mazak Mazatrol Matrix Programming Manual

PROGRAMMING MANUAL

Return to Library

for

MAZATROL MATRIX

(for Machining Centers)

EIA/ISO Program

MANUAL No. : H740PB0041E

Serial No. :

Before using this machine and equipment, fully understand the contents of this manual to ensure proper operation. Should any questions arise, please ask the nearest Technical Center or Technology Center.

IMPORTANT NOTICE

1. Be sure to observe the safety precautions described in this manual and the contents of the

safety plates on the machine and equipment. Failure may cause serious personal injury or material damage. Please replace any missing safety plates as soon as possible.

2. No modifications are to be performed that will affect operation safety. If such modifications are

required, please contact the nearest Technical Center or Technology Center.

3. For the purpose of explaining the operation of the machine and equipment, some illustrations

may not include safety features such as covers, doors, etc. Before operation, make sure all such items are in place.

4. This manual was considered complete and accurate at the time of publication, however, due to

our desire to constantly improve the quality and specification of all our products, it is subject to change or modification. If you have any questions, please contact the nearest Technical Center or Technology Center.

5. Always keep this manual near the machinery for immediate use.

6. If a new manual is required, please order from the nearest Technical Center or Technology

Center with the manual No. or the machine name, serial No. and manual name.

Issued by Manual Publication Section, Yamazaki Mazak Corporation, Japan

11. 2006

SAFETY PRECAUTIONS

Preface

Safety precautions relating to the CNC unit (in the remainder of this manual, referred to simply as the NC unit) that is provided in this machine are explained below. Not only the persons who create programs, but also those who operate the machine must thoroughly understand the contents of this manual to ensure safe operation of the machine.

Read all these safety precautions, even if your NC model does not have the corresponding functions or optional units and a part of the precautions do not apply.

Rule

1. This section contains the precautions to be observed as to the working methods and states usually expected. Of course, however, unexpected operations and/or unexpected working states may take place at the user site. During daily operation of the machine, therefore, the user must pay extra careful attention to its own working safety as well as to observe the precautions described below.

2. Although this manual contains as great an amount of information as it can, since it is not rare for the user to perform the operations that overstep the manufacturer-assumed ones, not all of “what the user cannot perform” or “what the user must not perform” can be fully covered in this manual with all such operations taken into consideration beforehand. It is to be understood, therefore, that functions not clearly written as “executable” are “inexecutable” functions.

SAFETY PRECAUTIONS

3. The meanings of our safety precautions to DANGER, WARNING, and CAUTION are as follows:

: Failure to follow these instructions could result in loss of life.

DANGER

: Failure to observe these instructions could result in serious harm to a human

life or body.

WARNING

: Failure to observe these instructions could result in minor injuries or serious

machine damage.

CAUTION

HGENPA0043E

S-1

Basics

SAFETY PRECAUTIONS

! After turning power on, keep hands away from the keys, buttons, or switches of the

operating panel until an initial display has been made.

WARNING

! Before proceeding to the next operations, fully check that correct data has been entered

and/or set. If the operator performs operations without being aware of data errors, unexpected operation of the machine will result.

! Before machining workpieces, perform operational tests and make sure that the machine

operates correctly. No workpieces must be machined without confirmation of normal operation. Closely check the accuracy of programs by executing override, single-block, and other functions or by operating the machine at no load. Also, fully utilize tool path check, Virtual Machining, and other functions, if provided.

! Make sure that the appropriate feed rate and rotational speed are designated for the

particular machining requirements. Always understand that since the maximum usable fee d rate and rotational speed are determined by the specifications of the tool to be used, those of the workpiece to be machined, and various other factors, actual capabilities differ from the machine specifications listed in this manual. If an inappropriate feed rate or rotational speed is designated, the workpiece or the tool may abruptly move out from the machine.

! Before executing correction functions, fully check that the direction and amount of

correction are correct. Unexpected operation of the machine will result if a correction function is executed without its thorough understanding.

! Parameters are set to the optimum standard machining conditions prior to shipping of the

machine from the factory. In principle, these settings should not be modified. If it becomes absolutely necessary to modify the settings, perform modifications only after thoroughly understanding the functions of the corresponding parameters. Modifications usually affect any program. Unexpected operation of the machine will result if the settings are modified without a thorough understanding.

Remarks on the cutting conditions recommended by the NC

! Before using the following cutting conditions:

- Cutting conditions that are the result of the MAZATROL Automatic Cutting Conditions

WARNING

Determination Function

- Cutting conditions suggested by the Machining Navigation Function

- Cutting conditions for tools that are suggested to be used by the Machining Navigation

Function

Confirm that every necessary precaution in regards to safe machine setup has been taken – especially for workpiece fixturing/clamping and tool setup.

! Confirm that the machine door is securely closed before starting machining.

Failure to confirm safe machine setup may result in serious injury or death.

