Wuhan Huazhong Numerical Control Co., Ltd HNC-18xp/T, HNC-19iT v4.0, HNC-21T, HNC-22T, HNC-18iT Programming Manual

Century

Century Star

Star

Star Turning

Turning

Turning CNC

CNC

CNC System

System

Programming

Programming Guide

Guide

V

V 3.3

November,

November, 2007

Wuhan

Wuhan Huazhong

Huazhong

Huazhong Numerical

Numerical

Numerical Control

3.3

3.3 2007

2007

Control

Control Co.,

Co.,

Co., Ltd

Ltd

Preface

Organization

Organization of

1. General

2. Preparatory Function

3. Interpolation Function

4. Feed Function

5. Coordinate System

6. Spindle Speed Function

7. Tool Function

8. Miscellaneous Function

9. Functions to Simplify Programming

10. Comprehensive Programming Example

11. Custom Macro

Applicability

This Programming Guide is applicable to the following CNC system:

HNC-18iT/19iT v4.0

of

documentation

of

documentation

of documentation

documentation

HNC-18xp/T

HNC-19xp/T

HNC-21TD/22TD v05.62.07.10

Internet

Internet Address

http://www.huazhongcnc.com/

Address

i

Table of Contents

Table

Table of

Preface ............................................................................................................................................. i

1 General ................................................................................................................................... 1

2 Preparatory Function (G code) ............................................................................................. 21

3 Interpolation Functions ......................................................................................................... 24

4 Feed Function ....................................................................................................................... 49

5 Coordinate System ................................................................................................................ 53

of

Contents

of

Contents

of Contents

Contents

1.1 CNC Programming ..................................................................................................... 2

1.2 Interpolation ................................................................................................................ 4

1.2.1 Linear Interpolation ........................................................................................ 4

1.2.2 Circular Interpolation ...................................................................................... 5

1.2.3 Thread Cutting ................................................................................................ 5

1.3 Feed Function ............................................................................................................. 6

1.4 Coordinate System ...................................................................................................... 7

1.4.1 Reference Point ............................................................................................... 7

1.4.2 Machine Coordinate System ........................................................................... 8

1.4.3 Workpiece Coordinate System ........................................................................ 9

1.4.4 Setting Two Coordinate Systems at the Same Position ................................ 10

1.4.5 Absolute Commands ..................................................................................... 11

1.4.6 Incremental Commands ................................................................................ 12

1.4.7 Diameter/Radius Programming .................................................................... 13

1.5 Spindle Speed Function ............................................................................................ 14

1.6 Tool Function ............................................................................................................ 15

1.6.1 Tool Selection ............................................................................................... 15

1.6.2 Tool Offset .................................................................................................... 15

1.7 Miscellaneous Function ............................................................................................ 18

1.8 Program Configuration ............................................................................................. 19

1.8.1 Structure of an NC Program ......................................................................... 19

1.8.2 Main Program and Subprogram .................................................................... 20

2.1 G code List ................................................................................................................ 22

3.1 Positioning (G00) ..................................................................................................... 25

3.2 Linear Interpolation (G01) ........................................................................................ 26

3.3 Circulation Interpolation (G02, G03) ....................................................................... 31

3.4 Chamfering and Rounding (G01, G02, G03) ............................................................ 37

3.4.1 Chamfering (G01) ......................................................................................... 37

3.4.2 Rounding (G01) ............................................................................................ 38

3.4.3 Chamfering (G02, G03) ................................................................................ 40

3.4.4 Rounding (G02, G03) ................................................................................... 41

3.5 Thread Cutting with Constant Lead (G32) ............................................................... 43

3.6 Tapping (G34) ........................................................................................................... 46

4.1 Rapid Traverse (G00) ............................................................................................... 50

4.2 Cutting Feed (G94, G95) .......................................................................................... 51

4.3 Dwell (G04) .............................................................................................................. 52

5.1 Reference Position Return (G28) .............................................................................. 54

5.2 Auto Return from Reference Position (G29) ............................................................ 55

5.3 Setting a Workpiece Coordinate System (G92) ........................................................ 57

5.4 Selecting a Machine Cooridinate System (G53) ....................................................... 58

5.5 Selecting a Workpiece Coordinate System (G54~G59) ............................................ 59

5.6 Origin of a Workpiece Coordinate System (G51, G50) ............................................ 61

5.7 Absolute and Incremental Programming (G90, G91) ............................................... 62

ii

Table of Contents

5.8 Diameter and Radius Programming (G36, G37) ...................................................... 64

5.9 Inch/Metric Conversion (G20, G21) ......................................................................... 66

6 Spindle Speed Function ........................................................................................................ 67

6.1 Limit of Spindle Speed (G46) ................................................................................... 68

6.2 Constant Surface Speed Control (G96, G97) ............................................................ 69

7 Tool Function ........................................................................................................................ 71

7.1 Tool Selection and Tool Offset (T code) ................................................................... 72

7.2 Tool Radius Compensation (G40, G41, G42) ........................................................... 74

8 Miscellaneous Function ........................................................................................................ 76

8.1 M code List ............................................................................................................... 77

8.2 CNC M-Function ...................................................................................................... 78

8.2.1 Program Stop (M00) ..................................................................................... 78

8.2.2 Optional Stop (M01) ..................................................................................... 78

8.2.3 End of Program (M02) .................................................................................. 78

8.2.4 End of Program with return to the beginning of program (M30) ................. 78

8.2.5 Subprogram Control (M98, M99) ................................................................. 79

8.3 PLC M Function ....................................................................................................... 81

8.3.1 Spindle Control (M03, M04, M05) ............................................................... 81

8.3.2 Coolant Control (M07, M08, M09) .............................................................. 81

9 Functions to Simplify Programming .................................................................................... 82

9.1 Canned Cycles .......................................................................................................... 83

9.1.1 Internal Diameter/Outer Diameter Cutting Cycle (G80) .............................. 83

9.1.2 End Face Turning Cycle (G81) ..................................................................... 88

9.1.3 Thread Cutting Cycle (G82) ......................................................................... 91

9.1.4 End Face Peck Drilling Cycle (G74) ............................................................ 94

9.1.5 Outer Diameter Grooving Cycle (G75) ........................................................ 96

9.2 Multiple Repetitive Cycle ......................................................................................... 98

9.2.1 Stock Removal in Turning (G71) .................................................................. 98

9.2.2 Stock Removal in Facing (G72) ................................................................. 104

9.2.3 Pattern Repeating (G73) ............................................................................. 108

9.2.4 Multiple Thread Cutting Cycle (G76) ......................................................... 111

10 Comprehensive Programming .................................................................................... 114

10.1 Example 1 ............................................................................................................... 114

10.2 Example 2 ............................................................................................................... 116

10.3 Example 3 ............................................................................................................... 118

10.4 Example 4 ............................................................................................................... 119

11 Custom Macro .................................................................................................................... 120

11.1 V ariables ................................................................................................................. 121

11.1.1 Type of Variables ........................................................................................ 121

11.1.2 System Variables ........................................................................................ 122

11.2 Constant .................................................................................................................. 129

11.3 Operators and Expression ....................................................................................... 130

11.4 Assignment ............................................................................................................. 131

11.5 Selection statement

IF,

ELSE,ENDIF ..................................................................... 132

11.6 Repetition Statement WHILE, ENDW ................................................................... 133

11.7 Macro Call .............................................................................................................. 134

11.8 Example .................................................................................................................. 136

iii

1. General

1

General

1

General

1

1 General

General

This chapter is to introduce the basic concepts in Computerized Numerical Control (CNC)

system: HNC-21T /22

T,

HNC-18iT/19iT, HNC-18xp/

T

, HNC-19xp/

T

.

1

1.1

CNC

1.1

CNC

1.1

1.1 CNC

CNC Programming

To

operate CNC machine tool, the first step is to understand the part drawing and produce a

program manual script. The procedure for machining a part is as follows (Figure 1.1):

1) Read drawing

2) Produce the program manual script

3) Input the program manual script by using the machine control panel

4) Manufacture a part

Programming

1. General

2

1. Read drawing

X

1. General

Φ60

Φ40

4 0

1 50

2. Produce the program manual script

N1 T0106 N2 M03 S460 N3 G00 X90Z20 N4 G00 X31Z3 N5 G01 Z-50 F100 N6 G00 X36 N7 Z3 …

3. Input the program manual script

Ζ

4. Manufacture a part

X

Z

Figure 1 . 1 The workflow of operation of CNC machine tool

3

1. General

X

Z

X

Z

1.2

Interpolation

1.2

Interpolation

1.2

1.2 Interpolation

Interpolation

Interpolation refers to an operation in which the machine tool moves along the workpiece

parts. There are five methods of interpolation: linear, circular, helical, parabolic, and cubic.

Most CNC machine can provide linear interpolation and circular interpolation. The other

three methods of interpolation (helical, parabolic, and cubic interpolation) are usually used

to manufacture the complex shapes, such as aerospace parts. In this manual, linear and

circular interpolation are introduced.

1.2.1

1.2.1 L

There are two kinds of linear interpolation:

L

inear

L

inear

L inear

inear Interpolation

1) Tool movement along a straight line (Figure 1.2).

2) Tool movement along the taper line

Interpolation

Figure 1 . 2 Linear Interpolation (1)

Figure 1 . 3 Linear Interpolation (2)

4

1. General

X

Z

1.2.2

1.2.2 Circular

Figure 1.4 shows a tool movement along an arc.

Note:

In this manual, it is assumed that tools are moved against workpieces.

Circular

Circular Interpolation

Interpolation

Figure 1 . 4 Circular Interpolation

1.2.3

1.2.3 Thread

There are several kinds of threads: c ylindrical, taper or face threads .

workpiece, the tool is moved with spindle rotation synchronously .

