1. CNC TURNING Programming
L3 EAL Diploma in Engineering Technology
CNC TURNING Programming
Kevin Stewart

2. Aims and objectives Aims:
Understand how to produce coded part programs of structure and format appropriate to CNC equipment in use.
Objectives:
Carry out suitable and sufficient data preparation to enable CNC component manufacture

3. INTRODUCTION What is meant by a part program????????
A series of numerical instructions used by a CNC machine to perform the necessary sequence of operations to machine a specific work- piece.
It is just the program for the part you are going to machine!!!!!!!!!!!!
INCONEL

4. Introduction
CNC, or Computer Numerical Control, uses electronics to control the motions
of machinery.
This allows accurate and repeatable forming processes,
controlled by
stored programs.
The controller may be a dedicated device or a computer.

5. Position Control
Actual value
Target
value
Command
Actual value
Tool
table
Feed spindle
Feed motor
Measuring system
CNC
Target value
Command
Measuring system
Feed motor
To work effectively, the CNC machine needs to be set up accurately.
The system uses sensors to detect changes of position, which are fed back to the controller.
The controller sends a signal to the appropriate motors to move the work piece or tool to achieve the correct cut.
Next >

6. INTRODUCTION
The main difference is that instead of cranking handles to position a slide to a certain point, the dimension is stored in the memory of the machine control.
The control will then move (interpolates) the machine to these positions each time the program is run.
The operation of the T1-Series Turning Centre requires that a part program be designed, written, and entered into the memory of the control.
There are several options for getting these programs to the control.

7. TYPES OF INTERPOLATION
Linear interpolation (G01)
Circular interpolation (G02 / G03 )

8. Lathe Coordinate System
Most lathes are based on a Z-X Coordinate System.
The Z-axis is parallel to the machine spindle and the X-axis is perpendicular to the spindle.
Normal spindle rotation is ?
Clockwise, though direction can be reversed for left-handed threads.

9. Spindle rotation
Spindle direction on lathes is often referred to as M03, clockwise (CW) and M04 counter clockwise (CCW).
This depends on the location from which you are viewing the spindle. Standing at the wrong end of the machine could allow you to inaccurately label the direction.
A simpler, more accurate method is to think in terms of forward and reverse.
When standing in front of the machine, this refers to whether the part is turning toward you or away from you.
M03 can be called forward rotation and M04 can be called reverse rotation.
Viewed from the tailstock
Viewed from the headstock

10. Lathe Coordinate System
Notice how the turret is set at an incline from horizontal. This so-called "slant bed" configuration keeps cutting chips from accumulating on flat surfaces inside the machine.
This is a more common layout for CNC machines in industry and is different to the machine in the college workshop.

11. Lathe Coordinate System
The X+ & X- will swap over depending on what side the tool post is. A basic rule will be that you are always cutting on the X+.

12. Cutting tool behind the rotating work piece
Turning Machine Coordinates
In conventional turning machines, such as lathes, the cutting tool is in front of the rotating work piece.
Headstock
Work piece +X +Z
In CNC turning machines, the cutting tool is often behind the rotating work piece.
Cutting tool
Cutting tool in front of rotating work piece
Turning uses two axes of tool movement: +X +Z
X (across the work piece diameter)
Cutting tool behind the rotating work piece
Z (lengthwise towards or away from the headstock)
Next >

13. Lathe Coordinate System
All CNC machines move tools to specific locations described by coordinate systems. With lathes the coordinate system can be simply described as two number lines that intersect.
The vertical number line is called the X-axis.
The horizontal number line is called the Z-axis.

14. Lathe in the college workshop
X -
Part X0, Z0 (Floating zero)
Machine zero
X +

15. Machine Zero & floating zero
As shown on the previous picture the centre line of the part becomes (X) zero.
Normally the front face of the part is designated as: “Z” zero.
The centre line of the lathe is always the “X” zero.
 The reason being it is easy to access and easier to program.
The “Z” zero location will float with the face of different parts.

