hitachi seiki 10L, 16T, 18T, 21L Programming Manual

Download

SEIKI - SEICOS

å10L/å16T/å18T/å21L

INSTRUCTION MANUAL

PROGRAMMING

42 Edition 1.01 NO-0000-1-0211-E-1-01

Hitachi Seiki Deutschland Werkzeugmaschinen GmbH

INTRODUCTION

This manual explains about the programming system of SEICOS-Σ10L, Σ16T,Σ18T and Σ21L. The manual contains explanation on all functions, however, there are certain functions that are not applicable depending on the type of the machine used. On this matter, please refer to the instruction manual of each machine model when you utilize these functions.

Items requiring attention when reading this manual.

(1) In this manual, those functions not specifically remarked “able” should be understood as

“unable”.

(2) The contents of this manual may be changed without notice to meet a future machine

improvement.

(3) In this manual, all the descriptions take G18 (Z-X) plane as the subject plane, unless otherwise

specifically mentioned. For cutting processes made on a plane other than G18, refer to “7.8 Lathe turning on other than the G18 plane”.

ΣΣ

Σ10L,

ΣΣ

The processing programs of Σ10L, Σ16T, Σ18T and Σ21L are nearly 100% compatible. As exceptions, Σ21L does not have the following functions.

ΣΣ

Σ16T,

ΣΣ

[1] 2.4 Helical interpolation [2] 2.5 Virtual axis interpolation [3] 4.6 Automatic corner override [4] 5.2 Inside arc cutting speed change [5] 6.5 Floating reference point return

ΣΣ

Σ18T and

ΣΣ

Σ21L

ΣΣ

CONTENTS

1. G CODE................................................................................................ 1 - 1

1.1 G Code System............................................................................................................. 1 - 1

1.2 List of G Code Groups................................................................................................... 1 - 3

1.3 List of G Codes .............................................................................................................1 - 4

2. INTERPOLATION FUNCTION............................................................. 2 - 1

2.1 Positioning (G00)........................................................................................................... 2 - 1

2.2 Linear Interpolation ........................................................................................................2 - 3

2.3 Circular Interpolation (G02, G03) ...................................................................................2 - 5

2.4 Helical Interpolation (G02, G03) .....................................................................................2 - 9

2.5 Virtual Axis Interpolation (G07)..................................................................................... 2 - 1 1

2.6 Cylindrical Interpolation (G271).................................................................................... 2 - 12

2.7 Polar Coordinate Interpolation (G120, G121)............................................................... 2 - 17

2.8 Angle Designated Linear Interpolation .........................................................................2 - 25

2.9 Skip Function (G31).....................................................................................................2 - 27

3. THREAD CUTTING .............................................................................. 3 - 1

3.1 Thread Cutting (G32).....................................................................................................3 - 1

3.2 Continuous Thread Cutting (G32) ................................................................................. 3 - 3

3.3 Multi-thread Cutting........................................................................................................3 - 4

3.4 Variable Lead Thread Cutting (G34) ..............................................................................3 - 5

4. FEED FUNCTION ................................................................................ 4 - 1

4.1 Feed Per Minute (G98) .................................................................................................. 4 - 1

4.2 Feed Per Revolution (G99)............................................................................................4 - 2

4.3 Dwell (G04) ...................................................................................................................4 - 3

4.4 Exact Stop (G09)...........................................................................................................4 - 4

4.5 Exact Stop Mode (G61) .................................................................................................4 - 5

4.6 Automatic Corner Override Mode (062).........................................................................4 - 6

4.7 T apping Mode (G63) ......................................................................................................4 - 8

4.8 Cutting Mode (G64) .......................................................................................................4 - 9

4.9 Multibuffer (G251) ........................................................................................................4 - 10

4.10 Acceleration/Deceleration Control ............................................................................... 4 - 11

5. SPEED CONTROL .............................................................................. 5 - 1

5.1 Feed Speed Command (F Data)................................................................................... 5 - 1

5.3 Scroll Cutting Speed Control (G128) ............................................................................. 5 - 4

5.4 Speed Control of Independent Axis ..............................................................................5 - 10

6. REFERENCE POINT ........................................................................... 6 - 1

6.1 Automatic Reference Point Return (G28)......................................................................6 - 1

6.2 Reference Point Return Check (G27) ...........................................................................6 - 2

6.3 Return from Reference Point (G29) ..............................................................................6 - 3

6.4 2nd-4th Reference Point Return (G30)..........................................................................6 - 4

6.5 Floating Reference Point Return (G301) .......................................................................6 - 5

7. COORDINATE SYSTEM ..................................................................... 7 - 1

7.1 Tool Nose Coordinate System....................................................................................... 7 - 1

7.2 Plane Designation (G17, G18, G19) ..............................................................................7 - 4

7.3 Work Coordinate System Change (G50) ......................................................................7 - 6

7.4 Work Length Modification (G54/G55).............................................................................7 - 7

7.5 Machine Coordinate System Selection (G53) ............................................................... 7 - 8

7.6 Setting the Local Coordinate System (G59) ..................................................................7 - 9

7.7 Work Coordinate System Preset (G921) ....................................................................7 - 10

7.8 Lathe Turning Other than the G18 Plane (Z-X) ............................................................ 7 - 11

8. COORDINATE...................................................................................... 8 - 1

8.1 Diameter Designation and Radius Designation.............................................................8 - 1

8.2 Absolute/Incremental Programming (G90, G91) ...........................................................8 - 2

8.3 Inch/mm Input (G20, G21) .............................................................................................8 - 3

9. SPINDLE FUNCTIONS........................................................................ 9 - 1

9.1 Spindle Functions (Function S) ..................................................................................... 9 - 1

9.2 Constant Surface Speed Control (G96, G97)................................................................ 9 - 2

9.3 Maximum Spindle Speed Setting (G50) .........................................................................9 - 3

9.4 Spindle Speed V ariation Detection (G25/G26) ...............................................................9 - 4

10. TOOL FUNCTION............................................................................ 10 - 1

10.1 Tool Function (T Function)........................................................................................... 10 - 1

10.2 ATC Canned Cycle...................................................................................................... 10 - 5

10.3 Rotary Tool Offset Auto Conversion (G159) .............................................................. 10 - 11

10.4 ATC Type-E Offset Automatic Change........................................................................10 - 16

11. MISCELLANEOUS FUNCTION....................................................... 11 - 1

11.1 Miscellaneous Function (M Function) .......................................................................... 1 1 - 1

11.2 2nd Miscellaneous Function ........................................................................................ 1 1 - 3

12. COMPENSATION FUNCTION ........................................................ 12 - 1

12.1 Automatic Tool Nose Radius Compensation and Cutter Compensation.....................12 - 1

12.2 Automatic Tool Nose Radius Compensation...............................................................12 - 2

12.3 Groove Width Compensation (G150, G151, G152)...................................................12 - 15

12.4 Multiple Offsets.......................................................................................................... 12 - 18

12.5 Cutter Compensation (G38-G42) .............................................................................. 12 - 22

12.6 Detailed Description of Cutter Compensation ........................................................... 12 - 28

13. CONVERTING FUNCTION.............................................................. 13 - 1

13.1 Programmable Mirror Image (G501, G511) .................................................................13 - 1

13.2 Setting Mirror Image ....................................................................................................13 - 3

13.3 Chamfering, Corner R .................................................................................................13 - 5

13.4 Optional Angle Chamfering/Corner R (, C, R) ............................................................. 13 - 7

13.5 Three Dimensional Coordinate Conversion (G268, G269)........................................13 - 10

14. SINGLE TYPE FIXED CYCLE........................................................ 14 - 1

14.1 O.D./I.D. Cutting Cycle (G90) ......................................................................................14 - 1

14.2 Canned Cycle for Thread Cutting (G92)......................................................................14 - 2

14.3 End/side Cutting Cycle (G94)......................................................................................14 - 5

14.4 Cautions Concerning Single Type Fixed Cycle............................................................14 - 6

15. MULTIPLE REPETITIVE CYCLE................................................... 15 - 1

15.1 Rough Planing of Inside & Outside Diameter (G71)....................................................15 - 2

15.2 Rough Planing Cycle of End Side (G72) .....................................................................15 - 9

15.3 Planing Cycle of Close Loop (G73) ...........................................................................15 - 12

15.4 Finish Cycle (G70).....................................................................................................15 - 14

15.5 Edge Cutting Cycle (G74) ......................................................................................... 15 - 15

15.6 Outside Diameter Edge Cutting Cycle (G75) ............................................................15 - 17

15.7 Combined Type Thread Cutting Cycle (G76) ............................................................ 15 - 19

15.8 Cautions Relating to Combined Type Fixed Cycle .................................................... 15 - 24

15.9 Alarms Relevant to Combined T ype Fixes Cycle ...................................................... 15 - 27

16. CANNED CYCLE FOR DRILLING .................................................. 16 - 1

16.1 Canned Cycle for Drilling (G80-G89, G831, G841, G861) ........................................... 16 - 1

16.2 Direct Tapping Cycle (G842, G843)........................................................................... 16 - 16

17. DATA SETTING............................................................................... 17 - 1

17.1 Programmable Data Input (G10) ................................................................................. 17 - 1

17.2 Programmable Parameter Input ..................................................................................17 - 5

18. STROKE LIMIT ................................................................................ 18 - 1

18.1 Stored Stroke Limit 1 ...................................................................................................18 - 1

18.2 Stroke Limit 2 to 4 (G22, G23) .....................................................................................18 - 3

18.3 Stroke Limit Check before Move.................................................................................. 18 - 6

iii

19. PROCESSING.................................................................................. 19 - 1

19.1 Rear Processing .........................................................................................................19 - 1

19.2 Polygon Turning (Polygon Turning Between S pindles) .............................................. 19 - 12

20. OPERATION ..................................................................................... 20 - 1

20.1 Program Resumption ..................................................................................................20 - 1

20.2 Return to Machining Interruption Point.........................................................................20 - 5

20.3 Sequence Number Comparison and Stop................................................................... 20 - 7

20.4 Manual Absolute ON/OFF............................................................................................20 - 8

20.5 Reset (Reset Associated with Automatic Operation) ................................................ 20 - 11

21. CUSTOM MACROS ........................................................................ 21 - 1

21.1 Program Call .............................................................................................................. 21 - 1

21.2 Multi-Call......................................................................................................................21 - 7

21.3 Argument Designation...............................................................................................21 - 12

21.4 Variables....................................................................................................................21 - 17

21.5 System V ariable ........................................................................................................21 - 20

21.6 Expression and Computation .................................................................................... 21 - 33

21.7 Control Command.....................................................................................................21 - 38

21.8 External Output Command........................................................................................21 - 41

22. COMPATIBILITY WITH SEICOS-LII/LIII......................................... 22 - 1

22.1 Drilling Fixes Cycle (G80-G89)....................................................................................22 - 2

23. MISCELLANEOUS .......................................................................... 23 - 1

23.1 Preread Stop Command .............................................................................................23 - 1

1.1 G Code System

Three kinds of G code systems including A, B, and C are available for selection. Any G code systems are almost the same in their functions and programming methods except only part of the G codes are different. When S pecifying the position of each axis, however, there is a difference in the absolute and incremental programming methods between the A system and non-A systems.

1.1.1 A system

Absolute programming and incremental programming use an axial address to specify an axial position. When X, Y, Z, B, or C is used for the axial address, they assume absolute programming, and when U, V, W, D, or H is used, they assume incremental programming. The following table shows the relations between axial names and axial addresses.

1. G CODE

Axial Name

Absolute Incremental X axis X U Y axis Y V Z axis Z W A axis A B axis B D

C axis C H

Axis A does not have the address of the incremental command. It is always specified by absolute. However , only for commands G28, G30 and G301, absolute commands and incremental commands of axis A can be switched over as follows. (1) When address Q is present on the same block

• Q=0 → Absolute command

• Q≠0 → Incremental command

(2) When address Q is not present on the same block

• Parameter AINC=0 → Absolute command

• Parameter AINC=1 → Incremental command

(AINC means 3 bits of parameter number 3404.)

Axial Address

1 - 1

1.1.2 B and C Systems

The following G codes are used to specify either absolute programming or incremental programming.

G90 : Absolute programming G91 : Incremental programming

These G codes are modal ones of Group 03.

(Note 1) The G code system A, B, and C are selected by the parameters GSB and GSC

(parameter No.3400.)

(Note 2) This command manual is described with the G codes of the A system unless

otherwise specified.

1 - 2

1.2 List of G Code Groups

Group Function Remarks

00 Non-modal 01 Positioning/linear interpolation/circular interpolation 02 Plane designation 03 (Absolute programming/incremental programming) 04 Stored stroke check 05 Feed per minute/feed per revolution 06 Inch/metric conversion 07 Cutter compensation 08 *2 09 Canned cycle for drilling 10 Initial point return/R-point return 11 *2 12 Work length modification 13 Cutting mode/exact stop mode/automatic corner override

mode 14 Macro modal call 15 Programmable mirror image 16 Groove width compensation 17 Constant surface speed control 18 Tool life management 19 *2 20 *2 21 *2 22 Polar coordinate interpolation 23 Spindle speed fluctuation detection 24 *2 25 Mirror image for double turrets * 26 *2 27 Automatic tool nose radius compensation/cutter

compensation enable/disable 28 *2 29 *2 30 *2 31 *2

(Notes) *2 Spare G code group for improvement of the functions.

