Content      ..      1       2         ..

Century Star Turning CNC System. Programming Guide (V3.5 April, 2015) - page 1

1. General

1. Read drawing

X







40

150

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

4. Manufacture a part

X

Z

Figure 1.1 The workflow of operation of CNC machine tool

3

1. General

1.2 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 Linear Interpolation

There are two kinds of linear interpolation:

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

X

Z

Figure 1.2 Linear Interpolation (1)

2) Tool movement along the taper line

X

Z

Figure 1.3 Linear Interpolation (2)

4

1. General

1.2.2 Circular Interpolation

Figure 1.4 shows a tool movement along an arc.

X

Z

Figure 1.4 Circular Interpolation

Note:

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

1.2.3 Thread Cutting

There are several kinds of threads: cylindrical, taper or face threads. To cut threads on

a workpiece, the tool is moved with spindle rotation synchronously.

Figure 1.5 Thread Cutting

5

1. General

1.3 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

feedrate.

-

Feed function refers to an operation to control the feedrate.

Tool

Chuck

Figure 1.6 Feed Function

For example:

F2.0

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

6

1. General

1.4 Coordinate System

1.4.1 Reference Point

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.

Tool post

Chuck

Reference

position

Figure 1.7 Reference Point

There are two ways to move to the 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

1.4.2 Machine Coordinate 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 correspondently. Due to different types of turning

machine, the axis direction can be decided by following the rule - “three finger rule” of

the right hand.

+Y

+B

+Z＇

+X +Y +Z

+Y

+X＇

+X

+C

+A

+Z

+A +B

+Y＇

+C

+X

+Z

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

-

The index points the Y axis. Y axis is usually a virtual axis.

-

The 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 Workpiece Coordinate System

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

workpiece coordinate system.

Y+

Z-

X+

90°

Figure 1.10 Workpiece Coordinate System

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

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

X

P4

P3 P2

Φ60

P1

Φ40

Φ25

7.5

Z

15

25

35

Figure 1.11 Example of defining points on workpiece coordinate system

9

1. General

1.4.4 Setting Two Coordinate Systems at the Same Position

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

1)

The coordinate zero point is set at chuck face

X

X









40

150

Figure 1.12 The coordinate zero point set at chuck face

2)

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

X

X









30

80

100

Figure 1.13 The coordinate zero point set at the end face of workpiece

10

1. General

1.4.5 Absolute Commands

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

coordinate system”.

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

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

X

P4

P3 P2

Φ60

P1

Φ40

Φ25

7.5

Z

15

25

35

Figure 1.14 Absolute Dimension

11

1. General

1.4.6 Incremental Commands

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:

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

X

P4

P3 P2

Φ60

P1

Φ40

Φ25

10

7.5

7.5

Z

Figure 1.15 Incremental Dimension

12

1. General

1.4.7 Diameter/Radius 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

X

B

A





Z

60

80

Figure 1.16 Diameter Programming

Example: Describe the points by radius programming.

A corresponds to X15 Z80

B corresponds to X20 Z60

X

B

A





Z

60

80

Figure 1.17 Radius Programming

13

1. General

1.6 Tool Function

1.6.1 Tool Selection

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

performed. As it is shown in Figure 1.18, a number is assigned to each tool. Then this

number is used in the program to specify that the corresponding tool is selected.

Tool number

01

06

02

05

Tool post

03

04

Figure 1.18 Tool Selection

1.6.2 Tool Offset

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

machining a workpiece, the tool path is affected by the tool geometry.

Rough

Thread

Standard

cutting

Finishing Grooving cutting

tool

tool

tool

tool

tool

workpiece

Figure 1.19 Tool Offset

15

1. General

z 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 1.20, 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=Tool tip

R=Radius

S=Cutting edge center

L2

Figure 1.20 Tool Length Compensation

z Tool Radius Compensation

Figure 1.21 shows the imaginary tool nose as a start position when writing a program.