Thread

Thread Cutting

Cutting

Figure 1 . 5 Thread Cutting

To

cut threads on a

5

1. General

Tool

Chuck

1.3

Feed

1.3

Feed

1.3

1.3 Feed

Feed Function

- Feed refers to an operation in which the tool moves at a specified speed to cut a

workpiece.

- Feedrate refers to a specified speed, and numeric is used to specified the fe e drate .

- Feed function refers to an operation to control the fe e drate .

Function

Figure 1 . 6 Feed Function

For example:

F2.0 //feed the tool 2mm, while the workpiece makes one turn

6

1.4

Reference position

Tool post

Chuck

Coordinate

1.4

Coordinate

1.4

1.4 Coordinate

Coordinate System

System

1. General

1.4.1

1.4.1 Reference

Reference point is a fixed position on CNC machine tool, which is determined by cams and

measuring system. Generally, it is used when the tool is required to exchange or the

coordinate system is required to set.

There are two ways to move to the reference point:

Reference

Reference Point

Point

Figure 1 . 7 Reference Point

- Manual reference position return: The tool is moved to the reference point by operating

the button on the machine control panel. It is only used when the machine is turned on.

- Automatic reference position return: It is used after the manual reference position return

has been used. In this manual, this would be introduced.

7

1. General

+

X

+

X

+

Y

＇

+Z+

Y

+

Z

+Y+

C

+

Z

＇

+A +

B

+

C

+ X +Y +

Z

+

A

+

B

+

X

＇

1.4.2

1.4.2 Machine

Machine

Machine Coordinate

Coordinate

Coordinate System

System

The coordinate system is set on a CNC machine tool. Figure 1.8 is a machine coordinate

system of turning machine, and shows the direction of axes:

Figure 1 . 8 Machine Coordinate System

In general , three basic linear coordinate axes of motion are X,

Y,

Z. Moreover, X,

Y,

Z axis

of rotation is named as A, B, C cor respond ently. Due to different types of turning machine,

the axis direction can be decided by following the rule – “ three finger rule ” of the right

hand.

Figure 1 . 9 “ three finger rule ”

- The thumb points the X axis. X axis controls the cross motion of the cutting tool.

“ +X ” means that the tool is away from the spindle centerline

- T he index points the Y axis. Y axis is usually a virtual axis.

- T he middle finger points the Z axis. Z axis controls the motion of the cutting tool.

“ +Z ” means that the tool is away from the spindle.

8

1. General

1.4.3

1.4.3 Workpiece

The coordinate system is set on a workpiece. The data in the NC program is from the

workpiece coordinate system.

Example: Those four points can be defined on workpiece coordinate system:

Workpiece

Workpiece Coordinate

Coordinate

Coordinate System

Z-

X-

Figure 1 . 10 Workpiece Coordinate System

System

Y+

W

Y-

X+

90 °

Z+

P1 corresponds to X25 Z-7.5

P2 corresponds to X40 Z-15

P3 corresponds to X40 Z-25

P4 corresponds to X60 Z-35

P4

P3

25

35

Figure 1 .11Example of defining points on workpiece coordinate system

X

P2

P1

7.5

15

Φ 60

Φ 40

Φ 25

Z

9

1. General

4 0

Ζ

Φ60

Φ40

1 50 X

Ζ

X

3 0

Ζ

Φ60

Φ30

8 0 X

10 0

Ζ

X

1.4.4

1.4.4 Setting

There are two methods used to define two coordinate systems at the same position.

Setting

Setting Two

1) The coordinate zero point is set at chuck face

2) The coordinate zero point is set at the end face of workpiece

Two

Coordinate

Two

Coordinate

Two Coordinate

Coordinate Systems

Figure 1 . 12 The coordinate zero point set at chuck face

Systems

Systems at

at

the

at

the

at the

the Same

Same

Same Position

Position

Figure 1 . 13 The coordinate zero point set at the end face of workpiece

10

1. General

1.4.5

1.4.5 Absolute

The absolute dimension describes a point at “ the distance from zero point of the coordinate

system ” .

E xample: These four point in absolute dimensions are the following:

Absolute

Absolute Commands

P1 corresponds to X25 Z-7.5

P2 corresponds to X40 Z-15

P3 corresponds to X40 Z-25

P4 corresponds to X60 Z-35

Commands

P4

P3

25

35

X

P2

P1

7.5

15

Φ 60

Φ 40

Φ 25

Z

Figure 1 . 14 Absolute Dimension

11

1. General

1.4.6

1.4.6 Incremental

The incremental dimension describes a distance from the previous tool position to the next

tool position.

Example: These four point in incremental dimensions are the following:

Incremental

Incremental Commands

P1 corresponds to X25 Z-7.5 //with reference to the zero point

P2 corresponds to X15 Z-7.5 //with reference to P1

P3 corresponds to Z-10 //with reference to P2

P4 corresponds to X20 Z-10 //with reference to P3

Commands

P4

10

X

P2

P3

P1

7.5

10

Φ 60

Φ 40

Φ 25

Z

Figure 1 . 15 Incremental Dimension

12

1. General

8

8 0

0

6

6 0

0

B

A

Φ40

X

Z

Φ30

8

8 0

0

6

6 0

0

B

A

20

X

Z

15

1.4.7

1.4.7 Diameter/Radius

Diameter/Radius

Diameter/Radius Programming

Programming

The coordinate dimension on X axis can be set in diameter or radius. It should be noted that

diameter programming or radius programming should be applied independently on each

machine.

Example: Describe the points by diameter programming.

A

corresponds to X30 Z80

B corresponds to X40 Z60

Figure 1 . 16 Diameter Programming

Example: Describe the points by radius programming.

A

corresponds to X15 Z80

B corresponds to X20 Z60

Figure 1 . 17 Radius Programming

13

1. General

N

·

min

-

1

Chuck

V: Cutting speed v m/min

1.5

Spindle

1.5

Spindle

1.5

1.5 Spindle

Spindle Speed

The cutting speed (v) refers to the speed of the tool with respect to the workpiece when the

workpiece is cut. The unit of the cutting speed is m/min. As for the CNC, the cutting speed

can be specified by the spindle speed (N) in min-1.

Speed

Speed Function

Figure 1 . 18 Cutting Speed and Spindle Speed

Function

The formula to get the spindle speed is:

N: the spindle speed

v: cutting speed

D: diameter value of the workpiece

Example: When the diameter of workpiece is 200mm, and the cutting speed is 300m/min,

v

then the spindle speed:

N

=

∗

=

D

The constant surface speed refers to the cutting speed even when the workpiece diameter is

changed, and the CNC changes the spindle speed.

1000

N

=

D

π

30010001000

∗

≈

200

∗

ππ

mr

/478

v

∗

14

1.6

Tool

1.6

Tool

1.6

1.6 Tool

Tool Function

Function

1. General

1.6.1

1.6.1 Tool

It is necessary to select a suitable tool when drilling, tapping, boring or the like is performed.

As it is shown in Figure 1.19, a number is assigned to each tool. Then this number is used in

the program to specify that the corresponding tool is selected.

1.6.2

1.6.2 Tool

When writing a program, the operator just use the workpiece dimensions according to the

dimensions in the part drawing. The tool nose radius center , the tool direction of the turning

Tool

Selection

Tool

Selection

Tool Selection

Selection

Tool

Offset

Tool

Offset

Tool Offset

Offset

01

02

03

Figure 1 . 19

06

04

Tool

05

Selection

Tool

number

Tool

number

Tool

Tool number

number

Tool

post

Tool

post

Tool

Tool post

post

tool, and the tool length are not taken into account. However, when machining a workpiece,

the tool path is affected by the tool geometry.

workpiece

Standard tool

Rough cutting tool

Figure 1 . 20

Finishing tool

Tool

Offset

15

Grooving tool

Thread cutting tool

1. General

T

ool nose radius center

P

Imaginary tool

nose

� Tool Length Compensation

There are two kind of ways to specify the value of tool length compensation.

- Absolute value of tool length compensation (the distance between tool tip and

machine reference point)

- Incremental value of tool length compensation (the distance between tool tip and

the standard tool)

As it is shown in Figure 1.21, L1 is the tool length on X axis. L2 is the tool length on Z axis.

It should be noted that the tool wear values on X axis or Z axis are also contained in the tool

length compensation.

R

S

P

P=Tool

P=Tool tip R=Radius

R=Radius

R=Radius S=Cutting

S=Cutting

S=Cutting edge

tip

Figure 1 . 21

edge

center

edge

center

edge center

center

Tool

Length Compensation

L2

L1

� Tool Radius Compensation

Figure 1.22 shows the imaginary tool nose as a start position when writing a program.

Figure 1 . 22 The imaginary tool nose

16

1. General

7

●

X

0 9

Z

●

8

3

4

5

6

2

1

● Imaginary tool nose

+

+ T o ol nose radius center

7

●

X

0 9

Z

●

5

6

8

2

3

4

1

● Imaginary tool nose

+

+ Tool nose radius center

The direction of imaginary tool nose is determined by the tool direction during cutting.

Figure 1.23 and Figure 1.24 show the relation between the tool and the imaginary tool tip.

Figure 1 . 23 The direction of imaginary tool nose (1)

Figure 1 . 24 The direction of imaginary tool nose (2)

17

1. General

1.7

Miscellaneous

1.7

Miscellaneous

1.7

1.7 Miscellaneous

Miscellaneous Function

Miscellaneous function refers to the operation to control the spindle, feed, and coolant. In

general, it is specified by an M code.

When a move command and M code are specified in the same block, there are two ways to

execute these commands:

1) Pre-M function

M command is executed before the completion of move command

2) Post-M function

M command is executed after the completion of move command.

