Content      ..     7      8      9      10     ..

HNC-818. User Manual - page 9

12. Fixed Cycle

value.

K

The relative distance from the cutting start point B

to the end point C along the Z axis.

F

Feed speed (indicates to move at the speed

specified by F) (mm/min)

The cutting process is along the path AĺBĺCĺDĺA. See the figure

below:

w

+X

B

1R

A

2F

4R

u/2

3F

k

C

D

z

x/2

+Z

Conduct machining for the workpiece as shown in the figure below: use

Example

G81 programming; The dotted lines indicate the workpiece.

33.5

8

3

%3323

N1 T0101; Establish the coordinate system, and choose tool 1

245

12. Fixed Cycle

12.2.3 Thread Cutting Cycle (G82)

This cycle can be used for machining straight thread or conical thread.

Straight thread cutting cycle

G82 X_/U_ Z_/W_ R_ E_ C_ P_ F_

Parameter

Description

X /U Z/W

The thread end point C at the workpiece coordinate

system for absolute value programming; The relative

distance from the thread end point C to the cycle start

point A for the incremental value programming. Use U

and W to express them in the blueprint and the direction

of path 1 and 2 determines whether it is a positive or a

negative value.

R E

The retreat of tailstock for thread cutting. R and E are

vectors. R indicates the retreat along the Z axis

direction, and E indicates the retreat along the X axis

direction. A positive value indicates the retreat

towards the positive X/Z direction, while a negative

value indicates the retreat towards the negative X/Z

direction. R and E can be left blank, which indicates

that there is no tailstock retreat function.

C

The number of threads. The value 0 or 1 indicates

single thread cutting.

P

During the single thread cutting, it inidcates the spindle

rotation angle between the spindle reference pulse and

the starting point of the cutting

(default value

0);

During multi-thread cutting, it indicates the spindle

rotation angle between the cutting start points of the

adjacent thread.

F

Metric thread lead (mm/r)

247

12. Fixed Cycle

The tool moves along the path AĺBĺCĺDĺA. See the figure below:

X

z

w

D

4R

A

3R

u/2

1R

e

2F

C

B

r

x/2

+Z

L

Conical thread cutting cycle

G82 X_/U_ Z_/W_ I_ R_ E_ C_ P_ F_

Parameter

Description

X /U Z/W

The thread end point C at the workpiece coordinate

system for absolute value programming; The relative

distance from the thread end point C to the cycle start

point A for the incremental value programming. Use

U, W to express them in the blueprint and the direction

of path 1 and 2 determines whether it is a positive or a

negative value.

I

The difference of radius between thread starting point

B and the thread end C. Either in the absolute value

programming or in the incremental value

programming, the sign (+ or -) of the difference value

determines whether the value of I is positive or

negative.

R E

The retreat of tailstock for thread cutting. R and E are

vectors. R indicates the retreat along the Z axis

direction, and E indicates the retreat along the X axis

direction. R and E can be left blank, which indicates

that there is no tailstock retreat function.

C

The number of threads. The value 0 or 1 indicates

single thread cutting.

248

12. Fixed Cycle

P

During the single thread cutting, it inidcates the

spindle rotation angle between the spindle reference

pulse and the starting point of the cutting

(default

value 0); During multi-thread cutting, it indicates the

spindle rotation angle between the cutting start points

of the adjacent thread.

F

Metric thread lead (mm/r)

The tool moves along the path AĺBĺCĺDĺA.

+X

z

w

4R

D

A

3R

1R

u/2

e

i

r

C

2F

x/2

B

+Z

L

Attention

1.

If the retreat function is required, the symbol of the R or E value

("+"/"-") should be coordinated with the thread cutting direction.

Otherwise, it may damage the threads. In addition, you can specify

only the R value without specifying E, but if E is specified, R must

be specified.

2.

Similar as G32 thread cutting, in the feed hold state, this cycle can

stop the movment only after all operations specified by this cycle

are completed.

249

12. Fixed Cycle

Example

Conduct machining for the workpiece shown in the figure below with

G82 programming. The blank shape has been worded.