16. Machine Zero & floating zero
It would not be easy or convenient to write a program using the machine zero coordinates. Instead programs are written with values that would correspond to dimensions found on drawings. To do this a secondary floating zero point is established using offsets. This floating zero is referred to as the PART ZERO or PART ORIGIN.

17. Machine offsets
When we setup a machine, we need to tell the machine the distance different tools are at home position from the part origin.
Each tool is manually touched off the face and diameter and these distance differences from machine zero to the part zero are saved in X and Z register of the Tool Offsets Page.

18. Four different quadrants

19. Four different quadrants
The diagram above shows the operator’s view of X and Z grid standing in front of the lathe (rear turret configuration). At the intersection of the X and Z axis is the Part Zero or Reference Point.
Note: there are four different quadrants with different positive and values for X and Z.
Note: that most of the X values in a part program are going to be positive.
Normally the only negative X value is going to be when you face the part off past centre line. As the Z zero is normally the face of the part when you are cutting into the part the Z values will be negative.

20. Face off & part off
X +
X -

21. Diameter and not radius
Note: that the X values on the Haas lathe are in diameters.
Therefore an X move from centre line or X0. to X40. Will only be moving the machine along the X axis 20mm in the positive direction.

22. Absolute and Incremental Positioning
By using WORK and TOOL OFFSETS a common point on the part is designated as “PART ZERO”.
This is some point on our part that we can physically find. The programmer uses this point as a base to write the intended movement of the tooling.
There are two methods used by the programmer to program the movements on our machine.

23. Absolute and Incremental Positioning

24. Absolute and Incremental Positioning
The programmer has another tool available to him called “INCREMENTAL POSITIONING”.
This is movement based on where the machine is currently sitting. It is also called point to point programming.
If a change of 10mm smaller diameter is required of the machine from where it is currently sitting U-10.0 is put in the code.
If a grooving tool is making a groove that is located 5mm behind a groove that is already finished, W-5.0 is input.

25. Absolute and Incremental Positioning
The letters X & Z represent ABSOLUTE POSTIONING
The letters U & W represent INCREMENTAL POSTIONING

26. Absolute and Incremental Positioning
The first XY positional axis move should be programed using absolute coordinates.
To ensure correct positional alignment for any subsequent incremental moves;
to avoid incorrect incremental positioning from previous program

27. Carry out activity in the workbook

28. Programming https://www.youtube.com/watch?v=SOzmDFaC0JY

29. A program is written as a set of instructions given in the order they are to be performed. The instructions, if given in English, might look like this:
LINE 1 = SELECT CUTTING TOOL.
LINE 2 = TURN THE SPINDLE ON AND SELECT THE RPM.
LINE 3 = TURN THE COOLANT ON.
LINE 4 = RAPID TO THE STARTING POSITION OF THE PART.
LINE 5 = CHOOSE THE PROPER FEED RATE AND MAKE THE CUT(S)
LINE 6 = TURN OFF THE SPINDLE AND THE COOLANT.
LINE 7 = RETURN TOOL TO HOLDING POSITION AND SELECT NEXT TOOL and so on.
**But our machine control understands only these messages when given in machine code**

30. Program Format (layout)
There are NO positional requirements for a line of CNC code.
That means the different codes in a program may be in any order on a line of code.
It will also make it easier for the machinist to understand when he runs the part, if the program has a standard level of organization.
However, some standard rules are followed so the code is easier to view.

31. Programming Instructions
Some common codes include the following:
Examples
G- code instructions provided to a machine controller that tells the motors where to move, how fast to move, and what path to follow.
G01
Linear feed
F – Feed rate (speed of tool movement per spindle revolution)
Tool moves at 2 mm per spindle revolution
F2.0
M – Control code
Rotate spindle in clockwise direction
M03
S – Spindle speed
S2000
Rotate spindle at 2,000 rpm
T – Tool number
Select tool number 1 and offset 1
T101

32. Program Format (layout) G & M Codes
G and M codes may be placed anywhere on a line, but convention is that the G codes come first and the M codes come at the end of the block.
This makes sense as the last thing to happen on a line is the M function.
The G codes are completed first then the M code is performed on any given line.
G0G99G97X60.Z2.1S2000T101M03;
G0X55.M8,

