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

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

+ 314 hidden pages