okuma OSP-P200L, OSP-P20L, OSP-P200L-R, OSP-P20L-R Programming Manual

Download

CNC SYSTEM

OSP-P200L/P20L OSP-P200L-R/P20L-R

PROGRAMMING MANUAL

(3rd Edition)

Pub No. 5238-E-R2 (LE33-013-R3) Aug. 2007

5238-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.

5238-E P-(ii)

SAFETY PRECAUTIONS

3. Precautions Relating to Manual/Continuous Operation

(1) Follow the instruction manual during operation.

(2) Do not operate the machine with the front cover, chuck cover, or another protective cover

removed.

(3) Close the front cover before starting the machine.

(4) When machining the initial workpiece, check for machine operations, run the machine under no

load to check for interference among components, cut the workpiece in the single block mode, and then start continuous operation.

(5) Ensure your safety before rotating the spindle or moving a machine part.

(6) Do not touch chips or workpiece while the spindle is rotating.

(7) Do not stop a rotating part with hand or another means.

(8) Check that the condition of hydraulic chuck jaws as mounted, operating pressure, and

maximum permissible revolving speed.

(9) Check the condition and location of the cutting tool as mounted.

(10) Check the tool offset value.

(11) Check the zero offset value.

(12) Check that the SPINDLE OVERRIDE and FEEDRATE OVERRIDE dials on the NC operation

panel are set to 100%.

(13) When moving the turret, check the software limits for X- and Z-axes or the locations of limit

switch dogs to prevent interference with the chuck and tailstock.

(14) Check the location of the turret.

(15) Check the location of the tailstock.

(16) Cut workpieces with a transmitted power and torque within the permissible range.

(17) Chuck each workpiece firmly.

(18) Check that the coolant nozzle is properly located.

4. 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.

5238-E P-(iii)

SAFETY PRECAUTIONS

5. 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 maitenance 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.

6. General 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.

5238-E P-(iv)

SAFETY PRECAUTIONS

(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.

7. 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

5238-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.

5238-E P-(i)

INTRODUCTION

Thank you very much for purchasing our numerical control unit. Before using this NC unit (hereafter simply called NC), thoroughly read this programming manual (hereafter called this manual) in order to ensure correct use. This manual explains how to use and maintain the NC so that it will deliver its full performance and maintain accuracy over a long term. You must pay particular attention to the cautions given in this manual, read them carefully, and make sure you fully understand them before operating the NC.

Display Screens

The NC display screens vary with the selected NC specifications. The screens shown in this manual, therefore, may not exactly the same with those displayed on your NC.

5238-E P-(i)

TABLE OF CONTENTS

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

1. Program Types ........................................................................................................................ 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............................................................................................................................ 4

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

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

6. Block Delete............................................................................................................................. 8

7. Comment Function (CONTROL OUT/IN) ................................................................................ 8

8. Program Storage Memory Capacity ........................................................................................ 9

9. Variable Limits ......................................................................................................................... 9

10.Determining Feedrate for Cutting along C-Axis ..................................................................... 10

10-1.Cutting by Controlling the C-axis Only........................................................................... 10

10-2.Cutting by Controlling Both C-axis and Z-axis Simultaneously ..................................... 11

10-3.Cutting by Controlling Both C-axis and X-axis Simultaneously ..................................... 12

10-4.Cutting by Simultaneous 3-axis Control of X-, Z-, and C-axis ....................................... 14

SECTION 2 COORDINATE SYSTEMS AND COMMANDS ......................................16

1. Coordinate Systems .............................................................................................................. 16

1-1. Coordinate Systems and Values .................................................................................... 16

1-2. Encoder Coordinate System........................................................................................... 16

1-3. Machine Coordinate System .......................................................................................... 16

1-4. Program Coordinate System .......................................................................................... 16

2. Coordinate Commands.......................................................................................................... 18

2-1. Controlled Axis ............................................................................................................... 18

2-2. Commands in Inch System............................................................................................. 20

2-3. Position of Decimal Point................................................................................................ 20

2-4. Absolute and Incremental Commands (G90, G91) ........................................................ 22

2-5. Diametric and Radial Commands................................................................................... 23

SECTION 3 MATH FUNCTIONS ...............................................................................24

1. Positioning (G00)................................................................................................................... 24

2. Linear Interpolation (G01)...................................................................................................... 24

3. Circular Interpolation (G02, G03)........................................................................................... 26

4. Automatic Chamfering ........................................................................................................... 30

4-1. C-chamfering (G75)........................................................................................................ 30

4-2. Rounding (G76) ..............................................................................................................32

5238-E P-(ii)

TABLE OF CONTENTS

4-3. Automatic Any-Angle Chamfering .................................................................................. 34

5. Torque Limit and Torque Skip Function................................................................................. 36

5-1. Torque Limit Command (G29)........................................................................................ 36

5-2. Torque Limit Cancel Command (G28)............................................................................ 36

5-3. Torque Skip Command (G22) ........................................................................................ 37

5-4. Parameter Setting...........................................................................................................38

5-5. Program Example........................................................................................................... 39

SECTION 4 PREPARATORY FUNCTIONS...............................................................40

1. Dwell (G04)............................................................................................................................ 40

2. Zero Shift/Max. Spindle Speed Set (G50) ............................................................................. 41

2-1. Zero Shift ........................................................................................................................ 41

2-2. Max. Spindle Speed Set ................................................................................................. 42

3. Droop Control (G64, G65) ..................................................................................................... 42

4. Feed Per Revolution (G95).................................................................................................... 43

5. Feed Per Minute (G94).......................................................................................................... 43

6. Constant Speed Control (G96/G97) ...................................................................................... 44

SECTION 5 S, T, AND M FUNCTIONS .....................................................................45

1. S Functions (Spindle Functions)............................................................................................ 45

2. SB Code Function.................................................................................................................. 45

3. T Functions (Tool Functions)................................................................................................. 46

4. M Functions (Auxiliary Functions).......................................................................................... 47

5. M-tool Spindle Commands .................................................................................................... 51

5-1. Programming Format...................................................................................................... 51

5-2. M Codes Used for C-axis Operation............................................................................... 52

6. STM Time Over Check Function ........................................................................................... 54

6-1. Check ON Conditions ..................................................................................................... 54

6-2. S, T, M Cycle Time Setting............................................................................................. 54

6-3. Timing Chart Example .................................................................................................... 55

SECTION 6 OFFSET FUNCTION .............................................................................56

1. Tool Nose Radius Compensation Function (G40, G41, G42) ............................................... 56

1-1. General Description........................................................................................................ 56

1-2. Tool Nose Radius Compensation for Turning Operations.............................................. 56

1-3. Compensation Operation................................................................................................ 57

1-4. Nose Radius Compensation Commands (G, T Codes).................................................. 59

1-5. Data Display ................................................................................................................... 60

1-6. Buffer Operation ............................................................................................................. 61

1-7. Path of Tool Nose "R" Center in Tool Nose Radius Compensation Mode ..................... 61

1-8. Tool Nose Radius Compensation Programming ............................................................ 62

2. Cutter Radius Compensation Function.................................................................................. 90

5238-E P-(iii)

TABLE OF CONTENTS

2-1. Overview......................................................................................................................... 90

2-2. Programming .................................................................................................................. 90

2-3. Operations ...................................................................................................................... 92

SECTION 7 FIXED CYCLES .....................................................................................96

1. Fixed Cycle Functions ........................................................................................................... 96

2. Fixed Thread Cutting Cycles ................................................................................................. 97

2-1. Fixed Thread Cutting Cycle: Longitudinal (G31, G33).................................................... 97

2-2. Fixed Thread Cutting Cycle: End Face (G32) ................................................................ 99

3. Non-Fixed Thread Cutting Cycle (G34, G35) ...................................................................... 102

4. Precautions when Programming Thread Cutting Cycles ..................................................... 103

5. Thread Cutting Compound Cycle (G71/G72) ...................................................................... 109

5-1. Longitudinal Thread Cutting Cycle (G71) ..................................................................... 109

5-2. Program Example for Longitudinal Thread Cutting Compound Fixed Cycle

(G71) ............................................................................................................................ 110

5-3. Transverse Thread Cutting Compound Fixed Cycle (G72) .......................................... 111

5-4. M Code Specifying Thread Cutting Mode and Infeed Pattern ...................................... 112

5-5. Multi-thread Thread Cutting Function in Compound Fixed Thread Cutting Cy-

cle ................................................................................................................................. 125

6. Grooving/Drilling Compound Fixed Cycle............................................................................ 126

6-1. Longitudinal Grooving Fixed Cycle (G73)..................................................................... 126

6-2. Example Program for Longitudinal Grooving Compound Fixed Cycle (G73) ............... 127

6-3. Transverse Grooving/Drilling Fixed Cycle (G74) .......................................................... 128

6-4. Example Program for Transverse Grooving/Drilling Fixed Cycle (G74) ....................... 129

6-5. Axis Movements in Grooving/Drilling Compound Fixed Cycle...................................... 129

7. Tapping Compound Fixed Cycle ......................................................................................... 130

7-1. Right-hand Tapping Cycle (G77).................................................................................. 130

7-2. Left-hand Tapping Cycle (G78) .................................................................................... 131

8. Compound Fixed Cycles...................................................................................................... 132

8-1. List of Compound Fixed Cycle Commands .................................................................. 132

8-2. Basic Axis Motions ....................................................................................................... 133

8-3. Address Characters...................................................................................................... 139

8-4. M Codes ....................................................................................................................... 139

8-5. Drilling Cycle (G181) .................................................................................................... 140

8-6. Boring Cycle (G182) ..................................................................................................... 141

8-7. Deep Hole Drilling Cycle (G183) .................................................................................. 142

8-8. Tapping Cycle (G184) .................................................................................................. 144

8-9. Longitudinal Thread Cutting Cycle (G185) ................................................................... 145

8-10.Transverse Thread Cutting Cycle (G186).................................................................... 146

8-11.Longitudinal Straight Thread Cutting (G187)............................................................... 147

8-12.Transverse Straight Thread Cutting (G188) ................................................................ 148

8-13.Reaming/Boring Cycle (G189)..................................................................................... 149

8-14.Key Way Cutting (G190).............................................................................................. 150

8-15.Synchronized Tapping Cycle....................................................................................... 153

5238-E P-(iv)

TABLE OF CONTENTS

8-16.Repeat Function .......................................................................................................... 156

8-17.Tool Relieving Command in Deep-hole Drilling Cycle for Chip Discharge. ................. 156

8-18.Drilling Depth Setting (Only for drilling cycles) ............................................................ 157

8-19.Selection of Return Point............................................................................................. 160

8-20.M-tool spindle Interlock Release Function (optional)................................................... 161

8-21.Other Remarks ............................................................................................................ 161

8-22.Program Examples ...................................................................................................... 162

SECTION 8 LATHE AUTO-PROGRAMMING FUNCTION (LAP)............................167

1. Overview.............................................................................................................................. 167

2. G Codes Used to Designate Cutting Mode (G80, G81, G82, G83) ..................................... 168

3. List of Cutting Modes........................................................................................................... 169

4. Code and Parameter Lists................................................................................................... 174

5. Bar Turning Cycle (G85)...................................................................................................... 176

6. Change of Cutting Conditions in Bar Turning Cycle (G84) .................................................. 177

7. Copy Turning Cycle (G86)................................................................................................... 178

8. Finish Turning Cycle (G87).................................................................................................. 179

9. Continuous Thread Cutting Cycle (G88).............................................................................. 180

10.AP Modes ............................................................................................................................ 181

10-1.AP Mode I (Bar Turning).............................................................................................. 181

10-2.AP Mode II (Copy Turning).......................................................................................... 190

10-3.AP Mode III (Continuous Thread Cutting Cycle) ......................................................... 196

10-4.AP Mode IV (High-speed Bar Turning Cycle).............................................................. 197

10-5.AP Mode V (Bar Copying Cycle) ................................................................................. 214

11.Application of LAP Function................................................................................................. 232

SECTION 9 CONTOUR GENERATION ..................................................................235

1. Contour Generation Programming Function (Face) ............................................................ 235

1-1. Function Overview........................................................................................................ 235

1-2. Programming Format.................................................................................................... 235

1-3. Programming Examples ............................................................................................... 236

1-4. Supplementary Information .......................................................................................... 244

2. Contour Generation Programming Function (Side) ............................................................. 247

2-1. Overview....................................................................................................................... 247

2-2. Programming Format.................................................................................................... 248

2-3. Cautions ....................................................................................................................... 248

SECTION 10COORDINATE SYSTEM CONVERSION............................................251

1. Function Overview............................................................................................................... 251

2. Conversion Format .............................................................................................................. 252

3. Program Examples ..............................................................................................................252

4. Supplementary Information.................................................................................................. 254

5238-E P-(v)

TABLE OF CONTENTS

SECTION 11PROGRAMMING FOR SIMULTANEOUS 4-AXIS CUTS (2S

Model) ..................................................................................................255

1. Programming ....................................................................................................................... 255

1-1. Turret Selection ............................................................................................................255

1-2. Synchronization Command (P Code) ........................................................................... 256

1-3. Waiting Synchronization M Code (M100) for Simultaneous Cuts................................. 257

2. Programming Format........................................................................................................... 258

3. Precautions on Programming Simultaneous 4-axis Cuts .................................................... 260

4. Programming Example ........................................................................................................ 262

4-1. Program Process Sheet ............................................................................................... 264

SECTION 12USER TASK ........................................................................................265

1. Overview.............................................................................................................................. 265

2. Types of User Task Function............................................................................................... 266

2-1. Relationship Between Types of Program Files and User Task Functions.................... 266

2-2. Comparison of User Task 1 and User Task 2 .............................................................. 266

2-3. Fundamental Functions of User Task........................................................................... 268

3. User Task 1 ......................................................................................................................... 269

3-1. Control Statement Function 1....................................................................................... 269

3-2. Variables....................................................................................................................... 272

3-3. Arithmetic Operation Function 1 ................................................................................... 286

4. User Task 2 ......................................................................................................................... 287

4-1. Control Functions 2 ...................................................................................................... 287

4-2. I/O Variables................................................................................................................. 297

4-3. Arithmetic Operation Function 2 ................................................................................... 298

5. Supplemental Information on User Task Programs............................................................. 301

5-1. Sequence Return in Program Using User Task ........................................................... 301

5-2. Data Types, Constants ................................................................................................. 301

5-3. Types/Operation Rules of Variables and Evaluation of Their Values ........................... 302

6. Examples of User Task Programs ....................................................................................... 305

SECTION 13SCHEDULE PROGRAMS...................................................................315

1. Overview.............................................................................................................................. 315

2. PSELECT Block................................................................................................................... 316

3. Branch Block........................................................................................................................ 318

4. Variables Setting Block........................................................................................................ 318

5. Schedule Program End Block.............................................................................................. 319

6. Program Example................................................................................................................ 319

SECTION 14OTHER FUNCTIONS..........................................................................321

1. Direct Taper Angle Command ............................................................................................. 321

2. Barrier Check Function........................................................................................................323

5238-E P-(vi)

TABLE OF CONTENTS

2-1. General Description...................................................................................................... 323

2-2. Chuck Barrier and Tailstock Barrier.............................................................................. 323

3. Operation Time Reduction Function.................................................................................... 326

4. Turret Unclamp Command (for NC Turret Specification)..................................................... 326

5. SPINDLE SPEED VARIATION CONTROL FUNCTION...................................................... 327

5-1. Outline .......................................................................................................................... 327

5-2. Method of Spindle Speed Variation Control ................................................................. 327

5-3. Control Specifications................................................................................................... 327

5-4. Programming Example ................................................................................................. 330

SECTION 15APPENDIX ..........................................................................................331

1. G Code Table ...................................................................................................................... 331

2. Table of Mnemonic Codes................................................................................................... 337

3. Table of System Variables................................................................................................... 345

SECTION 1 PROGRAM CONFIGURATIONS

1. Program Types

For OSP-P200L, three kinds of programs are used: schedule programs, main programs, and subprograms. The following briefly explains these three kinds of programs.

