hitachi seiki 10M, 16M, 18M Programming Manual

Download

SEIKI - SEICOS

å10M/16M/18M

INSTRUCTION MANUAL

6 PROGRAMMING

Edition 1.01 NP-0000-1-0221-E-1-01

Hitachi Seiki Deutschland Werkzeugmaschinen GmbH

CONTENTS

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

1-1 List of G Code Group(SEICOSΣ10M/16M/18M) ..........................................................1-1

1-2 List of G Codes (SEICOS Σ10M/16M/18M) ................................................................. 1-2

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

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

2-2 Linear Interpolation (G01) .......................................................................................... 2 - 2

2-3 Circular Interpolation (G02, G03) ............................................................................... 2 - 3

2-3-1 Radius Designation on Arc.................................................................................. 2 - 5

2-4 Helical Interpolation (G02, G03) ................................................................................. 2 - 7

2-5 Virtual Axis lnterpolation (G07) ................................................................................. 2 - 10

2-5-1 SIN Interpolation (G02, G03, G07) ..................................................................... 2 - 12

2-6 Single Direction positioning (G60) ........................................................................... 2 - 12

2-7 Involute Interpolation (G222, G223).......................................................................... 2 - 15

2-8 Cylindrical Interpolation (G271)................................................................................ 2 - 19

2-8-1 Command Format............................................................................................. 2 - 19

2-8-2 Feed Rate ......................................................................................................... 2 - 19

2-8-3 Cylindrical Interpolation Applied Axes................................................................. 2 - 20

2-8-4 Cylindrical Interpolation Applied Plane ............................................................... 2 - 20

2-8-5 Sample Program.............................................................................................. 2 - 20

2-8-6 Cautions............................................................................................................ 2 - 21

2-8-7 Associated Parameters .................................................................................... 2 - 22

2-8-8 Associated Alarms ............................................................................................ 2 - 22

2-9 Polar Coordinate Interpolation (G120, G121) ........................................................... 2 - 23

2-9-1 G Codes............................................................................................................ 2 - 23

2-9-2 Command Format............................................................................................. 2 - 23

2-9-3 Polar Coordinate Interpolation Axes .................................................................. 2 - 23

2-9-4 Polar Coordinate Interpolation plane.................................................................. 2 - 24

2-9-5 Program Command .......................................................................................... 2 - 24

2-9-6 sample Program (X-axis: Linear Axis, C-axis: Rotary Axis)............................... 2 - 25

2-9-7 Feed Rate Clamp.............................................................................................. 2 - 26

2-9-8 Rapid Traverse(G00) Operation........................................................................ 2 - 26

2-9-9 Precautions....................................................................................................... 2 - 26

2-9-10 Associated parameters ..................................................................................... 2 - 27

2-9-1 1 Associated Alarms ............................................................................................ 2 - 28

3. FEED FUNCTION.............................................................................. 3-1

3-1 Feed per Minute (G94)................................................................................................. 3-1

3-2 Feed per Rotary (G95)................................................................................................. 3-2

3-3 Inverse Time (G93) ...................................................................................................... 3-3

3-4 Exact Stop (G09) ......................................................................................................... 3-4

3-5 Exact Stop Mode (G61)................................................................................................ 3-4

3-6 Automatic Corner Override (G62)................................................................................ 3-5

3-6-1 Automatic Override in Inner Corner Area............................................................... 3-6

3-6-2 Inner Arc Cutting Speed Change ........................................................................... 3-7

3-7 T apping Mode (G63)..................................................................................................... 3-9

3-8 Cutting Mode (G64).................................................................................................... 3-10

3-9 Automatic Acceleration/Deceleration ......................................................................... 3-1 1

3-10 Dwell (G04)................................................................................................................ 3-11

4. REFERENCE POINT ........................................................................ 4-1

4-1 Automatic Reference Point Return (G28).................................................................... 4-1

4-2 Reference Point Return Check (G27).......................................................................... 4-2

4-3 Return from Reference Point (G29)............................................................................. 4-4

4-4 2nd-4th Reference Point Return (G30)........................................................................ 4-5

4-5 Reset of Floating Reference point (G301) ................................................................... 4-7

5. COORDINATE SYSTEM................................................................... 5-1

5-1 Machine Coordinate System Selection (G53).............................................................. 5-1

5-2 Work Coordinate system selection (G54 - G59).......................................................... 5-2

5-3 Addition of Work Coordinate system Pairs (G540 - G599) .......................................... 5-3

5-4 Local Coordinate System Setting (G52) ...................................................................... 5-5

5-5 Work Coordinate System Change (G92)..................................................................... 5-7

5-6 Work Coordinate System Preset (G921)..................................................................... 5-9

5-7 Work Coordinate System Shift (External Work Zero Point Offset Amount)............... 5-11

5-8 Plane Selection (G17, G18, G19) .............................................................................. 5-12

5-9 Rotary Table Dynamic Fixture Offset......................................................................... 5-14

6. COORDINATE................................................................................... 6-1

6-1 Absolute/Incremental Programming (G90,G91)........................................................... 6-1

6-2 Polar Coordinate Input (G15,G16) ............................................................................... 6-2

6-3 Inch/Metric Input (G20, G21) ........................................................................................ 6-5

7. SPINDLE FUNCTION (S FUNCTION) .............................................. 7-1

8. TOOL FUNCTION (T FUNCTION) .................................................... 8 - 1

9. Miscellaneous Function (M FUNCTION)............................................ 9- 1

9-1 Miscellaneous Function (M Function) .......................................................................... 9-1

9-2 2nd Miscellaneous Function (B Function).................................................................... 9-2

10 . Canned Cycle................................................................................... 10-1

10-1 Canned Cycle (G73, G74, G76, G80 - G89) .............................................................. 10-1

10-2 Direct Tap (G741, G841).......................................................................................... 10-16

10-3 Drilling Pattern Cycle (G70, G71, G72, G77) ........................................................... 10-22

10-4 True Circular Cutting (G302 ~ G305)....................................................................... 10-25

10-5 Square Outside Cutting (G322,323) ........................................................................ 10-34

10-6 Plane Cutting Cycle (G324, G325, G326)................................................................ 10-38

10-7 Poketing (G327 ~ G333) .......................................................................................... 10-50

10-7-1 Circular Poketing (G327)................................................................................... 10-55

10-7-2 Square Poketing (G328).................................................................................... 10-59

10-7-3 Track Inside (G329)........................................................................................... 10-64

10-7-4 Circle outside Pocketing (G330) ....................................................................... 10-67

10-7-5 Square Outside Cutting (G331)......................................................................... 10-70

10-7-6 Track Outside (G332)........................................................................................ 10-73

10-7-7 Circle (G333)..................................................................................................... 10-76

10-7-8 Special Fixed Cycles (G322 ~ G333) Type 2 .................................................... 10-78

10-8 A TC Canned Cycle (MO6)....................................................................................... 10-79

10-8-1 A TC Canned Cycle, Type A (VK, VKC, VG, VkII) ................................................ 10-82

10-8-2 A TC CANNED CYCLE TYPE E (VM40III).......................................................... 10-84

10-8-3 A TC CANNED CYCLE TYPE F (HG)................................................................ 10-86

10-8-4 A TC Canned Cycle, Type G (HK)...................................................................... 10-87

10-8-5 A TC Canned Cycle, Type I (Initial HS500) ......................................................... 10-89

10-8-6 A TC Canned Cycle, Type J (VS) ....................................................................... 10-91

10-8-7 A TC Canned Cycle, Type K(HS630) ................................................................. 10-93

10-8-8 A TC Canned Cycle, Type L (New HS500)......................................................... 10-95

10-8-9 A TC Canned Cycle, Type M (VS 16-tool) .......................................................... 10-96

10-8-10 A TC Canned Cycle, Type N (MS400H).............................................................. 10-98

10-9 High-Speed Machining Cycle ................................................................................... 10-99

10-9-1 Trochoid Cycle (G334) ...................................................................................... 10-99

10-9-2 Helical Drilling Cycle (G812, G813) ................................................................. 10-103

10-9-3 High Speed Side Face Cutting Cycle (G335) .................................................. 10-107

10-9-4 Z Feed Fluting Cycle (G336) ............................................................................10-111

10-9-5 Corner Pocket Cycle (G337)........................................................................... 10-113

10-9-6 Square Pocket Cycle (G338) .......................................................................... 10-116

11. COMPENSATION FUNCTION ........................................................ 11-1

11-1 Tool Length Compensation (G43, G44, G49)............................................................. 11-1

11-2 Tool Offset (G45 - G48) ............................................................................................. 11-6

11-3 Tool Diameter Compensation (G38 - G42) ................................................................ 11-9

11-3-1 Detailed Description of Tool Diameter Compensation ...................................... 11-15

11-4 3-D Tool Offset (G40 - G41)..................................................................................... 11-27

11-5 H and D Functions................................................................................................... 11-31

11-6 Tool Offset by Tool Number...................................................................................... 11-33

12. CONVERTING FUNCTION............................................................. 12-1

12-1 Programmable Mirror Image (G501, G51 1) ............................................................... 12-1

12-2 Setting Mirror Image................................................................................................... 12-4

12-3 Scaling (G50, G51) .................................................................................................... 12-7

12-4 Coordinate Ratation (G68, G69) .............................................................................. 12-10

12-5 Optional Angle Chamfering/Corner R (, C, R).......................................................... 12-15

13. MEASURMENT................................................................................ 13-1

13-1 Skip Function (G31)................................................................................................... 13-1

iii

13-2 Automatic Measurement of Tool Length (G37)........................................................... 13-3

13-3 Safety Guard (Tool Length) ........................................................................................ 13-5

13-4 Safety Guard (Comparison)....................................................................................... 13-9

14. DATA SETTING............................................................................... 14-1

14-1 Data Setting (G10)..................................................................................................... 14-1

14-1-1 Tool offset amount setting ................................................................................... 14-1

14-1-2 Work coordinate system offset amount setting................................................... 14-1

14-2 Programmable Parameter Input (G10) ...................................................................... 14-3

14-3 Plotting Parameter Setting......................................................................................... 14-5

15. SOFT OT ......................................................................................... 15-1

15-1 Soft OT (Stored Stroke Limit 1).................................................................................. 15-1

15-2 Stored Stroke Limits 2 and 3 (G22 and G23) ............................................................. 15-3

15-3 Soft-OT before Move ................................................................................................. 15-6

16. AXIS CONTROL.............................................................................. 16-1

16-1 Rotary Axis Controlling Function................................................................................ 16-1

16-2 Oscillation Function (G1 13, G114) ............................................................................. 16-4

16-3 Normal Direction Control (G41 1, G421, G401) .......................................................... 16-8

17 . HIGH-SPEED MACHINING............................................................. 17-1

17-1 Multibuffer (G251) ...................................................................................................... 17-1

17-2 Feed Rate Clamp by Circular Arc Radius.................................................................. 17-3

17-3 PRECONTROLLING ................................................................................................. 17-4

17-3-1 PRE-INTERPOLA TION LINEAR ACCELERA TION/DECELERATION ................ 17-5

17-3-2 AUTO CORNER DECELERATION .................................................................... 17-6

17-4 HIGH PRECISION PROFILE CONTROL .................................................................. 17-8

17-5 Smooth Interpolation................................................................................................ 17-10

17-6 NURBS Interpolation................................................................................................ 17-12

17-7 SHG Machining ........................................................................................................ 17-14

18. FIVE-FACE MACHINING ................................................................ 18-1

18-1 Selecting the Machining Plane (G240-G245) ............................................................. 18-1

18-2 Common Work Origin Offset..................................................................................... 18-2

18-3 Axis Changeover........................................................................................................ 18-5

18-3-1 Axis Changeover (T ype A)................................................................................... 18-5

18-3-2 Axis Changeover (T ype B)................................................................................... 18-6

19. AUTOMATIC OPERATION ............................................................. 19-1

19-1 Program Restart........................................................................................................ 19-1

19-2 Block Restart ............................................................................................................. 19-6