1 - 3

1.3 List of G Codes

Group

01 G00 G00 G00 Positioning

00 G04 G04 G04 Dwell

02 G17 G17 G17 Xp-Yp plane Xp: X axis or its

G code system

ABC

G01 G01 G01 Linear interpolation G02 G02 G02 Circular interpolation/helical interpolation CW G03 G03 G03 Circular interpolation/helical interpolation

CCW

G07 G07 G07 Virtual axis interpolation G09 G09 G09 Exact stop G10 G10 G10 Data setting G11 G11 G11 Data setting mode cancel

designation parallel axis

G18 G18 G18 Zp-Xp plane Yp: Y axis or its

designation parallel axis

G19 G19 G19 Yp-Zp plane Zp: Z axis or its

designation parallel axis

Function Remarks

06 G20 G20 G70 Inch input

G21 G21 G71 Metric input

04 G22 G22 G22 Stored stroke check ON

G23 G23 G23 Stored stroke check OFF

23 G25 G25 G2 5 Spindle speed fluctuation detection OFF

G26 G26 G26 Spindle speed fluctuation detection ON

00 G27 G27 G27 Reference point return check

G28 G28 G2 8 Reference point return G29 G29 G29 Return from reference point G30 G30 G30 2nd, 3rd, 4th reference point return

G301 G301 G301 Floating reference point return

G31 G31 G31 Skip function

01 G32 G32 G3 2 Thread cutting

G34 G34 G34 Variable lead thread cutting

00 G38 G38 G38 Tool nose radius compensation/cutter

compensation vector hold

G39 G39 G39 Tool nose radius compensation/cutter

compensation corner arc

07 G40 G40 G40 Cutter compensation cancel

G41 041 G41 Cutter compensation to the left G42 G42 G42 Cutter compensation to the right

1 - 4

Group

01 G50 G92 G92 Coordinate system setting/spindle

12 G54 G54 G54 Work length modification 1

00 G59 G59 G59 Local coordinate system setting 13 G61 G61 G61 Exact stop mode

00 G65 G65 G65 Macro calling 14 G66 G66 G66 Macro modal call

00 G70 G70 G72 Finishing cycle

G code system

ABC

maximum speed setting G52 G52 G52 Back face machining mode Back G53 G53 G53 Machine coordinate system selection

G55 G55 G55 Work length modification 2 *1

G62 G62 G62 Automatic corner override mode G63 G63 G63 Tapping mode G64 G64 G64 Cutting mode

G67 G67 G67 Macro modal call cancel

Function Remarks

G71 G71 G73 O.D./I.D. roughing cycle G72 G72 G74 End face roughing cycle G73 G73 G75 Closed loop turning cycle G74 G74 G76 End face cutting-off cycle G75 G75 G77 O.D./I.D. cutting-off cycle G76 G76 G78 Compound type thread cutting cycle

09 G80 G80 G80 Drilling cycle cancel

G81 G81 G81 Drilling cycle, spot drilling cycle G82 G82 G82 Drilling cycle, counter boring cycle G83 G83 G83 Peck drilling cycle

G831 G831 G831 Peck drilling cycle

G84 G84 G84 Tapping cycle

G841 G841 G841 Counter tapping cycle G842 G842 G842 Direct tapping cycle *1 G843 G843 G843 Counter direct tapping cycle *1

G85 G85 G85 Boring cycle G86 G86 G86 Boring cycle

G861 G861 G861 Fine boring cycle

G87 G87 G87 Back boring cycle G88 G88 G88 73. Boring cycle G89 G89 G89 74. Boring cycle

1 - 5

Group

01 G9 0 G77 G20 O.D./I.D. turning cycle

17 G96 G96 G96 Constant surface speed control

05 G98 G94 G94 Feed per minute

03 G90 G90 Absolute programming

22 G120 G120 G120 Polar coordinate interpolation mode cancel

00 G128 G128 G128 Scroll cutting speed control 18 G130 G130 G130 Tool life management OFF

G code system

ABC

G92 G78 G21 Single type thread cutting cycle G94 G79 G24 End face turning cycle

G196 G196 G196 Constant surface speed control (Back) Back

G97 G97 G97 Constant surface speed control cancel

G99 G95 G95 Feed per rotation

G91 G91 Incremental programming

G121 G121 G121 Polar coordinate interpolation mode

G131 G131 G131 Tool life management ON

Function Remarks

27 G140 G140 G140 Automatic tool nose compensation/cutter

compensation cancel mode

G143 G143 G143 Automatic tool nose compensation enable

mode

G144 G144 G144 Automatic tool nose radius compensation

enable mode (G144 = G143)

G145 G145 G145 Cutter compensation enable mode

00 G141 G141 G141 Automatic tool nose radius compensation

to the left

G142 G142 G142 Automatic tool nose radius compensation

to the right

16 G150 G150 G150 Groove width compensation cancel

G151 G151 G151 Groove width compensation for end face G152 G152 G152 Groove width compensation for O.D./I.D.

00 G159 G159 G159 Automatic Conversion of Rotation A TC-C

Tool Offset

25 G170 G170 G170 Face machining mode Back

G171 G171 G171 Back face machining mode Back

00 G194 G194 G194 External measurement compensation

1 - 6

Group

10 G198 G198 G198 Canned cycle for drilling initial point return

01 G212 G212 G212 Circular thread cutting CW *1

00 G251 G251 G251 Multibuffer

G code system

ABC

G199 G199 G199 Canned cycle for drilling R-point return

G213 G213 G213 Circular thread cutting CCW *1 G216 G216 G216 S pline interpolation *1 G222 G222 G222 Involute interpolation CW *1 G223 G223 G223 Involute interpolation CCW *1 G232 G232 G232 Exponential function interpolation CW *1 G233 G233 G233 Exponential function interpolation CCW *1

G261 G261 G261 S-designation for the spindle G262 G262 G262 S-designation for the rotary tool G263 G263 G263 S-designation for the subspindle Back

Function Remarks

G271 G271 G271 Cylindrical interpolation

15 G501 G501 G501 Resetting programmable mirror image

G511 G511 G511 Setting programmable mirror image

00 G921 G921 G921 Work coordinate system preset

(Note 1) *1 Reserve G code and not available for the moment. (Note 2) The G code systems, A,B, are selected by the parameters GSB and GSC

(parameter No. 3400).

(Note 3) “Back” in the Remarks column indicates availability for the back machining

system.

1 - 7

1 - 8

2. INTERPOLA TION FUNCTION

2.1 Positioning (G00)

Each axis moves to a program-specified position at an independent rapid traverse rate to perform positioning.

2.1.1 Command Format

G01 X___ Y___ Z___ ...... F___ ;

2.1.2 Sample Program

(1) Absolute programming (2) Incremental programming

G00 X50, Z100, ; G00 X50, Z100, ;

2.1.3 Cautions

(1) The rapid traverse rate has been set independently for each axis. (2) The tool path is non-linear . See to it that the tool does not interfere with the workpiece. (3) Linear acceleration/deceleration is applied. Confirm imposition (an accumulated

amount due to servo delay is within tolerance) at the end of the block, and then, proceed to the next block.

(4) The tool path can be made linear by altering the parameter.

G00 X50, Z100, ;

2 - 1

When linear interpolation positioning has been selected, shifting takes place in the speed which assures the shortest positioning time within the scope not exceeding rapid traverse rate for each axis.

(5) You can set with the parameter whether the reset state is to be the G00 or G01 mode.

2.1.4 Associated Parameters

No.1401, #1= 0 Positioning system is non-linear type.

= 1 linear type (linear interpolation).

No.1401, #6= 0 Dry run disabled for rapid traverse command.

Dry run enabled for rapid traverse command.

No.3402, #0 = 0 Reset state is G00 mode.

= 1 Reset state is G01 mode. No.1420 Rapid traverse rate for each axis. No.1620 Time constant of rapid traverse linear acceleration/deceleration for each axis.

2 - 2

2.2 Linear Interpolation

The toolmvoes linearly to a program-specified position at the cutting feed rate specified with an F code.

2.2.1 Command Format

2.2.2 Sample Program

(1) Absolute programming (2) Incremental programming

G01 X50. Z100. F200 ; G01 X50. W100. F200 ;

2.2.3 Cutting Feed Rate

The cutting feed rate specified with an F code is the speed at which the toolmoves linearly. In this case, the cutting feed rate is a composite speed of all the specified axes; the cutting feed rate of each axis is as follows.

G01 Ua Vb Wc Ff ;

X-axis cutting feed rate Fx = af/2L Y-axis cutting feed rate Fy = bf/L Z-axis cutting feed rate Fz = cf/L

where; L = (a/2)

(Note) When the rotary axis is specified in the identical block, linear interpolation is

performed taking it as a linear axis in the units of degree.

2+b2+c2

2 - 3

2.2.4 Cautions

(1) An alarm results when no F code has been specified in the G01 block or before. (2) Exponential type acceleration/deceleration is applied. (3) Set with the parameter whether the reset state is to be the G00 or G01 mode.

2.2.5 Associated Parameters

No.3402, #0 = 0 The reset state is the G00 mode

= 1 The reset state is the G01 mode No.1422 Maximum cutting feed speed (common to all axes) No.1622 Time constant of cutting feed exponential type acceleration/deceleration No.1623 FL speed of cutting feed exponential type acceleration/deceleration

2.2.6 Associated Alarms

No.102 F has not been specified in cutting feed. Or, F0 has been specified.

2 - 4

2.3 Circular Interpolation (G02, G03)

The tool moves to a program-specified position along an arc within the plane selected with a plane selection G code(G17, G18,G19) at the cutting feed rate specified with an F code.

2.3.1 Command Format

(1) Xp-Yp plane

G17

(2) Zp-Xp plane

G18

(3) Yp-Zp plane

G19

G02 G03 R_

Xp_ Yp_

Zp_ Xp_

Yp_ Zp_

I_ J_

K_ I_

J_ K_

F_ ;

where, Xp : X axis or its parallel axis

Yp : Y axis or its parallel axis Zp : Z axis or its parallel axis

2.3.2 Arc Rotating Direction

G02 : Clockwise (CW) G03 : Counterclockwise (CCW)

2 - 5

2.3.3 Arc Plane

The arc plane is specified with G17, G18, or G19.

G17 : Xp-Y p plane G18 : Zp-Xp plane G19 : Y p-Zp plane

2.3.4 Arc Center

The arc center is specified with I, J, or K corresponding to Xp, Yp, and Zp, respectively. In this case, I, j, and K are the vector components when viewing the arc center from its start point.

(Note 1) Instead of using I, J, and K, you can use R to assign an arc radius.

(R assignment of arc radius) When applying R assignment to an arc of 180° and above, specify an R in minus.

(Note 2) A full circle (360°) is not applicable in R assignment. Use I, J, and K for a full

circle. When an arc close to 180° or to 360° is specified in R assignment, calculation error may be produced, resulting in center deviation. In this case, assign the center by using I, J, and K.

2.3.5 Cutting Feed Rate

The cutting feed rate specified with an F code is the speed at which the tool moves on the arc.

2.3.6 Program Example

(1) Absolute Command Using I, J, and K:

G18 G00 X140. Z13.397 ; G02 X240. Z100. I-50. K86.603 F200 ;

2 - 6

(2) Incremental Command Using I, J, and K:

G18 G02 U100. W86.603 I-50. K86.603 F200 ;

(3) An Arc of 180° or Less Using Radius R Assignment:

G18 G02 U200. W100. R100. ;

(4) An Arc of 180° or more Using Radius R Assignment:

G18 G02 U200. W100. R100. ;

2.3.7 Cautions

(1) An alarm results when no F code has been specified in the G02/G03 block or before. (2) Exponential type acceleration/deceleration is applied. (3) An alarm results if an arc radius = 0 is specified. (4) I0, J0, and K0 are omissible.

2 - 7

(5) When there is no end point on the arc, the tool moves linearly the rest after moving

along an arc if the end point error of circular interpolation is within the parameter set value. Also, an alarm results if it is other than the p arameter set value.

(6) An alarm results if the axis not for the arc plane is specified. (7) When R is specified in the same block as I, J, and K, R is given priority. (8) When the canter of a circular arc is not calculated, alarm takes place.

2.3.8 Associated Parameters

No.1422 Maximum cutting feed speed (common to all axes) No.1622 Time constant of cutting feed exponential type acceleration/deceleration No.1623 FL speed of cutting feed exponential type acceleration/deceleration No.3459 Arc radius error limit value

2.3.9 Associated Alarms

No.102 No F has been commanded in cutting feed. Or, F0 has been commanded. No.131 The R value in arc radius R assignment is erroneous. No.132 An arc for which difference in radius values between the start point and the

end point is larger than the parameter set value has been commanded. (#001) No center command (I, J, K) (#002) Center command (I, J, K) is 0. (#003) Arc end point allowable error is too large.

(Note) When an option for helical interpolation is not added, specifying the axis for other

than the arc plane results in the alarm #191 (OPTION COMMAND).

2 - 8

2.4 Helical Interpolation (G02, G03)

If an arc command and any one axis for other than arc are specified, helical interpolation is enabled by control which performs linear interpolation synchronously with arc movement.

