okuma OSP-P200M, OSP-P200MA, OSP-P20M, OSP-P200M-R, OSP-P200MA-R Programming Manual

...

Download

CNC SYSTEM

OSP-P200M/P200MA/P20M OSP-P200M-R/P200MA-R/P20M-R

PROGRAMMING MANUAL

(10th Edition)

Pub No. 5228-E-R9 (ME33-018-R10) Oct. 2010

5228-E P-(i)

SAFETY PRECAUTIONS

The machine is equipped with safety devices which serve to protect personnel and the machine itself from hazards arising from unforeseen accidents. However, operators must not rely exclusively on these safety devices: they must also become fully familiar with the safety guidelines presented below to ensure accidentfree operation. This instruction manual and the warning signs attached to the machine cover only those hazards which Okuma can predict. Be aware that they do not cover all possible hazards.

1. Precautions Relating to Installation

(1) Please be noted about a primary power supply as follows.

• Do not draw the primary power supply from a distribution panel that also supplies a major

noise source (for example, an electric welder or electric discharge machine) since this could cause malfunction of the CNC unit.

• If possible, connect the machine to a ground not used by any other equipment. If there is

no choice but to use a common ground, the other equipment must not generate a large amount of noise (such as an electric welder or electric discharge machine).

(2) Installation Environment

Observe the following points when installing the control enclosure.

• Make sure that the CNC unit will not be subject to direct sunlight.

• Make sure that the control enclosure will not be splashed with chips, water, or oil.

• Make sure that the control enclosure and operation panel are not subject to excessive

vibrations or shock.

• The permissible ambient temperature range for the control enclosure is 5 to 40°C.

• The permissible ambient humidity range for the control enclosure is relative humidity 50%

or less at 40°C (no condensation).

• The maximum altitude at which the control enclosure can be used is 1000 m (3281ft.).

2. Points to Check before Turning on the Power

(1) Close all the doors of the control enclosure and operation panel to prevent the entry of water,

chips, and dust.

(2) Make absolutely sure that there is nobody near the moving parts of the machine, and that there

are no obstacles around the machine, before starting machine operation.

(3) When turning on the power, turn on the main power disconnect switch first, then the CONTROL

ON switch on the operation panel.

3. Precautions Relating to Operation

(1) After turning on the power, carry out inspection and adjustment in accordance with the daily

inspection procedure described in this instruction manual.

(2) Use tools whose dimensions and type are appropriate for the work undertaken and the machine

specifications. Do not use badly worn tools since they can cause accidents.

(3) Do not, for any reason, touch the spindle or tool while spindle indexing is in progress since the

spindle could rotate: this is dangerous.

(4) Check that the workpiece and tool are properly secured.

(5) Never touch a workpiece or tool while it is rotating: this is extremely dangerous.

(6) Do not remove chips by hand while machining is in progress since this is dangerous. Always

stop the machine first, then remove the chips with a brush or broom.

(7) Do not operate the machine with any of the safety devices removed. Do not operate the

machine with any of the covers removed unless it is necessary to do so.

(8) Always stop the machine before mounting or removing a tool.

5228-E P-(ii)

SAFETY PRECAUTIONS

(9) Do not approach or touch any moving part of the machine while it is operating.

(10) Do not touch any switch or button with wet hands. This is extremely dangerous.

(11) Before using any switch or button on the operation panel, check that it is the one intended.

4. Precautions Relating to the ATC

(1) The tool clamps of the magazine, spindle, etc., are designed for reliability, but it is possible that

a tool could be released and fall in the event of an unforeseen accident, exposing you to danger: do not touch or approach the ATC mechanism during ATC operation.

(2) Always inspect and change tools in the magazine in the manual magazine interrupt mode.

(3) Remove chips adhering to the magazine at appropriate intervals since they can cause

misoperation. Do not use compressed air to remove these chips since it will only push the chips further in.

(4) If the ATC stops during operation for some reason and it has to be inspected without turning the

power off, do not touch the ATC since it may start moving suddenly.

5. On Finishing Work

(1) On finishing work, clean the vicinity of the machine.

(2) Return the ATC, APC and other equipment to the predetermined retraction position.

(3) Always turn off the power to the machine before leaving it.

(4) To turn off the power, turn off the CONTROL ON switch on the operation panel first, then the

main power disconnect switch.

5228-E P-(iii)

SAFETY PRECAUTIONS

6. Precautions during Maintenance Inspection and When Trouble Occurs

In order to prevent unforeseen accidents, damage to the machine, etc., it is essential to observe the following points when performing maintenance inspections or during checking when trouble has occurred.

(1) When trouble occurs, press the emergency stop button on the operation panel to stop the

machine.

(2) Consult the person responsible for maintenance to determine what corrective measures need

to be taken.

(3) If two or more persons must work together, establish signals so that they can communicate to

confirm safety before proceeding to each new step.

(4) Use only the specified replacement parts and fuses.

(5) Always turn the power off before starting inspection or changing parts.

(6) When parts are removed during inspection or repair work, always replace them as they were

and secure them properly with their screws, etc.

(7) When carrying out inspections in which measuring instruments are used - for example voltage

checks - make sure the instrument is properly calibrated.

(8) Do not keep combustible materials or metals inside the control enclosure or terminal box.

(9) Check that cables and wires are free of damage: damaged cables and wires will cause current

leakage and electric shocks.

(10) Maintenance inside the Control Enclosure

a. Switch the main power disconnect switch OFF before opening the control enclosure door.

b. Even when the main power disconnect switch is OFF, there may some residual charge in

the MCS drive unit (servo/spindle), and for this reason only service personnel are permitted to perform any work on this unit. Even then, they must observe the following precautions.

• MCS drive unit (servo/spindle)

The residual voltage discharges two minutes after the main switch is turned OFF.

c. The control enclosure contains the NC unit, and the NC unit has a printed circuit board

whose memory stores the machining programs, parameters, etc. In order to ensure that the contents of this memory will be retained even when the power is switched off, the memory is supplied with power by a battery. Depending on how the printed circuit boards are handled, the contents of the memory may be destroyed and for this reason only service personnel should handle these boards.

(11) Periodic Inspection of the Control Enclosure

a. Cleaning the cooling unit

The cooling unit in the door of the control enclosure serves to prevent excessive temperature rise inside the control enclosure and increase the reliability of the NC unit. Inspect the following points every three months.

• Is the fan motor inside the cooling unit working?

The motor is normal if there is a strong draft from the unit.

• Is the external air inlet blocked?

If it is blocked, clean it with compressed air.

7. General Precautions

5228-E P-(iv)

SAFETY PRECAUTIONS

(1) Keep the vicinity of the machine clean and tidy.

(2) Wear appropriate clothing while working, and follow the instructions of someone with sufficient

training.

(3) Make sure that your clothes and hair cannot become entangled in the machine. Machine

operators must wear safety equipment such as safety shoes and goggles.

(4) Machine operators must read the instruction manual carefully and make sure of the correct

procedure before operating the machine.

(5) Memorize the position of the emergency stop button so that you can press it immediately at any

time and from any position.

(6) Do not access the inside of the control panel, transformer, motor, etc., since they contain high-

voltage terminals and other components which are extremely dangerous.

(7) If two or more persons must work together, establish signals so that they can communicate to

confirm safety before proceeding to each new step.

8. Symbols Used in This Manual

The following warning indications are used in this manual to draw attention to information of particular importance. Read the instructions marked with these symbols carefully and follow them.

DANGER

indicates an imminently hazardous situation which, if not avoided, will result in death or serious injury.

WARNING

indicates a potentially hazardous situation which, if not avoided, could result in death or serious injury.

CAUTION

indicates a potentially hazardous situation which, if not avoided, may result in minor or moderate injury.

CAUTION

5228-E P-(v)

SAFETY PRECAUTIONS

indicates a potentially hazardous situation which, if not avoided, may result in damage to your property.

SAFETY INSTRUCTIONS

indicates general instructions for safe operation.

5228-E P-(i)

INTRODUCTION

Thank you very much for choosing our NC system. This NC system is an expandable CNC with various features. Major features of the NC system are described below.

(1) Compact and highly reliable

The CNC system has become compact and highly reliable because of advanced hardware technology, including the computer boards equipped with high-speed microprocessors, I/O link, and servo link. The "variable software" as a technical philosophy of the OSPs supported by a flash memory. Functions may be added to the CNC system as required after delivery.

(2) NC operation panels

The following types of NC operation panels are offered to improve the user-friendliness.

• Thin color operation panels (horizontal)

• Thin color operation panels (vertical)

One or more of the above types may not be used for some models.

(3) Machining management functions

These functions contribute to the efficient operation of the CNC system and improve the profitability from small quantity production of multiple items and variable quantity production of variations. Major control functions are described below.

a. Reduction of setup time

With increase in small-volume production, machining data setting is more frequently needed. The simplified file operation facilitates such troublesome operation. The documents necessary for setup, such as work instructions, are displayed on the CNC system to eliminate the necessity of controlling drawings and further reduce the setup time.

b. Production Status Monitor

The progress and operation status can be checked on a real-time basis on the screen of the CNC system.

c. Reduction of troubleshooting time

Correct information is quickly available for troubleshooting.

(4) Help functions

When an alarm is raised, press the help key to view the content of the alarm. This helps take quick action against the alarm.

To operate the CNC system to its maximum performance, thoroughly read and understand this instruction manual before use. Keep this instruction manual at hand so that it will be available when you need a help.

Screens

Different screens are used for different models. Therefore, the screens used on your CNC system may differ from those shown in this manual.

5228-E P-(i)

TABLE OF CONTENTS

SECTION 1 PROGRAM CONFIGURATIONS .............................................................1

1. Program Types and Extensions............................................................................................... 1

2. Program Name ........................................................................................................................ 2

3. Sequence Name...................................................................................................................... 3

4. Program Format....................................................................................................................... 4

4-1. Word Configuration........................................................................................................... 4

4-2. Block Configuration .......................................................................................................... 4

4-3. Program............................................................................................................................ 5

4-4. Programmable Range of Address Characters.................................................................. 5

5. Mathematical Operation Functions.......................................................................................... 6

6. Optional Block Skip.................................................................................................................. 8

7. Program Branch Function (Optional) ....................................................................................... 9

8. Comment Function (Control OUT/IN) ...................................................................................... 9

9. Message Function (Optional)................................................................................................. 10

10.Operation Methods and Program Storage Memory Capacity ................................................ 10

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS .............13

1. Coordinate System ................................................................................................................ 13

1-1. Coordinate Systems and Values .................................................................................... 13

1-2. Machine Zero and Machine Coordinate System ............................................................ 13

1-3. Work Coordinate System................................................................................................ 14

1-4. Local Coordinate System ............................................................................................... 14

2. Coordinate Commands.......................................................................................................... 15

2-1. Numerically Controlled Axes .......................................................................................... 15

2-2. Unit Systems .................................................................................................................. 16

2-3. Travel Limit Commands (G22, G23) (Optional) .............................................................. 21

2-4. Home Position Command (G30) .................................................................................... 23

2-5. Absolute and Incremental Commands (G90, G91) ........................................................ 24

2-6. Coordinate Recalculation Command (G97).................................................................... 25

SECTION 3 FEED FUNCTIONS................................................................................26

1. Rapid Feed ............................................................................................................................ 26

2. Cutting Feed .......................................................................................................................... 26

2-1. Feed per Minute (G94) ................................................................................................... 26

2-2. Feed per Revolution (G95) ............................................................................................. 26

2-3. F1-digit Feed Function (Optional)................................................................................... 27

2-4. F0 Command During Cutting Feed................................................................................. 28

3. Exact Stop Check Function (G09, G61, G64)........................................................................ 29

4. Automatic Acceleration and Deceleration.............................................................................. 30

5228-E P-(ii)

TABLE OF CONTENTS

5. Following Error Check ........................................................................................................... 31

6. Positioning (G00)................................................................................................................... 32

7. Uni-directional Positioning (G60)........................................................................................... 33

8. Linear Interpolation (G01)...................................................................................................... 34

9. Plane Selection (G17, G18, G19) .......................................................................................... 35

10.Circular Interpolation (G02, G03)........................................................................................... 37

11.Helical Cutting (G02, G03) (Optional).................................................................................... 40

SECTION 4 PREPARATORY FUNCTIONS...............................................................41

1. Dwell Command (G04) .......................................................................................................... 41

2. Programmable Mirror Image (G62) (Optional)....................................................................... 42

3. Work Coordinate System Selection (G15, G16) .................................................................... 44

4. Work Coordinate System Change (G92) ............................................................................... 45

5. Unit System Check (G20, G21) (Optional) ............................................................................ 45

6. Coordinate System Conversion Functions ............................................................................ 46

6-1. Parallel Shift and Rotation of Coordinate Systems (G11, G10)...................................... 46

6-2. Copy Function (COPY, COPYE) .................................................................................... 48

7. Workpiece Geometry Enlargement / Reduction Function (G51, G50) (Optional).................. 50

SECTION 5 S, T, AND M FUNCTIONS .....................................................................52

1. S Code Function.................................................................................................................... 52

2. T Code Function .................................................................................................................... 52

3. M Code Function ................................................................................................................... 53

3-1. Examples of M Codes .................................................................................................... 53

SECTION 6 OFFSET FUNCTIONS...........................................................................56

1. Tool Length Offset Function (G53 - G59) .............................................................................. 56

2. Cutter Radius Compensation (G40, G41, G42)..................................................................... 57

2-1. Cutter Radius Compensation Function........................................................................... 57

2-2. Tool Movement in Start-up ............................................................................................. 59

2-3. Tool Movement in Cutter Radius Compensation Mode .................................................. 62

2-4. Tool Movement when Cutter Radius Compensation is Canceled .................................. 67

2-5. Changing Compensation Direction in Cutter Radius Compensation Mode .................... 71

2-6. Cutter Radius Compensation Type A ............................................................................. 74

2-7. Notes on Cutter Radius Compensation .......................................................................... 81

3. Cutter Radius Compensation Mode Override Function ......................................................... 90

3-1. Automatic Override at Corners ....................................................................................... 90

3-2. Circular Arc Inside Cutting Override ............................................................................... 92

4. Tool Radius Compensation G39 Command.......................................................................... 93

4-1. Parameter....................................................................................................................... 93

4-2. Corner Circular Interpolation .......................................................................................... 94

4-3. Corner Circular Interpolation Command Automatic Insertion ......................................... 96

5228-E P-(iii)

TABLE OF CONTENTS

5. Three-dimensional Tool Offset (G43, G44) (Optional)........................................................... 98

5-1. Three-dimensional Tool Offset Start-up ......................................................................... 98

5-2. Three-dimensional Tool Offset Vector............................................................................ 99

5-3. Canceling Three-dimensional Tool Offset .................................................................... 101

5-4. Actual Position Data Display And Feedrate.................................................................. 101

5-5. Relationship with Other G Functions ............................................................................ 102

5-6. Relationship to Other Tool Offset Functions................................................................. 102

SECTION 7 FIXED CYCLES ...................................................................................103

1. Table of Fixed Cycle Functions ........................................................................................... 104

2. Fixed Cycle Operations ....................................................................................................... 105

2-1. Determining the Positioning Plane and the Cycle Axis................................................. 106

2-2. Controlling the Return Level ......................................................................................... 107

2-3. Fixed Cycle Mode......................................................................................................... 107

2-4. Cycle Operation Conditions.......................................................................................... 108

3. General Rules for Programming Fixed Cycles .................................................................... 109

3-1. Programming Format (General Command Format) ..................................................... 109

3-2. Command Items Necessary for Fixed Cycle Function Commands .............................. 111

3-3. Absolute Programming Mode and Incremental Programming Mode............................ 112

3-4. Positional Relationship among Return Point Level, Point R Level and Point Z

Level ............................................................................................................................. 113

3-5. Axis Shift....................................................................................................................... 113

3-6. Z-axis G01 Mode Return Function ............................................................................... 114

3-7. Relationships between Fixed Cycle Functions and Other Functions ........................... 115

3-8. Notes for Programming a Fixed Cycle.......................................................................... 116

4. Specification of Return-point Level (G71)............................................................................ 117

5. High Speed Deep Hole Drilling Cycle (G73)........................................................................ 118

6. Reverse Tapping Cycle (G74) ............................................................................................. 119

7. Fine Boring (G76) ................................................................................................................ 120

8. Fixed Cycle Cancel (G80).................................................................................................... 121

9. Drilling Cycle (G81, G82).....................................................................................................122

10.Deep Hole Drilling Cycle (G83)............................................................................................ 123

11.Tapping Cycle (G84)............................................................................................................ 125

12.Boring Cycle (G85, G89) ..................................................................................................... 126

13.Boring Cycle (G86) .............................................................................................................. 127

14.Back Boring Cycle (G87) ..................................................................................................... 128

SECTION 8 COORDINATE CALCULATION FUNCTION (PATTERN FUNC-

TION) ...................................................................................................129

1. Table of Functions ............................................................................................................... 129

2. General Rules of Coordinate Calculation ............................................................................ 130

2-1. Programming Format for Coordinate Calculation ......................................................... 130

2-2. Plane on Which Coordinate Calculation is Performed, and Motion Axes..................... 132

5228-E P-(iv)

TABLE OF CONTENTS

2-3. Positioning at Calculated Pattern Points ...................................................................... 132

2-4. Others........................................................................................................................... 132

3. Omit (OMIT)......................................................................................................................... 133

4. Restart (RSTRT).................................................................................................................. 134

5. Line at Angle (LAA).............................................................................................................. 135

6. Grid (GRDX, GRDY)............................................................................................................ 136

7. Double Grid (DGRDX, DGRDY) .......................................................................................... 137

8. Square (SQRX, SQRY) ....................................................................................................... 139

9. Bolt Hole Circle (BHC)......................................................................................................... 141

10.Arc (ARC) ............................................................................................................................ 142

SECTION 9 AREA MACHINING FUNCTIONS........................................................143

1. List of Area Machining Functions......................................................................................... 143

2. Area Machining Operations ................................................................................................. 143

2-1. Basic Operations .......................................................................................................... 143

2-2. Tool Movements ........................................................................................................... 144

3. Area Machining Plane and Cycle Axis................................................................................. 146

4. General Rules...................................................................................................................... 147

4-1. Programming Format (General Command Format) ..................................................... 147

4-2. Area Machining Functions and Commands to be Used ............................................... 148

4-3. Data Entry in Incremental/Absolute Mode .................................................................... 149

4-4. Relationship among Present Point, Point R Level, and Finish Surface Level .............. 149

4-5. Definition of Machining Area (I, J) ................................................................................ 150

4-6. Notes on Area Machining ............................................................................................. 150

5. Face Milling Functions (FMILR, FMILF) .............................................................................. 151

6. Pocket Milling (PMIL, PMILR).............................................................................................. 156

6-1. Zigzag Pattern Pocket Milling Function (PMIL) ............................................................ 156

6-2. Spiral Pattern Pocket Milling Function (PMILR) ........................................................... 160

7. Round Milling Functions (RMILO, RMILI)............................................................................ 164

SECTION 10SUBPROGRAM FUNCTIONS.............................................................170

1. Overview.............................................................................................................................. 170

1-1. Calling a Subprogram................................................................................................... 170

2. Simple Call (CALL) .............................................................................................................. 173

3. Subprogram Call after Axis Movement (MODIN, MODOUT)............................................... 175

4. G and M Code Macro Functions.......................................................................................... 180

5. Program Call Function Using Variables............................................................................... 183

5-1. Outline .......................................................................................................................... 183

5-2. Program Call function by Variables .............................................................................. 183

5-3. Program Registration Function..................................................................................... 185

SECTION 11USER TASK.........................................................................................186

5228-E P-(v)

TABLE OF CONTENTS

1. User Task 1 ......................................................................................................................... 186

1-1. Branch Function ........................................................................................................... 186

1-2. Variable Function.......................................................................................................... 189

1-3. Math Functions ............................................................................................................. 195

1-4. System Variables.......................................................................................................... 196

2. User Task 2 ......................................................................................................................... 234

2-1. I/O Variables................................................................................................................. 234

2-2. Math Functions ............................................................................................................. 240

SECTION 12SCHEDULE PROGRAMS...................................................................243

1. Overview.............................................................................................................................. 243

2. PSELECT Block................................................................................................................... 244

3. Branch Block........................................................................................................................ 247

4. Variables Setting Block........................................................................................................ 248

5. Schedule Program End Block.............................................................................................. 248

SECTION 13OTHER FUNCTIONS..........................................................................249

1. Table Index Specification.....................................................................................................249

1-1. 5-Degree Index Commands ......................................................................................... 249

1-2. 1-Degree Index Commands ......................................................................................... 250

1-3. 0.001 Degree Commands (Optional)............................................................................ 252

2. Angular Commands............................................................................................................. 254

3. Manual Shift Amount Cancel Command.............................................................................. 255

4. Print Format Function .......................................................................................................... 258

SECTION 14FILE MANAGEMENT ..........................................................................259

1. Files ..................................................................................................................................... 259

2. Various Files........................................................................................................................ 260

SECTION 15APPENDIX ..........................................................................................261

1. G Code Table (Including Optional Functions)...................................................................... 261

2. Table of Mnemonic Codes (Including Optional Functions) .................................................. 265

3. M Code Table ...................................................................................................................... 268

4. Table of Reserved Local Variable Words ............................................................................ 277

5. Table of System Variables................................................................................................... 278

SECTION 1 PROGRAM CONFIGURATIONS

1. Program Types and Extensions

For OSP-E100M/E10M, four kinds of programs are used: schedule programs, main programs, subprograms, and library programs. The following briefly explains these four kinds of programs.

Schedule Program

When more than one type of workpiece is machined using a pallet changer or other loading and unloading equipment, multiple main programs are used. A schedule program is used to specify the order in which the main programs are executed and the number of times the individual main program is executed. Using a schedule program makes it possible to carry out untended operation easily. It is not necessary to assign a program name. The END code must be specified at the end of a schedule program. For details, refer to SECTION 12, “SCHEDULE PROGRAMS”.

Main Program

A main program contains a series of commands to machine one type of workpiece. Subprograms can be called from a main program to simplify programming. A main program begins with a program name which begins with address character “O” and ends with M02 or M30.

5228-E P-1

Subprogram

A subprogram can be called from a main program or another subprogram. There are two types of subprograms: those written and supplied by Okuma (maker subprogram), and those written by the customer (user subprogram). The program name, which must start with “O”, is required at the beginning of the subprogram. The RTS command must be specified at the end of the subprogram. For details, refer to SECTION 10, “SUBPROGRAM FUNCTIONS”.

Library Program

Subprograms and G code macros which are used frequently may be stored as library programs. Since library programs are automatically stored in the operation buffer area when the power is turned on, they can be accessed at any time. When a library program is stored in the operation buffer area, both a file name and an extension are stored. The file name format is shown below.

• Program file format

Main file name: Begins with alphabetic characters (max. 16 characters)

••• .

ExtensionMain file name

ME33018R1000300010001

• Extensions

SDF: Schedule program file MIN: Main program file MSB: Maker subprogram file SSB: System subprogram file SUB: User subprogram file LIB: Library program file

2. Program Name

All programs are assigned a program name or a program number, and a desired program can be called and executed by simply specifying the program name or number. A program name that contains only alphabetic characters is called a program label and the one that contains only numbers is called a program number. In this manual, both of them are referred to as a program name.

Program Name Designation

Enter letters of the alphabet (A to Z) or numbers (0 to 9) following address character “O”. Note

•

that no space is allowed between “O” and a letter of the alphabet or a number. Similarly, no space is allowed between letters of the alphabet and numbers.

• Up to four characters can be used.

• An alphabetic character can only be used in a program name if it begins with an alphabetic

character. Although a program beginning with an alphabetic character can contain a number in it, one that begins with a number cannot contain an alphabetic character.

• Although all of the four characters may be numeric, program names of the type “OO***” (***:

alphanumeric) cannot be used since this kind of program name is used for system operation, automating functions, etc.

5228-E P-2

SECTION 1 PROGRAM CONFIGURATIONS

• A block which contains a program name must not contain other commands.

• A program name may not be used for a schedule program.

• The program name assigned to a main program / subprogram must begin with address

character “O”.

• Since program names are handled in units of characters, the following names are judged to be

different program names.

• O0123 and O123

• O00 and O0

• All program names must be unique.

If program name “O1” is used for more than one program, the operation to call program “O1” may call a program differing from the desired one.

3. Sequence Name

All blocks in a program are assigned a sequence name that begins with address character “N” followed by an alphanumeric sequence. Functions such as a sequence search function, a sequence stop function and a branching function can be used for blocks assigned a sequence name. A sequence name that contains only alphabetic characters is called a sequence label and the one that contains only numbers is called a sequence number. In this manual, both of them are referred to as a sequence name.

Sequence Name Designation

Enter letters of the alphabet (A to Z) or numbers (0 to 9) following address character “N”.

•

• Up to five characters can be entered in succession to the address.

• Both alphabetic characters and numbers may be used in a sequence name. If an alphabetic

character is used in a sequence name, however, the sequence name must begin with an alphabetic character.

• Although a sequence name must be specified at the beginning of a block, an optional block skip

code may be placed before a sequence name.

5228-E P-3

SECTION 1 PROGRAM CONFIGURATIONS

• Sequence numbers may be specified in any order.

• Since sequence names are handled in units of characters, the following names are judged to be

different sequence names.

• N0123 and N123

• N00 and N0

• When a sequence label is used, place a space or a tab after the sequence label.

4. Program Format

4-1. Word Configuration

A word is defined as an address character followed by a group of numeric values, an expression, or a variable name. If a word consists of an expression or a variable, the address character must be followed by an equal sign “=”. Examples:

5228-E P-4

SECTION 1 PROGRAM CONFIGURATIONS

X - 100

Address Numeric value

Word

Y = 100∗SIN[50]

Address

• An address character is one of the alphabetic characters A through Z and defines the meaning

of the entry specified following it. In addition, an extended address character, consisting of two alphabetic characters, may also be used.

• Refer to SECTION 11, “Variable Function” for more information on variables.

• Hexadecimals may be used for numeric values.

Example: X#1000H (same as X4096)

4-2. Block Configuration

A group consisting of several words is called a block, and a block expresses a command. Blocks are delimited by an end of block code.

• The end of block code differs depending on the selected code system, lSO or EIA:

ISO: LF ElA: CR

• A block comprises several words.

Expression

Word

Z = VC1+VC2

Address

Variable

Word

ME33018R1000300040001

• A block may contain up to 158 characters.

A block consists of the following commands, for example.

N__ G__ X__ Y__ F__ S__ T__ M__

Feedrate

Sequence No.

Preparatory function

Coordinate values

Spindle speed

Tool No.

Miscellaneous function

ME33018R1000300050001

SECTION 1 PROGRAM CONFIGURATIONS

4-3. Program

A program consists of several blocks.

4-4. Programmable Range of Address Characters

The programmable ranges of numerical values of individual address characters are shown in the following table.

5228-E P-5

Address Function

O Program name 0000 - 9999 Same as metric

N Sequence name 00000 - 99999 Same as metric

G Preparatory function 0 - 399 Same as metric Mnemonics available

X, Y, Z, U, V, W

I, J, K

R Radius of arc ±99999.999mm ±9999.9999inch

A, B, C

S Spindle speed 0 - 65535 Same as metric

T Tool number 1 - 9999 Same as metric

Coordinate values

(linear axis)

Coordinate values of

center of arc

Coordinate values of

rotary axis

Feed per minute

Feed per revolution

Dwell time period 0.001 - 99999.999 sec Same as metric

Miscellaneous

function

Tool length offset

number

Cutter radius

compensation

number

Dwell time period

(during fixed cycle)

Second dwell time

period (during fixed

cycle)

Depth of cut (during

fixed cycle)

Repetition time

(schedule program)

Cut starting level

(during fixed cycle)

±99999.999mm ±9999.9999inch

±360.0000deg Same as metric

0.001 - 500.000

1 to maximum tool data

0.001 - 99999.999 sec Same as metric

±99999.999mm ±9999.9999inch

Programmable Range

Metric Inch

0.1 - 24000.0 mm/min

mm/rev

0 - 511 Same as metric

number

0 - 99999.999

1 - 9999 Same as metric

0.01 - 2400.00 inch/min

0.0001 - 50.0000 inch/rev

Same as metric

0 - 9999.9999inch

Alphabetic characters

specification

±9999.9999deg

Remarks

available

Multi-turn

*: An alarm occurs when any of the following addresses is specified more than once within a block:

X, Y, Z, U, V, W, A, B, C, F.

SECTION 1 PROGRAM CONFIGURATIONS

5. Mathematical Operation Functions

Mathematical operation functions are used to convey logical operations, arithmetic operations, and trigonometric functions. A table of the operation symbols is shown below. Operation functions can be used together with variables to control peripherals or to pass on the results of an operation.

Category Operation Operator Remarks

Exclusive OR EOR 0110 = 1010 EOR 1100 (See *3.)

Logical operation

Arithmetic operation

Trigonometric functions, etc.

Logical OR OR 1110 = 1010 OR 1100 (See *3.) Logical AND AND 1000 = 1010 AND 1100 (See *3.) Negation NOT 1010 = NOT 0101 Addition + 8 = 5 + 3 Subtraction - 2 = 5 - 3 Multiplication * 15 = 5 * 3 Division / (slash) 3 = 15/5 Sine SIN 0.5 = SIN [30] (See *4.) Cosine COS 0.5 = COS [60] (See *4.) Tangent TAN 1 = TAN [45] (See *4.) Arctangent (1) ATAN 45 = ATAN [1] (value range: -90° to 90°) Arctangent (2) ATAN2 30 = ATAN 2 [1,(Square root 3)] (See *1.) Square root SQRT 4 = SQRT [16] Absolute value ABS 3 = ABS [-3] Decimal to

hexadecimal conversion

Hexadecimal to decimal conversion

Integer implementation (rounding)

Integer implementation (truncation)

Integer implementation (raising)

Unit integer implementation (rounding)

Unit integer implementation (truncation)

Unit integer implementation (raising)

Remainder MOD 2 = MOD [17, 5]

BIN 25 = BIN [$25]

($ represents a hexadecimal number.)

BCD $25 = BCD [25]

ROUND 128 = ROUND [1.2763 x 102]

FIX 127 = FIX [1.2763 x 102]

FUP 128 = FUP [1.2763 x 102]

DROUND 13.265 = DROUND [13.26462] (See *2.)

DFlX 13.264 = DFlX [13.26462] (See *2.)

DFUP 13.265 = DFUP [13.26462] (See *2.)

5228-E P-6

SECTION 1 PROGRAM CONFIGURATIONS

Category Operation Operator Remarks

Brackets

*1. The value of ATAN2 [b, a] is an argument (range: -180° to 180°) of the point that is expressed

*2. In this example, the setting unit is mm. *3. Blanks must be placed before and after the logical operation symbols (EOR, OR, AND, NOT). *4. Numbers after function operation symbols (SIN, COS, TAN, etc.) must be enclosed in

Opening bracket [ Determines the order of calculation. Closing bracket ]

by coordinate values (a, b).

brackets “[ ]”. ( “a”, “b”, and “c” are used to indicate the contents of the corresponding bits.)

(Expression in inner brackets is calculated first.)

Logical Operations

Exclusive OR (EOR) c = a EOR b

•

If the two corresponding values agree, EOR outputs 0. If the two values do not agree, EOR outputs 1.

abc

000 011 101 110

5228-E P-7

• Logical OR (OR) c = a OR b

If both corresponding values are 0, OR outputs 0. If not, OR outputs 1.

abc

000 011 101 111

• Logical AND (AND) c = a AND b

If both corresponding values are 1, AND outputs 1. If not, AND outputs 0.

abc

000 010 100 111

• Negation (NOT) b = NOT a

NOT inverts the value (from 0 to 1, and 1 to 0).

01 10

• Arc tangent (1) (ATAN)

θ = ATAN [b/a]

Arc tangent (2) (ATAN2)

θ = ATAN2 [b/a]

• Integer implementation (ROUND, FIX, FUP)

Converts a specified value into an integer (in units of microns) by rounding off, truncating, or raising the number at the first place to the right of the decimal point.

6. Optional Block Skip

5228-E P-8

SECTION 1 PROGRAM CONFIGURATIONS

ME33018R1000300080001

[Function] Blocks preceded by “/n” are ignored in automatic operation mode if the BLOCK SKIP switch on the machine panel is set ON. If the switch is OFF, these blocks are executed normally. The optional block skip function allows an operator to determine if a specific block should be executed or ignored in automatic mode operation. When the block skip function is called, the entire block will be ignored. [Details]

• In the standard specification, one optional block skip can be specified; as an option, up to nine

are possible. These are distinguished in code as follows: “/1”, “/2”, “/3”. Note that “/” has the same meaning as “/1” when this option is selected.

• A slash code “/” must be placed at the start of a block. If it is placed in the middle of a block, an

alarm is activated. A sequence name may precede a slash code “/”.

• A slash code “/” may not be contained in the program name block.

• Blocks which contain a slash code “/” are also subjected to the sequence search function,

regardless of the BLOCK SKIP switch position.

• Sequence stop is not executed at a block which contains a slash code “/” in single block mode

operation if the BLOCK SKIP switch is ON. The succeeding block is executed, and then the operation stops.

• This function is also available in the schedule program.

SECTION 1 PROGRAM CONFIGURATIONS

7. Program Branch Function (Optional)

[Function] The program branch function executes or ignores the program branch command specified in a part program according to the ON/OFF setting of the PROGRAM BRANCH switch on the machine panel. The function corresponds to maximum two program branch switches, PROGRAM BRANCH 1 and PROGRAM BRANCH 2 (extended to maximum nine switches by additional option). If the switch is ON, the program branches when the following command is read.

• IF VPBR1 N*** The program branches to N*** block if the PROGRAM BRANCH 1 switch is

ON.

• IF VPBR2 N*** The program branches to N*** block if the PROGRAM BRANCH 2 switch is

ON.

Example:

5228-E P-9

IF VPBR1 N100

G00 X100 Z100 G00 Y100N100

IF VPBR1 N200

G00 X200 Z200 G00 Y200

N200

M02

Branching to N100 if PROGRAM BRANCH 1 switch is ON.

Branching to N200 if PROGRAM BRANCH 2 switch is ON.

[Details]

• In operation method B (large-volume program operation mode), use a sequence label name to

specify the branch destination.

• The program branch function has the same restrictions as the branch function of User Task 1.

• A program branch command (IF VPBR1 N*** or IF VPBR2 N***) must be specified in a block

without other commands.

8. Comment Function (Control OUT/IN)

A program may be made easier to understand by using comments in parentheses.

ME33018R1000300100001

• A comment must be parenthesized to distinguish it from general operation information. All

information placed in parentheses is regarded by the machine as comments.

• Comments are displayed in the normal character size.

Example:

N100 G00 X200 (FIRST STEP)

Comment

ME33018R1000300110001

9. Message Function (Optional)

[Function] For conditional branching it may be necessary to display a message, depending on the processing at the destination of the branching. The message function is used in such cases, and the message is displayed in enlarged characters. [Format] MSG (message statement) [Details]

• The display of a message statement on the screen is twice the size of normal characters.

• If the MSG code is not followed by a message statement, the comment statement given last up

to the present block will be displayed.

• Up to 128 characters may be used in a message statement.

• The message function is possible only during machine operation mode.

• The following code can be used in the program to return the screen to he previous status after

the message has been displayed: NMSG

5228-E P-10

SECTION 1 PROGRAM CONFIGURATIONS

10. Operation Methods and Program Storage Memory Capacity

(1) Operation Capacity

The NC has a memory to store machining programs. The memory capacity is selected depending on the size of the user program. On execution of a program, the program is transferred from the memory to the operation buffer (RAM). If the program size is larger than the operation buffer capacity, (for example, if the program size is larger than 320 m (1050 ft.) although the operation buffer capacity is 320 m (1050 ft.)), the program cannot be transferred from the memory to the operation buffer in batch (at one time). Depending on the size of a program in comparison to the operation buffer capacity, two types of operation methods are available (operation method A and operation method B), and restrictions apply in programming according to the operation method used.

Machining program Memory

Program selection

Operation buffer

(RAM)

Operation

ME33018R1000300130001

5228-E P-11

SECTION 1 PROGRAM CONFIGURATIONS

(2) Operation Methods

Select the operation method using the pop-up window MAIN PROGRAM SELECT (MEMORY MODE) that appears when calling a program to be run. The operation method can be also selected by the setting at the NC optional parameter (word) No. 11.

ME33018R1000300130002

• When A-Mtd is selected

Program running method A becomes effective. The program to be executed is transferred to the operation buffer in batch. This method is used when the program is smaller than the operation buffer capacity.

• When B-Mtd is selected

Program running method B becomes effective. The program to be executed is called to the operation buffer in several segments. This method is used when the program is larger than the operation buffer capacity. Since schedule programs, subprograms, and library programs are generally called to the operation buffer in batch, these programs must be created with restriction placed on their capacities.

• When S-Mtd is selected

Program running method S becomes effective. This method is used to execute a large program which does not use branch or subprogram call functions.

5228-E P-12

SECTION 1 PROGRAM CONFIGURATIONS

• When selecting an operation method, also select the program size and whether the

program has a sub program branch or not (only in the case of operation A and B). The table below shows the relation between the operation method and the program size.

Item

Program running method Method A Method B Method S

Main program Sub program

Program size limit

Sub program function Usable Usable Unusable (alarm) Branch function Usable Usable Unusable (alarm)

Destination of a jump specified in branch command

Main program sequence label limit

Program selection time *1 *1 Completed immediately

Library program

Schedule program

Main program Sub program Library

program Schedule

program

Program of normal

size

Total program size is 2MB.

Sequence label or sequence number

Unlimited Unlimited Unlimited

Large program

2GB

Total program size is about 1.8 MB.

Sequence label or sequence number

Total program size is about 1.8 MB.

*1. Time varies with the selected program size.

(3) Programming Restrictions for the Operation Method

For details of restrictions that must be taken into consideration when writing a program, refer to SECTION 12, “PSELECT BLOCK”.

(4) Others

• The maximum capacity for running the main program is about 2 GB when the operation

method B is selected.

• The library program capacity is equivalent to the designated library program buffer size.

This means that the library program buffer size is always contained in the operation capacity even if a library program is not registered.

• The number of subprograms and library programs stored in memory is independent of the

operation buffer size. They are always 126 and 65, respectively.

5228-E P-13

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

SECTION 2 COORDINATE SYSTEMS AND COORDI-

NATE COMMANDS

1. Coordinate System

1-1. Coordinate Systems and Values

In order to move a cutting tool to a target position, a coordinate system must be established to specify the target position using coordinate values in the coordinate system. The OSP-P200M uses three types of coordinate system (machine coordinate system, work coordinate system, and local coordinate system). These coordinate systems are briefly explained below.

• Machine coordinate system

The machine coordinate system is set by the machine tool manufactures. Although the setting may be changed by the user, machine dependent setting values such as pitch error compensation data and travel limit values must be changed accordingly.

• Work coordinate system

A work coordinate system is set by the user.

• Local coordinate system

A local coordinate system set temporarily by the commands in a program. The user can select the coordinate system to be used as needed from the coordinate systems indicated above. The coordinate value is represented by components of the axes which make up the coordinate system. Usually, a maximum of six axis components is used (the number differs depending on the NC unit specifications.) Example:

X__Y__Z__W__A__C__

The number of programmable axes, that is, the number of axis components used to define a coordinate value varies depending on the machine specifications. This manual, therefore, uses the following designation to indicate a coordinate value. IP__

1-2. Machine Zero and Machine Coordinate System

The reference point specific to the individual machine is referred to as the machine zero and the coordinate system having the machine zero as the origin is referred to as the machine coordinate system. The machine zero is set for each individual machine using system parameters. Since the travel end limits and the home positions are set in the machine coordinate system, the user should not change the location of the machine zero at his/her own discretion. A cutting tool may not always be moved to the machine zero.

ME33018R1000400010001

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

1-3. Work Coordinate System

The coordinate system used to machine workpieces is referred to as the work coordinate system.

• Work coordinate systems are established and stored with work coordinate system numbers in

the memory before starting operation. The desired work coordinate system may be called at the start of machining.

• Work coordinate systems are set by specifying the distance from the machine zero to the origin

of a work coordinate system as an offset value (work zero offset).

• For details, see SECTION 4, “Selection of Work Coordinate System” and SECTION 4, “Change

of Work Coordinate System”.

1-4. Local Coordinate System

Programming the entire operation of a workpiece using only a work coordinate system may sometimes be difficult on some portions of the workpiece. In such cases, programming is facilitated by setting a new coordinate system appropriate for a specific workpiece portion. The new coordinate system is referred to as a local coordinate system.

5228-E P-14

• The desired local coordinate system can be established by specifying the origin in reference to

the origin of the presently selected work coordinate system and the angle of rotation on the specified plane about the origin of the local coordinate system to be set with G11. Once a local coordinate system has been established, all coordinate values are executed in the newly set local coordinate system. To change the local coordinate system to another one, the position of the origin of the new local coordinate system and the angle of rotation about the origin should be specified with G11. As explained above, a local coordinate system can be established only by specifying the coordinate values of the origin and the angle of rotation in a program.

• To designate coordinate values in the work coordinate system, cancel the local coordinate

system by specifying G10.

• For details, refer to SECTION 4, “Parallel Shift and Rotation of Coordinates System”.

Coordinate system parallel shift amount (Specified in a program)

Work zero offset amount (Set by zero point data)

Machine zero offset amount (Set by system parameter)

Rotating angle of local coordinate system

Local coordinate system zero point

Work coordinate system zero point

Machine zero

Zero point for position encoder

ME33018R1000400040001

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

2. Coordinate Commands

2-1. Numerically Controlled Axes

• The following table lists the addresses to be specified to control the axes.

Address Contents

Basic axis X, Y, Z

Parallel axis U, V, W

Rotary axis A, B, C

Circular

interpolation

parameters

• An axis movement command consists of an axis address, a sign indicating the direction of the

axis movement, and a numeric value which describes the axis movement. Refer to “Absolute and Incremental Commands” for the designation of numeric values.

l, J, K

R Addresses specifying the radius of an arc

5228-E P-15

Addresses corresponding to the three axes orthogonal to one another

Addresses of three orthogonal axes parallel to the basic axes

Addresses of rotary axis in a plane right angle to the basic axis

Addresses specifying distances, parallel to an individual axis, from a start point to the center of an arc

• In this manual, to simplify the explanation for axis designation, “Xp”, “Yp”, and “Zp” are used

instead of the actual axis addresses. They represent the axis as follows: Xp X-axis and the axis parallel to X-axis (U-axis) Yp Y-axis and the axis parallel to Y-axis (V-axis) Zp Z-axis and the axis parallel to Z-axis (W-axis)

• The maximum number of controllable axes is six. This capability varies depending on the NC

model.

• The following table shows the number of simultaneously controllable axes in each of the axis

movement modes.

Number of Simultaneously Controllable Axes

(“n” represents the number of controllable axes.)

Positioning n

Linear interpolation n

Circular interpolation 2

Helical cutting 3

Manual operation 1

Pulse handle operation 1

In pulse handle operation, the optional 3-axis control function is available.

• The positive directions of the linear and rotary axes are defined as follows:

The definition of the coordinate axes and directions conforms to ISO R841. ISO: International Organization of Standardization

2-2. Unit Systems

The unit systems that can be used in a program are described below. Note that the unit system selected for programming and the unit system used for setting data such as zero point, tool data, and parameters are independent of each other. The unit systems to be used for inputting the data are set at NC optional parameter (INPUT UNIT SYSTEM).

5228-E P-16

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

ME33018R1000400050001

2-2-1. Minimum Input Unit

The minimum input unit is the smallest unit of a value that may be entered in a program. For a linear axis, the minimum input unit is 0.001 mm or 0.0001 inch. For the NC with metric / inch switchable specification, the unit system can be selected by the setting at LENGTH UNIT SYSTEM of NC optional parameter (INPUT UNIT SYSTEM). For a rotary axis, the minimum input unit is 0.001 degree or 0.0001 degree. Either 0.001 degree or

0.0001 degree can be selected by the setting at ANGLE of NC optional parameter (INPUT UNIT SYSTEM).

2-2-2. Basic Input Unit

The input unit may be changed to the “basic” unit by the setting at LENGTH of NC optional parameter (INPUT UNIT SYSTEM). The fundamental units are then 1 mm, 1 inch, 1 degree, and 1 second.

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

2-2-3. Numeric Values (inch / metric switchable as optional function)

As the unit for specifying program values, “mm”, “deg.”, “sec”, etc. are used. For these units, a decimal point may be used.

• Cautions on using a decimal point value

a. A decimal point value must not be used for addresses O, N, G, and M.

b. If a decimal point is not entered in a numeric value, the decimal point is assumed to exist at

the end of the specified numeric value.

c. If a value is set below the specified minimum input unit, the data is processed in the

following manner.

• For addresses S, T, H, D, Q, etc. that require integer type data, the value below the

minimum input unit is truncated.

• For addresses that use real data, the value below the minimum input unit is rounded.

• The input unit of dimension commands is determined by the setting at NC optional parameter

(INPUT UNIT SYSTEM) or NC optional parameter (bit) No. 3, bit 0 to bit 7 and No. 4, bit 0. How these bits set the input unit is shown below.

5228-E P-17

• NC optional parameter (INPUT UNIT SYSTEM) screen

ME33018R1000400090001

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

• NC optional parameter (bit) No. 3, bit 0 to bit 7 and No. 4, bit 0

5228-E P-18

Parameter

No.

Bit

No.

Sets the unit system of length, “inch” or “mm”.

(*2)

1 Sets the unit of 1 mm, 1 inch, 1 deg., and 1 sec.

2 Sets unit of length, “0.01 mm” or “0.001 mm”. 0.01 mm 0.001 mm

Sets the unit of feedrate, 0.1 mm/min, 0.01

inch/min, or 1 mm/min, 0.1 inch/min Sets the unit of feedrate, 0.001 mm/rev, 0.0001

inch/rev, or 0.01 mm/rev, 0.001 inch/rev

5 Sets the unit of time, “0.01 sec” or “0.1 sec”. 0.01 sec 0.1 sec

Sets the unit place at “1 mm”, “1 inch”, “1 deg”,

and “1 sec” when decimal point input is selected.

7 Sets the unit time, “0.001 sec” or “0.1 sec”.(*1) 0.001 sec 0.1 sec

Sets the unit of angle, “0.001 deg” or “0.0001 deg”.

Contents

With

Check Mark

inch mm

Unit of 1 mm,

1 inch, 1 deg.,

and 1 sec is

selected.

0.1 mm/min

0.01 inch/min

0.001 mm/rev

0.0001 inch/rev

Unit place is set

at “1 mm”,

“1 inch”,

“1 deg”, and

“1 sec”.

0.0001 deg 0.001 deg

Without

Check Mark

Conforms to the

setting for bit 2

to bit 5 and bit 7

of No. 3 and bit

0 of No. 4.

1 mm/min

0.1 inch/min

0.01 mm/rev

0.001 inch/rev

Conforms to the

setting for bit 1 to bit 5, and bit

*1: The unit of time is always “0.01 sec” if “1” is set for bit 5. *2: The setting for bit 0 is valid only when the inch/mm switchable specification is selected.

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

• Examples of parameter setting are given below.

(●: With check mark, O: Without check mark)

• mm system

• inch system

5228-E P-19

ME33018R1000400090002

ME33018R1000400090003

An asterisk (*) in the table indicates setting of “0” or “1” is allowed.

• µm / mm unit system

The unit system that handles the data in units of mm (inch) for real data and in units of microns (1/10000 inch) is called the “µm / mm unit system”. For this unit system, the unit is determined depending on whether or not a decimal point is used in the data when YES is selected at REAL NUMBER of NC optional parameter (INPUT UNIT SYSTEM). If a decimal point is used, the unit of “mm (inch)” is set and if a decimal point is not used, the unit of “microns (1/10000 inch)” is set. Example 1:

X100. X100

If an expression or a variable is used for the command of this unit system, the values are always treated as real data. Example 2: Local variables

PX 100=

100mm 100µm

PX=X

100mm

PX 100.=

ME33018R1000400090004

PX=X

100mm

ME33018R1000400090005

(The value is not “100 µm”.)

5228-E P-20

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

The following is a comparison how a numeric value is interpreted according to whether or not a decimal point is used when “µm / mm unit system” is selected.

Command Element Value

X 100 100 µm– X= 100 100 µm– X 100. 100 mm Decimal point X= 100. 100 mm Decimal point X 100+100 200 mm Expression X= 100.+100 200 mm Expression X= 100+100. 200 mm Expression X 100+100*2 300 mm Expression X= 100+100*2 300 mm Expression X= 100+100*2.5 350 mm Expression PK= 100 X= 100+PK PK= 100. X= 200-PK X= 200-100 100 mm Expression X -100 -100 µm– X -100. -100 mm Decimal point X +100 100 µm– X +100. 100 mm Decimal point X= ROUND[100] 100 mm (*1) Expression X= FIX[100.] 100 mm (*1) Expression X= FUP[-100] -100 mm (*1) Expression X= ROUND[100.] 100 µm (*2) – X= FIX[100.] 100 µm (*2) – X= FUP[-100.] -100 µm (*2) –

200 mm Variable

100 mm Variable

“mm unit system”

element

LA1=4 F=FIX[LA1] 4 mm/min

Variable

(*1) Decimal point is selected for designation of ROUND/FIX/FUP real number command. (*2) Integer is selected for designation of ROUND/FIX/FUP real number command.

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

2-3. Travel Limit Commands (G22, G23) (Optional)

Since the NC is equipped with absolute position encoders, it is possible to set the travel limit with the software. That is, if the travel limit is set as an absolute value by the software, the limit switch usually used to detect the travel limit may not be used. If the travel limit is set in this manner, it is possible to change the travel limit position by changing the travel limit value in a program. Note that two types of travel limit, one set by the manufacture (factory-set travel limit) and the other set by the user (user-set travel limit), are provided.

(1) Factory-Set Travel Limit (Soft-Limit)

• The travel limit is set in accordance with the maximum travel distance from the machine

zero of each axis. The travel limits are set both in the positive (P) and negative (N) directions using the system parameters.

• The area inside of the set values (from the N direction travel limit to the P direction travel

limit) is available for operation (operation permitted area). The outside area is called the operation inhibited area and axis movements into this area are not allowed.

• The travel limit function always monitors the programmed tool path. If the tool path enters

the operation inhibited area, even if the end point lies in the operation permitted area, this function disables the tool movement.

5228-E P-21

Operation inhibited area

End point

Start point

ME33018R1000400100001

(2) User-Set Travel Limit (Programmable Limit) (Optional)

The travel limit may be set by the user either with user parameters or by programs using the programmable travel limit function. Since both settings (user parameter and programmed command) establish an identical area and since the data is stored in the same area, the data entered last becomes the valid data, updating the previously set data. For example, when the travel limits are set using a program after setting them with the user parameters, the travel limit setting data is replaced with the data set for the user parameters. When setting the travel limits, both positive (P) and negative (N) direction limit data must be set. The area between the P and N travel limits is defined as the operation permitted area and that outside the travel limits is defined as the operation inhibited area.

5228-E P-22

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

• Setting the travel limits by a program

[Programming format]

G22 X__Y__Z__α__β__γ__I__J__K__P__Q__R__

...........

The numeric values entered are processed as coordinate values in the work coordinate system. “α”, “β”, and “γ” above do not represent an address. In actual programming, use axis addresses of the 4th to 6th axis (A, B, C, U, V, and W).

X Programmable limit in the P direction of X-axis Y Programmable limit in the P direction of Y-axis Z Programmable limit in the P direction of Z-axis

α Programmable limit in the P direction of 4th-axis β Programmable limit in the P direction of 5th-axis γ Programmable limit in the P direction of 6th-axis

I Programmable limit in the N direction of X-axis J Programmable limit in the N direction of Y-axis K Programmable limit in the N direction of Z-axis P Programmable limit in the N direction of 4th-axis Q Programmable limit in the N direction of 5th-axis R Programmable limit in the N direction of 6th-axis

ME33018R1000400100002

[Details]

• An alarm occurs if the command indicated above is executed for the machine equipped with a

multi-turn type rotary axis.

• The data set using G22 is backed up and is therefore valid even after the power is turned off.

• If the setting data is outside the factory-set soft limits, an alarm will occur.

• Which of the travel limits - the limits set with the system parameters (soft-limit) or the limits set

with user parameters or by a program (programmable limits) - becomes valid as the operation permitted area can be set by specifying an appropriate G code. G22: Selects the travel limits set with user parameters or those newly set by G22 are as the travel limits and checks the program according to the selected operation permitted area. G23: Cancels the G22 mode and selects the travel limits set with the system parameters. The program is checked according to the selected operation permitted area. If G22 is specified independently, the programmable limit values set with user parameters become valid.

• For setting the travel limits with user parameters, refer to User Parameter, SECTION 4

PARAMETER in III DATA OPERATION of OPERATION MANUAL.

• The programmed tool path is checked for entry into the operation inhibited area even if the end

point lies inside the operation permitted area.

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

2-4. Home Position Command (G30)

[Function] The term “home position” refers to a particular position that can be set for individual machines. The home position command is used to move the axes to the preset home position. The home position is used as the tool change position or the pallet change position. [Programming format] G30 P__ P: Home position number. Up to 32 home positions may be set. Home positions are set with coordinate values in the machine coordinate system using system parameters.

[Supplement]

The operating sequence of the axes to move to the home position and the position of the home position are determined by the machine tool builder and differ according to machine. Before operating the machine, you must thoroughly understand the axis operating sequence and the position of the home position for each home position number. For details on home positions, refer to SECTION 4 PARAMETER in III DATA OPERATION of OPERATION MANUAL.

5228-E P-23

How the individual axes move to the home position is determined according to the setting for NC optional parameter (bit) No. 46, bit 2, whether the path is generated along a straight line (linear interpolation mode) or not.

[Supplement]

After the execution of a home position command, it is necessary to execute positioning for all axes in the G90 mode (absolute command) before starting the next operation.

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

2-5. Absolute and Incremental Commands (G90, G91)

For the designation of axis movement distance, two types of commands (absolute commands, incremental commands) are available.

(1) Absolute Commands

G90 specifies the absolute dimensioning mode. In this mode, the coordinate values in the selected work coordinate system are used to specify the movement of axes.

(2) Incremental Commands

G91 specifies the incremental dimensioning mode. In this mode, the axis movement distance from the current position to the target position is used to specify the movement of axes. [Details]

• It is not permissible to specify G90 and G91 in the same block.

• Either G90 or G91 is always valid.

• Which of G90 and G91 is made valid when the power is turned ON or when the NC is reset

is determined by the setting for a parameter (NC optional parameter (bit) No. 18, bit 4).

5228-E P-24

• When an incremental command needs to be designated right after the completion of a

fixed cycle, specify the movement of the cycle axis of the fixed cycle in the absolute mode before specifying incremental commands.

G81 X_Y_Z_R_F_

X_Y_

•

X_Y_ G80 G00 Z_ G91 X_Y_Z_

•

ME33018R1000400120001

• After executing a command such as G15, G16, or G92 that changes a coordinate system,

it is necessary to execute positioning in the G90 mode for all axes. (After changing the coordinate system, a coordinate system must be established using absolute commands.)

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

2-6. Coordinate Recalculation Command (G97)

[Function] After changing the home position (G30) or the coordinate system (G15, G16, G92, etc.), it is usually necessary to issue G90 (absolute command) to position each axis (to define the coordinates). The coordinate recalculation command eliminates such need. [Programming format] G97

[Supplement]

1) G97 is effective only in one block.

2) G97 cannot be specified with an axis movement command in the same block. If attempted, an alarm occurs.

5228-E P-25

SECTION 3 FEED FUNCTIONS

1. Rapid Feed

In the rapid feed mode, each of the axes moves at the specified rapid feedrate independently of other axes that are moved at the same time. Note that rapid feedrate differs depending on the machine specification. Consequently, the individual axes arrive at the target point at different times. Override is possible.

2. Cutting Feed

2-1. Feed per Minute (G94)

[Function] This function sets the feedrate per minute of a cutting tool with a numeric value following address “F”. [Programming format] G94 Setting unit: Selection is possible from among 1 mm/min, 0.1 mm/min, 1 inch/min, 0.1 inch/min and 0.01 inch/min by setting NC optional parameter (INPUT UNIT SYSTEM). Setting range: 0.1 ~ 24000.0 mm/min, 0.01 ~ 2400.00 inch/min [Details]

5228-E P-26

SECTION 3 FEED FUNCTIONS

• The allowable maximum feedrate that is called the “clamp feedrate” is set with NC optional

parameter (long word) No. 10. If an axis is going to move beyond this limit, its feedrate is clamped at this clamp feedrate and the following alarm message is displayed at the alarm display line on the screen. 4204 ALARM-D Feedrate command limit over (replacing)

• The programmed feedrate can be overridden. The clamp feedrate is applied to the actual

feedrate, or the overridden feedrate.

2-2. Feed per Revolution (G95)

[Function] This function sets the feedrate per revolution of a cutting tool with a numeric value following address “F”. [Programming format] G95 Setting unit: Selection is possible from among l mm/rev, 0.01 mm/rev, 0.001 mm/rev, 1 inch/rev, 0.001 inch/rev or

0.0001 inch/rev by setting NC optional parameter (INPUT UNIT SYSTEM). Setting range:0.001 ~ 500.000 mm/rev, 0.0001 ~ 50.000 inch [Details]

• Since the clamp feedrate is set in units of “mm/min” it is converted into a value in “mm/rev” units

using the following formula: fm = fr × N where, N = spindle speed (rpm) fm = feedrate (mm/min) fr = feedrate (mm/rev)

2-3. F1-digit Feed Function (Optional)

The F1-digit feed function has two types of control: Switch-type control: In a program, feedrate commands are written with F1 to F8 and the actual feedrate is set with the corresponding setting switches (up to 8 sets) provided on the machine operation panel. Parameter-type control: The feedrate commands are written in a program in the same manner as with the switch-type control. Actual feedrates are set for 9 sets of parameters F1 through F9. For details of feedrate setting procedure for the parameter-type control, refer to the SECTION 11 F1digit Feed Command Function in Special Functions Manual.

• F1-digit feed designation is distinguished from F4-digit feed designation as follows.

5228-E P-27

SECTION 3 FEED FUNCTIONS

(1) F1-digit Feed

Switch-type control: An integer in the range of 1 to 8 Parameter-type control: An integer in the range of 1 to 9

(2) F4-digit Feed

If a real number (including a variable) is specified following address F (F1. for example), the feedrate command is interpreted as an F4-digit command. Therefore, for the F1-digit feed function, a variable cannot be used to specify 1 to 8 (for switch-type control) or 1 to 9 (for parameter-type control). Examples:

F1 F5.

LA1 = 8

F = LA1

The feedrate is determined by the setting of rotary switch F1. Feedrate = 5 mm/min

Feedrate = 8 mm/min

ME33018R1000500040001

• The selected feedrate code (F1 to F8 in the case of switch-type control and F1 to F9 in the

case of parameter-type control) is not cleared even when the NC is reset. It is cleared if an F4-digit command is specified or when power is turned OFF and then back ON.

• A feedrate override setting is invalid if a feedrate is specified by an F1-digit feedrate

command.

• If an F1-digit feedrate command is specified in the G95 mode (feed per revolution), an

alarm occurs.

2-4. F0 Command During Cutting Feed

F0 commands during the cutting feed are activated. When "F0", "F0.0", or "F0." is specified, the NC operates considering the setting value of the optional parameter long word No. 62 as an F command value. Specified F0 command is activated in the succeeding cutting blocks.

• If F0 commands are inactivated, the following alarm appears. "2244 ALARM-B Data word: 'F' 2"

Even if F0 commands are activated, an alarm appears as the current condition in the feed per revolution mode.

• If [F0], [F0.], or [F0.0] is specified in a block of cutting feed command (including in the NURBS

mode, excluding synchronized tapping command), the value of the optional parameter long word No.62 is adopted as the F value of the command. However, F0 commands are available other than when specifying F commands directly.

• Not only X-, Y-, and Z-axes, commands are issued to the same block, regardless of whether W-

axis command is specified. Since the upper-limit speed of the W axis is considerably low compared to the basic axes, if a command is specified at the same time as the basic axes, the following alarm appears. "ALARM-A CON speed over" (Same as usual.) If this alarm occurs, set a lower value to the setting value of the optional parameter long word No.62

5228-E P-28

SECTION 3 FEED FUNCTIONS

• The speed is clamped at the upper limit feedrate (in the Super NURBS control parameter). If a

desired speed cannot be achieved due to the upper limit feedrate, change the upper limit feedrate.

• The speed is changed by the cutting feed override.

However, when the setting value of the optional parameter long word No.62 is 10 m/min, the override is clamped at 10 m/min by the maximum feedrate value or upper limit feedrate even if the override is set 100 % or more.

a. Optional parameter long word

No. Description Details

Feedrate value when

specifying F0 command

Set an F command value for the case when the F0 is specified. The setting is allowed up to 10 m/min. If the setting value is "0", the initial value 10 m/min is automatically set on the initialization.

b. Optional parameter bit

NO. Bit Description

78 1 F0 command is not set as an

alarm.

Range 0 to 10000000 Initial value 10,000,000 Unit µm/min

Not set as alarm

Set as alarm (Initial value)

This parameter is not effective when turning on the power.

SECTION 3 FEED FUNCTIONS

3. Exact Stop Check Function (G09, G61, G64)

[Function]

• During axis feed control, the calculated value always precedes the actual value when an axis is

moving to the target point. Therefore, if the calculated value is at the target point, the actual value is behind the calculated value and is not at the target position. If the next block is executed at the time the calculated value reaches the target point, the actual position follows the calculated value, causing the tool path to stray from the programmed path at the join between two blocks.

• The exact stop function successfully eliminates errors caused by the axis control indicated

above. With the exact stop function, operation for the next block does not start until the actual value arrives at the target point even if the operation of the current block has completed, so that the tool path exactly follows the programmed path. The state where the current position has reached the target point is referred to as the “inposition” state. To establish the in-position state, the target point is defined with a band that is set using a system parameter.

Calculated value

5228-E P-29

Actual valu

ME33018R1000500060001

• The exact stop check mode may be either one-shot (valid only for a programmed block) or

modal, as explained in the following. Note that in the positioning mode (G00, G60), an exact stop check is always executed regardless of whether or not an exact stop check G code is specified.

[Programming format]

• One-shot exact stop check command: G09 IP

Exact stop check is executed only in the specified block.

• Modal exact stop check command: G61 IP__

Exact stop check is executed for all blocks until a cutting mode (G64) is specified.

• Cutting mode (cancel G61): G64 IP__

At a join between blocks containing cutting commands, the commands in the next block are executed immediately so that axis movements will not be decelerated at the join. Even in the cutting mode, however, an exact stop check is executed in the positioning mode (G00, G60) or in a block containing the one-shot exact stop command (G09). An exact stop check is also executed at blocks where cutting feed does not continue.

SECTION 3 FEED FUNCTIONS

4. Automatic Acceleration and Deceleration

At the start and end of axis movements, axis feedrate is automatically accelerated and decelerated.

(1) Automatic Acceleration/Deceleration in Positioning Mode / Manual Feed Mode

Axis feed is accelerated and decelerated in a linear pattern as shown below.

Feedrate

5228-E P-30

Start point End point

Position

ME33018R1000500070001

(2) Automatic Acceleration/Deceleration in the Cutting Feed Mode (G01, G02, G03)

In the cutting feed mode, axis feed is automatically accelerated and decelerated in the appropriate pattern as shown below.

Feedrate

Start point End point

Position

ME33018R1000500070002

(3) Processing Between Blocks

Type of New Block

Positioning Cutting Feed No Axis Movement

Type of Old Block

Positioning O O O Cutting Feed O X O No axis movement O O O

O: Program advances to the next block after executing the in-position check. X: Program advances to the next block without executing the in-position check. The term “in-position check” indicates the check if the actual axis position is within a predetermined width from the specified coordinate value. The in-position width is set for a system parameter.

(4) Exact Stop (G61, G09)

As indicated in the table above, since in-position check is not performed when cutting feed blocks continue, the join between cutting feed blocks will be dulled or rounded. The exact stop function prevents the join between such blocks from being dulled or rounded. For details, refer to SECTION 3, “Exact Stop Check”.

5. Following Error Check

Following error is defined as the difference between the command value output from the NC and the output of the position encoder. A DIFF over alarm occurs if a following error exceeds a certain value during rapid feed or cutting feed of an axis.

Axis Move Distance

5228-E P-31

SECTION 3 FEED FUNCTIONS

Command position

Actual machine position

Calculated value with acceleration/deceleration processing

Following error (ODIFF)

ME33018R1000500080001

6. Positioning (G00)

[Function] The axes move from the present position to the target position at rapid feedrate. During this movement, axes are automatically accelerated and decelerated. [Programming format] G00 IP__ In the positioning operation executed in the G00 mode, in-position check is executed. The commands in the next block are executed only after the in-position state is confirmed (in-position width is set for a system parameter). [Details]

• Whether positioning is executed in the linear pattern or a non-linear pattern is determined by the

setting for NC optional parameter (bit) No. 46, bit 0.

a. Linear interpolation pattern

The tool path is generated along a straight line from the actual position to the target position. In this movement, the feedrates of the individual axes are determined within the individual rapid feedrates so that positioning time can be minimized.

5228-E P-32

SECTION 3 FEED FUNCTIONS

Target position

Actual position

ME33018R1000500090001

b. Non-linear interpolation pattern

The individual axes move independently of each other at the individual rapid feedrates. Therefore, the resultant tool path is not always a straight line.

Target position

Actual position

ME33018R1000500090002

• The rapid feedrate of the individual axes is set by the machine tool builder and cannot be

changed.

• The in-position range is set for each axis using system parameters.

7. Uni-directional Positioning (G60)

[Function]

• In the positioning called by G00, positional error is unavoidable if positioning is executed in

different directions due to backlash in the axis feed mechanism. If positioning is always executed in the same direction, the influence of backlash is eliminated and therefore high positioning accuracy can be obtained. The function to always execute positioning in the same direction is called the unidirectional positioning function.

• If the positioning is going to be executed in the direction opposite to the direction set at

positioning direction of NC optional parameter (uni-directional positioning), the axis passes over the target point once and then moves back to the target point. The amount by which the axis passes beyond the target point (overrun amount) is set at either G60 overrun amount of NC optional parameter (uni-directional positioning) or user parameter.

[Programming format] G60 IP__

5228-E P-33

SECTION 3 FEED FUNCTIONS

[Details]

G00

G60

P direction (positive)

Target position

Overrun amount

N direction (negative)

ME33018R1000500100001

• When the linear interpolation mode positioning specification is provided, whether or not the

positioning is executed in the linear interpolation pattern is determined by the setting for NC optional parameter (bit) No. 46, bit 1.

• If the direction of the specified positioning agrees with the positioning direction set at positioning

direction of NC optional parameter (uni-directional positioning), the axis does not pass over the end point.

Start point

End point Start point

Overrun

ME33018R1000500100002

• G60 is a modal command.

• Uni-directional positioning is not valid for a cycle axis or shift movement in a fixed cycle.

• Uni-directional positioning is not valid on an axis for which no pass-over amount is set.

• Mirror image is not applied to the positioning direction.

8. Linear Interpolation (G01)

[Function] In the G01 linear interpolation mode, axes move directly from the actual position to the specified target point at the specified feedrate. [Programming format] G01 IP__F__ IP: Target point (end point) F: Feedrate. The specified feedrate remains valid until updated by another value. [Details]

• A feedrate value specified with address “F” is cleared to zero when the NC is reset. Note that

the F command value is saved when the NC is reset if a feedrate is specified in an F1-digit command.

5228-E P-34

SECTION 3 FEED FUNCTIONS

• The feedrate for each axis is as indicated below. (For values X, Y, and Z, convert them into an

incremental value.)

G01 XxYyZzFf Calculation of feedrates:

X-axis feedrate: FX =

Y-axis feedrate: FY =

Z-axis feedrate: FZ =

Where, L = x2+y2+z

For the rotary axis, the unit of feedrate is regarded as indicated below: 1 mm/min = 1 deg/min 1 inch/min = 1 deg/min

In linear interpolation including a rotary axis, the feedrates are determined according to the formulas given above for the individual axes. Example: G91 G01 X10 C20 F30.0 <“mm” input>

X-axis feedrate FX =

C-axis feedrate FC =

102+20

L y

L z

x 30 13.41 mm/min

x 30 26.83 deg/min

ME33018R1000500110001

ME33018R1000500110002

<“inch” input>

5228-E P-35

SECTION 3 FEED FUNCTIONS

X-axis feedrate FX =

C-axis feedrate FC =

102+20

x 30 13.41 inch/min

x 30 26.83 deg/min

• When the F command (F=1) to the rotary axis in the inch system is issued, whether to interpret

"F1" as 1 deg/min or as 25.4 deg/min is set by NC optional parameter (bit) No. 15, bit 7.

9. Plane Selection (G17, G18, G19)

[Function] Selecting a plane is necessary in order to perform the following functions:

• Circular interpolation (Helical cutting)

• Angle command (AG)

• Cutter radius compensation

• Coordinate rotation (Local coordinate system)

• Fixed cycle

ME33018R1000500110003

• Coordinate calculation

• Area machining

The planes that can be selected are indicated below:

G17 : Xp-Yp plane G18 : Zp-Xp plane G19 : Yp-Zp plane

[Programming format]

G17

G18

G19

Xp Yp Zp

... ... ...

X- or U-axis. Y- or V-axis. Z- or W-axis.

ME33018R1000500120001

ME33018R1000500120002

5228-E P-36

SECTION 3 FEED FUNCTIONS

[Details]

• Whether a basic axis (X, Y, Z) or a parallel axis (U, V, W) is selected is determined by the axis

addresses specified in the block containing G17, G18 or G19. Examples:

G17 G17 G18 G18 G19 G19

X U Z W Y Y

plane

ME33018R1000500120003

• In blocks where none of G17, G18, and G19 are specified, the selected plane remains

unchanged even if axis addresses are changed.

• In blocks where G17, G18, or G19 is specified, if an axis address is omitted, the basic axis (X,

Y, Z) is assumed to be omitted. Examples:

G17 G17 G17 G18 G18

X U

plane

ME33018R1000500120004

• If a command for an axis that does not exist in the plane selected in the G17, G18, or G19 block

is issued, the axis movement is performed regardless of selected plane.

• The plane to be selected when the power is turned ON or the NC is reset can be designated by

the setting at THE G CODE TO BE SET AUTOMATICALLY (PLANE) of the NC optional parameter (AUTO SET AT NC RESET/POWER ON).

• An alarm occurs if both the basic axis and its parallel axis are specified in a plane selection

block.

10. Circular Interpolation (G02, G03)

[Function] The circular interpolation function moves a tool from the actual position to the specified position along an arc at the specified feedrate. [Programming format]

5228-E P-37

SECTION 3 FEED FUNCTIONS

Arc on Xp-Yp plane : G17

Arc on Zp-Xp plane : G18

Arc on Yp-Zp plane : G19

G02

Xp__Yp__ F__

G03 G02

Zp__Xp__ F__

G03 G02

Yp__Zp__ F__

G03

I_J_

K_I_

J_K_

Xp = X-axis or U-axis Yp = Y-axis or V-axis Zp = Z-axis or W-axis

• G codes used for the circular interpolation function are indicated below.

G17 : Plane selection : Sets the circular arc in the Xp-Yp plane. G18 : Plane selection : Sets the circular arc in the Zp-Xp plane. G19 : Plane selection : Sets the circular arc in the Yp-Zp plane. G02 : Direction of rotation : Sets the clockwise direction. G03 : Direction of rotation : Sets the counterclockwise direction.

Two axes among Xp, Yp, and Zp, G90 mode: Sets the end point in the work coordinate system Two axes among Xp, Yp, and Zp, G91 mode: Sets the position in reference to the start point with signed values. Two axes among I, J, and K: Sets the distance from the start point to the center with signed values. R: Sets the radius of an arc. F: Sets the feedrate.

ME33018R1000500130001

[Details]

• Direction of rotation, clockwise or counterclockwise, is defined when viewing the plane from the

positive direction of the Zp-axis (Yp-axis, Xp-axis) on the Xp-Yp (Zp-Xp, Yp-Zp) plane, as shown in the illustrations below.

ME33018R1000500130002

5228-E P-38

SECTION 3 FEED FUNCTIONS

• The end point is defined by either an absolute value or an incremental value according to G90

or G91. The center point of an arc is determined by the I, J, and K values which correspond to Xp, Yp, and Zp, respectively. Their coordinate values are always specified as incremental values, regardless of G90 or G91.

End point

Center

Start point

End point

Center

Start point

End point

Center

Start poin

ME33018R1000500130003

A minus sign should be used for the I, J, and K values when necessary.

• The end point of an arc can be designated by specifying the coordinate value on one of the two

axes. If only one axis is specified, the processing may be selected from the following two methods.

a. For axes with no command, the previous command value is used as the end point of the

arc. (For this processing, set the value for axis not programmed (circular single-axis) of NC optional parameter (circular interpolation) as the current value.)

Vertical axis

Horizontal axis

Start point End point

X -70.711, Y -70.711

ex :

G02 X70.711 I70.711 J70.711

X -70.711, Y -70.711 G02 X10 I70.711 J70.711

When programming an arc as illustrated to the left, the end point of the arc can be designated with only the coordinate value of the horizontal axis, since the coordinate value of the vertical axis is the same at the start and end points. An alarm occurs if the end point does not lie on an arc. The left program defines a clockwise arc: Radius: 100 Center: (0, 0) Start point: (-70.711, -70.711) End point: (70.711, -70.711)

The left program will cause an alarm, since the end point (10, -70.711) is not on the arc.

ME33018R1000500130004

b. For the omitted axis, the coordinate value is calculated using the coordinate value of the

specified axis. For this processing, choose point on arc at command value for the axis not programmed (single-axis) of NC optional parameter (circular interpolation).

When programming an arc as illustrated in the left, the end point can be designated with only the horizontal axis coordinate value. The vertical axis coordinate value is calculated from the horizontal axis coordinate value.

ME33018R1000500130005

G02

Start point

End point

G03

5228-E P-39

SECTION 3 FEED FUNCTIONS

• If more than one end point is possible, the one which is reached first in the designated arc

direction is selected. Example:

X-70.711 Y-70.711 F200 G02 X10 I70.711 J70.711

The program to the left defines a clockwise arc: Radius: 100 Center: (0, 0) Start point: (-70.711, -70.711) End point: (10,99.499)

ME33018R1000500130006

The operations explained above also apply when designation of a vertical axis is omitted.

• The center of an arc can be defined by specifying the radius (R) of the arc instead of specifying

I, J, and K. If an arc is specified by the radius, four arcs that pass the same start and end points are defined. To define a specific arc from among these four arcs, an R value is used in the manner indicated below.

• Clockwise arc (G02)

An arc whose central angle is smaller than or equal to 180 degrees: Radius R > 0 An arc whose central angle is greater than 180 degrees: Radius R < 0

• Counterclockwise arc (G03)

An arc whose central angle is smaller than or equal to 180 degrees: Radius R > 0 An arc whose central angle is greater than 180 degrees: Radius R < 0

End point

Start point

End point

Start point

ii) Counterclockwise arc i) Clockwise arc

ME33018R1000500130007

• The feedrate in circular interpolation is the feedrate component tangential to the arc.

[Supplement]

• If I, J, or K is omitted, it is regarded that “0” is specified.

• An arc with radius 0 (R = 0) cannot be specified.

• If the values for Xp, Yp, and Zp are omitted, an arc having the start and end points on the same

point is defined in the following manner: a) If the center is specified by I, J, and/or K, a 360-degree arc b) If the radius is specified by R, a 0-degree arc

• It is not possible to specify R, and I, J, and K at the same time.

• It is not possible to specify any axis parallel to the axes which make up the selected plane. For

example, designation of the W-axis is not allowed when the Z-X plane is selected.

• An alarm will occur if the difference in radius between the start point and the end point of an arc

is greater than or equal to the value set at arc check data (difference in radius between start and end) of the NC optional parameter (circular interpolation).

11. Helical Cutting (G02, G03) (Optional)

[Function] Helical cutting or helical interpolation may be executed by synchronizing circular interpolation with linear interpolation of the axis which intersects at right angles the plane in which the arc is defined. [Programming format]

5228-E P-40

SECTION 3 FEED FUNCTIONS

XpYp plane : G17

α : An axis not parallel to the axes comprising the arc plane

G02

Xp__Yp__ α__F__

G03

I_J_

ME33018R1000500140001

[Details]

• Helical cutting may also be programmed on the Zp-Xp (G18) and Yp-Zp (G19) planes, using a

format similar to that above.

• To program helical cutting, simply add the command of the axis which intersects the arc plane

to the circular interpolation.

• Helical cutting is possible for an arc having a center angle of smaller than 360 degrees.

• The feedrate specified by an F command is valid for circular interpolation. Therefore, the

feedrate in the direction of the linear axis is calculated by the following formula:

Feedrate in the linear axis direction =

Motion distance of the linear axis

Arc length

x F

ME33018R1000500140002

• Tool length offset is valid for the axis at right angles to the arc plane.

• Cutter radius compensation is valid only for circular interpolation commands.

5228-E P-41

SECTION 4 PREPARATORY FUNCTIONS

G codes consisting of address character G and a three-digit number (00 to 399) set the mode that specifies how the commands are executed. Instead of using address character G, some G codes are expressed by mnemonics. A mnemonic code consists of up to eight alphabetic characters (A to Z).

• Valid range of G codes

One-shot G codes: Valid only in the specified block. Such G codes are automatically canceled when a program advances to the next block. Modal G codes: Once specified, such G codes remain valid until another G code in the same group is specified.

• Special G codes

Mnemonic codes used for subprogram call and those used as branch instructions are called special G codes. Special G codes must be specified at the beginning of a block and entry of such codes at a middle of a block is not allowed. Note, however, that a slash “/” code (optional block skip code) or a sequence name may be placed before a special G code.

• For the tables of G codes and mnemonic codes, refer to “G Code Table” and “Table of Mnemonic Codes”

in APPENDIX.

1. Dwell Command (G04)

[Function] At the end of the specified block, the dwell function suspends the execution of a program for the specified length of time before proceeding to the next block. [Programming format] The following two programming formats may be used to specify the dwell function.

• G04 F__

F: Sets the length of dwell time The unit of dwell time can be selected from 1, 0.1, 0.01 and 0.001 seconds by the NC optional parameter (INPUT UNIT SYSTEM). The maximum programmable dwell time is 99999.999 seconds.

• G04 P__

P: Sets the length of dwell time The unit of dwell time is selected in the same manner as when specified by F.

SECTION 4 PREPARATORY FUNCTIONS

2. Programmable Mirror Image (G62) (Optional)

[Function] The mirror image function creates a geometry which is symmetric around a specific axis. In addition to the mirror image switch on the machine panel, the programmable image function creates mirror images using programmed commands. The axis which is in the mirror image mode is identified on the screen display; a dash “-” is added before the axis name on the ACTUAL POSITION screen. [Programming format]

5228-E P-42

G62 IP

0 1

0 : Normal (Mirror image OFF) 1 : Mirror image

ME33018R1000600030001

[Details]

• The actual state of the mirror image function based on the specification of G62 and the

MIRROR IMAGE switch setting is displayed in the table below.

G62 Switch Setting Actual State

Normal Normal Normal Normal Mirror image Mirror image Mirror image Normal Mirror image Mirror image Mirror image Normal

ME33018R1000600030002

• A block in which G62 is specified must not contain any other commands.

• The mirror image function is modal.

• The axes not specified in the G62 block are assumed to be in the normal mode.

• All axes are in the normal mode when the power supply is turned on.

• Whether all axes will be set in the normal mode or not when the NC is reset can be set at AT AN

NC RESET, CLEARS THE G62 MIRROR IMAGE FOR ALL AXES of NC optional parameter (MIRROR IMAGE).

• The coordinate system (local or work) in which the mirror image function will be active can be

selected at local/work coordinate system select of NC optional parameter (MIRROR IMAGE).

Example:

G11 X40 Y10 P45 G01 X5

G62 X1

X30 Y5

Y30 Y5

S__F__

ME33018R1000600030003

5228-E P-43

SECTION 4 PREPARATORY FUNCTIONS

(1) If work is selected at local/work coordinate system select of NC optional parameter (MIRROR

IMAGE)

X - Y

: Work coordinate system

X' - Y'

: Local coordinate system

ME33018R1000600030004

(2) If local is selected at local/work coordinate system of NC optional parameter (MIRROR IMAGE)

ME33018R1000600030005

SECTION 4 PREPARATORY FUNCTIONS

3. Work Coordinate System Selection (G15, G16)

[Function] 20 sets of work coordinate systems are supplied as a standard feature and this can be expanded to 50, 100 or 200 sets optionally. [Programming format] Modal G code: G15 Hn (0 ≤ n ≤ 200) Once a new work coordinate system “n” is set using the modal G code, the coordinate values specified in the same and later blocks are interpreted as coordinate values in the selected work coordinate system “n”. One-shot G code: G16 Hn (0 ≤ n ≤ 200) If a new work coordinate system “n” is set using the one-shot G code, only the coordinate values specified in the same block are interpreted as coordinate values in the selected work coordinate system “n”. [Details]

• For G15 and G16, the work coordinate system number between 1 and 200 is specified by “n” (1

to 200). If “0” is specified for “n”, the machine coordinate system is selected.

• When the power supply is turned ON, and after the NC is reset, the work coordinate system

previously selected by G15 is automatically selected.

5228-E P-44

• G15 and G16 may not be specified in the following modes:

• Cutter radius compensation mode

• Three-dimensional offset mode

• Geometry enlargement/reduction mode

• Coordinate system parallel shift/rotation mode

[Supplement]

Axis feed commands specified immediately after G15 must be specified in the absolute mode.

SECTION 4 PREPARATORY FUNCTIONS

4. Work Coordinate System Change (G92)

[Function] The work coordinate system change function changes the work coordinate system. [Programming format] G92 IP__ [Details]

• G92 automatically changes the work zero offset value of the presently selected work coordinate

system so that the coordinate value of the present tool position will be the coordinate value specified as IP__.

• G92 changes only the work coordinate system that is selected at the time it is executed; it does

not affect any other work coordinate systems.

• The coordinate value P specified in this block is always treated as an absolute value regardless

of the specification of G90 (absolute mode) and G91 (incremental mode).

• For the axis not specified with the coordinate value P, the work zero offset value remains

unchanged.

• G92 may not be specified in the following modes:

5228-E P-45

• Cutter radius compensation mode

• Three-dimensional offset mode

• Geometry enlargement/reduction mode

• Coordinate system parallel shift/rotation mode

• Machine coordinate system selected mode

5. Unit System Check (G20, G21) (Optional)

[Function] The unit system check function checks the unit system selected by the setting at LENGTH UNIT SYSTEM of NC optional parameter (INPUT UNIT SYSTEM). If the selected system does not agree with the unit system specified by G20 / G21, an alarm occurs. [Programming format] G20:Checking for the selection of the inch system An alarm occurs if the metric system is selected by the setting for the parameter. G21:Checking for the selection of the metric system An alarm occurs if the inch system is selected by the setting for the parameter.

5228-E P-46

SECTION 4 PREPARATORY FUNCTIONS

6. Coordinate System Conversion Functions

6-1. Parallel Shift and Rotation of Coordinate Systems (G11, G10)

[Function] The parallel shift / rotation function shifts or rotates a work coordinate system. The new coordinate system defined by shifting or rotating a work coordinate system is called a local coordinate system. It is possible to cancel a local coordinate system. [Programming format] Parallel shift / rotation of coordinate system: G11 IP__ P__

IP: Parallel shift amount to establish a local coordinate system

Specify the shift amount as an absolute value in reference to the origin of the work coordinate system, regardless of the selected dimensioning mode, absolute mode (G90), incremental mode (G91), or mirror image (G62).

P: Rotation amount to establish a local coordinate system

Specify the angle of rotation in units of 1 degree, 0.001 degree, or 0.0001 degree in accordance with the selected unit system (LENGTH UNIT SYSTEM and ANGLE of NC optional parameter (INPUT UNIT SYSTEM)). If “P0” is specified or a P command is not specified, only work coordinate system shift takes place, without rotation. Rotation of a work coordinate system is executed in the plane (G17, G18, G19) that is active when G11 is specified, and it does not affect the axes not included in this plane. The direction of rotation is counterclockwise viewed from the positive direction of the axis not included in the rotation plane. Specify the angle of rotation as an absolute value, regardless of the selected dimensioning mode (G90, G91).

• Cancellation of local coordinate system: G10

When G10 is specified, the parallel shift amount and angle of rotation are canceled.

[Details]

• Once G11 is executed, the NC enters the state in which a local coordinate system is defined. If

G11 is executed again in this state, it will change the previously defined local coordinate system. At the second designation of G11, if the designation of an axis address is omitted, the value designated in the first G11 is assumed to apply. The set values are cleared when the power supply is turned OFF / ON, the NC is reset, or G10 (local coordinate system cancel) is executed.

• A block which contains G10 or G11 must not contain any other G codes.

• G10 and G11 are modal. G10 is set when the power is turned ON or when the NC is reset.

• G11 must not be specified in the following modes:

• Geometry enlargement/reduction mode

• When the machine coordinate system (H00) is selected

• Copy function mode

5228-E P-47

SECTION 4 PREPARATORY FUNCTIONS

[Example program] If a local coordinate system is used, the example workpiece shown below would be programmed as indicated in the example program.

Machine coordinate system

Zero point of local coordinate system

Zero point of work coordinate system

G00

N1 N2 N3 N4 N5 N6 N7 N8 N9 N10 N11 N12

∗ : The zero offset values of work coordinate system 1 are : x= 25, y = 15

G90

G15

F100

X60

G01 Y40 X0 Y0

X20X0Y10

G11

G17

X0 X30 Y10 X0 Y0

...................................

G10

..........

P40

....................

H01

Selecting work coordinate system 1

Setting a local coordinate system

Canceling a local coordinate system

ME33018R1000600070001

6-2. Copy Function (COPY, COPYE)

[Function] The copy function is used to facilitate part machining by repeating the same pattern with parallel shift and rotation. First, specify parallel shift and rotation of a local coordinate system using COPY instead of G11, then program the pattern to be repeated. Finally, specify the incremental value of parallel shift / rotation. [Programming format] Parallel shift/rotation of local coordinate system: COPY IP__ P__ Q__

IP: Initial value of parallel shift component to establish a local coordinate system

Specify this as an absolute value in reference to the origin of the presently selected work coordinate system.

P: Initial value of rotation component to establish a local coordinate system

Specify this value in units of 1 degree, 0.001 degree, or 0.0001 degree in accordance with the selected unit system (“LENGTH UNIT SYSTEM” and “ANGLE” of NC optional parameter (INPUT UNIT SYSTEM)). If a P command is not specified in the G11 mode, the previous setting is valid.

Q: The number of times the pattern should be repeated.

Setting range: 1 to 9999 Default value: 1

5228-E P-48

SECTION 4 PREPARATORY FUNCTIONS

Repeated pattern program: COPYE IP__ P__

IP: Incremental value for parallel shift of a local coordinate system.

Default value: 0

P: Incremental value for rotation of a local coordinate system.

Default value: 0

[Details]

• Both G11 and COPY may be specified while a local coordinate system is established by the

execution of G11. Once COPY is specified, however, an alarm occurs if G11 or COPY is specified again.

• If COPY is specified in the main program selected for operation method B (large-volume tape

operation), designation of IF and GOTO is not permissible in the program that defines the pattern to be repeated. The size of the program beginning with COPY and ending with COPYE must be within 10 m (33 ft) in tape length.

[Example program]

Zero point of local coordinate system

G11 G01 COPY G01 G03 G01 COPYE

X15 X30 Q4 X30 X0 X0

P - 30

Y25

M03

F100

...........................................

Y0 Y30I - 20J10

.........................................

Y30 P90

5228-E P-49

SECTION 4 PREPARATORY FUNCTIONS

Zero point of work coordinate system

Start point of arc

End point of arc

∗ : Circular interpolation commands must not be specified in the block immediately after the COPY block and the one immediately before the COPYE block.

ME33018R1000600080001

5228-E P-50

SECTION 4 PREPARATORY FUNCTIONS

7. Workpiece Geometry Enlargement / Reduction Function (G51, G50) (Optional)

[Function] The workpiece geometry enlargement / reduction function enlarges or reduces the geometry defined by a program in reference to the point specified in a local coordinate system. If a local coordinate system is not specified, a work coordinate system is used to specify the reference point for enlargement / reduction. [Programming format] Enlargement / reduction of geometry: G51 IP __ P__

IP: The center of the enlargement / reduction of geometry.

Specify this point in a local coordinate system. For axes not specified in this block, the coordinate value (in the local coordinate system) of the point at which G51 is specified is assumed to apply.

P: Multiplication factor for enlargement or reduction.

Programmable range: 0.000001 to 99.999999 Default value: 1

Cancellation of enlar

P0 P1 - P4 P'1 - P'4

ement / reduction : G50

: Center of enlargement / reduction : Programmed geometry : Reduced geometry

ME33018R1000600090001

[Details]

• The enlargement/reduction function is made valid or invalid on individual axes according to the

setting for NC optional parameter (geometry enlargement/reduction). However, an alarm will occur in the radius check if the parameter setting differs among the axes in the plane specified for circular interpolation.

• The enlargement/reduction function does not affect the following:

a. Local coordinate system setting values (G11)

b. Cutter radius compensation values and three-dimensional offset values (G41, G42, G43)

c. Tool length offset values (G54 to G59)

d. Work coordinate system setting values (G92)

SECTION 4 PREPARATORY FUNCTIONS

e. The following Z-axis movements in a fixed cycle:

• In-feed and retraction amounts in deep hole drilling cycle (G73, G83)

• X, Y shift amounts in fine boring or back boring (G76, G87)

Example: Cutter radius compensation and enlargement and reduction of workpiece geometry

5228-E P-51

ME33018R1000600090002

[Example program] An example program for setting a local coordinate system and enlarging/reducing workpiece geometry is shown below.

G17

G11

X50

G90

G51

X20

G01

X40 N4 N5 N6

Y20

Geometry after setting a local coordinate system and reducing geometry

Y30 Y10

P45

Setting of local coordinate system

P0.5

Reduction of geometry Positioning at P'1 Positioning at P'2 Positioning at P'3 Positioning at P'4

Local coordinate

system

Geometry after setting a local coordinate system

Reduction only

Geometry defined by a program

Work coordinate system

ME33018R1000600090003

5228-E P-52

SECTION 5 S, T, AND M FUNCTIONS

This section describes the S, T, and M codes which specify necessary machine operations other than axis movement commands. S: Spindle speed T: Tool number for tool change cycle M: Turning solenoids and other similar devices on and off Only one of each of these types of code may be specified in one block. If two or more commands of the same code type are issued to one block, the rightmost command of each code type will be executed.

<Example> M6 T1 T2------M6 T2 will be executed.

1. S Code Function

[Function] The spindle function specifies a spindle speed with a numeric value (up to five digits) entered following address S. [Details]

• The desired spindle speed (min

S. Programmable range: 0 to 65535

• If an S command is specified with axis movement commands in the same block, the S

command becomes valid at the same time axis movement commands are executed.

• Although an S command is not canceled when the NC is reset, it is cleared when the power

supply is turned off.

• To execute a spindle rotation command (M03, M04), an S command must be specified in the

same or a previous block.

2. T Code Function

[Function] The tool function selects a tool in the machine with a numeric value (up to four digits) entered following address T. [Details]

• The programmable range of a T command is indicated below.

Programmable range: 0 to 9999

• When a T code is executed, the next tool is prepared (indexing the next tool in the magazine, or

taking the next tool out of the magazine and setting it in the ready station position).

-1

) is directly specified by a numeric value following the address

• The actual tool change cycle is executed by M06.

• If a T command is specified with axis movement commands in the same block, the execution

timing of the T code can be selected from the following two timings: Executed simultaneously with axis movement commands Executed after the completion of axis movement commands

3. M Code Function

[Function] The M code function outputs an M code number, consisting of a three-digit number and address M, and the strobe to the PLC. The programmable range of M codes is from 0 to 511.

3-1. Examples of M Codes

The followings are examples of M codes.

(1) M02, M30 (End of Program)

These M codes indicate the end of a program. When M02 or M30 is executed, the main program ends and reset processing is executed. The program is rewound to its start. (In the case of a schedule program, execution of M02 or M30 in the main program does not reset the NC.)

(2) M03, M04, M05 (Spindle CW/CCW and Stop)

These M codes control spindle rotation and stop; spindle CW (M03), spindle CCW (M04), and spindle stop (M05).

(3) M19 (Spindle Orientation)

The M19 command is used with machines equipped with the spindle orientation mechanism. The spindle orientation function stops the spindle at a specified angular position.

5228-E P-53

SECTION 5 S, T, AND M FUNCTIONS

• Multi-point spindle indexing

By specifying “RS=angle” following M19, it is possible to index the spindle at the specified angular position. Although the following explanation uses M19 as an example, the same applies to M118 and M119. M19 RS = θ

• θ represents the desired index angle and it is specified in units of 1°. If a value smaller

than 1° is specified, it is truncated.

• Programmable range of θ: 0 to 360°

• θ specifies the desired index angle of the spindle, measured in the CW rotation angle

in reference to the spindle orientation position.

[Supplement]

• If M19 (M118, M119) is specified without argument RS, ordinary spindle orientation is

performed. That is, the called operation is the same as that called by “M19 RS=0”.

• RS must always be specified in the same block as M19 (M118, M119).

(4) M52 (Fixed Cycle - Return to the Retract End)

In various fixed cycles, this command sets the return position of the cycle axis 0.1 mm away from the travel limit of the Z-axis in the positive direction. For details, refer to SECTION 7, “Fixed Cycle Operations”.

(5) M53 (Fixed Cycle - Return to the Specified Point)

In various fixed cycles, this command sets the return position of the cycle axis at the position specified by G71. For details, refer to SECTION 7, “Fixed Cycle Operations”.

5228-E P-54

SECTION 5 S, T, AND M FUNCTIONS

(6) M54 (Fixed Cycle - Return to Point R Level)

In various fixed cycles, this command sets the return position of the cycle axis at the position specified by R command. For details, refer to SECTION 7, “Fixed Cycle Operations”.

(7) M132, M133 (Single Block Valid/Invalid)

These M codes set whether the single block function is made invalid (M132) or valid (M133) independently of the setting of the single block switch on the machine operation panel.

(8) M201 to M210 (M Code Macro)

By setting the program names which correspond to M201 to M210 in the parameters, the sub programs can be executed by specifying the M codes. For details of M code macro, refer to SECTION 10, “G and M Code Macro Functions”.

(9) M238, M239 (Soft-override Valid/Invalid)

These commands set whether or not the soft-override value (%) set for system variables <VFSOV> is valid (M238) or invalid (M239) for the cutting feedrate (F command × override value).

(10) M00 (Program Stop)

After the execution of M00, the program stops. If the NC is started in this program stop state, the program restarts.

(11) M01 (Optional Stop)

When M01 is executed while the optional stop switch on the machine operation panel is ON, the program stops. If the NC is started in this optional stop state, the program restarts.

(12) M06 (Tool Change)

This M code is used with machines equipped with the tool change mechanism as the tool change cycle start command.

(13) M15, M16 (Fourth Axis - Rotary Table CW, CCW)

These M codes are used with machines equipped with the rotary table as the fourth axis to specify the direction of rotary table rotation; CW (M15), CCW (M16). For details of the rotary table control, refer to “Additional Axis (Rotary Axis) Function” is SPECIAL FUNCTIONS Manual No.2.

(14) M115, M116 (Fifth Axis - Rotary Table CW, CCW)

These M codes are used with machines equipped with the rotary table as the fifth axis to specify the direction of rotary table rotation; CW (M115), CCW (M116) For details of rotary table control, refer to “Additional Axis (Rotary Axis) Function” is SPECIAL FUNCTIONS Manual No.2.

(15) M118, M119 (Spindle Index - CCW, Shorter Path)

These M codes are used with machines equipped with the spindle index mechanism as the spindle orientation direction specifying command. [Programming format]

• M118 Spindle index (CCW)

• M119 Spindle index (shorter path)

(16) M130, M131 (For Cutting Feed, Spindle Rotation Condition Valid / Invalid)

Usually, in the G01, G02, and G03 modes, the spindle must be rotating to execute axis feed. These M codes are set to ignore this condition (M130) or validate it (M131).

5228-E P-55

SECTION 5 S, T, AND M FUNCTIONS

(17) M134, M135 (Spindle Speed Override Valid / Invalid)

Even in the status in which spindle speed override control from the PLC is valid, the spindle speed override function can be made invalid (M134) or valid (M135) with these commands.

(18) M136, M137 (Axis Feed Override Valid / Invalid)

These M codes set whether the axis feed override function is made invalid (M136) or valid (M137) independently of the ON status of the axis feed override signal from the PLC.

(19) M138, M139 (Dry Run Valid / Invalid)

These M codes set whether the dry run function is made invalid (M138) or valid (M139) independently of the setting of the dry run switch on the machine operation panel.

(20) M140, M141 (Slide Hold Valid / Invalid)

These M codes set whether the slide hold function is made invalid (M140) or valid (M141) independently of the setting of the slide hold switch on the machine operation panel.

(21) M234 to M237 (Gear Selection Range for Synchronized Tapping)

These M codes set the gear selection range for synchronized tapping. For details, refer to “Torque Monitoring Function” in Synchronized Tapping of SPECIAL FUNCTIONS Manual.

(22) M326, M327 (Torque Monitor ON / OFF for Synchronized Tapping)

These M codes turn ON (M326) and OFF (M327) the torque monitor mode for synchronized tapping.

(23) M331, M332 (Sixth Axis - Rotary Table CW / CCW)

These M codes are used with machines equipped with the rotary table as the sixth axis to specify the direction of rotary table rotation; CW (M331), CCW (M332) For details of rotary table control, refer to “Additional Axis (Rotary Axis) Function” is SPECIAL FUNCTIONS Manual No.2.

(24) M396 to M399 (Gear Position Selection for Synchronized Tapping)

These are gear position commands, specially for synchronized tapping, introduced by the gear selection range specifying M codes (M234 to M237) and the S command. They are automatically generated by the NC.

• M396: 1st gear command for synchronized tapping

• M397: 2nd gear command for synchronized tapping

• M398: 3rd gear command for synchronized tapping

• M399: 4th gear command for synchronized tapping

SECTION 6 OFFSET FUNCTIONS

1. Tool Length Offset Function (G53 - G59)

[Function] The tool length offset function compensates for the position of a cutting tool so that the tip of the cutting tool is located at the programmed position. Available G Codes

G Code Function G53 Cancel tool length offset G54 Tool length offset, X-axis G55 Tool length offset, Y-axis G56 Tool length offset, Z-axis G57 Tool length offset, 4th-axis G58 Tool length offset, 5th-axis G59 Tool length offset, 6th-axis

[Programming format] {G54 - G59} IP__ H__

IP: Current position of tool tip after compensation H: Tool offset number

The standard tool offset numbers are H00 to H100, and this can be expanded to H200 or H300. The offset amount of H00 is always zero. Offset data is set in the tool data setting mode. Setting range: 0 to ±999.999 mm (0 to ±39.3700 inches)

5228-E P-56

[Details]

• The displayed actual tool position value always includes the tool length offset amount.

• The tool length offset cannot be applied to two or more axes at the same time or to the rotary

axis.

• The tool length offset may be changed directly without having to cancel the previous command

with G53.

• When the NC is reset, H00 is automatically set.

SECTION 6 OFFSET FUNCTIONS

2. Cutter Radius Compensation (G40, G41, G42)

2-1. Cutter Radius Compensation Function

[Function] The cutter radius compensation function automatically compensates for the cutter radius. Programming the geometry of a workpiece as it is will not result in a correct final product because the size (diameter) of the tool is not taken into consideration. It would, however, be extremely complicated and difficult to develop a program which takes the tool diameter into account. This problem may be solved by a function called cutter radius compensation which automatically compensates for the tool diameter. If the cutter radius compensation function is used for programming, the correctly offset tool center path is automatically generated by programming the tool path along the geometry of workpiece to be machined. [Programming format]

G17 G41 (G42) Xp__ Yp__ D__ G18 G41 (G42) Zp__Xp__ D__ G19 G41 (G42) Yp__Zp__ D__

G40: Cancel cutter radius compensation (The mode automatically selected when the power is

turned ON.) For details, refer to “Tool Movement when Cutter Radius Compensation is Canceled”.

G41: Cutting at left (Offset - the left side as seen from the tool moving direction; downward cutting)

For details, refer to “Changing Compensation Direction in Cutter Radius Compensation Mode”.

G42: Cutting at right (Offset to the right side as seen from the direction of tool motion; upward

cutting) The cutter radius compensation mode is set when either G41 or G42 is specified and this mode is canceled by G40. For details, refer to “Changing Compensation Direction in Cutter

Radius Compensation Mode”. G17: Xp-Yp plane selection Select the plane in the same manner as in the G02 or G03 mode. G18: Zp-Xp plane selection Select the plane in the same manner as in the G02 or G03 mode. G19: Yp-Zp plane selection Select the plane in the same manner as in the G02 or G03 mode. D**: Cutter radius compensation number. (For details, refer to “Notes on Cutter Radius

Compensation”.)

5228-E P-57

[Supplement]

• The explanation below assumes G17 (Xp-Yp plane), which is automatically set when power is

turned ON. For the Zp-Yp plane and the Yp-Zp plane, the same explanation applies.

• Entry to the cutter radius compensation mode is allowed only in the G00 or G01 mode. An

alarm occurs if the cutter radius compensation mode is called in other modes.

• The mode is changed to the cutter radius compensation mode in the first block that contains a

command that actually causes axis movement after the designation of the cutter radius compensation command.

5228-E P-58

SECTION 6 OFFSET FUNCTIONS

• The terms “inside” and “outside” are defined as follows:

The angle made between consecutive tool paths is measured at the workpiece side and “inside” and “outside” are defined by the magnitude of this angle. If the angle is larger than 180°, it is defined as “inside” and if the angle is in the range between 0 and 180°, it is defined as “outside”.

ME33018R1000800020001

• The symbols used in the illustrations in “Tool Movement in Start-up” to “Notes on Cutter Radius

Compensation” have the following meaning:

Single block stop point

Linear motion

Circular motion

Tangent to an arc

Cutter radius compensation amount

Angle at the workpiece side

Cross point, made when a programmed path (or the tangent to an arc) is shifted

by a compensation amount Programmed tool path

Tool center path

Auxiliary line

ME33018R1000800020002

2-2. Tool Movement in Start-up

2-2-1. Inside Corner Cutting (θ ≥ 180°)

(1) Straight line - Straight line

(2) Straight line - Arc

5228-E P-59

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800030001

2-2-2. Obtusely Angled Corner - Outside Cutting (90° ≤ θ ≤ 180°)

(1) Straight line - Straight line

(2) Straight line - Arc

ME33018R1000800030002

ME33018R1000800040001

ME33018R1000800040002

2-2-3. Acutely Angled Corner - Outside Cutting (θ < 90°)

(1) Straight line - Straight line

(2) Straight line - Arc

5228-E P-60

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800050001

(3) Exception

Outside cutting at an acute angle of 1° or less is considered to be “inside” as shown below.

≤

ME33018R1000800050002

ME33018R1000800050003

2-2-4. Start-up with Imaginary Approach Direction

If the block which starts up the cutter radius compensation includes any I__, J__, or K__ belonging to the offset plane (I__, J__ in the case of G17 plane), the axes move to the target point specified in this block from the direction defined by I__ and/or J__. In this case, note that the cross point is always calculated regardless of whether the cutting is “inside” or “outside.”

Imaginary approach direction

5228-E P-61

SECTION 6 OFFSET FUNCTIONS

N1 G41

X5000 Y5000 I-1J1D1

Imaginary approach direction

N1 G41

X100000

X5000 Y5000 I1J-1D1

X100000

ME33018R1000800060001

If no cross point exists, positioning is executed to the point obtained by a vertical shift by the compensation amount from the target point specified in the G41 block.

N1 G41

Imaginary approach direction

X5000 Y5000 I-1J0

X100000

ME33018R1000800060002

SECTION 6 OFFSET FUNCTIONS

2-3. Tool Movement in Cutter Radius Compensation Mode

[Supplement]

This section describes operations from the operation that begins after entering in the tool offset mode until just before canceling the cutter radius compensation mode. Example: Consecutive 4 blocks (zero movements of the axes in the selected plane)

5228-E P-62

Over-cutting •

Stops 5 times in single block

•

N4 X5000 Y500 N5 Z5000 N6 F1000 N7 M01 N8 G04 F50 N9 X100000

•

Example: One block (zero movement of the axes in the selected plane)

Over-cutting •

Stops 2 times in single block

•

N4 G91 X5000 Y5000 N5 X0 N6 X5000

•

ME33018R1000800070001

ME33018R1000800070002

2-3-1. Inside Cutting (θ ≥ 180°)

(1) Straight line - Straight line

(2) Straight line - Arc

5228-E P-63

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800080001

(3) Arc - Straight line

ME33018R1000800080002

ME33018R1000800080003

5228-E P-64

SECTION 6 OFFSET FUNCTIONS

(4) Arc - arc

ME33018R1000800080004

(5) Exception

There is an exception in processing where inside cutting at 1 degree or less for the straight line

- straight line configuration is replaced by outside cutting (this is explained later) because the ordinary method of finding the cross point will deviate significantly from the command value. Straight line - straight line θ ≤ 1°

ME33018R1000800080005

(6) The processing shown above is limited to the straight line - straight line configuration. In other

cases, such as the straight line - arc shown below, the ordinary method is used.

θ = 0°

ME33018R1000800080006

SECTION 6 OFFSET FUNCTIONS

2-3-2. Obtusely Angled Corner - Outside Cutting (90° ≤ θ ≤ 180°)

(1) Straight line - Straight line

(2) Straight line - Arc

5228-E P-65

ME33018R1000800090001

(3) Arc - Straight line

(4) Arc - arc

ME33018R1000800090002

ME33018R1000800090003

ME33018R1000800090004

2-3-3. Acutely Angled Corner - Outside Cutting (θ < 90°)

(1) Straight line - Straight line

(2) Straight line - Arc

5228-E P-66

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800100001

(3) Arc - Straight line

ME33018R1000800100002

ME33018R1000800100003

(4) Arc - arc

2-3-4. Inside Cutting, with Failure to Find Cross Point

As shown in the illustration below, there may be situations in which a cross point exists with a small compensation amount (D1), but not with a large compensation amount (D2). In this case, an alarm occurs and operation stops. In the single block mode, the alarm occurs in the block which precedes the one which will cause the alarm state. In other modes, the alarm occurs several blocks before the block causing the “no cross point” condition.

5228-E P-67

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800100004

Alarm stop (in the single block mode)

ME33018R1000800110001

2-4. Tool Movement when Cutter Radius Compensation is Canceled

[Function] When the following commands are executed in the cutter radius compensation mode, the cutter radius compensation cancel mode is set. [Programming format] G40 G00 (G01) Xp__ Yp__ The axis movement mode for canceling the cutter radius compensation mode must be either G00 or G01.

2-4-1. Inside Cutting (θ ≥ 180°)

(1) Straight line - Straight line

(2) Arc - Straight line

5228-E P-68

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800130001

2-4-2. Obtusely Angled Corner - Outside Cutting (90° ≤ θ ≤ 180°)

(1) Straight line - Straight line

(2) Arc - Straight line

ME33018R1000800130002

ME33018R1000800140001

ME33018R1000800140002

2-4-3. Acutely Angled Corner - Outside Cutting (θ < 90°)

(1) Straight line - Straight line

(2) Arc - Straight line

5228-E P-69

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800150001

ME33018R1000800150002

(3) Exception

Outside cutting at an acute angle of 1 degree or less is considered to be “inside” as shown below.

ME33018R1000800150003

2-4-4. Independent G40 Command

G40 given independently will position the axes at a point shifted in the vertical direction by an amount equivalent to the compensation amount (D) from the position specified in the preceding block. Straight line

5228-E P-70

SECTION 6 OFFSET FUNCTIONS

Stops two times in the single block mode

2-4-5. Cancel with Imaginary Approach Direction

If the block which cancels the cutter radius compensation mode includes any I__, J__, or K__ belonging to the offset plane (I__, J__ in the case of G17 plane), the axes move to the target point specified in this block from the direction defined by I__ and/or J__. In this case, note that the cross point is always calculated regardless of whether the cutting is “inside” or “outside”.

Imaginary approach direction

G41 X__Y__

•

G40

N6 G41 X10000 N7 G40 X20000 Y5000I-1J-1

ME33018R1000800160001

Imaginary approach direction

N6 G41 X10000 N7 G40 X20000 Y5000I1J-1

ME33018R1000800170001

5228-E P-71

SECTION 6 OFFSET FUNCTIONS

If no cross point exists, positioning is executed to the point obtained by a vertical shift by the compensation amount from the target point specified in the block immediately preceding the G40 block.

N6 G41 X10000 N7 G40 X20000 Y5000I1J0

ME33018R1000800170002

2-5. Changing Compensation Direction in Cutter Radius Compensa-

tion Mode

• The direction of compensation may be changed even in the cutter radius compensation mode

by executing G41 or G42 or by reversing the sign (plus or minus) of the compensation amount.

G Code

G41

G42

Offset to left

(cutting left side)

Offset to right

(cutting right side)

Positive/Negative Sign

Offset to right

(cutting right side)

Offset to left

(cutting left side)

• Execution conditions

Mode Command

G41 G41 Not valid

G42 G42

G41 G42 G42 G41

When changing the offset direction, there are no distinctions between inside and outside cutting, but there are differences depending on whether or not a cross point exists. The following descriptions assume that the compensation amount is positive.

Straight line -

Straight line

(When the plus or minus sign of the offset amount is not

Straight line -

Arc

Executable Alarm if no cross point exists

Arc - Straight

changed)

line

Arc - Arc

2-5-1. With Cross Point

(1) Straight line - Straight line

(2) Straight line - Arc

5228-E P-72

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800190001

(3) Arc - Straight line

(4) Arc - Arc

ME33018R1000800190002

ME33018R1000800190003

ME33018R1000800190004

2-5-2. Without Cross Point

(1) Straight line - Straight line

(2) Straight line - Arc

5228-E P-73

SECTION 6 OFFSET FUNCTIONS

ME33018R1000800200001

2-5-3. Circular Arc Forming an Overlapping Circle

If an overlapping circle (exceeding a full circle) is generated as the result of offset direction change, the tool will move along a shorter arc to reach the target point. To avoid this, the circular arc should be divided.

ME33018R1000800200002

ME33018R1000800210001

2-6. Cutter Radius Compensation Type A

2-6-1. Overview

Programs are often created using hypothetical cutter radius first and then used by setting the cutter radius compensation for the difference between the hypothetical and actual cutter radiuses. In the OSP system, cutting direction is determined by the sign for the cutter radius compensation value. However, over cutting error may result if cutting direction differs after difference between the hypothetical and actual cutter radiuses are set. This over cutting error is rather obvious at the beginning and the end of the compensation. Set the following parameter to prevent the cutting errors at the beginning and the end of the compensation.

2-6-2. Parameter

Conventional tool movement at the beginning of cutter radius compensation (G41/G42) and the end of it (G40) is referred to as "Type B". Tool movement at the beginning and end of cutter radius compensation in this section is referred to as "Type A". No difference between these two types occurs in the exception handling as in a case of outside cutting at an acute angle of 1° or less and machining with an imaginary approach direction. No difference occurs in the machine movement during cutter radius compensation mode as well.

5228-E P-74

SECTION 6 OFFSET FUNCTIONS

Following NC optional parameter is to switch Type A and B.

NC optional parameter bit

NO. Bit Contents

79 4 Selects type of tool movement at the beginning and end

of cutter radius compensation.

Type A Type B

(Conventional

specification)

Default setting is Type B.

SECTION 6 OFFSET FUNCTIONS

2-6-3. Tool Movement at the Beginning of Cutter Radius Compensation

Inside cutting θ ≥ 180°

Tool moves to the position of the vector vertical to the next command's origin irrespective of cutter radius compensation types.

(1) Straight line - Straight line

Single block stop point

Linear motion

Circular motion

Tangent to an arc

Cutter radius compensation amount

Angle at the workpiece side

Cross point, made when a programmed path (or the tangent to an arc) is shifted

by a compensation amount Programmed tool path

Tool center path

Auxiliary line

5228-E P-75

(2) Straight line - Arc

ME33018R1000800240001

ME33018R1000800240002

5228-E P-76

SECTION 6 OFFSET FUNCTIONS

Obtusely Angled Corner - Outside Cutting (90° ≤ θ < 180°)

In Type B, as is conventionally done, the tool detours by calculating an extension point as shown below.

(1) Straight line - Straight line

ME33018R1000800240003

(2) Straight line - Arc

ME33018R1000800240004

In Type A, the tool moves to the position of the vector vertical to the next command's origin as shown below.

(1) Straight line - Straight line

ME33018R1000800240005

(2) Straight line - Arc

ME33018R1000800240006

5228-E P-77

SECTION 6 OFFSET FUNCTIONS

Acutely Angled Corner - Outside Cutting (θ < 90°)

In Type B, as is conventionally done, the tool detours by calculating an extension point as shown below.

(1) Straight line - Straight line

ME33018R1000800240007

(2) Straight line - Arc

ME33018R1000800240008

In Type A, the tool moves to the position of the vector vertical to the next command's origin as shown below.

(1) Straight line - Straight line

ME33018R1000800240009

(2) Straight line - Arc

ME33018R1000800240010

SECTION 6 OFFSET FUNCTIONS

2-6-4. Tool Movement at the End of Cutter Radius Compensation

Inside cutting θ ≥ 180°

Tool moves to the position of the vector vertical to the previous command's end irrespective of cutter radius compensation types.

(1) Straight line - Straight line

(2) Straight line - Arc

5228-E P-78

ME33018R1000800250001

ME33018R1000800250002

5228-E P-79

SECTION 6 OFFSET FUNCTIONS

Obtusely Angled Corner - Outside Cutting (90° ≤ θ < 180°)

In Type B, as is conventionally done, the tool detours by calculating an extension point as shown below.

(1) Straight line - Straight line

ME33018R1000800250003

(2) Straight line - Arc

ME33018R1000800250004

In Type A, the tool moves to the position of the vector vertical to the previous command's end as shown below.

(1) Straight line - Straight line

ME33018R1000800250005

(2) Straight line - Arc

ME33018R1000800250006

5228-E P-80

SECTION 6 OFFSET FUNCTIONS

Acutely Angled Corner - Outside Cutting (θ < 90°)

In Type B, as is conventionally done, the tool detours by calculating an extension point as shown below.

(1) Straight line - Straight line

ME33018R1000800250007

(2) Straight line - Arc

ME33018R1000800250008

In Type A, the tool moves to the position of the vector vertical to the previous command's end as shown below.

(1) Straight line - Straight line

ME33018R1000800250009

(2) Straight line - Arc

ME33018R1000800250010

SECTION 6 OFFSET FUNCTIONS

2-7. Notes on Cutter Radius Compensation

2-7-1. Specifying the Cutter Radius Compensation Amount

• The compensation amount is specified as a D command. A D command is usually specified

with G41 or G42 in the same block. If no D command is included in a G41 or G42 block, the previously specified D command is used.

• The range of cutter radius compensation numbers is from D00 to D100 for the standard

specification, and this can be expanded to D200 or D300. The compensation amount of D00 is “0”. The compensation data is set in the tool data setting mode.

2-7-2. Changing the Compensation Amount

If the compensation amount is changed in the compensation mode, the new compensation amount becomes valid starting at the end of the block in which the new compensation amount is specified.

5228-E P-81

N1 G41 X__Y__D1

•

N6 Xa1 Yb1 N7 Xa2 D2 N8 Xa3 Yb3

2-7-3. Actual Position Data Display

For the present position display, the coordinate value of the tool center is displayed.

2-7-4. Inside Cutting of an Arc Smaller than the Cutter Radius

An alarm occurs and operation stops if the inside of an arc that is smaller than the cutter radius is going to be cut. In the single block mode, operation stops at the end point two blocks ahead of the block which specifies such an operation, and in other modes, operation stops several blocks ahead.

ME33018R1000800270001

ME33018R1000800290001

2-7-5. Under-cutting

Under-cutting may occur when cutting a step with a height smaller than the cutter radius.

5228-E P-82

SECTION 6 OFFSET FUNCTIONS

2-7-6. Cautions on Corner Cutting

• When cutting an outside corner, a polygonal tool path is generated. The axis move mode and

feedrate at the corners will follow the commands specified in the next block. If the interpolation mode in the next block is either G02 or G03, the tool moves in the G01 mode along the generated polygonal tool path.

Under-cutting

Axis movement for this inserted path is controlled by the command (F800) specified in N5.

N4 X__Y__ N5 Z__ N6 X__Y__

Z-axis movement is executed at point S

F500 F800

ME33018R1000800300001

ME33018R1000800310001

5228-E P-83

SECTION 6 OFFSET FUNCTIONS

• If the tool path inserted to cut a corner is very small (∆Vx ≤ ∆V and ∆Vy ≤ ∆V in the illustration),

the second point defining this movement is disregarded.

The second point defining extra movement is disregarded if ∆Vx ∆V and ∆Vy ∆V.

≤

∆V value: Set for COMPENSATION

VECTOR CHECK of NC optional parameter (CUTTER R COMPENSATION )

In this manner, the additional minute axis movement may be reduced. Note that this processing is not executed when the next block forms a full circle.

≤

ME33018R1000800310002

In the illustration shown above, correct movement should be as follows:

1) P0 - P1 - P2 Straight line

2) P2 - P3

Straight line

3) From point P3 Full circle However, if the movement from point P2 to point P3 is disregarded due to the minute movement processing, the movement up to point P3 is as follows:

1) P0 - P1 - P2 Straight line

2) P2 - P3 Arc Thus, the program generates a minute arc from P2 to P3 and disregards the full circle that should be generated after P3.

ME33018R1000800310003

2-7-7. Interference

[Supplement]

Interference refers to problems in which a cutting tool over-cuts or makes too deep a cut into a workpiece. The NC always monitors and checks the occurrence of interference. The NC judges interference to have occurred in the following case: When the difference between the direction of the programmed path and that of the path resulting from cutter radius compensation is between 90° and 270°. It is therefore possible that conditions that do not cause interference are regarded as interference and conditions that actually cause interference are regarded as an interference-free state. When a corner is cut along a polygonal tool path, each corner can be formed by up to four points. To check for interference, two corners, P1, P2, P3, P4 and P5, P6, P7, P8, are evaluated. Interference checks are made sequentially; the first interference check is made between the last point of a corner (P4) and the first point of the next corner (P5). If an interference is found, the point is disregarded and the next point is checked. If no interference is found halfway through the procedure, the interference check is not executed for the later points. The movement mode during the check is straight line movement. For the circular interpolation block, axes move along the inserted polygonal path in the G01 linear interpolation mode. If an interference remains after all points have been checked, an interference alarm occurs, but the very last point is not disregarded. As a result, over-cut can occur if the program is executed in the single block mode.

5228-E P-84

SECTION 6 OFFSET FUNCTIONS

How the interference check is executed is explained below using several examples.

(1) Interference not found

In this example, no interference is found in the first check (N4 → N5 and P4 → P5). Therefore, no checks are made on the later points and the interference is not discovered.

Although direction P3-P6 is reversed, this is not checked since there is no interference in the check on P4-P5.

ME33018R1000800320001

5228-E P-85

SECTION 6 OFFSET FUNCTIONS

(2) Interference check resulting in a path change

In this example, the following directions of movement are checked and disregarded because interference is discovered: N4 - N5, P4 - P5, P3 - P6 and P2 - P7. However, since interference is not found in the check on P1 - P8, the tool moves along this path (P1 - P8) in the G01 mode.

ME33018R1000800320002

(3) Interference check resulting in an alarm

In this example, each corner has only one point and point P1 remains and is not disregarded. In the single block mode, an alarm occurs and operation stops after positioning is executed at P1. In other operation modes, an alarm occurs and operation stops several blocks ahead of the block causing positioning at P1.

ME33018R1000800320003

(4) Non-interference considered interference

In this example, if N4-N5 is smaller than the cutter diameter, no interference will take place. However, since the direction of P4-P5 is opposite to that of N4-N5, an interference alarm occurs.

ME33018R1000800320004

5228-E P-86

SECTION 6 OFFSET FUNCTIONS

(5) Minute arc and quasi-full circle

A minute arc is defined as an arc in which the horizontal and vertical distances from start to end point is smaller than the value set at ERROR DATA RESULTING FROM CUTTER R COMP. CAL. of NC optional parameter (cutter R compensation). A quasi-full circle is defined as an arc which is close to a full circle; the horizontal and vertical distances of the break is smaller than the value set at ERROR DATA RESULTING FROM CUTTER R COMP. CAL. of NC optional parameter (cutter R compensation).

Minute arc

Quasi-full circle

ME33018R1000800320005

Here, Assume that ∆X ≤ ∆Y and ∆Y ≤ ∆V. ∆V: Set at ERROR DATA RESULTING FROM CUTTER R COMP. CAL. of NC optional parameter (cutter R compensation).

5228-E P-87

SECTION 6 OFFSET FUNCTIONS

For these two types of arcs, special interference checks are provided. “Problem” conditions detected in minute arcs and quasi-full circles by an interference check are not considered interference, but are regarded as operational errors. In the case of a minute arc, the end point is disregarded and the shape is regarded as a point; no movements along an arc are executed. In the case of a quasi-full circle, the end point is disregarded and the shape is processed as a full circle.

P2 is disregarded and circular interpolation is not executed.

Minute arc

Quasi-full Circle

P2 is disregarded and a full circle from P1 is formed.

ME33018R1000800320006

2-7-8. Manual Data Input

• If the cutter radius compensation mode is set while in the MDI mode, or if the MDI mode is set

in the cutter radius compensation mode, execution of a block of commands including an axis movement command is not allowed immediately after their input from the keyboard. In this case, the commands of the next axis movement must be input before executing the presently input commands. Alternatively, instead of inputting the next axis movement commands, inputting four successive blocks of commands not including axis movements also allows the execution of the presently input commands.

• In automatic operation with single block function OFF, if the mode is changed to the MDI mode,

the program is executed up to the block immediately ahead of the block that has been read to the buffer (the line identified by a “>>” symbol on the screen) and then operation stops. The commands input in the MDI mode are read next to the block in the buffer, then the cutter radius compensation function is executed.

5228-E P-88

SECTION 6 OFFSET FUNCTIONS

Stop

MDI input

ME33018R1000800330001

Example: Suppose that the MDI mode is established while block N1 is being executed. If the screen displays the program shown in Fig. 1, operation stops after block N4 is executed. After the operation is stopped, the screen displays the program as shown in Fig. 2.

•

• N1 X10 N2 Y30 N3 X30 N4 Y-30 N5 X50 N6 X80 Y10 N7 X100

•

Fig. 1 Fig. 2

•

• N1 X10 N2 Y30 N3 X30 N4 Y-30 N5 X50 N6 X80 Y10 N7 X100

•

ME33018R1000800330002

When the commands of block N56 are input from the keyboard and the CYCLE START button is pressed, block N5 is executed and then operation stops. If the operation mode is returned to an automatic mode and the CYCLE START button is pressed, blocks are executed in the order N56, N6", then N7.

okuma OSP-P200M, OSP-P200MA, OSP-P20M, OSP-P200M-R, OSP-P200MA-R Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTIONS

1. Precautions Relating to Installation

2. Points to Check before Turning on the Power

3. Precautions Relating to Operation

4. Precautions Relating to the ATC

5. On Finishing Work

6. Precautions during Maintenance Inspection and When Trouble Occurs

7. General Precautions

8. Symbols Used in This Manual

INTRODUCTION

SECTION 1 PROGRAM CONFIGURATIONS

1. Program Types and Extensions

2. Program Name

3. Sequence Name

4. Program Format

4-1. Word Configuration

4-2. Block Configuration

4-3. Program

4-4. Programmable Range of Address Characters

5. Mathematical Operation Functions

6. Optional Block Skip

7. Program Branch Function (Optional)

8. Comment Function (Control OUT/IN)

9. Message Function (Optional)

SECTION 2 COORDINATE SYSTEMS AND COORDINATE COMMANDS

1. Coordinate System

1-1. Coordinate Systems and Values

1-2. Machine Zero and Machine Coordinate System

1-3. Work Coordinate System

1-4. Local Coordinate System

2. Coordinate Commands

2-1. Numerically Controlled Axes

2-2. Unit Systems

2-3. Travel Limit Commands (G22, G23) (Optional)

2-4. Home Position Command (G30)

2-5. Absolute and Incremental Commands (G90, G91)

2-6. Coordinate Recalculation Command (G97)

1. Rapid Feed

2. Cutting Feed

2-1. Feed per Minute (G94)

SECTION 3 FEED FUNCTIONS

2-2. Feed per Revolution (G95)

2-3. F1-digit Feed Function (Optional)

2-4. F0 Command During Cutting Feed

3. Exact Stop Check Function (G09, G61, G64)

4. Automatic Acceleration and Deceleration

5. Following Error Check

6. Positioning (G00)

7. Uni-directional Positioning (G60)

8. Linear Interpolation (G01)

9. Plane Selection (G17, G18, G19)

10. Circular Interpolation (G02, G03)

11. Helical Cutting (G02, G03) (Optional)

SECTION 4 PREPARATORY FUNCTIONS

1. Dwell Command (G04)

2. Programmable Mirror Image (G62) (Optional)

3. Work Coordinate System Selection (G15, G16)

4. Work Coordinate System Change (G92)

5. Unit System Check (G20, G21) (Optional)

6. Coordinate System Conversion Functions

6-1. Parallel Shift and Rotation of Coordinate Systems (G11, G10)

6-2. Copy Function (COPY, COPYE)

7. Workpiece Geometry Enlargement / Reduction Function (G51, G50) (Optional)

SECTION 5 S, T, AND M FUNCTIONS

1. S Code Function

2. T Code Function

3. M Code Function

3-1. Examples of M Codes

SECTION 6 OFFSET FUNCTIONS

1. Tool Length Offset Function (G53 - G59)

2. Cutter Radius Compensation (G40, G41, G42)

2-1. Cutter Radius Compensation Function

2-2. Tool Movement in Start-up

2-3. Tool Movement in Cutter Radius Compensation Mode

2-4. Tool Movement when Cutter Radius Compensation is Canceled

2-6. Cutter Radius Compensation Type A