19-3 Machining Break Point Return (G206) ..................................................................... 19-11

19-4 Reverse Movement.................................................................................................. 19-14

19-5 Sequence Number Comparison and Stop ............................................................... 19-16

19-6 Reset (Reset Associated with Automatic Operation)............................................... 19-18

19-6-1 Details of Reset (Reset Associated with Automatic Operation) ........................ 19-18

20. MANUAL OPERATION .................................................................... 21-1

20-1 Manual Absolute ON/OFF .......................................................................................... 21-1

21 . TEST RUN ....................................................................................... 21-1

21-1 Miscellaneous Function Lock..................................................................................... 21-1

21-2 Miscellaneous Function Finish................................................................................... 21-1

22. CUSTOM MACROS ......................................................................... 22-1

22-1 Outline ....................................................................................................................... 22-1

22-2 Call Commands and Return Command.................................................................... 22-2

22-2-1 Types of Command ............................................................................................. 22-2

22-2-2 Multi-call .............................................................................................................. 22-8

22-2-3 Argument Designation....................................................................................... 22-13

22-3 Variables .................................................................................................................. 22-18

22-4 Representation of Variables..................................................................................... 22-31

22-5 Citation of Variables ................................................................................................. 22-31

22-6 Undefined V ariables ................................................................................................. 22-32

22-7 Expression and Computation .................................................................................. 22-33

22-8 Substitution Command ............................................................................................ 22-36

22-9 Branch Command ................................................................................................... 22-37

22-10Repeat Command ................................................................................................... 22-38

22-11 Naming Command.................................................................................................. 22-39

22-12IF Command............................................................................................................ 22-40

22-13External Output Commands .................................................................................... 22-42

23 . Interrupt Type Custom Macro .......................................................... 23-1

23-1 Custom Macro Interrupt Operation ............................................................................ 23-1

23-2 How to Specify........................................................................................................... 23-2

23-3 Interrupt T ype Custom Macro Proper......................................................................... 23-2

23-4 St atus Trigger Method and Edge T rigger Method (Parameters)................................. 23-2

23-5 Reversion and Modal Information .............................................................................. 23-3

23-6 System Variable in Interrupt Program ........................................................................ 23-3

23-7 Custom Macro Interrupt and Custom Macro Modal Call ............................................ 23-4

23-8 Interrupt Timing and Return Position in Each Mode................................................... 23-4

23-9 Associated Parameters ............................................................................................. 23-7

24. MEMORY OPERATION IN OTHER COMPANIES’ FORMATS ...... 24-1

24-1 Memory Operation in FS15 Format ........................................................................... 24-1

24-2 Memory Operation in i80M Format ............................................................................ 24-2

1. G CODE

1-1 List of G Code Group(SEICOS

Group Function Remarks

00 Non-modal 01 Positioning/liner interpolation/circular interpolation 02 Plane designation 03 Absolute programming/incremental programming 04 Stored stroke check 05 Inverse time/feed per minute/feed per revolution 06 Inch/metric conversion 07 Tool diameter compensation 08 Tool length compensation 09 Canned cycle 10 Initial point return/R point return 11 Scaling 12 Work coordinate system Selection 13 Cutting mode/exact stop mode/automatic corner override mode 14 Macro modal call 15 Programming mirror image 16 Coordinator rotation 17 Constant surface speed control *1 18 Tool life management 19 Normal direction control *1 20 Polar coordinate command 21 Oscillation function 22 Polar coordinate interpolation *1 23 Spindle speed fluctuation detection *1 24 Machining plane selection *1 25 Tool nose interference check *1 26 Axis switching/3-D coordinate conversion *1 27 *2 28 *2 29 *2 30 *2 31 *2

ΣΣ

Σ10M/16M/18M)

ΣΣ

(Note) *1 Reserved G code and not available for the moment

*2 Spare G code group for function improvement.

1 - 1

1-2 List of G Codes (SEICOS

ΣΣ

Σ10M/16M/18M)

ΣΣ

Code G00 G01 G02 G03 G04 G05 G07 G08 G09 G10 G1 1 G15 G16 G17 G18 G19 G20 G21 G22 G23 G25 G26 G27 G28 G29 G30 G31 G33 G34 G37 G38 G39 G40 G41 G42

Group

Function Remarks Positioning Linear interpolation Circular interpolation/helical interpolation CW Circular interpolation/helical interpolation CCW Dwell High-precision profile control Virtual axis interpolation Antecedent control Exact stop Data setting Data setting node cancel Polar coordinate command cancel Polar coordinate command XP YP plane where:XP : x axis or its parallel axis ZP XP plane YP : Y axis or its p arallel axis YP ZP plane ZP : Z axis or its parallel axis Inch input Metric input Store stroke check ON Stored stroke check OFF Spindle speed fluctuation detection OFF *1 Spindle speed fluctuation detection ON *1 Reference point return check Reference point return Return from reference point 2nd, 3rd, 4th reference point return Skip function Thread cutting *1 Variable lead thread cutting *1 Tool length automatic measurement Tool diameter compensation vector hold Tool diameter compensation corner arc Tool diameter compensation left/3-D tool offset cancel Tool diameter left/3-D tool offset Tool diameter compensation right

1 - 2

Code

G43 G44 G45 G46 G47 G48 G49 G50 G51 G52 G53 C54 G55 G56 G57 G58 G59 G60 G61 G62 G63 G64 G65 G66 G67 G68 G69 G70 G71 G72 G73 G74 G76 G77

Group

08 11

00 14

Function Remarks Tool length compensation + Tool length compensation Tool offset extension Tool offset contraction Tool offset double extension Tool offset double contraction Tool length compensation cancel Scaling cancel Scaling Local coordinate system Setting Machine coordinate system selection Work coordinate system 1 selection Work coordinate system 2 selection Work coordinate system 3 selection Work coordinate system 4 selection Work coordinate system 5 selection Work coordinate system 6 selection Single direction positioning Exact stop mode Automatic corner override mode Tapping mode Cutting mode Macro call Macro modal call Macro modal call cancel Coordinate rotation Coordinate rotation cancel Bolt hole cycle Arc Arc Peck drilling cycle Counter tapping cycle Fine boring cycle Grid cycle

Group 01 by parameter change

1 - 3

Code

G80 G81 G82 G83 G84 C85 G86 G87 G88 G89 G90 G91 G92 G93 G94 G95 G96 G97 G98

G99 G113 G114 G120 G121 G130 G131 G201 G203 G204 G206 G212 G213 G216

Group

03 00

Function Remarks Canned cycle cancel Drilling cycle, spot boring Drilling cycle, counter boring Peck drilling cycle Tapping cycle Boring cycle Boring cycle Back boring cycle Boring cycle Boring cycle Absolute programming Incremental programming

Work coordinate system change/maximun spindle speed setting

Inverse tine feed Feed per minute Feed per revolution Constant surface speed control *1 Constant surface speed control *1 Canned cycle initial level point return Canned cycle R point level return Oscillation node ON Oscillation node OFF polar coordinate interpolation mode cancel Polar coordinate interpolation mode Tool life management OFF Tool life management ON PMC data setting *1 High-speed machining program registration start *1 High-speed machining pro-gram registration end *1 Tool retract amount setting Circular thread cutting CW *1 Circular thread cutting CCW *1 Spline interpolation *1

1 - 4

Code G222 G223 G232 G233 G240 G241 G242 G243 G244 G245 G248 G249 G251 G264 G265 G271 G301 G302 G303 G304 G305 G311 G312 G313 G314 G322 G323 G324 G325 G326 G327 G328 G329 G330

Group

26 00 25

Function Remarks Involute interpolation CW Involute interpolation CCW Exponential function interpolation CW *1 Exponential function interpolation CCW *1 Machining plane 0 selection

(Machining plane selection cancel)

Machining plane 1 selection Machining plane 2 selection Machining plane 3 selection Machining plane 4 selection Machining plane 5 selection

(Available for an optional horizontal/vertical angle)

Axis switching/3-D coordinate conversion ON Axis switching/3-D coordinate conversion canel Multi-buffer Tool nose interference check ON *1 Tool nose interference check OFF *1 Cylindrical interpolation Floating reference point return Circular cutting inner diameter CW Circular cutting inner diameter CCW Circular cutting outer diameter CW Circular cutting outer diameter CCW Multi-step skip function 1 *1 Multi-step skip function 2 *1 Multi-step skip function 3 *1 Multi-step skip function 4 *1 Square outside cutting CW Square outside cutting CCW Square plane Square plane 1-directional Square plane 2-directional Circle inside (pocketing) Square inside (pocketing) Track inside (pocketing) circle outside (pocketing)

1 - 5

Code G331 G332 G333 G334 G335 G336 G337 G338 G401 G411 G421 C431 G501 G511

G540~

G599 G611 C653 G661 G721 G722 G741 G841 G812 G813 G921

Group

08 15

12 00

00 14

Function Remarks Square outside (pocketing) Track outside (pocketing) Circle (pocketing) Trochoid cycle High-speed side cutting cycle Z feed fluting cycle Corner pocket cycle Square pocket cycle Normal direction control cancel node Normal direction control left side ON Normal direction control right side ON Tool axis direction tool length compensation *1 Programmable mirror image Cancel Programmable mirror image Additional work coordinate system selection (60 pairs) Pre-interpolation acceleration/deceleration *1 Position check (Note) for Maintenance *1 Macro modal call B *1 Rotary copy *1 Parallel copy *1 Counter direct tap cycle Direct tap cycle Helical drilling cycle CW Helical drilling cycle CCW Work coordinate system preset

(Note 1) *1 Reserved G code and not available for the noment (Note 2) The G code marked in each group is selected in the reset state.

1 - 6

2. INTERPOLATION FUNCTION

2-1 Positioning (G00)

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

(1) command format

G90

 

G00 X_ Y_ Z_ ;

G91

 

(2) Sample program

(a) Absolute programming (b) Incremental programming

G90 G00 X100. Y50. : G91 G00 X100. Y50.

50.

End point

Start point

100.

Start point

100. End point

50.

(3) Cautions

(a) The rapid traverse rate has been set independently for each axis. (b) The tool path is non-linear. See to it that the tool does not interfere with the workpiece. (c) 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.

(d) G00, G90 are G91 ale modal G codes. Once they are specified, they remain effective

until the next associated G code is specified.

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

50.

Start point

End point

100.

(f) 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, # 6 = 0 Dry run made invalid for rapid traverse command.

1 Dry run made valid for rapid traverse command.

No.1401, # 1= 0 Non-linear interpolation as positioning interpolation system

1 Linear interpolation as positioning interpolation system

No.3402, # 0= 0 G00 mode in reset state

1 G01 mode in reset state

2-2 Linear Interpolation (G01)

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

(1) Command format

G90

{ }

G91

G01 X_ Y_ Z_...F_ ;

(2) Sample program

(a) Absolute programming. (b) Incremental programming G90 G01 X100. Y50. F200; G90 G01 X100. Y50. F200;

100. End point

50.

Start point

50.

End point

Start point

100.

(3) Cutting feed rate

The cutting feed rate specified with an F code is the speed at which the tool moves 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 G91 Xa Yb Zc Ff:

X-axis cutting feed rate: Fx = , where; L= a

Y-axis cutting feed rate: Fy =

z-axis cutting feed rate, Fz =

af L

bf L

cf L

+ b2 + c

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 - 2

G01 G91 X100. C90. F200 :

End Point

Cutting feed rate in the rotary axis (C axis) direction:

Start Point

Fc = (deg/min)

where; L = 100.

90. x 200 L

+ 90

(mm)

(4) Cautions

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

(5) Associated parameters

No.3402, #0 = 0 G00 mode in reset state

1 G01 mode in reset state

(6) Associated alarm

No. 102 F0 was specified in the G01/G02/G03 mode.

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.

(1) Command format

(a) X

plane

P YP

G02

 

G17 XP- YP- F_ ;

 

G03

(b) ZP -XP plane

G02

 

G18 ZP- YP- F_ ;

 

G03

G02

 

G19 YP-ZP- F_ ;

 

G03

Where; XP : X axis or its parallel axis

Y Z

(Note) To specify with R instead of I, J or K is called radius designation on arc.