2.4.1 Command Format

(1) Xp-Yp plane

G17

(2) Zp-Xp plane

G18

(3) Yp-Zp plane

G19

G02 G03 R_

Xp_ Yp_

Zp_ Xp_

Yp_ Zp_

I_ J_

K_ I_

J_ K_

.... Not available with

a_ F_ ;

ΣΣ

Σ21L.

ΣΣ

where; Xp : X axis or its parallel axis

Yp : Y axis or its parallel axis Zp : Z axis or its parallel axis α : Any optional linear axis for other than circular interpolation (up to 2 axes) F : Arc speed

2.4.2 Feed Speed

Feed speed command F in helical interpolation is equal to the speed in which a tool moves on an arc. Speed of the straight line axis = F × (length of the straight line axis/the arc length)

2.4.3 Sample Program

G17 G03 U-200. V100. R100. W50. F200 ;

2 - 9

2.4.4 Cautions

(1) See to it that the linear axis speed does not exceed the maximum value. (2) Cutter compensation is applied to circular interpolation. (3) The axes for other than circular interpolation can be specified up to 2 axes.

Specifying 3 axes or more results in an alarm.

(4) The tool speed can be the composite speed of arc and linear speeds by parameter

setting.

2.4.5 Associated Parameters

2.4.6 Associated Alarms

No.149 In helical cutting, 3 or more linear axes have been commanded.

2 - 10

2.5 Virtual Axis Interpolation (G07)

When a virtual axis is assigned, axis shift does not take place. In helical interpolation, by making one of circular command axes as a virtual axis, you can perform SIN interpolation.

2.5.1 Command Format

G07 α 0 ; Sets the α axis as the virtual axis

The α axis is the virtual axis in this section

G07 α 1 ; Cancels the α axis as the virtual axis

where ; α : Any one axis

2.5.2 Sample Program

G07 Y0 ; G17 G03 U0 V0 I-50. Z100. F200 ;

.... Not available with

ΣΣ

Σ21L.

ΣΣ

2.5.3 Cautions

(1) Virtual axis assignment is applicable only to 1 axis. If 2 or more axes should be

assigned, alarm takes place.

(2) When axial shift has been commanded for the axis assigned as a virtual axis, dwell

state equal to the shift time is produced.

(3) Command the virtual axis in incremental.

2.5.4 Associated Alarms

No.139 Two or more virtual axes are specified.

2 - 11

2.6 Cylindrical Interpolation (G271)

The stroke of the rotary axis internally specified in terms of angle is converted into the circumferential distance by specifying the stroke of the linear axis and the angle of the rotary axis with a program command. Since the circumferential distance can be regarded as the stroke of the linear axis on the circumference, linear interpolation and circular interpolation can be performed with other linear axes. Af ter interpolation, it is reconverted into the angle of the rotary axis.

2.6.1 Command Format

G271 C Cylinder radius ; Cylindrical interpolation ON

Cylindrical interpolation mode

G271 C0 ; Cylindrical interpolation cancel

C denotes the rotary axis.

The move angle of the rotary axis is calculated back from the circumferential stroke. For example, when you want to move 100.0 on the circumference of a cylinder whose radixis is 50.0, the move angle of the rotary axis is obtained from the following expression.

r : Cylinder radius θ : Move angle s : Circumferential stroke

Move angle=

(Circumferenttial stroke)

(Cylinder radius)

360×100.0 =

2×

π×50.0

114.591

2 - 12

2.6.2 Feed Rate

Feed rate command F in the cylindrical interpolation mode is the speed at which the tool moves around the perimeter of a cylinder .

2.6.3 Circular Interpolation Axis

A linear as well as a rotating axis for which circular interpolation is performed are set in parameters beforehand (S traight line axis: No.3426, Rot ary axis: No.3427). The set range for both parameters, however, should be within 1~ no. of control axes and the parameters should not be the same for both axis.

2.6.4 Circular Interpolation Plane

During the circular interpolation mode, a plane for which the rotating axis is set to 1st plane axis and the straight line axis to 2nd plane axis is automatically selected.

2 - 13

2.6.5 Sample Program (X Axis is Diameter Specification)

(C-Z plane selected with Parameter No. 3426/3427.)

T0100 ; G98 G145 G40 G80 ; G00 X120.0 Z-120.0 C0 ; G145 ; G271 C50.0 ; Cylindrical interpolation mode ON

N1 G42 G01 Z-40.0 F500 ; (Cylinder radius = 50.0)

G01 X100.0 F100 ; N2 C90.0 F500 ; N3 Z-100.0 C180.0 ; N4 C260.0 ; In the cylindrical N5 G03 Z-80.0 C282.918 R20.0 ; interpolation mode N6 G01 Z-60.0 ; N7 G02 W20.0 H22.918 R20.0 ; N8 G01 C360.0 ; N9 G40 G01 Z-120.0 ;

G271 C0 ; Cylindrical interpolation mode OFF

G00 Z50.0 C0 ;

Developed View of Cylinder Surface with Radius of 50.0

2 - 14

2.6.6 Cautions

(1) Arc radius programming with I, J, or K is not allowed during the cylindrical interpolation

mode. Use radius designation on arc and specify it with the coordinate value on the cylinder surface.

(2) During cylinder interpolation mode, the plane (plane selected by G17 - G19) before

entering the cylinder interpolation node will be canceled once, and then restored after completion of the cylinder interpolation mode.

(3) The circular arc radius specification method (which of the addresses I, J, K to use)

when performing circular arc interpolation during the cylinder interpolation mode, will be decided depending on which axis of the basic coordinate system the second axis (straight line axis) of the cylinder interpolation plane corresponds to, as shown below.

• When the straight line axis is the X axis or parallel to it, Zp-Xp plane will be taken, specified by K, I.

• When the straight line axis is the Y axis or parallel to it, Xp-Yp plane will be taken, specified by I, J.

• When the straight line axis is the Z axis or parallel to it, Yp-Zp plane will be taken, specified by J, K. Also, the circular arc radius can be specified by the R command.

(4) (G271 Cxx) (5) An alarm results if 2 or more rotary axes are specified with the G271 command. (6) Cylindrical interpolation is not available for the following functions:

• Machining break point return

• Manual intervention by manual absolute ON

(7) An alarm results if the following commands are given during the cylindrical

interpolation mode. G28, G30, G53 Machine coordinate system Thhttxx; (T command), G54, G50 Work coordinate system G70-G76, G81-G89, G831-G861, G861 G90-94 Various canned cycles G31, G121, G232 Others

(8) In the cylindrical interpolation mode, the angle of the rotary axis is converted into the

distance on the circumference, and after interpolation, it is converted the other way around. When this is done, a slight conversion error occurs.

(9) Due to the above conversion error, a circular interpolation alarm may occur if circular

interpolation with a small circular arc radius is performed during the cylindrical interpolation mode. When using, care should be taken. Also, a cutter compensation alarm may occur at the time of cutter compensation due to the above reason.

(10) An alarm results if G271 Cxx; (C ≠ 0) (cylindrical interpolation mode ON) is specified

during the cylindrical interpolation mode.

(1 1) The remaining stroke indicates the value at the time of moving on the perimeter of the

cylinder.

2 - 15

2.6.7 Related Parameters

No.3426 Axis number (1 - No of control axes) of the straight line axis for performing

circular interpolation

No.3427 Axis number (1 - No of control axes) of the rotating axis for performing circular

interpolation

2.6.8 Related Alarm

No.126 An error exists in cylindrical interpolation command. (#001) No rotary axis command exists. (#002) No independent command exists. (#003) Modal G code is not in correct state. No.127 An erroneous command has been give while in cylindrical interpolation mode. (#001) An erroneous G code has been commanded. (#003) Rotary axis shifting command has been given in G00 mode. (#004) Cylindrical interpolation has been commanded again while in cylindrical

interpolation mode.

No.189 (G271) Parameter setting is erroneous.

• Parameters No. 3426/No.3427 do not fall within 1 ~ no. of control axes. Or, No.3426 and No.3427 are equal.

• The straight line axis set in Parameter No.3427 does not correspond to or parallel to any of the basic three axes (X, Y, Z).

2 - 16

2.7 Polar Coordinate Interpolation (G120, G121)

Polar coordinate interpolation is a function to provide contour control by converting the command programmed in the orthogonal coordinate system into the movement of the linear axis (tool movement) and that of the rotary axis (workpiece rotation).

The relationship between (X1, C1) and (X1’, C1’) is as follows.

X1’ = X

+ C

C1’ = tan-1 (C1/X1)

2.7.1 G Codes

G121 : Polar coordinate interpolation mode G120 : Polar coordinate interpolation mode cancel

2.7.2 Command Format

G121 ; Turns polar coordinate interpolation mode ON

Performs polar coordinate interpolation.

G120 ; Cancels polar coordinate interpolation mode.

2.7.3 Polar Coordinate Interpolation Axes

A straight line axis as well as a rotating axis for the polar coordinate interpolation are set in the parameters beforehand (S traight line axis: No.3418, Rot ating axis: No.3419). The set range for both parameters should be within 1 ~ no. of control axes and the parameters should not be the same for both axis.

2.7.4 Polar Coordinate Interpolation Plane

When G121 is specified, the polar coordinate interpolation mode is put in effect, and the plane (polar coordinate interpolation plane) is selected, which assumes the origin of the work coordinate system as that of the coordinate system, the linear axis as the first plane axis, and virtual axis (rotary axis) orthogonal to the linear axis as the second plane

2 - 17

axis. Polar coordinate interpolation is performed on this plane. For the position specified by G121, the angle will be taken as 0 and polar coordinate interpolation started, regardless of the actual position. Therefore, create the program by taking the work coordinate value of the rotating axis as 0 when G121 has been specified.

2.7.5 Program Command

(1) The program command in the polar coordinate interpolation mode is given in terms of

the orthogonal coordinate value of the polar coordinate interpolation plane. The rotary axis address is used for the command address of the 2nd plane axis. However, the programmable unit is not degrees; the same unit as that for the 1st plane axis, linear axis (mm or inch). The 2nd plane axis assumes the same designation as the rotary axis; it is neither diameter designation nor radius designation.

(2) During the polar coordinate interpolation mode, linear interpolation (G01) and circular

interpolation (G02, G03) can be specified. Both absolute programming and incremental programming are allowed.

(3) When performing circular interpolation on the polar coordinate interpolation plane, the

circular arc specifying-method (which one of I, J, and K is to be used as the address) is determined as follows depending on to which axis of the basic coordinate system the 1st plane axis (linear axis) corresponds (parameter setting: No.1011).

• When the linear axis is either X axis or its parallel axis, the Xp-Yp plane is assumed, and I/J is used to specify the circular arc radius.

• When the linear axis is either Y axis or its p arallel axis, the Yp-Zp plane is assumed, and J/K is used to specify the circular arc radius.

• When the linear axis is either Z axis or its parallel axis, the Zp-Xp plane is assumed, and K/I is used to specify the circular arc radius.

It is also possible to specify the circular arc radius with an R command.

(4) Cutter compensation can be applied to the program command. Polar coordinate

interpolation is performed for the profile after cutter compensation. However, specify G121 and G120 in the cutter compensation cancel mode (G40).

(5) For feed rate, specify the shift speed of the tool in the polar coordinate interpolation

plane (orthogonal coordinate system) by F. Since this is normally specified by feed per minute (G98), the units of F will be mm/ min, inch/min.

2 - 18

2.7.6 Sample Program (X Axis [Diameter Assigned]: Linear Axis/C Axis[Radius Assigned]: Rotary Axis)

G00 X130.0 C0 ; Positioning to start position G145 ; Tool Diameter Compensation Effective mode

G121 ; Polar coordinate interpolation started. N1 G42 G01 X80.0 F100 ; N2 C40.0 ; N3 G03 X60.0 C50.0 R10.0 ; N4 G01 X-60.0 ; Profile program, N5 C-15.0 ; Program with orthogonal coordinate N6 G03 X-50.0 C-20.0 I5.0 J0 ; values on the X-C’ plane N7 G01 X80.0 ; N8 C0 ; N9 G40 X130.0 ;

G120 Polar coordinate interpolation cancelled.

2 - 19

2.7.7 Speed Clamping of the Rotating Axis

The maximum cutting feed speed for the polar coordinate interpolation can be set in the parameter . (Parameter No.3464) When any speed above this level is specified while in polar coordinate interpolation, it is clamped to this speed. With the set value being 0, clamping is performed to the ordinary maximum cutting feed speed (Parameter 1422) even while in polar coordinate interpolation. Further, in polar coordinate interpolation, as a shape having been programmed in the orthogonal coordinate system are converted into movement of the straight line and the rotating axes, rotating axis speed is increased in movement around the work center (origin of the coordinate system), even exceeding the limit speed of Machine. In the above case, the allowable speed of the rotating axis can be set in the parameter as follows: Allowable speed of rotating axis = Max. cutting feed speed (Parameter No. 3404) x Allowable ratio (Parameter No.3420) When the speed component of the rotating axis exceeds the allowable speed while in polar coordinate interpolation, override shown below is automatically applied (Automatic override):

Allowable speed of rotating axis

Override =

Speed component

× 100(%)

When the speed component of the rotating axis still exceeds the allowable speed even with override being applied, feed speed is clamped so that the speed component of the rotating axis does not exceed the maximum cutting feed speed. (Automatic speed clamp)

2.7.8 Rapid Traverse (G00) Operation

You can issue the G00 command during the polar coordinate interpolation mode. However, only the start point and the end point will be converted to the positions of the polar coordinate system for the G00 block. There will be no conversion during the path from the start point to the end point. Example: In the G121 mode, if the following command is issued:

G00 X100. C50.0 ;

The path will be the same as specified in the following command in the G120 mode:

G01 X141. 421 C45.0 ; In the shift of the rotating axis by G00, close rotation (shift within +/-180 degrees) will be performed and the processing time will be reduced.

