YAMAZAKI MAZAK INTEGREX e, INTEGREX i, VORTEX i Programming Manual

PROGRAMMING MANUAL

INTEGREX e series

INTEGREX i series

VORTEX i series

Programming Data for Post Processors

Manual No.: HA12PB0013E

Serial No.:

Before using this machine and equipment, fully understand the contents of this manual to ensure proper operation. Should any questions arise, please ask the nearest Technical Center or Technology Center.

IMPORTANT NOTICE

1. Be sure to observe the safety precautions described in this manual and the contents of the safety plates on the machine and equipment. Failure may cause serious personal injury or material damage. Please replace any missing safety plates as soon as possible.

2. No modifications are to be performed that will affect operation safety.

3. For the purpose of explaining the operation of the machine and equipment, some illustrations may not include safety features such as covers, doors, etc. Before operation, make sure all such items are in place.

4. This manual was considered complete and accurate at the time of publication, however, due to our desire to constantly improve the quality and specification of all our products, it is subject to change or modification. If you have any questions, please contact the nearest Technical Center or Technology Center.

5. Always keep this manual near the machinery for immediate use.

6. If a new manual is required, please order from the nearest Technical Center or Technology Center with the manual No. or the machine name, serial No. and manual name.

Issued by Manual Publication Section, YAMAZAKI MAZAK CORPORATION, Japan

04.2017

Original Instructions

Serial No. 294060

AVANS 294060

Serial No. 294060

CONTENTS

1 INTRODUCTION ................................................................................. 1-1

2 MACHINE INFORMATION .................................................................. 2-1

2-1 Controlled Axis Information ................................................................................ 2-1

2-1-1 Composition of controlled axes ............................................................................. 2-1

2-1-2 Outline of the machine structure ............................................................................ 2-5

2-1-3 Machine stroke ...................................................................................................... 2-6

2-1-4 Input limitation ..................................................................................................... 2-15

2-1-5 Rotating speed .................................................................................................... 2-15

2-1-6 Rapid feed rate.................................................................................................... 2-19

2-1-7 Cutting feed rate .................................................................................................. 2-22

2-2 Magazine .......................................................................................................... 2-28

2-2-1 INTEGREX i ........................................................................................................ 2-28

2-2-2 INTEGREX i-S ................................................................................................ .... 2-28

2-2-3 INTEGREX i-ST .................................................................................................. 2-28

2-2-4 INTEGREX e-H ................................................................................................... 2-29

2-2-5 INTEGREX e-H-S ............................................................................................... 2-29

2-2-6 INTEGREX e-H-ST ............................................................................................. 2-29

2-2-7 INTEGREX i-V ................................................................................................ .... 2-30

2-2-8 INTEGREX e-V ................................................................................................... 2-30

3 NC COMMAND ................................................................................... 3-1

3-1 Programming Format .......................................................................................... 3-1

2-2-9 VORTEX i-V ........................................................................................................ 2-31

3-1-1 Words and addresses ........................................................................................... 3-1

C-1

Serial No. 294060

3-1-2 Control out, control in ............................................................................................ 3-2

3-1-3 Optional block skip ................................................................................................ 3-2

3-1-4 Program end ......................................................................................................... 3-2

3-1-5 Program file name ................................................................................................. 3-2

3-2 Command ........................................................................................................... 3-3

4 MACHINING PROGRAM ..................................................................... 4-1

4-1 Set Up ................................................................................................................ 4-1

4-1-1 Setting of workpiece origin .................................................................................... 4-1

4-1-2 Parameter of tool length offset. ............................................................................. 4-1

4-1-3 Parameter for Nose / Tool radius compensation .................................................... 4-2

4-2 Programming Composition ................................................................................. 4-3

4-2-1 Programming composition ..................................................................................... 4-3

4-2-2 Method of making program.................................................................................... 4-4

4-3 Preparation Motion for Machining ....................................................................... 4-7

4-3-1 Sample program .................................................................................................... 4-7

4-3-2 Preparation for machining ..................................................................................... 4-7

4-4 Machining Motion ............................................................................................. 4-15

4-4-1 Turning program .................................................................................................. 4-15

4-4-2 Hole machining program ..................................................................................... 4-23

4-5 End Motion for Machining ................................................................................. 4-47

4-4-3 3-axis machining program ................................................................................... 4-28

4-4-4 4-axis machining program ................................................................................... 4-34

4-4-5 5-axis machining program ................................................................................... 4-38

4-5-1 Sample program .................................................................................................. 4-47

C-2

Serial No. 294060

4-5-2 End motion .......................................................................................................... 4-47

4-6 Programming for Compound Machining (ST Specification) .............................. 4-49

4-6-1 Function of programming for compound machining ............................................. 4-49

4-6-2 Sample programs ................................................................................................ 4-58

5 SUPPLEMENT .................................................................................... 5-1

5-1 Detail of Preparatory Function ............................................................................ 5-2

5-2 Detail of Miscellaneous Function ...................................................................... 5-63

5-3 Restriction of Combination ............................................................................... 5-75

C-3

E

SAFETY PRECAUTIONS

This manual is prepared only for the function or the device which is specified in the title of this manual. Therefore, you are required to carefully read and understand the operating manual of the machine, especially the section describing safety precautions, before using or operating the function or the device.

Serial No. 294060

C-4

1 INTRODUCTION

Serial No. 294060

This manual contains information for post processor to create EIA/ISO program according to the machine. This manual can be used as an EIA/ISO programming manual.

This manual describes the machines of the INTEGREX e-series, INTEGREX i-series, and VORTEX i-series.

The INTEGREX e-series and INTEGREX i-series are multi-tasking machines and support both milling and turning. The VORTEX i-series is a machining center and supports milling only.

Note that the turning function is excluded from the descriptions of the VORTEX i-series.

INTRODUCTION 1

1-1

1 INTRODUCTION

E

Serial No. 294060

1-2

2 MACHINE INFORMATION

X-axis

Refers to the vertical motion of the upper turret.

“+” (plus) indicates the upward direction (away from the spindle center); “–” (minus) indicates the downward direction (towards the spindle center).

Z-axis

Refers to the transverse motion of the upper turret.

“+” (plus) indicates the rightward direction (away from the chuck); “–” (minus) indicates the leftward direction (towards the chuck).

C-axis

Refers to the rotation of the work spindle.

“+” (plus) indicates the right-hand rotation (CW); “–” (minus) indicates the left-hand rotation (CCW).

Y-axis

Refers to the longitudinal motion of the upper turret.

“+” (plus) indicates the forward direction (to the front); “–” (minus) indicates the backward direction (to the rear).

C2-axis

Refers to the rotation of the secondary spindle.

“+” (plus) indicates the left-hand rotation (CCW); “–” (minus) indicates the right-hand rotation (CW).

W-axis

Refers to the transverse motion of the secondary headstock.

“+” (plus) indicates the rightward direction; “–” (minus) indicates the leftward direction.

X2-axis

Refers to the vertical motion of the lower turret.

“+” (plus) indicates the downward direction (away from the spindle center); “–” (minus) indicates the upward direction (towards the spindle center).

Z2-axis

Refers to the transverse motion of the lower turret.

“+” (plus) indicates the rightward direction; “–” (minus) indicates the leftward direction.

Serial No. 294060

2-1 Controlled Axis Information

This section describes Composition of controlled axes, machine specification, machine stroke, input limitation, rotating speed, rapid feed rate and cutting feed rate.

2-1-1 Composition of controlled axes

This section indicates composition of controlled axes.

1. INTEGREX i/i-S/i-ST/e-H/e-H-S/e-H-ST

The axes of coordinates used for machine control are defined as follows:

MACHINE INFORMATION 2

2-1

2 MACHINE INFORMATION

X

Y

+

–

– – C2 + –

W

C

–

+

–

+

Z2

–

+

Z

X2

+

–

Serial No. 294060

2-2

MACHINE INFORMATION 2

X-axis

Axis of transverse motion of the table

“+” (plus) indicates the leftward direction; “-” (minus) indicates the rightward direction.

Y-axis

Axis of longitudinal motion of the milling spindle

“+” (plus) indicates the backward direction (to the rear); “-” (minus) indicates the forward direction (to the front).

Z-axis

Axis of vertical motion of the milling headstock

“+” (plus) indicates the upward direction; “-” (minus) indicates the downward direction.

B-axis

Rotation of the milling spindle

“+” (plus) indicates the right-hand rotation (CW); “-” (minus) indicates the left-hand rotation (CCW), as viewed from the operator door.

C-axis

Rotation of the table

“+” (plus) indicates the right-hand rotation (CW); “-” (minus) indicates the left-hand rotation (CCW), as viewed from above.

X

Z

C

Rotation of the pallet

Y

+ – + + – – –

Rotation of the milling spindle

B

+ + –

Serial No. 294060

2. INTEGREX e-V

The axes of coordinates used for machine control are defined as follows: Note: The axes of coordinates are defined with the operator standing and facing the front of

the machine.

2-3

2 MACHINE INFORMATION

X-axis

Axis of transverse motion of the table

“+” (plus) indicates the leftward direction; “-” (minus) indicates the rightward direction.

Y-axis

Axis of longitudinal motion of the milling spindle

“+” (plus) indicates the backward direction (to the rear); “-” (minus) indicates the forward direction (to the front).

Z-axis

Axis of vertical motion of the milling headstock

“+” (plus) indicates the upward direction; “-” (minus) indicates the downward direction.

B-axis

Rotation of the milling spindle

“+” (plus) indicates the right-hand rotation (CW); “-” (minus) indicates the left-hand rotation (CCW), as viewed from the operator door.

C-axis

Rotation of the table

“+” (plus) indicates the right-hand rotation (CW); “-” (minus) indicates the left-hand rotation (CCW), as viewed from above.

X Z Y

+

– – + – +

Rotation of the spindle

Rotation of the pallet

B

+ – –

+

C

Serial No. 294060

3. INTEGREX i-V/VORTEX i-V

The axes of coordinates used for machine control are defined as follows: Note: The axes of coordinates are defined with the operator standing and facing the front of

the machine.

2-4

2-1-2 Outline of the machine structure

:Applicable, -: Not applicable

Number of simultaneously controlled axes

Kind of machining

Structure

Axis direction during

home return

4/5 axis (Note)

Multi-tasking machine



Spindle No. 1

-Z

-

Spindle No. 2



upper turret

-

lower turret

:Applicable, -: Not applicable

Number of simultaneously controlled axes

Kind of machining

Structure

Axis direction during

home return

4/5 axis (Note)

Multi-tasking machine



Spindle No. 1

-Z



Spindle No. 2



upper turret

-

lower turret

:Applicable, -: Not applicable

Number of simultaneously controlled axes

Kind of machining

Structure

Axis direction during

home return

4/5 axis (Note)

Multi-tasking machine



Spindle No. 1

-Z



Spindle No. 2



upper turret



lower turret

:Applicable, -: Not applicable

Number of simultaneously controlled axes

Kind of machining

Structure

Axis direction during

home return

4/5 axis (Note)

Vertical machining center

-

Turning spindle

-Z



Mill Spindle

Serial No. 294060

This section indicates outline of the machine structure.

1. INTEGREX i/e-H/i-V/e-V

Note: It is 5 axis when there is option of simultaneously controlled 5 axes, it is 4 axis when

there is not.

2. INTEGREX i-S/e-H-S

MACHINE INFORMATION 2

Note: It is 5 axis when there is option of simultaneously controlled 5 axes, it is 4 axis when

there is not.

3. INTEGREX i-ST/e-H-ST

Note: It is 5 axis when there is option of simultaneously controlled 5 axes, it is 4 axis when

there is not.

4. VORTEX i-V

Note : It is 5 axis when there is option of simultaneously controlled 5 axes, it is 4 axis when

there is not.

2-5

2 MACHINE INFORMATION

+Y

-Y

Y stroke

Y

Home Position

Holder end

-Z stroke

X stroke

X

Home Position

Z

Home Position

Z stroke

+Z stroke

Spindle center

-B stroke

+B stroke

B

Home Position

B stroke

W

Home Position

W stroke

Serial No. 294060

2-1-3 Machine stroke

This section indicates axis stroke.

1. Axis stroke

A. INTEGREX i/e-H

2-6

MACHINE INFORMATION 2

Machine specification

Xmax

Xmin

Ymax

Ymin

Zmax

Zmin

Bmax

Bmin

Unit

mm

(in)

mm

(in)

mm (in)

deg

i-100

-

0

(0)

-450

(-17.72)

105

(4.13)

-105

(-4.13)

84

(3.31)

-485

(-19.09)

210

-30

i-150

-

-370

(-14.57)

100

(3.94)

-100

(-3.94) 0 (0)

-435

(-17.13)

190

-10

i-200

1000U

-615

(-24.21)

130

(5.12)

[125

(4.92)]

-130

(-5.12)

[-125

(-4.92)]

497

(19.57)

-580

(-22.83)

210

-30

1500U

1005

(39.57)

i-300

1000U

497

(19.57)

1500U

1005

(39.57)

2500U

1983

(78.07)

i-400

1000U

497

(19.57)

1500U

1005

(39.57)

2500U

1983

(78.07)

e-420H

1500U

5

(0.20)

-840

(-33.07)

210

(8.27)

-210

(-8.27)

1143

(45.00)

-440

(-17.32)

3000U

2673

(105.24)

e-500H

1500U

-865

(-34.06)

250

(9.84)

-250

(-9.84)

1098

(43.23)

-500

(-19.69)

3000U

2622

(103.23)

4000U

3638

(143.23)

e-670H

3000U

-1020

(-40.16)

345

(13.58)

-325

(-12.80)

2382

(93.78)

-740

(-29.13)

4000U

3398

(113.78)

6000U

5430

(213.78)

e-800H

4000U

-1295

(-50.98)

400

(15.75)

-400

(-15.75)

3640

(143.31)

6000U

5640

(222.05)

8000U

7640

(300.79)

Serial No. 294060

Note : The value in [ ] shows the stroke of MATRIX-mounted machines.