   

I_ J_

   

K_ I_

   

J_ K_

: Y axis or its p arallel axis

: Z axis or its parallel axis

2 - 3

(2) Sample program

(a) Absolute programming (b) Incremental programming

G17 G90 G00 X13.397 Y70. F200: G17 C91 G02 X86.603 Y50 G02 X100. Y120. I86.603 J-50.: I86.603 J-50. F200:

120.

G02

Start point

186.603

End point

J=50

Center

100.

(3) Arc rotating direction

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

100.

G02

G03

G02

Start point

186.603

G03

G02

100.

End point

J=50

(4) Arc plane

The arc plane is specified with C17, G18 or G19.

G17 : X G18 : Z G19 : Y

-YP plane

-XP plane

-ZP plane

(5) Arc center

The arc center is specified with I, J or K corresponding to X

,YP and ZP respectively. In this

case, I, J and K are the vector components when viewing the arc center from its start point.

End Point

J I

Center point

Start Point

End Point

I K

Center point

Start Point

2 - 4

(6) Cutting feed rate

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

(7) Cautions

(a) An alarm results when no F code has been specified in the G02/G03 block or before. (b) An alarm results if an arc radius = 0 is specified. (c) I0, J0 and K0 are omissible. (d) 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 parameter set value.

End Point error

Start Point

End Point

Moves linearly

Center

(e) An alarm results if the axis not for the arc plane is specified. (f) When R is specified in the same block as I, J and K, R is given priority. (g) When the rotary axis is specified in the same block, circular interpolation is performed

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

(h) Exponential type acceleration/deceleration is applied.

(8) Associated parameters

No.3459 Arc end tolerance

(9) Associated alarm

No.102 F0 has been command with G01, G02 and G03. No.132 Arc interpolation error (#001) Center command, although available, is 0 in value. (#002) Difference in radius value between of start and end (#003) pints has exceeded parameter set value.

2-3-1 Radius Designation on Arc

In case of circular interpolation, an arc radius can be directly specified with R instead of specifying the arc center with I, J or K.

2 - 5

(1) Command format.

(a) X

P-YP

plane

G17 X

(b) Z

P-XP

G02

{ }

G03

plane

_ YP _ R ±_ F_ :

G02

G18 Z

P-ZP

{ }

G03

plane

_ YP _ R ±_ F_ :

G02

G19 Y

{ }

G03

where; X

P-ZP

: X axis or its parallel axis

: Y axis or its p arallel axis

: Z axis or its parallel axis

R+ : Arc of less than 180 R- : Arc of over 180°

(2) Sample program

(a) For the arc of less than 180°

G17 G91 G02 X100. Y100. R-100. F200:

_ R ±_ F_ :

(b) For the arc of over 180°

G17 G91 G02 X100. Y-100. R-100. F200 :

End Point

R100.

Start Point

Center

Less than 180°

Start Point

End Point

R100.

Center

(3) Cautions

(a) When I, J, K and R are specified in the same blocks, R is given priority. (b) When the arc center is not calculated, an alarm results.

G02

   

G03

(4) Associated parameters

More than 180°

2 - 6

(5) Associated alarms

No. 131 An arc radius R with which arc center position cannot be calculated has

been commanded.

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.

(1) Command format

G02

G17 X

G18 Z

G19 Y

where; X

   

G03 G02

   

G03 G02

   

G03

: X axis or its parallel axis

: Y axis or its p arallel axis

: Z axis or its parallel axis

α : Any optional linear axis for other than circulate interpolation (up to 2 axes)

F : Arc speed

Linear axis speed = F

R _

_ YP _ α_ F_ ;

_ ZP _ α_ F_ ;

   

I _ J _ R _

   

I _ J _ R _

   

I _ J _

Linear arc length

Arc length

2 - 7

(2) Sample program

G17 G91 G03 X-100. Y-100. R100. Z50. F200 :

End Point

Start Point

(3) The axes for other than circular interpolation can be specified up to 2 axes in the same

block. (Example) G17 G91 G03 I-100. Z100. V50. F200 :

I-100. Z100.V50.;

Tool Path

The V axis must be parallel with the Y axis.

(4) Cautions

(a) See to it that the linear axis speed does not exceed the maximum value. (b) Tool diameter compensation is applied to circular interpolation. (c) An alarm results if 3 or more linear axes are specified.

2 - 8

(5) Associated parameters

(6) Associated alarms

2 - 9

2-5 Virtual Axis lnterpolation (G07)

If the axis is specified as a virtual axis, it does not move. Interpolation can be perfomed with this axis and other one.

(1) Command format

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

G07 : The

: in this section. G07

α 1 ; Cancels the a axis as the virtual axis.

where ;

(2) Sample program

G07 X0 ; Sets the X axis as the virtual axis. G17 G91 G02 X0 Y0 I50. Z-1. 0 F200 ; SIN interpolation G01 X5. F100; Dwell state for the move time of the X axis G07 X1 ; Cancels the X axis as the virtual aixs.

(3) Cautions

(a) SIN interpolation results if one arc axis for helical interpolation is set as the virtual axis. (b) The virtual axis is any one axis.

An alarm results if 2 or more axes are set as virtual axes.

time valve is placed in the dwell state.

(d) Program virtual axis interpolation in the incremental manner.

Since the virtual axis does not move at any time, it is necessary to be careful when programming in the absolute manner.

α : Any one axis

α axis is the virtual axis

}

2 - 10

(4) Associated parameters

(5) Associated alarms

No.139 Two or more virtual axes have been specified.

2 - 11

2-5-1 SIN Interpolation (G02, G03, G07)

SIN interpolation can be performed by assuming one of axes for an arc command as a virtual axis in helical interpolation.

(1) Command format

G87 α0 ; Sets the virtual axis.

specify helical interpolation.

G07

α1 ; Cancels the virtual axis.

α is any one axis for the arc command.

(2) Sample program

G07 X0; G17 G91 G03 X0 Y0 I-50. Z100. F200 ; G07 X1;

(3) Cautions

(a) Effective only for automatic operation of the virtual axis. (b) Program the virtual axis in the incremental manner. (c) An alarm results if 2 or more virtual axes are specified.

2-6 Single Direction positioning (G60)

Performs final positioning always from a specified single direction. Using this function allows you to perform high-accuracy positioning.

(1) Command format

(a) For the one-shot G code

G60 X_Y_Z_... ; Effective only in the G60 specified block

2 - 12

(b) For the modal G code

G60 X_ Y_ Z_... ; X_ Y_ Z_...;

Single direction positioning

G00 ;

Cancels G60 if any G code in Group 01 other than G60 is given.

(2) Sample program

(a) When moving in the (b) When moving in the

+ direction - direction G60 G91 X100.; G60 G91 X-100.;

Start Point

End Point

Approach Amount

End Point

Approach Amount

Start Point

(3) Final positioning direction

Approach amount > 0 : The positioning direction is the + direction. Approach amount < 0 : The positioning direction is the - direction. Approach amount = 0 : Positioning is not performed in the - direction.

(4) Cautions

(a) Whether G610 is to be one-shot or modal is set with the parameter. (b) In the canned cycle, hole positioning is performed with G60.

However, single positioning is disabled for the shift amount of G76 and G87.

positioning.

(5) Associated parameters

2 - 13

(5) Associated parameters

No. 3458 Single positioning direction and approach amount of each axis No. 3400, #2 = 0 G60 is the G code of Group 00 (one-shot).

1 G60 is the G code of Group 01 (modal).

2 - 14

2-7 Involute Interpolation (G222, G223)

This function allows machining along an involute curve. It also provides cutter compensation. (1) Involute curve

The involute curve in the X-Y plane is defined as following.

θ) =R [cosθ + (θ- θ0) sinθ ] +X0

θ) =R [sinθ + (θ- θ0) cosθ ] +Y0

where;

X0, Y0:Central coordinate of the basic circle R : Radius of the basic circle

θ 0 : Angle of the point where the involute curve starts θ : Angle of the contact of the tangent from the current position to the basic circle

θ ), Y(θ ) :Current position of the X-and Y-axis

Start Point

involute Carve

(X, Y)

(X0, Y0)

Basic Circle

The involute curves in the Z-X and Y-Z planes are defined in the same manner as that in the XY plane.

θ 0

End Point

2 - 15

(2) Command format

(a) X

_ plane

P -YP

G222

 

G17 XP _YP _ I_ J_ R_ F_ ;

 

G223

(b) ZP-XP Plane

G222

 

G18 ZP _ YP_ K_ J_ R_ F_;

 

G223

G222

 

G19 YP_ ZP J_ K_ R_ F_ ;

 

G223

where;

G222 : Clockwise involute interpolation G223 : Counterclockwise involute interpolation X

, YP, ZP: Coordinate value of the end point

: X-axis or its parallel axis : Y-axis or its parallel axis : Z-axis or its parallel axis

I, J, K : Central position of the basic circle for the involute curve viewed from the

R : Radius of the basic circle F : Cutting feed rate

start point

(3) Start point and end point

The end point of the involute curve is specified with the address X, Y, or Z and expressed with an absolute or incremental value depending on G90 or G91. If the incremental value is used, specify the coordinate of the end point viewed from the start point of the involute curve. When a start or end point command is within the basic circle, an alarm results. The same results when an offset vector is brought into the basic circle by cutter compensation. Care should be taken when an offset is applied, in particular, to the inside of the involute curve.

(4) Basic circle command

The center of the basic circle is specified with I, J, and K, corresponding to X, Y, and Z, respectively. However, the numerals following I, J, and K are vector components, when the center of the basic center is viewed from the start point of the involute curve. They should be always programmed with incremental values, regardless of G90 or G91. Add a sign to I, J, and K as required.

2 - 16

(5) Feed rate

A feed rate for involute interpolation assumes a cutting feed rate specified with an F-code, and a speed along the involute curve (speed in the tangent direction of the involute curve) is controlled to be specified feed rate.

(6) Cutter compensation

Cutter compensation can be applied to the involute curve for perform machining. Cutter compensation is specified with G40, G41, or G42, like straight line or circular arc.

G40 : Cancels cutter compensation G41 : Offsets to the left of the tool advance direction

G42 : Offsets to the right of the tool advance direction Cutter compensation for the involute curve is achieved as follows. First, obtain a circular arc close to the curvature of the involute curve near the start point of the involute curve. Similarly, obtain the an intersecting point at offset time near the end point, and assume the involute curve passing those two points to be a tool center path.

You cannot specify cutter compensation start-up or cancel during the involute interpolation mode.

(7) End point error

When the end point is not located on involute curve passing the start point, the belowmentioned curve is assumed. An alarm will result if a shift amount between the involute curve passing the start point and that passing the end point is greater than a value set in a parameter. When there is an end point error, a feed rate cannot be assured.

End Point

Corrected Path

Start Point

True Involate Curve

2 - 17

(8) Modes available for involute interpolation

Involute interpolation is allowed even during the following G-code modes.

G41 : Cutter compensation to the left G42 : Cutter compensation to the right G511 : Programmable mirror image G68 : Coordinate rotation

(9) Limitations

(a) Rpm of the involute curve

Both start point and end point must be within 100 revolutions from an involute curve start point. The involute curve revolving one or more time can be also specified in one block.

(b) Unspecifiable function

Optional angle chamfering corner R cannot be specified during the involute interpolation mode. Helical interpolation and axis scaling are disallowed.

G411: Normal direction control to the left G412: Normal direction control to the right G121: Polar coordinate interpolation G16 : Polar coordinate command

(10) Associated parameters

No. 3465 Initial angle error limit value for involute interpolation

(1 1) Associated alarms

No. F242 A command value has an error.

1 The start or end point has been specified within the basic circle. 2 I, J, K, or R has been specified with 0. 3 The start or end point is beyond 100 revolutions from the involute curve

start point.

No. F243 The end point is not on the involute curve.