The sequence of the execution depends on the specification of the machine tool builder.

Function

18

1. General

%1000

N01 G91 G00 X50 Y60

N10 G01 X100 Y500 F150 S300 M03

N...... ;COMMENT

N200 M30

Program

Program block

Command character

Program number

N.. G .. X … Y … F.. M.. S..

Program block

Miscellaneous function

Spindle function

Feed Function

Coordinate - Dimension word

Preparatory function

Program block number

Program

1.8

Program

1.8

Program

Program Configuration

1.8

1.8.1

1.8.1 Structure

As it is shown in Figure 1.25, an NC program consists of a sequence of NC blocks

block is one of machining steps. Commands

Structure

Structure of

- Format of program

Configuration

of

an

of

of an

program

program name

NC

an

NC

an NC

NC Program

Commands

Commands in each block are the instruction.

Figure 1 . 25 Structure of an NC Program

name

Program

blocks

blocks . Each

The program name must be specified in the format OXXXX (X could be letters or

numbers).

program

- Format of program

T he program number should be started with %XXXX or OXXXX (X could be numbers

only).

- Format of blocks

A

block starts with the program block number.

program

program number

blocks

number

Figure 1 . 26 Structure of Block

19

end

Instruction 1

Instruction 2

Instruction n

Instruction n+1

Follow the direction

ofthe subprogra m

Instruction 1

Instruction 2

Return to the main pr ogram

Main program

Subprogram

of

- Format of end

The last block should contain M02 or M03 to indicate the end of program.

- Format of Comments

All information after the “ ; ” is regarded as comments.

All information between “ ( ) ” is regarded as comments.

end

end of

Comments

program

of

program

of program

program

1. General

1.8.2

1.8.2 Main

There are two type of program: main program and subprogram. The CNC operates

according to the main program. When a execution command of subprogram is at the

execution line of the main program, the subprogram is called. When the execution of

subprogram is finished, the system returns control to the main program.

Main

Main Program

Program

Program and

and

Subprogram

and

Subprogram

and Subprogram

Subprogram

Note:

Main program and its subprogram must be written in a same file with a different program

codes.

Figure 1 . 27 Main program and subprogram

20

2

Preparatory

2

Preparatory

2

2 Preparatory

Preparatory Function

There are two types of G code: one-shot G code, and modal G code.

Type

Type Meaning

One-shot G code The G code is only effective in the block in which it is specified

Modal G code The G code is effective until another G code is specified.

Example : G01 and G00 are modal G codes.

G00X_

Meaning

Function

Function (G

Table 2 1 Type of G code

(G

(G code)

code)

2. Preparatory Function

G01Z_

Z_

X_

G0 0 is effective in this range

21

2.1

G

2.1

2.1 G

The following table is the list of G code in HNC system.

code

G

code

G code

code List

G

code

G

code

G

G code

code Group

List

Group

Group Function

Function

Table 2 2 G code list

2. Preparatory Function

G00

G01

◣

01

G02

G03

G04 00 Dwell

G20

G21

◣

G28

G29

G32

G34

G36

◣

G37

G40

◣

G41

08

00

01

17

09

Positioning (Rapid traverse)

Linear interpolation (Cutting feed)

Circular interpolation CW

Circular interpolation CCW

Input in inch

Input in mm

R eference point return

Auto r eturn from reference point

Thread cutting with constant lead

Tapping

Diameter programming

Radius programming

Tool nose radius compensation cancel

Tool nose radius compensation on the left

G42

G46 16 Setting the limit of spindle speed

◣ G50

04

G51 Moving the origin of workpiece coordinate system

G53 00 Selecting a machine coordinate system

G54

◣

G55

G56

G57

G58

11 Setting a w orkpiece coordinate system

Tool nose radius compensation on the right

C anceling the workpiece’s origin movement

22

2. Preparatory Function

G59

23

2. Preparatory Function

G71

G72

Stock Removal in Turning

Stock Removal in Facing

G73

G74

G75

06

G76

G80

G81

G82

G90

◣

Pattern repeating

Front drilling cycle

Side drilling cycle

Multiple t hread cutting cycle

Internal diameter/ Outer diameter cutting cycle

End face turning cycle

Thread cutting cycle

Absolute programming

13

G91

Incremental programming

G92 00 Setting a c oordinate system

◣ G94

Feedrate per minute

14

G95

G96

Feedrate p er revolution

Constant cutting speed

16

Constant cutting speed cancel◣ G97

Explanation:

1) G codes in 00 group are one-shot G code, while the other groups are modal G

code.

2) ◣ means that it is default setting.

24

3

Interpolation

3

Interpolation

3

3 Interpolation

Interpolation Functions

This chapter would introduce:

1) Positioning Command (G00)

2) Linear Interpolation (G01)

3) Circular Interpolation (G02, G03)

4) Chamfering and Rounding (G01, G02, G03)

5) Thread Cutting with Constant Lead (G32)

6) Tapping (G34)

Functions

3. Interpolation Function

25

3.1

Positioning

3.1

Positioning

3.1

3.1 Positioning

Positioning (G00)

Programming

G00 X(U) … Z(W) …

(G00)

3. Interpolation Function

Explanation

Explanation of

X, Z Coordinate value of the end point in the absolute command

U, W Coordinate value of the end point in the incremental command

Function

The tool is moved at the highest possible speed (rapid traverse). I f the rapid traverse

movement is required to execute simultaneously on several axes, the rapid traverse speed is

decided by the axis which takes the most time. The operator can use this function to position

the tool rapidly, to travel around the workpiece, or to approach the tool change position.

Example

Move tool from P1 (45, 90) to P2 (10, 20) at the rapid traverse speed.

of

the

parameters

of

the

of the

parameters

the parameters

parameters

X

P1

P2

M

Absolute programming:

G00 X10 Z20

Incremental programming:

G00 U30 W70

W

Figure 3 . 1 Positioning (Rapid Traverse)

26

Z

3.2

Linear

3.2

Linear

3.2

3.2 Linear

Linear Interpolation

Programming

G01 X(U) … Z(W) … F …

Interpolation

Interpolation (G01)

(G01)

3. Interpolation Function

Explanation

Explanation of

X, Z Coordinate value of the end point in the absolute command

U, W Coordinate value of the end point in the incremental command

F Feedrate. It is effective until a new value is specified.

Function

The tool is moved along the straight line at the specified fe e drate .

of

the

parameters

of

the

of the

parameters

the parameters

parameters

27

3. Interpolation Function

Example

Example 1

1

Use G01 command to rough machining and finish machining the simple cylinder part .

%3306

Absolute command

（

N1 T0106

N2 M03 S460

N3 G00 X90Z20

N4 G00 X31Z3

N5 G01 Z-50 F100

N6 G00 X36

N7 Z3

Φ30

50

Figure 3 . 2 Linear Interpolation – Example 1

）

%3306

Φ35

Incremental command

（

N1 T0101

N2 M03 S460

N3 G00 X90Z20

N4 G00 X31Z3

N5 G01 W-53 F100

N6 G00 U5

N7 W53

）

N8 X30

N9 G01 Z-50 F80

N10 G00 X36

N11 X90 Z20

N12 M05

N13 M30

N8 U-6

N9 G01 Z-50 F80

N10 G00 X36

N11 X90 Z20

N12 M05

N13 M30

28

3. Interpolation Function

Example

Example 2

2

Use G01 command to rough machining and finish machining simple conical part.

%3307

N1 T0101

N2 M03 S460

N3 G00 X100Z40

N4 G00 X26.6 Z5

N5 G01 X31 Z-50 F100

N6 G00 X36

N7 X100 Z40

N8 T0202

Φ30

Figure 3 . 3 Linear Interpolation – Example 2

Φ26

Φ35

50

N9 G00 X25.6 Z5

N10 G01 X30 Z-50 F80

N11 G00 X36

N12 X100 Z40

N13 M05

N14 M30

29

3. Interpolation Function

Example

Example 3

3

Use G01 command to rough machining and finish machining the part.

2 × 4 5 °

Φ30

Figure 3 . 4 Linear Interpolation – Example 3

Φ28

Φ24

20

50

Φ35

%3308

N1 T0101

N2 M03 S450

N3 G00 X100 Z40

N4 G00 X31 Z3

N5 G01 Z-50 F100

N6 G00 X36

N7 Z3

N8 X25

N9 G01 Z-20 F100

N10 G00 X36

N11 Z3

N12 X15

N13 G01 U14 W-7 F100

N14 G00 X36

30

N15 X100 Z40

N16 T0202

N17 G00 X100Z40

N18 G00 X14 Z3

N19 G01 X24 Z-2 F80

N20 Z-20

N21 X28

N22 X30 Z-50

N23 G00 X36

N24 X80 Z10

N24 M05

3. Interpolation Function

N25 M30

31

3.3

Circulation

3.3

Circulation

3.3

3.3 Circulation

Circulation Interpolation

Programming

Interpolation

Interpolation (G02,

(G02,

(G02, G03)

G03)

3. Interpolation Function

G02

⎫

⎧

⎬

⎨

G03

⎭

⎩

Explanation

Explanation of

G02 a circular path in c lockwise direction (CW)

G03 a circular path in c ounterclockwise direction (CCW)

X , Z Coordinate values of the circle end point in a bsolute command

U , W Coordinate values of the circle end point with reference to the circle starting point

in incremental command.

I , K Coordinate values of the circle center point with reference to the circle starting

point in incremental command.

R Circle radius . R is valid when I, K, R are all specified in this command.