Schedule Program

When more than one type of workpiece is machined in continuous operation using a bar feeder or other 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 14, "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.

5238-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 13, USER TASK.

• Program file format

Main file name: Max. 16 alphanumeric characters starting with an alphabet Extension: Max. 3 alphabetic characters

••• .

ExtensionMain file name

LE33013R0300300010001

• Extensions

SDF : Schedule program file MIN : Main program file SSB : System subprogram file SUB : User subprogram file

2. Program Name

With the OSP-P200L, programs are called and executed by designating the program name or program number assigned to the beginning of individual programs. This simplifies programs. A program name that contains only numbers is called a program number.

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.

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

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

5238-E P-2

SECTION 1 PROGRAM CONFIGURATIONS

• The program name assigned to a subprogram must begin with address character "O", but this

is not mandatory for main programs.

• 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

• Do not assign the same name to more than one program, otherwise it will not be possible to

select the intended program.

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 numbers is called a sequence number.

Sequence Name Designation

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

•

• Up to four characters can be used.

• 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.

• A sequence name must be placed at the top of block. However, a block delete command may

be placed preceding a sequence name.

• Sequence numbers may be specified in any order. They can be used however desired,

provided there is no duplication of numbers.

5238-E P-3

SECTION 1 PROGRAM CONFIGURATIONS

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

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:

X-100 Z=100∗SIN[50] Z=V1+V2

Address Numerical

value

Word Word Word

• 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.

Address Formula Address Variable

5238-E P-4

SECTION 1 PROGRAM CONFIGURATIONS

LE33013R0300300040001

• Refer to SECTION 13, 3-2. "Variables" for more information on variables.

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 may contain up to 158 characters.

4-3. Program

A program consists of several blocks.

SECTION 1 PROGRAM CONFIGURATIONS

4-4. Programmable Range of Address Characters

5238-E P-5

Address Function

O Program name 0000 to 9999 same as left N Sequence name 0000 to 9999 same as left G Preparatory function 0 to 999 same as left

X, Z

I, K

D, U, W, H, L E ±99999.999 mm/rev ±9999.9999 inch/rev A, B 0 to 99999.999 deg. 0 to 9999.9999 deg.

T Tool number

S SB

QA C-axis revolution 1 to 1999 (rev.) same as left SA C-axis speed 0.001 to 20.000 min

Coordinate values (linear axis)

Coordinate values (rotary axis)

Coordinate values of center of arc Taper amount and depth of cut in fixed thread cutting cycle Shift amount in grooving cycle

Automatic programming commands

Feedrate per revolution

Feedrate per minute

Dwell time period 0.01 to 9999.99 sec same as left

Spindle speed M-tool speed

Miscellaneous function

±99999.999 mm ±9999.9999 inch

±359.999 deg. ±359.999 deg.

±99999.999 mm ±9999.9999 inch

0 to 99999.999 mm 0 to 9999.9999 inch

0.001 to 99999.999 mm/rev

0.001 to 99999.999 mm/min

6 digits 4 digits

0 to 9999 0 to 9999

0 to 511 same as left

Programmable Range

Metric Inch

0.0001 to 999.9999 inch/rev

0.0001 to 9999.9999 inch/min

same as left

-1

same as left

Remarks

Alphabetic characters available

6 digits (with nose R compensation) 4 digits (without nose R compensation)

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.

Brackets

Logical OR OR 1110 = 1010 OR 1100 Logical AND AND 1000 = 1010 AND 1100 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] Tangent TAN 1 = TAN [45] Arctangent (1) ATAN 45 = ATAN [1] (value range: -90 to 90)

Arctangent (2) ATAN2

Square root SQRT 4 = SQRT [16] Absolute value ABS 3 = ABS [-3]

Decimal to binary conversion BIN

Binary to decimal conversion BCD $25 = BCD [25] Integer implementation (rounding) ROUND 128 = ROUND [1.2763 x 102] Integer implementation (truncation) FIX 127 = FIX [1.2763 x 102] Integer implementation (raising) FUP 128 = FUP [1.2763 x 102] Unit integer implementation

(rounding) Unit integer implementation

(truncation) Unit integer implementation (raising) DFUP 13.265 = DFUP [13.26462] (See *2.) Remainder MOD 2 = MOD [17, 5] Opening bracket [ Determines the priority of an operation.

Closing bracket ]

DROUND

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

30 = ATAN 2 [1,(Square root 3)] (See *1.)

25 = BIN [$25] ($ represents a hexadecimal number.)

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

(Operations inside the bracket are performed first.)

5238-E P-6

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

by coordinate values (a, b). *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

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

Logical Operations

"a", "b", and "c" represent corresponding bits.

5238-E P-7

SECTION 1 PROGRAM CONFIGURATIONS

• 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

• 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

LE33013R0300300080001

LE33013R0300300080002

• 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

LE33013R0300300080003

LE33013R0300300080004

• 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 by rounding off, truncating, or raising the number at the first place to the right of the decimal point. (in units of microns)

6. Block Delete

5238-E P-8

SECTION 1 PROGRAM CONFIGURATIONS

LE33013R0300300080005

[Function] This function allows the operator to specify whether specific blocks are executed or ignored in automatic mode operation. Blocks preceded by "/" are ignored during automatic mode operation if the BLOCK DELETE switch on the machine operation panel is set on. If the switch is off, the blocks are executed normally. When the block skip function is activated, the entire block is ignored.

[Supplement]

• The slash "/" code must be placed at either the start of a block or immediately after a sequence

name (number). If it is placed in another position in a block, it will cause an alarm.

• The slash "/" may not be contained in the program name block.

• Blocks which contain a "/" code are also subject to the sequence search function, regardless of

the BLOCK DELETE switch position.

• The block delete function is not possible during SINGLE BLOCK mode. The succeeding block

is executed, and then the operation stops.

7. Comment Function (CONTROL OUT/IN)

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

• Comments must be parenthesized to distinguish them from general operation information.

• Comments are also subject to TV and TH checks.

Example:

N100 G00 X200 (FIRST STEP)

Comment

LE33013R0300300100001

SECTION 1 PROGRAM CONFIGURATIONS

8. Program Storage Memory Capacity

The NC uses memory to store machining programs. The memory capacity is selectable depending on the size of the machining program. For execution, a program is transferred from the memory to the operation buffer (RAM). The capacity of the operation buffer is indicated by one program capacity. If the size of the program to be executed is large, it is necessary to expand the one program capacity. The one program capacity can be selected from 320 m (1049.92 ft), 640 m (2099.84 ft.), 1280 m (4199.68 ft.), to expand program storage capacity.

9. Variable Limits

On execution of a command that specifies axis movement to a target point beyond the variable limit in the positive direction, the specified target point is replaced with the variable limit in the positive direction. For commands specifying axis movement to a target point beyond the variable limit in the negative direction, axis movement is not executed and an alarm occurs.

5238-E P-9

SECTION 1 PROGRAM CONFIGURATIONS

10. Determining Feedrate for Cutting along C-Axis

10-1. Cutting by Controlling the C-axis Only

Although it is possible to machine a workpiece by controlling the C-axis, tool movement distance in unit time (one minute) differs according to the diameter of the position to be machined because the feedrate is specified in units of deg/min. This must be taken into consideration when making a program. [Memo] To match the unit of the C-axis feed command with the X- and/or Z-axis command, the feedrate command (F) should be calculated by converting 360 into 500 mm. This conversion should also be carried out when only a C-axis command is given.

Example:

90°

200φ

50φ

5238-E P-10

90°

Axis movement distance along slot A: ⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅π × 50/4 = 39 mm

Axis movement distance along slot B: ⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅π × 200/4 = 156 mm

Therefore, if cutting is carried out at a feedrate of 100 mm per minute, the feedrate (deg/min) of the C-axis is calculated as follows:

Along slot A(deg/min)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅100/39 × 90 = 230

Along slot B(deg/min)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅100/156 × 90 = 58

Convert the unit of feed from "deg/min" into "mm/min".

Slot A: (mm/min)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅230/360 × 500 = 320 (F320)

Slot B: (mm/min)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅58/360 × 500 = 80 (F80)

LE33013R0300300130001

5238-E P-11

SECTION 1 PROGRAM CONFIGURATIONS

10-2. Cutting by Controlling Both C-axis and Z-axis Simultaneously

Example:

90°

Point A coordinate value X = 80

Z = 100

C = 120

Point B coordinate value

X = 80

Z = 50

C = 210

LE33013R0300300140001

When cutting the spiral from A to B with a two-flute end mill under the following cutting conditions, calculate the feedrate of C-axis as explained below:

Cutting conditions:

Feed per

0.05 mm

tooth M-tool speed 400 min

-1

Procedure :

1 Calculate the distance between A and B.

A development of the diagram above is indicated below.

90˚

The distance, L

1 = 80 × π ×

The distance, L

2 = 63

1, along the circumference is:

= 63 (mm)

360

2, between A and B is:

+ 502 = 80 (mm)

50 mm

LE33013R0300300140002

5238-E P-12

SECTION 1 PROGRAM CONFIGURATIONS

2 Calculate the cutting time, T, on the basis of the cutting conditions indicated above to feed the

axes along the slot.

(Feed per tooth) x (Number of teeth) x (min-1)

0.05 × 2 × 400

= 2 (min)

LE33013R0300300140003

3 Inside the computer, the distance L3 between A and B is calculated in the following manner.

X-axis travel

C-axis travel = 90° ×

= 50 mm

500 mm

360°

= 125 mm

(conversion based on 360° = 500 mm)

Therefore, the distance between A and B is calculated as below:

3 = 50

+ 125

= 135 (mm)

LE33013R0300300140004

4 The feedrate to be specified in the program is approximately calculated as below:

F =

135

= = 67.5

LE33013R0300300140005

Specify F67.5 in the program.

10-3. Cutting by Controlling Both C-axis and X-axis Simultaneously

Example:

90°

Point A coordinate value X = 80

Z = 100

C = 120

Point B coordinate value

X = 40

Z = 100

C = 210

LE33013R0300300150001

• The cutting conditions are the same as used in "Cutting by Controlling Both C-axis and Z-axis

Simultaneously".

Procedure :

1 Calculate the distance between A and B.

5238-E P-13

SECTION 1 PROGRAM CONFIGURATIONS

402+20

= 44.7 mm

LE33013R0300300150002

2 Calculate the cutting time, T, on the basis of the cutting conditions indicated above to feed the

axes along the slot.

T =

(Feed per tooth) × (Number of teeth) × (min-1)

44.7

0.05 × 2 × 400

= 1.12 min

LE33013R0300300150003

3 Inside the computer, the distance L3 between A and B is calculated in the following manner.

X-axis travel = 40 mm

C-axis travel = 90° ×

500 mm

360°

=125 mm

(conversion based on 360° = 500 mm)

Therefore, the distance between A and B is calculated as below:

+ 125

3 = 40

= 131.2 mm

LE33013R0300300150004

4 The feedrate to be specified in the program is approximately calculated as below:

131.2

F =

= = 117

1.12

Specify F117 in the program.

LE33013R0300300150005

5238-E P-14

SECTION 1 PROGRAM CONFIGURATIONS

10-4. Cutting by Simultaneous 3-axis Control of X-, Z-, and C-axis

Example:

90°

Point A coordinate value X = 80

Z = 50

C = 120

Point B coordinate value

X = 40

Z = 100

C = 210

LE33013R0300300160001

• When cutting a slot on a cone as indicated above, simultaneous 3-axis control of the X-, Z-, and

C-axis becomes necessary. The feedrate to be programmed should be calculated in the following manner. Note that the example below assumes the same cutting conditions as in 11-

2. "Cutting by Controlling Both C-axis and X-axis Simultaneously".

Procedure :

1 First, consider the development of the slot on the C-axis and X-axis. In this case, calculation of

the feedrate is possible in the same manner as in "Cutting by Controlling Both C-axis and X-

axis Simultaneously" .

The C and X-axis travel component, L2, is:

L3 = 402+ 20

= 44.7 mm

LE33013R0300300160002

SECTION 1 PROGRAM CONFIGURATIONS

2 Calculate the actual distance between A and B from L2 calculated in (1).

5238-E P-15

L4 =

44.72 + 50

= 67.1

Z-axis travel

LE33013R0300300160003

3 Calculate the cutting time T for distance L4:

(Feed per tooth) x (Number of teeth) x (min-1)

67.1

0.05 × 2 × 400

= 1.68 min

LE33013R0300300160004

4 Inside the computer, distance L5 between A and B is calculated in the following manner.

X-axis travel = 40 mm

Z-axis travel = 50 mm

C-axis travel

= 90

500 mm

365

= 125 mm

(conversion based on 360 = 500 mm)

L5 =

402+502+125

= 140.4 mm

5 The feedrate to be specified in the program is approximately calculated as below:

140.4

F =

= = 83.6

1.68

Specify F83.6 in the program.

LE33013R0300300160005

LE33013R0300300160006

5238-E P-16

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

1. Coordinate Systems

1-1. Coordinate Systems and Values

To move the tool to a target position, the reference coordinate system must be set first to define the target position, and the target position is defined by coordinate values in the set coordinate system. There are the three types of coordinate system indicated below. A program coordinate system is used for programming.

• Encoder coordinate system

• Machine coordinate system

• Program coordinate system

1-2. Encoder Coordinate System

An encoder is used to detect the position of a numerically controlled axis. The encoder coordinate system is established based on the position data output by the encoder. The position data directly output from the encoder is not displayed on the screen, and this coordinate system may be disregarded in daily operation.

1-3. Machine Coordinate System

The reference point in the machine is referred to as the machine zero and the coordinate system which has its origin at the machine zero is called the machine coordinate system. The machine zero is set for each individual machine using system parameters and it is not necessary to change the setting after the installation of the machine. If "0" is set for the encoder zero point offset (system parameter), the machine coordinate system agrees with the encoder coordinate system.