2 - 18

2-8 Cylindrical Interpolation (G271)

If the move amount of the linear axis and the angle of the rotary axis are given by a program command, the move amount of the rotary axis given in terms of angle will be internally converted into a distance on the circumference. Since the distance on the circumference can be considered the move amount of the linear axis on the circumference, linear or circular interpolation can be performed with other linear axis. After interpolation, it will be put back into the angle of the rotary axis again.

2-8-1 Command Format

G271 A Cylinder radius ; Cylindrical interpolation ON

: Cylindrical interpolation mode

G271 A0 ; Cylindrical interpolation cancel The A-axis is a rotary axis. The rotating angle of the rotary axis is calculated back from the move amount on the circumference. For example; when you want to move by 100.0 on the circumference of the cylinder whose radius is 50.0, obtain the rotating angle of the rotary axis from the following formula: r : Cylinder radius

θ : Rotating angle

s: Move amount on the cylinder

circumference

Rotating angle

2-8-2 Feed Rate

During the cylindrical interpolation mode, a feed rate command F is the speed at which the tool moves on the outer circumference of the cylinder.

θ=

360 x S (Move amount on circumference)

π x r (Cylinder radius)

360 x 10.00

= = 114.591

π x 50.0

Work

2 - 19

2-8-3 Cylindrical Interpolation Applied Axes

set in the parameters(no. 3426 for the linear axis, and no. 3427 for the rotary axis) the linear axis and rotary axis to which you want to apply cylindrical interpolation. A setting range for both parameters is 1 to the number of controlled axes; they must not have the same value.

2-8-4 Cylindrical Interpolation Applied Plane

During the cylindrical interpolation mode, the plane is automatically selected, which assumes the rotary axis to be the plane first axis, and the linear axis td be the plane second axis.

2-8-5 Sample Program

(Select the A-Y plane with the parameters 3426 and 3427) G40 G80 ,. G00 X-1204.0 Y0 A0 ,. G01 Z100.0 F100

G271 A50.0 ; Cylindrical interpolation mode ON N1 G42 G01 X-40.0 F500 ; (Cylinder radius = 50.0) N2 A90.0 F500 ; N3 X-100.0 A180.0 N4 A260.0 ; In Cylindrical interpolation mode N5 G03 X-80.0 A282.918 R20.0 ; N6 G01 X-60.0 ; N7 G02 X-40.0 A305.836 R20.0 ; N8 G01 A360.0 ; N9 G40 G01X-120.0 ;

G271 AO ; Cylindrical interpolation mode OFF G00 Z120.0 A0 ;

Developed View of Cylindrical Surface with Cylinder Radius = 50.0

A C (Rotary Axis)

Programmed Path

X (Linear

Axis)

Tool Center Path

246.892

282.918

Coordinate Value on Cylinder Surface

Specified Angle

R: (Cylinder Radius)

2 - 20

2-8-6 Cautions

(1) When specifying cutter compensation, start up/cancel during the cylindrical interpolation

mode.

(2) The plane (selected by G17 to G19) existing prior to entering the cylindrical interpolation

mode is canceled once during the cylindrical interpolation mode and revived at the end of the cylindrical interpolation mode.

(3) When performing circular interpolation during the cylindrical interpolation mode, the method

to specify the circular arc radius (which ones of I, J, and K addresses are to be used) is determined as follows, depending on the axis of the basic coordinate system to which the 2nd axis (linear axis) of the cylindrical interpolation plane corresponds (setting of the parameter no. 1011).

• When the linear axis is the X-axis or its parallel axis, specify with K and I, considering it the Z

p-Xp

plane.

• When the linear axis is the Y-axis or its parallel axis, specify with I and J, considering it the Xp-Yp plme.

• When the linear axis is the Z-axis or its parallel axis, specify with J and K, considering it the Yp-Zp plane.

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

(4) Specify a G271 command (G271 Axx; ) independently in a block.

If there is no axis command (G271;) after the G271 command, an alarm will result.

(5) If the axis not set in the parameter no. 3427 is specified with the G271 command, an alarm

will result.

(6) The follwing functions are not available:

• Return to the machining break point

• Manual intervention by manual absolute ON

(7) If the follwing comands are given during the cylindrical interpolation mode, an alarm will

result:

• G17, G18, G19 ------------------------ Plane designation

• G28, G30, G53 ------------------------ Machine coordinate system

• G54-59, G540-G599, G92, G52 --- Work coordinate system

• G73, G74, G76, G81-G89 ---------- Canned cycle

• G302-G305, G322-G333 ----------- Special canned cycle

• G00 (when including the cylindrical interpolation applied rotary axis)

2 - 21

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

distance on the circumference and converted back into the angle after interpolation. When this is done, a slight conversion error results.

(9) If circular interpolation with small circular arc radius is executed during the cylindrical

interpolation mode, a circular interpolation alarm may be caused by the above-mentioned conversion error. Care should be taken when using it. Even at the time of cutter compensation, a cutter compensation alarm may result due to the above-mentioned reason.

(10)If cylindrical interpolation mode ON (G271 Axx; (A

≠ 0) ) is specified again during the

cylindrical interpolation mode an alarm will result.

(11) The residual move amount indicates the value when moving on the outer circumference of

the cylinder.

2-8-7 Associated Parameters

No. 3426 Number of the linear axes(1 to number of controlled axes) to which

cylindrical interpolation is to be applied

No. 3427 Number of the linear axes(1 to number of controlled axes) to which

cylindrical interpolation is to be applied

2-8-8 Associated Alarms

No. 126 A cylindrical interpolation command has an error.

(#001) There is no rotary axis command. (#002) This is not an independent command. (#003) The modal G-code is not correct.

No. 127 A wrong command was given during the cylindrical interpolation

mode. (#001) A wrong G-code was given. (#003) A rotary axis move command was given in the G00 mode. (#004) Cylindrical interpolation was specified again during the cylindrical

interpolation mode.

No. 189 (G271) The parameter has not been set properly.

• The parameter no. 3426 or no. 3427 is not "1" to the number of controlled axes, or they have the same value.

• The linear axis set in the parameter no. 3426 is none of the three basic axes, X, Y, and Z, or not parallelto awy.

2 - 22

2-9 Polar Coordinate Interpolation (G120, G121)

polar coordinate interpolation is a function to provide contour control by converting a command programmed in the orthogonal coordinate system into a linear axis move(tool move) and rotary axis move(work rotation).

(X1,C1)

The following shows the relations between (X

, C1 ) and. (X1 ' , C1 ' ).

2-9-1 G Codes

G 121 : Polar coordinate interpolation mode G 120 : Cancel polar coordinate interpolation mode

2-9-2 Command Format

G121 ; Polar coordinate interpolation mode ON

: : Polar coordinate interpolation mode ON :

G120 ; Cancels polar coordinate interpolation mode

(X1’,C1’)

X’

’

X’

2-9-3 Polar Coordinate Interpolation Axes

The linear axis and rotary axis to which you want to apply polar coordinate interpolation should be set in the parameters (no. 3418 for the linear axis and no. 3419 for the rotary axis) in advance. For both parameters, set within a range of 1 to the number of controlled axes, and they must not be of identical value.

2 - 23

2-9-4 Polar Coordinate Interpolation plane

A G121 command effectuates the polar coordinate interpolation mode, assumes the zero pint of the work coordinate system to be that of the coordinate system, and selects the plane(polar coordinate interpolation plane) which assumes the linear axis to the first axis of the plane and a virtual axis(rotary axis) orthogonal to the linear axis to be the second axis of the plane. Polar coordinate interpolation is performed on this plane. Since polar coordinate interpolation is initiated, assuming the G121 specified position's angle to be zero (0), regardless of an actual position, prepare a program, assuming the work coordinate value of the rotary axis to be zero (0) when G121 is specified..

2-9-5 Program Command

(1) In the polar coordinate interpolation mode, specify a program command in terms of

orthogonal coordinate value in the polar coordinate interpolation plane. Use the axial address of the rotary axis as a command address for the second axis of the plane. The unit for the command is not degrees; specify in the same unit (rpm or in.) as the linear axis, the first axis of the plane.

(2) The polar coordinate interpolation mode allows you to specify linear interpolation (G01)

and circular interpolation (G02, G03). Both absolute programming and incremental programming are allowed.

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

circular arc radius specifying method (whether I, J, or K should be used) is determined as follow, depending on which axis in the basic coordinate system the first axis (linear axis) of the plane corresponds to(parameter setting: no. 1011).

• When the linear axis is either X-axis or its parallel axis, I and J are used, assuming the X

-YP plane.

• When the linear axis is either Y-axis or its parallel axis, J and K are used, assuming the Y

-ZP plane.

• When the linear axis is either Z-axis or its parallel axis, K and I are used, assuming the Z

-XP plane.

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 on the profile after cutter compensation. However, specify G121 and G120 in the cutter compensation cancellation mode (G40).

2 - 24

(5) For an feed rate, use F-code to specify a tool move rate in the polar coordinate

interpolation plane( orthogonal coordinate system ). Normally, it is specified in feed per minute (G94); the unit for the F-code will be mm/min. or in./min.

2-9-6 sample Program (X-axis: Linear Axis, C-axis: Rotary Axis)

N1 G00 X50.0 C0 ; N2 G121 ; N3 G42 G01 X30.0 F100 ; N4 C20.0 ; N5 G03 X20.0 C30.0 R10.0 ; N6 G01 X-30.0 N7 C-20.0 ; N8 G03 X-20.0 C-30.0

I0.0 J0; N9 G01 X30.0; N10 C0 ; N11 G40 X50.0 ; N12 G120 ;

Positions to the start position Starts polar coordinate interpolation

Profile program(program based on the orthogonal coordinate value In the X-C' plane)

Cancels polar coordinate interpolation

Rotaray Axis

Tool

Linear Axis

2 - 25

2-9-7 Feed Rate Clamp

The maximum cutting feed rate at polar coordinate interplation can be set in a parameter (no;

3464). If any feed rate higher than this one is specified during polar coordinate interpolation, it will be clamped to this rate. If a set value is 0, it will be clamped by the normal maximum cutting feed rate (parameter no. 1422) even during polar coordinate interpolation. As polar coordinate interpolation converts the profile programmed in the orthogonal coordinate system into the movements of the linear axis and rotary axis, a move near the work center (coordinate zero pint) may increase the speed of the rotary axis and exceed the limit speed of the machine. If this is the case, the allowable speed of the rotary axis can be set with the parameters as follows. Rotary axis allowable speed = Maximum cutting feed rate (parameter no. 3464) x Allowable ratio(parameter no. 3420) If the speed component of the rotary axis during polar coordinate interpolation exceeds the allowable speed, an override calculated by the formula below will be automatically applied. (Automatic override )

Override = x 100 (%)

If the speed component of the rotary axis stills exceeds the allowable speed even after a override has been applied, the feed rate will be clamped in such a manner that the speed component of the rotary axis will not exceed the maximum cutting feed rate. (Automatic speed clamp)

2-9-8 Rapid Traverse(G00) Operation

A G00 command can be executed during the polar coordinate interpolation mode. to the G00 block, however, only the end point is converted into a position in the polar coordinate system; a path remains unconverted.

(Example)"AG00 X100.0 C50.0;" in the G121 mode assumes the same path as "G01 X141.421

With G00, the rotary axis takes a short-cut. (move within +/-l80

2-9-9 Precautions

(1) Specify G120 and G121 in an independent block, respectively.

Allowable speed of the rotary axis Speed component of the rotary axis

C45.0;" in the G120 mode.

° ) to reduce the machining time.

(2) Prior to specifying G121, the work coordinate system must have been set, where the

center of the rotary axis can be the zero point of the coordinate system.

2 - 26

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

specifying G121 and restored by specifying G120.

(4) The following lists the G-codes which cam be specified during the G121 mode.

G00, G01, G02, G03, G04, G09, G40, G41, G42, G65, G66, G67, G98, G99

(5) Any axis outside the plane in the G121 mode moves independent of polar coordinate

interpolation.