F Feedrate

of

the

of

the

of the

the parameters

⎧

_)_Z( )X(

WU

⎨ ⎩

parameters

I_K_

⎫

F_

⎬

R_

⎭

+X

z

u/2

x/2

w

B

k

A

R

Circle center point

Figure 3 . 5 Description of G02/G03 parameter

i

＋ Z

32

z

x/2

u/2

+X

w

A

R

B

Circle center point

k

+Z

i

3. Interpolation Function

G02 and G03 are defined when the working plane is specified. Figure 3.6 shows the

direction of circular interpolation.

+X

G02

G03

G02

G03

+Y

Z

＋ Z

Z

G03

G02

+X

G02

Function

G03

G02

+Y

G02

Z

＋ Z

Z

G02

G03

Figure 3 . 6 Direction of Circular Interpolation

The tool is moved along a full circle or arcs.

33

3. Interpolation Function

27

R 15 40

31

R 5

Φ 26

Φ 22

Example

Example 1

1

U se the circular interpolation command to program

Figure 3 . 7 Circular Interpolation – Example 1

%3309

N1 T0101

N2 G00 X40 Z5

N3 M03 S400

N4 G00 X0

N5 G01 Z0 F60

N6 G03 U24 W-24 R15

N7 G02 X26 Z-31 R5

N8 G01 Z-40

N9 X40 Z5

N10 M30

34

3. Interpolation Function

35

Φ35

Φ30

R15

Example

Example 2

2

U se the circular interpolation command to program

Figure 3 . 8 Circular Interpolation – Example 2

%3310

Absolute programming

（

）

%3310

Incremental programming

（

）

N1 T0101

N2 M03 S460

N3 G00 X90Z20

N4 G00 X0 Z3

N5 G01 Z0 F100

N6 G03 X30 Z-15 R15

N7 G01 Z-35

N8 X36

N9 G00 X90 Z20

N10 M05

N11 M30

N1 T0101

N2 M03 S460

N3 G00 X90Z20

N4 G00 U-90 W-17

N5 G01 W-3 F100

N6 G03 U30 W-15 R15

N7 G01 W-20

N8 X36

N9 G00 X90 Z20

N10 M05

N11 M30

35

Example

24

40

Φ20

Φ 24

R10

R 4

Example

Example 3

3

U se the circular interpolation command to program .

Figure 3 . 9 Circular Interpolation – Example 3

%3311

N1 T0101

N2 M03 S460

3. Interpolation Function

N3 G00 X100 Z40

N4 G00 X0 Z3

N5 G01 Z0 F100

N6 G03 X20 Z-10 R10

N7 G01 Z-20

N8 G02 X24 Z-24 R4

N9 G01 Z-40

N10 G00 X30

N11 X100 Z40

N12 M05

N13 M30

36

Example

40

Φ26

20

Φ30

R2

Example

Example 4

4

U se the circular interpolation command to program

Figure 3 . 10 Circular Interpolation – Example 4

%3312

N1 T0101

N2 M03 S460

3. Interpolation Function

N3 G00 X80 Z10

N4 G00 X30 Z3

N5 G01 Z-20 F100

N6 G02 X26 Z-22 R2

N7 G01 Z-40

N8 G00 X24

N9 Z3

N10 X80 Z10

N11 M05

N12 M30

37

3.4

Chamfering

3.4

Chamfering

3.4

3.4 Chamfering

Chamfering and

Note:

Note: These commands can not be used in thread cutting.

and

and Rounding

Rounding

Rounding (G01,

(G01,

(G01, G02,

3. Interpolation Function

G02,

G02, G03)

G03)

3.4.1

3.4.1 Chamfering

Programming

G01 X(U)_ Z(W)_ C_

Explanation

Explanation of

X, Z Coordinate values of the intersect ion (point G) in absolute command

U, W Coordinate values of the intersection (point G) in incremental command

C Width of chamfer in original direction of movement (c)

Chamfering

Chamfering (G01)

of

the

of

the

of the

the parameters

(G01)

parameters

+X

D

C

1.1.1.1.1.1

z

1.1.1.1.1.1

c

1.1.1.1.1.2

w

A

u/2

B

G

x/2

+Z

Figure 3 .11Chamfering (G01)

Function

A

chamfer can be inserted between two blocks which intersect at a right angle (point A

→ C).

Note:

Note: The length of GA should be more than the length of GB

38

B

→

3. Interpolation Function

3.4.2

3.4.2 Rounding

Programming

Rounding

Rounding (G01)

(G01)

G01 X(U)_ Z(W)_ R_

Explanation

Explanation of

of

the

parameters

of

the

of the

parameters

the parameters

parameters

X, Z Coordinate values of the intersect ion (point G) in absolute command

U, W Coordinate values of the intersection (pint G) in incremental command

R Radius of the rounding (r)

w

+X

r

D

r

C

z

w

A

u/2

B

G

x/2

+Z

Figure 3 . 12 Rounding (G01)

Function

A

corner can be inserted between two blocks which intersect at a right angle (point A → B →

C).

Note:

Note: The length of GA should be more than the length of GB

39

Example

Use the chamfering and rounding command (G01):

70

3

R3

65

Φ

Figure 3 . 13 Chamfering and Rounding (G01) - Example

3. Interpolation Function

10

36

22

70

26

Φ

%3314

N1 M03 S460

N2 G00 U-70 W-10

N3 G01 U26 C3 F100

N4 W-22 R3

N5 U39 W-14 C3

N6 W-34

N7 G00 U5 W80

N8 M30

40

3. Interpolation Function

3.4.3

3.4.3 Chamfering

Programming

⎧ ⎨ ⎩

Explanation

Explanation of

X, Z Coordinate values of the intersection (point G) in absolute command

U, W Coordinate values of the intersection (point G) with reference to the circle starting

point (point A) in incremental command

R Circle Radius (r)

RL= Width of chamfer in original direction of movement (RL)

Chamfering

Chamfering (G02,

G02

⎫ ⎬

G03

⎭

of

the

of

the

of the

the parameters

WU

parameters

+X

(G02,

(G02, G03)

G03)

_ RL _ R _ ) Z( _ )X(

=

w

A

r

B

r

C

D

Function

A

chamfer can be inserted between two blocks which intersect at a right angle (point A

→ C).

Note:

Note: RL must be capitalized letters.

C

RL=

G

z

Figure 3 . 14 Chamfering (G02/G03)

G

+Z

B

→

41

3. Interpolation Function

3.4.4

3.4.4 Rounding

Programming

⎧ ⎨ ⎩

Explanation

Explanation of

X, Z Coordinate values of the intersection (point G) in absolute command

U, W Coordinate values of the intersection (point G) with reference to the circle starting

point (point A) in incremental command

R Circle radius (r)

RC Radius of rounding (rc)

Rounding

Rounding (G02,

G02

⎫ ⎬

G03

⎭

(G02,

(G02, G03)

WU

of

the

parameters

of

the

of the

parameters

the parameters

parameters

G03)

_ RC _ R _ )Z(_ )X(

=

w

+X

rc=

D

C

z

w

A

r

u/2

B

G

u/2

x/2

+Z

Figure 3 . 15 Rounding (G02/G03)

Function

A

corner can be inserted between two blocks which intersect at a right angle (point A → B →

C).

Note:

Note: RC must be capitalized letters.

42

Example

Use the chamfering and rounding command (G02/G03):

70

4

56

Φ

Figure 3 . 16 Chamfering and Rounding (G02/G03) - Example

36

R15

%3315

3. Interpolation Function

10

21

70

26

Φ

N1 T0101

N2 G00 X70 Z10 M03 S460

N3 G00 X0 Z4

N4 G01 W-4 F100

N5 X26 C3

N6 Z-21

N7 G02 U30 W-15 R15 RL=4

N8 G01 Z-70

N9 G00 U10

N10 X70 Z10

N11 M30

43

3.5

α

+ X

z

w

u /2

L

A

B

x /2

e

δ

Thread

3.5

Thread

3.5

3.5 Thread

Thread Cutting

Programming

G32 X ( U ) __Z ( W ) __R__E__P__F__

Cutting

Cutting with

with

with Constant

Constant

Constant Lead

3. Interpolation Function

Lead

Lead (G32)

(G32)

Explanation

Explanation of

X, Z Coordinate values of end point in absolute command

U, W Coordinate values of end point with reference to the starting point in incremental

command

R, E Coordinate value of retraction amount with reference to the end point in

incremental command. In general, R is set as two times value of thread lead, and E is set as

the thread height.

P Start point offset. It is used for multiple threads.

F Thread lead per revolution

of

the

parameters

of

the

of the

parameters

the parameters

parameters

Figure 3 . 17 Thread Cutting with Constant Lead

44

3. Interpolation Function

X

Start point offset in °

Starting angle for thread (setting data)

Z

Figure 3 . 18 Start point Offset

Function

Cylindrical thread, taper thread and face thread can be machined with G32.

Note:

1) T he spindle speed should remain constant during rough cutting and finish cutting.

2) The feed hold function is ineffective during the thread cutting. Even though the

“ feed hold ” button is pressed, it is effective until the thread cutting is done.

3) It is not recommended to use the constant surface speed control during the thread

cutting.

4) Allowant amount must be specified to avoid the error.

45

Example

3. Interpolation Function

Given that F=1.5mm,

=1.5mm,

δ

=1mm, cutting for four times and each cutting depth

′

δ

is separately: 0.8mm, 0.6 mm, 0.4mm, 0.16mm. It is diameter programming.