1-4. Program Coordinate System

The coordinate system used as the reference for program commands is called the program coordinate system. The position of the origin of the program coordinate system varies according to the kind of workpieces to be machined and the origin is set at the required position by setting the zero offset data. The program coordinate system used for machining a specific kind of workpiece is thus defined based on the set origin.

5238-E P-17

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

Although the origin of a program coordinate system (program zero) can be set at any position, it is usually set on the centerline of a workpiece for the X-axis and at the left end face of workpiece for the Z-axis.

Zm Zp

1 Z2

Machine coordinate system

Machine zero

Zero point of encoder

Program zero

Program coordinate system

Xd, Zd : Output value of position encoder (0: Zero point of position encoder)

Xm, Zm : Coordinate values in the machine coordinate system (0: Machine zero)

Xp, Zp : Coordinate values in the program coordinate system (0: Program zero)

X1, Z1 : Offset amount of position encoder

LE33013R0300400040001

2. Coordinate Commands

2-1. Controlled Axis

• The following table lists the addresses necessary for axis control.

Address Contents

Linear axis

Rotary axis C Rotary axis in a plane orthogonal to Z-axis

• A command used to move an axis consists of an axis address, a direction of movement, and a

target point. For the designation of a target point, two different methods are available: absolute commands and incremental commands. With absolute commands, the target point is specified using the coordinate values in the program coordinate system and with incremental commands the target point is defined by relative movement distance in reference to the actual position. For details of absolute and incremental commands, refer to "Absolute and Incremental commands".

5238-E P-18

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

Controlled axis in the direction parallel to the workpiece end face

Controlled axis in the direction parallel to the workpiece longitudinal direction.

• The basic coordinate system is a right-hand orthogonal coordinate system that is fixed on a

workpiece.

Single-saddle NC lathe

X-axis

Z-axis

Infeed direction .... X-axis

Directions of turret motion:

Lon

itudinal direction ... Z-axi

LE33013R0300400050001

Two-saddle NC lathe

5238-E P-19

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

X-axis

Turret A (upper turret)

Turret B (lower turret)

X-axis

Z-axis

Directions of turret motion:

C-axis coordinate system

Negative direction

M16 M15

C90˚

C180˚

Infeed direction

Longitudinal direction

Positive direction

C270˚

Chuck

X-axis

Z-axis

LE33013R0300400050002

(Viewed from tailstock)

LE33013R0300400050003

Rightward rotation is defined as positive direction of C-axis movement and is commanded by M15. M16 is used to specify C-axis movement in the negative direction.

2-2. Commands in Inch System

If the inch/metric switchable specification is selected, it is possible to specify dimensions in the inch unit system. Even if dimensions are specified in the inch system values in a part program, the NC processes the data on the basis of metric system values. The unit system to be selected for data input is determined according to the setting of an NC optional parameter (UNIT). The actual unit system for data input can be checked on the NC optional parameter (UNIT) screen.

[Supplement]

In the conversion from the inch system data to the metric system data, used for internal processing by the NC, real data values below the minimum input unit are rounded off. Integer data values are truncated.

2-3. Position of Decimal Point

It is possible to select the unit system of the place of a decimal point. Units of the data available with the control are shown below and the unit to be employed can be selected by entering a proper parameter data. Once the unit system of the command data is established, it applies to all numerical data to be entered, such as MDI operation and zero offset data.

5238-E P-20

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

2-3-1. Metric System

• 1 µm

• 10 µm

• 1 mm

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

2-3-2. Inch System (Inch/metric switchable specification):

• 1/10000 inch

• 1 inch

Unit Data Table (Value for data "1")

5238-E P-21

Dimension

Length:

X, Z, I, K, D, H, L,

U, W

Feed (/rev):

F, E

Feed (/min):

A, B, C

Angle:

A, B, C

Time:

F, E

Spindle

-1

min

Surface speed:

Example 1: 1 mm unit system

Commanding:

• 0.001 mm movement of X-axis X0.001

• 10 mm movement of X-axis X10

• 100.00 mm movement of X-axis X100.01

• Feedrate of 0.23456 mm/rev.

The following commands are all handed as X1 mm:

X1.0

X1.00

X1.000

Metric System Inch System

1 µm10 µm 1 mm 1/10000 inch 1 inch

0.001 (mm) 0.1 (mm) 1 (mm) 0.0001 (inch) 1 (inch)

0.001 (mm/rev) 0.01 (mm/rev) 1 (mm/rev)

0.0001 (inch/ rev)

1 (inch/rev)

0.1 (mm/min) 1 (mm/min) 1 (mm/min) 0.01 (inch/min) 1 (inch/min)

0.001 (°)0.01 (°)1 (°) 0.001 (°)1 (°)

0.01 (sec) 0.1 (sec) 1 (sec) 0.01 (sec) 1 (sec)

1 (min-1)1 (min

-1

)1 (min

-1

)1 (min

-1

)1 (min

1 (m/min) 1 (m/min) 1 (m/min) 1 (feet/min) 1 (feet/min)

F0.23456

-1

)

Example 2: 10 mm unit system

Commanding:

• 0.001 mm movement of X-axis X0.1

• 10 mm movement of X-axis X1000

• 100.010 mm movement of X-axis X10001

• Feedrate of 0.23456 mm/rev. F23.456

Example 3: 1 mm unit system

Commanding:

• 0.001 mm movement of X-axis X0.1

• 10 mm movement of X-axis X10000

• 100.010 mm movement of X-axis X100010

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

• Feedrate of 0.23456 mm/rev. F234.56

[Supplement]

For F words, numerical data smaller than the selected unit system is effective if it consists of up to eight digits.

F1.2345678 ⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅Acceptable

F100.000001⋅⋅⋅⋅⋅⋅⋅⋅⋅Alarm (9 digits)

2-4. Absolute and Incremental Commands (G90, G91)

The amount of axis movement can be expressed by either absolute commands or incremental commands.

(1) Absolute commands

Designated with G90 Commanded values are coordinate values in the program coordinate system. When the control is reset, it is in the G90 mode.

5238-E P-22

LE33013R0300400090001

(2) Incremental commands

Designated with G91 Commanded values are the travel from the actual position to the target position.

Example: (Positioning from point (1) to point (2)):

Absolute

(2)

X100 Z50

100

(1)

X50 Z150

G00 X50 Z150 (1)

X100 Z50 (2)

Incremental

G00 X50 Z150 (1)

*G91 X50 Z-100 (2) *Designate dimensional differences between points (2) and (1).

[Supplement]

1) In incremental programming, the X word should be expressed as a diameter.

2) It is not permissible to specify both G90 and G91 in the same block.

LE33013R0300400100001

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

2-5. Diametric and Radial Commands

In a turning operation, the workpiece is rotated while being is machined. Due to the nature of the turning operation, the tool cuts a circle with a radius equivalent to the distance from the center of rotation to the tool nose position. In a program, X-axis commands specify the diameter of the circle to be cut. If a command of "X100" is specified, for example, the actual position data displayed on the screen is "100" and the workpiece is machined to a cylinder of 100-mm diameter. In compound operations, commands in the X-axis direction are specified as diametric values too, although this type of operation is not a turning operation. In the coordinate conversion mode, however, the radial values (actual length in an orthogonal coordinate system) must be specified for both X- and Y-axis commands.

5238-E P-23

SECTION 3 MATH FUNCTIONS

1. Positioning (G00)

[Function] Each axis moves independently from the actual position to the target position at its own rapid feedrate. At the start and end of axis movement, it is automatically accelerated and decelerated. [Programming format] G00 X__ Z__ C__

X/Z/C : Indicates the target position for positioning operation.

[Details]

• In G00 mode positioning, execution of the commands in the next block begins only after the

positioning at the target position given in the current block is completed.

• Non-linear interpolation mode:

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

5238-E P-24

SECTION 3 MATH FUNCTIONS

Actual position

[Supplement]

The rapid feedrates of each axis are set by the machine specifications.

Target position

2. Linear Interpolation (G01)

[Function] The G01 command specifies the axes to move directly from the current position to the specified coordinate values at the specified feedrate. [Programming format] G01 X__ Z__ C__ F__

LE33013R0300500010001

X, Z, C : Target point (end point) F:Feedrate.

The specified value remains effective until updated by another value.

5238-E P-25

SECTION 3 MATH FUNCTIONS

[Supplement]

1) The feedrate becomes zero when the NC is reset.

2) The feedrate for each axis is indicated below. (Calculate feedrate for X and Z-axes as incremental values.) G01 XxZzFf Calculation of feedrates:

X-axis feedrate FX =

Z-axis feedrate FZ =

where

L3 = x2+z

x, z, f: Command values specified in a program

3. Circular Interpolation (G02, G03)

[Function] Circular interpolation can be used to generate a cutting path which follows an arc. [Programming format]

5238-E P-26

SECTION 3 MATH FUNCTIONS

G02 (G03)

X__ Z__ F__

L__

{}

I__ K__

LE33013R0300500030001

G02 : Direction of rotation : Sets clockwise rotation G03 : Direction of rotation : Sets counterclockwise rotation X, Z : G90 mode : Set the end point in the program coordinate system X, Z : G91 mode : Sets the end point in reference to the starting point

(values should include signs)

I, K : Set the distance of the center of the arc from the starting point (values should include

signs) L : Sets the radius of the arc F : Sets the feedrate

[Details]

• The two directions of rotation, clockwise and counterclockwise, are defined when viewing the Z-

X plane from the positive direction of the axis orthogonal to the plane in the right-hand orthogonal coordinate system.

GO3

GO2

LE33013R0300500030002

• The end point of an arc is defined as an absolute value or an incremental value depending on

the G90/G91 selection.

• The center of an arc is expressed by I and K, which correspond to X and Z respectively. That is,

I expresses the X coordinate value and K the Z coordinate value of the center of the arc in reference to the starting point of the arc.

5238-E P-27

SECTION 3 MATH FUNCTIONS

For I and K, signed incremental values are used regardless of the mode, G90 or G91.

X(I)

Arc end point

Arc start point

G02: Both I and K values are positive Z

1, X1 indicate the coordinate values

of the arc end point.

Arc center

Z(K)

X(I)

Arc end point

R Arc center

G03: Both I and K values are positive Z

1, X1 indicate the coordinate values of

the arc end point

Arc start point

Z(K)

LE33013R0300500030003

Determining Sign and Numeric Value of I and K Words: See the figure below. Assume the coordinate system has its origin at the arc start point. Draw a right-angled triangle taking the segment connecting the arc center and arc start point as the hypotenuse. The length of side (b), parallel to the Z-axis, is the value of the K word and that of side (c), parallel to the X-axis, is the value of the I word. Concerning the sign of these words, when side (b) lies in the positive direction of the assumed coordinate system, it is taken as a positive value and when it lies in the negative direction, it is negative. The sign of I words is determined in a similar way. That is, when side (c) lies in the positive direction of the coordinate system, the I word has a positive value and when it lies in the negative direction, the I word has a negative value.

Arc start point

K -

ID cutting

I + K -

X-axis

I +

(c)

K +

(a)

Z-axis

(b)

I -

Arc center

I - K -

IOD cutting

K -

I -

I +

K -

LE33013R0300500030004

5238-E P-28

SECTION 3 MATH FUNCTIONS

• Direct Radius Command

It is possible to execute circular interpolation by specifying the X and Z coordinate values of the target point and the radius of the arc instead of using I and K commands.

[Supplement]

• The G code used to call circular interpolation is G02 or G03, as when using I and K.

• The radius of the arc is expressed by an L word which must have a positive value.

• A block containing an L word without a K or I word is an arc radius command.

• When expressing an arc by its radius, the commands must contain both X and Z words.

• If either of them is omitted, an alarm results.

• If an L word is specified in a block containing I and/or K word, an alarm results.

• If the distance from the current position to the target point (end point) is larger than two times

the specified radius, an alarm results since circular interpolation cannot be performed.

• In direct arc command programming, one arc command yields two arcs; one with central angle

less than 180, and another larger than 180. The arc with central angle less than 180 is selected. To obtain the arc whose central angle is greater than 180, specify "CALRG" in the block commanding circular interpolation.

• The direct radius command programming is effective in:

LAP Tool nose radius compensation mode Subprograms

• Incremental programming mode (G91)

In direct radius command programming, the control automatically calculates the coordinates of the center of the arc, I and K, from the programmed radius L and the coordinates of the end point, X and Z, to perform circular interpolation.

The program for the example in the figure to the right is as follows. Program:

(Z2,X2)

N1 G01 X N2 G03 X2 Z2 Lr With the commands above, the arc indicated by a thick solid line is obtained.

To move the tool along the arc indicated by dashed lines, program as follows: N1 G01 X N2 G03 CALRG X2 Z2 Lr

1 Z1 F1

Center

(Z1,X1)

• Feedrates

The feedrate during circular interpolation is the feedrate component tangential to the arc.

LE33013R0300500030005

5238-E P-29

SECTION 3 MATH FUNCTIONS

[Supplement]

1) If I or K is omitted, I0 or K0 applies.

2) I and K values should be specified as radii.

3) An arc extending into two or more quadrants can be specified by the commands in a single block.

4) If either X or Z is omitted, circular interpolation is possible within one quadrant.

5) An alarm will be activated if the difference in radius between the start and end point of an arc is greater than the value set for optional parameter (OTHER FUNCTION 1) No. 6 Allowable error in circular interpolation.

4. Automatic Chamfering

When cutting a workpiece, it is often necessary to chamfer a sharp edge (either straight-line chamfering (C-chamfering) or rounding). Although such chamfering can be accomplished using conventional interpolation commands (G01, G02, G03), the automatic chamfering function permits chamfering to be done with a simple program. For chamfering at any required angle, the automatic any-angle chamfering function should be used. To use the automatic chamfering function, set "1" for optional parameter (OTHER FUNCTION 1) Auto. any-angle chamfering. If the automatic any-angle chamfering function is required, set "anyangle chamfering" for this parameter.

4-1. C-chamfering (G75)

(X120.00, Z50.00)

(X120.00, Z115.00)

5238-E P-30

SECTION 3 MATH FUNCTIONS

C (X120.00, Z120.00)

B (X110.00, Z120.00)

A (X50.00, Z120.00)

LE33013R0300500050001

To cut the contour shown above along the points A, B, D and E, program as follows: G75

G01 X120 L-5 FDD CR after positioning the cutting tool at point A. With the commands above, the cutting tool moves from point A to B and then to D, thus automatically chamfering the corner at 45 with a size of 5 mm.

G75 : Specifies C-chamfering X120 : X coordinate of Point C L-5 : Size of chamfered face

The sign is determined by the direction of axis movement; "+" when the Z-axis (X-axis) moves in the positive direction after X-axis (Z-axis) motion. "-" when the Z-axis (X-axis) moves in the negative direction after X-axis (Z-axis) motion.

