1. Part Programming
Turning Applications

2. Steps in Part Programming
Study of component drawing
Deciding sequence of operations
Identify machine tool
Selecting cutting tool
Deciding tool paths
Determining Machining Parameters
Preparing job and tool set-up plans
Writing Part Program
Testing Part Program
Documentation of Part Program

3. Terminology used in part programming
Absolute system :
The co-ordinates are mentioned with respect to one reference point (datum)
2. Incremental System :
The co-ordinates are mentioned with respect to the previous point (datum)

5. Terminology (Continued…)
3. Block and Words : Block - It is a group of words or coded instructions for the NC/CNC system to execute a particular movement Word - Each coded instruction

6. Terminology (Continued…)
The words in the block are in following order :
Sequence number (N)
Preparatory functions (G)
Dimensions (X,Y,Z,U,V,W and I,J,K)
Feed functions (F)
Spindle speed functions (S)
Tool functions (T)
Miscellaneous functions

7. Each line of program == 1 block
Each block is composed of several instructions, or (words)
Sequence and format of words:
N3 G X Y Z I J K F S4 T M2
destination coordinates
dist to center of circle
tool
sequence no
feed rate
spindle speed
preparatory function
miscellaneous function

8. 4. Formats Sequence of words in which information appears in a program
Word address format : Each word is identified by a letter
Tab sequence format : Each word is separated from the other by ‘Tab’ character
The words are identified by their respective
positions in the block

10. Commonly used ‘G’ codes
G00 Rapid Positioning 
Function: Moves to a new position as fast as possible. 
Syntax: G00 [axis words]
Example:
G00 X1.2 Y0.3 ; Moves to (1.2, 0.3)

11. G01 Linear Interpolation
Function: Moves to a new position linearly at some feed rate.
Syntax: G01 [axis words] [optional feed word]
Example:
G01 X1.2 Y0.3 F3.0  ;
Moves to (1.2,0.3) at 3 units/minute

12. G02 CW circular interpolation (3D)
Function:
Moves to a new position in a clockwise circular arc. The arc center is specified with signed offsets from the start position or implicitly by the magnitude of the radius
Syntax 1: G02 [two axis words (optional third)] [interpolation parameters] [optional feed word]
Syntax 2: G02 [two axis words (optional third)] [radius word] [optional feed word]

13. Example 1:
G (plane XY specified for clarity)
G00 X0 Y0 (get into start position)
G02 X2 Y0 I1 J0 F4

14. Example 2:
G (plane XY specified for clarity)
G00 X0 Y1 (get into start position) G02 X1 Y0 R1 F4

15. Important G- Codes G00 Rapid Transverse G01 Linear Interpolation G02
Circular Interpolation, CW
G03
Circular Interpolation, CCW
G17
XY Plane,G18 XZ Plane,G19 YZ Plane
G20/G70
Inch units
G21/G71
Metric Units
G40
Cutter compensation cancel
G41
Cutter compensation left
G42
Cutter compensation right
G43
Tool length compensation (plus)
G44
Tool length compensation (minus)
G49
Tool length compensation cancel
G80
Cancel canned cycles
G81
Drilling cycle
G82
Counter boring cycle
G83
Deep hole drilling cycle
G90
Absolute positioning
G91
Incremental positioning
Important G-
Codes

16. M-codes m Spindle off

17. COORDINATE SYSTEMS • Right hand rule
• Z axis align with the spindle - +Z moves away from the workpiece or the spindle.
• X axis - Lathe: perpendicular to the spindle.
Horizontal machine: parallel to the table.
Vertical machine: +X points to the right. 2

18. Z axis : align with the spindle
X axis : perpendicular to the spindle

19. Z axis : align with the spindle
X axis : perpendicular to the spindle

20. Other Axes Designations
Rotational axes (A,B,C)
Secondary linear axes (U,V,W)
Incremental dimensions in Circular Interpolation (I,J,K)

