Content      ..     3      4      5      6     ..

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

+X

△z

r

B

●

A

1

△d

r

△d

A’ _●

△x/2

+Z

Figure 9.16 Stock Removal in Turning without Groove (G71)

Function

This command can do a stock removal in facing without groove. The machining path

is A→A'→B

Note

1) G00 or G01 must be used in the finishing program - between P(ns) and Q(nf).

Otherwise, there is an alarm message.

2) G71 cannot be used in MDI mode.

3) G98 and G99 cannot used in the finishing program - between P(ns) and

Q(nf).

4) The direction of △ x and △ z is shown in the following figure.

A

B

B

A

A

B B

A

X(-) Z(-)

X(+) Z(+)

X(-)Z(+)

X(+) Z(-)

+Z

+X

A′

A′

A′

A′

A′

A′

A

′

A

′

+Z

+X

X(-) Z(-)

X(-)Z(+)

X(+) Z(-)

X(+) Z(+)

A

A

A

B

B

A

B

B

Figure 9.17 Direction of the finishing allowance in G71

116

Example 1

The initial point A is (46, 3). The depth of cut is 1.5mm (radius designation). The

retraction amount is 1mm. The finishing allowance in the X direction is 0.6mm, and

the finishing allowance in the Z direction is 0.1mm. The dashed line stands for the

original part.

82

62

52

35

25

R7

R5

2×45°

Figure 9.18 Outer Diameter Removal without Groove - Example

%3325

T0101

N1 G00 X80 Z80

N2 M03 S400

N3 G01 X46 Z3 F100

N4 G71U1.5R1P5Q13X0.6 Z0.1

N5 G00 X0

N6 G01 X10 Z-2

N7 Z-20

N8 G02 U10 W-5 R5

N9 G01 W-10

N10 G03 U14 W-7 R7

N11 G01 Z-52

N12 U10 W-10

N13 W-20

N14 X50

N15 G00 X80 Z80

N16 M05

N17 M30

117

Example 2

The initial point A is (6, 3). The depth of cut is 1.5mm (radius designation). The

retraction amount is 1mm. The finishing allowance in the X direction is 0.6mm, and

the finishing allowance in the Z direction is 0.1mm. The dashed line stands for the

original part.

82

62

52

35

25

R5

R7

2×45

°

Figure 9.19 Internal Diameter Removal without Groove - Example

%3326

N1 T0101

N2 G00 X80 Z80

N3 M03 S400

N4 X6 Z5

G71U1R1P8Q16X-0.6Z0.1 F100

N5 G00 X80 Z80

N6 T0202

N7 G00 G41X6 Z5

N8 G00 X44

N9 G01 Z-20 F80

N10 U-10 W-10

N11 W-10

N12 G03 U-14 W-7 R7

N13 G01 W-10

N14 G02 U-10 W-5 R5

N15 G01 Z-80

N16 U-4 W-2

N17 G40 X4

N18 G00 Z80

N19 X80

N20 M30

118

z Stock Removal in Turning with Groove

Programming

G71 U(△ d) R(r) P(ns) Q(nf) E(e) F(f) S(s) T(t)

Explanation of the parameters

U(△ d)

the cutting depth (radius designation). The cutting direction depends

on the direction of AA’.

R(r)

Retraction amount

P(ns)

Sequence number of the first block for the finishing program.

Q(nf)

Sequence number of the last block for the finishing program.

E(e)

Distance and direction of finishing allowance on X axis. It is positive

when it is outer diameter cutting. It is negative when it is internal diameter cutting.

F(f), S(s), T(t)

F, S, T function are only effective for the rough machining, i.e, it is

not effective in the finishing program - between P(ns) and Q(nf).

B

¹ A

r

△d

B’

e

A’

Figure 9.20 Stock Removal in Turning with Groove (G71)

Function

This command can do a stock removal in facing with groove. The machining path

A→A'→B’→B.

119

Example

Use G71 to program.

61.5

10

5

32.5

17

(8)

12

2×45°

R10

R4

4

30°

Figure 9.21 Stock Removal in Turning with Groove - Example

%3327

N1 T0101

N2 G00 X80 Z100

M03 S400

N3 G00 X42 Z3

N4G71U1R1P8Q19E0.3F100

N5 G00 X80 Z100

N6 T0202

N7 G00 G42 X42 Z3

N8 G00 X10

N9 G01 X20 Z-2 F80

N10 Z-8

N11 G02 X28 Z-12 R4

N12 G01 Z-17

N13 U-10 W-5

N14 W-8

N15 U8.66 W-2.5

N16 Z-37.5

N17 G02 X30.66 W-14 R10

N18 G01 W-10

N19 X40

N20 G00 G40 X80 Z100

N21 M30

120

9.2.2 Stock Removal in Facing (G72)

Programming

G72 W(Δd) R(r) P(ns) Q(nf) X(Δx) Z(Δz) F(f) S(s) T(t)

Explanation of the parameters

W(△ d)

the cutting depth (radius designation). The cutting direction depends

on the direction of AA’.