100

80

1.5

×

M30

Figure 3 . 19 Thread Cutting – Example

%3316

N1 T0101

N2 G00 X50 Z120

N3 M03 S300

N4 G00 X29.2 Z101.5

N5 G32 Z19 F1.5

N6 G00 X40

N7 Z101.5

N8 X28.6

N9 G32 Z19 F1.5

N10 G00 X40

N11 Z101.5

N12 X28.2

N13 G32 Z19 F1.5

N14 G00 X40

N15 Z101.5

N16 U-11.96

N17 G32 W-82.5 F1.5

N18 G00 X40

N19 X50 Z120

N20 M05

N21 M30

46

3.6

Tapping

3.6

Tapping

3.6

3.6 Tapping

Tapping (G34)

Programming

G34 K _ F _ P _

(G34)

3. Interpolation Function

Explanation

Explanation of

K The distance from the starting point to the bottom of the hole

F Thread lead

P Dwell time at the bottom of a hole

Function

With this command, the operator can rigid tap a thread.

of

the

parameters

of

the

of the

parameters

the parameters

parameters

X

K

Figure 3 . 20 Rigid Tapping

Z

In general, there is overshoot of the tap at the bottom of the thread during the

spindle-braking portion of the tapping cycle. It can be set by PMC parameters (Table 3-1) to

eliminate the overshoot errors.

47

Table 3 1 PMC parameters

CNC

system

CNC

system

CNC

CNC system

system PMC

#0062 Maximum spindle speed during tapping

PMC

parameters

PMC

parameters

PMC parameters

parameters

3. Interpolation Function

HNC 18/19i

#0063 Minimum spindle speed during tapping

#0064

#0065

Dwelled unit for tapping

Optional dwelled unit for tapping

#0017 Maximum spindle speed during tapping

#001 8 Minimum spindle speed during tapping

HNC 21/22

#001 9

#00 30

Dwelled unit for tapping

Optional dwelled unit for tapping

Optional dwelled unit for tapping is only effective when “ dwelled unit for tapping ” is

assigned to “ 0 ” . Moreover, it is not necessary to restart the system.

The following formular is to calculate the dwelled unit (X):

D = (S * S / C) * X / 10000 = L * 360 / F

D dwelled amount

S spindle speed

C Transmission gear ratio

X dwelled unit

L overshoot error

F thread lead

Since the workpiece is chucked on the spindle, the spindle decceleration time of turning

machine is more than a milling machine

’

s. The quicker the spindle rotates, the quicker the

feedrate on Z axis is, and then the more time the decceleration time takes. Thus, the spindle

speed should be set accoording to the thread length.

48

Example

The following is a tested data for tapping when the thread lead is 1.25mm.

%0034

T0101

S100

G90G1X0Z0F500

G34K-10F1.25P2

S200

G90G1X0Z0F500

G34K-10F1.25P2

S300

G90G1X0Z0F500

G34K-10F1.25P2

S400

G90G1X0Z0F500

3. Interpolation Function

G34K-20F1.25P2

S500

G90G1X0Z0F500

G34K-30F1.25P3

S600

G90G1X0Z0F500

G34K-40F1.25P3

S700

G90G1X0Z0F500

G34K-50F1.25P3

S800

G90G1X0Z0F500

G34K-50F1.25P2

S1000

G90G1X0Z0F500

G34K-60F1.25P3

M30

49

4

Feed

4

Feed

4

4 Feed

Feed Function

There are two kinds of feed functions:

1. Rapid Traverse

The tool is moved at the rapid traverse speed set in CNC.

2. Cutting Feed

The tool is moved at the programmed cutting feedrate.

Moreover, this chapter would introduce “ Dwell ” .

Function

4. Feed Function

50

4. Feed Function

4.1

Rapid

4.1

Rapid

4.1

4.1 Rapid

Rapid Traverse

Positioning command (G00) is to move the tool at the rapid traverse speed (the highest

possible speed).

This rapid traverse speed can be controlled by the machine control panel. For more detailed

information, please refer to turning operation manual.

Traverse

Traverse (G00)

(G00)

51

4.2

Cutting

4.2

Cutting

4.2

4.2 Cutting

Cutting Feed

Programming

G94 [F_ ]

G95 [F_ ]

Feed

Feed (G94,

(G94,

(G94, G95)

G95)

4. Feed Function

Explanation

Explanation of

G94 feedrate per minute.

On linear axis, the unit of feedrate is mm/min, or in/min.

On rational axis, the unit of feedrate is degree/min.

G95 feedrate per revolution

The unit of feedrate is mm/rev, or in/rev.

Note:

1) G94 is the default setting

2) G95 is only used when there is spindle encoder.

Function

The feedrate can be set by G94 or G95.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

52

4.3

Dwell

4.3

Dwell

4.3

4.3 Dwell

Dwell (G04)

Programming

G04 P_

(G04)

4. Feed Function

Explanation

Explanation of

P dwell time (specified in seconds)

Function

It can be used to interrupt machining to get the smooth surface. I t can be used to control the

groove cutting, drilling, and turning path.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

53

5

Coordinate

5

Coordinate

5

5 Coordinate

Coordinate System

This chapter would introduce:

1) Reference Position Return (G28)

2) Auto Return from Reference Position (G29)

3) Setting a Workpiece Coordinate System (G92)

4) Selecting a Machine Coordinat System (G53)

5) Selecting a Workpiece Coordinate System (G54~G59)

6) Origin of a W orkpiece Coordinate System (G51, G50)

7) Absolute and Incremental Programming (G90, G91)

8) Diameter and Radius Programming (G36, G37)

9) Inch/Metric Conversion (G20, G21)

System

5. Coordinate System

54

5.1

Reference

5.1

Reference

5.1

5.1 Reference

Reference Position

Programming

G28 X(U)_ Z(W)_

Position

Position Return

Return

Return (G28)

(G28)

5. Coordinate System

Explanation

Explanation of

X, Z Coordinate values of the intermediate point in absolute command

U,W Coordinate values of the intermediate point with reference to the starting point in

incremental command

Function

The tool is moved to the intermediate point rapidly, and then returned to the reference point.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

X

Intermediate position

Reference position

Z

Figure 5 . 1 Reference Position Return

Note:

1) In general, G28 is used to change tools or cancel the mechanical error. Tool radius

compensation and tool length compensation should be cancelled when G28 is

executed.

2) G28 can not only make the tool move to the reference point, but also can save the

intermediate position to be used in G29.

3) When the power is on and manual reference position return is not available, G28 is

same as the maunaul reference position return. The direction of this reference

position return (G28) is set by the axis parameter – reference approach direction.

4) G28 is one-shot G code.

55

5.2

Auto

5.2

Auto

5.2

5.2 Auto

Auto Return

Programming

G29 X(U)_ Z(W)_

Return

Return from

from

from Reference

Reference

Reference Position

5. Coordinate System

Position

Position (G29)

(G29)

Explanation

Explanation of

X, Z Coordinate value of the end point in absolute command

U, W Coordinate value of the end point in incremental command

Function

The tool is moved rapidly from the intermediate point defined in G28 to the end point. Thus,

G29 is generally used after G28 is defined.

Note:

G29 is one-shot G code.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

56

Example

Φ 40

B

C R

A

250

100

Φ 50

200

Φ 80

+X

+Z

Example

5. Coordinate System

Use G28, G29 command to program the track shown in. It moves from the starting point

to the intermediate point B , and then return s to the reference point R. At last, it moves from

the reference point R to the end point C through the intermediate point B.

Figure 5 . 2 Reference Position – Example

%3317

N1 T0101

A

N2 G00 X50 Z100

N3 G28 X80 Z200

N4 G29 X40 Z250

N5 G00 X50Z100

N6 M30

57

5.3

Setting

5.3

Setting

5.3

5.3 Setting

Setting a

Programming

G92 X_ Z_

a

Workpiece

a

Workpiece

a Workpiece

Workpiece Coordinate

Coordinate

Coordinate System

5. Coordinate System

System

System (G92)

(G92)

Explanation

Explanation of

X, Z Coordinate values of the tool position in the workpiece coordinate system.

Functions

G92 can set a workpiece coordinate system based on the current tool position (X_ Z_).

Example

Use G92 to set a workpiece coordinate system.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

+X

Origin

Origin on

left

end

left

end

left

left end

end face

254

44

180

on

end

end face

face

Φ

+Z

on

face

O

rigin

O

rigin

O

O rigin

rigin on

right

right end

Figure 5 . 3 Setting a Coordinate System – Example

If the origin is set on the left end face,

G92 X180 Z254

If the origin is set on the right end face

G92 X180 Z44

58

5.4

Selecting

5.4

Selecting

5.4

5.4 Selecting

Selecting a

Programming

G53 X_Z_

a

Machine

a

Machine

a Machine

Machine Cooridinate

Cooridinate

Cooridinate System

5. Coordinate System

System

System (G53)

(G53)

Explanation

Explanation of

X, Z Absoulte coordinate values of a point in the machine coordinate system.

Function

A

machine coordinate system is selected, and the tool moves to the position at the rapid

traverse speed.

Note:

1) Absolute values must be specified in G53. The incremental values would be

2) G53 is one-shot G code.

of

the

of

the

of the

the parameters

ignored by G53.

parameters

59

5.5

Selecting

5.5

Selecting

5.5

5.5 Selecting

Selecting a (G54~G59)

(G54~G59)

Programming

54

G

⎫

⎧

⎪

55

G

⎪

56

G

⎪

⎪ ⎨

G

⎪ ⎪

G

⎪ ⎪

G

⎩

X_ Z_

⎬

57

⎪ ⎪

58

⎪ ⎪

59

⎭

a

Workpiece

a

Workpiece

a Workpiece

Workpiece Coordinate

Coordinate

Coordinate System

5. Coordinate System

System

Explanation

Explanation of

X, Z Coordinate values of the point in absolute command

Function

There are six workpiece coordinate system to be selected. If one coordinate system is

selected, the tool is moved to a specified point.