(6) A display of "MOVE AMT." during the G121 mode refers to a remaining move amount in the

polar coordinate plane (orthogonal coordinates). However, the G00 block assumes the same unit as usual.

(7) The following functions are not available for the block in the G121 mode. Program restart,

Return to machining break point, Manual intervention by manual absolute ON

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

rotary axis can be rounded to 360

° through parameter setting. (0° 360°)

(9) When the work coordinate value of the linear Axis is negative at G121 command. To the

first move block, only the end point is converted into a position in the polar coordinate system; a path remains unconverted. (Same as linear G00 in the G121 mode) Starting from the next move block, polar coordinate conversion is applied to the move path. Only G00 and G01 can be specified in the first move block; G02 and G03 cannot be.

2-9-10 Associated parameters

No. 3410, #1 = 0 Does not Perform automatic override and automatic speed clamp

during the polar coordinate interpolation mode.

= 1 Performs automatic override and automatic speed clamp during the

polar coordinate interpolation mode.

No. 3418 Axis number of the linear axis to which you want to apply polar

coordinate interpolation

No. 3419 Axis number of the rotary axis to which you want to apply polar

coordinate interpolation

No. 3420 Automatic override allowable ratio during the polar coordinate

interpolation mode

No. 3464 Maximum cutting feed rate during the polar coordinate interpolation

mode.

2 - 27

2-9-11 Associated Alarms

No. 113 A polar coordinate interpolation command has an error.

(#001) G120 or G121 has not been independently specified. (#002) When G120 or G121 was specified, cutter compensation had not been

cancelled.

(#003) When the work coordinate value of the linear axis was negative at G121, a

G-code other than G00 and G01 was specified in the first move block.

No. 114 A wrong Command was specified during the polar coordinate interpolation

mode.

(#001) An unavailable G-code was specified.

No. 189 (G121) Parameter Setting is erroneous.

• The setting of the parameters nos. 3418 and 3419 is not within a range of 1 to the number of controlled axes, or the setting of the parameter no. 3418 is equal to that of no. 3419.

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

2 - 28

3. FEED FUNCTION

3-1 Feed per Minute (G94)

Until G95 is specified after G94 was specified, the stroke per minute (mm/min., inch/min.) is directly specified with a numerical value following F.

Feed rate F is the stroke per minute Metric system : mm/min Inch system : inch/nin.

(1) Command format

G94 ;

(2) Sample program

F100 ; The feed rate is a move of 100 mm per minute.

(3) The F code programmable range is as follows.

(a) Metric system

F60 : 1 ~ 999999 (mm/min.) F61 : 0.1~999999.9 (mm/min.)

(b) Inch system

F51 : 0.I ~ 99999.9 (inch/min.) F52 : 0.01 ~ 99999.99(inch/min.)

(5) Cautions

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

increment of 1 mm/min. or 0.1 m/min. is selected by parameter setting.

minute.

(6) Associated parameters

No. 3400, #1= 0 The least input increment for F61 in the metric system without a

decimal point is 1 mm/min.

1 The least input increment for F61 of the metric system without a

decimal point is 0.1 mm/min.

3 - 1

No. 3401, #2= 0 F51 for feed per minute in the inch system (inch/min. )

1 F52 for feed per minute in the inch system (inch/min. )

No. 3401, #3= 0 F60 for feed per minute in the metric system (mm/min. )

1 F61 for feed per minute in the metric system (mm/min. )

(7) Associated alarms

3-2 Feed per Rotary (G95)

Until G94 is specified after G95 was specified, the stroke per spindle revolution (mm/rev. inch/ rev.) is directly specified with a numerical value following F.

Feed rate F is the stroke per spindle revolution Metric system : mm/rev. Inch system : inch/rev.

(1) Command format

G95 ;

(2) Sample program

F1, 2 ; The feed rate is 1.2 mm per revolution.

(3) The F code programmable range is as follows.

(a) Metric system

F32 : 0.01 ~999.99 (mm/rev.) F33 : 0.001 ~ 999.999(mm/rev.)

(b) Inch system

F23 : 0.001 ~ 99.999 (inch/rev.) F24 : 0.0001 ~ 99.9999 (inch/rev.)

(4) Cautions

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

3 - 2

(5) Associated parameters

No. 3401, #0= 0 F23 for feed per revolution in the inch system (inch/rev.)

1 F24 for feed per revolution in the inch system (inch/rev.)

No. 3401, #1= 0 F32 for feed per revolution in the metric system (mm/rev.)

1 F33 for feed per revolution in the metric system (mm/rev.)

3-3 Inverse Time (G93)

when G93 is instructed, the program is put in the INVERSE TIME mode until G94 and G95 are instructed. Inverse time (FRM) is instructed directly with a value following F.

(1) Command format:

G93 ;

(2) Inverse time (FRN)

(a) For linear interpolation (G01)

FRN = (1/min)

(b) For circular interpolation (G02, G03):

FRN = (1/min)

where; Speed : Metric system (mm/min)

(3) F can be instructed within the following range:

F43 : 0.001 ~ 9999.999

(4) Sample program

G93 ; G91 G01 X100. F5. ; Y50. F10.

Speed

Distance

Speed

Distance

Inch system (inch/min)

Distance : Metric system (mm/min)

Inch system (inch)

Spped: 500mm/min

3 - 3

(5) Cautions

(a) In G93 mode, F code must be instructed per block.

When F code is omitted, a previously instructed F code becomes valid.

3-4 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, proceeds to the next block.

(1) Command format

G09 ------ ;

(2) Sample program

N1 G09 G91 G01 X100. F500 ; N2 G01 Y-50. ;

The corner has an edge when G09 is specified. The corner is rounded when G09 is not specified.

(3) Associated parameters

No.1826 Imposition width of each axis No.1827 Imposition width of each axis on cutting feed

3-5 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.

(1) Command format

G61 ;

3 - 4

(2) Sample program

N1 G61 G91 G01 X100. F500 ; N2 Y-50. ; N3 X - 100. ; N4 G64;

(3) Cautions

3-6 Automatic Corner Override (G62)

Exact stop effective blocks

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

When tool diameter 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 rate to reduce the cutting load. Once G62 is specified, it remains effective until G61, G63 or G64 is specified.

(1) Command format

G62 ;

(2) Types of automatic corner override

(a) Automatic override in the

inner corner area.

An overridde is applied to this part.

Tool Center Path

(b) Inner arc cutting speed change

Programmed Path

Center

Programmed Path

Tool Center Path

3 - 5

(3) Cautions

3-6-1 Automatic Override in Inner Corner Area

When the following conditions are met in the corner during the tool diameter condensation mode, an override is applied to cutting feed automatically.

[ The conditions are as follows for the blocks having the corner between them. ]

(a) When the G code of Group 01 is either G01, G02 or G03. (b) When an offset amount is other than 0 in the tool diameter offset mode. (c) When an offset is inside in 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. ( (g) When a corner start distance and a corner end distance are other than 0 and internal.

(Le, Ls)

An override is applied to cutting feed from the

Center

(1) An override amount for cutting feed is set with the parameter.

(Automantic corner override amount) 100 (%)

An actual cutting feed rate is as follows.

× (Automatic corner override amount) × (Feed rate override)

point a through point b.

where;

θ : Inner criterion angle

Le : Start distance Ls : End distance

θ)

3 - 6

(2) Sample program

(D10 = 10.) N1 G62 G42 G91 G00 X20. Y50. D10; N2 G01 X50. F200; N3 G03 X30. Y-30. R30.; N4 G64 G40 G00 X20.;

(3) Cautions

(4) Associated parameters

No. 1711 Inner criterion angle of automatic corner override No. 1712 Override amount of Automatic corner override. No. 1713 Start distance of automatic corner override No. 1714 End distance of automatic corner override

An override is applied from the point a though point b.

(5) Associated alarm

3-6-2 Inner Arc Cutting Speed Change

When arc cutting is offset inside during the tool diameter compensation node, an override of the ratio of radius of the tool diameter center path to that of the programmed path is applied to the specified cutting feed rate. The cutting speed in the tool diameter center path is as follows.

Fx where; Rc : Radius of the tool center path

Rp : Radius of the programmed path

Programmed Path

Tool Center Path

Center

3 - 7

(1) Sample program

N1 G62 G41 G91 G00 X50. D10; N2 G03 Y50. J25. F200; N3 C64 G40 G00 X-50.;

Override is aplied to the N2 block

(2) Cutting feed rate when automatic corner override overlaps inner arc cutting

F x x (Automatic corner override) x (Feed rate override)

(3) Cautions

(a) By parameter setting, inner arc cutting speed change can be enabled regardless of the

G62 mode.

(b) When the value of Rc/Rp is smaller than the parameter set value, the minimum

deceleration ratio of the parameter set value is used.

(4) Associated parameters

No. 3406, #0 = 0 Inner arc cutting speed change is regardless of the G62 mode.

1 Inner arc cutting speed change is enabled in the G62 mode.

No. 1710 Minimum deceleration ratio of the inner arc cutting speed

(5) Associated alarms

3 - 8

3-7 Tapping Mode (G63)

The control state of the NC unit is as follows until G61, G62 or G64 is specified after G63 is specified.

(a) Cutting feed rate override fixed at 100 %. (b) Feed hold disabled (c) Spindle override fixed at 100 % (a) Single block disabled (e) Decelerated stop disabled at the joint of the blocks (imposition check disabled) (f) Tapping mode signal output (g) Dry run disabled

(1) Command format

G63 ;

(2) Sample program

N1 G63 G91 G01 X10. F200 ; N2 Z -30. ; N3 Z30. ;, N4 X10. ; N5 Z - 30. .; N6 Z30. ; N7 G64 X10 ;

Tapping mode effective blocks

(3) Cautions

(a) By Parameter setting, you can invalidate dry run disabled.

(4) Associated parameters

No.1401, #5= 0 Disables dry run for thread cutting and tapping commands.

1 Enables dry run for thread cutting and tapping commands.

3 - 9

3-8 Cutting Mode (G64)

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

Programmed Path

Actual Tool Path

(1) Associated G code

G61 Exact stop G62 Automatic corner override G63 Tapping mode G64 Cutting mode

(2) Cautions

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

3 - 10

3-9 Automatic Acceleration/Deceleration

As post-interpolation acceleration/deceleration apply automatically to all commands, no special consideration is necessary.

Rapid traverse (G00, ) : Linear type acceleration/deceleration Cutting feed (G01, G02, G03, ) : Exponential type acceleration/deceleration

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

(a) For rapid traverse, acceleration/deceleration is always pefformed every one block. (b) For cutting feed, acceleration/deceleration is performed continuously instead of every

one block.

(2) Cautions

(a) Optimal values for parameters relating to acceleration/deceleration control have been

set for each machine

(b) For cutting feed, acceleration/deceleration is performed continuously instead of every

one block.

3-10 Dwell (G04)

When specifying by time: A G04 command causes the machine to wait for the time

When specifying by revolutions: A G04 command causes the machine to wait for the

(1) Command format

(a) When specifying by time

G94 G04 ;

P_or X_ : Dwell time (0.001 to 99999.999 sec.)

(b) When specifying by revolutions

G95 G04 ;

P_or X_ :Spindle rotation angle (0.001 to 9999.999 rev.)

specified with the address P or X and delays switching to the next block by this time.

spindle rpm specified with the address P or X And delays switching to the next block for this time.

P _

{ }

P _

{ }

3 - 11

(2) Sample program

G94 G04 P2000 ; Dwell time 2 seconds G04 X2. ; Dwell time 2 seconds

(3) Cautions

(a) By parameter setting, you can specify by time even during the feed per revolution

mode.

(4) Associated parameters

Not 3400, #5 = 0 G04 always specifies by time.

1 G04 follows G94 or G95.

3 - 12

4. REFERENCE POINT

4-1 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.

(1) Command format

G28 X_Y_Z_... ;

(2) Sample program

G28 G91 X-50.Y100. ;

Intermediate Point

(Positioning)

Start Point

1st Reference Point

(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(overtravel) occurs before completing reference point return, the axes retract by the amount set with the parameters and perform reference point return again.