21. Zero points and Reference points
Machine zero point (M)-positive end of each axis travel range (Home position)
Blocking Point-Workpiece zero point (A)
Program zero point (W)-starting point of workpiece or like A
Start point (B)-first tool starts the machining process & is determined in program
Reference point (R)-floating point (determined by measuring system)

23. Cutting Process Parameter Selection
Cutting Speed (V) :
V=DN/1000
Feed(fm) :
fm= N x frev
Depth of Cut (t) :
t=(D1-D2)/2

24. Canned cycles Multiple repetitive cycles
Consist of series of motions repeated no. of times e.g. drilling , boring , tapping
Drilling cycle consist of:
Rapid approach to workpiece
Drill at feed rate
Rapid return to initial position

25. Commonly used Canned cycles
G74-Stock removal cycle
G78-Multiple threading cycle
G81-Drilling cycle
G85-Boring cycle

26. General Structure of Turning Part Program
N0 G Absolute program mode
N1 G Metric mode
N2 G93 M41 S RPM range, Medium speed
N3 G Feed rate (mm/min)
N4 G28 U0 W Go to Home Position
N5 M06 T Tool change 01 with offset 01
N6 M03 S Spindle ON
N7 G00 X50 Z1 M Rapid tool positioning to (50,1)
Coolant ON .

27. General Structure of Turning Part Program (Continued….)
N18 G00 X0 Z1 Rapid tool positioning to (0,1) N19 G28 U0 W0 Go to Home Position N20 M05 Spindle OFF N21 M09 Coolant OFF N22 M02 Program END N23 M30 END of tape and REWIND

28. Example 01- Step Turning Operation
N7 G00 X42 Z1 M08 N8 G00 X40 Z1 N9 G74 X30 Z-60 F0.2 D1 stock removal cycle N10 G00 X32 Z1 N11 G00 X30 Z1 N12 G74 X20 Z-30 F0.2 D1 N13 G00 X22 Z1

29. Example 02-Clockwise Nose Turning
N7 G00 X42 Z-20 M08 N8 G01 X40 Z-20 F0.2 S1500 N9 G02 X0 Z0 I-20 K0 F0.2 S1500 N10 G00 X0 Z2

30. Example 03-Drilling & Boring Operation
N7 G00 X0 Z1 M08 N8 G00 X0 Z10 reference position of drill N9 G81 X0 Z-30 F0.1 S600 N10 G00 X0 Z1 N11 G00 X12 Z1 N12 G85 P10 Q10 U0 W0 F0.15 N13 G01 X12 Z-30 F0.15 S600 N14 G00 X0 Z-30 N15 G00 X0 Z1

31. Example 04-Threading Operation
N7 G00 X26 Z1 M08 N8 G78 X Z-30 I0 K F0.2 D1 A60 N9 G00 X26 Z1 N10 G28 U0 W0

32. Example 03- P.U.2008
N7 G00 X60 Z1 M08 N8 G74 X40 Z-40 F0.25 D1 N9 G02 X60 Z-50 I10 K0 F0.35 N10 G00 X62 Z1 N11 G00 X20 Z0 N12 G01 X40 Z-20 F0.35 S400 N13 G00 X42 Z1

33. Example 03- P.U.2010
N7 G00 X92 Z1 M08 N8 G74 X80 Z-120 F0.25 D1 N9 G00 X82 Z1 N10 G74 X60 Z-70 F0.25 D1 N11 G00 X62 Z1 N12 G00 X40 Z0 N13 G01 X60 Z-20 F0.25 S1500 N14 G00 X62 Z-20 N15 G00 X60 Z-70 N16 G03 X80 Z-80 I0 K-10 F0.25 N17 G00 X82 Z-80

34. Part Programming
Milling Applications

35. Milling Tools & Operations

38. Milling Machine Based on axis orientation : Horizontal Milling Machine
Vertical Milling Machine

39. Z axis : align with the spindle
X axis : perpendicular to the spindle

40. Cutting Process Parameter Selection
Cutting Speed (V) :
V=DN/1000
Feed(fm) :
The rate with which workpiece advances under the cutter