S-2

Programming

WARNING

SAFETY PRECAUTIONS

! Fully check that the settings of the coordinate systems are correct. Even if the designated

program data is correct, errors in the system settings may cause the machine to operate in unexpected places and the workpiece to abruptly move out from the machine in the event of contact with the tool.

! During surface velocity hold control, as the current workpiece coordinates of the surface

velocity hold control axes approach zeroes, the spindle speed increases significantly. For the lathe, the workpiece may even come off if the chucking force decreases. Safety speed limits must therefore be observed when designating spindle speeds.

! Even after inch/metric system selection, the units of the programs, tool information, or

parameters that have been registered until that time are not converted. Fully check these data units before operating the machine. If the machine is operated without checks being performed, even existing correct programs may cause the machine to operate differently from the way it did before.

! If a program is executed that includes the absolute data commands and relative data

commands taken in the reverse of their original meaning, totally unexpected operation of the machine will result. Recheck the command scheme before executing programs.

! If an incorrect plane selection command is issued for a machine action such as arc

interpolation or fixed-cycle machining, the tool may collide with the workpiece or part of the machine since the motions of the control axes assumed and those of actual ones will be interchanged. (This precaution applies only to NC units provided with EIA functions.)

! The mirror image, if made valid, changes subsequent machine actions significantly. Use

the mirror image function only after thoroughly understanding the above. (This precaution applies only to NC units provided with EIA functions.)

! If machine coordinate system commands or reference position returning commands are

issued with a correction function remaining made valid, correction may become invalid temporarily. If this is not thoroughly understood, the machine may appear as if it would operate against the expectations of the operator. Execute the above commands only after making the corresponding correction function invalid. (This precaution applies only to NC units provided with EIA functions.)

! The barrier function performs interference checks based on designated tool data. Enter the

tool information that matches the tools to be actually used. Otherwise, the barrier function will not work correctly.

! The system of G-code and M-code commands differs, especially for turning, between the

machines of INTEGREX e-Series and the other turning machines. Issuance of the wrong G-code or M-code command results in totally non-intended machine operation. Thoroughly understand the system of G-code and M-code commands before using this system.

Sample program Machines of INTEGREX e-Series Turning machines

S1000M3 S1000M203

The milling spindle rotates at 1000 min–1. The turning spindle rotates at 1000 min–1. The turning spindle rotates at 1000 min–1. The milling spindle rotates at 1000 min–1.

S-3

SAFETY PRECAUTIONS

! For the machines of INTEGREX e-Series, programmed coordinates can be rotated using

an index unit of the MAZATROL program and a G68 command (coordinate rotate command) of the EIA program. However, for example, when the B-axis is rotated through 180 degrees around the Y-axis to implement machining with the turning spindle No. 2, the plus side of the X-axis in the programmed coordinate system faces downward and if the program is created ignoring this fact, the resulting movement of the tool to unexpected positions may incite collisions. To create the program with the plus side of the X-axis oriented in an upward direction, use the mirror function of the WPC shift unit or the mirror imaging function of G-code command (G50.1, G51.1).

! After modifying the tool data specified in the program, be sure to perform the tool path

check function, the Virtual Machining function, and other functions, and confirm that the program operates properly. The modification of tool data may cause even a field-proven machining program to change in operational status. If the user operates the machine without being aware of any changes in program status, interference with the workpiece could arise from unexpected operation. For example, if the cutting edge of the tool during the start of automatic operation is present inside the clearance-including blank (unmachined workpiece) specified in the common unit of the MAZATROL program, care is required since the tool will directly move from that position to the approach point because of no obstructions being judged to be present on this path. For this reason, before starting automatic operation, make sure that the cutting edge of the tool during the start of automatic operation is present outside the clearance-including workpiece specified in the common unit of the MAZATROL program.

CAUTION

! If axis-by-axis independent positioning is selected and simultaneously rapid feed selected

for each axis, movements to the ending point will not usually become linear. Before using these functions, therefore, make sure that no obstructions are present on the path.

! Before starting the machining operation, be sure to confirm all contents of the program

obtained by conversion. Imperfections in the program could lead to machine damage and operator injury.

S-4

Operations

WARNING

SAFETY PRECAUTIONS

! Single-block, feed hold, and override functions can be made invalid using system variables

#3003 and #3004. Execution of this means the important modification that makes the corresponding operations invalid. Before using these variables, therefore, give thorough notification to related persons. Also, the operator must check the settings of the system variables before starting the above operations.

! If manual intervention during automatic operation, machine locking, the mirror image

function, or other functions are executed, the workpiece coordinate systems will usually be shifted. When making machine restart after manual intervention, machine locking, the mirror image function, or other functions, consider the resulting amounts of shift and take the appropriate measures. If operation is restarted without any appropriate measures being taken, collision with the tool or workpiece may occur.

! Use the dry run function to check the machine for normal operation at no load. Since the

feed rate at this time becomes a dry run rate different from the program-designated feed rate, the axes may move at a feed rate higher than the programmed value.