33. Common Format of a Block
Sequence #
Preparatory Function
Dimension Words
Feed Rate
Spindle Function
Tool Function
Misc. Function
N50
G01 G99
X60.Z 5.
F0.1
S1500
T01
M03
Individual Words

34. Program Format
On Haas machines only one M code is allowed on a block of code.
Command codes are first given by a letter then a number. Some codes like X,Z and F require decimal points. X10.1 / Z100.5 / F0.1
The decimal point should always be programed on axis movements (X,Y,Z – U,V,W)
To prevent the machine miss-reading the amount.
And crashing into the work piece!!
(X1 Is it 1mm or 1 micron?)
Others like S and G require a number with no fractional part. S3000 / G01 / G99

35. Definitions With in the Format
Leading Zero’s: There is no need to program zeros proceeding a number.
Example: G00 (G0) and M01 (M1).
Trailing zeros however must be programmed.
Example: M30 not M3, G70 not G7.

36. Definitions With in the Format
Character: A single alphanumeric character value or the “+” and “-“ sign.
Word: A series of characters defining a single command such as “X” movement or “F” Feed rate. X10. F2.0
Unique letters are assigned as the first character of a word, and each letter has either a plus (+) or minus (-) sign value of numbers. (no need to program a plus)
X10. Z-10

37. Definitions With in the Format
Block: Series of words defining a single instruction.
An instruction may consist of a single linear or circular motion,
Plus additional information such as a feed rate or stop command.
A block of code is on one single line.
G00G96T101.X100.Z-5.S120M03

38. Notes on Program Structure;
Notes on Program Structure
A CNC program consists of a one or more blocks of commands.
A block of code may be considered a line of text. At the end of the block is a semicolon (;)
This denotes the end of the text or block and is also called a (EOB) end of block symbol.
When at the machine and manually entering a program pressing the EOB key will enter the semicolon symbol and move down to the next line in the program. ; ;

39. Modal & Non modal commands
Modal Commands: Once a particular word, such as G, X, Z, F, S, T, and M is programmed, it is not necessary to repeat the word in the following blocks until a different word or change of value is required in subsequent blocks of information.
M8 coolant on is an example of a modal command.
Non-Modal Commands: A non-modal command is one that is active only in the program block in which it is issued.
G04 program DWELL is an example of a non-modal command.

40. Machine Defaults
The control automatically recognizes these G codes when your HAAS lathe is powered up:
G00 Rapid Traverse
G18 X, Z Circular Plane Selection
G40 Cutter Compensation Cancel
G54 Work Coordinate Zero (1 of 26 available)
G80 Canned Cycle Cancel
G97 Constant Surface Speed Cancel
G99 Feed Per Revolution

41. Machine Defaults
There is no default FEEDRATE (F code), but once an F code is programmed, it will apply until another feed rate is entered or the machine is turned off.
G1X15.F0.5
X9.9F0.05
G0X15.
W1.15
G1X13.85
W-0.2
G3X13.05W-0.4R0.4
G1X10.6
G2X9.8W-0.4R0.4
G1Z-16.15
W-1.15
W0.2
G2X13.05W0.4R0.4
G3X9.8W0.4R0.4
X12. F0.1

42. Lathe Programming G18 G21 G40 G54 G80 G97 G99 Safety line, First line
This is done to make sure the machine is in a safe start condition.
Some programmers however don’t employ a safety line in lathes.

43. Lathe Programming
G18: G18 is the default command for designating which plane (X,Z plane) a radius is thrown. If an arc is attempted in a G17(XY plane) or a G19 (YZ plane) the Haas lathe will alarm out.
G20: G20(inch) and G21(mm) make sure setting #9 is set to inch or metric. Normally most shops are either inch or metric.
If the wrong setting is active it will be clearly seen in graphics or the machine will give an over travel alarm.

44. Lathe Programming
G40: Cancels cutter compensation codes G41 or G42. Cutter compensation should be cancelled after it is used.
G54: Work offsets SHIFT
Always active. Check G54 is empty!!!!!!