When the coordinates of point E are commanded, the cutting tool moves from Point D to Point E. [Details]

• G75 is effective only in the G01 mode. If G75 is specified in another mode, it causes an alarm.

• G75 is non-modal and active only in the commanded block.

• If the axis movement dimension specified in the block calling for automatic chamfering (A - C in

the figure above) is smaller than the absolute value of the L word (B - C in the figure above), an alarm results.

• If the axis movement dimensions specified in the block calling for automatic chamfering are

zero both for X and Z, or if neither the X nor the Z value is zero in such a block, an alarm occurs. The block calling for the automatic chamfering mode can contain only one dimension word, either X or Z.

• The automatic chamfering program is effective in:

LAP Tool nose radius compensation mode

[Program example]

90.00

40.00

10.00

60.00

5238-E P-31

SECTION 3 MATH FUNCTIONS

N101

N102

N103

N104

N105

N106

G01

G75

160.00φ

X60

X100

X160

Z92

Z60

Z40

Z10

100.00φ

F0.1

F0.05 L3

60.00φ

L-2

L-5

LE33013R0300500050002

4-2. Rounding (G76)

5238-E P-32

SECTION 3 MATH FUNCTIONS

(X120.00, Z50.00)

(X120.00, Z115.00)

C (X120.00, Z120.00)

B (X110.00, Z120.00)

A (X50.00, Z120.00)

LE33013R0300500060001

To cut the contour shown above along the points A, B, D and E, program as follows: G76

G01 X120 L-5 FDD CR after positioning the cutting tool at point A. With the commands above, the cutting tool moves from point A to B and then to D, thus automatically rounding the corner to a radius of 5 mm.

G76 : Specifies rounding of a corner X120 : X coordinate of Point C L-5 : Radius of rounding circle

The sign is determined by the direction of axis movement; "+" when the Z-axis (X-axis) moves in the positive direction after the X-axis (Z-axis) motion. "-" when the Z-axis (X-axis) moves in the negative direction after the X-axis (Z-axis) motion.

When the coordinates of point E are commanded, the cutting tool moves from point D to point E. [Details]

• G76 is effective only in the G01 mode. If G76 is specified in a mode other than G01, an alarm

occurs.

• G76 is non-modal and active only in the commanded block.

• The rounding describes a 1/4 circle with the radius specified by an L word.

• If the axis movement dimension specified in the block calling for automatic chamfering (A - C in

the figure above) is smaller than the absolute value of the L word (B - C in the figure above), an alarm results.

• If the axis movement dimensions specified in the block calling for automatic chamfering are

zero both for X and Z, or if neither X nor Z value is zero in such a block, an alarm occurs. The block calling for automatic chamfering mode can contain only one dimension word, either X or Z.

• The automatic chamfering program is effective in:

LAP Tool nose radius compensation mode

[Program Example]

40.00

10.00

5238-E P-33

SECTION 3 MATH FUNCTIONS

90.00

60.00

N101

N102

N103

N104

N105

N106

G01

G76

160.00φ

X60

X100

X160

Z92

Z60

Z40

Z10

100.00φ

F0.1

F0.05 L3

L-2

L-5

60.00φ

LE33013R0300500060002

4-3. Automatic Any-Angle Chamfering

When cutting a workpiece, it is often necessary to chamfer the sharp (C-chamfer or R-chamfer) corners and edges. If chamfering is required on edges having an angle other than 90°, programming chamfering using G01, G02 and G03 commands is not easy. This automatic chamfering function can program chamfering easily. [Programming Examples]

(1) C-Chamfering (G75)

5238-E P-34

SECTION 3 MATH FUNCTIONS

I (X100, Z72.453)

H (X89.608, Z81.453)

(X60, Z90) F

(X60, Z95)

L6 L5 L6

F∆∆∆

120˚

(X60, Z114)

C (X60, Z120)

B (X48, Z120)

A (X20, Z120)

LE33013R0300500070001

N100 N110 N120 N130 N140

G00 G75 G75 G75

G01

A120

J (X100, Z30)

(X68.660, Z87,5) G

⋅ ⋅

X20 X60

X100

Z120

Z90

Z30

⋅ ⋅

With the program above, the cutting tool moves from point A to point J in the sequence A, B, D, E, G, H, I and J, thus accomplishing chamfering of B-D, E-G and H-I.

[Supplement]

Angle commands (A) are designated in reference to the Z-axis.

(2) R-Chamfering (G76)

5238-E P-35

SECTION 3 MATH FUNCTIONS

N100 N110 N120 N130 N140

G00 G76 G76 G76

J (X100, Z30)

X20

G01

X60

A120

X100

(X70, Z87.113)

(X60, Z90)

⋅ ⋅

Z120

Z90

Z30

⋅ ⋅

L10 L8

I (X100, Z73.884)

H (X92, Z80.762)

120˚

(X60, Z95.774)

F∆∆

10R

(X60, Z114)

C (X60, Z120)

B (X48, Z120)

A (X20, Z120)

LE33013R0300500070002

With the program above, the cutting tool moves from point A to point J in the sequence A, B, D, E, G, H, I and J, thus accomplishing chamfering of B-D, E-G, and H-I.

[Supplement]

With the C-chamfer function, axis movements in the G00, G01, G34 and G35 modes can be designated by simply entering an angle command A without X and/or Z coordinate data.

Example:

(X0, Z0)

-150˚

(X1, Z1)

(X2, Z2)

G00

G01X0A-150

-160˚

Z2F∆A-160

(X1, Z1) should not be designated; it is automatically generated in the NC.

LE33013R0300500070003

SECTION 3 MATH FUNCTIONS

[Supplement]

1) Both G75 and G76 are effective only in the G01 mode and if they are designated in a mode other than G01an alarm occurs.

2) If the axis movement amount is smaller than the chamfering size, an alarm occurs.

3) Chamfering is possible only at corners between two lines. Chamfering at corners between two arcs, between a line and an arc, or between an arc and a line is impossible. If chamfering at such corners is attempted, an alarm occurs.

4) The chamfering command is effective both in the LAP and nose radius compensation mode.

5) If only an angle command A is designated in G00, G01, G34, or G35 mode operations, the next axis movement command must contain A, X and Z commands so that the end point of the line commanded can be defined. If these commands are not designated and the end point cannot be defined, then an alarm occurs.

6) If chamfering commands G75 and G76 are designated without axis movement commands X and Y or if they are designated only with an A command, the control reads the commands in the next sequence to calculate the point of intersection automatically. Therefore, if the next sequence does not contain adequate data for this calculation, an alarm occurs.

5. Torque Limit and Torque Skip Function

5238-E P-36

To transfer a workpiece from the first-process chuck to the second-process chuck with multi-process models*, the end face of the second-process chuck jaws must be pushed against the workpiece for stable workpiece seating. The torque limit command and the torque skip command are used to control the torque of the second-process chuck feed servomotor and to push the workpiece with the optimal thrust. * Multi-process models include sub spindle models, opposing two-spindle models, etc.

5-1. Torque Limit Command (G29)

[Function] Prior to workpiece transfer, designate the torque limit command to control the maximum torque of the second-process chuck feed servomotor. [Program Format] G29 P D __ (Designate an axis to be fed: Z or W, for D.) [Details]

• The torque limit value is set as a percentage, taking the rated torque of the axis feed

servomotor as 100%.

• The maximum torque limit value is set for optional parameter (OTHER FUNCTION 2).

5-2. Torque Limit Cancel Command (G28)

[Function] The torque limit cancel command cancels the maximum torque limit designated with G29. When this command is designated, the axis feed motor can output its maximum output torque. [Programming format] G28

5-3. Torque Skip Command (G22)

[Programming format] G22 Z__ D__ L__ F__ PZ =__

Z : Target point (mm) D : Distance between the target point and the approaching point as an incremental value

(mm)

L : Distance between the target point and the virtual approaching point as an incremental

value (mm) F : Feedrate (mm/min or mm/rev) PZ : Preset torque value (%)

[Details]

• For the target point and the set torque value, designate the axis to be fed..

• An alarm (alarm A 1220) occurs if the preset torque value is not reached when the second-

process chuck has moved to the virtual approaching point.

• Designate a value equal to or smaller than "2.5 m/min (8.20 fpm)" for F.

5238-E P-37

SECTION 3 MATH FUNCTIONS

• Before setting a value for PZ, check the actual motor torque value** at axis feed at the feedrate

designated by F, and set a value for PZ which is larger than the actual torque value by 10%.

** Check the RLOAD value displayed on the axis data page of the CHECK DATA screen.

If the preset torque value is too small, it is reached during approaching motion, resulting in an occurrence of alarm 1219.

First-process chuck Second-process chuck

The explanation here is for a case in which a

workpiece is transferred from the first-process

chuck to the second-process chuck.

1. The second-process chuck approaches the

workpiece at feedrate F.

2. The feedrate is reduced to 1/5 of F at the

approaching point (Z - D) point).

3. The second-process chuck contacts the

workpiece at target point Z.

The servomotor is controlled so that the

second-process chuck is kept pushed

against the workpiece.

4. When the motor torque reaches the preset value,

the NC recognizes workpiece seating to be

complete, and the next program block is executed.

LE33013R0300500110001

Feedrate F → F/5

Z:Target point D : Distance between the target point and the approaching point as an incremental value L : Distance between the target point and the virtual approaching point as an incremental value

5-4. Parameter Setting

(1) Torque skip torque monitoring delay time

If motor torque monitoring is started at the start of torque skip feed designated by G22, the preset torque value could, in some cases, be exceeded on starting up the motor. To avoid this, set the torque monitoring delay time t for a parameter. Motor torque is not monitored for the time duration set for t.

Motor torque

Set torque value

5238-E P-38

SECTION 3 MATH FUNCTIONS

Time

Torque monitor OFF

Torque monitor ON

Optional parameter (OTHER FUNCTION 2)

Setting unit : 10 (ms) Setting range : 0 to 9999 Initial setting : 0

(2) Upper limit for torque skip torque limit

The upper limit for the P command value in the G29 block can be set. Optional parameter (OTHER FUNCTION 2)

Setting unit : 1 (%) Setting range : 1 to 100 Initial setting : 0

LE33013R0300500120001

5-5. Program Example

This is a program example for transferring a workpiece to the sub spindle chuck.

: G29 PW=30⋅⋅⋅⋅⋅⋅Limits the maximum torque of the sub spindle feed motor

(W-axis motor). (30 %)

G94 G22 W50 D5 L10 F1000 PW=25⋅⋅⋅⋅⋅⋅Pushes the sub spindle chuck against

the workpiece end face by torque skip

G29 PW=5⋅⋅⋅⋅⋅⋅Lowers the W-axis motor torque.

M248⋅⋅⋅⋅⋅⋅Sub spindle chuck close

M84⋅⋅⋅⋅⋅⋅Main spindle chuck open

G28⋅⋅⋅⋅⋅⋅Cancels W-axis torque limit.

G90 G00 W300⋅⋅⋅⋅⋅⋅Returns the W-axis to the retract position at the rapid feedrate.

5238-E P-39

SECTION 3 MATH FUNCTIONS

Feedrate

60 50 45

1000 mm/mim

200 mm/mim

LE33013R0300500130001

5238-E P-40

SECTION 4 PREPARATORY FUNCTIONS

G codes are used to specify particular functions which are to be executed in individual blocks. Every G code consists of the address "G" plus a 3-digit number (00 to 399)

• Effective G Code Ranges

One-shot : A one-shot G code is effective only in a specified block and is automatically canceled when program execution moves to the next block. Modal : A modal G code is effective until it is changed to another G code in the same group.

LE33013R0300600010001

• Special G Codes

The mnemonic codes of subprogram calls (G101 through GI 10, for instance) and branch instructions are called special G codes. Every special G code must be specified at the beginning of a block, not part way through a block. Note, however, that a "/" (block delete) and a sequence name may be placed before a special G code.

1. Dwell (G04)

[Function] If dwell is specified, execution of the next block is suspended for the specified length of time after the completion of the preceding block. [Programming format] G04 F__

F : Specify the length of time for which the execution of a program is suspended.

The unit of command values is determined by the selected programming unit system. For details, refer to the optional parameter (unit system). The maximum allowable length of a dwell period is 9999.99 seconds.

SECTION 4 PREPARATORY FUNCTIONS

2. Zero Shift/Max. Spindle Speed Set (G50)

2-1. Zero Shift

[Function] With the G50 code, zero offset value is automatically calculated and zero setting is carried out according to the calculated value. This feature is effective when cutting a workpiece on which the same contour is repeated. [Programming format] G50 X__ Z__ C__

X/Z/C : Specify the coordinate value to be taken as the actual position data after zero shift.

[Details] For the present X- and Z-axis position, the coordinate value specified following G50 are assigned. [Program]

N004

G00

N005

G50

N006

G00

5238-E P-41

LE33013R0300600030001

With the program above, the axes are positioned to the coordinate point (X0, Z0) by the commands in block N004 first. When the commands in N005 are executed, the coordinate system is reestablished so that (X0, Z0), where the axes have been positioned, now has the coordinate values (X1, Z1) which are specified following G50. This program shifts the origin of the coordinate system: X = X0 - X1 Z = Z0 - Z1 Provided X0 = 100 mm and X1 = 200 mm, zero offset amount is calculated as; 100 - 200 = -100 mm This amount can be checked on the screen. Dimension words in sequences N006 and after that are all referenced to the origin newly established by the commands in N005.

[Supplement]

1) Axes not specified in the block containing G50 are not subject to zero offset.

2) G50 is non-modal and active only in the programmed block. (Zero offset is calculated only in the G50 block. All dimension words after that block are referenced to the shifted new origin.)

3) When the control is reset, all zero set data are cleared and the initial zero offset data become effective.

4) No tool offset number entry is allowed in the block containing the G50 code.

2-2. Max. Spindle Speed Set

[Function] Sometimes the spindle speed must be clamped at a certain speed due to the restrictions on the allowable speed of a chuck, influence of centrifugal force on workpiece gripping force, imbalance of a workpiece, or other factors. This feature allows a maximum spindle speed to be set in such cases. [Programming format] G50 S__

S : Specify the maximum spindle speed.

[Details] Once set, the specified speed remains effective until another spindle speed is specified.

3. Droop Control (G64, G65)

[Function] The axis movements of the machine are controlled by a servo system in which the axis moves to eliminate the lag (termed DIFF or droop) between the actual tool position and the commanded coordinate. Due to existence of DIFF (servo error), the actual path does not precisely agree with the commanded tool path when cutting a sharp corner, as illustrated below: The Droop Corner Control Function is provided to eliminate or reduce such path tracing error to acceptable amounts by stopping the generation of functions (pulses) at the corner until the DIFF reaches the preset permissible droop amount.

5238-E P-42

SECTION 4 PREPARATORY FUNCTIONS

Droop

Programmed tool path

Actual tool path

LE33013R0300600050001

[Programming format]

• Droop corner control OFF command

G64 (The control is placed in the G64 mode when G64 is turned ON.)

• Droop corner control ON command

G65

[Details]

• With G65 presented, axis movement commands in G00, G01, G02, G03, G31, G32, G33, G34,

and G35 mode are completed after the DIFF amount becomes smaller than the permissible droop amount.

• The permissible droop amount can be set within a range from 0 to 1.000 mm for a user

parameter at the NC operation panel.

4. Feed Per Revolution (G95)

[Function] Specify G95 to control tool movement (feedrate) in terms of "distance per spindle revolution" for turning operations. [Programming format] G95 F__

F : Specify movement distance per spindle revolution.

The unit of setting is determined according to the setting for the optional parameter (UNIT)

[Details]

• The allowable maximum feedrate depends on the machine specifications.

• On turning on the power, and after reset, the feed per revolution mode is selected.

5. Feed Per Minute (G94)

[Function] Specify G94 to control tool movement (feedrate) in terms of "distance per minute" for turning operations. [Programming format] G94 F__

F : Specify tool movement distance per minute.

The unit of setting is determined according to the setting for the optional parameter (UNIT)

5238-E P-43

SECTION 4 PREPARATORY FUNCTIONS

[Details]

• The allowable maximum feedrate depends on the machine specifications.

SECTION 4 PREPARATORY FUNCTIONS

6. Constant Speed Control (G96/G97)

[Function] When the constant speed cutting function is selected, cutting at a constant cutting speed is possible. This feature can reduce cutting time and also assure stable finish in end face cutting operations.

Constant Speed Cutting Command

[Programming format] G96 S__

S : Set the cutting speed (setting unit: m/min)

Canceling Constant Speed Cutting

[Programming format] G97 S__

S : Set the spindle speed to be used after canceling the constant speed cutting mode.

[Program Example]

5238-E P-44

N ΟΟΟ G96 S100⋅⋅⋅⋅⋅⋅⋅All cutting following this block is executed at a cutting speed of 100 m/min.

-1

N ΟΟΟ G97 S500⋅⋅⋅⋅⋅⋅⋅After this block, cutting is carried out at a spindle speed of 500 min

LE33013R0300600080001

[Supplement]

1) If the spindle speed exceeds the maximum or minimum speed allowed within the range selected by an M code while in the constant speed cutting mode, it is fixed at the allowed maximum or minimum speed automatically; the LIMIT indication light on the operation panel goes on.

2) If the X-axis is moved a large distance at the rapid traverse rate while in the constant speed cutting mode, for example from the turret indexing position toward the workpiece or vice versa, there will be sudden changes in the rotational speed which, depending on the chucking method, could be dangerous. Therefore, the constant speed cutting mode must be cancelled before commanding positioning of the cutting tool near the workpiece, return of the tool to the turret indexing position, or any other operation that causes large X-axis travel.

3) A block containing G96 or G97 must contain an S word.

4) Thread cutting programs cannot be executed in the G96 constant speed cutting mode.

5) To activate the constant speed cutting mode on turret B, specify G111 with G96. To restore the constant speed cutting mode to turret A, specify G110.

6) To execute the commands over two blocks continuously with control in the constant speed cutting mode without waiting for the spindle speed arrived signal, specify M61. To cancel this, specify M60.

5238-E P-45

SECTION 5 S, T, AND M FUNCTIONS

This section describes the S, SB, T, and M codes that specify the necessary machine operations other than axis movement commands.

S : Spindle speed SB : Spindle speed of M-tool spindle T : Tool number, tool offset number, tool nose radius compensation number M : Miscellaneous function to control machine operation

One block can contain: one S code, one T code, and eight M codes.

1. S Functions (Spindle Functions)

[Function] By specifying number following address S, spindle speed can be specified. [Programming format] S__ [Details]

• S command range: 0 to 65535

• If there is an S command and an axis move command in the same block, the S command is

executed first and then the axis move command is executed.

• The S command will not be canceled when the NC is reset, however, it will be set to 0 when the

power supply is turned off.

• To rotate the spindle, the S command must be specified in a block that precedes the block

containing the spindle start command or in the same block.

[Supplement]

1) For a machine equipped with the transmission gears, the required gear range should be selected with the corresponding M code.

2) Spindle rotation (forward, reverse) and stop are specified by M codes.

2. SB Code Function

[Function] M-tool spindle speed is specified using address SB. [Programming format] SB = __ f an address consisting of two or more characters is used, an equal symbol must be entered before a numeric value.

• SB command range: 0 to 65535

• M-tool spindle rotation (forward, reverse) and stop are specified by M codes.

• The SB command will not be canceled when the NC is reset, however, it will be set to 0 when

the power supply is turned off.

• To rotate the M-tool spindle, the SB command must be specified in a block that precedes the

block containing the M-tool spindle start command or in the same block.

[Supplement]

1) For the machine equipped with the transmission gears for driving the M-tool spindle, the required gear range should be selected by a corresponding M code.

2) M-tool spindle rotation (forward, reverse) and stop are specified by M codes.

3. T Functions (Tool Functions)

[Function] By specifying a 4-digit number (NC without tool nose radius compensation function) or a 6-digit number (NC with tool nose radius compensation function) following address T, tool number, tool offset number, and tool nose radius compensation number are indicated. [Programming format]

TΟΟ∆∆

ΟΟ : Tool nose radius compensation number

∆∆ : Tool number (00 to 99, assuming maximum number of turret stations)

: Tool offset number

5238-E P-46

SECTION 5 S, T, AND M FUNCTIONS

LE33013R0300700040001

The setting ranges for nose radius compensation numbers and tool compensation numbers are as follows:

(1) For offset 32-set specification

• Tool offset number: 00 to 32

• Tool nose radius compensation number: 00 to 32

(if tool nose radius compensation function is supported.)

(2) For offset 64-set specification

• Tool offset number: 00 to 64

• Tool nose radius compensation number: 00 to 64

(if tool nose radius compensation function is supported.)

(3) For offset 96-set specification

• Tool offset number: 00 to 96

• Tool nose radius compensation number: 00 to 96

(if tool nose radius compensation function is supported.)

[Details] If there is a T command and an axis move command in the same block, the T command is executed first and then the axis move command is executed.

[Supplement]

The construction of the turret and its direction of rotation (forward, reverse, shorter-path) vary according to the machine specifications.

4. M Functions (Auxiliary Functions)

[Function] The M codes are used for miscellaneous ON/OFF control and sequence control of the machine operation such as spindle start/stop and operation stop at the end of program. The programmable range for M codes is from 0 to 511. [Examples of M codes] The M codes listed below are processed as special functions. For details on those M codes not listed here, refer to APPENDIX 3. "List of M Codes".

(1) M00 (program stop)

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

(2) M01 (optional stop)

When M01 is executed when 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.

(3) 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 its start. (In the case of a schedule program, execution of M02 or M30 in the main program does not reset the NC.)

5238-E P-47

SECTION 5 S, T, AND M FUNCTIONS

(4) M03, M04, M05 (spindle CW, CCW, stop)

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

(5) M12, M13, M14 (rotary tool CW, CCW, stop)

These M codes control rotary tool rotation and stop for the turning center; rotary tool stop (M12), rotary tool CW (M13), rotary tool CCW (M14).

(6) M15, M16 (C-axis positioning direction)

These M codes control the C-axis rotation direction for positioning for the turning center; C-axis positioning in the positive direction (M15), C-axis positioning in the negative direction (M16).

(7) M19 (spindle orientation)

This controls spindle orientation.

(8) M20, M21 (tailstock barrier ON, OFF)

These M codes set and cancel the tailstock barrier which generates an alarm if the tool enters the area defined by the barrier; tailstock barrier ON (M21), tailstock barrier OFF (M20).

(9) M22, M23 (chamfering ON, OFF for thread cutting)

These M codes set and cancel chamfering for thread cutting; chamfering ON (M23), chamfering OFF (M22).

(10) M24, M25 (chuck barrier ON, OFF)

These M codes set and cancel the chuck barrier which generates an alarm if the tool enters the area defined by the barrier; chuck barrier ON (M25), chuck barrier OFF (M24).

(11) M26, M27 (thread pitch axis X-axis, Z-axis)

These M codes specify the effective thread pitch axis for conventional thread cutting cycles; Xaxis pitch command (M27), Z-axis pitch command (M26).

5238-E P-48

SECTION 5 S, T, AND M FUNCTIONS

(12) M32, M33, M34 (thread cutting mode; straight, zigzag, straight (reversed))

These M codes are used to specify the thread cutting mode in the compound fixed cycle and LAP; M32 for infeed along one side of the thread face to be cut (straight), M33 for zigzag infeed, and M34 for straight infeed along the opposite thread face from the one in the M32 mode (straight (reversed)).

(13) M40, M41, M42, M43, M44 (spindle drive gear range; neutral, gear 1, gear 2, gear 3, gear 4)

These M codes are used to select the spindle drive gear range; neutral (M40), gear 1 (M41), gear 2 (M42), gear 3 (M43), and gear 4 (M44).

(14) M48, M49 (spindle speed override ignore)

When the spindle speed override ignore function is valid, the spindle speed override rate is fixed at 100% regardless of the setting of the spindle override switch. The spindle speed override ignore function is canceled by specifying the cancel M code, resetting the CNC, or changing the operation mode. < M codes >

Spindle speed override ignore⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅ M49

Spindle speed override ignore cancel⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅M48

LE33013R0300700050001

(15) M55, M56 (tailstock spindle retract, advance)

These M codes specify tailstock retract/advance operation.

(16) M60, M61 (fixed surface speed arrival ignore OFF, ON)

These M codes are used to specify whether or not a program with constant surface speed control is executed continuously without waiting for attainment of the specified surface speed; M61 specifies advance to the next block without waiting for attainment of the specified surface speed, and M60 specifies advance to the next block only after attainment of the specified surface speed.

(17) M63 (spindle rotation answer signal ignore)

The M codes relating to spindle control (M03, M04, M05, M19, M40 - M44) and S command are executed at the same time with axis move commands specified in the same block.

(18) M73, M74, M75 (thread cutting pattern 1, 2, 3)

In multi-machining fixed cycle and thread cutting cycle in LAP, the cutting pattern (infeed pattern) is specified by these M codes. M73 for pattern 1, M74 for pattern 2, and M75 for pattern 3.

(19) M83, M84 (chuck clamp, unclamp)

Regardless of the chuck clamp direction (I.D. or O.D.), the M code used to specify the clamping of a workpiece is always M83.

(20) M85 (no return to the start point after the completion of LAP roughing cycle)

In LAP4, a roughing cycle is called by G85 or G86. When this M code is specified, the cutting tool does not return to the reference point of the cycle after the completion of the called roughing cycle, and the next block is executed continuously.

(21) M86, M87 (turret clockwise rotation ON, OFF)

These M codes are used to specify whether or not the turret rotation direction is fixed in the clockwise direction; M86 specifies turret clockwise rotation ON, and M87 specifies turret clockwise rotation OFF.

5238-E P-49

SECTION 5 S, T, AND M FUNCTIONS

(22) M109, M110 (C-axis connection ON, OFF)

These M codes are used to select the spindle control mode for the multiple-process machining specification models. By specifying M110, the spindle is controlled in the C-axis control mode and by specifying M109, the control mode is returned to the spindle control mode. Note that M110 must be specified in a block without other commands.

(23) M124, M125 (STM time-over check ON, OFF)

These M codes are used to determine whether or not an alarm is generated if the counted STM execution cycle time exceeds the parameter-set time; M124 specifies that the alarm is generated, and M125 specifies that the alarm is not generated.

(24) M136 (shape definition for compound fixed cycle)

This M code is used to specify the shape for the compound fixed cycles provided for the multiple-process specification models. After the execution of the compound fixed cycle, the cutting tool returns to the start point of rapid traverse.

(25) M140 (tapping cycle rotary tool fixed speed arrived answer signal ignore)

This M code is used to ignore the tapping cycle rotary tool fixed speed arrived answer signal; by specifying this M code, the timing difference between the output of rotary tool fixed speed arrived answer signal and the start of cutting feed can be zeroed. Note that this M code is available with the multiple-process specification models.

(26) M141, M146, M147 (C-axis clamp used/not-used selection, C-axis unclamp, C-axis clamp)

For a compound fixed cycle carried out under light load on multiple-process specification models, it is not necessary to clamp the C-axis to carry out cutting. In such a case, M141 is used to select the "C-axis clamp is not used" state, thereby reducing cutting time. M146 and M147 are used to control C-axis clamping and unclamping; M146 for C-axis clamp and M147 for C-axis unclamp.

(27) M156, M157 (center work interlock ON, OFF)

When center work is selected, operation is possible only when the tailstock spindle is at the predetermined position. For chuck work, the tailstock spindle must be at the retract end position. These M codes are used to cancel the interlock function.

[Supplement]

• When the power supply is turned off or after the NC is reset, the NC is in the M156 state.

• The state selected by these M codes is effective only for MDI and automatic operation modes.

(28) M160, M161 (feedrate override fixed at 100% OFF, ON)

These M codes are used to specify whether or not the setting of the feedrate override dial, when other than 100%, is valid; in the M161 mode, if the setting of the feedrate override dial on the machine operation panel is in other than 100%, the setting is ignored and the feedrate commands are executed assuming a setting of 100%, and in the M160 mode, the setting of the feedrate override dial is valid.

(29) M162, M163 (rotary tool spindle override fixed at 100% OFF, ON)

These M codes are used to specify whether or not the setting of the rotary tool spindle speed override dial, when other than 100%, is valid; in the M163 mode, if the setting of the rotary tool spindle speed override dial on the machine operation panel is in other than 100%, the setting is ignored and the rotary tool spindle speed commands are executed assuming the setting of 100%, and in the M162 mode, the setting of the rotary tool spindle speed override dial is valid.

5238-E P-50

SECTION 5 S, T, AND M FUNCTIONS

(30) M164, M165 (slide hold and single block ignore OFF, ON)

These M codes are used to specify whether or not the slide hold ON and single block ON statuses, set by the switches on the machine operation panel, are valid; in the M165 mode, if the slide hold or single block function is set ON with the corresponding switch on the machine operation panel, these functions are made invalid, and in the M166 mode, if the slide hold or single block function is set ON by the corresponding switch on the machine operation panel, these functions are made valid.

(31) M166, M167 (tailstock spindle advance/retract interlock during spindle rotation ON, OFF)

To ensure safety, the tailstock spindle cannot normally be advanced or retracted while the spindle is rotating. However, tailstock spindle operation is permitted even while the spindle is rotating by turning OFF the interlock.

[Supplement]

• When the power supply is turned off or after the NC is reset, the NC is in the M166 state.

• The state selected by these M codes is effective only for MDI and automatic operation modes.

(32) M184, M185 (chuck open/close interlock ON, OFF)

To ensure safety, the chuck cannot normally be opened or closed while the spindle is rotating. However, chuck open/close operation is permitted even while the spindle is rotating by turning OFF the interlock.

[Supplement]

• When the power supply is turned off or after the NC is reset, the NC is in the M184 state.

• The state selected by these M codes is effective only for MDI and automatic operation modes.

• The state selected by these M codes is effective only when the door is closed.

• The chuck interlock OFF state is effective for chuck clamp/unclamp operation specified by M

codes or external commands and it is not effective for the operation using the foot pedal and pushbutton switches.

(33) M193, M194 (thread cutting phase matching control OFF, ON)

In the M194 mode, the phase offset amount at the thread cutting start point is calculated and compensation is carried out at the start and end points. After the completion of the thread cutting cycle, the M194 mode must be canceled by specifying M193 in a block without other commands.

(34) M195, M196 (thread cutting phase matching move amount valid OFF, ON)

By specifying M196 in the block preceding the block which contains the commands to stop a program for thread cutting phase matching, the amount of manual axis movement done in phase matching is stored. M196 must be specified in a block without other commands. After the completion of manual axis movement for phase matching, the M196 mode must be canceled by specifying M195 in a block without other commands.

(35) M197 (clearing thread cutting phase matching amount)

This M code is used to clear the amount which is stored as the manual axis movement amount for phase matching.

(36) M211, M212, M213, M214 (key-way cycle cutting mode; uni-directional, zigzag, specified

cutting amount, equally-divided cutting amount) M211 and M212 are used to specify the cutting direction in the key-way cutting cycle; unidirectional cutting (M211) and zigzag cutting (M212). M213 and M214 are used to specify the infeed pattern; M213 specifies the specified cutting amount and M214 specifies the equally-divided cutting amount.

(37) M241, M242 (rotary tool spindle speed range, LOW, HIGH)

These M codes are used to select the spindle speed range of the rotary tool spindle for the multiple-process specification models; low-speed range (M241), high-speed range (M242).

5. M-tool Spindle Commands

5-1. Programming Format

N001

N002

N003

N004

G00

G094

G01

X1000

X∆∆∆

X(Z)∆∆∆

Program block for rotary tool maching

Z1000

Z∆∆∆

F∆

C∆∆∆

5238-E P-51

SECTION 5 S, T, AND M FUNCTIONS

T∆∆

M110

M15(M16)

M147 M13 (M14)

SB=∆∆∆∆

N100

N101

N102

N103

G00

X(Z)∆∆∆

X1000 Z1000 M146

M109

M02

LE33013R0300700060001

[Details]

• M110 must be programmed in a block without other commands.

• It is advisable to limit the direction of rotation of the C-axis to either of the two directions, M15 or

M16, for better positioning accuracy.

• M110 and M147 cannot be reset or canceled even when the control system is reset. To cancel

them, specify M109 and M146, respectively.

• If commands relating to M-tools are specified while the C-axis is not engaged, an alarm occurs.

An alarm does not occur if the M-tool spindle interlock (optional) is designated.

5-2. M Codes Used for C-axis Operation

The following codes are necessary for programming C-axis movements.

Code Details

Used to designate the spindle to be controlled in the C-axis control mode.

M110

M109 Used for switchover from the C-axis control mode to the spindle control mode. M147 Used to clamp the C-axis.

M146

M141 C-axis clamp ineffective (compound fixed cycle mode)

M15

M16

QA =

When programming C-axis commands, first specify M110 in a block without other commands.

Used to unclamp the C-axis. The control system automatically selects the M146 mode when the power is turned on. Program M146 before starting C-axis rotation.

Used to rotate the C-axis in the positive direction.

Used to rotate the C-axis in the negative direction.

Used to specify the number of C-axis revolutions. For example, QA=5 rotates C-axis five times.

5238-E P-52

SECTION 5 S, T, AND M FUNCTIONS

M16 M15

Chuck end face

* When the NC is reset, it is placed in the M15 mode. [Example of Program]

C90

120φ

C180

Program zero

C270

100

ø15 mm hole

Tool No. : T0101

Tool : ø15 mm drill

Command point

SB = 400min

-1

LE33013R0300700070002

SECTION 5 S, T, AND M FUNCTIONS

To drill two 15 mm dia. holes, create a program as indicated below:

5238-E P-53

N099

N100

N101

N102

N103

N104

N105

N106

N107

N108

N109

N110

N111

Continued from turning operation program

G00

G94

G01

G00

G01

G00

G095

X1000

X120

X1000

Z1000

Z102

Z75

Z102

Z75

Z102

Z1000

M15

C90

F40

C270

M05

M01

M110

T0101

SB=400

M13

M147

M146

M147

M12

M146

M109

M02

Designates the spindle as the C-axis.

Indexes C-axis in the positive direction.

The spindle indexes at the 90° position in positive direction and the drill is positioned near the workpiece surface at the rapid feedrate.

(G00)

Feedrate in mm/min mode is selected.

The drill starts rotation at 400 min-1{rpm} in the leftward direction. After thespindle is clamped, 15 mm dia. hole is drilled at a feedrate of 40 mm/min.

(G01)

The drill returns to the commanded point at the rapid feedrate.

The spindle is indexed at the 270 position after it is unclamped.

The second hole is drilled after the spindle is clamped.

The M-tool stops and the turret returns to the turret index position.

LE33013R0300700070003

• Calculate the feedrate (mm/min) for drilling with the equation below:

Feedrate (mm/min) = Tool speed (rpm) x Feedrate (mm/rev) Therefore, when the tool speed is 400 min-1{rpm} and the feedrate is 0.1 mm/rev, the feedrate (mm/min) is calculated as: F = 400 x 0.1 = 40 mm/min

• When an end mill is used, its feedrate (mm/min) is calculated with the following equation:

Feedrate (mm/min) = Tool speed (rpm) Feed (mm/blade) Number of end mill blades

• Assuming an end mill with four blades (flutes) is used at 300 min-1{rpm} and a feedrate of 0.05

mm/blade, the feedrate (mm/min) is F = 300 x 0.05 x 4 = 60 mm/min

6. STM Time Over Check Function

The duration of S, T, M cycle time is measured and if the measured time exceeds the parameter-set cycle time, an alarm occurs.

6-1. Check ON Conditions

• The check function is set effective or ineffective according to the setting for a machine

parameter.

• The check function is turned on and off using the following M codes.

M124 : STM time over check start M125 : STM time over check end

6-2. S, T, M Cycle Time Setting

Set, for the machine parameter, the allowable limit of cycle time when executing an S, T, and M codes.

5238-E P-54

SECTION 5 S, T, AND M FUNCTIONS

• Parameter setting

Units : 0.1 seconds Maximum

setting

: 600 seconds

6-3. Timing Chart Example

(1) Parameter setting

Parameter: ON STM time over check start Parameter: OFF STM time over check end

STM operation in progress

Parameter

Time over check

5238-E P-55

SECTION 5 S, T, AND M FUNCTIONS

Parameter-set

cycle time

(2) M Codes

M124 : STM time over check start M125 : STM time over check end

Part program in progress

M124

M125

Alarm B

LE33013R0300700110001

Parameter-set

cycle time

Time over check

Alarm B

LE33013R0300700110002

5238-E P-56

SECTION 6 OFFSET FUNCTION

1. Tool Nose Radius Compensation Function (G40, G41, G42)

1-1. General Description

The tool tip point radius of most cutting tools used in turning operation is the cause of inconsistencies between the designated tool paths and the actually finished workpiece contour. With the tool radius compensation function, such geometric error is automatically compensated for by simple programming.

1-2. Tool Nose Radius Compensation for Turning Operations

Tool Offset and Nose Radius Compensation

In turning operations, various types and different shapes of tools are used to finish one workpiece. ID cutting tools, OD cutting tools, rough cut tools, finish cut tools, drills, etc. Accordingly, the tool nose radius compensation function has to be activated simultaneously with the tool offset function.

Nose radius compensation

Position com

ensation

LE33013R0300800020001

Tool Nose Radius Compensation at Discontinuous Point

Point A in the figure above constitutes a discontinuous point and an angle less than 180°. By using the tool nose radius compensation function, the tool path shown above can be generated by simply entering the coordinates of points A and B.

LE33013R0300800020002

1-3. Compensation Operation

Geometrical Cutting Error due to Tool Nose Radius

If cutting along paths A-B-C-D-E in the figure below is intended but the tool nose radius compensation function is not activated, the shaded portions will remain uncut and cause geometrical errors. This is because the tool setting is made to locate the imaginary cutting point P at the datum point and trace the programmed path as controlled by NC commands. However, the actual cutting tip point is not precisely located on that datum point because of the tool nose radius and this produces geometrical errors. The tool nose radius compensation function automatically compensates for the inconsistency between the designated and actual tool paths caused by the tool nose radius (see the figure below).

Nose radius

Point P

5238-E P-57

SECTION 6 OFFSET FUNCTION

Tool Setting Point

Tool Path and Resulting Error Without Tool Nose Radius Compensation

LE33013R0300800030001

5238-E P-58

SECTION 6 OFFSET FUNCTION

Compensation Movement

With the tool nose radius compensation function activated, the error in the tool path described in (1) is compensated for as shown below to finish the workpiece to the dimensions specified in a program.

Tool Path with Tool Nose Radius Compensation

LE33013R0300800030002

Nose radius compensation during LAP mode

To use the tool nose radius compensation function in the LAP mode, programs for the respective turrets must contain the tool nose radius compensation programs independently as shown below.

LAP shape designation

Nose radius

compensation

G81

G42

G40

G80

Possible

G42

G81

G40

G80

Not possible

LAP cycle call

G42

Possible

G40

G85

G42

Not possibl

G85

G40

LE33013R0300800030003

SECTION 6 OFFSET FUNCTION

1-4. Nose Radius Compensation Commands (G, T Codes)

The programming commands - G and T codes, used to activate the tool nose radius compensation function, are detailed in this section.

G Codes

G40 : Used to cancel the tool nose radius compensation mode. G41 : Tool nose radius compensation - Left

Used when the tool moves on the left side of the workpiece.

G42 : Tool nose radius compensation - Right

Used when the tool moves on the right side of the workpiece.

The term indicating the side of the workpiece, right or left, is determined according to the direction in which the tool is advancing.

G42 : Right of workpiece

X+

5238-E P-59

Z+

G41 : Left of workpiece

LE33013R0300800040001

Since G41 and G42 codes are selected to agree with the coordinate system (right-hand system) the machine employs, they should be selected as below for lathes which have a coordinate system in which the positive direction of the X-axis is directed toward the operator.

G41

Z+

X+

G42

LE33013R0300800040002

T Codes

Six numerical characters following address character "T" specify the nose radius compensation number, tool number, and tool offset number.

TΟΟ∆∆

ΟΟ: Tool nose radius compensation number

∆∆: Tool number

: Tool offset number

LE33013R0300800040003

5238-E P-60

SECTION 6 OFFSET FUNCTION

[Supplement]

To change the tool offset during the execution of tool nose radius compensation, designate the tool nose radius compensation number and the tool number.

Example:

G01

G03

G01

G03

Xa Za T010101

Xb Zb

Zd T110111

Xd Zd KI

Entry of only the tool offset No. (T01 or T11) in G code command (1) or (2) will cancel the nose radius compensation amount.

1-5. Data Display

The screen display during nose radius compensation is described here.

(1) Actual Position

Actual position data is displayed on the screen as with the conventional control system. However, the data displayed on the screen may be different from the programmed data because of the tool nose radius compensation.

......

LE33013R0300800040004

B′ B

Command point

Point indicated on display unit

LE33013R0300800050001

(2) Alarm Display

If an alarm relating to the tool nose radius compensation function occurs, the ALARM light under STATUS DISPLAY goes on and the screen displays the message indicating the alarm contents.

1-6. Buffer Operation

The NC usually operates in the 3-buffer mode. While the positioning command from point A to point B is being executed, the positioning point data of points C, D and E are read and stored in the buffer. This is called the 3-buffer function. When the tool nose radius function is activated, the target point E is calculated from straight lines DE and EF. This means that the data in the block four blocks ahead the current target point are read if the tool nose radius compensation function is active.

Fourth positioning point

5238-E P-61

SECTION 6 OFFSET FUNCTION

Reading point (four blocks ahead)

Second positioning point

Third positioning point

Data in Buffer

Immediate target point

Present tool position

LE33013R0300800060001

1-7. Path of Tool Nose "R" Center in Tool Nose Radius Compensation

Mode

To execute the motion shown below in the following program in the tool nose radius compensation mode, the path of the tool nose R center is obtained as follows:

G42

G41

N5′ N4′

X+

Z+

N3′ N2′

N3 N2

N1′

LE33013R0300800070001

5238-E P-62

SECTION 6 OFFSET FUNCTION

(1) To obtain point N2’ when the center of the tool nose R is at point N1’, proceed as follows:

• Draw a straight line parallel to the direction of tool advance, N1 - N2, offset in the specified

direction, (to the right since G42 is specified), by the tool nose radius compensation amount. This yields the straight line passing N1’ and N2’.

• Draw a straight line parallel to the direction of tool advance, N2 - N3, offset in the specified

direction, (to the right of or above N2 - N3 since G42 dominates the compensation mode) by the tool nose radius compensation amount. This yields the straight line passing N2’ and N3’.

• The nose R center for the commanded point N2’ is the point of intersection of these two

straight lines. The center of the tool nose radius advances from point N1’ to N2’.

(2) To obtain point N3’:

• Draw a straight line parallel to the direction of tool advance, N2 - N3, offset in the specified

direction, (to the right of or above N2 - N3 since G42 dominates the compensation mode), by the tool nose radius compensation amount. This yields the straight line passing N2’ and N3’.

• Draw a straight line parallel to the direction of tool advance, N3 - N4, offset in the specified

direction, (to the left since G41 is specified), by the tool nose radius compensation amount. This yields the straight line passing N3’ and N4’.

• The nose R center for commanded point N3 is the point of intersection of these two straight

lines. The center of the tool nose radius advances from point N2’ to point N3’.

(3) To obtain point N4’:

Follow the same procedure indicated above using points N3, N4 and N5.

1-8. Tool Nose Radius Compensation Programming

1-8-1. G41 and G42

The G41 and G42 codes are used to call out the tool nose radius compensation mode. Since the uses of these G codes are often confused in programming a part, this section deals with their particular differences.

G41 : This tool nose radius compensation code is used when the cutting tool moves on the left

side of the workpiece in relation to its direction of advance.

G42 : This tool nose radius compensation code is used when the cutting tool moves on the right

side of the workpiece in terms of its direction of advance.

SECTION 6 OFFSET FUNCTION

1-8-2. Behavior on Entering Tool Nose Radius Compensation Mode

5238-E P-63

N2 G01 X2

G00 X0

G42 X1 TΟΟΟΟΟΟ

LE33013R0300800090001

The following example uses the program above to perform OD cuts with an OD turning tool.

( Z0c, X0c )

Starting point N0 ( Z0, X0 )

( Z2c, X2c )

( Z1c, X2c )

N1 ( Z1, X1 )

N2 ( Z2, X2 ) Workpiece

LE33013R0300800090002

Without the tool nose radius compensation function, positioning is performed so that the tool tip reference point is located exactly at the programmed coordinates. At the start up of the tool nose radius compensation mode activated by either G41 or G42, positioning is carried out so that the tool tip circle contacts the segment passing the programmed coordinates in the block containing G41 or G42 and those in the next block. This motion of the axes is called "Start-Up".

• At the start up of the tool nose radius compensation mode, both X- and Z-axis may move even

if the block contains only one dimension word, either X or Z.

G00

X100

Z100

G42

X80

G01

Z50

X+

Z+

Although the programmer might expect the axis movement indicated by broken lines because the N2 block contains only an X word, the actual tool path generated at the start up of the tool nose radius compensation mode is as shown by solid lines.

S1000 T010101 M3

F0.2

LE33013R0300800090003

SECTION 6 OFFSET FUNCTION

• Example of an ideal program for entry into the compensation mode:

G00

X100

Z100

X80

G42

Z90

S1000 T010101 M3

F0.2N4 Z50G01

5238-E P-64

N3 N2

LE33013R0300800090004

In this program, the G42 block contains only a Z word, and points N2, N3 and N4 are all positioned on the same straight line.

• Either G00 or G01 must dominate the operation mode when entering into the tool nose radius

compensation mode. Otherwise, an alarm will occur.

• When neither an X nor Z word is presented at the start up of the tool nose radius compensation

mode, or when the point where the axes are presently located is specified in the start-up block, positioning is executed so that tool tip circle comes in contact with the segment passing through the designated coordinates and the coordinates in the next sequence. The tool nose radius compensation motion is activated from the following sequence.

X+

Z+

( Z3c, X3c )

Workpiece

( Z1c, X1c )

( Z2c, X2c )

N2,N1

G00

G42

N4 Z50

X100

X60

X100

Z100 F0.2

Z80

S1000 T010101 M3

LE33013R0300800090005

With the program above, the tool tip circle is positioned so that it comes into contact with segments N2N3 and N3N4. That is, the blocks of commands after N3 sequence are all executed in the tool nose radius compensation mode.

5238-E P-65

SECTION 6 OFFSET FUNCTION

• If the same point as in the start-up block is specified in the succeeding block, an alarm will result

if the successive two blocks after that do not have dimension words, X and Z. Faulty program example 1:

G01

X50

Z100 F0.2

G42

N4 Z80

X50

Z100

X60

X100N5 Z50

Since sequence N3 designates a point identical to the one designated in the start-up sequence N2, an alarm occurs. Faulty program example 2:

G01

X50 Z100 F0.2 S500

G42

X50N5 Z100

X60N6 Z80

S1000 T010101 M3

LE33013R0300800090006

T010101 M3

S1000

M08

LE33013R0300800090007

Since sequences N3 and N4, the successive two sequences after the start-up of the tool nose radius compensation mode, do not contain X and Z axis movement commands, an alarm occurs.

5238-E P-66

SECTION 6 OFFSET FUNCTION

• I and K command with G41 and G42

In the block containing G41 and G42, by entering I and K words that specify the imaginary point, along with X and Z words that specify the nose radius compensation start-up, unnecessary axis motion required in conventional start-up program is eliminated.

G00

X100

Z100

F0.2

S1000 T010101 M3

G42

X60

Z80

K20

G01

X80

Z65

Z50

Imaginary point for positioning N2′ (I,K)

LE33013R0300800090008

If block N2 containing G42 had no I and K words, positioning of the cutting tool by the commands in block N2 would be executed so that the tool nose radius comes into contact with line N2-N3 at designated point N2 and then moves to N3. Addition of I and K words in block N2 positions the cutting tool to the point where the tool nose R is brought into contact with straight line N2-N3 and imaginary straight line N2-N2’ when the commands in block N2 are executed. Execution of the commands in block N3 brings the cutting tool to the programmed point N3 where the tool nose radius compensation is not active.

[Supplement]

• I and K words should be commanded in incremental values. In this case the dimensions are

referenced to point N2.

• When only either I or K is provided without the other, the control interprets the word to have the

value "0". Therefore, KO in the above program can be omitted.

1-8-3. Behavior in Tool Nose Radius Compensation Mode

The tool nose radius compensation function provides the means to automatically compensate for the tool nose radius in continuous cutting. Since such compensation is performed automatically, there are some restrictions in programming when the tool nose radius compensation function is used.

Straight line to straight line cutting

Midpoint on a straight line

•

When specifying a midpoint on a straight line, the point should be commanded carefully. When point N2 in the figure below is located on line N1 - N3, the cutting tool is positioned so that the tool tip circle comes into contact with line N1 - N3 at point N2.

• Returning along a straight line

Such axis movement causes no problem when the program is written without using the tool nose radius compensation function. However, when this function is used the axis movements must be programmed carefully. Program Example:

5238-E P-67

SECTION 6 OFFSET FUNCTION

X+

G42

G41

Z+

N2 N3 N1

G01 X1

Cutting tool stops at this point in single block mode of operation

LE33013R0300800100001

In this example points N2 and N3 are commanded while the cutting tool is at point N1. When the cutting tool advances from point N1 to point N2, G42 is designated since the cutting tool moves on the right side of the workpiece with respect to the direction of tool advance. However, in the return motion of the tool from point N2 to point N3, the cutting tool is on the left side of the workpiece with respect to the direction of tool advance. Therefore, G41 is specified instead of G42.

X+

5238-E P-68

SECTION 6 OFFSET FUNCTION

N2′ N3′

Z+

N2 N3

N1′

LE33013R0300800100002

The axis movements above are possible by the special processing for the tool nose radius compensation function. Let’s consider the operation in this program in the light of section 1-7. "Path of Tool Nose "R" Center in Tool Nose Radius Compensation Mode."

a. The center of the tool nose R (N2’) at point N2 is obtained as follows:

• The line parallel to the straight line N1 - N2 is obtained, with an upward offset (G42) by

the tool nose radius amount effective at N1.

• The line parallel to the straight line N2 - N3 is obtained, with an upward offset (G41) by

the tool nose radius amount effective at N2.

• The center of the tool nose R is obtained as the point of intersection of the two straight

lines obtained in steps in 1) and 2). However, since those two lines are parallel to each other, no point of intersection is obtained in this case. For such case, the control has a special processing feature in which the positioning is carried out so that the tool nose R comes into contact with point N2. Therefore, the path of the tool nose R center, when the cutting tool advances from point N1 to point N2, is obtained as N1’ - N2’.

b. The center of the tool nose R (N3’) at point N3 is obtained in the same manner as in 1).

In this way, the program on the previous page can return the cutting tool along the same straight line with the tool nose radius compensation function active. If any of these three points is not precisely located on the same straight line, the tool path will be shifted considerably from the expected path.

• Two lines making an acute angle

In the figure below, although positioning from N1 to N2 is intended, the cutting tool cannot reach point N2. This is because it can move only up to the point where the tool nose R comes into contact with line N2 - N3.

X+

Z+

N2 N1

LE33013R0300800100003

This example illustrates a case where programmers are apt to be confused. Another example is provided below.

Example of faulty program 1 (completion of cutting):

X+

G42 G01

G00

X100 Z100 F0.2

Z50

Z300 M05X300

Z+

S1000 T010101 M3

Portion left uncut

N2 N1

5238-E P-69

SECTION 6 OFFSET FUNCTION

LE33013R0300800100004

With the program above, the programmer expected to cut up to point N2, (i.e., up to Z50) allowing a slight uncut portion on the sharp corner due to tool nose R. Contrary to this intention, however, the cutting tool leaves a considerable uncut section since it stops before reaching the desired point. To improve such a program, enter one more point in the program as shown below: Example of improved program 1:

G42 G01 X100 Z100 F0.2

N21

Z50

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

X104

N3 G00 X300 Z300 M05

X+

S1000 T010101 M3

[ > 100 + 4 x (nose R) ]

N 2 1

Z+

N2 N1

Uncut (due to tool nose radius)

LE33013R0300800100005

The improved program generates the tool path shown above, and almost all the cutting can be accomplished as expected except for a slight uncut section due to the tool nose R. To relieve the tool along X-axis in the positive direction in the N21 block, an X word must have a value larger than four times the nose R. This is because a distance twice the nose R is

5238-E P-70

SECTION 6 OFFSET FUNCTION

necessary for the tool tip circle to fit in. In addition, because X words are expressed as diameters, the X word data has to be doubled. That is, the numerical value in such an X word must be larger than four times the tool nose R. If a value smaller than the required amount is used, it might cause the cutting tool to move in the opposite direction toward point N21 and cut into the N1 - N2 surface. Example of improved program 2 (using G40):

G42

G01

G40 G00

X100 Z100

X300

Z50

Z300

F0.2

I10

S1000 T010101 M03

M05

X+

Z+

I 10

N 2

N 3

N 1

LE33013R0300800100006

The G40 command in N3 cancels the tool nose radius function. At point N2, the cutting tool moves so that the tool nose R contacts the line N1 - N2 and the vector I10 extending from point N2.

• Two lines making an obtuse angle

Consider the case where the cutting tool is fed along the path N0 - N1 - N2 - N3 - N4 in the figure below. Angle N2N3N4 is an acute angle and the cutting tool moves along the line outside of that angle. Therefore, the cutting tool is moved to a point some distance from the workpiece at point N3. When preparing a program in which cutting similar to this contour is required, it is necessary to check the safety of tool motion and ensure that the tool does not strike against obstacles when moving to such a distant point.

N 4

N 2

N 1

N 3

X +

Z +

N 0

LE33013R0300800100007

5238-E P-71

SECTION 6 OFFSET FUNCTION

Example program for the path above:

N0 G42 G00 X100 Z300 S1500 T010101 M03

G01 Z100 F0.2

G00

N4 G01

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

X104

X200

Z300

Z50 S1000

[ > 100 + 4 × (nose R) ]

LE33013R0300800100008

It is advantageous to improve the program and eliminate a positioning sequence to a distant point through commands in the N3 block. If N2N3N4 were not a sharp angle, such a problem would not occur. To eliminate sharp angles from the required contour, one possible solution is to interpose a short straight line N3 - N31.

X +

N 4

Z +

N 2

N 3

N 31

LE33013R0300800100009

In some cases, such a modification is not possible. In these cases, to cut a sharp angle without positioning the cutting tool at a distant point, follow the steps detailed below. Example of Improved Program:

Imaginary shape

N 6

N 7

N 2

N0 G42 G00 X100 Z300 S1500

G01 Z100 F0.2

G00

N4 X198.48

X104

X200.48

Z301

Z301.24 F1

N5 X198 Z300.24

G01

N6 X200 Z300

N7 Z50

F0.2

S1000

N 5

N 3

X+

N 4

Z+

T010101 M03

LE33013R0300800100010

In this improved program, the cutting tool moves along the imaginary square N3N4N5N6. This permits the operator to estimate the departure of the cutting tool from the programmed contour. Note that one side of the imaginary square must be longer than twice the nose radius.

• Two lines forming a right angle

X+

N 4

5238-E P-72

SECTION 6 OFFSET FUNCTION

N 3

N1 G42 G01 X100

X150

Z+

Z100 F0.2

Z60

Z20

N 2

S1000 T010101 M03

N 1

LE33013R0300800100011

There are no particular problems in this case.

• Command of identical point

a. If a block without axis movement commands is programmed during the tool nose radius

compensation mode, the path of the tool nose R is the same as the one generated when there is no such block.

N1 G42 G01 X50

X60 Z70

Z100 F0.2

Z80

S1000 T010101 M03

M08

X+

N 4

Z+

N 1

N 3, N2

LE33013R0300800100012

b. When two or more blocks without axis movement commands are programmed, or when the

same point as commanded in the preceding sequence is repeatedly commanded during the tool nose radius compensation mode: In this case, an axis motion that brings the tool nose R into contact with the programmed contour at the programmed coordinate point takes place. When the block of commands containing dimension words, X and/or Z, is read, the cutting tool returns to the correct compensated position.

SECTION 6 OFFSET FUNCTION

Program 1:

S1000 T010101 M04

Z80

F0.2

M08

N1 G42 G01 X50 Z100

X60 Z70

A program like this might cause overcutting as shown below:

5238-E P-73

LE33013R0300800100013

X+

N 4

Z+

Overcut portion

N 1

N 3, N2

LE33013R0300800100014

Depending on the contour to be cut, the unexpected motion may not result in overcut, as in program 2. Program 2:

N1 G42 G01 X50

X+

X40 Z70

Z100 F0.2

Z80

S1000 T010101 M04

M08

Z+

N3, N2

LE33013R0300800100015

5238-E P-74

SECTION 6 OFFSET FUNCTION

Straight line to arc cutting (arc to straight line cutting)

Arc within one quadrant

•

In a program where the cutting tool moves continuously from a straight line to an arc, the movement of the cutting tool is handled in the same way as in a case where the movement is from a straight line to a straight line.

X+

N1 G42

G03

G01

G01 X100

X140

Z+

Z100 F0.2

Z80

Z60

Z40

N2 N1

S1000 T010101 M04

K − 20

LE33013R0300800100016

The tool position at point N2 is determined so that the tool nose R comes into contact with both line N1 - N2 and arc N2 - N3. At point N3, the cutting tool is positioned in a similar way - the tool nose R makes contact at point N3. When the cutting tool moves from point N3 to point N4, the cutting mode changes from circular interpolation to linear interpolation. If discontinuity at point N3 results during the tool path calculation, an alarm is displayed and machine operation is stopped.

• Arc in two quadrants

a. Case where the arc radius is greater than "2 x nose R":

5238-E P-75

SECTION 6 OFFSET FUNCTION

X+

N1 G42

G02

G01

G01 X100

X140

Z100 F0.2

Z80

Z60

I20

Z40

S1000 T010101 M04

LE33013R0300800100017

The tool position determined by the commands in the N2 block is the point where the tool nose R comes into contact with line N1 - N2 at point N2. In the N3 sequence, the cutting tool is positioned so that it comes into contact with both the extension of straight line N2 N3 and the extension of arc N3 - N4.

b. Case where the arc radius is equal to "2 x nose R":

Z+

X+

N1 G42

G02

G01

Z+

G01 X100

X103.2

N4 N3

Z100 F0.2

Z80

Z78.4

I1.6

Z40

Tool nose R = 0.8 mm

S1000 T010101 M04

LE33013R0300800100018

5238-E P-76

SECTION 6 OFFSET FUNCTION

When the radius of the programmed arc equals twice the tool nose R, the cutting tool is located at the point where the tool nose R comes into contact with both the extension of arc N2 - N3 and the extension of straight line N3 - N4, after the execution of the commands in N3 block (see the figure in "1)" above). That is, the cutting tool is positioned right above point N2, as shown in the figure directly above.

c. Case where the arc radius is less than "2 x nose R" (impossible):

X+

N4 N3

N2 N1

S1000 T010101 M04

N1 G42

G02

G01

G01 X100

X102

Z+

Z100 F0.2

Z80

Z79

Z40

The commands in block N3 specify positioning of the cutting tool at the point where the tool nose R comes into contact with both the extension of arc N2-N3 and the extension of straight line N3-N4; however, such a point cannot be obtained. Therefore, when the control executes the commands in block N3, an alarm occurs and the machine stops. In this kind of case, cutting using the tool nose radius compensation function is not possible.