! After operation has been stopped temporarily and insertion, deletion, updating, or other

commands executed for the active program, unexpected operation of the machine may result if that program is restarted. No such commands should, in principle, be issued for the active program.

CAUTION

! During manual operation, fully check the directions and speeds of axial movement. ! For a machine that requires manual homing, perform manual homing operations after

turning power on. Since the software-controlled stroke limits will remain ineffective until manual homing is completed, the machine will not stop even if it oversteps the limit area. As a result, serious machine damage will result.

! Do not designate an incorrect pulse multiplier when performing manual pulse handle feed

operations. If the multiplier is set to 1000 times and the handle operated inadvertently, axial movement will become faster than that expected.

S-5

BEFORE USING THE NC UNIT

Limited Warranty

The warranty of the manufacturer does not cover any trouble arising if the NC unit is used for its non-intended purpose. Take notice of this when operating the unit.

Examples of the trouble arising if the NC unit is used for its non-intended purpose are listed below.

1. Trouble associated with and caused by the use of any commercially available software products (including user-created ones)

2. Trouble associated with and caused by the use of any Windows operating systems

3. Trouble associated with and caused by the use of any commercially available computer equipment

Operating Environment

1. Ambient temperature

During machine operation: 0° to 50°C (32° to 122°F)

2. Relative humidity

During machine operation: 10 to 75% (without bedewing) Note: As humidity increases, insulation deteriorates causing electrical component parts to

deteriorate quickly.

Keeping the Backup Data

Note: Do not attempt to delete or modify the data stored in the following folder.

Recovery Data Storage Folder: D:\MazakBackUp

Although this folder is not used when the NC unit is running normally, it contains important data that enables the prompt recovery of the machine if it fails.

If this data has been deleted or modified, the NC unit may require a long recovery time. Be sure not to modify or delete this data.

S-6

CONTENTS

Page

1 CONTROLLED AXES........................................................................... 1-1

1-1 Coordinate Words and Controlled Axes ............................................................. 1-1

2 UNITS OF PROGRAM DATA INPUT................................................... 2-1

2-1 Units of Program Data Input...............................................................................2-1

2-2 Units of Data Setting...........................................................................................2-1

2-3 Ten-Fold Program Data......................................................................................2-1

3 DATA FORMATS.................................................................................. 3-1

3-1 Tape Codes........................................................................................................3-1

3-2 Program Formats ...............................................................................................3-5

3-3 Tape Data Storage Format................................................................................. 3-6

3-4 Optional Block Skip ............................................................................................3-6

3-5 Program Number, Sequence Number and Block Number: O, N ........................3-7

3-6 Parity-H/V...........................................................................................................3-8

3-7 List of G-Codes ................................................................................................3-10

4 BUFFER REGISTERS.......................................................................... 4-1

4-1 Input Buffer.........................................................................................................4-1

4-2 Preread Buffer.................................................................................................... 4-2

5 POSITION PROGRAMMING................................................................ 5-1

5-1 Dimensional Data Input Method.........................................................................5-1

5-1-1 Absolute/Incremental data input: G90/G91............................................................. 5-1

C-1

5-2 Inch/Metric Selection: G20/G21..........................................................................5-3

5-3 Decimal Point Input ............................................................................................5-4

6 INTERPOLATION FUNCTIONS........................................................... 6-1

6-1 Positioning (Rapid Feed): G00...........................................................................6-1

6-2 One-Way Positioning: G60.................................................................................6-4

6-3 Linear Interpolation: G01....................................................................................6-5

6-4 Circular Interpolation: G02, G03.........................................................................6-6

6-5 Radius Designated Circular Interpolation: G02, G03..........................................6-9

6-6 Spiral Interpolation: G2.1, G3.1 (Option)..........................................................6-11

6-7 Plane Selection: G17, G18, G19......................................................................6-19

6-7-1 Outline .................................................................................................................. 6-19

6-7-2 Plane selection methods....................................................................................... 6-19

6-8 Virtual-Axis Interpolation: G07..........................................................................6-21

6-9 Spline Interpolation: G06.1 (Option).................................................................6-22

6-10 NURBS Interpolation: G06.2 (Option)...............................................................6-33

6-11 Cylindrical Interpolation: G07.1 ........................................................................6-40

6-12 Helical Interpolation: G02, G03 ........................................................................6-49

7 FEED FUNCTIONS.............................................................................. 7-1

7-1 Rapid Traverse Rates.........................................................................................7-1

7-2 Cutting Feed Rates.............................................................................................7-1

7-3 Asynchronous/Synchronous Feed: G94/G95.....................................................7-1

7-4 Selecting a Feed Rate and Effects on Each Control Axis...................................7-3

C-2

7-5 Automatic Acceleration/Deceleration..................................................................7-6

7-6 Speed Clamp......................................................................................................7-7

7-7 Exact-Stop Check: G09......................................................................................7-7

7-8 Exact-Stop Check Mode: G61..........................................................................7-10

7-9 Automatic Corner Override: G62...................................................................... 7-10

