlocks.
• Ball screw: recirculating-ball lead screw, preloaded to eliminate backlash, efficiency about 90% against roughly 30-40% for an acme screw; this is why CNC axes can be position-controlled accurately.
• Why a recirculating ball nut and not a plain nut: rolling contact gives low friction, no stick-slip at low feed, and long life at high duty.

Classification of CNC systems

• By motion: point-to-point (PTP) - positioning only, path between points not controlled (drilling, boring, spot welding, punch press); straight-cut - motion along one axis at a controlled feed; contouring (continuous path) - simultaneous coordinated axes, required for profiles and curves (milling, turning, flame cutting).
• By control loop: open loop - stepper motors, no feedback, cheap, used on light routers and plasma tables, loses steps under load; closed loop - servo with encoder feedback, corrects position error, used on all production machines.
• By feedback location: semi-closed loop - encoder on the motor/ball screw (does not see screw wear or thermal growth); full closed loop - linear scale on the slide, measures the actual table position.
• By number of axes: 2-axis (lathe: X, Z), 2½-axis (milling in XY with stepped Z), 3-axis, 4-axis (rotary table A or B), 5-axis (two rotary axes; simultaneous 5-axis for impellers, blisks, dies), and multi-tasking mill-turn centres.
• Machine types: CNC turning centre (with/without sub-spindle, Y-axis, bar feeder), vertical machining centre (VMC) and horizontal machining centre (HMC), CNC drilling/tapping centre, CNC cylindrical and surface grinders, CNC EDM and wire-EDM, turret punch press, laser/plasma profile cutters, CNC gear hobbing.
• Axis convention (ISO 841 / IS 8403 style): Z is always along the spindle axis, positive away from the work; X is the longest travel perpendicular to Z; Y completes the right-hand set. A, B, C are rotations about X, Y, Z. On a lathe, X is the cross-slide (diameter direction), Z along the bed.

Part programming - structure, G codes and M codes

• Program structure: program number (O1234 or %), blocks (lines) of words; a word = address letter + number (G01, X25.0, F120). Block format used today is word address with variable block length; older formats were fixed-block and tab-sequential.
• Common addresses: N block number, G preparatory, X/Y/Z coordinates, I/J/K arc-centre vectors or arc radius alternative R, F feed, S spindle, T tool, M miscellaneous, D/H offset numbers, P/Q/R cycle parameters.
• Coordinate modes: G90 absolute - all coordinates from the program zero; G91 incremental - each move measured from the present point. (On many Fanuc lathes, U and W are the incremental words instead.)
• Key preparatory functions:
  • G00 rapid traverse; G01 linear interpolation at feed; G02 circular clockwise; G03 circular counter-clockwise.
  • G04 dwell; G17/G18/G19 plane selection XY/ZX/YZ; G20/G21 inch/metric (G70/G71 on some lathes).
  • G28 return to machine reference (home); G40/G41/G42 cutter radius compensation off/left/right; G43/G44/G49 tool length compensation positive/negative/cancel.
  • G54-G59 work coordinate systems (work offsets); G92 set/shift coordinate system (on lathes also thread-cutting in some dialects); G94/G95 feed per minute / per revolution; G96/G97 constant surface speed on/off (lathe).
  • G98/G99 (milling) return to initial plane / R plane after a drilling cycle.
• Canned (fixed) cycles - milling: G81 drill, G82 drill with dwell (counterbore), G83 peck drill (deep holes, chip breaking), G84 tapping, G85/G86 boring, G76 fine boring. Format: G81 X.. Y.. Z.. R.. F..; R is the rapid-approach plane.
• Canned cycles - turning (Fanuc style): G71 rough turning, G72 rough facing, G70 finishing, G73 pattern repeat, G74/G75 peck drilling/grooving, G76 multiple-repetitive threading, G92 single-cycle threading.
• Miscellaneous (M) functions: M00 program stop, M01 optional stop, M02 end of program, M03/M04 spindle CW/CCW, M05 spindle stop, M06 tool change, M08/M09 coolant on/off, M30 end and rewind, M98/M99 subprogram call/return.
• Compensations: tool length offset (H) accounts for each tool's gauge length so one program suits any tool; cutter radius compensation (G41 left / G42 right of the direction of travel) lets the programmer write the finished part profile, not the cutter-centre path, and lets a resharpened or different-diameter cutter be used by changing only the D offset value. Tool nose radius compensation (G41/G42 with the lathe nose radius in the offset page) corrects taper and radius profiles on turning.
• Subprograms and macros: repeated features are written once and called with M98 P… L… (Fanuc) or as parametric macros (custom macro B - variables #100 series, IF/WHILE/GOTO) for bolt-hole circles and families of parts.
• Program zero and setting: machine zero (home) is fixed by limit switches/encoder reference; work zero (program zero) is chosen by the programmer at a convenient datum (a corner, a bore centre, the component face on a lathe) and set into G54 by edge finder, dial indicator or 3D probe; tool lengths are set by a tool presetter or by touching off.