45. Lathe Programming G80: Cancels canned cycles.
G97: Spindle on. A G97 should be programmed at the beginning and end of every tool in a program with a spindle speed.
G99: Feed per revolution: This is the default. Normally lathes are always in G99 mode, they are never changed to G98 (Feed per minute).

46. Start of a program % O7687 (your name) (EAL Practice Turn)
Transmission Character
Program Number
Program Name  
Job title in brackets
Other useful info in brackets %
O7687
(your name)
(EAL Practice Turn)
Bar size, date, hang out, G54, tools used

47. What do these lines of programming mean??
The first seven lines
An example of the first seven lines of a program might look like this:
G18 G21 G40 G54 G80 G97 G99;
T101;
G50 S2000;
G97 S2000 M03;
G54 G00 X40. Z1. M08;
G96 S250;
What do these lines of programming mean??

48. The first seven lines (for each tool call)
1. Safety line
G18 G21 G40 G54 G80 G97 G99
2. The second line of code indexes the turret to the appropriate tool giving proper geometry or tool shifts.
T101- Tool 1 offset 1 
3. The third line may contain a spindle speed maximum, G50, for the lathe during any operation. 
G50 S4000- Spindle will not go above the set speed 
4. The fourth line or block should cancel any constant surface speed mode (G97) and specify a spindle speed command (S____) along with a spindle direction CCW (M03).  
G97S2000M3- Spindle will run at 2000RPM CCW

49. The first seven lines
6. The fifth line should contain a preparatory code (G00) for a rapid movement to a start X and Z position and to turn on the coolant (M08). 
G00X40.Z1.M08 
7. The sixth line may optionally specify a Constant Surface Speed (G96) and a surface meters per minute (SMM) defined with an (S____) command. 
G96 S120- machine will run at 120 MPM up to spindle clamp setting

50. End of tool and end of Program
End of tool:
G00 X35.
Z5.
X200. Z200. M5 M9
M00
End program:
G00 X35.
Z5.
G00 X200. Z200. M5 M9
G28 X0.
Z0.
M30 %

51. Notes on Program Structure%
Notes on Program Structure
Programs must begin and end with the transmission characters (percentage symbol %).
To open/close transmission of CNC program between off-line devices and CNC controller
These symbols will not be seen on the controls of the Haas.
If however you save the program to say a USB device and look at the program using a computer they will be there.
If you are trying to load a program into the CNC without percentage symbols at the beginning and end of a program the CNC machine will alarm out and not accept the program. %

52. Notes on Program Structure
After the first % sign the next line of the program requires a program name using the letter O and a four digit number on older machines or 5 digit number on newer machines.
This symbol identifies a particular program and is used to call up the correct program. %
O3008(SPINDLE ROLLER HD1)
(TREND MARINE PRODUCTS)
(DRWG NO, 06STD-R REV B)
(MAT. 8MM PG ST/ST 316)
(12/04/12)
O3008

53. Notes on Program Structure
Text inside the ( ) is not seen or used by the machine.
It is information for the operator.
This text will show up in list program screen of the memory.

54. Common G codes G00 Rapid Position Motion
G01 Linear Interpolation Motion
G02 CW Circulation Interpolation Motion - Modal
G03 CCW Circular Interpolation Motion - Modal
G04 Dwell (P) P=Seconds.
G18 Circular Motion ZX Plane Selection (G02, G03)
G21 Verify Metric Coordinate Positioning - Modal
G28 Rapid to machine zero return through Ref. Point
G40 Tool Nose Compensation Cancel G41/G42
G41 Tool Nose Compensation, Left - Modal
G42 Tool Nose Compensation, Right - Modal
G50 Spindle Speed Maximum RPM Limit (S) - Modal
G70 Finishing Cycle
G71 O.D. / I.D. Stock Removal Cycle Example
G76 Threading Cycle, Multiple Pass O.D. / I.D.
G96 Constant Surface speed, CSS On - Modal
G97 Constant Non-Varying Spindle Speed, CSS Off (S)
G98 Feed Per Minute (F) - Modal
G99 Feed Per Revolution