7-10 Tapping Mode: G63 ..........................................................................................7-15

7-11 Cutting Mode: G64 ...........................................................................................7-15

7-12 Geometry Compensation/Accuracy Coefficient: G61.1/,K................................7-16

7-12-1 Geometry compensation function: G61.1.............................................................7-16

7-12-2 Accuracy coefficient (,K)....................................................................................... 7-17

7-13 Inverse Time Feed: G93 (Option).....................................................................7-18

8 DWELL FUNCTIONS ........................................................................... 8-1

8-1 Dwell Command in Time: (G94) G04..................................................................8-1

8-2 Dwell Command in Number of Revolutions: (G95) G04.....................................8-2

9 MISCELLANEOUS FUNCTIONS......................................................... 9-1

9-1 Miscellaneous Functions (M3-Digit)....................................................................9-1

9-2 No. 2 Miscellaneous Functions (A8/B8/C8-Digit)................................................9-2

10 SPINDLE FUNCTIONS ...................................................................... 10-1

10-1 Spindle Function (S5-Digit Analog)...................................................................10-1

10-2 Spindle Clamp Speed Setting: G92..................................................................10-1

11 TOOL FUNCTIONS............................................................................ 11-1

11-1 Tool Function (4-Digit T-Code).........................................................................11-1

C-3

11-2 Tool Function (8-Digit T-Code).........................................................................11-1

12 TOOL OFFSET FUNCTIONS............................................................. 12-1

12-1 Tool Offset........................................................................................................12-1

12-2 Tool Length Offset/Cancellation: G43, G44, or T-Code/G49............................12-5

12-3 Tool Position Offset: G45 to G48......................................................................12-7

12-4 Tool Diameter Offset Function: G40, G41, G42 .............................................12-13

12-4-1 Overview............................................................................................................. 12-13

12-4-2 Tool diameter offsetting...................................................................................... 12-13

12-4-3 Tool diameter offsetting operation using other commands................................. 12-22

12-4-4 Corner movement............................................................................................... 12-29

12-4-5 Interruptions during tool diameter offsetting ....................................................... 12-29

12-4-6 General precautions on tool diameter offsetting................................................. 12-31

12-4-7 Offset number updating during the offset mode ................................................. 12-32

12-4-8 Excessive cutting due to tool diameter offsetting................................................ 12-34

12-4-9 Interference check.............................................................................................. 12-36

12-5 Three-Dimensional Tool Diameter Offsetting (Option)....................................12-43

12-5-1 Function description............................................................................................ 12-43

12-5-2 Programming methods ....................................................................................... 12-44

12-5-3 Correlationships to other functions..................................................................... 12-48

12-5-4 Miscellaneous notes on three-dimensional tool diameter offsetting................... 12-48

12-6 Programmed Data Setting: G10.....................................................................12-49

12-7 Tool Offsetting Based on MAZATROL Tool Data...........................................12-57

12-7-1 Selection parameters.......................................................................................... 12-57

12-7-2 Tool length offsetting .......................................................................................... 12-58

C-4

12-7-3 Tool diameter offsetting...................................................................................... 12-59

12-7-4 Tool data update (during automatic operation)................................................... 12-60

12-8 Shaping Function (Option)..............................................................................12-61

12-8-1 Overview............................................................................................................. 12-61

12-8-2 Programming format........................................................................................... 12-62

12-8-3 Detailed description............................................................................................ 12-62

12-8-4 Remarks ............................................................................................................. 12-69

12-8-5 Compatibility with the other functions.................................................................12-70

12-8-6 Sample program.................................................................................................12-71

13 PROGRAM SUPPORT FUNCTIONS................................................. 13-1

13-1 Hole Machining Pattern Cycles: G34.1/G35/G36/G37.1...................................13-1

13-1-1 Overview............................................................................................................... 13-1

13-1-2 Holes on a circle: G34.1 ....................................................................................... 13-2

13-1-3 Holes on a line: G35............................................................................................. 13-3

13-1-4 Holes on an arc: G36............................................................................................ 13-4

13-1-5 Holes on a grid: G37.1.......................................................................................... 13-5

13-2 Fixed Cycles.....................................................................................................13-7

13-2-1 Outline .................................................................................................................. 13-7

13-2-2 Fixed-cycle machining data format....................................................................... 13-8

13-2-3 G71.1 (Chamfering cutter CW)........................................................................... 13-11

13-2-4 G72.1 (Chamfering cutter CCW) ........................................................................ 13-12

13-2-5 G73 (High-speed deep-hole drilling)................................................................... 13-13

13-2-6 G74 (Reverse tapping) ....................................................................................... 13-14

13-2-7 G75 (Boring).......................................................................................................13-15

C-5

13-2-8 G76 (Boring).......................................................................................................13-16

13-2-9 G77 (Back spot facing)....................................................................................... 13-17

13-2-10 G78 (Boring) ....................................................................................................... 13-18