41. Cutting Process Parameter Selection
Three Methods :
Feed per tooth (fz) :
The distance workpiece advances in the time between engagement by two successive teeth (mm/tooth)
Feed per cutter revolution (frev) :
The distance workpiece advances in the time when the cutter turns through one complete revolution (mm/rev)

42. Cutting Process Parameter Selection
(iii) Feed per minute (fm) :
The distance workpiece advances in one minute (mm/min.)
All the above methods are related by the equation :
fm= N x frev = fz x Z x N
where, Z=No of teeth on the cutter

43. Cutting Process Parameter Selection
Depth of Cut (t) :
The thickness of material removed in one pass of the workpiece under the cutter
It is the perpendicular distance measured between original and final surface of workpiece

44. Common Preparatory Functions
Principal Plane Selection
(i) XY plane selection (G17)
(ii) XZ plane selection (G18)
(iii) YZ plane selection (G19)
2. Interpolations
Linear Interpolations (G01)
Circular Interpolations (G02 & G03)
(iii) Helical Interpolations (G32 & G33)

45. Tool Compensations Tool Length Compensations (G43) :
Tool Pre setter- tool measuring device
mechanical ,electrical, optical
Tool Length offset ‘H’
Tool register

46. Cutter Radius Compensations
For Contouring Operations
Need to calculate tool cutter path by offsetting the contour by an amount equal to the radius of the cutter
Compensation OFF (G40)
Cutter radius compensation left (G41)
Cutter radius compensation right (G42)

47. Cutter Compensation (G41)

48. Cutter Compensation (G41/G42)

49. General Structure of Milling Part Program
N0 G Principle XY Plane selection
N1 G Metric mode
N2 G CANCEL cutter radius compensation
N3 G CANCEL canned cycle
N4 G28 U0 W Incremental input ,Tool axis pullout
N5 G91 Z Position to tool reference point
N6 X0 Y0
N7 G Reset origin point
N8 M06 T01
N9 G rapid travel to part zero
N10 G90 X0 Y absolute programming
N11 G43 Z0 M08 H tool length compensation
N12 G00 X_ Y_ M03 S spindle ON
N13 G01 Z_ F move tool downwards

50. General Structure of Milling Part Program
. N21 G28 U0 V0 W0 TOOL AXIS PULLOUT N22 G91 Z0 N23 G28 RETURN TOOL TO HOME & SPINDLE OFF N24 G91 X0 Y0 M05 N25 G40 CANCEL CUTTER RADIUS COMPENSATION N26 G80 CANCEL CANNED CYCLE N27 G49 CANCEL TOOL LENGTH COMPENSATION N28 M09 COOLANT OFF N29 M02 N30 M30

51. Example: P.U. May 2007
N11 G43 Z0 M08 H01 TOOL LENGTH COMPENSATION N12 G00 X22 Y22 M03 S500 N13 G01 Z-2 F0.1 N14 G42 X25 D06 CUTTER RADIUS COMPENSATION-RIGHT N15 G01 X90 N16 Y40 N17 X75 N18 G02 X75 Y55 I00 J7.5 N19 G01 X90 N20 Y80 N21 G03 X75 Y95 I-15 J00 N22 G01 X55 N23 X25 Y75 N24 Y25 N25 G00 Z00

52. Example: P.U. May 2009
N11 G43 Z0 M08 H01 N12 G00 X30 Y30 M03 S500 N13 G01 Z-14 F0.1 N14 G00 Z02 M05 N15 G00 X90 Y30 M03 S500 N16 G01 Z-14 F0.1 N17 G00 Z02 M05 N18 G00 X90 Y70 M03 S500 N19 G01 Z-14 F0.1 N20 G00 Z02 M05 N21 G00 X30 Y70 M03 S500 N22 G01 Z-14 F0.1 N23 G00 Z02 M05 N24 G00 X0 Y0 M06 T02 N25 G43 Z2 M08 H01 N26 G00 X60 Y50 M03 S500 N27 G01 Z-14 F0.1 N28 G00 Z02 M05 N28 G00 Z00