55. Common M codes M00 Program Stop - Modal M01
Optional Program Stop - Modal
M03
Spindle on Forward (S) - Modal
M04
Spindle on Reverse (S) - Modal
M05
Spindle Stop - Modal
M08
Coolant On - Modal
M09
Coolant Off - Modal
M23
Angle Out of Thread On - Modal
M24
Angle of Thread Off - Modal
M30
Program End and Reset - Modal

56. HAAS PROGRAM START % O00559 (VICE DRAW BAR) (25MM BMS)
(HANG OUT 100MM)
(G54= 50)
(T101= CCMT ROUGH TURN 0.8 RAD)
(T202= DCMT FINISH TURN 0.4 RAD)
(T404= THREADING INSERT 1.75P)
(T303= 2MM WIDE GROOVING TOOL)
G18 G21 G40 G80 G97 G99 (SAFETY LINE)
T101 (NEEDS A TOOL CALL TO START)
G00 X200. Z200. (TOOL CHANGE POS)
M00 (PROGRAM STOP, PUT TOOL IN)
G50 S1500 (SPINDLE CLAMP, MAX RPM)
G97 S500 M03 (SPINDLE ON IN CCW) N1
T101
G96 S100 M03 (CONSTANT SURFACE SPEED)
G54 G00 X50. Z10. (RAPID POSITION)
X27. Z0.
M08 (COOLANT ON)
G01 X-1. F0.1 (FACE OFF)

57. HAAS PROGRAM END
X50. F0.2
G00 X200. Z200.
M05
M09
G28
M30 %

58. Programme example N1 T101 G96 S100 M03 (CONSTANT SURFACE SPEED)
G54 G00 X50. Z10. (RAPID POSITION)
X42. Z0.
M08 (COOLANT ON)
G01 X-1. F0.1 (FACE OFF)
X7.F0.2
X10.Z-1.5
Z-20.
X16.
X20.Z-22.
Z-40.
X40.
Z-70.
G0X60.
M05
M09
G00 X200. Z200.
M00
Programme example

59. Programming position for chamfering (45°)
When programming a 45 degree chamfer it is important to remember that the tool needs to move double the amount in X as it has in Z.
As shown in the diagram a 5 x 45° chamfer ending at Ø30, Ø20.
Both axis move together (programme X & Z same line)

60. Programming position for radii
When programming a radii it is important to remember that the tool needs to move double the amount in X as it has in Z.
As shown in the diagram a radii of 6 ending at Ø30, Ø18.
Both axis move together (programme X & Z same line)

61. Complete the activity using the information you have been given. (006)

62. G02 CW & G03 CCW
Circular Interpolation

63. G02 CW & G03 CCW Circular Interpolation Motion
G03 will generate a counter clockwise circular motion, but is otherwise defined the same as a G02 clockwise circular motion.
Circular interpolation commands are used to move a tool along a circular arc to the commanded end position.

65. To move the cutter in a clockwise direction from the START POINT to the END POINT, the programming coding would be like this:
N12 G00 X0. Z1. (tool rapids to X0 Z1.mm in front of part)
N13 G01 Z0. F.012 (tool feeds to Z0. face of part)
N14 X10. (tool feeds up in X-axis to a 10mm dia, start point of rad)
N15 G03 X30.Z-10. R10. (tool at 10mm dia. machines rad)
N16 G01 Z-30.(second rad start point)
N17 G02 X50. Z-40. R10 (cuts 10mm rad)
N18 G01 X70. (tool feeds up in X-axis
to a 70mm dia.)

66. Complete the activity using the information you have been given. (007)

67. Threading G76

68. Threading G76
Haas G76 threading cycle can be used for, external threads, internal threads, straight threads, taper threads.
With Haas G76 threading cycle, a programmer can easily command multiple cutting passes along the length of the thread.
The nature of tool load and wear can be controlled by using the P code. The P code can specify which side the tool cuts on and it can specify how much material will be cut.

