Okuma OSP-P200L Owner's manual

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
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 accident-
free 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.

5238-E P-(iv)
SAFETY PRECAUTIONS
(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.
(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.

5238-E P-(v)
SAFETY PRECAUTIONS
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.
indicates an imminently hazardous situation which, if not avoided, will result in death or serious
injury.
indicates a potentially hazardous situation which, if not avoided, could result in death or serious
injury.
indicates a potentially hazardous situation which, if not avoided, may result in minor or moderate
injury.
indicates a potentially hazardous situation which, if not avoided, may result in damage to your
property.
indicates general instructions for safe operation.
DANGER
WARNING
CAUTION
CAUTION
SAFETY INSTRUCTIONS

5238-E P-(i)
INTRODUCTION
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
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

5238-E P-1
SECTION 1 PROGRAM CONFIGURATIONS
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.
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
LE33013R0300300010001
•Extensions
SDF : Schedule program file
MIN : Main program file
SSB : System subprogram file
SUB : User subprogram file
••• .
ExtensionMain file name

5238-E P-2
SECTION 1 PROGRAM CONFIGURATIONS
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.
•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.

5238-E P-3
SECTION 1 PROGRAM CONFIGURATIONS
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.
•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.

5238-E P-4
SECTION 1 PROGRAM CONFIGURATIONS
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:
LE33013R0300300040001
•An address character is one of the alphabetic characters A through Z and defines the meaning
of the entry specified following it. In addition, an extended address character, consisting of two
alphabetic characters, may also be used.
•Refer to SECTION 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.
X-100 Z=100∗SIN[50] Z=V1+V2
Address Numerical
value Address Formula Address Variable
Word Word Word

5238-E P-5
SECTION 1 PROGRAM CONFIGURATIONS
4-4. Programmable Range of Address Characters
Address Function Programmable Range Remarks
Metric Inch
O Program name 0000 to 9999 same as left Alphabetic
characters available
N Sequence name 0000 to 9999 same as left
G Preparatory function 0 to 999 same as left
X, Z Coordinate values
(linear axis) ±99999.999 mm ±9999.9999 inch
CCoordinate values
(rotary axis) ±359.999 deg. ±359.999 deg.
I, K
Coordinate values of
center of arc
Taper amount and
depth of cut in fixed
thread cutting cycle
Shift amount in
grooving cycle
±99999.999 mm ±9999.9999 inch
D, U, W, H, L Automatic
programming
commands
0 to 99999.999 mm 0 to 9999.9999 inch
E±99999.999 mm/rev ±9999.9999 inch/rev
A, B 0 to 99999.999 deg. 0 to 9999.9999 deg.
F
Feedrate per
revolution
0.001 to 99999.999
mm/rev
0.0001 to 999.9999
inch/rev
Feedrate per minute 0.001 to 99999.999
mm/min
0.0001 to 9999.9999
inch/min
Dwell time period 0.01 to 9999.99 sec same as left
T Tool number 6 digits
4 digits same as left
6 digits (with nose R
compensation)
4 digits (without nose
R compensation)
S
SB
Spindle speed
M-tool speed
0 to 9999
0 to 9999 same as left
MMiscellaneous
function 0 to 511 same as left
QA C-axis revolution 1 to 1999 (rev.) same as left
SA C-axis speed 0.001 to 20.000 min-1 same as left

5238-E P-6
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
Logical
operation
Exclusive OR EOR 0110 = 1010 EOR 1100 (See *3.)
Logical OR OR 1110 = 1010 OR 1100
Logical AND AND 1000 = 1010 AND 1100
Negation NOT 1010 = NOT 0101
Arithmetic
operation
Addition + 8 = 5 + 3
Subtraction - 2 = 5 - 3
Multiplication * 15 = 5 * 3
Division / (slash) 3 = 15/5
Trigonometric
functions, etc.
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 30 = ATAN 2 [1,(Square root 3)] (See
*1.)
Square root SQRT 4 = SQRT [16]
Absolute value ABS 3 = ABS [-3]
Decimal to binary conversion BIN 25 = BIN [$25]
($ represents a hexadecimal number.)
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) DROUND 13.265 = DROUND [13.26462] (See *2.)
Unit integer implementation
(truncation) DFlX 13.264 = DFlX [13.26462] (See *2.)
Unit integer implementation (raising) DFUP 13.265 = DFUP [13.26462] (See *2.)
Remainder MOD 2 = MOD [17, 5]
Brackets
Opening bracket [ Determines the priority of an operation.
(Operations inside the bracket are
performed first.)
Closing bracket ]
*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.)

5238-E P-7
SECTION 1 PROGRAM CONFIGURATIONS
Logical Operations
"a", "b", and "c" represent corresponding bits.
LE33013R0300300080001
If the two corresponding values agree, EOR outputs 0.
If the two values do not agree, EOR outputs 1.
LE33013R0300300080002
If both corresponding values are 0, OR outputs 0.
If not, OR outputs 1.
LE33013R0300300080003
If both corresponding values are 1, AND outputs 1.
If not, AND outputs 0.
LE33013R0300300080004
NOT inverts the value (from 0 to 1, and 1 to 0).
abc
000
011
101
110
abc
000
011
101
111
abc
000
010
100
111
ab
01
10
• Exclusive OR (EOR) c = a EOR b
• Logical OR (OR) c = a OR b
• Logical AND (AND) c = a AND b
• Negation (NOT) b = NOT a