13-2-11 G79 (Boring) ....................................................................................................... 13-19

13-2-12 G81 (Spot drilling)............................................................................................... 13-19

13-2-13 G82 (Drilling)....................................................................................................... 13-20

13-2-14 G83 (Deep-hole drilling)...................................................................................... 13-21

13-2-15 G84 (Tapping)..................................................................................................... 13-22

13-2-16 G85 (Reaming) ................................................................................................... 13-23

13-2-17 G86 (Boring) ....................................................................................................... 13-23

13-2-18 G87 (Back boring)............................................................................................... 13-24

13-2-19 G88 (Boring) ....................................................................................................... 13-25

13-2-20 G89 (Boring) ....................................................................................................... 13-25

13-2-21 Synchronous tapping (Option)............................................................................ 13-26

13-3 Initial Point and R-Point Level Return: G98 and G99 .....................................13-30

13-4 Scaling ON/OFF: G51/G50.............................................................................13-31

13-5 Mirror Image ON/OFF: G51.1/G50.1..............................................................13-44

13-6 Subprogram Control: M98, M99 .....................................................................13-45

13-7 End Processing: M02, M30, M998, M999.......................................................13-52

13-8 Linear Angle Commands................................................................................13-53

13-9 Macro Call Function: G65, G66, G66.1, G67..................................................13-54

13-9-1 User macros ....................................................................................................... 13-54

13-9-2 Macro call instructions........................................................................................ 13-55

13-9-3 Variables............................................................................................................. 13-64

C-6

13-9-4 Types of variables............................................................................................... 13-66

13-9-5 Arithmetic operation commands.........................................................................13-84

13-9-6 Control commands.............................................................................................. 13-88

13-9-7 External output commands (Output via RS-232C).............................................. 13-92

13-9-8 External output command (Output onto the hard disk)....................................... 13-94

13-9-9 Precautions......................................................................................................... 13-96

13-9-10 Specific examples of programming using user macros ...................................... 13-98

13-10 Geometric Commads (Option)......................................................................13-102

13-11 Corner Chamfering and Corner Rounding Commands.................................13-103

13-11-1 Corner chamfering ( , C_)................................................................................. 13-103

13-11-2 Corner rounding ( ,R_)...................................................................................... 13-105

14 COORDINATE SYSTEM SETTING FUNCTIONS.............................. 14-1

14-1 Fundamental Machine Coordinate System, Workpiece Coordinate

Systems, and Local Coordinate Systems.........................................................14-1

14-2 Machine Zero Point and Second, Third, and Fourth Reference Points.............14-2

14-3 Fundamental Machine Coordinate System Selection: G53..............................14-3

14-4 Coordinate System Setting: G92......................................................................14-4

14-5 Automatic Coordinate System Setting..............................................................14-5

14-6 Reference Point Return: G28, G29 ..................................................................14-6

14-7 Second, Third, or Fourth Reference Point Return: G30....................................14-8

14-8 Reference Point Check Command: G27 ........................................................14-10

14-9 Workpiece Coordinate System Setting and Selection: (G92) G54 to G59......14-11

14-10 Additional Workpiece Coordinate System Setting and Selection: G54.1........14-16

C-7

14-11 Local Coordinate System Setting: G52...........................................................14-22

14-12 Reading/Writing of MAZATROL Program Basic Coordinates.........................14-27

14-12-1 Calling a macroprogram (for data writing) .......................................................... 14-27

14-12-2 Data reading ....................................................................................................... 14-27

14-12-3 Rewriting............................................................................................................. 14-28

14-13 Workpiece Coordinate System Rotation.........................................................14-29

14-14 Three-Dimensional Coordinate Conversion: G68...........................................14-42

15 MEASUREMENT SUPPORT FUNCTIONS........................................ 15-1

15-1 Skip Function: G31...........................................................................................15-1

15-1-1 Function description.............................................................................................. 15-1

15-2 Skip Coordinate Reading..................................................................................15-2

15-3 Amount of coasting in the execution of a G31 block.........................................15-3

15-4 Skip coordinate reading error...........................................................................15-4

15-5 Multi-Step Skip: G31.1, G31.2, G31.3, G04 .....................................................15-5

16 PROTECTIVE FUNCTIONS............................................................... 16-1

16-1 Pre-move Stroke Check ON/OFF: G22/G23 ....................................................16-1

17 THREADING: G33 (Option)................................................................ 17-1

17-1 Equal-Lead Threading......................................................................................17-1

17-2 Continuous Threading......................................................................................17-4

17-3 Inch Threading .................................................................................................17-4

18 DYNAMIC OFFSETTING: M173, M174 (Option) ............................... 18-1

C-8

19 HIGH-SPEED SMOOTHING CONTROL FUNCTION (OPTION)....... 19-1

19-1 Programming Format........................................................................................19-2

19-2 Commands Available in the High-Speed Smoothing Control Mode .................19-2

19-3 Additional Functions in the High-Speed Smoothing Control Mode...................19-3