(4) Cautions

(a) The G28 command onward is high-speed return after completion of reference point

return.

(b) The G28 command makes a reference point return check upon completion of high-

speed return, and if the axes have not returned, an alarm results.

specified with G53, and then, they return to the reference point.

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

4 - 1

(5) Associated parameters

(6) Associated alarms

4-2 Reference Point Return Check (G27)

After positioning the axes to the program -specified position, a G27 command checks whether they have returned to the 1st reference point, and when they have not returned to the 1st reference point, an alarm results.

(1) Command format

G27 X_ Y_ Z_ ... ;

(2) Sample program

G27 G91 X100. Y-50. ; After the X axis and Y axis moved by 100 and - 50, respectively, it is checked whether they have returned to the 1st reference point.

(3) Cautions

(a) The position reached with a G27 command has tool length compensation, tool offset

and tool diameter compensation amounts added to it. (b) Only the axis specified in the G27 block is checked whether it has returned. (c) The 2nd to 4th reference point return check is possible.

G27 P_ X_ Y_ Z_ ... ;

Where; P2 - P4 : Specify corresponding to the 2nd through 4th reference points. (d) The axis for which the machine lock function is turned on has no position check

conducted on the reference point. (e) The G27 command confirms imposition upon return to the reference point.

4 - 2

(4) Associated parameters

(5) Associated alarms

4 - 3

4-3 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.

(1) Command format

G29 X_Y_Z_... ;

(2) Sample program

N1 G28 G91 X-50. Y100. ; N2 G29 G91 X50. Y50.;

N2(G29)

Intermediate Point

N2(G29)

N1(G28)

Reference Point

(3) Cautions

(a) If G29 is specified with no G28 or G30 specified once, the intermediate point becomes

zero.

N1(G28)

4 - 4

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

A G30 command can automatically return the axes specified in the program to the 2nd to 4th reference point after positioning them to the intermediate point. The 2nd, 3rd, and 4th reference points are the positions specific to the machine and set with the parameters.

(1) Command format

P2 P3

G30 X_ Y_ Z_ ...;

{ }

where; P2 : 2nd reference point return

P3 : 3rd reference point return P4 : 4th reference point return Default : 2nd reference point return

(2) Sample program

G30 G91 P3 X-50. Y100.; Y

3rd Reference Point

(3) Cautions

(a) The G30 command confirms imposition upon return to the reference point. (b) If G90 G30 G53 P_X_Y_Z_...; is specified, the axes are positioned to the position

specified with G53, and then, returned to the 2nd - 4th reference point.

Intermediate Point

Start Point

4 - 5

(4) Associated parameters

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

(5) Associated alarms

4 - 6

4-5 Reset of Floating Reference point (G301)

G301 instruction may be automatically reset to the following reference point after an axis instructed by the program is positioned at a middle point. The floating reference point is a selected point on the machine. The floating reference point can be set in accordance with the following procedure:

1 Pressing the POSITION key selects the position screen. 2 Pressing F6 and Y keys set a present position of the polar coordinate system as a

floating reference point.

(1) Command format

G301 X_Y_Z... ;

(2) Sample program

G301 G91 X-50. Y100 ;

Floating Reference Point

(3) Cautions

(a) G301 instruction checks In-Position when reset to the floating reference point. (b) G90, G301, G53 and X_Y_Z resets the floating reference point after positioning them

to G53 instruction.

(4) Associated parameters

No. 1229 Floating reference point of each axis.

Middle Point

Start Point

4 - 7

4 - 8

5. COORDINATE SYSTEM

5-1 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.

(1) Command format

G90 G53 X_ Y_ Z_... ;

(2) Sample program

G90 G53 X20. Y10. ;

End

10.

Point

Machine Coordinate System

(3) Cautions

(a) An alarm results if this is specified in the G91 mode. (b) Specify this after cancelling tool diameter compensation. (c) The G53 command is effective only in the block where it is specified. (d) The G53 command confirms imposition at the end point of the block.

(4) Associated parameters

(5) Associated alarms

No. 146 Machine coordinate system selection was specified in the G91 mode.

20.

(G00)

Start Point

Work Coordinate System

5 - 1

5-2 Work Coordinate system selection (G54 - G59)

Six peculiar coordinate systems can be set by specifying G54 - G59, respectively. Before specifying G54 - G59, set the offset amount (machine coordinate system position when the tool nose is positioned to the zero point of the work coordinate system) from the machine zero point to the zero point of each work coordinate system.

(1) Command format

G54 ; Work coordinate system 1 selection C55 ; Work coordinate system 2 selection C56 ; Work coordinate system 3 selection G57 ; Work coordinate system 4 selection G58 ; Work coordinate system 5 selection G59 ; Work coordinate system 6 selection

G54 Work Coordinate System

G54 Offset Amount

Machine Coordinate System

Amount

G55 Work Coordinate System

G55

Offset

Amount

(2) Sample program

N1 G54 G90 G00 X0 Y0 ; where; G54 offset amount is;

X - 200.

Y - 250. This Command positions the axes to (0, 0) of the work coordinate system; the then position of the machine coordinate system is (-200., -250.).

Offset

G56 Work Coordinate System

G56 Amount

Offset

G57

Machine Coordinate System

Start Point

G54 Work Coordinate System

G57 Work Coordinate System

Offset Amount

G59 Offset Amount

G58

-200

(0.0)

G58 Work Coordinate System

G59 Work coordinate system

G54

Offset

Amount

250

5 - 2

(3) Cautions

(a) The G54 work coordinate system is selected in the reset state. (b) The G54 coordinate system is set upon completion of zero point return. (c) When the offset amount of the work coordinate system is changed, the new work

coordinate system is set when corresponding G54 - G59 is specified next time.

(d) When G54 - G59 is specified after setting the new coordinate system with a G92

command, the zero point of the machine coordinate system and the offset amount of the G54 - G59 work coordinate system are changed relatively by the amount set newly with G92.

(e) When establishing the G54 - G59 work coordinate system after specifying G92, it is

necessarily to specify manual zero point return or G921 (work coordinate system preset) in the reset state.

(f) Set the G54 through G59 offset amounts in the work coordinate screen.

5-3 Addition of Work Coordinate system Pairs (G540 - G599)

Sixty peculiar coordinate systems can be set by specifying G540 - G599, respectively. Before specifying G540 - G599, set the offset amount (machine coordinate system position when the tool nose is positioned to the zero point of the work coordinate system) from the machine zero point to the zero point of each work coordinate system.

(1) Commad format

G540 ; G540 work coordinate system selection G541 ; G541 work coordinate system selection C542 ; G542 work coordinate system selection

:: ::

G599 ; G599 work coordinate system selection

Offset

G541 Work Coordinate System

G541

Offset Amount

G540 Work Coordinate System

G540 Offset Amount

Amount

G542 Work Coordinate System

G542

G599 Work Coordinate System

G599

Offset Amount

Machine Coordinate System

5 - 3

(2) Sample program

NI G540 G90 G00 X0 Y0; where; G540 offset amount is;

X - 210.

Machine Coordinate System

-210.

Y - 260. This command positions the axes to (0, 0) of the work coordinate

Start Point

system; then the position of the machine coordinate system will be (-210., -260.).

G540 Work Coordinate System

-260.

(3) Cautions

(a) G540 through G599 aid G54 through G59 are the G codes of the same group. (b) When G540 - G599 is specified after setting the new coordinate system with a G92

command, the zero point of the machine coordinate system and the offset amount of the G540 - G599 work coordinate system are changed relatively by the amount set newly with G92.

necessary to specify manual zero point return or G921 (work coordinate system preset) in the reset state.

(f) Set the G540 through G599 offset amounts in the Work Coordinate screen.

5 - 4

5-4 Local Coordinate System Setting (G52)

One additional coordinate system can be set in the selected work coordinate system by specifying G52.

(1) Command format

G54 X _ Y _ Z _... ; Local coordinate system setting

Offset Amount of Local Coordinate System Setting

Local Coordinate System

Local Coordinate System Offset Amount

Work Coordinate System

Work Coordinate System Offset Amount

Machine Coordinate system

G52 X0 Y0 Z0...; Local Coordinate System Setting Cancel

(2) Sample program

N1 G54 ; N2 G52 X-150. Y-100.; N3 G90 G00 X0. Y0.;

where; G54 offset amount;

Machine Coordinate System

-350.

-200.

X - 200.

Y - 250. Executing the N1 block sets the G54 work coordinate system. Executing the N2 block sets the local coordinate system. Executing the N3 block positions the axes to (0, 0) of the local coordinate

Start Point

G54 Work Coordinate System

Local Coordinate System

-150.

(0, 0)

Offset

Amount

(0, 0)

Local Coordinate System Offset Amount

-100.

system; the then position of the machine coordinate system will be (-350., -350.).

(3) Rotation of the offset amount

When the local coordinate system is set during the coordinate rotation (type A) mode, the offset amount rotates. However, rotation of the offset amount is not cancelled even if coordinate rotation is cancelled by specifying G69. When the local coordinate system is set during coordinate rotation, cancel the local coordinates first and then, cancel coordinate rotation.

G54

-250.

-350.

5 - 5

(4) Cautions

(a) In the reset state, the local coordinate system A is cancelled. (b) The local coordinate system of the axis specified with G92 is cancelled. (c) An alarm results if G52 is specified during the tool diameter compensation mode. (d) G52 is a one-shot command. The local coordinate system created with G52 remains

effective until next G52 is specified.

(5) Related parameters

No. 1200, #0 = 0 The offset Amount of the local coordinate system rotates.

1 The offset amount of the local coordinate system does not rotate.

5 - 6

5-5 Work Coordinate System Change (G92)

By specifying G92, you can create the coordinate system on the program without using the G54

-G59 of G540 - G569 work coordinate system. (1) Command format

G92 X_Y_Z...;

Position to Specify Current Position in G92 Work Coordinate System.

G92 Command Position

Old Work Coordinate System

Machine Coordinate System

Work Coordinate System by G92 Command

(2) Sample program

N1 G90 G00 X50. Y50. ; N2 G92 X150. Y200. ; Executing the N2 block creates the work coordinate system in which the current position will be (150., 200.).

200.

50.

(0, 0)

Machine Coordinate System

G92 Command Position

(0, 0)

50.

Old Work Coordinate System

Work Coordinate

150. System by G92 Commamd

(3) When G92 is specified with the G54 - G59 or G540 - G599 work coordinate system

established; The G92 command shifts all of the G54 -G59 and G540 - G599 work coordinate systems which are based on the machine coordinate system.

5 - 7

(4) Cautions

(a) G92 is a one-shot command. (b) G92 has nothing to do with absolute (G90)/incremental(G91) programming. (c) If G92 is specified while tool diameter compensation, tool length compensation or tool

offset is applied, the coordinate system is set as if G92 is specified at the position prior

to compensation. (d) The local coordinate system of the axis specified with G92 is cancelled. (e) There are two methods available for invalidating the work coordinate system with the

G92 command.

(i) Perform manual zero point return inthe reset state.

(ii) Specify G921 X0 Y0 Z0... ; (work coordinate system preset).

5 - 8

5-6 Work Coordinate System Preset (G921)

If you perform first manual reference point return after turning on the NC unit, the machine coordinate system is set, and then, the work coordinate system is set. Manual reference point return in the reset state sets the work coordinate system. The work coordinate system is shifted from the machine coordinate system by the following command or operation. In this case, it is called "work coordinate system preset" to set the work coordinate system again based on the machine coordinate system.

(a) When a manual absolute signal is turned off and manual operation intervenes. (b) When an axis move command is specified in the machine lock mode. (c) When moving the axes by handle interrupt or manual automatic simultaneous

operation. (d) Work coordinate system shift with the G92 command. (e) Work coordinate system origin by MDI operation.

G54(or other) Work coordinate System and G54(or other) Work Coordinate system after Work Coordinate System Preset.