Note:

1) The workpiece coordinate system must be set before these commands (G54~G59)

2) Reference position must be returned before these commands (G54~G59) are

3) G54 is the default setting.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

are used. The workpiece coordinate system can be set by using the MDI panel. For

detailed information, please refer to the turning operation manual.

executed.

60

Example

G54

O

A

X

Z

G59

O

30

40

30

B

X

Machine Zero Point

Example

5. Coordinate System

Select one of workpiece coordinate system, and the tool path is Current point→A

Figure 5 . 4 Workpiece Coordinate System – Example

%3303

N01 G54 G00 G90 X40 Z30

N02 G59

N03 G00 X30 Z30

N04 M30

B.

→

61

5.6

Origin

5.6

Origin

5.6

5.6 Origin

Origin of G50)

G50)

Programming

G51 U_ W_

G50

of

a

of

of a

Workpiece

a

Workpiece

a Workpiece

Workpiece Coordinate

Coordinate

Coordinate System

System

System (G51,

5. Coordinate System

(G51,

Explanation

Explanation of

G51 can move the origin of workpiece coordinate system.

U, W Coordinate values of the position in incremental command

G50 can cancel the movement.

Function

The origin of workpiece coordinate system can be moved.

Note:

1) G51 is only effective when T command or G54~G59 is defined in the program.

2) G50 is only effective when T command or G54~G59 is defined in the program.

Example

%1234

G51 U30 W10

M98 P1111 L4

of

the

parameters

of

the

parameters

of the

the parameters

parameters

G50

T0101

G01 X30 Z14

M30

%1111

T0101

G01 X32 Z25

G01 X34.444 Z99.123

M99

62

5.7

Absolute

5.7

Absolute

5.7

5.7 Absolute

Absolute and G91)

G91)

Programming

G90 X_ Z_

G91 U_W_

and

and Incremental

Incremental

Incremental Programming

5. Coordinate System

Programming

Programming (G90,

(G90,

Explanation

Explanation of

G90 Absolute programming

X, Z Coordinate values on X axis and Z axis in the coordinate system

G91 Incremental programming

U, W Coordinate values with reference to the previous position in the coordinate system

Function

The tool is moved to the specified position.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

63

5. Coordinate System

1

Φ

Φ 15

15

Φ

Φ 25

25

30

40

4

3

2

1

Φ

Φ 50

50

2

Example

Move the tool from point 1 to point 2 through point 3, and then return to the current point.

Figure 5 . 5 Absolute and Incremental Programming – Example

Absolute Programming

%0001 N 1 T0101 N 2 M03 S460 N3 G90 G00 X50 Z2 N4 G01 X15 N 5 Z-30 N 6 X25 Z-40 N 7 X50 Z2 N 8 M30

Incremental Programming

%0001 N 1 M03 S460 N 2 G91 G01 X-35 N 3 Z-32 N 4 X10 Z-10

N 5 X25 Z42 N 6 M30

Absolute and I ncremental

%0001 N 1 T0101 N 2 M03 S460 N 3 G00 X50 Z2 N 4 G01 X15 N 5 Z-30 N 6 U10 Z-40 N 7 X50 W42 N 8 M30

64

5.8

Diameter

5.8

Diameter

5.8

5.8 Diameter

Diameter and

Programming

G36

G37

and

and Radius

Radius

Radius Programming

Programming

Programming (G36,

(G36,

(G36, G37)

5. Coordinate System

G37)

Explanation

Explanation of

G36 Diameter programming

G37 Radius programming

Function

The coordinate value on X axis is specified in two ways: diameter or radius. It allows to

program the dimension straight from the drawing without conversion.

Note:

1) In all the examples of this book, we always use diameter programming if the

2) If the machine parameter is set to d iameter programming, then d iameter

of

the

parameters

of

the

parameters

of the

the parameters

parameters

r adius p rogramming is not specified.

programming is the default setting . However, G36 and G37 can be used to

ex change. T he system shows the d iameter value.

3) If the system parameter is set to radius programming, then radius programming is

the default setting . However, G36 and G37 can be used to ex change. T he system

shows the radius value.

65

Example

Φ

180

160

+X

44

254

Φ

20

50

Φ

Example

Use Diameter programming and Radius programming for the same path

Figure 5 . 6 Diameter and Radius Programming – Example

5. Coordinate System

Diameter Programming Radius Programming Compound Programming

%3304

N1 G92 X180 Z254

N2 M03 S460

N3 G01 X20 W-44

N4 U30 Z50

N5 G00 X180 Z254

N6 M30

%3314

N1 G37 M03 S460

N2 G54 G00 X90 Z254

N3 G01 X10 W-44

N4 U15 Z50

N5 G00 X90 Z254

N6 M30

%3314

N1 T0101

N2 M03 S460

N3 G37G00 X90 Z254

N4 G01 X10 W-44

N5 G36 U30 Z50

N6 G00 X180 Z254

N7 M30

66

5.9

Inch/Metric

5.9

Inch/Metric

5.9

5.9 Inch/Metric

Inch/Metric Conversion

Programming

G20

G21

Conversion

Conversion (G20,

(G20,

(G20, G21)

G21)

5. Coordinate System

Explanation

Explanation of

G20: Inch input

G21: Metric input

The units of linear axis and circular axis are shown in the following table

Function

Depending on the part drawing, the workpiece geometries can be programmed in metric

measures or inches.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

Table 5 1

Inch system (G20) Inch Degree

Metric system (G21) Mm Degree

. Unit of Linear axis and Circular axis

Linear axis Circular axis

67

6. Spindle Speed Function

6

Spindle

6

Spindle

6

6 Spindle

Spindle Speed

Spindle function controls the spindle speed (S), the unit of spindle speed is r/min. S pindle

speed is the cutting speed when it is at the constant speed, the unit of speed is m/min .

S is modal G code command; it is only available when the spindle is adjustable. Spindle

speed programmed by S code can be adjusted by overrides on the machine control panel.

This chapter would introduce

1) Limit of spindle speed (G46)

2) Constant surface cutting control (G96, G97).

Speed

Speed Function

Function

68

6.1

Limit

6.1

Limit

6.1

6.1 Limit

Limit of

Programming

G46 X_ P_

of

Spindle

of

Spindle

of Spindle

Spindle Speed

Speed

Speed (G46)

(G46)

6. Spindle Speed Function

Explanation

Explanation of

X The minimum speed of the spindle when using constant surface speed （ r/min ）

P The maximum speed of the spindle when using constant surface speed

Function

G46 command can set the minimum of spindle speed, and the maximum of spindle speed.

Note:

It can only used with G96 (constant surface speed control command).

of

the

parameters

of

the

parameters

of the

the parameters

parameters

r/min

（

）

69

6.2

Constant

6.2

Constant

6.2

6.2 Constant

Constant Surface

Programming

G96 S

G97 S

Surface

Surface Speed

Speed

Speed Control

Control

Control (G96,

(G96,

(G96, G97)

6. Spindle Speed Function

G97)

Explanation

Explanation of

G 96 activate the constant surface speed

S surface speed (m/min)

G97 deactivate the constant surface speed

S spindle speed (r/min)

Function

G96 and G97 commands are to control the constant surface speed.

Note

Note :

1) The spindle speed must be controlled automatically when the constant surface

2) The maximum of spindle speed can be set by the axis parameter.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

cutting command is executed.

70

Example

27

R 15 40

31

R 5

Φ 26

Φ 22

Example

Use the c onstant surface control command

Figure 6 . 1 Constant Surface Control – Example

%3318

6. Spindle Speed Function

N1 T0101

N2 G00 X40 Z5

N3 M03 S460

N4 G96 S80

N5 G46 X400 P900

N5 G00 X0

N6 G01 Z0 F60

N7 G03 U24 W-24 R15

N8 G02 X26 Z-31 R5

N9 G01 Z-40

N10 X40 Z5

N11 G97 S300

N12 M30

71

7

Tool

7

Tool

7

7 Tool

Tool Function

This chapter would introduce:

1) Too selection and Tool offset (T code)

2) Tool radius compensation (G40, G41, G42)

Function

7.

Tool

Function

72

7.1

Tool

7.1

Tool

7.1

7.1 Tool

Tool Selection

Programming

T XX XX

Selection

Selection and

and

and Tool

Tool

Tool Offset

Offset

Offset (T

(T

code)

(T

code)

(T code)

code)

7.

Tool

Function

Explanation

Explanation of

XX Tool number (two digits). The number of tool depends on manufacture’s

configuration.

XX Tool offset number (two digits). It corresponds to the specific compensation value.

Functions

To

select the desired tool, T command makes the turret turn, selects a cutter, and calls the

compensation value.

Note:

1) T command is only effective when it is used with tool move command, such as

2) When T command and tool move command are in the same program block, T

3) The same tool can have different compensation values. F or example, T0101,

of

the

parameters

of

the

parameters

of the

the parameters

parameters

G00

command is executed at first.

T0102, T0103 are possible.

4) Different tool can have same compensation values. For example, T0101, T0201,

and T0301 are possible.

73

Example

%0012

N01 T0101

N02 M03 S460

N03 G00 X45 Z0

N04 G01 X10 F100

N05 G00 X80 Z30

N06 T0202

N07 G00 X40 Z5

N08 G01 Z-20 F100

N09 G00 X80 Z30

N10 M3 0

7.

Tool

Function

74

7.2

Tool

7.2

Tool

7.2

7.2 Tool

Tool Radius

Programming

40

G

⎫

⎧ ⎪

⎨

G

⎪

G

⎩

G

⎧

⎪ ⎬

41

⎨

G

⎩

⎪

42

⎭

Radius

Radius Compensation

00

⎫

X _ Z_

⎬

01

⎭

Compensation

Compensation (G40,

(G40,

(G40, G41,

G41,

G41, G42)

G42)

7.