19-4 Related Parameters..........................................................................................19-4

19-5 Remarks...........................................................................................................19-4

19-6 Related Alarms.................................................................................................19-4

20 FUNCTION FOR SELECTING THE CUTTING CONDITIONS........... 20-1

21 TORNADO TAPPING (G130)............................................................. 21-1

22 HIGH-SPEED MACHINING MODE FEATURE (OPTION)................. 22-1

23 AUTOMATIC TOOL LENGTH MEASUREMENT: G37 (OPTION) ..... 23-1

24 DYNAMIC OFFSETTING II: G54.2P0, G54.2P1 - G54.2P8

(OPTION)............................................................................................ 24-1

25 EIA/ISO PROGRAM DISPLAY........................................................... 25-1

25-1 Procedures for Constructing an EIA/ISO Program ...........................................25-1

25-2 Editing Function of EIA/ISO PROGRAM Display..............................................25-2

25-2-1 General................................................................................................................. 25-2

25-2-2 Operation procedure............................................................................................. 25-2

25-3 Macro-Instruction Input.....................................................................................25-8

25-4 Division of Display (Split Screen)......................................................................25-9

25-5 Editing Programs Stored in External Memory Areas ......................................25-12

C-9

- NOTE -

C-10

1 CONTROLLED AXES

1-1 Coordinate Words and Controlled Axes

Under standard specifications, there are three-dimensional controlled axes. With an added feature and a special option, the machine can control up to a maximum of six axes, including the three fundamental axes. The direction of machining can be designated using a predetermined coordinate word consisting of an alphabetic character.

For X-Y table

CONTROLLED AXES 1

+Y +X

Program coordinates

Workpiece X-Y table

For X-Y table and turntable

Table moving directions

Bed

MEP001

Table moving directions

Workpiece

Table turning direction

1-1

+Y +X

Program coordinates

MEP002

1 CONTROLLED AXES

- NOTE -

1-2

2 UNITS OF PROGRAM DATA INPUT

2-1 Units of Program Data Input

The movements on coordinate axes are to be commanded in the MDI mode or machining program. The movement data are expressed in millimeters, inches or degrees.

2-2 Units of Data Setting

Various data commonly used for control axes, such as offsetting data, must be set for the machine to perform an operation as desired. The units of data setting and those of program data input are listed below.

UNITS OF PROGRAM DATA INPUT 2

Units of program data input 0.0001 mm 0.00001 in. 0.0001 deg Units of data setting 0.0001 mm 0.00001 in. 0.0001 deg

Note 1: Inch/metric selection can be freely made using either bit 4 of parameter F91 (“0” for

metric, “1” for inches; validated through power-off and -on) or G-code command s (G20, G21). Selection using the G-code commands is valid only for program data input. Variables and offsetting data (such as tool offsetting data) should therefore be set beforehand using the appropriate unit (inch or metric) for the particular machining requirements.

Note 2: Metric data and inch data cannot be used at the same time.

2-3 Ten-Fold Program Data

Using a predetermined parameter, machining program data can be processed as set in units of one micron. There may be cases that a machining program which has been set in units of one micron is to be used with a numerical control unit based on 0.1 micron increment s. In such cases, use of this parameter allows the machine to perform the required machining operations without rewriting the program. Use bit 0 of user parameter F91 for this purpose. All types of coordinate data (axis movement data) not provided with the decimal point will be multiplied by a factor of 10. This does not apply, indeed, to preset tool-offsetting data designated with addresses H and D.

Linear axis

Metric system Inch system

Rotational axis

Linear axis

Rotational axis

Program

command

X1 (Y1 / Z1)

Moving distance when program commands are executed

NC (A) for which the

program was prepared

1 micron 0.1 micron 1 micron Applicable

0.001° 0.0001° 0.001° Applicable

Bit 0 of F91 = 0 Bit 0 of F91 = 1

MAZATROL (B)Controlled axis

2-1

Program

applicability

(A) → (B)

2 UNITS OF PROGRAM DATA INPUT

- NOTE -

2-2

3 DATA FORMATS

3-1 Tape Codes

This numerical control unit (in the remainder of this manual, referred to as the NC unit) uses

command information that consists of letters of the alphabet (A, B, C .... Z), numerics (0, 1, 2 ....

9), and signs (+, –, /, and so on). These alphanumerics and signs are referred to collectively as

characters. On paper tape, these characters are represented as a combination of a maximum of eight punched holes. Such a representation is referred to as a code. The NC unit uses either the EIA codes (RS-244-A) or the ISO codes (R-840).

Note 1: Codes not included in the tape codes shown in Fig. 3-1 will result in an error when they

are read.

Note 2: Of all codes specified as the ISO codes but not specified as the EIA codes, only the

following codes can be designated using the data I/O (Tape) parameters TAP9 to TAP14:

[ Bracket Open ] Bracket Close # Sharp ∗ Asterisk = Equal sign

:Colon However, you cannot designate codes that overlap existing ones or that result in parity error.