2 - 20

2.7.9 Special Specification A for Polar Coordinate Interpolation (Optional)

Through parameter setting, machining by a program of the X-Y coordinate system is made available in the same manner with the machining center. In G121 mode, the following conversion processes will be performed immediately after the program is read in.

• X axis commands are processed as radius commands.

(X axis command is doubled)

• Y axis commands are converted to C axis commands. (Y → C, V → H)

(Note 1) Since the above conversion processes are performed on the basis of axis

name, the parameters must be set with the straight line axis as the X axis and the rotating axis C axis that are subject to the polar coordinate interpolation.

(Note 2) Although X axis commands are possible with radius values, the coordinate

indication will follow the convention of the mechanical specification. (usually diameter values)

(Note 3) Evan if the special specification A for polar coordinate interpolation is employed,

either the standard of special specification can be selected with the parameters.

2 - 21

2.7.10 Cautions

(1) G120 and G120 should be specified in an independent block. (2) Before specifying G121, the work coordinate system where the center of the rotary

axis serves as the origin of the coordinate system must be set. During the G121 mode, the coordinate system must not be altered.

(3) The plane(selected by G17, G18, or G19) prior to G121 is cancelled once by G121 and

restored by G120.

(4) The following G codes can be specified in the G121 mode:

G00, G01, G02, G03, G04, G09, G40, G41, G42, G65, G66, G67, G98, G99, G140, G143, G144, G145

(5) For the axis move command outside the plane of the G121 mode, the axis moves

regardless of polar coordinate interpolation.

(6) The display of the “remaining stroke” in the G121 mode represents that in the polar

coordinate plane (orthogonal coordinates). For G00 block, however, the unit for the ordinary case is applied.

(7) The following functions are not available for the blocks which are in the G121 mode:

Program restart, Machining break point return, Manual intervention by manual absolute ON

(8) On completion of polar coordinate interpolation (G120), the work coordinate of the

rotating axis can be rounded at 360° through parameter setting. (0° coordinate value < 360°)

(9) When the work coordinate value of straight line axis during G121 command is

negative for the first shift block, only the end point will be converted to the polar coordinate system position. There will be no conversion during the shift. (Same as the straight line type G00 in the G121 mode.) From the next shift block, polar coordinate conversion will be performed for the shift path. For the first, shift block, only G00 and G01 can be specified; G02 and G03 cannot be specified.

(10) Through parameter setting, you can specify G codes (G120/G121) for polar coordinate

interpolation by using G126/G127. In specification with G126/G127, they are converted into standard G codes (G120/ G121) when an NC program is read into the buffer . Therefore, command values and alarms are displayed in the standard G codes.

2 - 22

2.7.1 1 Associated Parameters

No.3404, #4= 0 Work coordinates of rotating axis is not rounded on completion of

polar coordinate interpolation.

= 1 Work coordinates of rotating axis is rounded at 360° completion of

polar coordinate interpolation.

No.3404, #6= 0 Y-axis command in the polar coordinate interpolation is moved as Y-

axis command.

= 1 Y-axis command in the is moved by being replaced by C-axis

command.

No.3404, #7= 0 X-axis command in polar coordinate interpolation mode follows

machine specifications.

= 1 X-axis command in polar is taken as radius assignment.

No.3409, #0= 0 G codes for polar coordinate interpolation are G120/G121 (standard)

= 1 G126/G127

No.3410, #1= 0 Neither automatic override nor automatic speed clamp is performed

while in polar coordinate interpolation mode.

= 1 Automatic override and automatic speed clamp are performed while in

polar coordinate interpolation mode.

No.3418 Axis number of the linear axis for which polar coordinate interpolation is

performed

No.3419 Axis number of the rotary axis for which polar coordinate interpolation is

performed

No.3420 Axis number of the linear axis for which polar coordinate interpolation is

performed.

No.3464 Maximum cutting feed speed while in polar coordinate interpolation.

2 - 23

2.7.12 Associated Alarms

No.1 13 An error exists in the polar coordinate interpolation command. (#001) G120/G121 commands is not independent type. (#002) When G120/G121 is specified, cutter compensation has not been cancelled. (#003) When the work coordinate value of the linear axis is in minus on specification

of G121, a command other than G00/G01 has been specified in the first shift block.

No.1 14 An erroneous command has been specified while in the polar coordinate

interpolation mode. (#001) A G code not useable has been specified. (#002) A T code has been specified. No.189 (G121) An error exist s in parameter setting.

• Parameters No.3418/No.3419 are not within 1 ~ no. of control axes, or No.3418 is equal to No.3419.

• The linear axis set in Parameter No.3418 is none of the basic three axes (X/Y/Z), or not parallel to any of them.

2 - 24

2.8 Angle Designated Linear Interpolation

By commanding an angle (A) formed between X or Z axis shifted and +Z axis, you can perform angle designated linear interpolation.

2.8.1 Command Format

G01 X___ A___ ; G01 Z___ A___ ;

2.8.2 Angle A

(1) Scope of angle A

-360.000 A 360.000 (deg)

(2) Angle A code

Plus ..........Counterclockwise angle from +Z axis

Minus ........Clockwise angle from +Z axis

2.8.3 Program Example

G18 G01 U20. A60. ; W20. ; W10. A-30. ;

30°

2 - 25

2.8.4 Cautions

(1) When A is used as an axis name, this function is made invalid.

Address A indicates A axis, not an angle.

(2) Angle designated linear interpolation on other planes (G17/G19) is available.

As this angle A, an angle formed by the horizontal axis of the coordinate system in plus direction (G17:+X, G19:+Y) is commanded.

(3) When the shift direction of the commanded axis and the shift direction after calculation

are opposite, alarm takes place.

G01 W100. A100. ;

<<Available A Range for Commanding in +Z Direction Command>>

2.8.5 Associated Parameters

2.8.6 Associated Alarms

No.177 An error exists in the command of angle designate linear interpolation. (#001) Angle A value is out of the range. (#002) An angle in opposite shift direction has been commanded.

2 - 26

2.9 Skip Function (G31)

Linear interpolation is performed by a G31 command. If an external skip signal is input during linear interpolation, the program proceeds to the next block, stopping the axes and discarding the remaining stroke.

2.9.1 Command Format

G31 X___ Y___ Z___ ....... F___ ;

2.9.2 Sample Program

N1 G98 G31 W50. F100 ; N2 G01 U50. W25. ;

2.9.3 Cautions

(1) G31 cannot be specified while in the corner R compensation/tool system

compensation mode.

(2) When the block next to the G31 command has been given by incremental

programming, the next block functions in the incremental manner from the

positioninterrupted by the skip signal. (3) The G31 command is effective only in the block where it is specified. (4) Position where skip has been input (work coordinates) can be read by the macro

system variable.

2.9.4 Associated Parameters

No.6200, #7= 0 Automatic acceleration/deceleration is made invalid to G31 skip

command.

= 1 Automatic acceleration/deceleration is made valid to G31 skip

command.

2.9.5 Associated Alarms

2 - 27

2 - 28

3. THREAD CUTTING

3.1 Thread Cutting (G32)

With a G32 command, straight threads and tapered threads can be cut ata equal leads synchronously with the pulses from the spindle encoder.

3.1.1 Command Format

(1) Straight thread cutting at equal leads

G32 α___ F___ (E___) ;

where; α : Any one axis

F (E) : Thread lead

(2) Tapered thread cutting at equal leads

G32 α___ β___ F___ (E___) ;

where; α, β : Any one axis

F (E) : Thread lead

(3) Thread cutting at equal leads by specifying the number of threads per inch

G32 α___ β___ E___ ;

where; α, β : Any one axis

E : No. of threads per inch

(Note) Use a parameter to set whether to specify the thread lead with an E code or the

number of threads per inch.

3.1.2 Sample Program

(1) Straight thread cutting at equal leads

G32 W-10. F2.0 ; (2) Tapered thread cutting at equal leads

G32 U-10. W-20. F2.0 ;

(3) Straight thread cutting at equal leads by specifying the number of threads per inch

G32 W-50. E5.0 ;

(5 threads per inch; Thread lead = 5.08 mm)

3 - 1

3.1.3 The Range of Thread Lead will be as Follows

(a) Metric programming

F35 : 0.00001 ~ 999.99999 (mm/rev)

F26 : 0.000001 ~ 99.999999(mm/rev) (b) Inch programming

F26 : 0.000001 ~ 99.999999 (inch/rev)

F17 : 0.0000001 ~ 9.9999999 (inch/rev)

(Note) The number of significant digits for F and E is the same.

3.1.4 Cautions

(a) The feed hold function is disabled during thread cutting. If the FEED HOLD button is

pressed during thread cutting, the program stops at the end point of the block next to

the non-thread cutting block. (b) Cutting feed override and spindle override is disabled and fixed at 100 % during thread

cutting. (c) An alarm results if 3 axes or more are specified in the same block. (d) Give the thread lead (F or E) in the first G32 mode. (e) If E is given during the G32 mode, it remains effective until F is given. Also, if F and E

are given in the same block, F is given priority.

3.1.5 Associated Parameters

No.1401, #5= 0 Dry run disabled during thread cutting and tapping.

= 1 Dry run enabled during thread cutting and tapping.

No.3401, #4= 0 F/E code for thread cutting in inch input is F26.

= 1 F/E code for thread cutting in inch input is F17.

No.3401, #5= 0 F/E code for thread cutting in mm input is F35.

= 1 F/E code for thread cutting in mm input is F26.

No.3403, #7= 0 E code for thread cutting is equal to the number of threads per inch of

the thread lead.

3 - 2

3.1.6 Associated Alarms

No.103 An error exists in the thread cutting command. (#001) Commands have been given for 3 or more axes.

3.2 Continuous Thread Cutting (G32)

Continuous thread cutting is enabled by continuously specifying the thread cutting command blocks.

3.2.1 Sample Program

N1 G32 U-10.0 W-20.0 F3.0 ; N2 W-10.0 ; N3 U10.0 W20.0 ;

3.2.2 Cautions

(a) Stop at single block is not possible during thread cutting.

3 - 3

3.3 Multi-thread Cutting

If you specify Q together with the thread cutting command (G32, G34, G76, G92), you can shift the thread cutting start angle by the specified shift Q. If you execute thread cutting of the same shape after changing the Q value, you can execute multi-thread cutting.

3.3.1 Command Format

G32 α___ β___ Q___ F___ ;

Where, alpha, beta: Any one axis

: Thread lead in the direction of the longitudinal axis

F Q : Thread cutting start shift angle (0 to 360 degrees)

Other thread cutting commands are similar to the one described above.

3.3.2 Example of Program

G32 W-30.0 F2.0 Q180 ;

Shift by 180 degrees with respect to the reference point.

3.3.3 Precautions

(1) Either 1 degree or 0.001 can be selected as the unit for shift angle Q, by parameter

setting. (2) If you have selected 1 degree as the unit for Q, specify Q without the decimal point.

• Q1 → Indicates 1 degree

• Q1.0 → Indicates 1000 degrees

(3) If you have selected 0.001 as the unit for Q, specify Q with the decimal point.

• Q1 → Indicates 0.001 degrees

• Q1.0 → Indicates 1.0 degree

(4) When you use a macro variable in Q, select 0.001 degree as the unit for Q. Example:

Q#510 (5) Even if you select 0.001 in the unit for Q, since the feedback pulse from the spindle

encoder is normally 4096 pulse / rev . , the actual resolution will become 360 degrees/

4096 = 0.088 degree. (6) The Q specification for continuous thread cutting will be effective only in the thread

cutting start block. (7) If the Q specification exceeds the 0 to 360 degree range, alarm will occur .

3.3.4 Related Parameters

No.3404, #2= 0 Unit for the shift angle Q is 1 degree.

= 1 Unit for the shift angle Q is 0.001 degree.

3.3.5 Related Alarm

No.103 An error exists in the thread cutting command. (#001) Commands have been given for 3 or more axes. (#002) Q command value has exceeded the set range.

3 - 4

3.4 Variable Lead Thread Cutting (G34)

Variable lead threads can be cut by specifying an incremental or decremental amount per revolution of thread in the G34 command block.

3.4.1 Command Format

G34 α___ β___ F___ K___ ;

where; α, β : Any one axis

F : Thread lead in the longitudinal direction at thread cutting start time K : Incremental amount (decremental amount for a nagative value) per

revolution

The programmable range of K is as follows.

Metric system : ±0.001 to ±99999.999 (mm/rev) Inch system : ±0.0001 to ±9999.9999 (inch/rev)

3.4.2 Sample Program

Straight thread cutting at variable leads (Thread lead at start time: 2.0 mm, Incremental amount per rev. : 0.5mm)

G34 W-10.0 F2.0 K0.5 ;

In variable lead thread cutting, feed speed is changed constantly as above so that lead is changed for every rotation. The lead for 1st rotation in thread cutting becomes “F± (K/2)” and the lead for 2nd rotation on is increased/decreased by K for every rotation.