CAM - from CAD model to verified program

1. Geometry: import or create the model (STEP/IGES/Parasolid, or native SolidWorks/CATIA/NX/Creo); identify machined faces and stock.
2. Stock and setup definition: billet/casting size, work coordinate system, clamping, machine selection.
3. Operation/feature selection: face, contour (2D profile), pocket, slot, drill, thread mill, 3D surface roughing and finishing (parallel, contour/Z-level, scallop, pencil trace), rest machining of leftover material.
4. Tool and cutting-data selection: tool from the library with holder, then Vc, fz, ap (depth of cut), ae (width of cut), stepover, stepdown - usually from the tool maker's catalogue data for the work material.
5. Tool-path generation and link/lead moves: entry (ramp, helical, pre-drilled plunge), exit, clearance planes, rapid links, trochoidal/high-efficiency roughing for hard materials, constant-engagement (adaptive) roughing to hold a steady chip load.
6. Simulation and verification: tool-path verify, material removal simulation, gouge and holder-collision check, machine-kinematics (full-machine) simulation for 4/5-axis, then post-processing by a machine-specific post processor into G code.
7. Transfer and proving: DNC/USB transfer, dry run above the part, single-block with feed override, first-off inspection, then production; good shops keep the proven program and offsets under revision control.
8. CAM strategies to know: 2½-axis vs 3-axis vs 5-axis; climb (down) milling - preferred on CNC because the ball screw has no backlash, giving better finish and tool life; conventional (up) milling on hard-skinned castings; constant surface speed on lathes; high-speed machining (HSM) - light depth, high feed, smooth corner-looping tool paths, trochoidal slots.
9. APT (Automatically Programmed Tool): the classic language-based CAM - statements of three kinds: geometry (P1 = POINT/10,20,0; L1 = LINE/P1,P2), motion (GOTO, GOLFT, TLLFT, GOFWD) and post processor/auxiliary (CUTTER/10, FEDRAT/150, SPINDL/1200, COOLNT/ON, FINI). It is examined mainly for the geometry and motion statement syntax; industry now uses interactive graphic CAM.
10. CNC simulators used for teaching in India: Fanuc/Siemens control simulators, MasterCAM, Fusion 360, NX CAM, SolidCAM, and ITI/NSQF workshop practice; "CNC operator - turning/milling" and "CNC programmer" are NSQF-aligned job roles under the Capital Goods Skill Council.

Accuracy, metrology and machine capability

• Resolution (BLU - basic length unit): the smallest programmable increment, typically 0.001 mm on production machines; resolution = ball-screw pitch / (encoder pulses per rev × gear ratio).
• Accuracy vs repeatability: accuracy is closeness to the commanded position; repeatability is scatter on repeated approach - a machine can be repeatable but inaccurate, and that can be compensated (pitch-error compensation tables), whereas poor repeatability cannot.
• Error sources: ball-screw pitch error, backlash and lost motion, thermal growth of screw and spindle, geometric errors (straightness, squareness, parallelism), tool deflection and wear, servo lag at corners, workholding error.
• Testing standards: ISO 230 series for machine-tool test code (geometric accuracy, positioning accuracy and repeatability, thermal effects) and ISO 10791 for machining centres; India adopts these as IS 2063 / IS 13178-type machine-tool test codes - check the current IS number as revisions occur. Laser interferometer, ballbar (circular test), and the NAS 979 circle-diamond-square cutting test are used for acceptance.
• Feed-rate interaction: a sharp corner in contouring causes servo-lag rounding; CAM therefore inserts corner feed reduction or looping. Interpolation approximates a circle by short linear chords inside a chordal-deviation tolerance; a coarse tolerance shows as faceting.
• Spindle and axis monitoring: vibration, spindle load meter, tool-breakage detection, in-process probing (Renishaw) for datum setting and post-process measurement.

Economics, safety and maintenance

• Advantages: high accuracy and repeatability; complex contours impossible manually; low setup-to-setup variation; fewer jigs and fixtures (soft jaws, simple plates instead of drill jigs); reduced lead time and inspection; one operator per several machines; easy design change by editing the program; consistent cycle time for costing.
• Limitations: high capital cost (a decent Indian-built VMC is roughly ₹18-40 lakh and an imported 5-axis machine ₹1 crore and above - prices vary widely, treat as indicative); skilled programmers and maintenance needed; higher power and air-conditioned/clean environment for high-end machines; not economical for one or two very simple parts; downtime cost is high.
• Break-even: CNC wins where batch size, complexity or tolerance make conventional setup time dominate; conventional/special-purpose machines win at very high volume with a single simple part.
• Safety and law: machines fall under the Occupational Safety, Health and Working Conditions Code, 2020 (OSH Code, in force 21 November 2025, which repealed the Factories Act, 1948) and its rules, which carry the former Section 21 (fencing of machinery) and Section 24 (striking gear) duties - guard interlocks, emergency stop, two-hand/door interlock on bar feeders; IS/ISO 16090 style safety requirements for machining centres; compressed-air and coolant mist control, coolant-management (skin and bacteria risk), chip-handling PPE, and lockout-tagout for maintenance.
• Maintenance: daily - coolant level and concentration (refractometer), chip clearing, way-lube level, air-filter water drain; weekly - filter cleaning, spindle taper cleaning; periodic - ball-screw and guideway lubrication, backlash check, geometric check with ballbar, spindle-run-out check, battery replacement for parameter/encoder memory (losing it loses the machine's zero).
• Industry 4.0 link: MTConnect/OPC-UA data from controls, machine monitoring dashboards (OEE), digital twin, tool-life prediction - increasingly asked by employers like Bosch, Tata Motors and the Indian machine-tool makers (BFW, Jyoti CNC, Ace Micromatic, Macpower, HMT).

Key points

• CNC - machine control by a stored program run on a dedicated computer, allowing editing, canned cycles and interpolation on the machine.
• CAM - software that converts CAD geometry into tool paths and, through a post processor, into machine-specific G code.
• MCU - the control unit; DPU reads and decodes blocks, CLU drives the axes and reads feedback.
• PTP vs contouring - PTP controls only end positions (drilling); contouring controls the whole path (profile milling, turning).
• Open vs closed loop - stepper without feedback vs servo with encoder; production machines are closed loop.
• Semi-closed vs full closed loop - feedback from the motor/screw vs a linear scale on the slide.
• Ball screw - preloaded recirculating-ball screw, near-zero backlash, about 90% efficient; makes accurate position control possible.
• Z axis - always along the spindle axis, positive away from the work (ISO convention); X is the longest travel perpendicular to Z.
• G90/G91 - absolute (from program zero) vs incremental (from the current point) programming.
• G00/G01/G02/G03 - rapid, linear feed, circular CW, circular CCW interpolation.
• G41/G42 - cutter radius compensation left/right of the travel direction, so the part profile can be programmed directly.
• G43/H - tool length offset, letting each tool run the same program regardless of its gauge length.
• G54-G59 - work coordinate systems; work zero is the programmer's datum, machine zero is fixed by the reference switches.
• Canned cycle - one block replacing many (G81 drill, G83 peck, G84 tap, G71 rough turn, G76 thread).
• M codes - machine functions: M03 spindle CW, M06 tool change, M08 coolant on, M30 end and rewind.
• BLU/resolution - smallest programmable step = screw pitch / (encoder counts × gear ratio), typically 0.001 mm.
• Climb milling is preferred on CNC (no backlash), giving better surface finish and tool life.
• Accuracy vs repeatability - a systematic accuracy error can be mapped and compensated; poor repeatability (scatter) cannot.

Formulas and examples

Example 1 - speed, feed and milling time. A 63 mm, 5-insert face mill cuts mild steel at Vc = 180 m/min, fz = 0.2 mm/tooth. The face is 300 mm long; approach + overtravel = 70 mm; ap = 2 mm, ae = 50 mm.

• N = 1000 × 180 / (π × 63) = 180000 / 197.92 = 909 rpm (set 900 rpm).
• At 900 rpm: Vf = 0.2 × 5 × 900 = 900 mm/min.
• Travel L = 300 + 70 = 370 mm → T = 370 / 900 = 0.411 min ≈ 24.7 s.
• MRR = 2 × 50 × 900 = 90,000 mm³/min = 90 cm³/min.

Example 2 - turning passes and cycle time. A shaft of 60 mm diameter is turned to 50 mm over a 200 mm length, Vc = 150 m/min, f = 0.25 mm/rev, maximum depth of cut 1.25 mm. Approach 5 mm.

• Radial stock = (60 − 50)/2 = 5 mm → passes = 5 / 1.25 = 4 passes.
• Using the mean diameter 55 mm for speed: N = 1000 × 150 / (π × 55) = 150000 / 172.79 = 868 rpm.
• Feed rate Vf = 0.25 × 868 = 217 mm/min; length per pass = 205 mm → 205 / 217 = 0.945 min per pass.
• Cutting time ≈ 4 × 0.945 = 3.78 min (a real CNC with G96 constant surface speed would differ slightly, as N rises as the diameter falls).

Example 3 - absolute vs incremental and a full milling program. Mill a 60 × 40 mm rectangular profile (outside contour, corner radius 8 mm) and drill two 8 mm holes, work zero at the bottom-left corner of the profile, Ø10 mm cutter, G42 with D01 = 5.0.

O0101
N10 G21 G17 G40 G49 G80 G90        (metric, XY plane, cancels on)
N20 G54 G00 X-20. Y-20. S1800 M03  (work offset, clear start, spindle on)
N30 G43 H01 Z25. M08              (tool length offset, coolant on)
N40 G00 Z2.
N50 G01 Z-5. F80                  (plunge 5 mm deep, clear of the part)
N60 G42 D01 G01 X0 Y0 F150        (cutter comp right, approach profile)
N70 G01 X52. Y0
N80 G03 X60. Y8. R8.              (CCW corner radius 8)
N90 G01 X60. Y32.
N100 G03 X52. Y40. R8.
N110 G01 X8. Y40.
N120 G03 X0 Y32. R8.
N130 G01 X0 Y8.
N140 G03 X8. Y0 R8.
N150 G40 G01 X-20. Y-20.          (cancel comp, retract clear)
N160 G00 Z25. M09
N170 T02 M06                      (8 mm drill)
N180 G43 H02 S2400 M03
N190 G00 X15. Y20.
N200 G99 G81 Z-18. R2. F120       (drill cycle, return to R plane)
N210 X45.                         (second hole, cycle repeats)
N220 G80 G00 Z25. M09
N230 G28 G91 Z0
N240 G90 M30

• In G91 the same two holes would be N190 G90 G00 X15. Y20. then G91 X30. - the second hole is 30 mm to the right of the first, not at 45 from the datum. Mixing the two is the commonest programming error.

Example 4 - resolution and chordal deviation. A machine has a 5 mm pitch ball screw directly coupled to a 1,000-pulse/rev encoder with ×4 quadrature decoding.

• Effective counts = 1000 × 4 = 4,000 per revolution → BLU = 5 / 4000 = 0.00125 mm (1.25 µm).
• If a 20 mm radius arc is approximated by 1 mm chords, h ≈ 1² / (8 × 20) = 0.00625 mm (6.25 µm) - visible as faceting on a finished surface, so the CAM tolerance must be tightened or true G02/G03 circular interpolation used.

Example 5 - CNC versus conventional, break-even. A bracket needs 45 min on a conventional milling machine (₹400/h machine + operator) with 90 min setup, or 9 min on a VMC (₹900/h) with 30 min setup and a ₹2,500 one-time programming cost.

• Conventional, batch Q: cost = (90/60 × 400) + Q × (45/60 × 400) = 600 + 300Q.
• CNC, batch Q: cost = 2500 + (30/60 × 900) + Q × (9/60 × 900) = 2500 + 450 + 135Q = 2950 + 135Q.
• Break-even: 600 + 300Q = 2950 + 135Q → 165Q = 2350 → Q ≈ 14.2, so from about 15 pieces onward the CNC is cheaper, and the gap widens fast (at Q = 100: ₹30,600 against ₹16,450).