100

80

%3324

N1 G54 G00 X35 Z104; Select coordinate system G54, to the cycle start

point

N2 M03 S300; Rotate spindle in the CW direction at 300 r/min

N3 G82 X29.2 Z18.5 C2 P180 F3; The first cycle thread cutting with

depth 0.8 mm

N4 X28.6 Z18.5 C2 P180 F3; The second cycle thread cutting, with

depth 0.4 mm

N5 X28.2 Z18.5 C2 P180 F3; The third cycle thread cutting with depth

0.4 mm

N6 X28.04 Z18.5 C2 P180 F3; The forth cycle thread cutting with depth

0.16 mm

N7 M30; Stop spindle, end the main program, and reset

250

12. Fixed Cycle

12.2.4 End-Face Deep-Hole Drilling Cycle (G74)

This cycle is used to conduct end-face deep-hole drilling. See the figure

below:

W

Z

U

i

p

ΔK

e

X

Format

G74 X_/U_Z_/W_ Q(ΔK)_R(e)_ I(i)_P(p)_

Parameter

Description

X/U

For the absolute value programming, this value is the

coordinates of the end point at the hole bottom along

the X axis in the workpiece coordinate system; for the

incremental value programming this value is the

relative distance from the end point at the hole bottom

to the start point of the cycle. Use U to express it in

the blueprint. This value is optional.

Z/W

For the absolute value programming, this value is the

coordinates of the end point at the hole bottom along

the Z axis in the workpiece coordinate system; for the

incremental value programming this value is the

relative distance from the end point at the hole bottom

to the start point of the cycle. Use W to express it in

the blueprint.

R

The retract amount along the Z axis. This value must

be a positive value, and is optional.

Q

The feed depth which must be positive.

251

12. Fixed Cycle

I

The feed width for wide-hole drilling. This value must be a

positive value, and is optional.

P

The retract amount along the X axis. When I is specified, P

must be a positive value. When I is not specified, P may be a

positive or a negative value. This parameter is optional.

Conduct end-face deep hole drilling cycle with G74.

Example

60

10

Z

X

%1234

T0101

M03S500

G01 X0 Z10F2000

G74 X-10Z-60R1Q5I3P1

M30

252

12. Fixed Cycle

12.2.5 Outer Diameter Grooving Cycle (G75)

This cycle is used to conduct grooving for the outer diameter of the

workpiece. See the figure below:

W

i

Z

ΔK

U/2

e

p

X

Format

G75X_/U_Z_/W_ Q(ΔK)_R(e)_ I(i)_P(p)_

Parameter

Description

X/U

For the absolute value programming, this value is

the coordinates of the end point at the hole bottom

along the X axis in the workpiece coordinate

system; for the incremental value programming

this value is the relative distance from the end

point at the hole bottom to the start point of the

cycle. Use U to express it in the blueprint.

Z/W

For the absolute value programming, this value is

the coordinates of the end point at the hole bottom

along the Z axis in the workpiece coordinate

system; for the incremental value programming

this value is the relative distance from the end

point at the hole bottom to the start point of the

cycle. Use W to express it in the blueprint. This

value is optional.

R

The retract amount along the X axis. This value

must be a positive value, and is optional.

Q

The feed depth which must be positive.

253

12. Fixed Cycle

I

The groove width. This value must be a positive value, and is

optional.

P

The retract amount along the Z axis. When I is specified, P

must be a positive value. When I is not specified, P may be a

positive or negative value. It is optional.

Example

Conduct outer diameter grooving cycle with G75.

ĭ80

Z

50

X

%1234

T0101

M03S500

G01 X50 Z50F2000

G75 X10Z60R1Q5I3P2

M30

254

12. Fixed Cycle

12.3 Fixed Cycle for Drilling of Turning Machines (T)

Commands of fixed cycle for

G Code

Description

drilling of turning machines

G83

Axial drilling cycle

G87

Radial drilling cycle

G84

Axial rigid tapping cycle

G88

Radial rigid tapping cycle

Attention

The commands in this section have no positioning function. To conduct

positioning, you need to specify G01 or G00 outside the fixed cycle.

255

12. Fixed Cycle

12.3.1 Axial Drilling Cycle (G83)/Radial Drilling Cycle (G87)

This cycle is used for the high-speed deep-hole drilling, with the cutting

feed speed for drilling, specified distance for tool exit, and periodically

repeat until the hole bottom. The chips is discharged out of the hole

during tool exit.

Format

G87X(U)_R_Q_K_P_F_H_

Parameter

Description

X/Z

Hole bottom coordinates.