3.4.3 Cautions

(1) A G34 command with K omitted results in thread cutting at equal leads (G32

command).

3 - 5

3 - 6

4. FEED FUNCTION

4.1 Feed Per Minute (G98)

Until G99 is specified after G98, specify the stroke per minute (mm/min., inch/min.) with a numerical value following F as to the cutting feed rate.

4.1.1 Command Format

G98 ;

4.1.2 Sample Program

G98 F100 ; The cutting feed rate is 100 mm per minute.

4.1.3 The F Code Programmable Range is as Follows

(1) Metric system

F60 : 1~ 999999 (mm/min)

F61 : 0.1~ 999999.9 (mm/min) (2) Inch system

F51 : 0.1~ 99999.9 (inch/min)

F52 : 0.01~ 99999.99 (inch/min)

4.1.4 Cautions

(1) One of F60, F61, F51, and F52 is selected by. parameter setting. (2) When F61 is specified without a decimal point in the metric system, the least input

increment of 1 mm/min. or 0.1 mm/min. can be selected by parameter setting. (3) In case of thread cutting (G33), feed per revolution is assumed temporarily even

during the G98 mode.

4.1.5 Associated Parameters

No.3400, #1= 0 The unit without a decimal point for metric input F61 is 1mm/min.

= 1 The unit without a decimal point for metric input F61 is 0.1mm/min.

No.3401, #2= 0 Feed per minute for inch input is F51.

= 1 Feed per minute for inch input is F52.

No.3401, #3= 0 Feed per minute for metric input is F60.

= 1 Feed per minute for metric input is F61.

4.1.6 Associated Alarms

No.102 F has not been specified in cutting feed. Or, F0 has been specified.

4 - 1

4.2 Feed Per Revolution (G99)

Until G98 is specified after G99, specify the stroke per minute (mm/rev., inch/rev.) with a numerical value following F as to the cutting feed rate.

4.2.1 Command Format

G99 ;

4.2.2 Sample Program

G99 F12 ; The cutting feed rate is 1.2 mm per revolution.

4.2.3 The F Code Programmable Range is as Follows

(1) Metric system

F32 : 0.01 ~ 999.99 (mm/rev)

F33 : 0.001 ~ 999.999 (mm/rev) (2) Inch system

F23 : 0.001 ~ 99.999 (inch/rev)

F24 : 0.0001 ~ 99.9999 (inch/rev)

4.2.4 Cautions

(1) One of F32, F33, F23, and F24 is selected by parameter setting.

4.2.5 Associated Parameters

No.3401, #0 = 0 Feed per rotation for inch input is F23.

= 1 Feed per rotation for inch input is F24.

No.3401, #1= 0 Feed per rotation for metric input is F32.

= 1 Feed per rotation for metric input is F33.

4.2.6 Associated Alarms

No.102 F has not been specified in cutting feed. Or, F0 has been specified.

4 - 2

4.3 Dwell (G04)

A G04 command can delay migration of operation to the next block. When specifying by time: The command causes the machine to wait for the

When specifying by revolutions: The command causes the machine to wait while the

4.3.1 Command Format

(1) When specifying by time

G98 G04 P___ ; P: Dwell time (0.001 to 99999.999 sec.)

(2) When specifying by revolutions

G99 G04 P___ ; P: Dwell revolutions (0.001 to 99999.999 rev .)

(Note) X or U can be used instead of P.

4.3.2 Sample Program

specified time.

spindle rotates the number of revolutions specified.

G98 G04 P2000 ; Dwell time 2 seconds G04 X2.0 ; Dwell time 2 seconds

4.3.3 Cautions

(1) It is normally set to dwell specified by time (per-minute dwell).

Through parameter setting, however , dwell specified by rot ation (per-rot ation dwell)

can be set in the per-rotation feed mode.

4.3.4 Associated Parameters

No.3400, #5= 0 G04 always specfies by time

1 G04 follows G94 or G95

4 - 3

4.4 Exact Stop (G09)

If a G09 command is specified in the same block as a move block, it decelerates and stops the machine upon completion of one block, and after confirming that the machine position is within the range in which a command position was specified, executes the next block.

4.4.1 Command Format

G09 .......... ;

4.4.2 Sample Program

N1 G09 G01 W50.0 F2.0 ; N2 G01 U-50.0 ;

4.4.3 Associated Parameters

No.1801, #4= 0 Imposition width for cutting feed is Parameter No.1826 (Common to

rapid traverse)

= 1 Imposition width for cutting feed is Parameter No.1827 (Common to

rapid traverse) No.1826 Imposition width of each axis No.1827 Imposition width of each axis for cutting feed

4 - 4

4.5 Exact Stop Mode (G61)

Until G62, G63, or G64 is specified after G61 was specified, this function decelerates and stops the machine, confirms that the machine position is within the specified range, and then, proceeds to the next block.

4.5.1 Command Format

G61 ;

4.5.2 Sample Program

N1 G61 G01 W-100. F1.0 ; N2 U50. ; N3 W-100. ;

The corner has an edge when the G61 mode is effective. The corner is rounded when the G61 is ineffective.

4.5.3 Switching Into M Code

Through setting a parameter, you can specify Exact Stop mode by using M21 command instead of using G61 command. M21, as it is replaced by G61 inside NC for execution, is not output in Machine side. Also, with M21 command, G62 to G64 modes are cancelled.

4.5.4 Associated Parameters

No.1801, #4 = 0 Imposition width for cutting feed is Parameter No.1826 (Common to

rapid traverse)

= 1 Imposition width for cutting feed is Parameter No.1827 (Common to

rapid traverse) No.3409, #1 ON/OFF command system for Exact Stop mode is:

= 0 G61 (ON) / G64 (OFF)

= 1 G61 or M21 (ON) / G64 or M22 (OFF) No.1826 Imposition width of each axis No.1827 Imposition width of each axis for cutting feed

4 - 5

4.6 Automatic Corner Override Mode (062)

When cutter compensation is applied, since the tool center path is located inside the program-specified path in the inner corner and inner arc area and a cutting load increases, an override is applied automatically to the cutting feed ate to reduce the cutting load. Once G62 is specified, it remains effective until G61, G63, or G64 is specified.

4.6.1 Command Format

G62 ;

4.6.2 Override Conditions

When the following conditions are met with respect to the blocks which are located before and after the corner in the cutter compensation mode, an override is applied to cutting feed automatically. (a ) When the G code of Group 01 is G1, G02, or G03. (b ) When an offset amount is not 0 in the cutter compensation offset mode. (c ) When an offset is inside at the corner (d ) When there is an axis in the offset plane. (e ) When the G41 or G42 is not contained. ( f ) When an inner corner angle is smaller than a parameter set value. (θ) (g ) When a corner start distance and a corner end distance are other than 0 and internal.

(Le, Ls)

.... Not available with

ΣΣ

Σ21L

ΣΣ

4.6.3 Override Amount

1 Automatic corner override 100 (%)

An actual cutting feed rate is as follows.

F × Automatic corner override × Cutting feed rate override

where; θ : Inner criterion angle

Le : Start distance

Ls : End distance An override is applied to cutting feed from the point a through the point b.

4 - 6

4.6.4 Sample Program

N1 G62 G42 G00 U40. V50. ; N2 G01 U100. F200 ; N3 G03 U60. V-30. R30. ; N4 G64 G40 G00 U40. ;

4.6.5 Cautions

(1) When a block not shifting has been specified between two blocks subject to automatic

corner override, tool diameter compensation is supplied while automatic corner override is not.

4.6.6 Associated Parameters

No.1711 Inner criterion angle of automatic corner override (θ : deg.) No.1712 Override of automatic corner override (%) No.1713 Start distance (Le) of automatic corner override No.1714 End distance (Ls) of automatic corner override

4 - 7

4.7 Tapping Mode (G63)

The control state of the NC unit is as follows until G61, G62, or G64 is specified after G63 is specified. (1) Cutting feed rate override fixed at 100 % (2) Spindle override fixed at 100 % (3) Single block disabled (4) Dry run disabled (5) Feed hold disabled (6) Decelerated stop disabled at the joint of the blocks (imposition check disabled) (7) Tapping mode signal output The G63 mode is effective until G61, G62, or G64 is specified.

4.7.1 Command Format

G63 ;

4.7.2 Sample Program

N1 G63 G01 X10. F200 ; N2 Z0 ; N3 X20. ; N4 Z-5. ; Tapping mode effective blocks. N5 X30. ; N6 Z-10. ; N7 G64 X40. ;

4.7.3 Cautions

(1) By parameter setting, you can invalidate dry run disabled.

4.7.4 Associated Parameters

No.1401, #5= 0 Enables dry run during thread cutting and tapping.

= 1 Disables dry run during thread cutting and tapping.

4 - 8

4.8 Cutting Mode (G64)

Until G61, G62, or G63 is specified after G64 was specified, the next block is executed continuously without decelerating to a stop between the blocks. The G64 mode is effective until G61, G62, or G63 is specified. When cutting is performed in the G64 mode, the corner may be rounded at the time of cutting feed.

4.8.1 Command Format

4.8.2 Sample Program

N1 G64 G01 X10. F200 ; N2 Z0 ; N3 X20. ; N4 Z-5. ; Cutting mode effective blocks N5 X30. ; N6 Z-10. ; N7 G61 X40. ;

4.8.3 Switching Into M Code

Through setting a parameter , you can specify Cutting mode by using M22 command instead of using G64 command. M22, as it is replaced by G64 inside NC for execution, is not output in Machine side. Also, with M22 command, G61 to G63 modes are cancelled.

4.8.4 Associated Parameters

No.3409, #1 ON/OFF command system for Exact Stop mode is:

= 0 G61 (ON) / G64 (OFF) = 1 G61 or M21 (ON) / G64 or M22 (OFF)

4.8.5 Cautions

(1) G64 is set in the reset state. (2) A G00 command decelerates the machine to a stop regardless of the G64 mode.

4 - 9

4.9 Multibuffer (G251)

During automatic operation, the number of blocks to be preread is as follows. (1) During the automatic tool nose radius compensation enable mode (G143) → 4 blocks (2) During cutter compensation (G41/G42 in the G145 mode) → Max. 4 blocks (3) Others → 1 block A multibuffer command prereads up to 12 blocks. This function makes it possible to reduce a stop time between the blocks when executing the program having very small continuous blocks.

4.9.1 Command Format

G251 P0 ; or G251 ; Multibuffer mode ON G251 P1 ; Multibuffer mode ON

4.9.2 Sample Program

G251 ; Multibuffer mode ON

Prereads up to 12 blocks in this portion.

G251 P1 ; Multibuffer mode OFF

4.9.3 Cautions

(1) The macro statement is not included in the number of preread blocks. (2) Specify the G251 command in an independent block. (3) When the very small blocks are executed continuously, there will be no preread

blocks, making an execution time shorter than the processing time of one block.

(4) The blocks may not be preread even in the multibuffer mode ON state, depending on

the commands. (Example) G10, G20, G21, G22, G23

G28, G30, G31, G53 M00, M01, M02, M30 Coordinate system setting by a T command

(5) The reset state can be turned to the multibuffer mode ON state by parameter setting.

4.9.4 Associated Parameters

No.3402, #6= 0 Multibuffer mode OFF at reset time

= 1 Multibuffer mode ON at reset time

4.9.5 Associated Alarms

No.130 There is an erroneous command in the block.

(#001) G251 is not an independent command.

4 - 10

4.10 Acceleration/Deceleration Control

4.10.1 Automatic Acceleration/Deceleration

Acceleration/deceleration are automatically applied at the start and the end of shifting so that the machine system is protected from shock. Acceleration/deceleration include the following types:

[Linear type [Exponential type acceleration/deceleration] acceleration/deceleration]

[Bell type acceleration/deceleration]

(1) Acceleration/deceleration types for standard setting are as follows:

1) Rapid traverse........................................... Linear acceleration/deceleration

2) Cutting feed (G01, G02, G03, G32) ........... Exponential type acceleration/

3) Manual continuous feed (JOG feed)..........Exponential type acceleration/

4.10.2 Other Acceleration/Deceleration (Optional)

(1) Rapid Traverse Bell Type Acceleration/Deceleration

Rapid traverse bell type acceleration/deceleration, through application of smooth acceleration/deceleration to rapid traverse speed, can reduce mechanical shock due to change in acceleration. Compared with linear acceleration/deceleration, this enables setting of smaller time constant, thus shortening time required for acceleration/deceleration.

(2) Linear Acceleration/Deceleration Following Cutting Feed Interpolation

Compared with the exponential type acceleration/deceleration, the linear acceleration/ deceleration following cutting feed interpolation reduces delay to a command to 1/2, when given the same time constant, thus reducing time required for acceleration/ deceleration.

deceleration

4 - 11

Further, in the arc interpolation especially in high speed cutting, the actual tool p ath subject to acceleration/deceleration has an error to the arc in its radius direction. This error,. also, is reduced compared with that in the exponential type acceleration/ decelation.

(3) Bell T ype Acceleration/Deceleration Following Cutting Feed Interpolation

Bell type acceleration/deceleration following cutting feed interpolation is a function to reduce shock given to the mechanical system by smoothing acceleration and deceleration.