2-7

2 MACHINE INFORMATION

Machine specification

Wmax

Wmin

C

Holder end

Spindle

center

Without

steady rest

With

steady rest

Unit

mm

(in)

deg

mm

(in)

mm

(in)

i-100

-

0

(0)

-807

(-31.77)

-

±360

[Cycloid

type]

80

(3.15)

-400

(-15.75)

i-150

-

-300

(-11.81)

-320

(-12.60)

i-200

1000U

-1026

(-40.39)

170

(6.69)

-490

(-19.29)

1500U

-1562

(-61.50)

i-300

1000U

-1026

(-40.39)

1500U

-1562

(-61.50)

2500U

-2250

(-88.58)

i-400

1000U

-1026

(-40.39)

1500U

-1562

(-61.50)

2500U

-2250

(-88.58)

e-420H

1500U

-1505

(-59.25)

-1335

(-52.56)

249

(9.80)

-715

(-28.15)

3000U

-3035

(-119.49)

-2769

(-109.02)

e-500H

1500U

1

(0.04)

-1466

(-57.72)

-1157.8 (-45.58)

300

(11.81)

-850

(-33.46)

3000U

-2990

(-117.72)

-2681.8

(-105.58)

4000U

-

-3528

(-138.90)

e-670H

3000U

-2879

(-113.35)

-2690

(-105.91)

-1005

(-39.57)

4000U

-3890

(-153.15)

-3480

(-137.01)

6000U

-

-5054

(-198.98)

e-800H

4000U

0

(0)

-4055

(-159.65)

-1275

(-50.20)

6000U

-5010

(-197.24)

8000U

-6870

(-270.47)

Serial No. 294060

2-8

MACHINE INFORMATION 2

Machine specification

Xmax

Xmin

Ymax

Ymin

Zmax

Zmin

Bmax

Bmin

Unit

mm

(in)

mm

(in)

mm

(in)

deg

i-100S

-

0

(0)

-450

(-17.72)

105

(4.13)

-105

(-4.13)

419

(16.50)

-485

(-19.09)

210

-30

i-100BARTAC-S

-

i-200S

1000U

-615

(-24.21)

130

(5.12)

-130

(-5.12)

497

(19.57)

-580

(-22.83)

1500U

1005

(39.57)

i-300S

1500U

2500U

1983

(78.07)

i-400S

1500U

1005

(39.57)

2500U

1983

(78.07)

e-420H-S

1500U

5

(0.197)

-840

(-33.071)

210

(8.268)

-210

(-8.268)

948

(37.323)

-440

(-17.323)

3000U

2673

(105.236)

e-500H-S

1500U

-865

(-34.055)

250

(9.843)

-250

(-9.843)

1098

(43.228)

-500

(-19.685)

3000U

2622

(103.228)

e-670H-S

3000U

-1020

(-40.157)

345

(13.583)

-325

(-12.795)

2382

(93.78)

-740

(-29.134)

4000U

3398

(133.78)

+Y

-Y Y Home Position

Holder end

Y stroke

X stroke

-Z stroke

+Z stroke

Z stroke

Z

Home Position

W stroke

Spindle center

W

Home Position

-B stroke

+B stroke

B

Home Position

B stroke

X

Home Position

Serial No. 294060

B. INTEGREX i-S/e-H-S

2-9

2 MACHINE INFORMATION

Machine specification

Wmax

Wmin

C

Holder end

Spindle

center

Without

steady rest

With

steady rest

Unit

mm (in)

deg

mm

(in)

mm (in)

i-100S

-

0

(0)

-903

(-35.55)

-

±360

[Cycloid

type]

80

(3.15)

-400

(-15.75)

i-100BARTAC-S

-

i-200S

1000U

-1066

(-41.97)

170

(6.69)

-490

(-19.29)

1500U

-1574

(-61.96)

i-300S

1500U

2500U

-2175

(-85.63)

i-400S

1500U

-1574

(-61.97)

2500U

-2175

(-85.63)

e-420H-S

1500U

2

(0.08)

-1370

(-53.94)

-1054

(-41.50)

249

(9.80)

-715

(-28.15)

3000U

-3078

(-121.18)

-2762

(-108.74)

e-500H-S

1500U

5

(0.20)

-1524

(-60.00)

-

300

(11.81)

-850

(-33.46)

3000U

-3048

(-120.00)

-2458

(-96.77)

e-670H-S

3000U

-1005

(-39.57)

4000U

-

-3209

(-126.34)

Serial No. 294060

2-10

MACHINE INFORMATION 2

Machine specification

X1max

X1min

Ymax

Ymin

Z1maz

Z1min

Bmax

Bmin

Unit

mm

(in)

mm

(in)

mm

(in)

deg

i-100ST

-

0

(0)

-450

(-17.72)

105

(4.13)

-105

(-4.13)

419

(16.5)

-485

(-19.09)

210

-30

i-100BARTAC-ST

-

i-200ST

1500U

-615

(-24.21)

130

(5.12)

-130

(-5.12)

1005

(39.57)

-580

(-22.83)

i-300ST

1500U

i-400ST

1500U

e-420H-ST

2000U

5

(0.197)

-840

(-33.071)

210

(8.268)

-210

(-8.268)

1648

(64.882)

-440

(-17.323)

Machine specification

Wmax

Wmin

X2max

X2min

Z2max

Z2min

C1

C2

Unit

mm

(in)

mm

(in)

mm

(in)

deg

i-100ST

-

0

(0)

-903

(-35.55)

0

(0)

-220

(-8.66)

542

(21.34)

-361

(-14.21)

±360

[Cycloid

type]

±360

[Cycloid

type]

i-100BARTAC-ST

-

i-200ST

1500U

-1539

(-60.59)

-230

(-9.06)

951

(37.44)

-437

(-17.20)

i-300ST

1500U

i-400ST

1500U

e-420H-ST

2000U

2

(0.08)

-1961

(-77.20)

2

(0.08)

-360

(-14.17)

1471

(57.913)

-422

(-16.614)

Machine specification

Holder end

Spindle center

Unit

mm

(in)

mm

(in)

i-100ST

-

80

(3.15)

-400

(-15.75)

i-100BARTAC-ST

-

i-200ST

1500U

170

(6.69)

-490

(-19.29)

i-300ST

1500U

i-400ST

1500U

e-420H-ST

2000U

249

(9.803)

-715

(-28.150)

+Y

-Y

+Y

-Y

Y

Home Position

Holder end

Y stroke

X stroke

Z stroke

-Z stroke

+Z stroke

X Home Position

Z

Home Position

Spindle center

X2 stroke W stroke

Z2 stroke

-Z2 stroke

+Z2 stroke

Serial No. 294060

C. INTEGREX i-ST/e-H-ST

2-11

2 MACHINE INFORMATION

Machine specification

Xmax

Xmin

Ymax

Ymin

Zmax

Zmin

Bmax

Bmin

Unit

mm

(in)

mm

(in)

mm

(in)

deg

e-1060V

-

0

(0)

-1525

(-60.039)

5

(0.197)

-1055

(-41.535)

0

(0)

-1345

(-52.952)

120

-30

e-1250V/8

Single

-1875

(-73.818)

0

(0)

-1250

(-49.213)

2-pallet

e-1550V

-

-1550

(-61.023)

e-1600V/10

Single

-2165

(-85.236)

-1600

(-62.992) 2-pallet

-2315

(-91.142)

e-1850V

-

-3055

(-120.275)

-1850

(-72.834)

-1800

(-70.866)

i-500V/5

2-pallet

-1100

(-43.307)

-800

(-31.496)

-900

(-35.433)

i-630V/6

Single

-1425

(-56.102)

-1050

(-41.338)

-1050

(-41.338)

2-pallet

+

–

+ – –

+ Y Home Position

Y center

Y

stroke

Z

stroke

Z

Home Position

X

Home Position

Spindle center

X stroke

B

stroke

+B

stroke

-B

stroke

Holder end

Serial No. 294060

D. INTEGREX e-V/i-V

2-12

Machine specification

C

Holder end

Spindle center

Y center

Unit

deg

mm

(in)

mm

(in)

mm

(in)

e-1060V

-

±360

[Cycloid type]

300

(11.811)

-985

(-38.779)

-530

(-20.866)

e-1250V/8

Single

-1335

(-52.559)

-625

(-24.606)

2-pallet

e-1550V

-

-1775

(-69.881)

-775

(-30.511)

e-1600V/10

Single

-800

(-31.496)

2-pallet

e-1850V

-

-2130

(-83.858)

-925

(-36.417)

i-500V/5

2-pallet

249

(9.803)

-1020

(-40.157)

-400

(-15.748)

i-630V/6

Single

350

(13.779)

-1395

(-54.921)

-525

(-20.669)

2-pallet

Machine specification

Xmax

Xmin

Ymax

Ymin

Zmax

Zmin

Bmax

Bmin

Unit

mm

(in)

mm

(in)

mm

(in)

deg

i-630V/6

Single

0

(0)

-1425

(-56.102)

0

(0)

-1050

(-41.339)

0

(0)

-1050

(-41.339)

120

-30

2-pallet

i-800V/8

Single

10

(0.394)

-1690

(-66.535)

-1500

(-59.055)

-1150

(-45.276)

2-pallet

Machine specification

C

Holder end

Spindle center

Y center

Unit

deg

mm

(in)

mm

(in)

mm

(in)

i-630V/6

Single

±360

[Cycloid type]

350 (13.780)

-1395

(-54.921)

-525

(-20.669)

2-pallet

i-800V/8

Single

-1690

(-66.535)

-750

(-29.528)

2-pallet

+ – + – –

+

Y

Home Position

Y center

Y stroke

Z stroke

Z

Home Position

X

Home Position

Spindle center

X stroke

B stroke

+B stroke

-B stroke

Holder end

Serial No. 294060

E. VORTEX i-V

MACHINE INFORMATION 2

2-13

2 MACHINE INFORMATION

Parameter

Contents

Setting range

Setting unit

BA62

Amount of offset for the B-axis — spindle distance

±99999999

0.0001 mm

0.00001 in

Parameter

Contents

Setting range

Setting unit

S5

Rotational center of the table

±99999999

0.0001 mm

0.00001 in

D734P2014

BA62

S5

Reference point of the workpiece

Offset vector from tool holder end to B-axis center

Machine origin

Axis of B-axis rotation

Axis of C-axis rotation

Serial No. 294060

2. Offset for the axis of rotation of the rotational axis

A. Offset for the axis of rotation of B-axis

B. Offset for the axis of rotation of C-axis

Fig. 2-1 Horizontal type

2-14

2-1-4 Input limitation

Axis

Maximum command unit

Minimum command unit

Number of digit after the

decimal point

Linear axes [mm]

±99999.9999

0.0001

4-digit

Linear axes [in]

±9999.99999

0.00001

5-digit

Rotary axes [°]

±99999.9999

0.0001

4-digit

[min-1]

Machine specification

Spindle No. 1

Spindle No. 2

Mill Spindle

(12000min-1)

Standard

Mill Spindle

(20000min-1)

Option

i-100

-

35 to 6000

-

35 to 12000

35 to 20000

i-150

-

35 to 5000

i-200

1000U

1500U

i-300

1000U

35 to 4000

1500U

2500U

i-400

1000U

35 to 3300

1500U

2500U

[min-1]

Machine specification

Spindle No. 1

Spindle No. 2

Mill Spindle

(12000min-1)

Standard

Mill Spindle

(20000min-1)

Option

i-100S

-

35 to 6000

35 to 12000

35 to 20000

i-100BARTAC-S

-

35 to 2000

i-200S

1000U

35 to 5000

1500U

i-300S

1500U

35 to 4000

2500U

i-400S

1500U

35 to 3300

2500U

Serial No. 294060

This section indicates input limitation value of NC.

Input limitation

2-1-5 Rotating speed

This section indicates limiting value of rotating speed. Limitations of the rotating speed of the turning spindle will vary according to the chuck used. * The values in the table indicate the rotating speed for the standard chuck.

1. INTEGREX i

MACHINE INFORMATION 2

Remark: 3000 min

2. INTEGREX i-S

Remark: 3000 min

-1

is upper limit value during tapping cycle.

-1

is upper limit value during tapping cycle.

2-15

2 MACHINE INFORMATION

[min-1]

Machine specification

Spindle No. 1

Spindle No. 2

Mill Spindle

(12000min-1)

Standard

Mill Spindle

(20000min-1)

Option

i-100ST

-

35 to 6000

35 to 12000

35 to 20000

i-100BARTAC-ST

-

35 to 2000

i-200ST

1500U

35 to 5000

i-300ST

1500U

35 to 4000

i-400ST

1500U

35 to 3300

Machine specification

Lower turret (Note)

i-100ST

-

35 to 6000

i-100BARTAC-ST

-

i-200ST

1500U

i-300ST

1500U

i-400ST

1500U

[min-1]

Machine specification

Spindle No. 1

Standard

Spindle No. 1

Option

Mill Spindle

(12000min-1)

Standard

Mill Spindle

(20000min-1)

Option

e-420H

1500U

35 to 4000

35 to 2500

35 to 12000

-

3000U

e-500H

1500U

35 to 3300

35 to 1600

35 to 10000

3000U

4000U

e-670H

3000U

4 to 1600

3 to 1000

25 to 5000

4000U

6000U

e-800H

4000U

1 to 700

-

25 to 10000

6000U

8000U

Serial No. 294060

3. INTEGREX i-ST

Note: Only turret for milling (option). Remark: 3000 min

-1

is upper limit value during tapping cycle.

4. INTEGREX e-H

Remark: 3000 min

* The data are value for the following specifications:

 e-420H : Spindle through hole diameter 91  e-500H : Spindle through hole diameter 104  e-670H : Spindle through hole diameter 170 (270 for e-670H6000U)

-1

is upper limit value during tapping cycle.

2-16

5. INTEGREX e-H-S

[min-1]

Machine specification

Spindle No. 1

Standard

Spindle No. 1

Option

Spindle No. 2

Standard

Spindle No. 2

Option

e-420H-S

1500U

35 to 4000

35 to 2500

35 to 4000

35 to 2500

3000U

e-500H-S

1500U

35 to 3300

35 to 1600

35 to 3300

3000U

e-670H-S

3000U

4 to 1600

3 to 1000

4 to 1600

4000U

Machine specification

Mill Spindle

(12000min-1)

Standard

Mill Spindle

(20000min-1)

Option

e-420H-S

1500U

35 to 12000

-

3000U

e-500H-S

1500U

35 to 10000

3000U

e-670H-S

3000U

25 to 5000

4000U

[min-1]

Machine specification

Spindle No. 1

Standard

Spindle No. 1

Option

Spindle No. 2

Standard

Spindle No. 2

Option

e-420H-ST

2000U

35 to 4000

35 to 2500

35 to 4000

35 to 2500

Machine specification

Mill Spindle

(12000min-1)

Standard

Mill Spindle

(20000min-1)

Option

Lower turret (Note)

e-420H-ST

2000U

35 to 12000

-

35 to 6000

Serial No. 294060

MACHINE INFORMATION 2

Remark: 3000 min * The data are value for the following specifications:

 e-420H-S : Spindle through hole diameter 91  e-500H-S : Spindle through hole diameter 104  e-670H-S : Spindle through hole diameter 170

6. INTEGREX e-H-ST

Note: Only turret for milling (option). Remark : 3000 min

* The data are value for the following specifications:

 e-420H-ST : Spindle through hole diameter 91

-1

is upper limit value during tapping cycle.

-1

is upper limit value during tapping cycle.

2-17

2 MACHINE INFORMATION

[min-1]

Machine specification

Turning spindle

Mill Spindle

(12000min-1)

Standard

Mill Spindle

High torque

specification

Option

Mill Spindle

High-speed spindle

specification

Option

i-500V/5

2-pallet

35 to 1000

35 to 12000 - -

i-630V/6

Single

2 to 550

25 to 10000

25 to 5000

25 to 15000

2-pallet

[min-1]

Machine specification

Turning

spindle

Standard

Turning

spindle

Option

Mill Spindle

(10000min-1)

Standard

Mill Spindle High torque

specification

Option

Mill Spindle High-speed

spindle

specification

Option

e-1060V

-

5 to 600

3 to 300

25 to 10000

25 to 5000

-

e-1250V/8

Single

1.8 to 500

1.1 to 300

2-pallet

e-1550V

-

3 to 300

-

e-1600V/10

Single

5 to 300

25 to 15000

2-pallet

e-1850V

-

5 to 250

5 to 150

-

[min-1]

Machine specification

Mill Spindle

(10000min-1)

Standard

Mill Spindle

High torque specification

Option

Mill Spindle

High-speed spindle

specification

Option

i-630V/6

Single

25 to 10000

25 to 5000

25 to 15000

2-pallet

i-800V/8

Single

2-pallet

Serial No. 294060

7. INTEGREX i-V

Remark: 3000 min

-1

is upper limit value during tapping cycle.

* Limitations on the rotation of the turning spindle will vary with pallet specifications.

8. INTEGREX e-V

Remark : 3000 min

-1

is upper limit value during tapping cycle.

9. VORTEX i-V

Remark: 3000 min

-1

is upper limit value during tapping cycle.

2-18

2-1-6 Rapid feed rate

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

W

i-100

-

40000 (1574)

14400

199800

8000 (314)

i-150

-

30000 (1181)

i-200

1000U

50000 (1968)

8000 (314)

1500U

i-300

1000U

1500U

2500U

40000 (1574)

i-400

1000U

50000 (1968)

1500U

2500U

40000 (1574)

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C1 W C2

i-100S

-

40000

(1574)

40000

(1574)

40000

(1574)

14400

199800

30000

(1181)

199800

i-100BARTAC-S

-

i-200S

1000U

50000

(1968)

40000

(1574)

50000

(1968)

1500U

i-300S

1500U

2500U

40000

(1574)

18000

(708)

i-400S

1500U

50000

(1968)

30000

(1181)

2500U

40000

(1574)

18000

(708)

Serial No. 294060

This section indicates limiting value of rapid feed rate.

1. INTEGREX i

MACHINE INFORMATION 2

2. INTEGREX i-S

2-19

2 MACHINE INFORMATION

[mm/min (in/min) or deg/min]

Machine specification

X1 Y Z1 B C1 W i-100ST

-

40000

(1574)

40000

(1574)

40000

(1574)

14400

199800

30000

(1181)

i-100BARTAC-ST

-

i-200ST

1500U

50000

(1968)

50000

(1968)

i-300ST

1500U

i-400ST

1500U Machine specification

X2

Z2

C2

i-100ST

-

40000

(1574)

40000

(1574)

199800

i-100BARTAC-ST

-

i-200ST

1500U

i-300ST

1500U

i-400ST

1500U

[mm/min (in/min) or deg/min]

Machine specification

X1 Y Z1 B C

W

e-420H

1500U

50000 (1968)

18000

199800

6000 (236)

3000U

40000 (1574)

4500 (177)

e-500H

1500U

40000 (1574)

10800

7200

6000 (236)

3000U

4000U

e-670H

3000U

12000

(472)

4000U

30000 (1181)

6000U

18000

(708)

6000 (236)

e-800H

4000U

18000

(708)

18000

(708)

24000

(944)

4500

6000U

18000

(708)

8000U

[mm/min (in/min) or deg/min]

Machine specification

X1 Y Z1 B C1 W C2

e-420HS

1500U

50000

(1968)

50000

(1968)

50000

(1968)

18000

199800

30000

(1181)

199800

3000U

40000

(1574)

12000

(472)

e-500HS

1500U

40000

(1574)

40000

(1574)

10800

7200

3000U

e-670HS

3000U

4000U

30000

(1181)

10000

(393)

Serial No. 294060

3. INTEGREX i-ST

4. INTEGREX e-H

5. INTEGREX e-H-S

2-20

6. INTEGREX e-H-ST

[mm/min (in/min) or deg/min]

Machine specification

X1 Y Z1 B C1 W C2

e-420HST

2000U

50000

(1968)

50000

(1968)

50000

(1968)

18000

199800

30000

(1181)

199800

Machine specification

X2

Z2

e-420HST

2000U

20000

(787)

32000

(1259)

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

i-500V/5

2-pallet

50000

(1968)

50000

(1968)

50000

(1968)

18000

36000

i-630V/6

Single

52000

(2047)

52000

(2047)

52000

(2047)

10800

18000

2-pallet

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

e-1060V

-

42000

(1653)

42000

(1653)

42000

(1653)

10800

6545

e-1250V/8

Single

9000

2-pallet

e-1550V

-

3272

e-1600V/10

Single

3600

2-pallet

7200

e-1850V

-

40000

(1574)

40000

(1574)

40000

(1574)

2400

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

i-630V/6

Single

52000

(2047)

52000

(2047)

52000

(2047)

10800 10800

2-pallet

i-800V/8

Single

9000

2-pallet

Serial No. 294060

7. INTEGREX i-V

8. INTEGREX e-V

MACHINE INFORMATION 2

9. VORTEX i-V

2-21

2 MACHINE INFORMATION

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

W

i-100

-

8000

(314)

8000

(314)

8000

(314)

5000

STD:36000

BT:10800

8000

(314)

i-150

-

36000

i-200

1000U

1500U

i-300

1000U

1500U

2500U

i-400

1000U

1500U

2500U

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

W

i-100

-

40000 (1574)

14400

199800

40000 (1574)

i-150

-

i-200

1000U

1500U

i-300

1000U

1500U

2500U

i-400

1000U

1500U

2500U

Serial No. 294060

2-1-7 Cutting feed rate

This section indicates limiting value of cutting feed rate.

1. INTEGREX i

A. On turning/milling

B. On milling (During geometry compensation)

2-22

2. INTEGREX i-S

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C1 W C2

i-100S

-

8000

(314)

8000

(314)

8000

(314)

5000

STD:

36000

BT:

10800

8000

(314)

36000

i-100BARTAC-S

-

i-200S

1000U

36000

1500U

i-300S

1500U

2500U

i-400S

1500U

2500U

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C1 W C2

i-100S

-

40000

(1574)

40000

(1574)

40000

(1574)

14400

199800

40000

(1574)

199800

i-100BARTAC-S

-

i-200S

1000U

1500U

i-300S

1500U

2500U

i-400S

1500U

2500U

[mm/min (in/min) or deg/min]

Machine specification

X1 Y Z1 B C1

W

i-100ST

-

8000 (314)

5000

STD:36000

BT:10800

8000 (314)

i-100BARTAC-ST

-

i-200ST

1500U

36000

i-300ST

1500U

i-400ST

1500U Machine specification

X2

Z2

C2

i-100ST

-

8000 (314)

36000

i-100BARTAC-ST

-

i-200ST

1500U

i-300ST

1500U

i-400ST

1500U

Serial No. 294060

A. On turning/milling

B. On milling (During geometry compensation)

MACHINE INFORMATION 2

3. INTEGREX i-ST

A. On turning/milling

2-23

2 MACHINE INFORMATION

[mm/min (in/min) or deg/min]

Machine specification

X1 Y Z1 B C1 W i-100ST

-

40000 (1574)

14400

199800

40000 (1574)

i-100BARTAC-ST

-

i-200ST

1500U

i-300ST

1500U

i-400ST

1500U Machine specification

X2

Z2

C2

i-100ST

-

40000 (1574)

199800

i-100BARTAC-ST

-

i-200ST

1500U

i-300ST

1500U

i-400ST

1500U

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

W

e-420H

1500U

8000 (314)

7200

36000

8000 (314)

3000U

e-500H

1500U

2100

1800

1200

(47)

3000U

4000U

e-670H

3000U

4000U

6000U

e-800H

4000U

6000U

8000U

Serial No. 294060

B. On milling (During geometry compensation)

4. INTEGREX e-H

A. On turning/milling

2-24

B. On milling (During geometry compensation)

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

W

e-420H

1500U

50000 (1962)

50000

50000 (1962)

3000U

e-500H

1500U

10800

7200

3000U

4000U

e-670H

3000U

4000U

6000U

e-800H

4000U

20000

(785)

20000

(785)

20000

(785)

4500

20000

(785)

6000U

8000U

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C1 W C2

e-420HS

1500U

8000

(314)

8000

(314)

8000

(314)

7200

36000

8000

36000

3000U

e-500HS

1500U

2100

1800

3000U

e-670HS

3000U

4000U

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C1 W C2

e-420HS

1500U

50000

(1962)

50000

(1962)

50000

(1962)

50000

(1962)

50000

3000U

e-500HS

1500U

10800

7200

3000U

e-670HS

3000U

4000U

[mm/min (in/min) or deg/min]

Machine specification

X1 Y Z1 B C1 W C2

e-420HST

2000U

8000

(314)

8000

(314)

8000

(314)

7200

36000

8000

(314)

36000

Machine specification

X2

Z2

e-420HST

2000U

8000 (314)

Serial No. 294060

5. INTEGREX e-H-S

A. On turning/milling

MACHINE INFORMATION 2

B. On milling (During geometry compensation)

6. INTEGREX e-H-ST

A. On turning/milling

2-25

2 MACHINE INFORMATION

[mm/min (in/min) or deg/min]

Machine specification

X1 Y Z1 B C1 W C2

e-420HST

2000U

50000

(1962)

50000

(1962)

50000

(1962)

50000

(1962)

50000

Machine specification

X2

Z2

e-420HST

2000U

50000

(1962)

50000

(1962)

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

i-500V/5

2-pallet

8000

(314)

8000

(314)

8000

(314)

3600

i-630V/6

Single

3000

1800

2-pallet

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

i-500V/5

2-pallet

52000

(2041)

52000

(2041)

52000

(2041)

18000

36000

i-630V/6

Single

10800

2-pallet

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

e-1060V

-

8000 (314)

8000

(314)

3600

540

e-1250V/8

Single

2500

2-pallet

e-1550V

-

540

e-1600V/10

Single

2000

2-pallet

450

e-1850V

-

540

Serial No. 294060

B. On milling (During geometry compensation)

7. INTEGREX i-V

A. On turning/milling

B. On milling (During geometry compensation)

8. INTEGREX e-V

A. On turning/milling

2-26

B. On milling (During geometry compensation)

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

e-1060V

-

42000 (1653)

18900

2835

e-1250V/8

Single

10800

18000

2-pallet

e-1550V

-

18900

2835

e-1600V/10

Single

2500

(98)

2500

(98)

2500

(98)

10800

7200

2-pallet

e-1850V

-

42000 (1653)

18900

2835

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

i-630V/6

Single

8000

(314)

8000

(314)

8000

(314)

3600

3000

2-pallet

i-800V/8

Single

2-pallet

[mm/min (in/min) or deg/min]

Machine specification

X Y Z B C

i-630V/6

Single

52000

(2041)

52000

(2041)

52000

(2041)

10800

2-pallet

i-800V/8

Single

2-pallet

Serial No. 294060

9. VORTEX i-V

A. On turning/milling

MACHINE INFORMATION 2

B. On milling (During geometry compensation)

2-27

2 MACHINE INFORMATION

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

36-tool magazine

72-tool magazine

110-tool magazine

i-100

-





-

i-150

-

i-200

1000U



1500U

i-300

1000U

1500U

2500U

i-400

1000U

1500U

2500U

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

36-tool magazine

72-tool magazine

110-tool magazine

i-100S

-





-

i-100BARTAC-S

-

i-200S

1000U



1500U

i-300S

1500U

2500U

i-400S

1500U

2500U

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

36-tool magazine

72-tool magazine

110-tool magazine

i-100ST

-





-

i-100BARTAC-ST

-

i-200ST

1500U  i-300ST

1500U

i-400ST

1500U

Serial No. 294060

2-2 Magazine

This section indicates magazine.

2-2-1 INTEGREX i

2-2-2 INTEGREX i-S

2-2-3 INTEGREX i-ST

2-28

2-2-4 INTEGREX e-H

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

40-tool magazine

80-tool magazine

120-tool magazine

e-420H

1500U

  

3000U

e-500H

1500U

3000U

4000U

e-670H

3000U

4000U

6000U

e-800H

4000U

6000U

8000U

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

40-tool magazine

80-tool magazine

120-tool magazine

e-420H-S

1500U

  

3000U

e-500H-S

1500U

3000U

e-670H-S

3000U

4000U

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

40-tool magazine

80-tool magazine

120-tool magazine

e-420H-ST

2000U

  

Serial No. 294060

2-2-5 INTEGREX e-H-S

MACHINE INFORMATION 2

2-2-6 INTEGREX e-H-ST

2-29

2 MACHINE INFORMATION

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

Chain type magazine

40-tool

magazine

43-tool

magazine

80-tool

magazine

120-tool

magazine

160-tool

magazine

i-500V/5

2-pallet  -



-

i-630V/6

Single

-





2-pallet

Machine specification

Magazine capacity

Rack type magazine

180-tool magazine

240-tool magazine

348-tool magazine

i-500V/5

2-pallet



-

i-630V/6

Single



2-pallet

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

Chain type magazine

40-tool magazine

80-tool magazine

120-tool magazine

160-tool magazine

e-1060V

-

  



e-1550V

-

  



e1850V

-

  



Machine specification

Magazine capacity

Rack type magazine

42-tool magazine

84-tool magazine

120-tool magazine

162-tool magazine

e-1250V/8

Single

  



2-pallet

e-1600V/10

Single

  



2-pallet

Serial No. 294060

2-2-7 INTEGREX i-V

2-2-8 INTEGREX e-V

2-30

2-2-9 VORTEX i-V

: Standard accessory, : Special accessory, -: Not supported

Machine specification

Magazine capacity

Chain type magazine

43-tool magazine

80-tool magazine

120-tool magazine

160-tool magazine

i-630V/6

Single

  



2-pallet

i-800V/8

Single

2-pallet

Machine specification

Magazine capacity

Rack type magazine

206-tool magazine

276-tool magazine

348-tool magazine

i-630V/6

Single

  

2-pallet

i-800V/8

Single

2-pallet

Serial No. 294060

MACHINE INFORMATION 2

2-31

2 MACHINE INFORMATION

E

Serial No. 294060

2-32

3 NC COMMAND

Item

Address

Command range

Program No.

O

1 to 99999999

Sequence No.

N

1 to 99999

Preparatory function

G

0 to 999.9

Moving axis

X, Y, Z … 

B, C ... 

0 to ±99999.9999 (mm)

0 to ±9999.99999 (in)

0 to ±99999.9999 (°)

Auxiliary axis

I, J, K

0 to ±99999.9999 (mm)

0 to ±9999.99999 (in)

0 to ±99999.9999 (°)

Dwell

X

0 to 99999.999

P

0 to 99999999

Feed

F

0 to 200000.0000 (mm)

0 to 20000.00000 (in)

Fixed cycle

R, Q, P, L

0 to ±99999.9999 (mm)

0 to ±9999.99999 (in)

0 to ±99999.9999 (°)

Tool offset

H, D

0 to 999

Miscellaneous function

M

0 to 999

Spindle function

S

0 to 99999

Tool function

T

0 to 99999999

No.2 miscellaneous function

A

0 to 99999999

Subprogram

P

1 to 99999999

Variables number

#

1 to 999999

Serial No. 294060

3-1 Programming Format

3-1-1 Words and addresses

Table 3-1 Type and format of words

NC COMMAND 3

1. The number of digits in the words is checked by the maximum number of digits of the addresses.

2. When data with decimal point is used for address for which decimal input is not available, decimal figures will be ignored.

3. If the number of integral digits exceeds the specified format, an alarm will result.

4. If the number of decimal digits exceed the specified format, the excess will be rounded.

5. If “0” is set at the head of number, it is skipped. e.g. G01 = G1, M06 = M6

6. The maximum number of characters per line (per 1 block) is 248.

7. The above table shows the range of number for each command. If the command exceeds these, the alarm generates. And, do not command a value which will exceed the machine limit value (axis stroke, rotating speed ...etc).

3-1

3 NC COMMAND

File name

Assign a work number.  Any string of up to 32 characters can be used as a work number. For the use of numerals only,

however, the work number can be only up to eight digits (from 1 to 99999999).

 Characters available are letters (capital and small: A to Z and a to z), numerals, and the following

symbols: “+” “–” “_” and “.” It should be noted here that no distinction is made between capital and small letters. That is, a new program cannot be named “aBC” if a program with the name “ABC” already exists in the storage area concerned. Moreover, the program name must not begin with a period (.).

 The work number which is composed exclusively of numerals must begin with a numeral other

than zero. The leading zeros of the file name are always ignored.

Extension

Identification of an EIA/ISO program  All EIA/ISO programs must have this extension assigned.

File name

Extension

PROGRAM12345678.EIA

Serial No. 294060

3-1-2 Control out, control in

The entire information in the area from Control Out “(” to Control In “)” will be ignored in regard to machine control, while they will surely be displayed on the data display unit. Thus, this area can be used to contain information which is not directly related to control. The NC unit will enter the Control In status when power is turned on.

3-1-3 Optional block skip

Optional block skip is a function that selectively ignores that specific block within a machining program which begins with the slash code “/” or slash & number code “/1” to “/9”.

Any block beginning with “/” will be ignored if the [BLOCK SKIP] menu function is set to ON, or will be executed if the menu function is set to OFF.

3-1-4 Program end

M02, M30, M99, M998, M999 or % is used as program end code. If these commands exist in the process of the programming, the machine will stop in that block.

3-1-5 Program file name

Program file is designated as directed below. The file names here serve as the work numbers to be searched for in an automatic operation.

3-2

3-2 Command

Parameter

Description

F94 bit4

Tool command method using T-codes 0: Group-number designation 1: Tool-number designation

Code value

Description

Setting range

t1

Tool-number of the tool to be changed for

000 to Tool quantity: (Note)

t2

Tool-number of the tool to be used next

000 to Tool quantity:

t3

Group-number of the tool to be changed for

0 to 99999999

t4

Group-number of the tool to be used next

0 to 99999999

c1

Tool ID code of the tool to be changed for

00 to 26, 61 to 86

c2

Tool ID code of the tool to be used next

00 to 26, 61 to 86

Parameter

Description

F162 bit4

0: 4 digits in T-command for turning (T**00) 1: 6 digits in T-command for turning (T***000)

Serial No. 294060

1. Tool indexed function

A next tool can be designated for the machine provided with ATC function by commanding T-code in the format shown below. The next tool refers to a tool used for the next machining, which can be assigned when it is currently accommodated in the magazine. The next tool in the magazine can be indexed at ATC position beforehand by commanding the next tool, thus permitting reduced ATC time. See “2. M-code (ATC)” in “5-2 Detail of Miscellaneous Function” for more information.

(1) Programming format

[With Upper turret]

 T t1 . c1 T t2 . c2 M06 (Tool-number designation)  T t3 T t4 M06 (Group-number designation)

[With Lower turret]

 T t1 000. c1 (Tool-number designation)  T t3 (Group-number designation)

NC COMMAND 3

It depends on the setting of F94 bit4 whether Tool-number designation or Group-number designation is selected.

(2) Command data

Note : Use F162 bit4 to select the number of digits for the tool function with lower turret. The

appropriate code (“000” or “00”) should be commanded after T-code depending on setting the parameter.

3-3

3 NC COMMAND

Function

code

Group

Positioning

G00

01

Linear interpolation

G01

01

Circular interpolation (CW)

G02

01

Circular interpolation (CCW)

G03

01

Dwell

G04

00

High-speed machining mode

G05

00

Polar coordinate interpolation ON

G12.1

26

Polar coordinate interpolation OFF

G13.1

26

XY-plane selection

G17

02

ZX-plane selection

G18

02

YZ-plane selection

G19

02

Reference point return

G28

00

Return to 2nd, 3rd and 4th reference points

G30

00

Skip function

G31

00

Thread cutting

G32

01

Nose radius/Tool radius compensation OFF

G40

07

Nose radius/Tool radius compensation (left)

G41

07

Tool radius compensation for five-axis machining (left)

G41.2

07

Nose radius/Tool radius compensation (right)

G42

07

Tool radius compensation for five-axis machining (right)

G42.2

07

Tool length offset (+)

G43

08

Tool length offset in tool-axis direction

G43.1

08

Tool tip point control (Type 1) ON

G43.4

08

Tool tip point control (Type 2) ON

G43.5

08

Tool position offset OFF

G49

08

Coordinate system setting/Spindle speed range setting

G92

00

Selection of machine coordinate system

G53

00

Tool-axis direction control

G53.1

00

Selection of workpiece coordinate system 1

G54

12

Workpiece setup error correction

G54.4

27

Selection of workpiece coordinate system 2

G55

12

Selection of workpiece coordinate system 3

G56

12

Selection of workpiece coordinate system 4

G57

12

Selection of workpiece coordinate system 5

G58

12

Selection of workpiece coordinate system 6

G59

12

Selection of additional workpiece coordinate systems

G54.1

12

Dynamic offsetting II

G54.2

23

High-accuracy mode (Geometry compensation)

G61.1

13

Cutting mode

G64

13

Single user macro call

G65

00

3-D coordinate conversion ON

G68

16

3-D coordinate conversion OFF

G69

16

Serial No. 294060

2. Program code

The following table is shown Preparatory and Miscellaneous function commandable in EIA/ISO programming. See each section in “5-1 Detail of Preparatory Function” and “5-2 Detail of Miscellaneous Function” for more information.

3-4

NC COMMAND 3

Function

code

Group

Inclined-plane machining ON

G68.2

16

Inclined-plane machining (by specifying tool-axis direction) ON

G68.3

16

Inclined-plane machining OFF

G69

16

Finishing cycle

G270

09

Longitudinal roughing cycle

G271

09

Transverse roughing cycle

G272

09

Compound thread-cutting cycle

G276

09

Fixed cycle OFF

G80

09

Face driling cycle

G283

09

Face tapping cycle

G284

09

Face boring cycle

G285

09

Fixed cycle A (Longitudinal turning cycle)

G290

09

Threading cycle

G292

09

Fixed cycle B (Transverse turning cycle)

G294

09

Fixed cycle (Chamfering cutter 1, CW)

G71.1

09

Fixed cycle (Chamfering cutter 2, CCW)

G72.1

09

Fixed cycle (High-speed deep-hole drilling)

G73

09

Fixed cycle (Reverse tapping)

G74

09

Fixed cycle (Boring)

G75

09

Fixed cycle (Back spot facing)

G77

09

Fixed cycle (Tapping)

G84

09

Fixed cycle (Reaming)

G85

09

Fixed cycle (Back boring)

G87

09

Absolute data input

G90

03

Incremental data input

G91

03

Inverse time feed

G93

05

Constant surface speed control ON

G96

17

Constant surface speed control OFF

G97

17

Feed per minute (asynchronous)

G94

05

Feed per revolution (synchronous)

G95

05

Polar coordinate input ON

G16

18

Polar coordinate input OFF

G15

18

Selection between diameter and radius data input

G10.9

00

Two-Process Control by One Program

G109

00

Cross machining control ON

G110

20

Cross machining control OFF

G111

20

Function

code

Program stop

M00

Optional stop

M01

Reset and rewind

M30

Subprogram call

M98

Return to main program

M99

Tool change

M06

Dynamic offsetting ON

M173

Dynamic offsetting OFF

M174

Function for selecting the cutting conditions

M821 to M830

Serial No. 294060

3-5

3 NC COMMAND

Function

code

HD1 spindle selection

M901

HD2 spindle selection

M902

Pressing setup

M508

End of pressing

M509

Turning spindle synchronized rotation (master: turning spindle No. 1, slave: turning spindle No. 2)

M511

Turning spindle synchronized rotation (master: turning spindle No. 2, slave: turning spindle No. 1)

M512

Turning spindle synchronized rotation OFF

M513

Transfer mode ON

M540

Transfer mode OFF

M541

Balance cut start

M562

Balance cut end

M563

Waiting Command

M950 to M997

Turning spindle 1 Start of forward rotation

M203

Turning spindle 1 Start of backward rotation

M204

Turning spindle 1 Rotation stop

M205

Turning spindle 2 Start of forward rotation

M303

Turning spindle 2 Start of backward rotation

M304

Turning spindle 2 Rotation stop

M305

Start of forward milling spindle rotation

M03

Start of backward milling spindle rotation

M04

Stop of milling spindle rotation

M05

Turning spindle 1 C-axis connect/Milling mode select

M200

Turning spindle 1 C-axis disconnect/turning mode select

M202

Turning spindle 2 C-axis connect/Milling mode select

M300

Turning spindle 2 C-axis disconnect/turning mode select

M302

Spindle speed attainment check

M250

Flood coolant ON

M08

All coolant OFF

M09

Milling spindle-through coolant ON

M51

Milling spindle-through coolant OFF

M163

Flood air blast

M129

B-axis clamping

M107

B-axis unclamping

M108

Turning spindle 1 C-axis clamping

M210

Turning spindle 1 C-axis unclamping

M212

Turning spindle 1 Chuck open

M206

Turning spindle 1 Chuck close

M207

Turning spindle 2 Chuck open

M306

Turning spindle 2 Chuck close

M307

Mist collector ON

M613

Mist collector OFF

M614

Select pallet No. 1 (optional) (INTE iV/eV)

M71

Select pallet No. 2 (optional) (INTE iV/eV)

M72

Select pallet No. 1 (optional) (INTE iV/eV)

M911

Select pallet No. 2 (optional) (INTE iV/eV)

M912

Serial No. 294060

3-6

NC COMMAND 3

Serial No. 294060

 G-codes of group 00 are those which are not modal, and they are valid only for blocks in

which they are entered.

 If G-codes belong to different groups each other, any G-code can be commanded in the

same block. The G-codes are then processed in order of increasing group number. If two or more G-codes belonging to the same group are given in the same block, the G-code entered last is valid.

3-7

3 NC COMMAND

E

Serial No. 294060

3-8

4 MACHINING PROGRAM

Parameter

bit

meaning

value

description

standard

recommended

F93

3

Tool length of tool data for an EIA/ISO program

0

Invalid

1

Valid

F94

2

Tool length offset validity by G28/G30 execution

0

Canceled

1

Not canceled

F94

7

Tool offset source in EIA/ISO program

0

LENG. CO. of tool offset

1

0

1

Offset No/LENG. CO. of tool data

F114

3

Axis motion at G49 command in G43 mode

0

Axis moves

1

No movement

C-axis rotational center

Machine home position

workpiece origin

X

Z

Serial No. 294060

This chapter explains how to make a machining program.

4-1 Set Up

This section explains how to set a workpiece origin and tool offset parameter.

4-1-1 Setting of workpiece origin

This manual explains on assumption that workpiece origin is set on the C-axis center. Set the workpiece origin by a touch probe or a tool.

MACHINING PROGRAM 4

4-1-2 Parameter of tool length offset.

This manual explains how to make programs when below parameters are set as recommended. With the recommended setting, tool length data is taken from MAZATROL tool data, and (additional) tool length offset is taken from tool offset data.

Parameter of Tool length offset

4-1

4 MACHINING PROGRAM

Pattern

Data items used

Parameter

Programming

format

F94 bit 7

F93 bit 3

[1]

Tool offset

Tool offset No.

0

G43H

[2]

MATATROL Tool Data

Length

1

T + G43

Length + Offset No. Length + LENG. CO.

T + G43H

[3]

Offset No. LENG. CO.

1

0

G43 H

[4]

Tool offset No. + Tool Data

Tool offset No. + Length

0

1

T + G43H parameter

bit

meaning

value

description

standard

recommended

F92

7

Radius/NOSE-R in the Tool Data display for an EIA/ISO program

0

invalid

0/1

1

valid

F94

7

Tool offset amount effectuated in an EIA/ISO program

0

ACT-CO. of tool offset

1

0

1

OFFSET No. of tool data

ACT-CO. of tool data

Pattern

Data items used

Parameter

Programming

format

F92 bit 7

F94 bit 7

[1]

Tool offset No.

0

G41/G42 D

[2]

Tool Data (MAZATROL)

Radius + OFFSET No. NOSE-R/Radius + ACT-CO.

1

G41/G42 T

[3]

ACT-CO. OFFSET No.

0

1

G41/G42 T

[4]

Tool Offset + Tool Data

Tool offset No. + NOSE-R/Radius

1

0

G41/G42 D + T

recommended

Serial No. 294060

Tool length offsetting

4-1-3 Parameter for Nose / Tool radius compensation

This manual explains how to make machining programs when below parameters are set by the recommended value. With the recommended setting, nose R or tool diameter data is taken from MAZATROL tool data, and (additional) tool radius offset is taken from tool offset data.

Parameter for Nose/Tool radius compensation

Note : Standard parameter of “F92bit7”: i150->0 i200/400/300->1

Tool radius compensation

4-2

4-2 Programming Composition

Preparation for machining

1. Turret selection

2. Head selection

3. Modal command

4. Home return

5. Tool change

6. Home return after tool change

7. B-axis positioning

8. Spindle rotation command

9. Radius/Diameter data input

10. Coolant command

11. Others

Machining motion

A

Turning

Approach

Turning

Escape

B

Drilling

Approach

Hole

Escape

C

3-axis

Approach

3-axis

Escape

D

4-axis

Approach

4-axis

Escape

E

5-axis

Approach

5-axis

Escape

End motion for machining

1. Coolant stop command

2. Rotation stop command

3. Home return

4. Program end

Serial No. 294060

This section explains programming composition.

4-2-1 Programming composition

The figure shows program composition which is explained in this manual.

The program consists of three compositions: “Preparation motion for machining”, “Machining

motion”, and “End motion for machining”.

Machining motions are selected from A-E according to machining processes. Figure. Program composition

MACHINING PROGRAM 4

4-3

4 MACHINING PROGRAM

2.Head selection

1.Turret selection

3.Modal command

4.Home return

5.Tool change

6.Home return after tool change

7.B-axis positioning

8.Rotation command

9.Radius/Diameter

10.Coolant

G109L1 M901 M200 M212 G00G90G94 G54G97 G40G49G80G67G69 G91 G28X0 G28Z0 G28Y0 T001T002.15M06 G91 G28X0 G28Z0 G28Y0 M108 G90G53B90.0 G97S12000M03 G10.9X0 M08

Preparation motion for machining

4-3-2 1.

4-3-2 2.

4-3-2 3.

4-3-2 4.

4-3-2 5.

4-3-2 6.

4-3-2 7.

4-3-2 10.

4-3-2 9.

4-3-2 8.

Serial No. 294060

4-2-2 Method of making program

This section explains how to make a machining program. First command steps 1. to 10. (or 11.) of Preparation for machining. Select A-E in Machining motion. Command steps 1. to 4. In End motion for machining.

See 4-6 besides 4-3, 4-4 and 4-5 for Programming for Compound Machining. 4-6 explains method of making one program for multi-process, waiting command and transfer operation.

4-4

MACHINING PROGRAM 4

1. Rotation stop command

2. Coolant stop command

3. Home return

4. Program end

M05 M09 G91G28X0 G28Z0 G28Y0 M108 G90G53B0 M30

End motion for machining

4-5-2 1.

4-5-2 2.

4-5-2 3.

4-5-2 4.

Machining Motion

Turining

Milling

Drilling

Turining

Hole

3-axis

4-axis

5-axis

Inclined-Plane

Polar Coodinate Interpolatio

5-axis machining

Tool Radiuus Compensation

for 5-axis

4-4-1 1.

4-4-1 2.

4-4-2 1.

4-4-3 1.

4-4-3 2.

4-4-5 1.

4-4-5 2.

4-4-4 1.

Serial No. 294060

4-5

4 MACHINING PROGRAM

Upper turret & HD1 Lower turret & HD2

4-6-2 3. A, B

Dual workpiece program

Upper turret & HD2 Lower turret & HD1

4-6-2 3. C, 0

Transfer

4-6-2 4. A

Transfer

Note: INTE i-S can be used.

Programming for Compound Machining (for INTE i-ST)

Separate machining program

Parallel

machining of

HD1 sides

4-6-2 2. A

Upper turret & HD1

4-6-2 1. A

Lower turret & HD1

4-6-2 1. B

Lower turret & HD2

4-6-2 1. C

Parallel machining program

Parallel

machining of

HD2 sides 4-6-2 2. B

Upper turret & HD2

4-6-2 1. D

Serial No. 294060

4-6

4-3 Preparation Motion for Machining

G109L1: Upper turret G109L2: Lower turret

G109L1 M901 M200 M212

G00G90G94 G54G97 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001T002M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B90.0

G97S12000M03 G10.9X0 M08

HD1 Upper turret Milling

G109L1 M901 M202

G00G18G90G95G54G96 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001.1T002.15M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B90.0

G92S3000R1 G96S150M204 G10.9X1 M08

HD1 Upper turret Turming

Preparation motion for machining

Serial No. 294060

This section explains “Preparation motion for machining”.

4-3-1 Sample program

This figure shows sample programs for preparation for machining. Refer to 4-3-2 for more information about each motion.

MACHINING PROGRAM 4

4-3-2 Preparation for machining

Each motion of “Preparation for machining” is explained 1.-11.. Select the motions to suit machining method

1. Turret selection

Select a turret to use. As “INTE i series” and “INTE is series” have no lower turret, all machining are selected as upper turret. So these machines do not require these commands.

4-7

4 MACHINING PROGRAM

HD1

HD2

X

Z

M901: HD1 spindle selection

M200: Turning spindle 1

C-axis connect/Milling mode select

M202: Turning spindle 1

C-axis disconnect/turning mode select

M210: Turning spindle 1 C-axis clamping M211: Turning spindle 1 C-axis braking M212: Turning spindle 1 C-axis

unclamping

M902: HD2 spindle selection

M300: Turning spindle 2

C-axis connect/Milling mode select

M302: Turning spindle 2

C-axis disconnect/turning mode select

M310: Turning spindle 2 C-axis clamping M311: Turning spindle 2 C-axis braking M312: Turning spindle 2 C-axis

unclamping

M-codes for Head selection

Upper turret

G109L1

Lower turret

G109L2

Serial No. 294060

2. Head selection

Select a head according to machining method. Select milling-mode or turning-mode for the head. Command a turning spindle clamp code if a milling-mode is selected.

* INTE i-V/e-V cannot issue M-codes for head selection (M901/M902).

4-8

3. Modal command

Group

G-codes

Function

1 G0

Positioning G1

Linear interpolation

2 G17

XY-plane selection

G18

ZX-plane selection

G19

YZ-plane selection

3

G90

Absolute data input

G91

Incremental data input

5 G94

Feed per minute (asynchronous)

G95

Feed per revolution (synchronous)

6

G20

Inch data input

G21

Metric data input

7

G40

Nose/Tool radius compensation OFF



8

G49

Tool position offset OFF

 9 G80

Fixed cycle OFF



12

G54

Selection of workpiece coordinate system



G55-G59

14

G67

Modal user macro call OFF



16

G69

Inclined-plane machining OFF



17

G96

Constant surface speed control ON

G97

Constant surface speed control OFF

HD1

HD2

C1

unclamping

M901 M202

M902 M302

M901 M200 M210

M901 M200 M211

M901 M200 M212

M902 M300 M310

M902 M300 M311

M902 M300 M312

turning

milling

turning

milling

C1

Clamping

C1

Brake

C2

unclamping

C2

Clamping

C2

Brake

Serial No. 294060

This figure shows modal G-codes. Initial condition G-codes may be commanded at the head of program for the case they are not cancelled by previous operation (for example command G80 to cancel G82 left by the previous operation).

The codes marked with  are automatically selected in each group upon power-on or reset for initializing the modal G codes. So they may not be commanded to start operation but sample program includes those G code commands for a sake of safety.

MACHINING PROGRAM 4

4-9

4 MACHINING PROGRAM

G91G28X0 (X-axis home return) G28Y0 (Y-axis home return) G28Z0 (Z-axis home return)

Home return after tool change

(The order of home return is XYZ)

T001T002M06 (Tool changed for No.1 , and set No.2 as next tool)

T001.11T002.15M06 (Tool changed for No.1-K, and set No.2-P as next tool)

No Tool ID command

Tool ID command

G91G28X0 (X axis home return) G28Z0 (Z axis home return) G28Y0 (Y axis home return)

(The order of home return XZY)

Home return

G00G18G90G94G54G97 G40G49G80G67G69

Modal command

Note: It is not necessary to command G-codes that are not changed. (G21 etc.)

Serial No. 294060

4. Home return

Home returns are commanded before tool change. Change the order of the home returns, depending on the turret position.

Sample program shows the order of X-Z-Y.

5. Tool change

Tool change is performed. Sample programs show tool change commands with no suffix and with suffix.

Refer to [99 Supplement] for the detail of tool change command.

6. Home return after tool change

Change the order of Home return like “4”.

4-10

MACHINING PROGRAM 4

Milling Spindle (G109L1)

M03: Start of forward

milling spindle rotation

M04: Start of reverse

milling spindle rotation

(M05: Stop of milling spindle rotation)

Turning spindle 1

M203: Turning Spindle 1

start of forward rotation

M204: Turning Spindle 1

start of reverse rotation

(M205: Turning spindle 1 Rotation stop)

Turning spindle 2

M303: Turning spindle 2

start forward rotation

M304: Turning spindle 2

start reverse rotation

(M305: Turning spindle 2 Rotation stop)

Milling spindle (G109L2)

M03: Start of forward

milling spindle rotation

M04: Start of reverse

milling spindle rotation

(M05: Stop of milling spindle rotation)

M108 (B-axis unclamping) G90G53B***.** (B-axis positioning)

B-axis positioning

M108 (B-axis unclamping) G90G53B***.** (B-axis positioning) M107 (B-axis clamping)

B-axis positioning(In case of turning)

Serial No. 294060

7. B-axis positioning

Perform B-axis positioning. If the B axis is already indexed, it is not necessary to command B positioning here.

For turning, command B axis clamp (Turning spindle does not turn if B axis is being unclamped).

8. Spindle rotation command

Command a rotation for Turning-Spindle/Milling-Spindle. M-codes are shown in the figure below. S-address means rotational speed (G97) or surface speed (G96) by modal G-code group 17. In case of Mill-machining, G96 cannot be used.

When G96 is used, command G92 to set the maximum min-1.

4-11

4 MACHINING PROGRAM

D740PB006

Lower turret

Upper turret

R1

Turning spindle 2

Turning spindle 1

R2

R1

R2

G92S3000R1 G96S150R1M204

Rotational command

Maximum spindle speed is set to 3000 min-1. Turning spindle1 is set to 150 m/min(reverse)

(In case of select

Turning spindle1 & Upper turret)

G97S12000M03

Rotational command

Rotation of the milling spindle at 1200 min-1

Serial No. 294060

Command for rotation speed

Command for Constant surface speed

R command

1. Spindle for speed clamping is to be set by address R. R1: Turning spindle (see the figure below)

R2: Turning spindle (see the figure below) R3: Milling spindle

4-12

MACHINING PROGRAM 4

M-codes

Function

Cancel

M08

Flood coolant ON

M09

M51

Milling spindle through coolant

M163

M129

Flood air blast

M08: Flood coolant M51: Mill spindle through coolant M129: Flood air blast

Machining zero point

100

Radius data input: X 50.0 X

Z

50

G10.9X1: Diameter data input G10.9X0: Radius data input

Serial No. 294060

9. Radius/Diameter data input

Select the Diameter / Radius data input by machining method. Usually, diameter data input is selected for turn-machining, and radius data input is selected for mill-machining.

Radius/Diameter data input

10. Coolant command

Command a coolant code by machining method.

All the coolant codes must be cancelled by a cancel code, M9, in “End motion for machining”, if

they have been turned on. This Table shows coolant M-codes. Check if they are available before commanding. Coolant M-codes

Coolant locations

4-13

4 MACHINING PROGRAM

M821

Accuracy level 1

M822

Accuracy level 2

M823

Accuracy level 3

M824

Accuracy level 4

M825

Accuracy level 5

M826

Accuracy level 6

M827

Accuracy level 7

M828

Accuracy level 8

M829

Accuracy level 9

M830

Accuracy level 10

M613: Mist collector ON M614: Mist collector OFF

Highest Speed

Highest accuracy

Serial No. 294060

11. Others

Command any as required besides above ten commands. This section explains “cutting level selection M codes” and mist collector.

A. Accuracy level (M821 to M830) (Option: High-Speed Smoothing Control)

Each work piece can be machined under the specific cutting conditions by specifying one of the ten accuracy levels.

The accuracy level is to be specified either by an M-code in the program or manually in the CUTTING LEVEL SELECT window.

This Table shows M-code input method. M-codes

B. Mist collector (M613) (Option)

This code starts and stops mist collector.

4-14

4-4 Machining Motion

G109L1 M901 M202

G00G18G90G95G54G97 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001.1T002.15M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B0.0

M107 G97S2000M204 G10.9X1 M08

G90G43G0X0.0Y0Z5.0 H1P1

M250 G274R1.0 G274X0Z-50.0P0Q15.0F0.2

G0X300.0Z50.0

G80

M205 M09

G91G28X0 G28Z0 G28Y0

M30

Preparation Motion for machining

• G109L1: Upper turret selection

• M901: HD1 spindle selection

• M202: C-axis disconnect / turning mode

• G95: Feed per revolution

• G97: Constant surface speed control OFF

• T001.1M6: Tool change (TNo.01.A)

• B-axis positioning

• M107: B-axis clamping

• G97S2000: Rotation speed 2000 min-1

• M204: Turning spindle1 backward rotation

• G10.9X1: Diameter data input mode

• M08: Flood coolant ON.

End motion

• M205: Turning spindle1 Rotation stop

• M09: All coolants OFF

• Each axis positioning to zero return

• M30: Reset and rewind

Machining motion

• G43H**P1: Tool length offset

• M250: Spindle speed attainment check

• G274: Longitudinal cut-off cycle

• G80: Fixed cycle OFF

(Turning operation – Turn drilling operation)

Serial No. 294060

This section explains “Machining motion”.

This section describes “program composition”, “parameter setting” and “sample program” for

each machining method.

4-4-1 Turning program

This section explains turning operation programs.

1. Turn–drilling operation

Turn-drilling needs to use a G97 (Constant surface speed control OFF) as it cuts at the spindle center.

A. Sample program

MACHINING PROGRAM 4

4-15

4 MACHINING PROGRAM

Parameter

bit

Standard

Setting

Description

F114

3 1 1

Moving axes by using G49 (tool length offset cancel) in G43 (tool length offset) mode Invalid

SU104

-

Pecking return distance in grooving (G274/G275, G74/G75)

G00G90G43XxYyZzHhP1 M250 M107

G274Rr G274X0ZzQqFf G0XxZz G80

Machining motion of program composition – Turn–drilling operation

--- Tool Length offset (for Turning)

--- Spindle speed attainment check

--- B-axis clamping

--- G274 input

--- G274 input (X address is zero)

--- Escape

--- Fixed cycle (G274) OFF

Command in

machining motion

Command in

preparation motion

for machining

Upper turret

HD1

Turning

Tool length offset (P1)

Compound fixed cycle

Program composition element

Serial No. 294060

B. Program composition

C. Relevant parameter setting

The main parameter of processing is described. The table shows the standard parameter and setting set in this manual.

Parameter setting

4-16

MACHINING PROGRAM 4

G-codes

Group

Description

G43P1

8

Tool length offset (+)

For turning tools

G274

9

Longitudinal cut-off cycle

G80

9

Fixed cycle OFF

TEP141’

i

d

A

x

z

k

e

Serial No. 294060

D. G-codes / M-codes

See the document [99 Supplement] for details. G-codes

 Longitudinal cut-off cycle G274

1. Programming format

G274 Re; G274 Xx Zz Pi Qk Rd Ff Ss;

e : Return distance

The value is modal and remains valid until it is overwritten with a new value. x : Final X-axis position in absolute/incremental data z : Final Z-axis position in absolute/incremental data

i : X-axis movement step (in an absolute value) k : Z-axis depth of cut (in an absolute value) d : Tool escape distance at the bottom of cut

Normally set in an absolute value. When omitting the arguments X and P,

however, set the value with a sign as required for the direction of escape. f : Feed function (rate of feed) s : Spindle function

The distance “e” is set by parameter SU104 (pecking return distance in grooving process).

4-17

4 MACHINING PROGRAM

M-codes

Description

M107

B-axis clamping

M108

B-axis unclamping

M250

Spindle speed attainment check

G codes

Function

G270

Finishing cycle

G271

Longitudinal roughing cycle (leaving finishing allowance)

G272

Transverse roughing cycle (leaving finishing allowance)

G273

Contour-parallel roughing cycle



G274

Longitudinal cut-off cycle

G275

Transverse cut-off cycle

G276

Compound thread-cutting cycle

Serial No. 294060

M-codes

Compound Fixed Cycles

Note :  is G-code used by sample program.

See the programming manual, if you use the other patterns.

4-18

2. Turning machining

Preparation motion for machining

 G109L1: Upper turret selection  M901: HD1 spindle selection  M202: C-axis disconnect/Turning mode  G18: ZX-plane selection  G95: Feed per revolution  G96: Constant surface speed control ON  T001.1M06: Tool change (TNo.01.A)  B-axis positioning  G271: Longitudinal roughing cycle  G92S3000: Spindle speed range setting  G96S120: Surface speed 120 m/min  M204:Turning spindle1 backward rotation  G10.9X1: Diameter data input mode  M08: Flood coolant ON.

End motion for machining

 M205: Turning spindle1 rotation stop  M09: All coolants OFF  Each axis positioning to zero return  M30: Reset and rewind

Machining motion

 G43H**P1: Tool length offset  M250: Spindle speed attainment check  M107: B-axis clamping  N115-N116: Machining contour  G42D**: Nose radius compensation(right)  G40: Nose radius compensation OFF  G80: Fixed cycle OFF

Machining contour

(Turning Machining_ Longitudinal roughing cycle)

G109L1 M901 M202

G00G18G90G95G54G96 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001.1T002.15M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B90.0

M107 G92S3000R1 G96S120M204 G10.9X1 M08

G90G43G0X300.0Y0 Z3.0 H1P1

M250 G271U2.0R1.0 G271P115Q116U0.3W0.1F0.25 N115G42G0X53.0 Z3.0 D51

G1X60.0Z-0.5F0.1 Z-20.0 X95.0 X96.0Z-20.5 Z-40.0 X115.0 X116.0Z-40.5 Z-80.0 X125.0Z-81.0

N116X130.0

G0X300.0Z50.0

G40G80 M205

M09

G91G28X0 G28Z0 G28Y0 M108 G90G53B0

M30

Serial No. 294060

This section explains Turn-machining.

A. Sample program

MACHINING PROGRAM 4

4-19

4 MACHINING PROGRAM

Parameter

bit

Standard

Setting

Description

F114

3 1 1

Moving axes by using G49 (tool length offset cancel) in G43 (tool length offset) mode Invalid

SU102

-

Return distance in Z-axis at wall during rough cutting in bar machining or in corner machining

SU103

-

Cutting depth in the composite-type fixed cycle

G00G90G43XxYy Zz HhP1

M250 G271UdRr G271PpQqUuWwFf NpG41(G42) DdG0Xx Zz

(Finishing contour) NqXxZz G0XxZz G40G80

Machining motion of program component –Turning machining-

--- Tool length offset (for turning tool) This point will be a cycle start point.

--- Spindle speed attainment check

--- G271 input( details shown on other page)

--- G271 input

--- Head block for finishing contour Nose radius compensation

--- Turning for work shape

--- End block for finishing contour

--- Escape

--- Nose radius compensation OFF Fixed cycle OFF

Same value

with cycle

start block

Instruction in

preparation motion

for machining

Instruction in

machining motion

Upper turret

HD1

Turning

Tool length offset(P1)

Nose radius compensation

Compound fixed cycles

Program composition element

Serial No. 294060

B. Program composition

C. Parameter setting

The main parameter of processing is described. The table shows the standard parameter and setting set in this manual.

Parameter setting

Note : SU103 and SU102 are to be used respectively as arguments R (SU102) and U

(SU103), when R or U in G271 is omitted.

4-20

MACHINING PROGRAM 4

G-codes

Group

Description

G43P1

8

Tool length offset (+)

G271

9

Longitudinal roughing cycle

G41

7

Nose radius/Tool radius compensation (left)

G42

7

Nose radius/Tool radius compensation (right)

G40

7

Nose radius/Tool radius compensation OFF

G80

9

Fixed cycle OFF

Serial No. 294060

D. G-codes/M-codes

See the document [99 Supplement] for details. G-codes

 Longitudinal roughing cycle G271

1. Programming format G271 Ud R_

G271 A_ P_ Q_ Uu W_ F_ S_ T_

Ud : Depth of cut

Set an absolute value (in radius value). The value is modal and remains valid until it is overwritten with a new value.

R : Escape distance

The value is modal and remains valid until it is overwritten with a new value. A : Finishing contour program No. P : Head sequence No. for finishing contour Q : End sequence No. for finishing contour Uu : Finishing allowance and direction along the X-axis

(in diameter or radius value) W : Finishing allowance and direction along the Z-axis F_S_T_ : Feed, Spindle and Tool functions

The roughing cycle is executed using the F-, S- and T-functions specified in or before the G271 block, in stead of those existing in the program section designated by P and Q.

Note 1: Even if F- and S-codes exist in the program section designated by P and Q, they

are considered as for the finishing cycle only and, therefore, ignored in the roughing cycle.

Note 2: d and u are both specified with address U. The differentiation depends on

whether P and Q are specified in the same block.

Note 3: The block of G271 Ud R_ can be omitted when the external settings in

parameters SU103 and SU102 are to be used respectively as arguments U (d) and R.

4-21

4 MACHINING PROGRAM

M-codes

Description

M107

B-axis clamping

M108

B-axis unclamping

M250

Spindle speed attainment check

G codes

Function

G270

Finishing cycle



G271

Longitudinal roughing cycle (leaving finishing allowance)

G272

Transverse roughing cycle (leaving finishing allowance)

G273

Contour-parallel roughing cycle

G274

Longitudinal cut-off cycle

G275

Transverse cut-off cycle

G276

Compound thread-cutting cycle

Serial No. 294060

M-codes

Compound Fixed Cycles

Note :  is G-code used by sample program.

See the programming manual, if you use the other patterns.

4-22

4-4-2 Hole machining program

G109L1 M901 M200 M212

G0G90G94G55G97 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001T00M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B45.0

G97S2500M03 G10.9X0 M08

M212M108 G68.2P1X0Y0Z0I0J45K0 G53.1 M210M107

G90G43G00X42.271Y7.62Z3.H1

G82Z-1.R3.F115.

Y0. Y-7.62

G80

Z50.0

G69

M05 M09

G91G28X0 G28Z0 G28Y0 M108 G90G53B0

M30

Preparation motion for machining

 G109L1: Upper turret selection  M901: HD1 spindle selection  M200: C-axis connect/Milling mode select  M212: C-axis unclamping  G94: Feed per minute  G97: Constant surface speed control OFF  T001M06: Tool change (TNo.01)  B-axis positioning  G97S2500: Rotation speed 2500 min-1  M03: Mill spindle forward rotation  G10.9X0: Radius data input mode  M08: Flood coolant

Machining motion

 M212M108: Rotation axes unclamping  G68.2: Inclined-plane machining  P1: Using roll, pitch, and yaw angles  G53.1: Tool-axis direction control  M210M107: Rotation axes clamping  G43H**(P0): Tool length offset  G82: Drilling cycle  (Drilling motion)  G80: Fixed cycle OFF  G69: Inclined-plane machining OFF

End motion for machining

 M05: Stop of milling spindle rotation  M09: All coolants OFF  Each axis positioning to zero return  M30: Reset and rewind

(Drill fixed cycle )

Serial No. 294060

This section explains how to make hole-machining program.

1. Hole machining

This section explains hole machining program using fixed cycles.

A. Sample program

MACHINING PROGRAM 4

4-23

4 MACHINING PROGRAM

Parameter

bit

Standard

Setting

Description

F34

4 0 0

Programming type for inclined-surface machining. Always select type A

F114

3 1 1

Moving axes by using G49 (tool length offset cancel) in G43 (tool length offset) mode Invalid

F144

1 0 1

Selection of table rotary axis reference position for inclined-surface machining Table rotary axis 0-degree position as the reference

M108M212 G68.2P1XxYyZzIiJjKk

G53.1 M107M210 G90G43G00XxYyZzHh G82ZzRrFf (Drilling positioning) G80 G69

Processing operation of program component –Hole machining-

--- Rotation axes unclamping

--- Inclined-Plane machining Using roll, pitch, and yaw angle

--- Tool axis direction control

--- Rotation axes clamping

--- Tool length offset

--- Hole-machining fixed cycle

--- Drilling positioning

--- Fixed cycle OFF

--- Inclined-plane machining OFF

Because BC axes are moved by G53.1. Rotation axes have to clamp

G82

G80

Fixed cycle G68.2

G69

Inclined-plane machining

The figure below indicates setting each mode.

Instruction in

machining motion

Instruction in

preparation motion

for machining

Program composition element

Upper turret

HD1

Milling

Tool length offset(P0)

Inclined-plane machining

Using roll, pitch, and yaw angle

Hole fixed cycle

Serial No. 294060

B. Program composition

C. Parameter setting

The main parameter of processing is described. The table shows the standard parameter and setting set in this manual.

Parameter setting

Note 1: Type A: Combined use with the other 5-axis machining functions, and cannot allow

interruption during Inclined-Plane machining

Note 2: Type B: Combined cannot use with the other 5-axis machining functions, and allowing

interruption during Inclined-Plane machining

4-24

MACHINING PROGRAM 4

G-codes

Group

Description

G68.2P1

16

Inclined-plane machining ON

Using roll, pitch, and yaw angles

G53.1

0

Tool-axis direction control

G43

7

Tool length offset (+)

G82

9

Fixed cycle (Drilling)

G codes

Description

G68.2[P0]

Using Eulerian angles



G68.2P1

Using roll, pitch, and yaw angles

G68.2P2

Using three points in the plane

G68.2P3

Using two vectors

G68.2P4

Using projection angles

G68.3

Using tool-axis direction

q

Axis of the first rotation

Axis of the second rotation

Axis of the third rotation

123

X-axis

Y-axis

Z-axis

132

X-axis

Z-axis

Y-axis

213

Y-axis

X-axis

Z-axis

231

Y-axis

Z-axis

X-axis

312

Z-axis

X-axis

Y-axis

321

Z-axis

Y-axis

X-axis

Serial No. 294060

D. G-codes/M-codes

See the document [99 Supplement] for details. G-codes

Inclined-Plane Machining

Note :  is G-code used by sample program.

See the programming manual, if you use the other patterns.

 G68.2P1 Setting with roll, pitch, and yaw angles

1. Programming format G68.2 P1 Qq Xx Yy Zz I J K

G68.2 P1: Inclined-plane machining ON (Setting with roll, pitch, and yaw angles) x, y, z: Coordinates of the origin of feature coordinate system. To be specified with

its absolute values in the currently active workpiece coordinate system.

q: Order of rotations

: Angle of rotation around the X-axis [Roll angle]. : Angle of rotation around the Y-axis [Pitch angle]. : Angle of rotation around the Z-axis [Yaw angle].

(Setting range: –360° to 360°.)

1. The designation of X, Y, or Z can be omitted when the argument is zero (0: no shift along the particular axis). Set zero for X, Y, and Z if no translation of the origin is required.

2. The designation of I, J, or K can be omitted when the argument is zero (0: no rotation around the axis concerned).

4-25

4 MACHINING PROGRAM

G-codes

Description

G-codes

Description

G73

High-speed deep-hole drilling

G82.2

Pecking

G74

Reverse tapping

G83

Deep-hole drilling

G75

Boring 1 G84

Tapping

G76

Boring 2 G84.2

Synchronous tapping

G77

Back spot facing

G84.3

Synchronous reverse tapping

G78

Boring 3 G85

Reaming G79

Boring 4 G86

Boring 5

G81

Spot drilling G87

Back boring



G82

Drilling G88

Boring 6

G89

Boring 7

GX_Y_Z_Q_R_P_D_K_I_J(B)_E_H_F_L_

Hole position data

Repeat times Hole-machining data

Hole-machining mode

Conversion by means of roll, pitch, and yaw angles

Zw

Xw

Yw

z y x



Xw

Zw

Yw

y1

z1

Workpiece coordinate

system

1) Translation of the system

2) Rotation on Xw by °

3) Rotation on Yw by °

D740PB0096

Yw

z

Z

X

y

Y

Zw

Xw

x

Xw

Zw

Yw

y1 z1

y2 z2  x2

Xw

Zw

Y

z2

y2

Z

x2 X Yw



4) Rotation on Zw by °

Feature coordinate system

Serial No. 294060

3. Use of any other addresses than P, Q, X, Y, Z, I, J, and K will lead to an alarm (1809 TILTED PLANE CMD FORMAT ERROR).

4. Argument Q can be omitted if Q123 is required.

5. The designation of Q with any other value than enumerated above will lead to an alarm (1809 TILTED PLANE CMD FORMAT ERROR).

Fixed Cycles

Note :  is G-code used by sample program.

See the programming manual, if you use the other patterns.

 Setting fixed-cycle machining data

Set fixed-cycle machining data as follows:

 Hole-machining mode (G-code)

See the list of the fixed cycles.

4-26

MACHINING PROGRAM 4

M-codes

Description

M107

B-axis clamping

M108

B-axis unclamping

M210

Turning spindle 1 C-axis clamping

M212

Turning spindle 1 C-axis unclamping

Serial No. 294060

 Hole position data (X, Y)

Set hole positions using incremental or absolute data.

 Hole-machining data

Z .... Set the distance from R-point to the hole bottom using incremental data, or set the

position of the hole bottom using absolute data.

Q ... Set this address code using incremental data. (This address code has different

uses according to the type of hole-machining mode selected.)

R ... Set the distance from the initial point of machining to R-point using incremental

data, or set the position of R-point using absolute data.

P.... Set the desired time or the number of spindle revolutions, for dwell at the hole

bottom. (Set the overlapping length for the chamfering cutter cycles G71.1 and G72.1.)

D ... Set this address code using incremental data. (This address code has different

uses according to the type of hole-machining mode selected.)

K.... Set this address code using incremental data.

(This address code has different uses according to the type of hole-machining mode selected.)

I ..... Set the feed override distance for the tool to be decelerated during the last cutting

operation of drilling with a G73, G82, or G83 command code.

J(B) ... For G74 or G84, set the timing of dwell data output; for G75, G76, or G87, set

the timing of M3 and M4 output, or; for G73, G82, or G83, set the feed override

ratio for deceleration during the last cutting operation.

E.... Set a cutting feed rate (for G77, G79 and G85).

H ... Select synchronous/asynchronous tapping cycle and set the return speed override

during a synchronous tapping cycle.

F .... Set a cutting feed rate.

 Repeat times (L)

If no data is set for L, it will be regarded as equal to 1. If L is set equal to 0, hole-machining will not occur; hole-machining data will only be stored into the memory.

M-codes

4-27

4 MACHINING PROGRAM

(3-axis machining_Inclined plane)

G109L1 M901 M200 M212

G0G90G94G55G97 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001T00M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B0.0

G97S1000M03 G10.9X0 M08

G61.1 M108M212 G68.2 P1X10.0 Y0 Z0 I-60.0 J0 K0 G53.1 M107M210

G90 G43 X30.0 Y90.0 Z20.0 H1 G1 Z15.0 F500 Y-90.0 (Machining contour) Y-90.0 Z3. G0 Z50.0

G69 G64

M05 M09

G91G28X0 G28Z0 G28Y0 M108 G90G53B0

M30

Preparation motion for machining

 G109L1: Upper turret selection  M901: HD1 spindle selection  M200: C-axis connect/Milling mode select  M212: C-axis unclamping  G94: Feed per minute  G97: Constant surface speed control OFF  T001M06: Tool change (TNo.01)  B-axis positioning  G97S1000: Rotation speed 1000 min-1  M03: Milling spindle forward rotation  G10.9X0: Radius data input mode  M08: Flood coolant ON

End motion for machining

 M05: Stop of milling spindle rotation  M09: All coolants stop  Each axis positioning to zero return  M30: Reset and rewind

Machining motion

 G61.1: Geometry compensation  M108M212: Rotation axes unclamping  G68.2: Inclined-plane machining  P1: Using roll, pitch, and yaw angles  G53.1: Tool-axis direction control  M107M210: Rotation axes clamping  G43H**(P0): Tool length offset  (Machining contour)  G69: Inclined-plane machining OFF  G64: Geometry compensation OFF

Machining contour

Serial No. 294060

4-4-3 3-axis machining program

This section explains 3-axis machining programs.

1. Inclined-plane machining

This section explains 3-axis machining program using the G68.2 inclined plane machining mode.

A. Sample program

4-28

MACHINING PROGRAM 4

Parameter

bit

Standard

Setting

Description

F34

4 0 0

Programming type for inclined-surface machining Type A

F114

3 1 1

Moving axes by using G49 (tool length offset cancel) in G43 (tool length offset) mode Invalid

F144

1 0 1

Selection of table rotary axis reference position for inclined-surface machining Table rotary axis 0-degree position as the reference

G61.1 M108M212 G68.2 P1XxYyZzIiJjKk

G53.1 M107M210 G90G43XxYyZzHh G1XxYyZzFf (Machining nontour) G0XxYyZz G69 G64

Machining motion of program composition –Inclined plane machining-

--- Geometry compensation

--- Rotation axes unclamping

--- Inclined-plane machining Using roll, pitch, and yaw angle

--- Tool-angle direction control

--- Rotation axes unclamping

--- Tool length offset

--- Head block for machining contour

--- machining contour

--- Escape

--- Inclined-plane machining

--- Geometry compensation OFF

G68.2

G69

Geometry compensation

G61.1

G64

Inclined-plane machining

Command G68.2 while in the G61.1 mode.

BC axes need to be unclamped prior to G53.1. as G53.1 indexes the rotary axes.

Instruction in

preparation motion

for machining

Instruction in

machining motion

Upper turret

HD1

Milling

Tool length offset

Inclined-plane machining

Roll, pitch, and yaw angle

Geometry compensation

Program composition element

Serial No. 294060

B. Program composition

C. Parameter setting

The main parameter of processing is described. The table shows the standard parameter and setting set in this manual.

Parameter setting

Note 1: Type A: Combined use with the other 5-axis machining functions, and cannot allow

Note 2: Type B: Combined cannot use with the other 5-axis machining functions, and allowing

interruption during Inclined-Plane machining

4-29

4 MACHINING PROGRAM

G-codes

Group

Description

G61.1

13

High-accuracy mode (Geometry compensation)

G68.2P1

16

Inclined-plane machining ON

Using roll, pitch, and yaw angles

G53.1

0

Tool-axis direction control

G43

8

Tool length offset (+)

G69

16

Programmed coordinate rotation OFF

G64

13

Cutting mode (Geometry compensation OFF)

G codes

Description



G61.1

Geometry compensation

G61.2

Modal spline interpolation

G codes

Description

G68.2[P0]

Using Eulerian angles



G68.2P1

Using roll, pitch, and yaw angles

G68.2P2

Using three points in the plane

G68.2P3

Using two vectors

G68.2P4

Using projection angles

G68.3

Using tool-axis direction

M-codes

Description

M107

B-axis clamping

M108

B-axis unclamping

M210

Turning spindle 1 C-axis clamping

M212

Turning spindle 1 C-axis unclamping

Serial No. 294060

D. G-codes/M-codes

See the document [99 Supplement] for details. G-codes

Note : The geometry compensation reduces geometry errors caused by the delay in the

High-accuracy mode

smoothing circuits and servo systems.

Note 1:  is G-code used by sample program. Note 2: G61.2 is a geometry compensation with fine spline interpolation feature for a further

better quality surface for the CAM-made minute increments block by block data operation.

Inclined-Plane Machining

Note 1:  is G-code used by sample program.

See the programming manual, if you use the other patterns.

Note 2: See the document [supplement] or “4-4-2 1. Hole machining” for details of

inclined-Plane Machining.

M-codes

4-30

2. Polar coordinate interpolation

G109L1 M901 M200 M212

G0G90G94G54G97 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001T00M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B0.

G97S3000M03 G10.9X0 M08

G61.1 M108

G90G53B0. G90G00C0.

M107

G90G43G00X70.0Y0.Z-15.0H1

G17G90G00X70.0C0. G12.1 G01G42D51X50.C50.F500.

C-50. X-50. C50. X50. Z10.0

G40 G13.1 G64

M05 M09

G91G28X0 G28Y0 G28Z0

M30

(3-axis machining_ Polar coordinate interpolation)

Preparation motion for machining

 G109L1: Upper turret selection  M901: HD1 spindle selection  M200: C-axis connect/Milling mode select  M212: C-axis unclamping  G94: Feed per minute  G97: Constant surface speed control OFF  T001M06: Tool change (TNo.01)  B-axis positioning  G97S3000: Rotation speed 3000 min-1  M03: Forward milling spindle rotation  G10.9X0: Radius data input mode  M08: Flood coolant ON

End motion for machining

 M05: Stop of milling spindle rotation  M09: coolants OFF  Each axis positioning to zero return  M30: Reset and rewind

Machining motion

 G61.1: Geometry compensation  Rotational axis positioning  G17XC: XC-plane selection  G43H**(P0): Tool length offset  G12.1: Polar coordinate interpolation ON  G41D**: Tool radius compensation (left)  (Machining pattern)  G40: Tool radius compensation OFF  G13.1: Polar coordinate interpolation OFF  G64: Geometry compensation OFF

Machining contour

Serial No. 294060

This section explains how to make the program of Polar coordinate interpolation in 3-axis machining program.

A. Sample program

MACHINING PROGRAM 4

4-31

4 MACHINING PROGRAM

Parameter

bit

Standard

Setting

Description

F114

3 1 1

Moving axes by using G49 (tool length offset cancel) in G43 (tool length offset) mode Invalid

G61.1 M108 G90G53Bb G90G00Cc M107 G90G43G00XxYyZzHh G17G90G00XxCc G12.1

G01G41(G42)DdXxCcFf (Machining pattern) G40 G13.1

G64

Machining motion of program composition -Polar coordinate interpolation-

--- Geometry compensation

--- B-axes unclamping

--- B-axis positioning

--- C-axis positioning

--- B-axes clamping

--- Tool length offset

--- XC-plane selection

--- Polar coordinate interpolation ON

--- Tool radius compensation

--- Machining pattern

--- Tool radius compensation OFF

--- Polar coordinate interpolation OFF

--- Geometry compensation OFF

G41/42

G40

Tool radius compensation

G12.1

G13.1

Polar coordinate interpolation

The figure below indicates setting of each mode

G61.1

G64

Geometry compensation

When G17 XC is commanded, X and C move to the specified positions.

Instruction in

preparation motion

for machining

Instruction in

machining motion

Upper turret

HD1

milling

Polar coordinate interpolation

Tool radius compensation

Geometry compensation

Program composition element

Serial No. 294060

B. Program composition

C. Parameter setting

Parameter setting

4-32

MACHINING PROGRAM 4

G-codes

Group

Description

G12.1

26

Polar coordinate interpolation ON

G13.1

26

Polar coordinate interpolation OFF

G40

7

Nose radius/Tool radius compensation OFF

G41

7

Nose radius/Tool radius compensation (left)

G43

8

Tool length offset (+)

G61.1

13

High-accuracy mode (Geometry compensation)

G64

13

Cutting mode

G codes

Description



G61.1

Geometry compensation

G61.2

Modal spline interpolation

M-codes

Description

M107

B-axis clamping

M108

B-axis unclamping

Serial No. 294060

D. G-codes/M-codes

See the document [99 Supplement] for details. G-codes

Note 1: When G12.1 is commanded, a workpiece coordinate system must be set using the

center of rotational axis as the zero point of the coordinate system. The coordinate system must not be changed during the G12.1 mode.

Note 2: The geometry compensation reduces geometry errors caused by the delay in the

smoothing circuits and servo systems.

High-accuracy mode

Note 1:  is G-code used by sample program. Note 2: G61.2 is a geometry compensation with fine spline interpolation feature for a further

better quality surface for the CAM-made minute increments block by block data operation.

M-codes

4-33

4 MACHINING PROGRAM

Serial No. 294060

4-4-4 4-axis machining program

This section explains how to make 4-axis machining program.

1. 4-axis machining

This section explains the programming method for machining with the B-axis fixed. In case G43P1 is used as tool length offset, caution should be paid as the feed rate of the tool based on the work may vary from the programmed value. To minimize the error G43P1 program should have least rotational distance between the blocks.

If tool tip point control G43.4 is available, the use of G43.4 instead of G43P1 can guarantee the feedrate of the tool tip to the work piece to the F command. G43.4 has “Joint interpolation” and

“Uniaxial rotation interpolation”. Joint interpolation is suitable for most ball end mill applications

as to linearly interpolate the rotary axes between the blocks.

4-34

A. Sample program

G109L1 M901 M200 M212

G0G90G94G55G97 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001T00M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B40.0

G97S12000M03 G10.9X0 M51

G61.1

M108 G17 G90G53B40. G90G00C0. G90G43G00X58.03Y9.992Z131.564B40.C0.H1P1

M107 G05P2

X33.9245Z102.8365 G01X33.5319Y0.F250. X33.5672Z102.6365C-4.5 (Machining contour) X36.7457Y-9.9923 G00X58.03Z112.2021

G05P0 G64

M05 M09

G91G28X0 G28Z0 G28Y0 M108 G90G53B0

M30

Machining contour

Preparation motion for machining

 G109L1: Upper turret selection  M901: HD1 spindle selection  M200: C-axis connect/Milling mode select  M212: C-axis unclamping  G94: Feed per minute  G97: Constant surface speed control OFF  T001M06: Tool change (TNo.01)  B-axis positioning  G97S12000: Rotation speed 12000 min-1  M03: Forward milling spindle rotation  G10.9X0: Radius data input mode  M51: Milling spindle-through coolant ON

Machining motion

 G61.1:

Geometry compensation

 Rotational axis positioning  G43H**P1: Tool length offset  M107: B-axis clamp  G5P2: High-speed

machining mode ON

 (Machining pattern)  G5P0: High-speed

machining mode OFF

 G64:

Geometry compensation OFF

End motion for machining

 M05: Stop of milling spindle rotation  M09: coolants OFF  Each axis positioning to zero return  M30: Reset and rewind

(4-axis machining)

Serial No. 294060

MACHINING PROGRAM 4

4-35

4 MACHINING PROGRAM

Parameter

bit

Standard

Setting

Description

F3

- 1 1

High-speed smoothing control valid (No deceleration at very slightly stepped sections)

F85

3 1 1

Tool tip point control scheme Joint interpolation

F96

1 0 1

Fairing function Valid

6 1 1

Rotational axis shape correction Valid

F114

3 1 1

Moving axes by using G49 (tool length offset cancel) in G43 (tool length offset) mode Invalid

G61.1 M108 G90G53Bb G90G00Cc. G90G43G00XxYyZzBbCcHhP1 B107 G05P2 G01XxYyFf (Machining pattern) G00XxZz G05P0 G64

Machining motion of program composition -4-axis machining-

Note: Feed rate based on work may differ from F command if there are rotation commands in the

blocks. Use G43.4 tool tip point control function if possible. (Reference: 4-4-5 5-axis machining program)

--- Geometry compensation

--- B-axes unclamping

--- B-axis positioning

--- C-axis positioning

--- Tool length offset (P1)

--- B-axes clamping

--- High-speed machining mode ON

--- Head block for machining contour

--- Machining pattern

--- Escape

--- High-speed machining mode OFF

--- Geometry compensation OFF

G5P2

G5P0

High-speed machining mode

The figure below indicates setting of each mode

G61.1

G64

Geometry compensation

Instruction in

machining motion

Instruction in

preparation motion

for machining

Upper turret

HD1

milling

Tool length offset (P1)

High-speed machining mode

Geometry compensation

Program composition element

Serial No. 294060

B. Program composition

C. Parameter setting

The main parameter of processing is described. The table shows the standard parameter and setting set in this manual.

Parameter setting

Note : See 4-4-5: 5-axis machining program for the tool tip point control (G43.4).

4-36

MACHINING PROGRAM 4

G-codes

Group

Description

G5P0

0

High-speed machining mode OFF

G5P2

0

High-speed machining mode ON

G43P1

8

Tool length offset

G61.1

13

High-accuracy mode (Geometry compensation)

G64

13

Cutting mode

G codes

Description



G61.1

Geometry compensation

G61.2

Modal spline interpolation

M-codes

Description

M107

B-axis clamping

M108

B-axis unclamping

Serial No. 294060

D. G-codes/M-codes

See the document [99 Supplement] for details. G-codes

Note 1: The geometry compensation reduces geometry errors caused by the delay in the

smoothing circuits and servo systems.

Note 2: The high-speed machining mode features high-speed execution of free form programs

such as die and mold machining approximated by fine increments data. Combined with the geometrical correction function, it produces high quality surface finish.

High-accuracy mode

Note 1:  is G-code used by sample program. Note 2: G61.2 is a geometry compensation with fine spline interpolation feature for a further

better quality surface for the CAM-made minute increments block by block data operation.

M-codes

4-37

4 MACHINING PROGRAM

G109L1 M901 M200 M212

G0G90G94G55G97 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001T00M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B64.967

G97S12000M03 G10.9X0 M51 M821

G61.1

M108 G90G53B64.967 G90G00C30.759

G43.4G00X31.86Y32.98Z-21.168B64.967C30.759H1 G5P2

G01X24.0743Y28.3517Z-25.4001F104. X26.7769Y25.9326Z-27.9776B65.4857C27.3136F69. X29.2975Y23.1739Z-30.3815B65.9455C23.7912 (Machining contour) X26.7766Y-25.9326Z-27.9771B65.4858C-27.3138 X24.0741Y-28.3516Z-25.3996B64.967C-30.7598 G00X31.8601Y-32.9856Z-21.1682

G5P0 G49 G64

M05 M09

G91G28X0 G28Z0 G28Y0 M108 G90G53B0

M30

Preparation motion for machining

 G109L1: Upper turret selection  M901: HD1 spindle selection  M200: C-axis connect/Milling mode select  M212: C-axis unclamping  G94: Feed per minute  G97: Constant surface speed control OFF  T001M06: Tool change (TNo.01)  B-axis positioning  G97S12000: Rotation speed 12000 min-1  M03: Forward milling spindle rotation  G10.9X0: Radius data input mode  M51: Milling spindle-through coolant ON  M821: Accuracy level 1

Machining motion

 G61.1:

Geometry compensation

 Rotational axis positioning  G43.4H**:

Tool tip point control

 G5P2: High-speed

machining mode ON

 (Machining pattern)  G5P0: High-speed

machining mode OFF

 G49: Tool position

offset OFF

 G64: Geometry

compensation OFF

Machining contour

End motion for machining

 M05: Stop of milling spindle rotation  M09: Coolants OFF  Each axis positioning to zero return  M30: Reset and rewind

(5-axis machining)

Serial No. 294060

4-4-5 5-axis machining program

This section explains how to make the program of 5-axis machining.

1. 5-axis machining

This section explains how to make the general 5-axis machining.

A. Sample program

4-38

MACHINING PROGRAM 4

G61.1 M108 G90G53Bb G90G00Cc G43.4G00XxYyZzBbCcHh G5P2 G01XxYyZzFf (Machining pattern) G00XxYyZz G5P0 G49 G64

Machining motion of program compositon -5-axis machining-

--- Geometry compensation

--- B-axes unclamping

--- B-axis positioning

--- C-axis positioning

--- Tool tip point control ON

--- High-speed machining mode ON

--- Head block for machining contour F-code

--- Machining pattern

--- Escape

--- High-speed machining mode OFF

--- Tool tip point control OFF

--- Geometry compensation OFF

G5P2

G5P0

High-speed machining mode

G43.4

G49

Tool tip point control

The figure below indicates the setting of each mode

G61.1

G64

Geometry compensation

Note: G43.4 should be commanded after positioning B and C axis

to avoid unexpected axis motion.

Instruction in

machining motion

Instruction in

preparation motion

for machining

Upper turret

HD1

milling

High-speed machining mode

Geometry compensation

Tool tip point control

Table coordinate system

Program composition element

Serial No. 294060

B. Program composition

4-39

4 MACHINING PROGRAM

Parameter

bit

Standard

Setting

Description

F3

- 1 1

High-speed smoothing control valid (No deceleration at very slightly stepped sections)

F85

2 1 0

Type of coordinate system for controlling the tool tip point The table coordinate system

3 1 1

Tool tip point control scheme Joint interpolation

F86

2 1 1

Override scheme for G0 The clamping speed at the machine control point

5 1 1

Override scheme for G1 The clamping speed at the machine control point

6 0 1

C-axis reference position 0 degrees

F96

6 1 1

Rotational axis shape correction Valid

F114

1 1 1

The axis does not move when command G49 is issued

F162

0 0 1

During independent start of tool tip point control No movement

Serial No. 294060

C. Parameter setting

The main parameter of processing is described. The table shows the standard parameter and setting set in this manual.

Parameter setting

Note 1: High-speed smoothing control function is valid during high-speed mode with the shape

Some of the outstanding features of high-speed smoothing control are listed below.

 Effective for machining a die of a smooth shape using a microsegment program.  Speed control is insusceptible to the effects of any errors contained in the tool path.  If adjacent paths are similar in terms of geometrical accuracy, acceleration and

 Even at the sections where corner deceleration is not necessary with respect to the

correction being selected.

deceleration patterns will also be similar.

angle, speed will be clamped if the estimated acceleration is great.

4-40

MACHINING PROGRAM 4

G-codes

Group

Description

G5P0

0

High-speed machining mode OFF

G5P2

0

High-speed machining mode ON

G43.4

8

Tool tip point control (Type 1) ON

G49

8

Tool position offset OFF

G61.1

13

High-accuracy mode (Geometry compensation)

G64

13

Cutting mode

D740PB0037

X

Y

Z

Y

X

D740PB0035

X

Y

Z

Z

Y

X

Serial No. 294060

Note 2: Coordinate system for controlling the tool tip point is defined as follows.

The TABLE coordinate system (F85 bit 2: 0)

The table coordinate system will rotate as the table rotates. But the tool axis rotation (e.g. the B axis for INTE) does not rotate the coordinate.

The WORK PIECE coordinate system (F85 bit 2: 1)

The current workpiece coordinate is the programming coordinate system which is fixed in the orthogonal coordinate and does not rotate with the table.

D. G-codes/M-codes

See the document [99 Supplement] for details. G-codes

Note 1: The geometry compensation reduces geometry errors caused by the delay in the

smoothing circuits and servo systems.

Note 2: The high-speed machining mode features high-speed execution of free form programs

such as die and mold machining approximated by fine increments data. Combined with the geometrical correction function, it produces high quality surface finish.

4-41

4 MACHINING PROGRAM

G codes

Description



G61.1

Geometry compensation

G61.2

Modal spline interpolation

M-codes

Description

M107

B-axis clamping

M108

B-axis unclamping

Serial No. 294060

High-accuracy mode

Note 1:  is G-code used by sample program. Note 2: G61.2 is a geometry compensation with fine spline interpolation feature for a further

M-codes

better quality surface for the CAM-made minute increments block by block data operation.

4-42

2. Tool Radius compensation for 5-axis machining

G109L1 M901 M200 M212

G0G90G94G55G97 G40G49G80G67G69 G91G28X0 G28Z0 G28Y0

T001T00M06

G91G28X0 G28Y0 G28Z0 M108 G90G53B0.0

G97S12000M03 G10.9X0 M51 M825

G61.1

M108 G90G53B0. G90G00C0.

G43.4G00X76.1704Y118.5904Z350.B0.C0.H1 G41.5 D51

(G05P2) G01X23.0544Y50.1894Z300.F796. X21.175Y47.7693 X19.4744Y45.2203 (Machining contour) X29.6674Y62.4938Z150.9717 X29.6685Y62.4749Z150.9705 X115.2461Y67.3568Z202.4743 (G05P0)

G40 G49 G64

M05 M09

G91G28X0 G28Z0 G28Y0 M108 G90G53B0

M30

Preparation motion for machining

 G109L1: Upper turret selection  M901: HD1 spindle selection  M200: C-axis connect/Milling mode select  M212: C-axis unclamping  G94: Feed per minute  G97: Constant surface speed control OFF  T001M06: Tool change (TNo.01)  B-axis positioning  G97S12000: Rotation speed 12000 min-1  M03: Forward milling spindle rotation  G10.9X0: Radius data input mode  M51: Milling spindle-through coolant ON  M825: Accuracy level 5

Machining motion

 G61.1: Geometry compensation  Rotational axis positioning  G43.4H**: Tool tip point control  G41.5D**: Tool radius

compensation for 5-axis machining

 (Machining pattern)  G40: Tool radius compensation

for 5-axis machining OFF

 G49: Tool tip point control OFF  G64:Geometry compensation OFF

End motion for machining

 M05: Stop of milling spindle rotation  M09: coolants OFF  Each axis positioning to zero return  M30: Reset and rewind

(5-axis Machining _Tool Radius Compensation)

Machining contour

Serial No. 294060

This section explains how to make the program of 5-axis Machining using Tool Radius Compensation for 5-axis Machining.

A. Sample program

MACHINING PROGRAM 4

4-43

4 MACHINING PROGRAM

Machining motion of program composition

-Tool radius compensation for 5-axis machining-

G61.1 M108 G90G53Bb G90G00Cc G43.4G00XxYyZzBbCcHh G41.5Dd

G01XxYyZzFf

(Machining pattern) G0XxYyZz G40

G49 G64

--- Geometry compensation ON

--- B-axis unclamping

--- B-axis positioning

--- C-axis positioning

--- Tool tip point control ON

--- Tool radius compensation for 5-axis machining

--- Head block for machining contour F-code

--- Machining pattern

--- Escape

--- Tool radius compensation for 5-axis machining OFF

--- Tool tip point control OFF

--- Geometry compensation OFF

G41.5

G40

Tool radius compensation for 5-axis machining

G43.4

G49

Tool tip point control

The figure below indicates setting of each mode

G61.1

G64

Geometry compensation

Note 1: G43.4 should be commanded after the positioning of B and C axis, otherwise a large C axis motion

will cause unexpected motion.

Note 2: Giving a command for high-speed machining will lead to an alarm (807 ILLEGAL FORMAT) under

a combined use of tool radius compensation for five-axis machining with tool tip point control (Reference: EIA manual 29-3-5.2)

Instruction in

machining motion

Instruction in

preparation motion

for machining

Upper turret

HD1

milling

Tool radius compensation for

5-axis machining

Geometry compensation

Tool tip point control

Table coordinate system

Program composition element

Serial No. 294060

B. Program composition

4-44

C. Parameter setting

Parameter

bit

Standard

Setting

Description

F3

- 1 1

High-speed smoothing control valid (No deceleration at very slightly stepped sections)

F85

2 1 0

Type of coordinate system for controlling the tool tip point The table coordinate system

3 1 1

Tool tip point control scheme Joint interpolation

F86

2 1 1

Override scheme for G0 The clamping speed at the machine control point

5 1 1

Override scheme for G1 The clamping speed at the machine control point

6 0 1

C-axis reference position 0 degrees

F96

6 1 1

Rotational axis shape correction Valid

F114

1 1 1

The axis does not move when command G49 is issued

F162

0 0 1

During independent start of tool tip point control No movement

G-codes

Group

Description

G40

7

Tool radius compensation OFF

G41.5 7 Tool radius compensation for five-axis machining (left)

G43.4

8

Tool tip point control (Type 1) ON

G49

8

Tool position offset OFF

G61.1

13

High-accuracy mode (Geometry compensation)

G64

13

Cutting mode

G codes

Description



G61.1

Geometry compensation

G61.2

Modal spline interpolation

Serial No. 294060

The main parameter of processing is described. The table shows the standard parameter and setting set in this manual.

Parameter setting

Note 1: See 4-4-5 1. C. for coordinate system for controlling the tool tip point

MACHINING PROGRAM 4

Note 2: See 4-4-5 1. C. for the setting the workpiece coordinate system

D. G-codes/M-codes

See the document [99 Supplement] for details. G-codes

Note 1: The geometry compensation reduces geometry errors caused by the delay in the

smoothing circuits and servo systems.

Note 2: The high-speed machining mode features high-speed execution of free form programs

such as die and mold machining approximated by fine increments data. Combined with the geometrical correction function, it produces high quality surface finish.

High-accuracy mode

Note 1:  is G-code used by sample program. Note 2: G61.2 is a geometry compensation with fine spline interpolation feature for a further

better quality surface for the CAM-made minute increments block by block data operation.

4-45

4 MACHINING PROGRAM

M-codes

Description

M107

B-axis clamping

M108

B-axis unclamping

Serial No. 294060

M-codes

4-46

4-5 End Motion for Machining

Milling spindle (G109L1)

M05: Stop of milling spindle rotation

M03: Start of forward milling spindle rotation M04: Start of backward milling spindle

rotation

Turning spindle 1

M205: Turning spindle 1 Rotation stop

M203: Turning spindle 1 Start of forward

rotation

M204: Turning spindle 1 Start of backward

rotation

Turning spindle 2

M305: Turning spindle 2 Rotation stop

M303: Turning spindle 2 Start of forward rotation M304: Turning spindle 2 Start of backward

rotation

Milling spindle (G109L2)

M05: Stop of milling spindle rotation

M03: Start of forward milling spindle

rotation

M04: Start of backward milling spindle

rotation

M09 M05 G91G28Z0 G28X0 G28Y0 M108 G90G53B0 M30

M09 M205 G91G28Z0 G28X0 G28Y0 M108 G90G53B0 M30

HD1 turning mode

Upper turret milling mode

Serial No. 294060

This section explains on “End motion for machining”.

4-5-1 Sample program

This is a sample program of the processing end operation. See the following for more details.

4-5-2 End motion

MACHINING PROGRAM 4

This section explains End motion. Program the following commands from 1. to 4.. Select the order of home return depending on the machining method.

1. Rotation stop command

Stops the milling spindle/turning spindle. Refer to the figure below for rotation stop M-codes .

4-47

4 MACHINING PROGRAM

M00: Program stop

Program execution will be stopped, At this time, the milling spindle and the

turning spindle rotations will also be stopped.

M02: End of program

NC is reset and all the machine motions: spindle rotation, coolant, air. etc. will

be stopped.

M30: Reset and rewind

This function code stops the machine similarly to M02, and calls the head of the

program.

M99: Subprogram return command

This command returns the operation from subprogram to the main program

where the subprogram was called.

Note: M30 contains the reset of NC.

G00G90G53Zz (Z-axis Positioning) G53Xz (X-axis Positioning) G53Yy (Y-axis Positioning) M108 G90G53Bb (B-axis Positioning)

Positioning (by G53)

(for home return in order of ZXY)

G28G91Z0 (Z-axis home ) G28X0 (X-axis home ) G28Y0 (Y-axis home ) M108 G28B0 (B-axis home)

Home return (by G28)

Used to bring the axes home return.

Used to position the axes to an arbitrary position. If zero they are the same with home.

M09: All coolants OFF

This M code turns off all machining-related fluids such as coolants and air.

Serial No. 294060

2. Coolant stop command

This command turns off all coolant and air. It is not necessary to program the coolant stop command if they are not turned on in the preparation motion for machining.

3. Home return

Perform home return on each axis. Select the order of home return for safety. Depending on the machining method, the mill spindle may need to move to a safe position. In that case, set the coordinate values by G53. Home return commands are not necessary for the axes which have already returned home such as B axis.

4. Program end

M-codes of program end are shown in the figure below. Select an appropriate command by the machining method. M30 is used for program end in this manual.

4-48

4-6 Programming for Compound Machining (ST Specification)

Commands for the upper turret

Commands for the lower turret

Parameter

Setting

Description

F162 bit 4

0

4 digits in T-command for turning

1

6 digits in T-command for turning

Serial No. 294060

This section explains how to make programming for compound machining. Refer to this section and 4-3, 4-4, 4-5 to make a program.

S specifications machines (with HD2 spindle, no lower turret) cannot use command about lower turret, but can use command about HD2.

4-6-1 Function of programming for compound machining

This section explains the function necessary to programming for compound machining.

1. Method of making compound machining program

The movement of the upper and lower turrets is to be controlled in a single program as follows.

G109 L1; ............... Selection of the upper turret

M30;

G109 L2; ............... Selection of the lower turret

MACHINING PROGRAM 4

M30;

2. Tool change of lower turret

Care of tool change command because lower turret is turret-Indexing systems. Digit number for tool change command can be selected the parameter.

Parameter of tool change for lower turret

4-49

4 MACHINING PROGRAM

Serial No. 294060

A. Tool function [4-digit T-Code for turret-indexing systems]

Tool function, also referred to as T-code function, is used to designate the tool number. Of a four-digit integer at address T, upper and lower two digits are respectively used to specify the tool number and trailing zeros (00). Use bit 4 of parameter F162 to select the number of digits for the tool function (0 or 1 for 4- or 6-digit T-code).

T  00. ;

Designate the tool ID code with reference to the settings on the TOOL DATA display. Only one T-code can be included in a block, and the available range of T-codes depends on the machine specifications. For further details, especially on how to number the actual tools to be used, refer to the operating manual of the relevant machine.

The T-code can be given with any other commands in one block, and the T-code given together with an axis motion command is executed, depending upon the machine specifications, in one of the following two timings:

 The T-code is not executed till completion of the motion command, or  The T-code is executed simultaneously with the motion command.

Remark: Instead of zeros, other numerals can be specified as well in the lower two digits

Tool ID code

Tool number

without exercising any influence upon the machine control.

B. Tool function [6-digit T-Code for turret-indexing systems]

This function is also used to designate the tool number. Of a six-digit integer at address T, upper and lower three digits are respectively used to specify the tool number and trailing zeros (000). See the above description of the 4-digit T-code for the meaning of the decimal fractions.

The available range of T-codes depends on the machine specifications. For further details, refer to the operating manual of the relevant machine.

Only one T-code can be included in a block. Use bit 4 of parameter F162 to select the number of digits for the tool function (0 or 1 for 4- or

6-digit T-code).

T  000. ;

Tool ID code

Tool number

Remark: Instead of zeros, other numerals can be specified as well in the lower three digits

without exercising any influence upon the machine control.

4-50

MACHINING PROGRAM 4

G-codes

Group

Description

G109

0

Single program multi-process control

G110

20

Cross machining control ON

G111

20

Cross machining control OFF

HD1

HD2

G109L1 G90(G91)X_Y_Z_

G109L2 G90(G91)X_Y_Z_

Moving order of upper turret

Moving order of lower turret

[1]

G109L1 M902 (*2) M300 (*3) M03S___ G110C2 C__ (*5) G111

G109L1 M901 (*1) M200 (*3) M03 (*4) C__ (*5)

[2]

G109L2 M901 M200 M03S___ G110C1 C__ (*5) G111

G109L2 M902 M300 M03 C__ (*5)

[4]

[3]

*1 M901 for the 1st spindle selection. *2 M902 for the 2nd spindle selection. *3 M200/M300 for milling mode selection for 1st/2nd spindle. *4 M03 for milling spindle’s normal rotation. *5 Machining data

Serial No. 294060

3. Combination of turret and turning spindle

There are four kinds of combinations about turret and turning spindle. And make the program by use it.

The following are the program examples at the milling.

4. Related G codes of programming for compound machining

G-codes

A. Single program multi-process control (G109)

Axis motion of upper turret and lower turret are commanded like the figure. Axis motion of upper turret and lower turret

Note : Axis motion commands after reset effect to upper turret and lower turret till instructed

on G109.

4-51

4 MACHINING PROGRAM

1: Axis controlled by HD1 2: Axis controlled by HD2

Serial No. 294060

B. Cross machining control (G110/G111)

Axis control of HD2 side by HD1 side or that of HD1 side by HD2 side is referred to as cross machining control. Specify after G110 an axis address and the HD number controlling the axis.

(Refer to 4-6-2 1. A, 4-6-2 1. D and 4-6-2 2. B for the sample program.)

 Programming format

G110 X_ Y_ Z_; .................... Cross machining control axis and HD number are specified.

G111; ..................................... Cross machining control axis specified by G110 is returned

Example: Operation at HD1 side

to normal control (not cross machining).

G110 X2; Changed to X-axis of HD2 G00 X10. Z10.; X of HD2 moves to 10, Z of HD1 moves to 10. G110 Z2; Changed to Z-axis of HD2 G00 X20. Z20.; X of HD2 moves to 20, Z of HD2 moves to 20. G110 X1 Z1; Changed to X-axis and Z-axis of HD1 G00 X30. Z30.; X of HD1 moves to 30, Z of HD1 moves to 30.

Specify the Z-axis for the lower turret as follows: Example:

G110 Z2; Selection of the lower turret’s Z-axis G00 Z100.; All the Z-axial commands between G110 and G111 are processed  as those for the lower turret. G111; Cancellation of G110

Specify the C-axis on the 2nd headstock side as follows: Example:

G110 C2; Selection of the 2nd headstock’s C-axis G00 C45.123.; All the C-axial commands between G110 and G111 are processed  as those for the 2nd headstock side. G111; Cancellation of G110

4-52

YAMAZAKI MAZAK INTEGREX e, INTEGREX i, VORTEX i Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

1 INTRODUCTION

2 MACHINE INFORMATION

2-1 Controlled Axis Information

2-1-1 Composition of controlled axes

2-1-2 Outline of the machine structure

2-1-3 Machine stroke

2-1-4 Input limitation

2-1-5 Rotating speed

2-1-6 Rapid feed rate

2-1-7 Cutting feed rate

2-2 Magazine

2-2-1 INTEGREX i

2-2-2 INTEGREX i-S

2-2-3 INTEGREX i-ST

2-2-4 INTEGREX e-H

2-2-5 INTEGREX e-H-S

2-2-6 INTEGREX e-H-ST

2-2-7 INTEGREX i-V

2-2-8 INTEGREX e-V

2-2-9 VORTEX i-V

3 NC COMMAND

3-1 Programming Format

3-1-1 Words and addresses

3-1-2 Control out, control in

3-1-3 Optional block skip

3-1-4 Program end

3-1-5 Program file name

3-2 Command

4 MACHINING PROGRAM

4-1 Set Up

4-1-1 Setting of workpiece origin

4-1-2 Parameter of tool length offset.

4-1-3 Parameter for Nose / Tool radius compensation

4-2 Programming Composition

4-2-1 Programming composition

4-2-2 Method of making program

4-3 Preparation Motion for Machining

4-3-1 Sample program

4-3-2 Preparation for machining

4-4 Machining Motion

4-4-1 Turning program

4-4-2 Hole machining program

4-4-3 3-axis machining program

4-4-4 4-axis machining program

4-4-5 5-axis machining program

4-5 End Motion for Machining

4-5-1 Sample program

4-5-2 End motion

4-6 Programming for Compound Machining (ST Specification)

4-6-1 Function of programming for compound machining