R

The distance from the initial plane to the R plane.

Q

The cutting depth for each time.

P

The duration when the tool remains at the hole

bottom.

F

Feed speed.

K

Tool exit distance.

H1

Exit with the specified distance K.

H2

Exit to the R point.

H3

Directly drilling to the hole bottom.

• H1 Mode

MĮ

Initial plane

MĮ

M (Į+1), P2

M (Į+1)

Point R

Point R

Point R

P2

q

q

d

d

q

q

d

d

q

q

P1

Point Z

P1

Point Z

G83 or G87 (G98)

G83 or G87 (G99)

256

12. Fixed Cycle

• G83Z(W)_R_Q_K_P_F_H_

• H2 mode

MĮ

Initial plane

MĮ

M (Į+1)

M (Į+1), P2

Point R

Point R

P2

q

q

d

d

q

q

d

d

q

q

Point Z

Point Z

P1

P1

G83 or G87 (G98)

G83 or G87 (G99)

• H3 mode

MĮ

Initial plane

MĮ

R plane

R plane

M (Į+1), P2

M (Į+1), P2

Point Z

Point Z

P1

P1

G83 or G87 (G98)

G83 or G87 (G99)

257

12. Fixed Cycle

12.3.2 Axial Rigid Tapping Cycle (G84)/Radial Rigid Tapping Cycle (G88)

This cycle is used for tapping. In this cycle, the spindle rotates in the

counter clockwise direction when it reaches the hole bottom.

Format 1

G84 Z(W)_R_P_Q_E_J_K_F_H_

Parameter

Description

Z

Hole bottom coordinates.

R

The distance from the initial plane to the R plane.

P

The duration when the tool remains at the hole

bottom.

F

Feed speed.

Q

Cutting depth.

K

Retract amount

E1

Clockwise tapping.

E2

Counter clockwise tapping

J1

Tapping with the first spindle C.

J2

Tapping with the second spindle A.

H1

Exit with the distance specified by K.

H2

Back to the point R.

H3

Directly back to the hole bottom.

Format 2

G88X(U)_R_E_Q_K_H_P_F_(Tapping with the second spindle A only)

Parameter

Description

E1

Clockwise tapping.

E2

Counter clockwise tapping

Q

Cutting depth.

K

Retract amount

H1

Exit with the distance specified by K.

H2

Back to the point R.

H3

Directly back to the hole bottom.

259

12. Fixed Cycle

Initial plane

Spindle CW

MĮ

MĮ

rotation

Spindle CW

rotation

Plane of point

Point R

Point R

R

P1

Point Z

P1

Point Z

Spindle CCW rotation

Spindle CCW rotation

G84 or G88 (G98)

G84 or G88 (G99)

Example

M3 S1=1000; Rotate No. 1 spindle

G0X50Z50

M5

G84Z-10R20P1000F1000H1

M33 S2=1000; Rotate No. 2 spindle

G4P1000

M55

G84Z-10R20P1000F1H2

G88X-10R20P1000F1

M30

260

12. Fixed Cycle

12.4.1 Inner (Outer) Diameter Roughing Compound Cycle (G71)

This cycle can be divided into inner (outer) diameter roughing compound

cycle with groove and without groove.

Inner

(outer) diameter roughing

G71 U(Δd) R(r) P(ns) Q(nf) X(Δx) Z(Δz) F(f) S(s) T(t);

compound cycle without groove

Parameter

Description

U

Cutting depth

(each cutting amount). The symbol

("+/"-") is not specified with the value. The direction

is determined by the vector AA'.

R

Each retract amount.

P

The first program block sequence number for finish

machining (AA' in the figure below).

Q

The last program block sequence number for finish

machining (B'B in the figure below).

X

Finishing allowance in the X axis direction.

Z

Finishing allowance in the Z axis direction.

F S T

During roughing, the F, Sand T in G71 are valid, while

in finishing, the F, S and T between the ns program

block and nf program block are valid.

Description

This cycle is used for the roughing as shown in the figure below, and the

tool returns to the cycle start point. The finishing path AĺA'ĺB'ĺB is

executed based on the command order.

A

B

Δd

45 degrees

r

B’

Δx/2

A’

Δz

262

12. Fixed Cycle

XZ symbol ("+"/"-")

In the cutting cycle G71, the cutting feed direction is parallel to the Z

axis. The symbol of X (ΔU) and Z (ΔW) is as shown below, where "+"

indicates a positive direction along the axis, "-" indicates the negative

direction along the axis.

B B

B B

A

A

A

A

X(+) Z(-)

X(+) Z(+)

X(-) Z(-)

X(-)Z(+)

Aƍ

Aƍ

A

Aƍ

Aƍ

Aƍ

A

Aƍ

X(-) Z(-)

X(-)Z(+)

X(+) Z(-)

X(+)

A

B

B

A

A

B

B

A

Attention

1.

In the last program block of the finishing path with Q, there must be

X axial movements.

2.

In outer diameter roughing compound cycle G71, the cycle start

point must be the highest point, and in the inner diameter of the

roughing compound cycle , it must be the lowest point.

Example 1

Use outer diameter roughing compound cycle to create a machining

program for the workpiece shown as below: cycle start point: A (46, 3);

cutting depth

1.5 mm

(radius); retract amount:

1 mm; finishing

allowance along the X axis: 0.4 mm; finishing allowance along the Z

axis: 0.1 mm. The dotted lines indicate the workpiece.

263

12. Fixed Cycle

82

62

52

35

25

R7

R5 2×45°

%3325

T0101; Define coordinate system, and select No. 1 tool.

N1 G00 X80 Z80; Go to the program start point

N2 M03 S400; Spindle rotates at 400r/min

N3 G01 X46 Z3 F100; The tool goes to the cycle start point.

N4 G71U1.5R1P5Q14X0.4 Z0.1; Roughing amount: 1.5 mm; finishing

amount: X0.4 mm, Z0.1 mm

N5 G00 X0; Start finishing contour , go to the extended line of chamfer

N6 G01 X10 Z-2; Conduct finishing for chamfer of 2×45 degrees

N7 Z-20; Conduct finishing for ĭ10 outer circle

N8 G02 U10 W-5 R5; Conduct finishing for R5 arc

N9 G01 W-10; Conduct finishing for ĭ20 outer circle

N10 G03 U14 W-7 R7; Conduct finishing for R7 arc

N11 G01 Z-52; Conduct finishing for ĭ34 outer circle

N12 U10 W-10; Conduct finishing for outer cone

N13 W-20; Conduct finishing for ĭ44 outer circle

N14 U1; End finishing

N15 X50; Exit the machined face

N16G00 X80 Z80; Back to the tool exchange position

N17 M05; Stop spindle

264

12. Fixed Cycle

N18 M30 ; End the main program and reset

Example 2

Use inner diameter roughing compound cycle to create a machining

program for the workpiece shown as below: cycle start point: A (6, 5);

cutting depth:

1.5 mm

(radius); retract amount:

1 mm; finishing

allowance along the X axis: 0.4 mm; finishing allowance along the Z

axis: 0.1mm. The dotted lines indicate the workpiece.

82

62

52

35

25

R5

R7

2×45°

%3326

N1 T0101; Select No.1 tool, and define the coordinate system

N2 G00 X80 Z80; Go to the program start point or tool exchange

position.

N3 M03 S400; Rotate Spindle in the clockwise direction at 400r/min

N4 X6 Z5; Go to the cycle start point

G71U1R1P8Q16X-0.4Z0.1 F100; Start roughing

N5 G00 X80 Z80; After roughing, go to the tool exchange position

N6 T0202; Change to No.2 tool, and define the coordinate system

N7 G00 G41X6 Z5; Add tool nose arc radius compensation to No.2 tool

N8 G00 X44; Start finishing , go to the outer circle of ĭ44

N9 G01 Z-20 F80; Conduct finishing for the outer circle of ĭ44

N10 U-10 W-10; Conduct finishing for the outer cone

265

12. Fixed Cycle

N11 W-10; Conduct finishing for the outer circle of ĭ34

N12 G03 U-14 W-7 R7; Conduct finishing for the arc of R7

N13 G01 W-10; Conduct finishing for the outer circle of ĭ20

N14 G02 U-10 W-5 R5; Conduct finishing for the arc of R5

N15 G01 Z-80 ; Conduct finishing for the outer circle of ĭ10

N16 U-4 W-2; Conduct finishing for

2×45° chamfer, and end the

finishing

N17 G40 X4; Exit the machined face, and cancel the tool arc radius

compensation

N18 G00 Z80; Exit the inner hole of the workpiece

N19 X80; Return to the program start point or the tool exchange position

N20 M30; Stop spindle, end the main program, and reset

Inner

(outer) diameter roughing

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

compound cycle with groove

Parameter

Description

Format

U

Cutting depth

(each cutting amount). The symbol

("+"/"-") is not specified with the value. The direction

is determined by the vector AA'.

R

Each retract amount.

P

The first program block sequence number for

finishing path (AA' in the figure below).

Q

The last program block sequence number for finishing

path (B'B in the figure below).

E

The finishing allowance, which indicates the distance

along the X axis; It is positive for outer diameter

cutting and negative for inner diameter cutting.

F S T

During roughing, the F, S, and T in G71 are valid,

while in finishing, the F, S, and T between the ns

program block and nf program block are valid.

Description

This cycle is used for the roughing as shown in the figure below. The

finishing path is AĺA'ĺB'ĺB.

266

12. Fixed Cycle

B

A

45°

r

Δd

e

A'

B'

Attention

1.

G71 must have ns and nf of P/Q, which should correspond to the

start and end number of the finishing path; otherwise, the cycle

cannot be executed.

2.

The program block of ns must be G00/G01. In other words, the

action from A to A' must be a straight line or point positioning

movement.

3.

In the program blocks from ns to nf, no subprogram (4.03) should

be included.

267

12. Fixed Cycle

Example

Use outer diameter roughing compound cycle with groove to create a

machining program for the workpiece shown as below: the dotted lines

indicate the workpiece.

61.5

10

5

32.5

17

(8)

12

R4

R10

2×45 degrees

degrees

30 degrees

%3327

N1 T0101; Select No. 1 tool and define coordinate system

N2 G00 X80 Z100; Go to the program start point or tool exchange

position

M03 S400; Rotate spindle in the clockwise direction at 400 r/min

N3 G00 X42 Z3; The tool goes to the cycle start point.

N4G71U1R1P8Q19E0.3F100; Conduct rough cutting cycle with groove.

N5 G00 X80 Z100; After roughing, go to the tool exchange position

N6 T0202; Select No.2 tool, and define the coordinate system

N7 G00 G42 X42 Z3; Add tool nose arc radius compensation to No.2

tool

N8 G00 X10; Conduct finishing, go to the extended line of chamfer

N9 G01 X20 Z-2 F80; Conduct finishing for 2×45° chamfer

N10 Z-8; Conduct finishing for ĭ20 outer circle

N11 G02 X28 Z-12 R4; Conduct finishing for R4 arc

N12 G01 Z-17; Conduct finishing for ĭ28 outer circle

N13 U-10 W-5; Conduct finishing for under-cut cone

268

12. Fixed Cycle

12.4.2 End-Face Roughing Compound Cycle (G72)

This cycle is similar as G71. The difference is that the cutting of G72 is

parallel to the X axis.

Foramt

G72 W(ǻd) R(r) P(ns) Q(nf) X(ǻx) Z(ǻz) F(f) S(s) T(t);

Parameter

Description

W

Cutting depth

(each cutting amount). The sign

(positive or negative) is not specified with the value.

The direction is determined by the vector AA'.

R

Each retract amount.

P

The first program block sequence number for

finishing path (AA' in the figure below).

Q

The last program block sequence number for

finishing path (BB' in the figure below).

X

Finishing allowance in the X axis direction.

Z

Finishing allowance in the Z axis direction.

F S T

During roughing, the F, S, and T in G72 are valid,

while in finishing, the F, S, and T between the ns

program block and nf program block are valid.

Description

This cycle is used for the roughing and finishing as shown in the figure

below. The finishing path is AĺA'ĺB'ĺB.

Δz

Δd

Δd

+X

A

A'

Δd

r

r

B'

Δx/2

B'

+Z

270

12. Fixed Cycle

In the cutting cycle of G72, the cutting feed direction is parallel to the X

axis, and the sign of X(ΔU) and Z(ΔW) is shown in the figure below. The

sign "+" indicates the movement along the positive direction of the axis

Symbol of XZ value ("+"/"-")

while "-" indicates the movement along the negative direction of the

axis.

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

Attention

1.

The G72 command should have the address specified by P or Q;

otherwise, this cycle cannot be executed.

2.

The ns program should include G00/G01 coammnds, to execute the

action from A to A'. In addition, this program block should not have

the commands for the movement along the X axis.

3.

The program blocks from ns to nf may include G02/G03 commands,

but cannot include subprograms.

Example 1

Create a machining program for the workpiece shown as below: cycle

start point: A (80, 1); cutting depth 1.2 mm; tool exit quantity: 1 mm;

finishing allowance along the X axis: 0.2 mm; finishing allowance along

the Z axis: 0.5 mm. The dotted lines indicate the workpiece.

271

12. Fixed Cycle

60

50

40

26

15

R4

R2 _2×45

degrees

%3328

N1 T0101; Select No. 1 tool and define coordinate system

N2 G00 X80 Z80; Go to the program start point

N3 M03 S400; Rotate spindle in the clockwise direction at 400r/min.

N4 X80 Z1; Go to the cycle start point

N5 G72W1.2R1P8Q17X0.2Z0.5F100; Conduct roughing for the external

end face

N6 G00 X100 Z80; Go to the tool exchange position after roughing.

N7 G42 X80 Z1; Add tool nose arc radius compensation

N8 G00 Z-53; Start finishing , go to the extended line of the cone

N9 G01 X54 Z-40 F80; Conduct finishing for the cone.

N10 Z-30; Conduct finishing for ĭ54 outer circle

N11 G02 U-8 W4 R4; Conduct finishing for R4 arc

N12 G01 X30; Conduct finishing for Z26 end face

N13 Z-15; Conduct finishing for ĭ30 outer circle

N14 U-16; Conduct finishing for Z15 end face

N15 G03 U-4 W2 R2; Conduct finishing for R2 arc

N16 G01 Z-2; Conduct finishing for ĭ10 outer circle

N17 U-6 W3; Conduct finishing for 2×45° chamfer, complete finishing

N18 G00 X50; Exit the machined face

N19 G40 X100 Z80; Cancel the radius compensation and back to the

program start point

N20 M30; Stop spindle, end the main program, and reset

272

12. Fixed Cycle

Example 2

Create a machining program for the workpiece shown as below: cycle

start point: A (6, 3); cutting depth: 1.2 mm; tool exit quantity: 1 mm;

finishing allowance along the X axis: 0.2 mm; finishing allowance along

the Z axis: 0.5 mm. The dotted lines indicate the workpiece.

60

11

34

10

10

R4

2×45 degrees

R2

%3329

N1 T0101; Define coordinate system

N2 G00 X100 Z80; Go to the start point

N3 M03 S400; Rotate spindle in the clockwise direction at 400r/min

N4 G00 X6 Z3; Go to the cycle start point

N5 G72W1.2R1P6Q16X-0.2Z0.5F100; Inner end face roughing process

N6 G00 Z-61; Conduct finishing , go to the extended line of chamfer

N7 G01 U6 W3 F80; Conduct finishing for the chamfer 2×45°

N8 W10; Conduct finishing for the outer circle of ĭ10

273

12. Fixed Cycle

12.4.3 Closed Cutting Compound Cycle (G73)

This cycle can be used to cut workpiece with fixed graphics. It can be

used to effectively cut cast molding, forging molding or rough

workpieces.

Without groove

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

Parameter

Description

U

Total finishing allowance in the X axis direction.

W

Total finishing allowance in the Z axis direction.

R

Rough cutting count.

P

The first program block sequence number for

finishing path (AA' in the figure below).

Q

The last program block sequence number for finishing

path (BB' in the figure below).

X

Finishing allowance in the X axis direction.

Z

Finishing allowance in the Z axis direction.

F S T

During roughing, the F, S, and T in G73 are valid,

while during finishing, the F, S, and T between the ns

program block and nf program block are valid.

Description

instruction is a closed loop shown in the figure below. The tool feeds

gradually and cuts the workpiece to the final shape step by step. The

finishing path is AĺA'ĺB'ĺB. See the figure below:

Δk+Δz

ǻz

A

+X

ΔI+Δx/2

A

ǻx/2

A’

A’

●

ǻz ǻx/2

The tool path specified by the

275

Content      ..     7      8      9      10     ..