4.10.3 Associated Parameters

No.1610, #0/#1 Acceleration/Deceleration Available for Cutting Feed

(Including feed by dry run) :

Parameter No.1610

#1 #0

0 0 Exponential type acceleration/deceleration 0 1 Linear acceleration/deceleration following interpolation 1 0 Bell type acceleration/deceleration following interpolation

No.1610, #4= 0 Acceleration/deceleration for manual continuous feed (JOG feed) is by

exponential type acceleration/deceleration.

= 1 Acceleration/deceleration for manual continuous feed (JOG feed) is by

the same way as that of cutting feed.

No.6200, #7= 0 Automatic acceleration/deceleration of skip function (G31) is made

invalid.

= 1 Automatic acceleration/deceleration of skip function (G31) is made

valid.

No.1620 Time constant of linear acceleration/deceleration of rapid traverse for each

axis or time constant of rapid traverse bell type acceleration/deceleration T1.

No.1621 Time constant of linear acceleration/deceleration of rapid traverse for each

axis T2.

No.1622 Time constant of cutting feed exponential type acceleration/deceleration for

each axis, time constant of bell type acceleration/deceleration following cutting feed interpolation, or time constant of linear acceleration/deceleration following cutting feed interpolation.

No.1623 FL speed of exponential type acceleration/deceleration of cutting feed for each

axis.

Acceleration/Deceleration

4 - 12

No.1624 Time constant of exponential type acceleration/deceleration of manual

continuous feed for each axis, time constant of bell type acceleration/ deceleration following interpolation, or time constant of linear acceleration/ deceleration following interpolation.

No.1625 FL speed of exponential type acceleration/deceleration of manual continuous

feed for each axis.

No.1626 Time constant of exponential type acceleration/deceleration of thread cutting

cycle for each axis.

No.1627 FL speed of exponential type acceleration/deceleration of thread cutting cycle

for each axis.

4 - 13

4 - 14

5. SPEED CONTROL

5.1 Feed Speed Command (F Data)

5.1.1 Modal In Per-Minute Feed and Per-rotation Feed

Feed rate “F”, once commanded, remains valid (modal) until the next command is given. However , as “F” role is tot ally different between per-minute feed and per-rotation feed, it is hardly of any use even if “F” is held modal in per-minute feed and per-rotation feed. Oppositely, it can even cause danger.

For example, it can be dangerous if, after “F” having been commanded in per-minute feed, axis shift is performed in per-rotation feed without commanding “F”.

N1 G98 G01 Z__ F2000 ; Speed is 2000mm/min N2 G99 Z__ ; Speed is 20.00mm/rev

Modal “F”, therefore should be treated as follows:

Per-minute feed and per-rotation feed (incl. thread cutting) are held modal independently.

In other words, NC holds two “F” data including ones for per-minute feed and the other for per-rotation feed. Depending on the feed mode for execution, the “F” to be used is determined. They are explained in details as follows: The number of effective digits below a decimal point for “F” are 0 for per-minute feed/ 2 for per-rotation feed/ 5 for thread cutting. And, “F” being made valid in that block is expressed in [ ].

(Per-Minute Feed) (Per-Rotation Feed)

On Supply of Power 0 0.00 N1 G99 F1.23 ; 0 [1.23] N2 ——— ; 0 [1.23] N3 G98 F1000 ; [1000] 1.23 N4 ——— ; [1000] 1.23 N5 G32 F2.34567 ; 1000 [2.34567] N6 ——— ; 1000 [2.34567] N7 G99 ; 1000 [2.34] N8 ——— ; 1000 [2.34] N9 G98 ; [1000] 2.34 N10 —— ; [1000] 2.34 N1 1 G32 ; 1000 [2.34567]

5 - 1

Also, when the feed per minute F is specified, the feed per revolution F can be made 0 by parameter setting (No. 3401, #7=1) ; conversely, when the feed per revolution F is specified, the feed per minute F can be made 0. In this case, for the previous example, the feed per revolution F = 0 in N3 and the feed per minute F = 0 in N5, therefore, the effective F in N9, N10, N11 will become 0.

When the inch input/mm input is changed by using the G code (G20/G21), inch/mm conversion will be performed for modal data “F” also.

1000mm/min ←→ 39.3inch/min

5.1.2 F Command for Rotating Axis by Inch Input

The shift (deg) of rotating axis (C) is converted to inch and used.

[Example 1] G98 G01 U10.0 W20.0 H30.0 F20.0 ;

30 (deg) will be treated as 30 (inch).

Interpolation, distance (L) is:

L = (10/2)2 + 202 + 302 = 36.401 (inch)

Interpolation distance (T) is:

T = L/F = 36.401/20 = 1. 82(min)

Speed (Fc) of axis C becomes:

Fc = 30/T = 16 .483 (deg/min)

[Example 2] G98 G01 H360.0 F180.0 ;

L = 360 (inch) T = 360/180 = 2 (min) Fc = 360/T = 180 (deg/min)

5 - 2

5.2 Changing of Inner Circular Cutting Speed

.... Not available with

For circular cutting which is offset internally while in the tool diameter compensation mode, the override equal to the ratio of a radius of the tool diameter center path to a radius of the program path is applied to the specified cutting feed speed.

Cutting rate of the tool diameter center path is as follows:

F × Rc/Rp where Rc : Radius of tool center path

ΣΣ

Σ21L

ΣΣ

Rp : Radius of program path

5.2.1 Cautions

(1) Inner circular cutting speed change is part of the automatic corner override function.

Therefore, this function is invalid unless the automatic corner override function is added.

(2) Through parameter setting, changing of inner circular cutting speed is made valid in

G62 mode.

(3) When Rc/Rp value is smaller than the parameter set value, use the minimum override

of the parameter.

(4) When automatic corner override is added to inner circular cutting, the cutting feed

speed gets as follows:

F × (Rc/Rp) × Auto corner override × Cutting feed rate override

5.2.2 Associated Parameters

No.3406, #0= 0 Change of inner circular cutting speed is held always valid.

= 1 Change of inner circular cutting is speed valid in G62 mode.

No.1710 Minimum override of inner circular cutting speed

5 - 3

5.3 Scroll Cutting Speed Control (G128)

Scroll (vobute) shape can be cut by performing straight line interpolation of rotating axis and the straight line axis that moves in the direction of the diameter. However, in the straight line interpolation (G01) of the straight line axis and rotating axis, the cutting speed normally does not become constant. This is because the interpolation sped is constant, regardless of the position (radius of circle) of the straight line axis.This function controls the interpolation speed of the straight line axis and the rotating axis based on the position of the straight line axis so that the cutting speed becomes equal to the command speed at that position.

5.3.1 Command Format

G128 G98 G01 α___ β___ F___ (E___) (Q___) (p___) ;

G128: One-shot G code that indicates that this function is performed G98 : Feed per minute G01 : Straight line interpolation

α : End point position of straight line axis (mm, inch) β : End point position of rotating axis (deg)

F : (First) cutting speed (mm/min, inch/min) (E) : Second cutting speed (mm/min, inch/min) (Q) : Speed changeover remaining angle (degree) (P) : Inside cutting / outside cutting specification (1: Outside, 2: Inside)

5 - 4

5.3.2 Control Axis

It is necessary to set in advance, in the parameters (linear axis: No.3418, rotating axis: No.3419), the straight line axis and the rotating axis which are subject to scroll cutting speed control. Where, however , No.3418 ≠ No.3419. These parameters will be used for polar coordinate interpolation (G121) also.

5.3.3 Speed Control Method

The interpolation speed is changed according to the change in the cutting radius, so that the cutting speed at that position becomes the command speed. Since a work coordinate value of a straight line axis is employed for the cutting radius (1/2 when the diameter is specified), the origin of the work coordinate system must match the center of the work rotation. Since the work coordinate value is not showing the cutting position but the tool center, however, the speed will not be controlled for the cutting position but the tool center if the work coordinate is selected as the cutting radius. (The acutual cutting position is equal to the work coordinate position ± the tool radius.) When the address P is specified, the cutting radius can be the corrected value of the absolute work coordinate with the tool radius (addition or subtraction). P=1 : Outer cutting correction (subtracting the tool radius) P=2 : Inner cutting correction (adding the tool radius) Value of P other than above or P omitted: No compensation

(Note 1) Specify address P without the decimal point. (Note 2) Set the tool compensation amount “R (shape), Q (wear)” in the tool diameter.

The tool diameter becomes R + Q. Set 9 in the virtual tip point (T). Compensation will not be performed if the value is other than 9.

5 - 5

5.3.4 Speed Changeover Function

By specifying address E (second cutting speed) and address Q (speed changeover remaining angle) in the same block as G128, the cutting speed can be changed during execution of that block. When the remaining shift of the rotating axis becomes less than Q, the cutting speed will be changed from F to E. Both the remaining shift of the rotating axis and the Q value will be treated as absolute values (no symbols). This function will be effective when both E and Q are specified and whez Q is not equal to

0. If this condition is not satisfied, the cutting speed will become the normal first cutting speed F. Q at this stage indicates the angle, therefore, the position of the decimal point of the data is the same as the position of the decimal point of the address.

5 - 6

5.3.5 Program Example (Straight Line Axis: X Axis, Rot ating Axis: C Axis)

N1 T△△ 00 ; N2 M13 ; Rotating tool forward rotation N3 G00 X150.0 Z10.0 C0 ; N4 X85.0 ; N5 Z-10.0 ; N6 G98 G01 X90.0 F2000 ; Approach the start position N7 G128 X30.0 C-720.0 ; F800 W600 Q90.0 P2 ; Scroll cutting (inside)

Tool diameter: 5 mm Tool center path (800 mm/min)

○○○

Gutting point path Tool center path (600 mm/min)

5 - 7

5.3.6 Precautions

(1) G128 is a one-shot G code and is effective only in the specified block. (2) The G128 function can be executed only during straight line interpolation (G01) in feed

per minute (G98).

(3) The axes that can be controlled are two in number - the straight line axis and the

rotating axis set in the parameters. Make sure you specify the two axes in the G128 block and do not specify any other axis. If this condition is not satisfied, alarm will be output.

(4) When the shift of the straight line axis or the rotating axis is 0, the G128 function

becomes ineffective, similar to the condition when G128 is not specified. (No alarm will be output.)

(5) Alarm will be output if there is an error in the parameter setting.

• When Parameter No.3418 is equal to No.3419.

(6) Feed override is effective. The specified speed to which override is applied, will

become the cutting speed.

(7) Dry run is effective but the dry run speed will become the compensated speed, and

not the cutting speed. (Same as the condition when G128 is not specified.)

(8) The work coordinate of the straight line axis will be used in the radius value at the

cutting position. Therefore, set the work coordinate system so that the origin of the work coordinate system is at the center of the work rotation.

(9) The following restrictions will be applied to the coordinate values of the start and end

points of a straght line axis.

• Neither of the specified coordinate values of the start and end points should be zero.

• The signs of the spcified coordinate values of the start and end points should be

equal. (When the start point is positive, the end point should be also positive. When the start point is negative. the end point should be also negative.)

• Both of the cutting radiuses of the start and end points should not be zero or negative.

Unless these conditions are met, the alarm will be given.

5 - 8

5.3.7 Related Parameters

No.3418 Axis number of straight line axis performing G128 (1 ~ no. of control axes) No.3419 Axis number of rotating axis performing G128 (1 ~ no. of control axes)

5.3.8 Related Alarms

No.183 Error in the G128 command. (#001) It is not G98/G01. (#002) An error exists in an axial command. (#003) Start/end points of straight line axis are not correct. No.189 (G128) Error in the parameter setting.

5 - 9

5.4 Speed Control of Independent Axis

Offset speed F of the normal axis NC (X, Y, Z etc.) has following meanings. [1] Supplement of straight line (G01) : speed on diagonal line [2] Supplement of arc (G02 and G03) : speed on circumference [3] Wrenching (G32) : speed of an axis with greater amount of movement (lead of screw) However, the normal speed control is insufficient for axes which move during the planing and are not involved in the planing, namely “the oscillation halt axis” which is used to halt oscillation generated during rotation in a long work. If the oscillation halt axis and the planing axis are specified in the same block, the actual planing speed does not equal the specified speed F. (The more the movement amount of the oscillation halt axis increases, the more the planing speed decreases.) Therefore, the oscillation halt axis is called “independent axis”, and the other axes are called “the ancillary axes”. And the following function is added.

“Speed control function which makes the planing speed of the ancillary axis F regardless of the movement amount of the independent axis.”

This control function is called "speed control function of the independent axis".

5.4.1 Specification of Indepandent Axis

It is possible to control, as an independent axis, only one among CNC control axes. The independent axis is assigned in Parameter No.1012, #6.

(Note) When two or more axes being assigned as independent axes, an axis with the

smallest axis number is controlled as an independent axis.

5.4.2 Control Contents

(1) Block in which speed control of the independent axis is performed

Speed control of the independent axis performed only in blocks which meet the following conditions.

• G01 (straight line supplement), G32 (wrenching), G34 (wrenching of variable leads) However, G01 in G128 (scroll planing speed control) is excepted.

• The ancillary axes and independent axes are moving in the same block.

(2) Speed control of independent axis

When speed control of the independent axis is performed, speed of each axis is controlled in order that;

• Speed of the ancillary axis equals the specified speed F (The same as when independent axis is not specified.), or

• Speed of the independent axis equals the speed of simult aneous termination of supplement with ancillary axis.