Tool

Function

Explanation

Explanation of

G40 Deactivate tool radius compensation

G41 Activate tool radius compensation, tool operates in machining operation to the left

of the contour.

G42 Activate tool radius compensation, tool operates in machining operation to the

right of the contour.

of

the

parameters

of

the

parameters

of the

the parameters

parameters

Figure 7 . 1

G42

G41

Tool

Radius Compensation

X, Z Coordinate values of the end point. It is the point where the tool radius

compensation is activated or deactivated.

Function

These commands can control the tool radius compensation to get the equidistant tool paths

for different tools.

Note:

1) G40, G41, and G42 must be used with G00 or G01.

2) The tool radius compensation value is assigned in T code.

75

Example

27

R 15 40

31

R 5

Φ 26

Φ 22

Example

Use the tool radius compensation, and program for the part shown in Fig ure 7.2

7.

Tool

Function

%3323

N1 T0101

N2 M03 S400

N3 G00 X40 Z5

N4 G00 X0

N5 G01 G42 Z0 F60

N6 G03 U24 W-24 R15

N7 G02 X26 Z-31 R5

N8 G01 Z-40

N9 G00 X30

N10 G40 X40 Z5

N11 M30

Figure 7 . 2

Tool

Radius Compensation

76

8. Miscellaneous Function

8

Miscellaneous

8

Miscellaneous

8

8 Miscellaneous

Miscellaneous Function

As it is mentioned in Chapter 1.8, there are two ways of execution when a move command

and M code are specified in the same block.

1) Pre-M function

M command is executed before the completion of move command.

2) Post-M function

M command is executed after the completion of move command

There are two types of M code: one-shot M code, and modal M code.

Type

Type Meaning

One-shot M code The M code is only effective in the block in which it is specified

Modal M code The M code is effective until another M code is specified.

Meaning

Function

Table 8 1 Type of M code

77

8.1

M

8.1

8.1 M

The following is a list of M command.

CNC

CNC M-function

code

M

code

M code

code List

M-function

M-function Type

M00 One-shot Program stop P ost-M function

M01 One-shot Optional stop P ost-M function

M02 One-shot End of program Post-M function

List

Type

Type of

of

Mode

of

Mode

of Mode

Mode Function

Table 8 2 M code List

Function

Function Pre/Post-M

8. Miscellaneous Function

Pre/Post-M

Pre/Post-M function

function

M30 One-shot

M98 One-shot C alling of subprogram Post-M function

M99 One-shot End of subprogram Post-M function

PLC

M-function

PLC

M-function

PLC

PLC M-function

M-function Type

M03 M odal Spindle forward rotation Pre-M function

M04 M odal Spindle reverse rotation Pre-M function

M05 M odal ◣ Spindle stop Post-M function

M07 M odal Number1 Coolant on Pre-M function

M08 M odal Number2 Coolant on Pre-M function

M09 M odal

◣ : default setting

Type

Type of

End of program with return to the beginning of program

of

Mode

of

Mode

of Mode

Mode Function

◣ Coolant off

Post-M function

Function

Function Pre/Post-M

Pre/Post-M

Pre/Post-M function

Post-M function

function

78

8.2

CNC

8.2

CNC

8.2

8.2 CNC

CNC M-Function

M-Function

8. Miscellaneous Function

8.2.1

8.2.1 Program

M00 is one-shot M function, and it is post-M function .

The program can be stopped , so that the operator could measure the tool and the part, adjust

part and change speed manually, and so on.

When the program is stopped, the spindle is stopped and the coolant is off. All of the current

mod al information remains unchanged. Resuming program could be executed by pushing

“ Cycle Run ” button on the machine control panel .

8.2.2

8.2.2 Optional

M01 is one-shot M function, and it is post-M function.

Similarly to M00, M01 can also stop the program. All of the modal information is

maintained. The difference between M00 and M01 is that the operator must press M01

button ( ) on the machine control panel. Otherwise, the program would not be stopped

even if there is M01 code in the program.

Program

Program Stop

Optional

Optional Stop

Stop

Stop (M00)

Stop

Stop (M01)

(M00)

(M01)

8.2.3

8.2.3 End

M02 is one-shot M function, and it is post-M function.

When M02 is executed, spindle, feed and coolant are all stopped. It is usually at the end of

the last program block.

panel.

8.2.4

8.2.4 End

M30 is one-shot M function, and it is post-M function.

Similarly to M02, M30 can also stop the program. The difference is that M30 returns control

to the beginning of program.

operational panel.

End

End of

End

End of (M30)

(M30)

of

Program

of

Program

of Program

Program (M02)

To

restart the program, press “ Cycle Run ” button on the operational

of

Program

of

Program

of Program

Program with

(M02)

with

with return

To

return

return to

restart the program, press “ Cycle Run ” button on the

to

the

to

to the

79

beginning

the

beginning

the beginning

beginning of

of

of program

program

8. Miscellaneous Function

8.2.5

8.2.5 Subprogram

� End of Subprogram (M99)

M99 indicates the end of subprogram and returns control to the main program. It is one-shot

M function, and it is post-M function.

�

M98 is used to call a subprogram. It is one-shot M function. Moreover, it is post-M

function.

Subprogram

Subprogram Control

C alling a S ubprogram (M98)

M98 P_ L_

P program n umber of the subprogram

L repeated times of subprogram

Control

Control (M98,

(M98,

(M98, M99)

M99)

80

Example

8. Miscellaneous Function

R60

24

Φ

21.2

Φ

14.77

Φ

R8

%3111

N1 G92 X32 Z1

N2 G00 Z0 M03 S46

N3 M98 P0003 L5

N4 G36 G00 X32 Z1

N5 M05

N6 M30

%0003

N1 G37 G01 U-12 F100

N2 G03 U7.385 W-4.923 R8

R40

73 . 436

Figure 8 . 1 Subprogram Control - Example

4 . 923

44 . 8

N3 U3.215 W-39.877 R60

N4 G02 U1.4 W-28.636 R40

N5 G00 U4

N6 W73.436

N7 G01 U-5 F100

N8 M99

8.3

PLC

8.3

PLC

8.3

8.3 PLC

PLC M

M

Function

M

Function

M Function

Function

81

8. Miscellaneous Function

8.3.1

8.3.1 Spindle

M03 starts spindle to rotate CW at the set speed set in the program.

M04 starts spindle to rotate CCW at the set speed in the program.

M05 stops spindle.

M03, M04 are modal M code , and they are pre-M function . M05 is modal M code , and it is

post-M function . M05 is the default setting .

8.3.2

8.3.2 Coolant

M07, M08 can turn on the coolant.

M09 can turn off the coolant.

M07 and M08 are modal M code , and they are pre-M function . M09 is one-shot M code ,

and it is post-M function . Moreover, M09 is the default setting .

Spindle

Spindle Control

Coolant

Coolant Control

Control

Control (M03,

Control

Control (M07,

(M03,

(M03, M04,

(M07,

(M07, M08,

M04,

M04, M05)

M08,

M08, M09)

M05)

M09)

82

9

Functions

9

Functions

9

9 Functions

Functions to

T his chapter would introduce:

1) Canned Cycle

Internal diameter/ Outer diameter cutting cycle (G80)

End face turning cycle (G81)

Thread cutting cycle (G82)

End face peck drilling cycle (G74)

Outer diameter grooving cycle (G75)

2) Multiple Repetitive Cycle

Stock Removal in Turning (G71)

Stock Removal in Facing (G72)

Pattern Repeating (G73)

Multiple Thread Cutting Cycle (G76)

9. Functions to Simplify Programming

to

Simplify

to

Simplify

to Simplify

Simplify Programming

Programming

83

9. Functions to Simplify Programming

9.1

Canned

9.1

Canned

9.1

9.1 Canned

Canned Cycles

To

simplify programming, the canned cycle command can execute the specific operation

using one G code, instead of several separated G commands in the program.

Cycles

9.1.1

9.1.1 Internal

�

� Straight

Programming

G80 X(U)_ Z(W)_ F_

Explanation

Explanation of

X, Z Coordinate values of end point (point C) in absolute command

U, W Coordinate values of end point (point C) with reference to the initial point (point A)

in incremental command

F Feedrate

Internal

Internal Diameter/Outer

Straight

Straight Cutting

+X

Diameter/Outer

Diameter/Outer Diameter

Cutting

Cutting Cycle

of

of the

Cycle

the

parameters

the

parameters

the parameters

parameters

z

D

3R

Diameter

Diameter Cutting

w

4R

Cutting

Cutting Cycle

Cycle

Cycle (G80)

1R

A

(G80)

u/2

2F

BC

x/2

+Z

Rapid traverse speed

Feed rate

Figure 9 . 1 Straight cutting cycle (G80)

Function

This command can implement the straight cutting. The machining path is

A → B → C → D → A.

84

A: Initial point B: Starting point of cutting C: End point of cutting D: Retraction point

�

Taper

�

Taper

�

� Taper

Taper Cutting

Programming

Cutting

Cutting Cycle

Cycle

G80 X(U)_ Z(W)_ I_ F_

9. Functions to Simplify Programming

Explanation

Explanation of

of

the

parameters

of

the

parameters

of the

the parameters

parameters

X, Z Coordinate values of end point (point C) in absolute command

U, W Coordinate values of end point (point C) with reference to the initial point (point A)

in incremental command

I The radius difference between starting point B and end point C. It is negative, if

the radius of point B is less than the radius of point C. Otherwise, it is positive.