P

Tool nose radius center

Imaginary tool nose

Figure 1.21 The imaginary tool nose

16

1. General

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

Figure 1.22 and Figure 1.23 show the relation between the tool and the imaginary tool

tip.

4

8

3

●

●

●

Z

5

0

9

7

●

●

●

X

●

●

●

1

6

2

● Imaginary tool nose

+ Tool nose radius center

Figure 1.22 The direction of imaginary tool nose (1)

1

6

2

●

●

●

Z

5

0

9

7

●

●

●

X

●

●

●

4

8

3

● Imaginary tool nose

+ Tool nose radius center

Figure 1.23 The direction of imaginary tool nose (2)

17

1. General

1.8 Program Configuration

1.8.1 Structure of an NC Program

As it is shown in Figure 1.24, an NC program consists of a sequence of NC blocks.

Each block is one of machining steps. Commands in each block are the instruction.

Program

Program number

%1000

N01 G91 G00 X50 Y60

N10 G01 X100 Y500 F150 S300 M03

Program block

N

;COMMENT

N200

M30

Command character

Figure 1.24 Structure of an NC Program

-

Format of program name

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

numbers).

-

Format of program number

The 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 block

N..

G..

X…Y… F..

M..

S..

Spindle function

Miscellaneous function

Feed Function

Coordinate - Dimension word

Preparatory function

Program block number

Figure 1.25 Structure of Block

19

1. General

-

Format of end of program

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.

1.8.2 Main Program and Subprogram

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 program

Subprogram

Instruction 1

Instruction 1

Instruction 2

Instruction 2

Follow the direction

ofthe subprogram

Instruction n

Instruction n+1

Return to the main program

Figure 1.26 Main program and subprogram

Note:

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

program codes.

20

2. Preparatory Function

2 Preparatory Function (G code)

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

Table 2-1 Type of G code

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_

Z_

G00 is effective in this range

X_

G01Z_

21

2. Preparatory Function

2.1 G code List

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

Table 2-2 G code list

G code

Group

Function

G00

Positioning (Rapid traverse)

◣G01

Linear interpolation (Cutting feed)

01

G02

Circular interpolation CW

G03

Circular interpolation CCW

G04

00

Dwell

G20

Input in inch

08

◣G21

Input in mm

G28

Reference point return

00

G29

Auto return from reference point

G32

Thread cutting with constant lead

01

G34

Tapping

◣G36

Diameter programming

17

G37

Radius programming

◣G40

Tool nose radius compensation cancel

G41

09

Tool nose radius compensation on the left

G42

Tool nose radius compensation on the right

G46

16

Setting the limit of spindle speed

◣G50

Canceling the workpiece’s origin movement

04

G51

Moving the origin of workpiece coordinate system

G53

00

Selecting a machine coordinate system

◣G54

G55

G56

11

Setting a workpiece coordinate system

G57

G58

G59

22

2. Preparatory

Function

G71

Stock Removal in Turning

G72

Stock Removal in Facing

G73

Pattern repeating

G74

Front drilling cycle

G75

06

Side drilling cycle

G76

Multiple thread cutting cycle

G80

Internal diameter/Outer diameter cutting cycle

G81

End face turning cycle

G82

Thread cutting cycle

◣G90

Absolute programming

13

G91

Incremental programming

G92

00

Setting a coordinate system

◣G94

Feedrate per minute

14

G95

Feedrate per revolution

G96

Constant cutting speed starts

16

◣G97

Constant cutting speed is cancelled

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.

23

3. Interpolation Function

3.1 Positioning (G00)

Programming

G00 X(U)… Z(W)…

Explanation of the parameters

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). If 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.

X

P1

P2

M

W

Z

Figure 3.1 Positioning (Rapid Traverse)

Absolute programming:

G00 X10 Z20

Incremental programming:

G00 U30 W70

25

Content      ..      1       2         ..

//////////////////////