69. G76 - M5 THREAD G00 X8. Z5.(START POINT)
G76 THREADING
G00 X8. Z5.(START POINT)
G76 X4.018 Z-15. K0.490 D0.1 A60 F0.8
G00X20. (END POINT)
Z10.
D- First pass cutting depth
K- Thread height, defines limit of multiple passes, radius measure
X- X-axis absolute location, maximum thread I.D.
Z- Z-axis absolute location, maximum thread length
U- X-axis incremental distance, start to maximum thread I.D.
W- Z-axis incremental distance, start to maximum thread length
I- Thread taper amount, radius measure
P- Subsequent pass positioning algorithm, cutting method
F- Feedrate (specifies feedrate for threading – also indicates the pitch or lead)
A- Tool nose angle (0 to 120 degree) Defaults to 0. Do not use decimal point.

70. G76 M5 THREAD INFO G00 X8. Z5.(START POINT)
G76 X4.018 Z-15. K0.490 D0.1 A60 F0.8
G00X20. (END POINT)
Z10.
Zeus book ISO thread chart

71. Carry out the activity Page 36

72. Cutter Compensation
G41 / G42

73. Tool Nose Radius Compensation on Turning Centres
Facing and Straight Turning
When facing or straight turning, the tool nose radius has no effect on the part other than leaving a radius on inside corners.

74. Tool Nose Radius Compensation on Turning Centres
This tangent point finishes faces.
This tangent point finishes diameters.
Theoretical sharp point is what we program.

75. The Problem
When turning tapers or radii, the tool nose radius leaves excess material as shown here:
Excess Material Here

76. The Solution
1. Manually program the exact tangent points. This is time consuming since it requires trig calculations or accurate CAD drawings to locate the tangent points.
2. Use tool nose radius compensation. The tool nose radius is entered into the machine controller, and the program turns on compensation, and then turns it off. The machine calculates the tangent points so we can continue programming as if the cutter has a sharp point.

77. Tool nose compensation on the TL1 (College lathe)
TIP 2
TIP 3

78. Approach And Departure Moves
The first X or Z motion in the same line that contains a G41 or G42 is called the APPROACH move.
The first move must be a linear move, a G01 or G00. At the start of an approach move, the current position is not compensated. At the end of the approach move, the machine position will be fully compensated. This is shown in the following figure.
G40
G42
END
START

79. Turning Nose Radius Compensation On( approach):
The machine must move at least the distance of the nose radius in X and Z.
For easy calculations, back away from the start point around 5mm in Z and 4mm in X. Remember X is diameter based, so 4mm in X is actually 2mm radially.
G40

80. Approach And Departure Moves
Any line containing a G40 will cancel tool nose compensation. This is called the DEPARTURE move.
The last move must be a linear move, a G01 or G00. At the start of a departure move, the current position is fully compensated. At the end of the departure move, the machine position is not compensated.

81. Example, cutter comp G00 G42 X8. Z2. (CUTTER COMP ON)
T101 (ROUGH TURN)
G96 S120 M03 (CONSTANT SURFACE SPEED)
G00 X40. Z10. (RAPID POSITION)
G01 X34. Z0.2 F0.5 (FFED POSITION)
M08 (COOLANT ON)
G01 X-1. F0.1 (FACE OFF WITH ALLOWENCE)
G00 X32. Z5.
G00 G42 X8. Z2. (CUTTER COMP ON)
G01 Z0. F0.05
X12. Z-2. F0.11
Z-15.9
X14.93
Z-26.
X18.
G03 X22. Z-28. R2.
G01 Z-36.
G00 X50.
G00 G40 X60. Z10. (CUTTER COMP CANCEL)
Example, cutter comp

82. Turning Nose Radius Compensation Off
To turn compensation off, we feed the cutter completely off the work and then make a move larger than the nose radius while calling G40.
Note: Do not reverse the Z direction with nose radius compensation on !
The machine may get confused, and then later cuts may be off by some multiple of the nose radius. Always call G40 BEFORE reversing the Z direction!
2. C C off in this move
1. move tool away

83. Imaginary tool tip and direction
Tool nose compensation calculates a compensated tool path for a tool that has a radius at the tool tip. This tool tip is known as the TOOL NOSE RADIUS (TNR).
The control can calculate where the centre of the tool radius is by using the tool:
Geometry X Z offsets
Tool radius offsets,
Which side of the line the cutter is on
left (G41) or right (G42), and
The direction tool tip is pointing (1-9).
See figure on the next page.