[Supplement]

When cutting inside an arc, the programming must satisfy the following condition: R 2 x R

(where R: arc radius, RN: nose R)

LE33013R0300800100019

• Arc in three quadrants

5238-E P-77

SECTION 6 OFFSET FUNCTION

X+

N1 G42

G02

G01

N4 N3

Z+

G01 X100

X120

X160 Z80

Z100 F0.2

I20

Z60

S1000 T010101 M04

LE33013R0300800100020

Positioning by the commands in block N2 is to the point where the tool nose R comes into contact with both the extension of straight line N1 - N2 and the extension of arc N2 - N3. Other axis motions of the cutting tool are identical to those for cutting an arc in two quadrants.

5238-E P-78

SECTION 6 OFFSET FUNCTION

Arc to arc cutting

Arc to arc cutting can be programmed in the same manner as straight line to arc cutting. The tool path is generated so that the tool nose R is brought into contact with each arc or its extension. If the tool path becomes discontinuous in the process of path calculation due to an error, the machine stops with an alarm displayed on the screen. Other motions of the cutting tool are as explained in (2), "Straight line to arc cutting".

N4N5

X+

Z+

N1 G42

G02

G03

G01

G01 X100

X140

X180

Z100 F0.2

Z80

I20

Z60

K − 20Z40

Z20

S1000 T010101 M04

LE33013R0300800100021

5238-E P-79

SECTION 6 OFFSET FUNCTION

Switching from G41 to G42 or from G42 to G41

Before switching the tool nose radius compensation mode from G41 to G42 or from G42 to G41, it is advisable to cancel the compensation mode by specifying G40. If a switch-over is to be done with the compensation mode active, carefully check the movement of the cutting tool resulting from the switch-over.

• Switch-over in straight line to straight line cutting

Program Example:

Expected tool position

LE33013R0300800100022

X+

N1 G42

G01

G41

G00

N4 X

Z+

The motion of the cutting tool generated by the above program is as follows: Commands in blocks, N1 and N2 are governed by G42 and those in blocks N3 and later are governed by G41. To position the cutting tool at point N2, the tool nose R center lies to the right side of straight line N1 - N2 since block N2 is in the G42 mode. As for block N3, the tool nose R center lies to the left side of straight line N2 - N3 since block N3 is in the G41 mode. As a result, the cutting tool is positioned at point A as shown above. Positioning in block N2 is carried out at the left side of straight line N2 - N3.

• Switch-over in straight line to arc cutting

The concept is the same as for straight line to straight line cutting.

G41

G42

N1 G42

G41

X+

G01

G03

Z+

LE33013R0300800100023

SECTION 6 OFFSET FUNCTION

• Switch-over in arc to straight line cutting

Again, the concept is the same as for straight line to straight line cutting.

N1 G42

G03

G41

X+

G01

N3 N2

5238-E P-80

Z+

• Switch-over in arc to arc cutting

Once again, the concept is the same as for straight line to straight line cutting.

N1 G42

G02

G41

X+

G01 X

Z+

LE33013R0300800100024

LE33013R0300800100025

5238-E P-81

SECTION 6 OFFSET FUNCTION

1-8-4. Behavior on Cancelation of the Tool Nose Radius Compensation Mode

G40 given with X- or Z-axis motion command

To cancel the tool nose radius compensation mode, the G40 code is used. It is essential to understand the cutting tool movements that result from the cancelation of the compensation mode in order to avoid unexpected trouble. In the tool nose radius compensation mode, the tool path is generated so that the tool nose R is always in contact with the programmed contour, but the axis position is controlled so that the tool tip reference point traces the programmed contour when the tool nose radius compensation mode is not active. Therefore, under- or over-cut often results when entering into or when canceling the tool nose radius compensation mode.

X+

Position left uncut

Z+

Overcut portion

N2 N1

LE33013R0300800110001

Cutting a contour comprising straight line segments as illustrated above is programmed as shown below if the tool nose radius compensation mode is not active.

N1 G01

N5 X300 Z300G00

X100

X120

X130 Z20

F0.2

Z100 S1000 T010101 M03

Z60

LE33013R0300800110002

With the commands above, the cutting tool moves along the path indicated by broken lines. That is, for designated point N3 the tool center is positioned at point O3, and at point O4 for designated point N4. The uncut part parallel to straight line N3 - N4 is left. Therefore the tool nose radius compensation function can be effectively used to cut such a contour accurately. See the programs on the following pages.

• When the tool nose R compensation cancel command is designated:

N1 G42 G01

G40

N5 X300 Z300G00

X100

X120

X130 Z20

F0.2

Z100 S1000 T010101 M03

Z60

LE33013R0300800110003

5238-E P-82

SECTION 6 OFFSET FUNCTION

The tool path generated in the above program is shown by solid lines. Positioning fort programmed point N3 is carried out at the point where the tool nose R comes into contact with point N3, and that for programmed point N4 is carried out at point O4; the same point reached by the program in which the tool nose radius compensation function is not activated. Therefore, the uncut part will be near point N4 while the section near point N3 is overcut. Improved program:

X+

Z+

N1 G42 G01

N5 X300

G40 G00

X100

X120

X130 Z20

F0.2

Z100 S1000 T010101 M03

Z60

Z300

N2 N1

LE33013R0300800110004

To cut the exact contour up to Point N4, the G40 command which cancels the tool nose radius compensation mode is specified in block N5. Although the program yields almost the expected contour, the tool nose R goes beyond the designated point N4 along Z-axis since it comes into contact with line N3 - N4 at point N4. When this kind of overtravel causes no interference or overcutting, there are no problems.

SECTION 6 OFFSET FUNCTION

• Eliminating possible overcutting along Z-axis, see the program below:

5238-E P-83

F0.2

I10

LE33013R0300800110005

X+

N1 G42 G01

N5 X300 Z300G40 G00

Z+

X100

X120

X130

Portion left uncut due to round tip

Z100 S1000 T010101 M03

Z60

Z20

I and K words specified in the G40 block allow the tool to move to the point where the tool nose R is brought into contact with both line N3 - N4 and line N4 - N5.

I and K command with G40

In the block containing G40, by entering I and K words that specify the imaginary point along with X and Z words that specify the point where nose radius compensation is canceled, unnecessary axis motion required in conventional canceling program is eliminated.

N1 G42 G01

N5 X300 Z300 I10 K0G40 G00

X+

X100

X120

X130 Z20

Imaginary point for positioning N5' (I, K)

Z+

F0.2

Z100 S1000 T010101 M03

Z60

Portion left uncut due to round tip

LE33013R0300800110006

5238-E P-84

SECTION 6 OFFSET FUNCTION

If block N5 containing G40 has no I and K words, positioning of the cutting tool by the commands in block N4 is executed so that the tool nose R comes into contact with line N3 - N4 at designated point N4 and then moves along the path indicated by broken lines toward point N5. Addition of I and K words in block N5 positions the cutting tool to the point where the tool nose R is brought into contact with straight line N3 - N4 and imaginary straight line N4 - N5’ when the commands in block N4 are executed. Execution of the commands in block N5 brings the cutting tool to the programmed point N5 where tool nose radius compensation is not active.

[Supplement]

• I and K words should be commanded as incremental values. In this case the dimensions are

referenced to point N4.

• When either I or K only is specified without the other, the control interprets the word to have the

value "0". Therefore, K0 in the above program can be omitted.

Independent G40

When the G40 code is programmed without other commands in the same block, positioning is carried out at the point where the tool nose R comes into contact with the point specified in the previous block since the G40 block has no X and Z words which call for axis movement.

N1 G42 G01

N5 G40

N6 X300 Z300G00

X+

X100

Z60

X120

X130 Z20

N4, N5

Z+

F0.2

Z100 S1000 T010101 M03

LE33013R0300800110007

When the tool nose radius compensation mode is canceled (G40), the mode of operation must be either G00 or G01. If not, an alarm occurs.

1-8-5. Relieving Tool to Change "S" or "M" Code during Cutting

The tool nose radius compensation function is designed to automatically compensate the tool nose radius in a continuous cutting program; with the dimensions of the workpiece programmed, compensation is automatically applied to finish the part to the programmed dimensions. However, such a powerful function requires careful programming when continuous cutting is interrupted to change S and/or M commands. This section deals with some programming examples in which the programmer experienced unexpected results by relieving the cutting tool during cutting on a continuous path.

Original contour and associated program (program 1):

5238-E P-85

SECTION 6 OFFSET FUNCTION

X+

Z+

LE33013R0300800120001

Program 1:

N1 G42 G01 X100

X120

F0.2

Z100 S1500

Z80

Z40

S1000

Z20

T010101 M03

LE33013R0300800120002

The original contour comprises: straight line - slope - straight line.

Program 2

The contour is the same as in program 1, but the cutting tool is relieved at point N3 in the +X direction to change the spindle speed, then continuous cutting is intended.

S" code change

N31

X+

Z+

N32

Uncut portion is left

LE33013R0300800120003

Program 2:

G42

N31

N32

G00

G01

G01 X100

X120

X124

X120

Z100

Z80

Z40

Z20

F0.2 S1500

S1000

T010101 M03

LE33013R0300800120004

In program 2, the cutting tool is positioned at a point where the tool nose R is in contact with line N3

- N31 at point N31 when the commands in block N31 are executed since the three designated points

5238-E P-86

SECTION 6 OFFSET FUNCTION

N3, N31 and N32 lie on the same straight line. From N3 to N31, the positioning is on the right hand side of the line. Commands in block N32 position the cutting tool at the point where the tool nose R is brought into contact with straight lines N31 - N32 and N3 - N4 on the right side of the direction of tool advance. This causes the cutting tool to move not only in the X-axis direction but also in the Zaxis direction although block N32 contains only an X word. Such cutting tool movements leave an uncut portion as shown above.

Program 3

In this program, an attempt is made to eliminate the uncut portion caused by program 2.

Imaginary shape

N32

LE33013R0300800120005

X+

N31

Z+

Overcut portion

Program 3:

G42

G01

N31

N32

G00

X100

X120

X124

X120

G01

Z100

Z80

Z40

Z42

Z20

F0.2 S1500

S1000

T010101 M03

LE33013R0300800120006

When the control feeds the cutting tool from point N2 to point N3, it reads the position data of point N31 as well as those of point N3. This permits the tool nose R to be positioned at the point where it is in contact with the two straight lines N2 - N3 and N3 - N31. After that, positioning is carried out at the point where the tool nose R comes into contact with the two straight lines N3 - N31 and N31 - N32, when positioning is performed with the commands in block N31. This moves the cutting tool in the -X direction although the commands in that block specify tool movement in the +X direction. This is due to the positioning in block N3, where the tool nose R goes beyond side N31 - N32. Similarly, positioning of the cutting tool in block N32 is carried out at the point where the tool nose R comes into contact with both straight lines N31 - N32 and N32 - N4. This also causes the cutting tool to move in the direction opposite to the programmed direction. The result is overcutting.

5238-E P-87

SECTION 6 OFFSET FUNCTION

Program 4

N31

Imaginary shape

X+

Z+

Program 4: In this program, a tool looping similar to that performed in program 3 is executed with the numeral values modified to avoid overcutting.

N32

LE33013R0300800120007

G42

N31

N32

G00

G01

G01 X100

X120

X126

X120

Z100

Z80

Z40

Z43

Z20

F0.2 S1500

S1000

T010101 M03

LE33013R0300800120008

This program almost yields the expected finish. However, there are still latent problems, such as:

• overcutting is caused depending on the size of the tool nose R

• the length of side N31 - N32 cannot be readily found.

These problems are solved by looping the tool path along a square as explained next.

Program 5

Program 5 solves the problems encountered with program 4.

N31

X+

N32

Imaginary shape

Z+

Portion left uncut

N33

LE33013R0300800120009

okuma OSP-P200L, OSP-P20L, OSP-P200L-R, OSP-P20L-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 Manual/Continuous Operation

4. On Finishing Work

5. Precautions during Maintenance Inspection and When Trouble Occurs

6. General Precautions

7. Symbols Used in This Manual

INTRODUCTION

SECTION 1 PROGRAM CONFIGURATIONS

1. Program Types

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. Block Delete

7. Comment Function (CONTROL OUT/IN)

8. Program Storage Memory Capacity

9. Variable Limits

10. Determining Feedrate for Cutting along C-Axis

10-1. Cutting by Controlling the C-axis Only

10-2. Cutting by Controlling Both C-axis and Z-axis Simultaneously

10-3. Cutting by Controlling Both C-axis and X-axis Simultaneously

10-4. Cutting by Simultaneous 3-axis Control of X-, Z-, and C-axis

SECTION 2 COORDINATE SYSTEMS AND COMMANDS

1. Coordinate Systems

1-1. Coordinate Systems and Values

1-2. Encoder Coordinate System

1-3. Machine Coordinate System

1-4. Program Coordinate System

2. Coordinate Commands

2-1. Controlled Axis

2-2. Commands in Inch System

2-3. Position of Decimal Point

2-4. Absolute and Incremental Commands (G90, G91)

2-5. Diametric and Radial Commands

1. Positioning (G00)

SECTION 3 MATH FUNCTIONS

2. Linear Interpolation (G01)

3. Circular Interpolation (G02, G03)

4. Automatic Chamfering

4-1. C-chamfering (G75)

4-2. Rounding (G76)

4-3. Automatic Any-Angle Chamfering

5. Torque Limit and Torque Skip Function

5-1. Torque Limit Command (G29)

5-2. Torque Limit Cancel Command (G28)

5-3. Torque Skip Command (G22)

5-4. Parameter Setting

5-5. Program Example

SECTION 4 PREPARATORY FUNCTIONS

1. Dwell (G04)

2. Zero Shift/Max. Spindle Speed Set (G50)

2-1. Zero Shift

2-2. Max. Spindle Speed Set

3. Droop Control (G64, G65)

4. Feed Per Revolution (G95)

5. Feed Per Minute (G94)

6. Constant Speed Control (G96/G97)

SECTION 5 S, T, AND M FUNCTIONS

1. S Functions (Spindle Functions)

2. SB Code Function

3. T Functions (Tool Functions)

4. M Functions (Auxiliary Functions)

5. M-tool Spindle Commands

5-1. Programming Format

5-2. M Codes Used for C-axis Operation

6. STM Time Over Check Function

6-1. Check ON Conditions

6-2. S, T, M Cycle Time Setting

6-3. Timing Chart Example

SECTION 6 OFFSET FUNCTION