5 - 10

If the supplement distance of the ancillary axes is Ld, and the movement distance of the independent axes is Li, speed of the independent axis (Fi) is expressed as follows.

Fi = Li × F / Ld (F: Command speed = Speed of ancillary axis)

(Notes) Feeding override is effective. (Speed of each axis is overridden.)

In the case of dry run, speed of ancillary axis becomes the dry run speed.

5.4.3 Operation Examples to be Controlled

If axes X and Z are ancillary axes, axis A is an independent axis, and each axis makes the following commands from the work coordinates 0, speed of the independent axis is expressed as follows. (1) G01 (straight line supplement)

G98 G01 X50.0 Z100.0 A200.0 F100 ;

• Supplement distance of ancillary axis

Ld = (50/2)2 + 1002 = 103.078 (mm)

• Speed of independent axis

Li Fi = Ld 103.078

× F =

200 × 100

= 194.028 (mm/min)

(*1) The X axis is processed by radius value conversion. (*2) Feeding for each rotation is processed by radius value conversion.

(2) G32 (Wrenching)

G32 X50.0 Z100.0 A200.0 F10.0 ;

• Supplement distance of ancillary axis. Ld = 100 (mm) → Movement amount of the X-axis (25mm) is larger than that of the Z-axis (100mm)

• Speed of independent axis

Li Fi = Ld 100

(*1) In the case of taper wrenching, though this processing method has been

traditionally used, more than two axes can not be specified.

(*2) In the case of G34 (variable lead wrenching), speed of the A-axis varies as the

speed of the independent axis changes.

× F =

200 × 100

= 20.0 (mm/rev)

5.4.4 Operation Not to be Controlled

Special processing is not performed for the code G other than above. And an axis which is specified as an independent axis is treated as an ancillary axis. Main codes G not to be controlled are described below. (1) In the case of G00 (location setting)

Location setting of the non-straight form (standard) and the straight form is performed as before.

5 - 11

(2) In the case of G02 and G03 (arc supplement)

Conventional processing is applied.

• The independent axis is inside the arc surface.

• The independent axis is outside the arc surface.

(3) In the case of fixed cycle (single, complex, holing)

Usually independent axis is not specified in the fixed cycle. If fixed cycle is specified, and is executable, it will be executed. However, operations conform to their specifications, because they are composed of G00, G01 and G32.

5.4.5 Notes

(1) If speed control of the independent axis is performed, speed of the independent axis

will be proportional to the ratio of the supplement distance of the ancillary axis and the movement distance of the independent axis. Therefore, if [supplement distance of ancillary axis] << [movement distance of independent axis] (Right side is much larger than left side.), speed of the independent axis will be excessively high. Therefore, this should be considered when creating programs.

(2) For the block in which speed control of the independent axis is performed, manual

absolute becomes OFF. (Offset of the amount of manual intervention will not be performed for the movement after the manual intervention.)

→This cannot happen, but if it is specified, usual arc is executed.

→Helical supplement is executed. Straight line command upon the Helical

supplement effective in only two axes. Therefore, there is no problem in the execution. However , alarm is generated, if option of the Helical supplement is not att ached.

5 - 12

6. REFERENCE POINT

6.1 Automatic Reference Point Return (G28)

After positioning the axes specified by the program to the intermediate point, a G28 command can automatically return them to the 1st reference point.

6.1.1 Command Format

G28 X___ Y___ Z___ ...... ;

6.1.2 Sample Program

G28 U100. W25. ;

6.1.3 When G28 is Specified without Completing Manual Reference Point Return After Turning on the Power.

After positioning the program-specified axes to the intermediate point, reference point return is performed automatically in the same sequence as manual reference point return. When OT takes place before completion of the reference point returning, following returning to the deceleration dog, reference point returning is performed once again.

6.1.4 Cautions

(1) If G28 G53 X___ Y___ Z___ ... ; is specified, the axes are positioned to the specified

position of the machine coordinate system, and then, they return to the reference point.

(2) The G28 command confirms imposition upon return to the reference point.

6.1.5 Related Parameters

No.1225 Machine coordinate values of 1st reference point for each axis

6 - 1

6.2 Reference Point Return Check (G27)

After positioning the axes to the program-specified position, a G27 command checks whether that position is the 1st reference point, and if not, an alarm results.

6.2.1 Command Format

G27 X___ Y___ Z___ ...... ;

6.2.2 Sample Program

G27 X100. Z-50. ; After the X axis moved to 100.0 and the Z axis to -50.0, it is checked whether they have returned to the 1st reference point.

6.2.3 Cautions

(1) The position reached with a G27 command includes tool offset, tool nose radius

compensation, and cutter compensation amounts. (2) Only the axis specified in the G27 block is checked whether it has returned. (3) No reference point return check is not made on the axis for which the machine lock

function is turned on. (4) The G27 command confirms imposition after positioning.

6.2.4 Associated Parameters

6.2.5 Associated Alarms

No.F092 It has not been returned to the origin.

6 - 2

6.3 Return from Reference Point (G29)

A G29 command positions the program-specified axes from the reference point to the intermediate point of G28 or G30 specified just before, and then, positions them to the specified position.

6.3.1 Command Format

G29 X___ Y___ Z___ ...... ;

6.3.2 Sample Program

N1 G28 U100. W25. ; N2 G29 U-70. W-10. ;

6.3.3 Cautions

(1) If 029 is specified with no G28 or G30 specified once, the intermediate point becomes

zero.

6 - 3

6.4 2nd-4th Reference Point Return (G30)

A G30 command can automatically return program-specified axes to the 2nd-4th reference point after positioning them to the intermediate point. The 2nd ~ 4th reference points are set in parameters at positions set especially for the machine.

6.4.1 Command Format

G30 P___ X___ Y___ Z___ ...... ;

P = 2, 3, and 4 correspond to the 2nd through 4th reference points, respectively. If P is omitted, the 2nd reference point return is assumed.

6.4.2 Sample Program

G30 P3 U100 . W25. ;

6.4.3 Cautions

(1) If G30 G53 X___ Y___ Z___ ...... ; is specified, the axes are positioned to the

specified position of the machine coordinate system, and then, return to the reference point.

(2) The G30 command confirms imposition upon return to the reference point.

6.4.4 Associated Parameters

No.1226 Machine coordinate value of 2nd reference point of each axis No.1227 Machine coordinate value of 3rd reference point of each axis No.1228 Machine coordinate value of 4th reference point of each axis

6 - 4

6.5 Floating Reference Point Return (G301)

A G301 command can automatically return the axes specified by the program to the floating reference point after positioning them to the intermediate point. The floating reference point is the set position on the machine. The floating reference point can be set in accordance with the following operation.

6.5.1 Command Format

G301 X___ Y___ Z___ ...... ;

6.5.2 Sample Program

G301 U100. W25. ;

.... Not available with

ΣΣ

Σ21L

ΣΣ

6.5.3 Cautions

(a) G301 G53 X___ Y___ Z___ ; returns the axes to the floating reference point after

positioning them to the specified position of the machine coordinate system.

(b) The G301 command confirms imposition upon return to the floating reference point.

6.5.4 Associated Parameters

No.1229 Floating reference point of each axis

6 - 5

6 - 6

7. COORDINA TE SYSTEM

7.1 Tool Nose Coordinate System

The tool nose coordinate system always presents the distance between the tool nose position and machining origin correctly. Therefore, at the time of zero point return, Z setter, Q setter, or turret index, set the coordinate system simultaneously to correct to proper coordinate values.

7.1.1 Configuration of the Tool Nose Coordinate System

T ool Offset

Coordinate System of z-x Plane

Since the tool nose coordinate system is defined as the distance between the tool nose position and machining origin, the coordinate values are obtained by the following expressions. X axis: Work shift amount (XO) + Machine coordinate (Xm) - Tool offset (X) (-External

work origin off set) (Xop)

Y axis: Work shift ainount (YO) + Machine coordinate (Ym) - Tool offset (Y) (- External

work origin offset) (Yop)

Z axis: Work shift amount (ZO) + Machine coordinate (Zm) - Tool offset (Z)-Work Length

[K] (- External work origin off set)(Zop)

7 - 1

C axis: Work shift amount (CO) + Machine coordinate (Cm) (- External work origin offset)

(Cop)

B axis: Work shift amount (BO) + Machine coordinate (Bm) (-External work origin off

set)(Bop)

(Note) The OP work origin offset indicates the stun of the “external work origin offset” and

the “thermal displacement work origin offset”, each of which is used optionally.

(1) Work shift amount (X0, Y0, Z0, ...)

Length between the machine origin and jaw end face. It can be input from [Machining Reference Point Shift] of the [Work Coordinate] screen. No input, however, can be made for x axis on this p age. It needs to be input on the parameter page.

(2) Work length (K)

Length between the chuck jaw end face and machining origin. It can be input from [Work Length] of the [Work Coordinate] screen. It can be also altered by executing G54 Z (W)___ ;.

(3) Machining origin

Reference point of the machining program

(4) Tool offset (X, Y, Z)

Tool offset amount. It can be altered in the [T ool] screen.

(5) Outer work origin offset (Xe, Ye, Ze, ......)

Those are offset amount that shift the whole work coordinate system. Input is possible from the [Outer Offset] in the [Work coordinate] screen. The specified amount of the outer work origin offset will not, however, become valid unless the coordinate system (T command, manual turret index and the like) is set. (The offset amount will not be reflected in the coordinate system.)

7.1.2 Setting of Tool Nose Coordinate System

If the tool is indexed to the cutting position by turret index operation, the coordinate values of the “tool nose position” will change. This is because setting of the coordinate system is done in order to correctly display the distance between the tool nose position and machining origin at any time. Setting of the coordinate system is done in the following cases: (1) When T is specified in the automatic (memory, MDI) mode. (2) When the tool rest is rotated by pressing the turret index switch in the manual (handle,

feed, return to the origin) mode. (3) When the work length is altered with G54 Z(W) __ ; in the automatic mode. (4) When the automatic mode is started from the reset state (OP = 0). But ouly when the

parameter No.1202, #3 = 1. (5) When manual return to the origin is performed.

But only the initial return to the origin as for the straight lire axis. (6) When measurement is made with Q setter or Z setter.

7 - 2

(7) When an offset value for the tool at a cutting position is altered through the screen

input in the manual mode. (8) When both the work shift and work length are altered in the manual mode.

Axes subject to setting coordinate systems for the above (1) through (8) will be as follows: (1) through (4): all the axes.

(5) through (8): control axes only

7.1.3 Cautions

(1) If G50 X___ Y___ Z___ ...... ; is executed and the coordinate system is changed, the

coordinate value displayed at [Tool Nose Position] will not coincide with the distance

from the machining origin to the tool nose position. (2) When the T command and coordinate system setting (G50) are specified in the same

block like G50 X___ Y___ Z___ T___ ;, the T command becomes effective and

G50 is ignored. (3) As described above, the T-command does not set the coordinate system for the rotary

axis. Therefore, even if a work shift amount for the rotary axis is altered using a G10

command or custom macro, the T-command cannot reflect it in the coordinate

system.

If this is the case, use “work coordinate system preset (G921)” which allows you to

set the work coordinate system independently for each axis with a program

command. (For G921, see Section 7.7.)

But, a coordinate system will not be set for a rotating axis (Parameter No. 1010, #0=1)

7.1.4 Associated Parameters

No.1209 Work length No.1233 Work shift amount (Work reference point shift amount)

7 - 3

7.2 Plane Designation (G17, G18, G19)

With a G17, G18, or G19 command, this function specifies the plane in which circular interpolation, cutter compensation, etc. are performed.

7.2.1 Command Format

G17 Xp___ Y p___ ; Xp- Yp plane G18 Zp___ Xp___ ; Zp-Xp plane G19 Y p___ Zp___ ; Y p-Zp plane G17 ; X-Y plane G18 ; Y-Z plane G19 ; Z-Y plane where; Xp: X axis or its parallel axis

Yp: Y axis or its parallel axis Zp: Z axis or its parallel axis

(Note) The

- β plane refers to the orthogonal coordinate system which assumes the α-

axis to be the axis of abscissas and the

7.2.2 Sample Program

G17 U0 H0 ; Selects the X-C plane.

G18 W0 D0 ; Selects the Z-B plane.

Enables the X-C plane.

-axis to be the axis of ordinates.

7.2.3 Cautions

(1) Set with the parameter to which one of the X, Y, and Z axes the additional axis is

parallel. (2) The reset state is the G18 mode. (3) Set properly the relations between the parameter No.1023 (programmed axis name of

each axis) and No.1024 (sets which axis of the basic coordinate system each axis is

to be).

Enables the Z-B plane.

7 - 4

(4) An alarm results when the plane is not determined in the block where G17, G18, or

G19 was specified.

(Example) G17 X___ Y___ D___ ;

When the B axis is parallel to the Y axis, it is uncertain whether the X-Y or

X-B plane is selected. (5) A move command is irrelevant to plane selection. (6) As an ordinary lathe does not have Y axis, nothing except G18 (Z-X) plane can be

selected. On the other hand, as a drilling axis in the drilling fixed cycle is set to the basic axes (X, Y, Z) other than those of the plane, neither X nor Z axis can be assigned as a drilling axis for G18 plane. In the above case, set a Y-axis set value (2) to an axis other than control axes of Parameter No.1024. A vertual Y-axis is set on the coordinate system, where selection of G17(X-Y)/G19(Y-Z) planes is enabled and drilling with the X or Z axis can be performed. (As it is the virtual Y axis on the coordinate system, command of Y axis, even if it is made, is ignored.