84. Imaginary tool tip and direction

86. The tool tip direction
The tool tip direction of each tool is coded as a single number from 0 to 9.
The tip direction code is found next to the radius offset on the geometry offsets page. 3

87. USING TOOL NOSE COMPENSATION
Tool nose compensation works by programming the TOOL PATH profile and defining what side of the line the cutter is on, right or left. (G41/G42) The programmer will usually program the tool path, to the parts finished size. When tool nose compensation is used, the control will compensate for a tool's radius based on special instructions written into the program.

88. Carry out the activity Page 45

89. Machining Cycles for the Lathe
Caned cycles
G76
G70

90. Caned cycles
Canned cycle – a series of permanently held machine instructions called into use by an appropriate code.
A machining cycle is used to simplify the programming of a part. Machine cycles are defined for the most common machining operations.
They can be divided into two types. There are machine cycles for turning and grooving. There are cycles for drilling and tapping.
G71

91. **THE 3 WE WILL LOOK AT ARE G70, G71 & G76**
Caned cycles
G70 Finishing Cycles
G71 O.D./I.D. Stock Removal Cycle
G72 End Face Stock Removal Cycle
G74 End Face Grooving or Turning with Chip Break Cycle
G75 O.D./I.D. Grooving or Turning with Chip Break Cycle
G76 Thread Cutting Cycle, Multiple Pass
G92 Thread Cutting Cycle Modal
**THE 3 WE WILL LOOK AT ARE G70, G71 & G76**

92. G71 / G70
Roughing and finishing cycle

93. G71 O.D./ I.D. STOCK REMOVAL CYCLE
P- Starting Block number of path to rough
Q- Ending Block number of path to rough
U- X-axis value and direction of G71 rough stock allowance, diameter
W- Z-axis value and direction of G71 rough stock allowance
D- Depth of cut for each pass of stock removal, positive radius
I-X-axis stock value and direction for a G71 finish pass, radius
K- Z-axis stock value and direction for a G71 finish pass
S- Spindle speed to use throughout G71 PQ bock
T- Tool and offset to use throughout G71 PQ block
F- Feed rate to use throughout G71 PQ block

94. G71 / G70 N11 T101 (ROUGH TURN) G96 S120 M03 G00 X40. Z10.
G01 X34. Z0.2 F0.5
G01 X-1. F0.1 (FACE OFF)
G00 X32. Z2.
G71 P1 Q2 D1. W0.1 U0.5 F0.15 (ROUGH TURNING CYCLE)
N1 G00 G42 X0.
G01 Z0. F0.05
X12. Z-2. F0.15
Z-16.
X14.93
Z-26.
X18.
G03 X22. Z-28. R2.
G01 Z-36.
X24.57 Z-52.93
X35. F0.2 N2
G00 G40 X55. Z10.
X200. Z200. M5 M9
M00
N12
G50 S1500
G97 S500 M03
T202(FINISH TURN)
G00 X32. Z10. M08
Z0.
G1X-1.F0.1
G01 Z2. F0.5
G70 P1 Q2 (READ BETWEEN N1 N2)

95. G71 O.D./ I.D. STOCK REMOVAL CYCLE
G71 / G70
haas

96. G71 O.D./ I.D. STOCK REMOVAL CYCLE
Control manufacturers use G71 to rough leaving a specified amount of excess material and G70 to finish.
These two cycles greatly simplify programming complex parts.

97. How the G71 Works

98. How the G70 Works

99. Carry out the activity
Page 48
Practice Job

100. Program Format G18 G21 G40 G54 G80 G97 G99 Safety line T101;
G97 S2000 M03;
G00 X45. Z5. M08;
G96 S450 M3;
Safety line
Tool & offset call
Clamp speed
CCW
Rapid to position, coolant on
Constant surface speed