Shift by G92

Machine coordinate System

(1) Command format/operation

(a) By the G code

G921 X0 Y0 Z0 ...;

Work Coordinate System Preset Axes

(b) By operation

Perform manual reference point return in the reset state (OP signal OFF).

G54(or other) Work Coordinate System Shifted by G92

Shift by Work Coordinate Preset

5 - 9

(2) Cautions

(a) Using a G921 Command cancels tool diameter compensation, tool length

compensation and tool offset. (b) By parameter setting, the work coordinate system can be preset just before executing

the first block in which the machine is switched over from the reset state to automatic

operation.

(3) Associated parameters

No. 1202, #0 Presetting of work coordinate system on recovery of manual

reference point is: =0 Carried out in reset state. =1 Carried out in any circumstance.

No. 1202, #2 Presetting of work coordinate system on recovery of manual

reference pint: =0 Follows #0 of Parameter No. 1202. =1 No presetting takes place for any axis.

No. 1202, #3 Work coordinate system, on starting of auto operation following reset

state : =0 Does not perform presetting. =1 Performs presetting.

(Note 1) When "presetting takes place in any circumstance" (No.2403, #0=1) has been set,

processing is carried out only when no pre-read block exists and a execution block has been completed.

(4) Associated alarms

5 - 10

5-7 Work Coordinate System Shift (External Work Zero Point Offset Amount)

The entire G54 or other work coordinate system can be shifted by the specified amount (external work zero point offset amount) by setting an offset amount in the external offset of the work coordinate system in the NC screen.

G54 Work Coordinate System

External Work Zero Point Offset Amount

Machine Coordinate System

G55 Work Coordinate System

G599 Work Coordinate System

G599 Offset Amount

(Note 1) When the external work zero point offset amount is changed, it becomes effective

from the block where the G54 or other work coordinate system is specified.

(Note 2) If set to parameter No. 1201, #0.= 1, enabled as soon as the external work origin

offset amount is changed.

5 - 11

5-8 Plane Selection (G17, G18, G19)

With a G17, G18. or G19 Command, this function specifies the plane in which an arc command, tool diameter compensation, coordinate rotation, etc. are performed.

(1) Command format

G17 X G18 Z G19 Y G17 ; X-Y plane G18 , Z-X plane G19 ; Y-Z plane

(2) Sample program

G00 G91 ; G17 U0 Y0; Selects the U-Y plane.

G00 G91 ; G18 W0 X0; Selects the W-X plane

_ YP _; XP-YP plane

_ XP_; ZP-XP plane

_ ZP_; YP-ZP plane

where; XP: X axis or its parallel axis

: Y axis or its parallel axis

: Z axis or its parallel axis

: : The U-Y plane is effective. :

: : The W-X plane is effective.

(3) Cautions

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

parallel. (b) Set with the parameter whether the reset state is to be the G17 or G18 mode. (c) An alarm results when the plane is not determined in the block where G17, G18 or

G19 was specified.

(Example) G17 X_ U_ Y_ ; It is uncertain whether the X-Y or U-Y plane is selected. (d) A move command is irrelevant to plane selection.

5 - 12

(4) Associate parameters

No. 3402, #5 =0 The reset state is the G17 mode

1 The reset state is the G18 mode

(5) Associate alarms

No. 106 A plane seleection (G17 - G 19) commend has an error.

5 - 13

5-9 Rotary T able Dynamic Fixture Offset

When loading a workpiece on the rotary table and set a work coordinate system after measuring a position of workpiece if the rotary table has rotated before starting cutting, the work coordinate system should be set again by measurement of a position of workpiece once more. However, if a position of workpiece at a certain position of the rotary table is set at the standard fixture offset amount, even if the rotary table rotate, calculate a fixture offset amount at this time automatically from an angle of the rotary table and make a work coordinate system according to this value. In view of these facts, if a position is set once at the standard fixture offset amount, the work coordinate system can be held dynamically corresponding to a position even if The rotary table rotates any position. A position adding a work reference point offset amount on the fixture offset amount on the fixture offset amount becomes the work coordinate reference point.

(1) Setting of data.

1 Three-piece set of parameter designated a rotary axis and two linear axes constructed

a rotary plane. In each set, the 1st parameter is for a rotary axis number, and the 2nd and 3rd ones for linear axis numbers. Set the two linear axis numbers so that rotation from the positive direction of the 2nd linear axis to that of the 3rd linear axis will be positive directional rotation of the 1st rotary axis. To calculate a fixture offset amount, calculate it for the rotary axis of the 1st set, and then, calculate it for the 2nd and 3rd sets with respect to that result. If you do not need as many as 3 sets, set 0 for the rotary axis. When there are two or more rotary axes and the rotating plane is changed by other rotation, set the rotating plane when the position of the rotary axis is 0 degree.

2 Standard fixture offset amount at the standard angle of rotary axis. Set a certain

position of rotary axis (standard angle) and a fixture offset amount at the time. Setting is done by the fixture offset screen. Number of sets are 8 sets.

5 - 14

W : Work Shift Amount F : Fixture Offset Amount at

F’

Reference Angle

Machine Zero Point

3 Parameter for effective/ineffective of fixture offset for each axis (No. 1208, #0)

Set 1 for the axis to be effective of fixture offset.

4 Type of fixture offset (No.1200, #1)

When a vector of fixture offset has changed (command of G522 or when a rotary axis

is moved during a command of G522),set whether a changing amount of vector is

moved or not moved.

When it is 0, it moves. (Work coordinate is not changed and machine coordinate is

When it is 1, it does not move. (Work coordinate is changed and machine coordinate

(2) Command form

G522 Pn ;

n : No. of fixture offset amount (1-8) By a command of G522 Pn ;,calculate a fixture offset amount by a present rotary angle and a data designated by n and make the fixture offset amount effective. By a command of G522 P0 ;,make the fixture offset amount ineffective. Also, if a rotary axis which is related a fixture offset during G522 mode is moved, execute a calculation of vector again.

changed.)

is not changed.)

5 - 15

(3) Program example and notion

parameter No.1285 4 (C axis)

No.1286 1 (X axis) No.1208, #0 (X) =1 (X axis is effective) No.1287 2 (Y axis) No.1208, #0 (Y) =1 (Y axis is effective)

Data of n= 1 X = -10.0

Y=0 C = 180.0 (standard angle)

C=180

(Reference Angle)

C=90

[N3]

Center of Rotation

Work coordinate value

Machine coordinate value

Fixture offset amount

Program X Y C X Y C X Y C

N1 G90 G00 X0 Y0 C90.;0 0 90. 0 0 90. 0 0 0 N2G 522 P1 0 0 90. 0 10. 90. 0 10. 0

[ 0 -10. 90. 0 0 90. 0 10. 0 ] N3 G01 X10. Y2. F100; 10. 2. 90. 10. 12. 90. 0 10. 0 N4 G02 X2. Y10. R10.; 2. 10. 90. 2. 20. 90. 0 10. 0 N5 G01 X0 Y0,. 0 0 90. 0 10. 90. 0 10. 0

In the bracket show #1 = 1 of parameter 1200

(4) Motion at reset

At the time of reset, whether the fixture offset is cancelled or not is according to the #2 of parameter 1200. When it is 1, a vector before reset is held. When it is 0, a vector is cleared. However, the machine does not move for a vector cleared.

5 - 16

(5) Screen of fixture offset

To select the Fixture offset screen, use F6/FIXTURE OFFSET or F4/WORK COORDINATE .

ACT at the upper left of the screen displays the currently selected fixture offset number (P) and fixture offset vector.

(6) Input/output of fixture offset amount

Setting and input/output of data in a program with outside is available. (a) Setting of standard fixture offset amount by G10

Standard fixture offset amount or standard angle in a program can be set. G10 L22 P_ X_ Y_ Z ... ;

P1 - P8 : Fixture offset No.

X, Y, Z... : Standard fixture offset amount or standard angle of each axis.

When it is executed in the G90 mode, a value itself is set. When it is executed in the G91 mode, a value add on the previous value is set.

(7) Precautions

(a) A command of G522 and rotary axis related a fixture offset during a command of G522

is restrained a buffering.

5 - 17

(b) If a parameter or standard fixture offset amount are changed during the G522 mode, it

becomes effective after a command of next G522.

calculation for vector of fixture offset is not executed. Also, command the first designated rotary axis by the G90 mode.

Command by the machine coordinated system (G53) Change of the work coordinate system (G92, G52, G54 to G59, G540 to G599) Reference point return related (G27, G28, G30, G301)

(d) A movement by changing a vector of fixture offset is according to a G code of group

01 at that time. A command of G522 should be done in the G00 or G01 mode.

(e) When stopping an automatic operation by the single block during the G522 mode etc.

and move a rotary axis by hand, a vector of fixture offset is not changed. Execute a calculation of vector when a commanding a rotary axis at automatic or MDI operation or commanding the G522. However, after a rotary axis is moved by hand, execute a calculation of vector by using a coordinate value which is nor reflected an intervenient value by hand when a rotary axis is command in the G91 mode.

(f) The coordinate values of the rotary axis used in fixture offset calculation are those in

the work coordinate system. If an offset is applied such as a tool offset, use the coordinate values available prior to applying an offset. Use also the pre-offset coordinate values as to mirror image and scaling.

(g) High-accuracy contour control cannot be command in the G522 mode.

Even if high-accuracy contour control is provided in the G522 node and the rotary axis is moved, the vector will hot be calculated.

(h) When using the rollover function for the rotary axis, be sure to assume a move amount

per revolution of the rotary axis to be 360 degrees.

(8) Related parameters

No.1200, #1 = 0 Moves when the fixture offset vector changes.

= 1 Does not move when the fixture offset vector changes.

No.1200, #2 = 0 Clears the modal information by reset.(clears the vector )

= 1 Does not clear the modal information by reset.(Holds the vector)

5 - 18

No.1200, #3 = 0 Enables only the fixture offset axis setting parameters in the 1st set.

= 1 Enables the fixture offset axis setting parameters in the three sets.

No.1208, #0 = 0 Disables fixture offset (for each axis).

= 1 Enables fixture offset (for each axis).

No.1285 Fixture offset target rotary axis number (1st set) No.1286 Axis number of the linear axis-1 which consists the fixture offset plane

(1st set)

No.1287 Axis number of the linear axis-2 which consists the fixture offset plane

(1st set) No.1288 Fixture offset target rotary axis number (2nd set) No.1289 Axis number of the linear axis-1 which consists the fixture offset plane

(2nd set) No.1290 Axis number of the linear axis-2 which consists the fixture offset plane

(2nd set) No.1291 Fixture offset target rotary axis number (3rd set) No.1292 Axis number of the linear axis-1 which consists the fixture offset plane

(3rd set) No.1293 Axis number of the linear axis-2 which consists the fixture offset plane

(3rd set)

(9) Related alarms

No.155 Fixture offset command error (#001) No offset number (#002) Offset number beyond the range (#003) Erroneous parameter setting (No. 1285 to No. 1293) (#004) Not in the G00 or G01mode

5 - 19

5 - 20

6. COORDINATE

6-1 Absolute/Incremental Programming (G90,G91)

In programming, you can select either absolute progaramming which causes an axial move following the axial address to move to the specified position of the coordinate system, or incremental programming which causes it to move to the incremental position of the current position.

(1) Command format

G90 ; Absolute programming G91 ; Incremental programming

(2) Sample program

(a) Absolute programming (b) Incremental programming

G90 G01 X100. Y50. F200 ; G90 G01 X100. Y50. F200 ;

Start Point

End Point

X100.

50.

Start Point

End Point

100.

(3) Cutions

(a) The G90 and G91 command are modal G codes.

Once G90 is specified, it remains effective until G91 is specified.

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

(4) Associated parameters

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

1 The reset state is the G90 mode.

Y50.

6 - 1

6-2 Polar Coordinate Input (G15,G16)

This command allows you to specify the end point coordinate value of the mochining program in terms of radius and angle.