7.2.4 Associated Parameters

No.1023 Programmed axis name of each axis No.1024 Sets which axis of the basic coordinate system each axis will be.

7.2.5 Associated Alarms

No.106 A plane selection (G17-G19) command has an error.

7 - 5

7.3 Work Coordinate System Change (G50)

By specifying G50, you can create the work coordinate system in which a current position will be a specified one.

7.3.1 Command Format

G50 X___ Y___ Z___ ...... ;

7.3.2 Sample Program

N1 G00 X50. Z25. ; N2 G50 X150. Z50. ;

If the N2 block is executed, the work coordinate system will be set so that the current position will be X = 150.0, Z = 50.0.

7.3.3 Cautions

(1) G50 is effective only in the block where it is specified. (2) G50 can be specified by both absolute programming and incremental programming.

The axes for absolute programming assume specified coordinate values. For the axes for incremental programming, the coordinate system is shifted by a specified amount.

(3) If G50 is specified with tool nose radius compensation or cutter compensation applied,

the work coordinate system is set so that the position before compensation will be a specified one.

(4) The work coordinate system is validated with a G50 command as follows.

• Set the coordinate system with a T command. (However, the coordinate system of the rot ating axis makes no change.)

7 - 6

7.4 Work Length Modification (G54/G55)

Work length of the front (spindle)/rear (subspindle) sides are changed.

7.4.1 Command Format

G54 Z___ ; (Spindle side: Input of the absolute value of the work length)

W___ ; (Spindle side: Input of the incremental value of the work length)

G55 B___ ; (Subspindle side: Input of the absolute value of the work length)

D___ ; (Subspindle side: Input of the incremental value of the work length)

7.4.2 Notes

(1) Command data of G54 are set in Parameter No.1209.

A command value is written in a parameter in G54, whereas a command value is added to a parameter in W command.

(2) Command data of G55 are set in Parameter No.1210.

A command value is written in a parameter in B command, whereas a command

value is added to a parameter in D command. (3) Following G54/G55 command, the coordinate system is automatically set. (4) Work length is used in the calculation of the corner R coordinate system. (5) G55 command is useable only when the rear processing function has been provided.

As for the rear face coordinate system, see “19.1 Rear processing.”

7.4.3 Associated Parameters

No.1209 Work length 1 (Spindle side) No.1210 Work length 2 (Subspinle side)

7 - 7

7.5 Machine Coordinate System Selection (G53)

When a G53 command, the axes are positioned to the position of the machine coordinate system specified by the program.

7.5.1 Command Format

G53 X___ Y___ Z___ ...... ;

7.5.2 Sample Program

G53 X50. Z50. ;

7.5.3 Cautions

(1) An alarm results if an incremental axis command is given. (2) Specify G53 after cancelling tool nose radius compensation/ cutter compensation. (3) The G53 command is effective only in the block where it is specified.

7.5.4 Associated Parameters

7.5.5 Associated Alarms

No.146 An incremental axis command has been given for machine Coordinate

System Selection (G53.)

7 - 8

7.6 Setting the Local Coordinate System (G59)

You can set another coordinate system (local coordinate system) in the work coordinate system by specifying the G59 command.

7.6.1 Command Format

G59 X___ Y___ Z___ ...... ;

X, Y, Z: Offsets of local coordinate system(position of origin of local coordinate system

taking the origin of the work coordinate system as the reference)

7.6.2 Program Example

N1 G00 X150. Z50. ; N2 G59 X100. Z25. ;

If you execute the N2 block, the local coordinate system will be set with the values X = 100 and Z = 25 of the work coordinate system as the origin.

7.6.3 Precautions

(1) G59 is effective only for the specified block. (2) There is no differentiation in absolute commands/incremental commands for

G59.G59X10.; and G59U10.; are the same. (3) The local coordinate system will be canceled only for the command axis in case of the

following:

• When an offset of 0 is specified in G59

• When coordinate system is set in G50.

(4) The local coordinate system of all the axes will be canceled in case of the following:

• Reset

• Coordinate system is set in the T command.

7 - 9

7.7 Work Coordinate System Preset (G921)

A G921 command can be used to preset the work coordinate system independently for each axis (setting of the tool nose coordinate system). It is valid for coordinate system setting of the rotary axis (parameter No.1010, #0 = 1) for which the coordinate system cannot be set with a T-command.

7.7.1 Command Format

G921 X___ Y___ Z___ C___ ...... ; S pecification of the axis for which you want to preset

the coordinate system.

7.7.2 Sample Program (C-axis = Rotary Axis)

N1 G28 H0 ;.................. Returns the C axis to the zero point.

N2 G50 C0 ;.................. Sets the C-axis zero point to C0.

N3 G10 P0 C___ ; .......Alters a C-axis work shift amount.

N4 G921 C0 ;................ Presets the C-axis work coordinate system.

7.7.3 Cautions

(1) G921 simply specifies the axis for which you want to preset the coordinate system,

and its value has no meaning; X0 and X1.0 have the same meaning.

Also, absolute programming and incremental programming do not make any

difference. (X1 = U1)

7 - 10

7.8 Lathe Turning Other than the G18 Plane (Z-X)

The command system and operations in the functions given below differ according to the selected plane (G17 to G19). [1] Circular arc interpolation [including helical interpolation] (G02, G03) *[2] Chamfering, corner R (I, J, K, R) [3] Arbitrary angle chamfering, corner R (,C/,R) *[4] Angle-specified straight line interpolation *[5] Automatic tip R compensation *[6] Groove width compensation (G150~G152) [7] T ool diameter compensation (G40~G42) *[8] Single fixed cycle (G90, G92, G94) *[9] Compound fixed cycle (G70~G76) [10] Drilling fixed cycle (G80~G89, G831, G841, G861) [1 1] Direct tap cycle (G842, G843)

(Note) Items marked with ‘*’ are functions that are unique to lathes.

Lathe turning is normally performed in the G18 plane (horizontal axis: Z axis, longitudinal axis: X axis). In this instructional manual also, functions unique to the lathe are described in the G18 plane, but to rend general purpose features to the NC unit, each function can be executed in other planes (G17, G19) also. Within the NC unit, the axis commands in the selected plane are regarded as horizontal axis (longitudinal direction) commands and longitudinal axis (diameter direction) commands of the plane, and all the commands are executed. Therefore, commands in other planes are generally executed as described below.

“Axis command” Replaces the X axis and Z axis in the G18 plane by longitudinal axis,

horizontal axis of the selected plane.

“I, J, K” Specifies the X axis direction as I, Y axis direction as J, and Z axis direction

as K.

7 - 11

From the axis configuration of the machine, the Z axis becomes the longitudinal direction, the X axis becomes the diameter direction, and if the Y axis exists then the Y axis also becomes the diameter direction.

No lathe turning is assumed in the G17 plane but if it is convenient to perform turning in the Y axis instead of the X axis, then lathe turning in the G19 plane becomes necessary . However, for the G19 plane, the longitudinal direction becomes the Y axis, and the diameter direction becomes the Z axis, therefore, the G19 plane cannot be used for functions that issue the command recognizing the longitudinal direction and the diameter direction ([6], [8], and [9] mentioned above).

Therefore, the longitudinal direction and the diameter direction for the G19 plane are regarded as Z axis and Y axis respectively, and the functions of [6], [8] and [9] are executed. (Take care because these functions will be executed as they are in the G17 plane.)

(Note) Set the virtual tip point (control point) of the tool according to the axis configuration

of the standard plane. (See figure below.) Automatic tip R compensation will be performed on this plane.

< G19: When the horizontal axis is taken as the Z axis >

7 - 12

Explanations about the “groove width compensation,” “single fixed cycle,” “compound fixed cycle” are given below. For det ailed explanations, refer to the respective items in the G18 plane.

(1) Groove width compensation (G150 - G152)

[Groove width compensation in the Y-Z plane]

G150 : Cancel groove width compensation G151 : Groove width compensation for end face / rear end face (Y coordinate system

shift)

G152 : Groove width compensation for outer diameter /inner diameter (Z coordinate

system shift) The virtual tip point will be changed as shown below.

(2) Single fixed cycle (G90, G92, G94)

Explanations about the fixed cycle of G90 are given here but these are similar for other fixed cycles also (G92, G94).

[Single fixed cycle in the Y-Z plane (G90)]

G90 Y___ Z___ J___ F___ ; (Note the J notation carefully)

R : Rapid traverse F : Cutting feed

(Note 1) Specify the position of C point by Y, Z. (Note 2) J is the incremental value (radius value) seeing point B with reference to

point C in the Y direction.

7 - 13

(3) Compound fixed cycle (G70 - G76)

Specify the X axis direction command “X, U, I” of the G18 plane by the Y axis direction command “Y, V, J” in the G19 plane. Explanations about the fixed cycle of G71 are given here, but these are similar to the explanations for other fixed cycles (G72 - G76).

[Compound fixed cycle (G71) in the Y-Z plane]

F : Cutting feed, R : Rapid traverse e : Escape amount (PRM6213)

G71 P(ns) Q(nf) V±__ W±__ J±__ K±__ D__ F__ S__ ;

N(ns) ------ ; Specify the finished shape of A - A’ - B in the block from sequence number (ns) to (nf). N(nf) ------ ;

P : First sequence number of the finished shape block (ns) Q : Last sequence number of the finished shape block (nf) V : Finished shape in the Y direction (∆v) W : Finished shape in the Z direction (∆w) J : Y direction allowance of the roughing cycle (∆J) K : Z direction allowance of the roughing cycle (∆k)

D : Cutting depth (∆d) ...... Specify without notation.

7 - 14

8. COORDINA TE

8.1 Diameter Designation and Radius Designation

The dimensions of each axis can be specified in two methods; using a diameter value or a radius value. The former is called diameter designation and the latter radius designation. Although which one is to be specified can be selected by the parameter DIAX (parameter No.1010; available for each axis), it has been predetermined for each machine. So, make setting suitable for the mechanical system. Normally , the NC lathe assumes diameter designation for the X axis, and radius designation for the other axes. As this may vary from one machine to another, refer to the instruction manual for each machine.

D1, D2 ...... Diameter designation

R1, R2 ...... Radius designation

When diameter designation is assumed for the X axis, pay attention to the conditions listed in the following table.

Itemrks Remarks

Non-X-axis command Regardless of the diameter/ radius (including the incremental command by the address V. W, D, or H)

X-axis command Specify with a diameter value. (including the incremental command by the address U)

Coordinate system setting (G50) Specify the X-axis coordinate value

with a diameter. X value of the tool position offset amount Specify with a diameter value. Parameters (D, I, K) for X-axis depth of Specify with a radius value.

cut, etc. used for the canned cycle (G90, G92, G94, G70-G76, etc.)

Radius for circular interpolation (R, I, K) Specify with a radius value. Chamfering, corner R amount (R, I, K) Specify with a radius value. Tool nose radius Specify with a radius value. Feed rate in the X-axis direction Radius change/rev .,

Radius change/min. Display of the X-axis position Display with a diameter value.

(Note 1) This manual is described assuming diameter designation for the X axis and

radius designation for the other axes, unless otherwise specified.

8 - 1

8.2 Absolute/Incremental Programming (G90, G91)

These G codes are available only when the G code system B or C is selected. You can select either absolute programming which gives the specified position of the coordinate system with a value following the axis address, or incremental programming which gives a stroke from a current position.

8.2.1 Command Format

G90 : Absolute programming G91 : Incremental programming

8.2.2 Sample Program

8.2.3 Cautions

(1) When the G code system A is selected, specify with an axis command address

instead of using G90/G91. (Refer to “1.1 G Code System”)

(2) The G90 and G91 commands are modal G codes. If one of them is specified, it

remains effective until the other one is specified.

(3) Set with the parameter whether the reset state is to be the G90 or G91 mode.

8.2.4 Associated Parameters

No.3402, #1= 0 The reset state is the G91 mode.

= 1 The reset state is the G90 mode.

8 - 2

8.3 Inch/mm Input (G20, G21)

With a G20 or G21 command, either inch or mm system can be selected as the increment system of program commands.

8.3.1 Command Format

G20 : Inch system G21 : mm system

8.3.2 The Following Systems of Units are Changed with the G20/G21 Command

(1) Feed rate command with an F code (2) Commands related to the position (3) Work origin shift amount (4) Tool offset amount (5) Part of parameters (6) Unit of one graduation of the manual pulse generator

8.3.3 Cautions

(1) S pecify G20/G21 command in an independent block after returning the control axis to

the machine origin. Note that, with changeover of inch input/mm input (change in G20/G21 command or the parameter), an axis not on the machine origin enters the origin returning incomplete state.

(2) When the G20/G21 command is executed, preset the work coordinate system.

8.3.4 Associated Parameters

No.1000, #2 = 0 The input increment system is mm.

= 1 The input increment system is inch.

No.1010, #0 = 0 Enables inch/mm switching for each axis (linear axis)

= 1 Disables inch/mm switching for each axis (rotary axis)

8 - 3

8 - 4

hitachi seiki 10L, 16T, 18T, 21L Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual