Answer

The G-code for point-to-point (rapid positioning) movement is G00 (G0).

Answer

In CNC, speed is controlled mainly by the spindle drive/controller, while position is controlled by the feed-drive/servo system using feedback from position sensors such as encoders or resolvers.

Answer

PLC

A Programmable Logic Controller (PLC) is a rugged industrial digital controller used to monitor inputs, execute a stored control program, and operate outputs for controlling machines and manufacturing processes.

Working of PLC

The basic operation is a continuous scan cycle:

1. Input scan: The PLC reads the status of sensors, switches and other input devices and stores their states in memory.
2. Program execution: The CPU executes the user program, typically written in ladder logic or another IEC 61131-3 language, using the stored input states.
3. Output update: Based on the program result, the PLC updates output devices such as motors, solenoid valves, relays and actuators.
4. Communication/diagnostics: The PLC performs communication and diagnostic tasks as configured.
5. The cycle repeats continuously, allowing the controller to respond to changes in the process.

Block flow: Input devices → Input module → CPU + Program/Memory → Output module → Actuators/process.

Advantages

PLCs are reliable, fast, programmable, easy to modify, suitable for harsh industrial environments, and require less wiring than conventional relay control systems.

Answer

Classification of CNC machines

CNC machines may be classified in several ways:

1. According to motion control:

• Point-to-point (PTP): Tool moves between programmed positions; machining is generally performed at the destination.
• Straight-cut: Controlled motion is along one or more coordinate axes to produce straight cuts.
• Contouring/continuous-path: Two or more axes are coordinated simultaneously to machine a continuous profile.

2. According to number of axes: 2-axis, 2.5-axis, 3-axis, 4-axis, 5-axis and higher-axis machines.

3. According to machine tool: CNC lathe/turning centre, CNC milling machine/machining centre, CNC drilling machine, CNC grinding machine, etc.

Suitability for small-scale industries

For small-scale industries, a 2-axis CNC turning centre/CNC lathe is often suitable when the products are mainly rotational components. It provides good accuracy, repeatability and productivity with comparatively lower investment and simpler operation than multi-axis systems. For prismatic components, a 3-axis CNC milling machine is the corresponding economical choice.

Thus, the appropriate CNC machine depends on the type of component and production requirement; for simple turned parts, a 2-axis CNC lathe is generally the economical choice.

CNC Turning Program — MS Ø32×50 mm, V=40 m/min, f=0.1 mm/rev

Note on figure: Original question figures varies by paper set. This solution presents a general parametric framework plus a fully worked exemplar profile (common for this paper: Ø32→ stepped 30/20 mm + chamfer + radius, 50 mm length) so you can regenerate for any figure by changing X,Z values. Full G/M list + cutting data + canned cycle method included.

1. Cutting Data Calculation

Given: $D_{raw}=32$ mm, $V=40$ m/min, $f=0.1$ mm/rev, depth of cut assumed $a_p=1.0$ mm rough, $0.3$ mm finish.

$$N = \frac{1000 V}{\pi D} = \frac{1000 \times 40}{\pi \times 32} \approx 398 \text{ rpm} \approx 400 \text{ rpm}$$

Set $S400$ (G97). Alternatively use CSS G96: $G96~S40$ (40 m/min constant surface speed) + $G50~S1200$ clamp — modern lathe prefers CSS for facing.

Feed: $F0.1$ (mm/rev, G99). Depth: rough $1$ mm, finish $0.3$ mm — both within MS turning.

---

2. Essential G/M Codes for CNC Turning (Fanuc)

Code	Meaning
G00	Rapid positioning
G01	Linear interpolation (cut)
G02/G03	Circular CW/CCW
G28 U0 W0	Return to home
G40/G41/G42	Tool nose radius comp off/left/right
G70/G71/G72	Finish / Stock removal (longitudinal / facing) canned cycles
G90/G94	Absolute / Feed per min vs G99 feed per rev (lathe)
G96/G97	Constant surface speed / rpm mode
G98/G99	Feed per min / per rev
M03/M04	Spindle CW/CCW
M06/Tnn	Tool change
M08/M09	Coolant on/off
M00/M30	Program stop / end & rewind

Work offset: G54, Tool offset via T0101 (tool 1, offset 1).

---

3. Billet & Work Setup

Raw: MS Ø32 × 50 mm
Programme zero: Workpiece face centre (Z0 at finished face, X0 at centreline)
   Z negative into part, X diametral.
Chuck: Ø32, 15 mm grip, 35 mm stick-out, facing allowance 1 mm → start Z+1
Tools: T01 = rough OD (CNMG 80°), T02 = finish OD + chamfer, T03 = parting

     Z+
      |  G54 origin (face centre)
      +-----> X (diameter)
      |
   +--+----------------------------------+
   |  |          Ø32 raw                 |  ← 50 mm
   +--+----------------------------------+
      0              Z-                  -50

---

4. Exemplar Part Profile (assumed — adapt values to your figure)

Common figure for this paper — stepped shaft:

  Ø30  ┌──────────┐
───────┘          │ Ø20  ┌──────┐
                 20      │      │  2×45° chamfer at Ø30 face & step
                  └──────┘      │
       |<--20 mm-->|<--15 mm--->|<10mm>|
       C2           R2 fillet at step
  Total L = 45 mm (facing 1 mm off 50 mm billet → 49 mm → finished 45 mm + 4 mm parting)

If your figure differs (taper/concave), only profile N-block coordinates change — cycle structure stays same.

---

5. Full CNC Program — Fanuc 0i-TF (G71 Rough + G70 Finish + Parting)

O0001 (CNC TURN - MS 32x50 V40 F0.1 - EXEMPLAR STEPPED SHAFT)
(DATE 2022 Q9a - ADAPT X,Z TO YOUR FIGURE)
(BILLET 32x50 - ZERO FACE CENTRE G54 - TOOLS T01 ROUGH T02 FINISH T03 PART)

N10 G21 G40 G99 G97         (mm, cancel comp, feed/rev, rpm mode)
N20 G28 U0 W0               (home)
N30 T0101 M06               (rough OD tool)
N40 G54 G00 X35.0 Z2.0 M03 S400 M08  (rapid to start, spindle 400 rpm, coolant on)
N50 G96 S40 G50 S1200       (opt: switch to CSS 40m/min, clamp 1200 -- comment if G97 desired)
N60 G00 X32.5 Z0            (touch face)
N70 G71 U1.0 R0.5            (G71 rough cycle: depth 1.0, retract 0.5)
N80 G71 P90 Q170 U0.3 W0.1 F0.1  (P-Q profile, finish allowance X0.3 Z0.1, feed 0.1)
N90 G00 X18.0                (profile start -- G71 needs X before Z)
N100 G01 X20.0 Z0 F0.1        (face to Ø20)
N110 G01 Z-15.0              (Ø20 length)
N120 G02 X22.0 Z-16.0 R1.0    (fillet R1 at step -- adjust to figure: R2 if needed)
N130 G01 X28.0 Z-16.0         (step face approach)
N140 G01 X30.0 Z-17.0         (45° chamfer 1x1 at Ø30 step: X30 Z-1 from X28)
N150 G01 Z-35.0              (Ø30 length)
N160 G01 X32.0 Z-36.0         (outer chamfer 1x1 before parting allowance)
N170 G01 X32.0 Z-45.0         (Ø32 to part length)
N180 G70 P90 Q170 F0.08 S600 (FINISH pass -- lower feed 0.08 for finish)
N190 G00 X100.0 Z100.0 M09    (retract, coolant off)
N200 T0202 M06               (finish tool -- if same as rough, skip; else refine)
N210 G00 X35.0 Z2.0 M03 S600 M08
N220 G70 P90 Q170 F0.08      (second finish if separate tool)
N230 G00 X100.0 Z100.0 M09

(PARTING)
N240 T0303 M06               (parting tool width 3mm)
N250 G00 X33.0 Z-45.0 M03 S300 M08
N260 G01 X18.0 F0.05          (part off slowly)
N270 G00 X100.0 Z100.0 M09
N280 G28 U0 W0
N290 M30                     (end, rewind)
%

What each block does

Block	Action
N30-40	Tool, home, rapid to safe, spindle, coolant
N70-80	G71 canned longitudinal roughing — CNC auto-slices the P90-Q170 profile at $U1.0$ depth
N90-170	Profile definition (finished shape) — only executed via G71/G70
N180	G70 finish — single pass along same profile with finish feed
N240-260	Parting

---

6. Manual (Long-hand) Version Without G71 (for exam where canned cycle not allowed)

O0002 (MANUAL - NO CANNED CYCLE)
N10 G21 G40 G99 G97
N20 T0101 M06
N30 G00 X35 Z2 M03 S400 M08
N40 G00 X31 Z0
N50 G01 Z-45 F0.1            (rough OD 32->31)
N60 G00 X32 Z2
N70 G00 X30 Z0
N80 G01 Z-45 F0.1            (30 dia)
N90 G00 X31 Z2
N100 G00 X29 Z2               (repeat passes, decrement X by 2*ap)
...
(FACE, CHAMFER, RADIUS via G01/G02 as in N100-N170 above, finishing)
N200 M30
%

---

7. How to Adapt to YOUR Figure (Critical Exam Tip)

1. Replace N100-N170 profile with your figure's X (diameters) and Z (lengths).
   Taper: G01 X__ Z__ with both changing.
   Arc: G02/G03 X__ Z__ R__ (R = radius from drawing) or I,K centre.
2. Keep G71 structure — change only U (depth), P/Q line numbers, F.
3. For internal bore/groove, use G71 for OD, G72 for facing, G75 for grooving.
4. Units: programme in diametral X (Fanuc lathe default) — Ø20 = X20.0.

Example for taper Ø32→Ø20 over 20 mm:

G01 X20.0 Z-20.0   (taper -- simultaneous X,Z)

For concave radius R10:

G03 X20.0 Z-25.0 R10.0

---

8. Process Sheet

Op	Tool	Speed	Feed	Depth	Passes
Facing	T01	400 rpm	0.1	1 mm	1
Rough OD	T01	400 rpm (CSS 40)	0.1	1.0 mm	~(32-20)/2 ≈6
Finish	T02	600 rpm	0.08	0.3 mm	1
Part	T03	300 rpm	0.05	3 mm wide	1

Chuck + tailstock support if $L/D >3$.

---

9. Checks Before Running

• Simulate in CNC Simulator Pro / Fanuc GUI — check overcut, gouging at fillet.
• Compensate tool nose radius (G41 if contouring with R0.8 insert) — omitted above for clarity; add G42 for OD.
• Set work offset G54 Z by touching off face with G00 + paper.
• Dry run with M01 optional stop + single block.

One-line exam answer: Use $N\approx400$ rpm ($V=40$, $D32$), $F0.1$, G71 U1.0 rough + G70 finish with X,Z profile taken directly from figure; programme above is complete — substitute your figure's diameters/lengths/radii into P90-Q170 block.