R(r)

Retraction amount

P(ns)

Sequence number of the first block for the finishing program.

Q(nf)

Sequence number of the last block for the finishing program.

X(△ x)

Distance and direction of finishing allowance on X axis

Z(△ z)

Distance and direction of finishing allowance on Z axis

F(f), S(s), T(t)

F, S, T function are only effective for the rough machining, i.e, it is

not effective in the finishing program - between P(ns) and Q(nf).

△z

△d

△d

+X

A’

A

r

r

△x/2

B

+Z

O

Figure 9.22 Stock Removal in Facing (G72)

Function

This command can do a stock removal in facing. The machining path is A→A'→B

121

Note

1) G00 or G01 must be used in the finishing program - between P(ns) and Q(nf).

Otherwise, there is an alarm message.

2) G72 cannot be used in MDI mode.

3) G98 and G99 cannot used in the finishing program - between P(ns) and

Q(nf).

4) The direction of △ x and △ z is shown in the following figure.

A

A

A

A'

A'

A

A'

A'

X(+) Z(+)

X(+) Z(-)

X(-) Z(+)

X(-) Z(-)

X

Z

B

B

B

B

B

B

B

B

Z

X

X(-) Z(-)

X(-) Z(+)

X(+) Z(-)

X(+) Z(+)

A

A

A'

A'

A

A'

A'

A

Figure 9.23 Direction of the finishing allowance in G72

122

Example 1

Use G72 to program. The initial point A is (80, 1). The depth of cutting is 1.2mm. The

retraction amount is 1mm. The finishing allowance in the X direction is 0.2mm, and

the finishing allowance in the Z direction is 0.5mm. The dashed line stands for the

original part.

60

50

40

26

15

R4

2×45°

R2

Figure 9.24 Outer Diameter Removal in Facing - Example

%3328

N1 T0101

N2 G00 X100 Z80

N3 M03 S400

N4 X80 Z1

N5 G72W1.2R1P8Q17X0.2Z0.5F100

N6 G00 X100 Z80

N7 G42 X80 Z1

N8 G00 Z-53

N9 G01 X54 Z-40 F80

N10 Z-30

N11 G02 U-8 W4 R4

N12 G01 X30

N13 Z-15

N14 U-16

N15 G03 U-4 W2 R2

N16 G01 Z-2

N17 U-6 W3

N18 G00 X50

N19 G40 X100 Z80

N20 M30

123

Example 2

Use G72 to program. The initial point A is (80, 1). The depth of cutting is 1.2mm. The

retraction amount is 1mm. The finishing allowance in the X direction is 0.2mm, and

the finishing allowance in the Z direction is 0.5mm. The dashed line stands for the

original part.

60

11

34

10

10

R2

R4

2×45°

Figure 9.25 Internal Diameter Removal in Facing - Example

%3329

N1 T0101

N2 G00 X100 Z80

N3 M03 S400

N4 G00 X6 Z3

N5 G72W1.2R1P5Q15X-0.2Z0.5F100

N6 G00 Z-61

N7 G01 U6 W3 F80

N8 W10

N9 G03 U4 W2 R2

N10 G01 X30

N11 Z-34

N12 X46

N13 G02 U8 W4 R4

N14 G01 Z-20

N15 U20 W10

N16 Z3

N17 G00 X100 Z80

N18 M30

124

9.2.3 Pattern Repeating (G73)

Programming

G73 U(ΔI) W(ΔK) R(r) P(ns) Q(nf) X(Δx) Z(Δz) F(f) S(s) T(t)

Explanation of the parameters

U(△ I)

distance and direction of total roughing allowance in the X direction

(radius designation).

W(△ K)

distance and direction of total roughing allowance in the X direction

(radius designation)

R(r)

Repeated times of cutting

P(ns)

Sequence number of the first block for the finishing program.

Q(nf)

Sequence number of the last block for the finishing program.

X(△ x)

Distance and direction of finishing allowance on X axis

Z(△ z)

Distance and direction of finishing allowance on Z axis

F(f), S(s), T(t)

F, S, T function are only effective for the rough machining, i.e, it is

not effective in the finishing program - between P(ns) and Q(nf).

Δk+Δz

A

1

Δz

+X

ΔI+Δx/2

A

Δx/2

●

B



A

1

A_●

’

Δz Δx/2

O

Figure 9.26 Pattern Repeating (G73)

125

Example

Use G73 to program. The initial point A is (60, 5). The total roughing allowance on X

and Z axis are 3mm, 0.9mm, respectively. The times of rough cutting is 3. The

finishing allowance on X and Z axis are

0.6mm,

0.1mm respectively. The

dash-dot-line is the part’s blank.

62

52

35

25

R7

R5

2×45°

Figure 9.27 Pattern Repeating - Example

%3330

N1 T0101

N2 G00 X80 Z80

N3 M03 S400

N4 G00 X60 Z5

N5 G73U3W0.9R3P5Q13X0.6Z0.1F120

N6 G00 X0 Z3

N7 G01 U10 Z-2 F80

N8 Z-20

N9 G02 U10 W-5 R5

N10 G01 Z-35

N11 G03 U14 W-7 R7

N12 G01 Z-52

N13 U10 W-10

N14 U10

N15 G00 X80 Z80

N16 M30

127

9.2.4 Multiple Thread Cutting Cycle (G76)

Programming

G76 C(c) R(r) E(e) A(a) X(x) Z(z) I(i) K(k) U(d) V(Δdmin) Q(Δd) P(p) F(L) O

Explanation of the parameters

C(c)

Repetitive count in finishing (1~99), modal value

R(r)

Retraction amount on Z axis (00~99), modal value

E(e)

Retraction amount on X axis (00~99), modal value

A(a)

Angle of tool tip (two-digit number), modal value. It must be more than

10° and less than 80°.

X, Z

Coordinate value of end point (point C) in absolute command.

x, z

Coordinate value of end point (point C) with reference to the initial point

(point A) in incremental command

I(i)

Difference of thread radius. If i=0, it is straight thread cutting.

K(k)

Height of thread. This value is specified by the radius value on X axis.

U(d)

The finishing allowance (radius) (Figure 9.29).

V(Δdmin) The minimum cutting depth (radius). The cutting depth is Δdmin when

the cutting depth (d

n d

n1_{) is less than Δdmin (Figure 9.29).}

Q(Δd)

Depth of cutting at the first cut (radius)

P(p)

spindle angle of spindle reference pulse to the start point of cutting

F(L)

Thread lead (same as G32)

O

Acceleration constant of thread cutting retraction. When it is set to zero,

the acceleartion is maximum. The more this value is, the acceleration time is longer,

and the retraction is longer. Q must be set to zero or more than zero. O is modal code.

+X

A

D

(R)

(R)

u/2

(R)

(F)

e

d

K

i

C

r

B

x/2

z

w

+Z

Figure 9.28 Multiple Thread Cutting Cycle (G76)

128

Angle of tool tip

a

Δd

1st

k

2nd

Δd

n

d

nth

Figure 9.29 The depth of cutting

Function

G76 command can do the multiple thread cutting. The machining path is

A→B→C→D.

Note

1) In G76, X(x) and Z(z) realize cycle machining. When incremental

programming, note the sign of x and w (determined by the direction of tool

path of AC and CD).

2) G76 cycle do singal-side cutting to reduce the stress of tool point. The cutting

depth in 1st cut is Δd, the cutting depth in nth cut is

d

n . The bite of each

d（

n



n

1

）

cycle is

3) The cutting speed of CD path is specified by feedrate. And the other paths

are specified by rapid traverse speed.

129

Example

Use G76 to program. The thread is ZM60×2. Sizes in bracket is from standards.

(tan1.79=0.03125)

30

4

6

(18)

(12)

(1.79°)

Figure 9.30 Multiple Thread Cutting Cycle - Example

%3331

N1 T0101

; Change No.1 tool, set its coordiante

N2 G00 X100 Z100

; To start of program or the position of changing tool

N3 M03 S400

; Spindle CW 400r/min

N4 G00 X90 Z4

; To the position of simple cycle start

N5 G80 X61.125 Z-30 I-1.063 F80 ; Machining cone thread surface

N6 G00 X100 Z100 M05

;To the position of program start or tool change

N7 T0202

; Change No.2 tool, set its coordiante

N8 M03 S300

; Spindle CW 300r/min

N9 G00 X90 Z4

; To the positon of thread cycle start

N10 G76C2R-3E1.3A60X58.15Z-24I-0.875K1.299U0.1V0.1F2

N11 G00 X100 Z100

; Return to start or change tool position

N12 M05

; Return to start or change tool position

N13 M30

; Main program end and reset

130

10. Comprehensive Programming

10 Comprehensive Programming

10.1 Example 1

Program for the part shown in the figure. The processing condition: material: #45 steel,

or aluminum; diameter of the part is Φ54mm, length of the part is 200mm. Tool

selection: number 1 face tool is used to machine the part face, number 2 face

cylindrical tool is used to rough turning the contour, number 3 face cylindrical tool is

used to finish turning the contour, and number 4 cylindrical triple screw is used to

machine the thread whose lead is 3mm, pitch is 1mm.

133

50

10

12

20

33

11

10

26

R15

2×45°

R2

R25

R6

1×45°

24

Figure 10.1 Comprehensive Program Example 1

%3365

N1 T0101

N2 M03 S500

N3 G00 X100 Z80

N4 G00 X60 Z5

N5 G81 X0 Z1.5 F100

N6 G81 X0 Z0

N7 G00 X100 Z80

N8 T0202

N9 G00 X60 Z3

N10 G80 X52.6 Z-133 F100

N11 G01 X54

N12 G71 U1 R1 P16 Q32 E0.3

131

10. Comprehensive Programming

10.2 Example 2

Program for the part shown in the figure. The processing condition: material: #45 steel,

or aluminum; diameter of the part is Φ26mm, length of the part is 70mm. Tool

selection: number 1 cylindrical tool is used to rough turning the contour, number 2

cylindrical tool is used to finish turning the contour, number 3 cylindrical thread tool is

used to machine the thread. The pitch is 2mm. At last, number 4 parting-off tool is

used to cut off the part.

2×45°

R10

R10

18

38

45

Figure 10.2 Comprehensive Programming Example 2

%3368

N1 T0101

N2 M03 S600

N3 G00 X100 Z30

N4 G00 X27 Z3

N5 G71 U1 R1 P9 Q E0.2 F100

N6 G00 X100 Z30

N7 T0202

N8 G00 G41 X27 Z3

N9 G00 X14 Z3

N10 G01 X24 Z-2 F80

N11 Z-18

N12 G02 X20 Z-24 R10

N13 G01 Z-31.39

N14 G02 X25 W-6.61 R10

N15 G01 Z-45

133

10. Comprehensive Programming

10.3 Example 3

Program for the tapered thread ZG2″ shown in the figure. According to the standard,

the pitch is 2.309mm(25.4/11), the thread height is 1.479mm. Other sizes are shown

in the figure. The depth of cut at each time is separately(diameter designation) 1mm,

0.7 mm, 0.6mm , 0.4mm and 0.26mm, and the angle of tool tip is 55° (tan1.79=0.031).

40

4

4

(26)

(16)

(1.79°)

Figure 10.3 Comprehensive Programming Example 3

%3366

N1 T0101

N2 M03 S300

N3 G00 X100 Z100

N4 X90 Z4

N5 G80 X61.117 Z-40 I-1.375 F80

N6 G00 X100 Z100

N7 T0202

N8 G00 X90 Z4

N9 G82 X59.494 Z-30 I-1.063 F2.31

N10 G82 X58.794 Z-30 I-1.063 F2.31

N11 G82 X58.194 Z-30 I-1.063 F2.31

N12 G82 X57.794 Z-30 I-1.063 F2.31

N13 G82 X57.534 Z-30 I-1.063 F2.31

N14 G00 X100 Z100

N15 M30

135

10. Comprehensive Programming

10.4 Example 4

Program for the M40×2 inner thread shown in the figure. According to the standard,

the pitch is 2.309mm(25.4/11), thread height is 1.299mm. Other sizes are shown in

the figure. The depth of cut at each time(diameter designation) is 0.9mm, 0.6mm,

0.6mm, 0.4mm and 0.1mm. The angle of tool tip is 60°.

38

30

Figure 10.4 Comprehensive Programming Example 4

%3367

N1 T0101

N2 M03 S300

N3 G00 X100 Z100

N4 X20 Z4

N5 G80 X37.35 Z-38 F80

N6 G00 X100 Z100

N7 T0202

N8 G00 X20 Z4

N9 G82 X38.25 Z-30 R-4 E-1.3 F2

N10 G82 X38.85 Z-30 R-4 E-1.3 F2

N11 G82 X39.45 Z-30 R-4 E-1.3 F2

N12 G82 X39.85 Z-30 R-4 E-1.3 F2

N13 G82 X39.95 Z-30 R-4 E-1.3 F2

N14 G00 X100 Z100

N15 M30

136

11. Custom Macro

11.1 Variables

Format and Explanation

#_

Variable is composed of a number sign (#) and a number.

Example

#1

#1=#2+100

11.1.1 Type of Variables

There are four types of variables.

Table 11-1 Type of Variables

Variable

Type of variables

Function

number

They are used in a

macro

#0~#49

Local variables

program.

They can be shared

among

#50~#199

Common variables

different macro programs.

#200~#249

0 layers local variables

#250~#299

1 layers local variables

#300~#349

2 layers local variables

#350~#399

3 layers local variables

#400~#449

4 layers local variables

#450~#499

5 layers local variables

#500~#549

6 layers local variables

#550~#599

7 layers local variables

They are used to read and write

#600~

System variables

NC data.

Note:

1) The operator can only use the #0~#599 local variables for programming.

2) Variables after #599 can only be used by the system programmer for reference.

138

Content      ..     3      4      5      6     ..