DATA FORMATS 3

Note 3: EIA/ISO code identification is made automatically according to the first EOB/LF code

appearing after the NC unit has been reset. (EOB: End Of Block, LF: Line Feed)

1. Significant information area (LABEL SKIP function)

During tape-based automatic operation, data storage into the memory, or data searching, the NC unit will ignore the entire information up to the first EOB code (;) in the tape when the unit is turned on or reset. That is, significant information in a tape refers to the information contained in the interval from the time a character or numeric code appears, following the first EOB code (;) after the NC unit has been reset, until a reset command is given.

2. Control Out, Control In

The entire information in the area from Control Out “(” to Control In “)” will be ignored in regard to machine control, while they will surely be displayed on the data display unit. Thus, this area can be used to contain information, such as the name and number of the command tape, that is not directly related to control. During tape storage, however, the information in this area will also be stored. The NC unit will enter the Control In status when power is turned on.

3-1

3 DATA FORMATS

Example of EIA Code

Control InControl Out

CON

P R 1 10

Name of tape is printed out

CON

1 1 1 1

Name of tape is punched in captital letters.

D E

R R R O

N U

.ONMARGO

N UL1

E O

1 1

E L

2DE

LCI

MEP003

Example of ISO Code

OBG0 X–8500 0 640 C U T T E R

Operator information is printed out.

Control Out

0 0 0

0 0 0G0 X 500 0 40 C U T T E R

(

The information at this portion is ignored and nothing is executed.

E T U R N )–

E T U R NR

Control In

E O B

3. EOR code (%)

In general, the EOR (End Of Record) code is punched at both ends of a tape and has the following functions:

- To stop rewinding (only when a rewinding device is provided)

- To start rewinding during tape data search (only when a rewinding device is provided)

- To terminate the storage of tape data.

MEP004

3-2

DATA FORMATS 3

4. Tape creation method for tape operation (Only when a rewinding device is used)

;

10 cm

2m First block Last block 2m

!!!!!!!!!

; ;

!!!!!!!!!

;

10 cm %%

TEP005

The two meters of dummy at both ends and the EOR (%) at the head are not required when a rewinding device is not used.

3-3

3 DATA FORMATS

EIA/ISO identification is made automatically by detecting whether EOB or LF initially appears after the NC unit has been reset.

EIA code (RS-244-A)

Feed holes

87654 321

Channel number

1 2 3 4 5 6 7 8 9 0

B C D E F G H I J K L M N O P Q R S T U V W X Y Z + – . , / EOR (End of Record) EOB (End of Block) or CR CO (2+4+5) CI (2+4+7)

Definable in parameters

BS (Back Space) TAB SP (Space) &

DEL (Delete)

S (All Space=Feed)* M (All Mark=EOB+DEL)*

ISO code (R-840)

Feed holes

87654 321

Channel number

1 2 3 4 5 6 7 8 9 0

B C D E F G H I J K L M N O P Q R S T U V W X Y Z + – . , / % LF (Line Feed) or NL ( (Control Out) ) (Control In) : # ? = [ ]

BS (Back Space) HT (Horizontal Tab) SP (Space) & CR (Carriage Return) $ ' (Apostrophe) ; < > ? @

" DEL (Delete) NULL DEL (Delete)

[1]

[2]

* The codes asterisked above are not EIA codes,

but may be used for the convenience’s sake.

Fig. 3-1 Tape codes

LF or NL acts as EOB and % acts as EOR.

MEP006

3-4

Codes in section [1] will only be stored as tape data when they are present in a comment section,

and ignored elsewhere in the significant information area. Codes in section [2] are non-operative and will always be ignored (but undergo the parity-V check). A dotted area indicates that the EIA Standard provides no corresponding codes.

3-2 Program Formats

A format predetermined for assigning control information to the NC unit is referred to as a program format. The program format used for our NC unit is word address format.

1. Words and addresses

A word is a set of characters arranged as shown below, and information is pro ce ssed in words.

DATA FORMATS 3

Word

Numeral

lphabet (address)

Word configuration

The alphabetic character at the beginning of a word is referred to as an address, which defines the meaning of its succeeding numeric information.

Table 3-1 Type and format of words

Item Metric command Inch command Program No. O8 Sequence No. N5 Preparatory function

Moving axis

Auxiliary axis

Dwell

Feed

Fixed cycle

Tool offset Miscellaneous function M3 × 4 Spindle function S5 Tool function No. 2 miscellaneous function B8, A8 or C8 Subprogram Variables number #5

Input unit

0.0001 mm (deg.),

0.00001 in.

0.0001 mm (deg.),

0.00001 in.

0.001 mm (rev),

0.0001 in.

0.0001 mm (deg.),

0.00001 in.

0.0001 mm (deg.),

0.00001 in.

