Content      ..     2      3      4      5     ..

Century Star Turning CNC System. Programming Guide (V3.5 April, 2015) - page 4

7. Tool Function

Standard offset is the directed distance of the workpiece origin relative to the standard

tool position on the cutter frame.

Standard tool

Non-standard Tool

Offset compensation on axis Z

B

△x

A

△z

Offset compensation on axis Z

Figure 7.3 Incremental tool offset compensation

If there is tool setting gauge, the following steps are for the measurement of relative

tool offset:

1) Move the standard tool to the cross center of tool setting gauge.

2) Press MDI function key, and set the current position of tool as the relative

origin.

3) Change a tool and move the other tool to the cross center of tool setting

gauge. The shown value is the offset relative to the standard tool.

If there is no tool setting gauge, the following steps are for the measurement of

relative tool offset:

1) Press “MDI” function key, and set the current position of axis Z as the relative

origin in the trial face cutting of the workpiece. (no movement on axis Z before

setting zero).

2) Press “MDI” function key, and set the current position of axis X as the relative

origin in the trial cylindrical surface cutting of the workpiece (no movement on

axis X before setting zero). The standard tool has set a reference point on the

workpiece. When the standard tool is at the reference point, it is the position

of the relative origin.

3) Change a tool and move the another tool to the reference point of workpiece.

The shown value is the offset relative to the standard tool.

The system would automatically calculate the distance of the workpiece origin relative

to the tool position, and compare with the standard tool’s value to get the tool offset

relative to the standard tool’s, when the cutter frame is at the machine origin. The

procedures are as followed:

86

7. Tool Function

Machine origin

Zw

ΔX/2

D_M/2

ZM

ΔZ

Workpiece

origin

Dw/2

DM′/2

ZM′

Figure 7.4 Setting the incremental tool offset compensation

1) Press “MDI->Tool Offset” function key;

2) Use the tool to cut the front face of workpiece, and input the coordinates value of

workpiece coordinates on axis Z, i.e. the length of workpiece. If the workpiece

origin is set at the front face of workpiece, input “0” (no movement on axis Z before

setting zero). The system would automatically calculate the distance of workpiece

origin relative to the tool position of standard tool, i.e. the standard tool offset on

axis Z.

3) Input the coordinate value of workpiece coordinates on axis X in the trial

cylindrical surface cutting of the workpiece, i.e. the diameter of workpiece (no

movement on axis X before setting zero). The system would automatically

calculate the distance of workpiece origin relative to the tool position of standard

tool, i.e. the standard tool offset on axis Z.

4) Press “Tool Offset->Standard Tool” to set the standard tool offset as the reference.

5) Change a tool and repeat the steps 2~3 to get the tool offset relative to the

standard’s and automatically input to the table of tool offset.

7.1.2 Tool Wear-out

There would be size error after the tool is used for a long time. Thus, the

compensation is required. This compensation and the tool offset compensation are

saved in the same address of register. The wear-out compensation is only valid for the

corresponding tool’s (including the standard tool).

87

7. Tool Function

Programming

T XX XX

Explanation of the parameters

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. “00” means the compensation is 0, i.e. compensation cancelled. The tool

compensation function validated or cancelled is implemented by controlling cutter

carriage. The tool offset number is the address number of register of tool offset

compensation. This register saves the data of offset compensation and wear-out

compensation of X-axis and Z-axis.

The offset number and tool number can be same or not, i.e. one tool can corresponds

to several tool offset number. As it is shown in Figure7.5, if there is compensation on

axis X and Z at the tool path relative to the programming path (compensation vector is

composed of the compensation on axis X and Z), the end point of tool path is the

position of end point of program plus or minus the compensation (compensation

vector) assigned by T code.

Compensation path

Compensation vector

(composed of the amount of

axis-X and axis-Z)

Programming path

Program with T code

Figure 7.5 Tool wear-out compensation

Example

As it is shown in the following figure, set the tool wear-out compensation, and then

cancel it.

88

7. Tool Function

X

100

T0202

Compensation route

G01 X50 Z100

Z200

50

X100 Z250 T0200

Programming route

M30

Z

100

200

250

89

7. Tool Function

7.2 Tool Radius Compensation (G40, G41, G42)

Programming

G40





G00

G41



 X_ Z_

G01









G

42





Explanation of the parameters

Tool nose radius compensation is specifies by G41, G42 and G40 or tool nose radius

compensation number specified by T code to add or cancel radius compensation.

G40 Tool nose radius compensation cancels

G41 Left cutter compensation (on the left of tool move direction) (Figure 7.6).

G42 Right cutter compensation (on the right of tool move direction) (Figure 7.6).

X, Z

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

compensation is activated or deactivated.

Note: G40, G41 and G42 are modal G-code.

Z

X

G42 On the right of tool

move direction

G41 On the left of tool

move direction

Z

G41 On the right of tool

move direction

X

G42 On the left of tool

move direction

Figure 7.6 Tool Radius Compensation

90

7. Tool Function

Function

NC program is generally aimed at cutting tool on a point at which the cutter location,

according to the contour of the workpiece size preparation. Turning tool cutter locus

ideal state of is the imagined cutter-tip A or arc center point O. Actually, tool nose is an

arc rather than a point. When the tool moves along an arc, it causes an error which

can be cancelled by tool nose radius compensation.

Note:

1) When G41/G42 without parameters, the compensation number representing

the tool nose radius compensation is assigned by T code. This corresponds

to the tool offset number.

2) G40, G41, and G42 must be used with G00 or G01. G02 or G03 cannot be

used.

In the register of tool radius compensation, it defines the direction of tool nose and

tool radius. The direction number of turning tool nose gives an identity of the position

relationship between CL point and tool nose circle center. There are 10 directions

from 0 to 9.

X

4

8

3

Z

0

9

5

7

1

6

2

● CL point A，+ Tool nose circle center O

1

6

2

Z

X

0

9

7

5

4

8

3

● CL point A，+ Tool nose circle center O

Figure 7.7 Position code of Tool Nose

91

7. Tool Function

Example

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

40

31

27

R15

Figure 7.8 Tool Radius Compensation

%3323

N1 T0101

(Change NO.1knife to define its coordinate)

N2 M03 S400

(Spindle:400r/min CW)

N3 G00 X40 Z5

(To the position of program start)

N4 G00 X0

(The tool moves to workpiece center)

N5 G01 G42 Z0 F60

(Add tool radius compensation, and be close to workpiece)

N6 G03 U24 W-24 R15

(Machine R15 circular block)

N7 G02 X26 Z-31 R5

(Machine R5 circular block)

N8 G01 Z-40

(MachineΦ26 excircle)

N9 G00 X30

(Withdraw from the machined surface)

N10 G40 X40 Z5

(Cancel radius compensation, and return to the program start)

N11 M30

(Spindle stop, the main program end and reset)

92

8. Miscellaneous Function

8 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.

Table 8-1 Type of M code

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.

93

8. Miscellaneous Function

8.1 M code List

The following is a list of M command.

Table 8-2 M code List

CNC

Pre/Post-M

Type of Mode

Function

M-function

function

M00

One-shot

Program stop

Post-M function

M01

One-shot

Optional stop

Post-M function

M02

One-shot

End of program

Post-M function

End of program with return

to

M30

One-shot

Post-M function

the beginning of program

M98

One-shot

Calling of subprogram

Post-M function

M99

One-shot

End of subprogram

Post-M function

PLC

Pre/Post-M

Type of Mode

Function

M-function

function

M03

Modal

Spindle forward rotation

Pre-M function

M04

Modal

Spindle reverse rotation

Pre-M function

M05

Modal

◣Spindle stop

Post-M function

M07

Modal

Number1 Coolant on

Pre-M function

M08

Modal

Number2 Coolant on

Pre-M function

M09

Modal

◣Coolant off

Post-M function

◣: default setting

94

8. Miscellaneous Function

8.2 CNC M-Function

8.2.1 Program Stop (M00)

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 modal information remains unchanged. Resuming program could be executed

by pushing “Cycle Run” button on the machine control panel.

8.2.2 Optional Stop (M01)

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.

8.2.3 End of Program (M02)

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

operational panel.

8.2.4 End of Program with return to the beginning of program

(M30)

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. To restart the program, press “Cycle Run” button

on the operational panel.

8.2.5 Counting (M64)

The system can calculate the number of machining workpiece at the end of program

with M30. It can also calculate the accumulation of machining workpiece by executing

M64. It is required to set the parameter->machine parameters->the judgment of

95

8. Miscellaneous Function

If

…

…

#1191=1

//the first part of program, it can be set to any values if necessary

else

…

…

#1191=0

//the second part of program, it can be set to any values

endif

M91

//user-defined output, the value of #1191 is assigned to *ch_user_out(0)

The code should be added in the function PLC1 of PLC program:

If(*ch_user_out(0)==1)

//if the first part of program is run

Y[0]|=0x10;

//Y0.4=1, output signal Y0.4 is valid (high level)

else

Y[0]&=~0x10;

//if the second part of program is run, Y0.4=0

8.2.7 Saving Macro (M94)

M94 is to save macro (#1300~#1399) to the files.

8.2.8 Subprogram Control (M98, M99)

z Calling a Subprogram (M98)

M98 P_ L_

P program number of the subprogram

L repeated times of subprogram

P ○○○○ L □□□□

Times of subprogram calling (1-9999)

It can be ignored, if the times is once.

Program number of subprogram (0000-9999)

If the times of calling is not input, the prefix “%”

of subprogram number can be omitted.

When inputing the times of calling, the digits of

subprogram must be four.

In Auto mode, CNC would call the subprogram specified by the parameter P after the

rest of code of program is run, when M98 is executed. The maximum times of

subprogram calling is 9999. M98 is not valid in MDI mode.

97

8. Miscellaneous Function

Note: Calling subprogram can be used with parameters. Blank space is not

allowed at the beginning of the subprogram.

z End of Subprogram (M99)

M99 indicates the end of subprogram and returns control to the main program. It is not

valid in MDI mode.

Example

R60

R8

4.923

R40

44.8

73.436

Figure 8.1 Subprogram Control - Example

%3111

(main program name)

N1 T0101

(Tool No.1)

N2 G92 X32 Z1

(coordinates setting, the position of aligning tool)

N3 G00 Z0 M03 S46

(move to the start of subprogram, spindle CW)

N4 M98 P0003 L5

(subprogram call, repeated times: 5)

N5 G36 G00 X32 Z1

(return to the position of aligning tool)

N6 M05

(spindle stop)

N7 M30

(main program ends and resets)

%0003

(subprogram name)

N1 G37 G01 U-12 F100

(radius programming, move to the start of cutting)

N2 G03 U7.385 W-4.923 R8

(R8 arc)

N3 U3.215 W-39.877 R60

(R60 arc)

N4 G02 U1.4 W-28.636 R40

(R40 arc)

N5 G00 U4

(leave the cutting surface)

N6 W73.436

(return to the beginning of cycle of axis-Z)

N7 G01 U-5 F100

(set the cutting amount of cycles)

N8 M99

(subprogram ends, return to the main program)

98

9.1 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.

9.1.1 Internal Diameter/Outer Diameter Cutting Cycle (G80)

z Straight Cutting Cycle

Programming

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

Explanation of the 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

F

Feedrate

+X

z

w

D

4R

A

3R

1R

u/2

2F

C

B

x/2

+Z

A: Initial point

Rapid traverse speed

B: Starting point of cutting

Feedrate

C: End point of cutting

D: Retraction point

Figure 9.1 Straight cutting cycle (G80)

Function

This command can implement the straight cutting. The machining

path

is

A→B→C→D→A.

101

z Taper Cutting Cycle

Programming

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

Explanation of the 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

4R

A

3R

1R

u/2

C

2F

i

x/2

B

+Z

Rapid traverse speed

A: Initial point

B: Starting point of cutting

Feedrate

C: End point of cutting

D: Retraction point

Figure 9.2 Taper Cutting Cycle (G80)

Function

This command can implement the taper cutting. The machining

path

is

A→B→C→D→A.

102

Example 1

Use G80 command to machine the cylindrical part in two steps - rough machining and

finish machining.

30

35

50

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

103

Example 2

Use G80 command to machine the tapered part in two steps - rough machining and

finish machining.







50

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

N7 G00 X40 Z5

N8 G80 X30 Z-50 I-2.2 F80

N9 G00 X100 Z40

N10 M05

N11 M30

104

Example 3

Use G80 command to machine the tapered part in two steps - rough machining and

finish machining.

2×45°

30

28

24

35

20

50

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

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

105

9.1.2 End Face Turning Cycle (G81)

z Face Cutting Cycle

Programming

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

Explanation of the 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

F

Feedrate

w

+X

B

1R

A

2F

4R

u/2

3F

D

C

x/2

+Z

z

Rapid traverse speed

A: Initial point

B: Starting point of cutting

Feedrate

C: End point of cutting

D: Retraction point

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.

106

z Taper Face Cutting Cycle

Programming

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

Explanation of the 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

w

B

1R

A

2F

4R

u/2

3F

C

D

k

x/2

z

+Z

A: Initial point

Rapid traverse speed

B: Starting point of cutting

Feedrate

C: End point of cutting

D: Retraction point

Figure 9.7 Taper Face Cutting Cycle (G81)

Function

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

A→B→C→D→A.

107

Example

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

33.5

3

8

Figure 9.8 End Face Turning Cycle (G81)

%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

108

+X

z

w

D

4R

A

3R

u/2

1R

e

2F

C

B

r

x/2

+Z

L

Figure 9.9 Cylindrical Thread Cutting Cycle (G82)

Function

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

A→B→C→D→E→A.

Note

This command is same as G32 (Thread cutting with constant lead). This cycle would

stop after the whole action is done in the state of feed hold.

z Taper Thread Cutting Cycle

Programming

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

Explanation of the 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 Retraction amount of thread cutting. R and E are vectors. R is the retraction

of axis-Z, and E is the retraction of axis-X. R and E can be omitted, and it means that

the retraction function is not required.

C

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

P

Uni-tip thread cutting, it is the spindle turning corner of spindle pulse to start

(defaule is 0). Muti-tip thread cutting, it is the spindle turning corner of start points.

F

Thread lead per revolution

J

Thread lead in inch measurement

110

Q

1)

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.

2)

When there is no Q, the set acceleration constant on each axis is used in the

retraction.

3)

R and E must be set when the retraction function is required.

4)

The retraction ratio of minor axis:major axis should not be more than “20“.

5)

Q is one-shot G code.

+X

z

w

D

4R

A

3R

u/2

1R

e

i

C

2F

x/2

r

B

+Z

L

Figure 9.10 Taper Thread Cutting Cycle (G82)

Function

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

A→B→C→D→A.

Example

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

head is 2.

1

80

Figure 9.11 Thread Cutting Cycle - Example

111

%3324

N1 G54 G00 X35 Z104

(Choose coordiante system G54, to cycle start)

N2 M03 S300

(Spindle CW 300r/min)

N3 G82 X29.2 Z18.5 C2 P180 F3 (1st thread cutting cycle,Depth 0.8mm)

N4 X28.6 Z18.5 C2 P180 F3

(2nd thread cutting cycle, Depth 0.4mm)

N5 X28.2 Z18.5 C2 P180 F3

(3rd thread cutting cycle, Depth 0.4mm)

N6 X28.04 Z18.5 C2 P180 F3

(4th thread cutting cycle, Depth 0.16mm)

N7 M30

(Spindle stop. Main system end and reset)

9.1.4 End Face Peck Drilling Cycle (G74)

Programming

G74 Z(W)_ R(e) Q(△ K) F_

Explanation of the parameters

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

W

Z

△K

e

X

Figure 9.12 End Face Peck Drilling Cycle (G74)

Function

This command can drill a hole on end face.

112

Example

Use G74 to drill a hole on a workpiece.

60

10

Z

X

Figure 9.13 End Face Peck Drilling Cycle - Example

%1234

T0101

M03S500

G01 X0 Z10

G74 Z-60R1Q5F1000

M30

9.1.5 Outer Diameter Grooving Cycle (G75)

Programming

G75 X(U)_ R(e) Q(△ K) F_

Explanation of the parameters

X

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

U

Coordinate value on X 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 grooving(△ K) for each feed. It must be absolute value.

F

Feedrate

113

Z

△K

U/2

e

X

Figure 9.14 Outer Diameter Grooving Cycle (G75)

Function

This command can be used for grooving.

Example

Use G75 to groove a hole on a workpiece.

Φ80

Z

50

X

Figure 9.15 Outer Diameter Grooving Cycle - Example

%1234

T0101

M03S500

G01 X50 Z50

G75 X10R1Q5F1000

M30

114

Content      ..     2      3      4      5     ..