F Feedrate

+X

z w

D

3R

C

x/2

4R

2F

A

1R

B

u/2

i

+Z

A: Initial point B: Starting point of cutting C: End point of cutting D: Retraction point

Function

Rapid traverse speed

Feed rate

Figure 9 . 2 T aper Cutting Cycle (G80)

This command can implement the taper cutting. The machining path is A → B → C → D → A.

85

9. Functions to Simplify Programming

50

Φ

35

Φ

30

Example

Example 1

1

U se G80 command to machine the cylindrical part in two steps – rough machin ing and finish

machin ing .

Figure 9 . 3 Internal Diameter/Outer Diameter Cutting Cycle – Example 1

%3320

N1 T0101

N2 M03 S460

N3 G00 X90Z20

N4 X40 Z3

N5 G80 X31 Z-50 F100

N6 G80 X30 Z-50 F80

N7 G00X90 Z20

N8 M30

86

9. Functions to Simplify Programming

Example

Example 2

U se G80 command to machine the tapered part in two steps – rough machin ing and finish

machin ing .

2

Figure 9 . 4 Internal Diameter/Outer Diameter Cutting Cycle – Example 2

%3321

N1 T0101

N2 G00 X100Z40 M03 S460

N3 G00 X40 Z5

N4 G80 X31 Z-50 I-2.2 F100

N5 G00 X100 Z40

N6 T0202

Φ30

Φ26

Φ35

50

N7 G00 X40 Z5

N8 G80 X30 Z-50 I-2.2 F80

N9 G00 X100 Z40

N10 M05

N11 M30

87

9. Functions to Simplify Programming

Example

Example 3

U se G80 command to machine the tapered part in two steps – rough machin ing and finish

machin ing .

3

2 × 45 °

Figure 9 . 5 Internal Diameter/Outer Diameter Cutting Cycle – Example 3

%3322

N1 T0101

N2 M03 S460

N3 G00 X100 Z40

N4 X40 Z3

N5 G80 X31 Z-50 F100

N6 G80 X25 Z-20

N7 G80 X29 Z-4 I-7 F100

N8 G00 X100 Z40

N9 T0202

30

Φ

28

Φ

24

Φ

20

50

35

Φ

N10 G00 X100 Z40

N11 G00 X14 Z3

N12 G01 X24 Z-2 F80

N13 Z-20

N14 X28

N15 X30 Z-50

N16 G00 X36

N17 X80 Z10

N18 M05

N19 M30

88

9. Functions to Simplify Programming

9.1.2

9.1.2 End

�

� Face

Programming

G81 X(U)_ Z(W)_ F_

Explanation

Explanation of

X, Z Coordinate values of end point (point C) in absolute command

U, W Coordinate values of end point (point C) with reference to the initial point (point A)

in incremental command

F Feedrate

End

End Face

Face

Cutting

Face

Cutting

Face Cutting

Cutting Cycle

of

of the

Face

Face Turning

Turning

Turning Cycle

Cycle

the

parameters

the

parameters

the parameters

parameters

+X

Cycle

Cycle (G81)

B

2F 4R

(G81)

w

1R

A

u/2

3F

C

z

Rapid traverse speed

Feed rate

Figure 9 . 6 Face Cutting Cycle (G81)

Function

This command can implement the end face cutting. The machining path is

A → B → C → D → A.

89

D

x/2

+Z

A: Initial point B: Starting point of cutting C: End point of cutting D: Retraction point

�

Taper

�

Taper

�

� Taper

Taper Face

Programming

Face

Cutting

Face

Cutting

Face Cutting

Cutting Cycle

G81 X(U)_ Z(W)_ K_ F_

Cycle

9. Functions to Simplify Programming

Explanation

Explanation of

of

the

parameters

of

the

parameters

of the

the parameters

parameters

X, Z Coordinate values of end point (point C) in absolute command

U, W Coordinate values of end point (point C) with reference to the initial point (point A)

in incremental command

K The distance on Z axis of the starting point (point B) with reference to the end

point (point C). It is negative, if the value of point C on Z axis is more than point B’s. It is

positive, if the value of point C on Z axis is less than point B’s.

F Feedrate

+X

B

2F

w

1R

A

4R

u/2

3F

D

x/2

+Z

A: Initial point B: Starting point of cutting C: End point of cutting D: Retraction point

Function

k

z

Rapid traverse speed

Feedrate

Figure 9 . 7 T aper Face Cutting Cycle (G81)

C

This command can implement the taper face cutting. The machining path is

A → B → C → D → A.

90

9. Functions to Simplify Programming

Example

Use G81 to program. The dashed line stands for the roughcast .

33.5

33.5 3

3

8

25

55

Φ

Figure 9 . 8 End Face Turning Cycle (G81)

25

Φ

%3323

N1 T0101

N2 G00 X60 Z45

N3 M03 S460

N4 G81 X25 Z31.5 K-3.5 F100

N5 X25 Z29.5 K-3.5

N6 X25 Z27.5 K-3.5

N7 X25 Z25.5 K-3.5

N8 M05

N9 M30

91

9. Functions to Simplify Programming

9.1.3

9.1.3 Thread

�

� Cylindrical

Programming

G82 X (U) _ Z (W) _ R_ E_ C_ P_ F (J) _

Explanation

Explanation of

X, Z Coordinate values of end point (point C) in absolute command

U, W Coordinate values of end point (point C) with reference to the initial point (point A)

in incremental command

R, E Coordinate value of retraction amount with reference to the end point (point C) in

incremental command.

C The number of thread head. It is single thread when C is 0 or 1.

P Start point offset. It is used for multiple threads.

F Thread lead per revolution

J Thread lead in inch measurement

Thread

Thread Cutting

Cylindrical

Cylindrical Thread

Thread

Thread Cutting

of

the

of

the

of the

the parameters

Cutting

Cutting Cycle

parameters

Cycle

Cycle (G82)

Cutting

Cutting Cycle

Cycle

(G82)

+ X

e

x/2

Figure 9 . 9 Cylindrical Thread Cutting Cycle (G82)

F

unction

F

unction

F

F unction

unction

This command can implement the cylindrical thread cutting. The machining path is

A → B → C → D → A. Moreover, this command is same as G32 (Thread cutting with constant

lead).

z

D

3R

C

r

w

4R A

2F

L

1R

u/2

B

+Z

92

�

Taper

�

Taper

�

� Taper

Taper Thread

Programming

G82 X (U) _ Z (W) _ I_ R_ E_ C_ P_ F (J) _

Thread

Thread Cutting

Cutting

Cutting Cycle

Cycle

9. Functions to Simplify Programming

Explanation

Explanation of

of

the

parameters

of

the

parameters

of the

the parameters

parameters

X, Z Coordinate values of end point (point C) in absolute command

U, W Coordinate values of end point (point C) with reference to the initial point (point A)

in incremental command

I The radius difference between starting point B and end point C. It is negative, if

the radius of point B is less than the radius of point C. Otherwise, it is positive.

R, E Coordinate value of retraction amount with reference to the end point (point C) in

incremental command.

C The number of thread head. It is single thread when C is 0 or 1.

P Start point offset. It is used for multiple threads.

F Thread lead per revolution

J Thread lead in inch measurement

+X

e

x/2

z

D

3R

C

r

w

4R

A

1R

2F

u/2

B

i

+Z

L

Figure 9 . 10 Taper Thread Cutting Cycle (G82)

F

unction

F

unction

F

F unction

unction

This command can implement the taper thread cutting. The machining path is

A → B → C → D → A.

93

9. Functions to Simplify Programming

Example

Use G82 command to program. The screw’s pitch is 1.5, and the number of thread head is 2.

100

80

30

30 Φ 30

Φ

Figure 9 .11Thread Cutting Cycle - Example

%3324

N1 G54 G00 X35 Z104

N2 M03 S300

N3 G82 X29.2 Z18.5 C2 P180 F3

N4 X28.6 Z18.5 C2 P180 F3

N5 X28.2 Z18.5 C2 P180 F3

N6 X28.04 Z18.5 C2 P180 F3

N7 M30

94

9. Functions to Simplify Programming

9.1.4

9.1.4 End

Programming

G74 Z(W)_ R (e) Q ( △ K) F_

Explanation

Explanation of

Z Coordinate value on Z axis of the end point in absolute command

W Coordinate value on Z axis of the end point with reference to the starting point in

incremental command

R Retraction amount(e) for each feed. It must be absolute value.

Q Depth of drilling( △ K) for each feed. It must be absolute value.

F Feedrate

End

Face

End

Face

End Face

Face Peck

of

the

of

the

of the

the parameters

Peck

Peck Drilling

parameters

Drilling

Drilling Cycle

Cycle

Cycle (G74)

W

(G74)

Z

△ K

Figure 9 . 12 End Face Peck Drilling Cycle (G74)

Function

This command can drill a hole on end face.

e

X

95

Example

Use G74 to drill a hole on a workpiece.

Figure 9 . 13 End Face Peck Drilling Cycle – Example

%1234

T0101

M03S500

G01 X0 Z10

G74 Z-60R1Q5F1000

9. Functions to Simplify Programming

10

60

Z

X

M30

96

Wuhan Huazhong Numerical Control Co., Ltd HNC-18xp/T, HNC-19iT v4.0, HNC-21T, HNC-22T, HNC-18iT Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Preface

General

CNC Programming

Interpolation

Circular Interpolation

Thread Cutting

Feed Function

Coordinate System

Reference Point

Absolute Commands

Incremental Commands

Diameter/Radius Programming

Tool Function

Tool Selection

Tool Offset

Miscellaneous Function

Program Configuration

Interpolation Functions

Positioning (G00)

Chamfering (G01)

Rounding (G01)

Tapping (G34)

Feed Function

Dwell (G04)

Coordinate System

Tool Function

Miscellaneous Function

CNC M-Function

Canned Cycles