X+54 Y+54 Z+54 α+54 X+45 Y+45 Z+45 α+45

I+54 J+54 K+54 I+45 J+45 K+45

F54 (per minute) F33 (per revolution)

R+54 Q54 P8 L4 R+45 Q45 P8 L4

G3 or G21

X54 P8 U54

F45 (per minute) F24 (per revolution)

H3 or D3

T4 or T8

P8 H5 L4

3-5

3 DATA FORMATS

1. Code O8 here indicates that program number can be set as an unsigned integer of eight digits following O, and for X+54, “+” indicates that the value can be signed (negative) and the two-digit number (54) indicates that the decimal point can be used and that five digits before and four after the decimal point are effective (5 + 4 = 9 digits are effective for a designation without decimal point).

2. The alpha sign ( rotational axis.

3. The number of digits in the words is checked by the maximum number of digits in the addresses.

4. When data with decimal point is used for address for which decimal input is not available, decimal figures will be ignored.

5. If the number of integral digits exceeds the specified format, an alarm will result.

6. If the number of decimal digits exceed the specified format, the excess will be rounded.

2. Blocks

A block, unit of instruction, contains a number of words which constitute information necessary for the NC machine to perform an operation. The end of each block must be indicated by an EOB (End Of Block) code.

3. Programs

A number of blocks form one program.

4. Program end

M02, M30, M99, M998, M999 or % is used as program end code.

α) denotes additional axis address. +44 will be used when α is specified for

3-3 Tape Data Storage Format

As with tape operation, tape data to be stored into the memory can be either of ISO or EIA code. The first EOB code read in after resetting is used by the NC unit for automatic identification of the code system ISO or EIA. The area of tape data to be stored into the memeory is, if the NC unit has been reset, from the character immediately succeeding the first EOB code the EOR code, and in all other cases, from the current tape position to the EOR code. Usually, therefore, start tape data storage operation after resetting the NC unit.

3-4 Optional Block Skip

1. Function and purpose

Optional block skip is a function that selectively ignores that specific block within a machining program which begins with the slash code “/”. Any block beginning with “/” will be ignored if the [BLOCK SKIP] menu function is set to ON, or will be executed if the menu function is set to OFF. For example, if all blocks are to be executed for a type of parts but specific blocks are not to be executed for another type, then different parts can be machined using one and the same program that contains the “/” code at the beginning of the specific blocks.

3-6

2. Operating notes

1. Blocks that have already been read into the pre-read buffer cannot be skipped.

2. This function is valid even during sequence number search.

3. During tape data storage (input) or output, all blocks, including those having a “/” code, are in- or outputted, irrespective of the status of the [BLOCK SKIP] menu function.

3-5 Program Number, Sequence Number and Block Number: O, N

Program numbers, sequence numbers, and block numbers are used to monitor the execution status of a machining program or to call a machining program or a specific process within a machining program. Program numbers are assigned to command blocks as required. A program number must be set using the letter O (address) and a numeric of a maximum of eight digits that follow O. Sequence numbers identify command blocks forming a machining program. A sequence number must be set using the letter N (address) and a numeric of a maximum of five digits that follow N. Block numbers are counted automatically within the NC unit, and reset to 0 each time a program number or a sequence number is read. These numbers will be counted up by one if the block to be read does not have an assigned program number or sequence number. All blocks of a machining program, therefore, can be uniquely defined by combining program number, sequence number, and block number as shown in the table below.

DATA FORMATS 3

NC input machining program

O1234 (DEMO. PROG) G92X0Y0 G90G51X–150. P0.75 N100G00X–50. Y–25. N110G01X250. F300 Y–225. X–50. Y–25. N120G51Y–125. P0.5 N130G00X–100. Y–75. N140G01X–200. Y–175. X–100. Y–75. N150G00G50X0Y0 N160M02 %

NC monitor display

Program No. Sequence No. Block No.

1234 0 0

1234 0 1

1234 0 2

1234 100 0

1234 110 0

1234 110 1

1234 110 2

1234 110 3

1234 120 0

1234 130 0

1234 140 0

1234 140 1

1234 140 2

1234 140 3

1234 150 0

1234 160 0

3-7

3 DATA FORMATS

3-6 Parity-H/V

One method of checking if the tape is correctly created is by parity checks. Parity checks are performed to check a tape for errors in punched codes, that is, for punching errors. There are two types of parity checks: parity-H and parity-V.

1. Parity-H check

Parity-H checks are intended to check the quantity of punched holes which form one character, and performed during tape operation, tape loading, and sequence-number searching. A parity-H error occurs in the following cases:

- ISO Codes

If a code with an odd number of punched holes is present in the significant information area.

- EIA Codes

If a code with an even number of punched holes is present in the significant information area or if non-punched holes (sprockets only) are present after a significant code in one block.

Example 1: Parity-H error (for EIA codes)

This character leads to a Parity-H error.

One block

This non-punched character will result in a Parity-H error.

These non-punched characters will not result in a Parity-H error.

If a parity-H error occurs, the tape will stop at the position next to the error code.

MEP007

3-8

+ 382 hidden pages