Where it is used

• Automotive and auto components: engine blocks, cylinder heads, crankshafts, transmission housings and fasteners at Maruti Suzuki, Tata Motors, Bosch, Bharat Forge, Sundram Fasteners, Rane and the Pune-Chakan, Chennai, Gurgaon-Manesar and Rajkot supplier clusters - HMC lines with pallet changers and in-process probing.
• Aerospace and defence: 5-axis machining of blisks, structural ribs and casings at HAL, BEL, Godrej Aerospace, Tata Advanced Systems, L&T Defence - full-machine simulation is mandatory because collisions are costly.
• Die, mould and tool rooms: CNC HSM of hardened steel, graphite electrodes, wire-EDM; Pune, Faridabad, Coimbatore, Ludhiana and Rajkot tool rooms, plus government tool rooms (CITD Hyderabad, IGTR Aurangabad/Indore).
• Machine-tool builders: Ace Micromatic, BFW, Jyoti CNC, Macpower, HMT and Lakshmi Machine Works build and service CNC machines; Fanuc, Siemens and Mitsubishi supply controls.
• Job roles: CNC programmer/CAM engineer, setter-cum-operator, process planner, tool engineer, production engineer, applications engineer at tool makers (Sandvik, Kennametal, Taegutec), CMM/quality engineer, service engineer on controls and drives.
• Medical, electronics and energy: implants and surgical instruments, enclosures and heat sinks, turbine and pump components at BHEL and Kirloskar.

Interview questions

• Q: What is the difference between NC and CNC? A: NC used hard-wired logic reading a tape block by block with no memory; CNC stores the program in a computer, so it can be edited, calculated with, and given canned cycles, interpolation and diagnostics.
• Q: Why is the Z axis defined along the spindle? A: By the ISO convention Z lies along the main spindle axis with positive away from the work, so tool-length and depth programming is consistent on any machine.
• Q: Explain cutter radius compensation and why it is useful. A: G41/G42 offsets the cutter centre from the programmed line by the radius in the D offset, so the finished profile can be programmed directly and a different or resharpened cutter needs only a change of offset value, not of the program.
• Q: G90 or G91 - which would you use for a bolt-hole pattern repeated at four places? A: Program the pattern incrementally in a subprogram and call it from four absolute positions; that way the pattern is written once.
• Q: What is the difference between semi-closed and full closed loop? A: Semi-closed loop takes feedback from the motor or screw end, so screw wear and thermal growth are invisible; full closed loop reads a linear scale on the slide and measures where the table actually is.
• Q: Why do CNC machines use ball screws? A: Rolling contact gives about 90% efficiency, no stick-slip at low feed and, when preloaded, almost no backlash, which is essential for accurate position control and climb milling.
• Q: Which is better on CNC, climb or conventional milling, and why? A: Climb (down) milling, because the backlash-free ball screw can resist the pull-in force; it gives thinner chips at exit, better finish and longer tool life. Conventional milling is still used on hard-skinned castings and forgings.
• Q: What does a post processor do? A: It translates the CAM system's generic tool-path file (CL data) into the exact G/M-code dialect, formats and limits of a particular machine and control.
• Q: A part comes out oversize by 0.2 mm on diameter. What do you check? A: Tool wear and the tool nose-radius/diameter offset first, then the work offset, tool deflection and whether the finishing pass had enough stock; correct by trimming the wear offset by 0.2 mm on diameter (0.1 mm on radius).
• Q: What is the difference between machine zero and work zero? A: Machine zero (home) is a fixed reference found by the limit switch/encoder marker; work zero is the programmer's datum on the part, stored in G54-G59 as an offset from machine zero.
• Q: How do you prove a new program safely? A: Simulate and collision-check in CAM, then on the machine run a dry run with the Z axis shifted up, single-block with 10-25% feed override and hand on the feed-hold, check the first piece fully, then release to production.
• Q: What is adaptive control, and where would you use it? A: The control adjusts feed or speed in real time from measured force, power or vibration; it is useful when the stock allowance varies, as on castings and forgings, or to protect a long fragile tool.

Common mistakes

• Mixing G90 and G91 in the same block sequence, so later moves land at the wrong place - and forgetting that a canned cycle repeats on every following coordinate block until G80.
• Writing the cutter-centre path and also switching on G41/G42, so the part comes out undersize or oversize by the full cutter diameter.
• Forgetting G43 H.. (tool length offset) or leaving the previous tool's H active - the classic cause of a crash into the table.
• Quoting the cutting speed Vc as the spindle speed N, or using the work diameter instead of the tool diameter in milling and drilling.
• Using feed per tooth as the feed rate: Vf = fz × z × N, so a 5-tooth cutter runs five times the per-tooth value.
• Leaving out approach and overtravel in machining-time questions, and ignoring the number of passes when the depth of cut is limited.
• Assuming a repeatable machine is automatically accurate, or that a simulation that looks right is a collision-free proof - the holder and fixture must be modelled too.

Related topics

• Theory of metal cutting · Machining and machine tools · Jigs and fixtures · Metrology and quality control · Non-traditional machining · Additive manufacturing (3D printing)