(1) G code

G15 : Polar coordinate command cancel G16 : Polar coordinate command ON

(2) Command format

G16 ; Polar coordinate command ON : : Polar coordinate command cancel : G15 ; Polar coordinate command cancel The following shows the command format in the polar coordinate command mode.

G17 G18

{ }

G19

where; α : Radius (1st axis in the plane)

(a) Specify the plane for a polar coordinate command with plane selection (G17, G18,

G19).

(b) The radius is given as follows.

(i) When a radius value is given by absolute programming, the zero point of the

(ii) When the radius value is given by incremental programming, the current position

When the Radius Value Is Absolute When the Radius Value Is Incremental

G90

α _ β _ ;

{ }

G91

Radius

β : Angle (2nd axis in the plane)

local coordinate system (G52) (zero point of the G54 or other work coordinate system when the local coordinate system has not been set) will be the polar coordinate center.

will be the polar coordinate center.

Emd Point

Angle

End Point

Radius

(Angle)

Polar Coordinate Center

Start Point

6 - 2

Start Point

End Point

Radius

(Angle)

Polar Coordinate Center

(i) When the angle is given by absolute programming, it will be exactly the angle

specified in the block.

(ii) When the angle is given by incremental programming, it will be added to the

angle set in the previous block.

When the Angle Is Absolute

Radius End Point

Angle

Start Point

End Point

When the Angle Is Incremantal

Radius

Angle

(3) Sample program

G17 ; G54 G90 G00 X0 Y0 ; G43 Z0 H01 ; G16 ; Polar coordinate command ON G81 G90 X100. Z-15. R-3 F100 L0 ; N1 G91 Y45. ; Rabius value: Absolute command N2 Y90. ; N3 Y90. ; Angle: Incremental command N4 Y90. ; N5 G15 G80 ; Polar coordinate command cancel

Radius

90°

N3 N4

Angle

45°

6 - 3

(4) Cautions

(a) The following G codes are invalid in the polar coordinate command mode.

G04, G10, G52, G92, G53, G22, G68, G511, G501, G51

(b) The radius for circular interpolation and helical cutting in the polar coordinate

command mode should be specified by radius designation on arc.

6 - 4

6-3 Inch/Metric Input (G20, G21)

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

(1) Command format

G20 ; Inch system G21 ; Metric sysytem (Note) Specify this in an independent block at the beginning of the program.

(2) The following systems of units are changed with the G20 and G21 commands.

(a) Feed rate command with an F code (b) Commands related to the position (c ) Work zero point offset amount, external work zero point offset amount, common

work zero point offset amount (d) Tool offset amount (e) Part of parameters (f ) Unit of one graduation of the manual pulse generator

(3) Cautions

(a) Specify the G20/G21 command in an unit block. (b) When the G20/G21 command is executed, preset the work coordinate system. (c) Do not switch the G20/G21 command halfway the program. (d) Switching inch/metric input can switch by parameter (setting). For switching used by

parameter, turn off the power and then turn on.

6 - 5

(4) Associated parameters

No. 1000, #0 = 0 The increment system is metric.

1 The increment system is inch.

(5) Associated alarms

6 - 6

7. SPINDLE FUNCTION (S FUNCTION)

With the number of revolution of the main spindle (rpm) being commanded in a numerical value of max. 5 digits following Address S, binary code signals, strobe signals (SF), analog signals corresponding to the spindle motor rpm, gear signals, etc. are sent out to Machine side.

(1) Specify a set of S command in one block. (2) Program example:

S1000; Spindle speed 1000 rpm M03; Spindle rotation : : M05; Spindle stop

(3) Cautions

(a) When a negative value has been specified in an S command, the sign always

becomes positive.

7 - 1

7 - 2

8. TOOL FUNCTION (T FUNCTION)

With a value of max. 8 digits following Address T being command, code signals of BCD 8 digits and strobe signals (TF) are output in Machine side.

(1) Specify a set of T command in one block. (2) Program example:

T01; Tool No. 01 is set to Standby : G30 G90 X0 Y0 Z0 M19; T01 M06; Tool change (Tool No. 01 is set to the main spi ndle.)

(3) Cautions

(a) When a negative value has been specified in a T command, the sign always

becomes positive.

8 - 1

8 - 2

9. Miscellaneous Function (M FUNCTION)

9-1 Miscellaneous Function (M Function)

If the address M followed by an up to 8-digit numerical value is specified, the BCD 8-digit code signal and strobe signal (MF) are output to the machine side.

(1) Specify a set of M command in one block.

(2) The following M commands are used as special functions.

(a) M00 (Program stop)

If M00 is specified during automatic operation , automatic operation stops after executing that block. Pressing the CYCLE START switch restarts automatic operation.

(b) M01 (Operational stop)

If the OPERATIONAL STOP switch of the machine operation panel is turned on and M01 is specified, automatic operation stops after executing that block. Pressing the CYCLE START switch restarts automatic operation.

Specify M02 at the end of the program. If M02 is specified during automatic operation, automatic operations tops after executing that block, and the NC unit is reset.

(d) M30 (Program end)

Specify M30 at the end of the program. If M30 is specified during automatic operation, automatic operations tops after executing that block, the NC unit is reset, and you are returned to the beginning of the program.

(e) M98 (Subprogram call)

Call a subprogram with the command ; M98 P_ ;

(f) M99 (subprogram end)

Specify M99 at the end of the subprogram.

9 - 1

(3) Sample program

G30 G91 X0 Y0 Y0 M19 ; T01 M06 ; Tool change M03 ; Spindle forward rotation G54 G90 G00 X0 Y0 ; G43 Z0 H01; : : M05 ; Spindle stop M30 ; Program end %

(4) Cautions

(a) If M00, M01, M02 or M30 is specified, the NC unit stops prereading. (b) When M98 or M99 is specified, the code signal and strobe signal are not sent out. (c) When a negative value is specified in an M command, the sign always become

positive.

9-2 2nd Miscellaneous Function (B Function)

If you specify any one of the parameter-set address U, V, W, A, B and C followed by an up to 8-digit numerical value (-79999999 ~ +79999999), the BCD 8-digit code signal and strobe signal (BF) are output to the machine side.

(1) Specify a set of 2nd miscellaneous function in one block.

(2) Sample program

B180; Indexes the index table by 180 : : B270; Indexes the index table by 270

(3) Caution

(a) The 2nd miscellaneous function is output to the machine side as 32-bit signal data.

Therefore, its programmable range is -79999999 ~ +79999999.

(b) Set the command address (U, V, W, A, B, C) of the 2nd miscellaneous function in the

parameter No. 1020.

°.

9 - 2

(4) Associated parameters

No.1020 Command address of the 2nd miscellaneous function

(5) Associated alarms

9 - 3

9 - 4

10. Canned Cycle

10-1 Canned Cycle (G73, G74, G76, G80 - G89)

This function allows you to specify the machining cycle such as drilling, tapping, boring, etc. in one block. The canned cycle is cancelled if you specify G80 or the G code of Group 01 (G00, G01, G02, G03, etc.) during the canned cycle mode.

(1) G code

G73 : High-speed peck drilling cycle G74 : Counter tapping G76 : Fine boring G80 : Canned cycle cancel G81 : Drilling, spot drilling G82 : Drilling, counter boring G83 : Peck drilling cycle G84 : Tapping G85 : Boring G86 : Boring G87 : Boring, back boring G88 : Boring G89 : Boring

(2) Command format

G98

{ }

G99

G_ X_ Y_ Z_ R_ ,R_ Q_ P_ L_ F_ E_

;

Cutting

feed rate Cutting feed rate

No. of repeats

Dwell time Depth of cut by G73/G83 or shift amount by G76/G77

,R point position

R point position

Z point position

Drilling position

G code of the conned cycle (G73, G74, G76, G81-89)

Return point

(Note 1) men the number of repeats (L) is omitted, L = 1 is assumed.

If L = 0 is specified, the tool moves to the drilling position to invalidate drilling. (Note 2) I, J and K may be used in the G73, G76, G83 and G87 commands. (Note 3) The R point, z point, P, Q, I, J and K are modal in the canned cycle mode.

10 - 1

(3) Machining cycle

The canned machining cycle generally consists of the following movements 1 through 6 .

Where; Rapid traverse

Cutting feed

(Note 1) (Note 2) The ,R-Point command is allowed in the following cycles:

(Note 3) The E-command in the tapping cycle (G74, G84) will result in the feed rate for the

Single block operation is prohibited in the movements 4 , 5 and 6 .

• G81, G82 (Drilling cycle)

• G73, G83 (Peck drilling cycle)

If the ,R-command is omitted, the movement 4 (feed rate F) will be executed after the R-Point, skipping the movement 3 . If the E-command is omitted, the movements designated at the feed rats E will run at the feed rate F.

movement 6. . If the E-command is omitted, the movement 6. will also run at the feed rate F.

Initial Point

R Point

'R Point

Z point

1 : Positioning to the drilling position 2 : Rapid traverse to the R point 3 : Cutting feed to the ,R point (Feed rate E) 4 : Drilling to the Z point (Feed rate F) 5 : Movement at the Z point 6 : Return to the R point 7 : Rapid traverse to the initial point

(4) Return point

The return point of the canned cycle is specified with the following G codes.

G98 : Initial point level return G99 : R point level return.

(Note 1) The initial point is the position of the drilling axis when the canned cycle

cancellation state is switched to the canned cycle mode.

10 - 2

(5) "R-point," "Z-point," and ",R-point"

The R-point and Z-Pint will be as follows in the G90 and G91 commands, but the ,R-point will be always of incremental command.

[ G90 ] [ G91 ]

Initial point

Position

R point

,R point

Z point

(Note 1) The ,R-point is at a position incremental from the R-point.

(6) Plane of the drilling position and drilling axis

The plane of the drilling position is determined with a G17, G18 or G 19 command. The drilling axis is the X, Y or Z axis which does not constitute the plane of the drilling position, or its parallel axis. Whether the drilling axis is the basic axis of parallel axis depends on the drilling axis address Specified in the block containing G73, G 74, G76 or G81 - G89.

G17 G_ X

_ YP_ ZP_ R_ Q_ P_ L_ F_ :

R point

,R point Z point

Mode Drilling Drilling

position Axis

G18 G_ Z

_ XP_ YP_ R_ Q_ P_ L_ F_ :

Mode Drilling Drilling

position Axis

G19 G_ Y

_ ZP_ XP_ R_ Q_ P_ L_ F_ :

Mode Drilling Drilling

position Axis

where : XP : X axis or its parallel axis

: Y axis or its parallel axis

: Z axis or its parallel axis

(Note 1) When Changing over the plane of the drilling position, cancel the canned cycle

first.

(Note 2) By Parameter setting, the drilling axis can be limited to the Z axis regardless of

the G17 - G19 commands.

10 - 3

(7) Description of the movements in the canned cycle

The following. description of the movements in the canned cycle assumes the drilling position to be on the X-Y Plane, and the drilling axis to be the Z axis. (a) G73 (High-speed peck drilling drill)

[Fixed pitch]

G98

G73 X_ Y_ Z_ R_ ,R_ Q_ P_ L_ F_ E_ ;

G99

{ }

[ G98 ] [ G99 ]

Q Q Q

(X, Y)

pr pr pr

(X, Y)

Initial point R point

,R point

Z point

pr : Parameter setting

[Variable pitch]

G98

G73 X_ Y_ Z_ R_ ,R_ I_ J_ K_ P_ L_ F_ E_ ;

{ }

G99

[ G98 ] [ G99 ]

(X, Y)

Initial point

R point ,R point

Z point

Initial point

R point ,R point

I - J

I - 2J

pr pr

I - J

I - 2J

pr pr

Z point

pr : Parameter setting

where ; I : Initial value of the depth of cut (positive value)

J : Decremental value in 2nd cut onward (positive value) K : Final value of the depth of cut (positive value)

(Note 1) When there is a Q command before specifying the variable pitch with

I, J and K, specify Q.

(Note 2) Dwell operation is enabled at the hole bottom by parameter setting.

10 - 4

R point ,R point

Z point

hitachi seiki 10M, 16M, 18M Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual