mazak Mazatrol Matrix Programming Manual

PROGRAMMING MANUAL

Return to Library

for

MAZATROL MATRIX

For INTEGREX IV

Programming EIA/ISO

MANUAL No. : H740PB0030E

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

01. 2006

Notes:

Return to Library

SAFETY PRECAUTIONS

Return to Library

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 m achine are explained below. Not onl y 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 t he pr ec aut ions t o b e obs erved as to the working methods and states usually expected. Of course, however, unexpec ted operations and/or un expected 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 c ontains as great an amount of information as it can, since it is not rare for the user to perfor m the operations that ov erstep the manufacturer -assumed ones, not all of “what the user ca nnot perform” or “what the user must not perform” c an 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, W ARNING, and CAUTION are as follows:

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

DANGER

: Failure to observe these ins tructions cou ld result i n serious har m to a h uman

life or body.

WARNING

: Failure to observe these instr uctions could result in m inor injuries or serio us

machine damage.

CAUTION

HGENPA0040E

S-1

Basics

Return to Library

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 pr oceeding to the next operati ons, fully check that c orrect data has been enter ed

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

! Bef ore machining workpieces , perform operational tes ts and make sure that the m achine

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 b y operating the machine at no load. Also, full y utilize tool path check, solid check, 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 feed rate and rotational speed ar e det er mined by the specifications of the to ol to be used, those of the workpiece to be m achined, and various ot her factors, actual c apabilities differ from the machine specif ications listed in this manual. If an inappropriate fee d rate or rotationa l 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 s tandard machining c onditions prior to shipping of the

machine from the fac tor y. In princ iple, these settings s houl d not be m odif ied. If it b ecom es absolutely necessary to modify the settings, perform modifications only after thoroughly understanding the func tions of the correspondin g parameters. Modifications usu ally aff ect any program. Unexpected operat ion 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 sugg es ted b y the Machini ng Na vig atio n Fu nctio n

- Cutting conditions for tools t hat are suggested to be used b y the Machining Navigation

Function

Confirm that every necessary precaution in regards to safe machine setup has been taken – especially for workpiec e fixtur ing/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

Return to Library

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

Return to Library

! For the machines of INT EGREX e-Series, programmed coor dinates can be rot ated using

an index unit of the MAZAT ROL program and a G68 command (coordinate rotate c ommand) of the EIA program. Ho wever, for exam ple, when the B-ax is is rotated thro ugh 180 degrees around the Y-axis to im plem ent mac hining with the tur ning spi ndle N o. 2, the pl us 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 progr am with the plus s id e of the X -ax is oriented in an up ward d irec tion, us e 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 solid check f unction, and other func tions, and confir m that the progr am operates properly. T he m odification of tool dat a ma y cause even a f ield-prove n m achining program to change in operational status. If the user operates the machine without be ing aware of an y 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- inc lu din g b lank (unmachined work piec e) s pecified in the common unit of the MAZATROL program, care is required since the tool will directly move from that position to the approac h point because of no obstructions be ing judged to be pres ent 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 in dependent posit ioning is se lected and sim ultaneously ra pid feed sel ected

for each axis, movem ents to the ending point wi ll not usually bec ome linear. Befor e using these functions, therefore, make sure that no obstructions are present on the path.

S-4

Operations

Return to Library

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 re lated persons. Also, the operator must check the setti ngs of the system variables before starting the above operations.

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

function, or other functions ar e execut ed, the wor kpiec e coord inate s ystems will usua ll y be shifted. When making machine restart after manual intervention, machine locking, the mirror image func tion, or other functions, c onsider the result ing amounts of s hift 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 mac hine for normal operation at no load. Since t he

feed rate at this tim e becomes a dry run r ate different from the program-designated f eed rate, the axes may move at a feed rate higher than the programmed value.

! After operation has been stopped tem porarily 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 ar ea. As a result, serious machine damage will result.

! Do not designate an incorr ect pulse multip lier when perf orming manual pulse h andle 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

OPERATIONAL WARRANTY FOR THE NC UNIT

Return to Library

OPERATIONAL WARRANTY FOR THE NC UNIT

The warranty of the manufacturer does not co ver a n y tr oub le aris i ng if the NC un it is us ed f or 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 pur pose 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 comm ercially available computer equipment

Operating Environment

1. Ambient temperature

During machine operation: 0° to 50°C (0° 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.

S-6

CONTENTS

Return to Library

Page

1 INTRODUCTION.................................................................................. 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 (Series T) ............................................................ 5-1

5-1-2 Absolute/Incremental data input: G90/G91 (Series M)........................................... 5-2

C-1

5-2 Inch/Metric Selection: G20/G21..........................................................................5-4

Return to Library

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

5-4 Polar Coordinate Input ON/OFF: G122/G123 [Series M: G16/G15]...................5-8

5-5 X-axis Radial Command ON/OFF: G122.1/G123.1 (Series T)...........................5-9

5-6 Selection between Diameter and Radius Data Input: G10.9 (Series M)...........5-10

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

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

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

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

6-4 Circular Interpolation Commands: G02, G03...................................................... 6-7

6-5 Radius Designated Circular Interpolation Commands: G02, G03 ....................6-10

6-6 Spiral Interpolation: G2.1, G3.1 (Option)..........................................................6-12

6-7 Plane Selection Commands: G17, G18, G19...................................................6-20

6-7-1 Outline .................................................................................................................. 6-20

6-7-2 Plane selection methods....................................................................................... 6-20

6-8 Polar Coordinate Interpolation ON/OFF: G12.1/G13.1.....................................6-21

6-9 Virtual-Axis Interpolation: G07..........................................................................6-25

6-10 Spline Interpolation: G06.1 (Option).................................................................6-26

6-11 NURBS Interpolation: G06.2 (Option)...............................................................6-37

6-12 Cylindrical Interpolation Command: G07.1.......................................................6-44

6-13 Threading.........................................................................................................6-47

6-13-1 Constant lead threading: G32 [Series M: G33]..................................................... 6-47

C-2

6-13-2 Inch threading: G32 [Series M: G33]....................................................................6-50

Return to Library

6-13-3 Continuous threading............................................................................................ 6-51

6-13-4 Variable lead threading: G34................................................................................ 6-52

6-13-5 Threading with C-axis interpolation: G01.1........................................................... 6-53

6-13-6 Automatic correction of threading start position (for overriding in a threading

cycle) .................................................................................................................... 6-55

6-14 Helical Interpolation: G17, G18, G19 and G02, G03 ........................................6-57

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

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

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

7-3 Asynchronous/Synchronous Feed: G98/G99 [Series M: G94/G95]....................7-1

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

7-5 Threading Leads.................................................................................................7-6

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

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

7-8 Exact-Stop Check Command: G09.....................................................................7-8

7-9 Exact-Stop Check Mode Command: G61.........................................................7-11

7-10 Automatic Corner Override Command: G62.....................................................7-11

7-11 Cutting Mode Command: G64..........................................................................7-16

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

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

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

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

C-3

8-1 Dwell Command in Time: (G98) G04 [Series M: (G94) G04]..............................8-1

Return to Library

8-2 Dwell Command in Number of Revolutions: (G99) G04 [Series M: (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 Constant Peripheral Speed Control ON/OFF: G96/G97...................................10-1

10-3 Spindle Clamp Speed Setting: G50 [Series M: G92]........................................10-3

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

11-1 Tool Function [for ATC systems]......................................................................11-1

11-2 Tool Function [4-Digit T-Code for Turret-Indexing Systems] (Series T) ............11-1

11-3 Tool Function [6-Digit T-Code for Turret-Indexing Systems] (Series T) ............11-2

11-4 Tool Function [8-digit T-code]...........................................................................11-2

12 TOOL OFFSET FUNCTIONS (FOR SERIES T)................................. 12-1

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

12-2 Tool Position Offset..........................................................................................12-3

12-3 Nose R/Tool Radius Compensation: G40, G41, G42.......................................12-5

12-3-1 Outline .................................................................................................................. 12-5

12-3-2 Tool nose point and compensation directions ...................................................... 12-7

12-3-3 Operations of nose R/tool radius compensation................................................... 12-8

12-3-4 Other operations during nose R/tool radius compensation................................. 12-15

C-4

12-3-5 Commands G41/G42 and I, J, K designation.....................................................12-22

Return to Library

12-3-6 Interruptions during nose R/tool radius compensation ....................................... 12-27

12-3-7 General precautions on nose R/tool radius compensation................................. 12-29

12-3-8 Interference check..............................................................................................12-30

12-4 Programmed Data Setting: G10.....................................................................12-35

12-5 Tool Offsetting Based on MAZATROL Tool Data...........................................12-44

12-5-1 Selection parameters.......................................................................................... 12-44

12-5-2 Tool diameter offsetting......................................................................................12-45

12-5-3 Tool data update (during automatic operation)................................................... 12-46

13 TOOL OFFSET FUNCTIONS (FOR SERIES M)................................ 13-1

13-1 Tool Offset........................................................................................................13-1

13-2 Tool Length Offset/Cancellation: G43, G44, or T-code/G49............................. 13-7

13-3 Tool Position Offset: G45 to G48....................................................................13-15

13-4 Tool Diameter Offset Function: G40, G41, G42 .............................................13-21

13-4-1 Overview............................................................................................................. 13-21

13-4-2 Tool diameter offsetting......................................................................................13-21

13-4-3 Tool diameter offsetting operation using other commands................................. 13-30

13-4-4 Corner movement............................................................................................... 13-37

13-4-5 Interruptions during tool diameter offsetting ....................................................... 13-37

13-4-6 Nose-R compensation........................................................................................13-39

13-4-7 General precautions on tool diameter offsetting................................................. 13-40

13-4-8 Offset number updating during the offset mode ................................................. 13-41

13-4-9 Excessive cutting due to tool diameter offsetting................................................ 13-43

13-4-10 Interference check .............................................................................................. 13-45

C-5

13-5 Three-Dimensional Tool Diameter Offsetting (Option)....................................13-52

Return to Library

13-5-1 Function description............................................................................................ 13-52

13-5-2 Programming methods ....................................................................................... 13-53

13-5-3 Correlationships to other functions.....................................................................13-57

13-5-4 Miscellaneous notes on three-dimensional tool diameter offsetting...................13-57

13-6 Programmed Data Setting: G10.....................................................................13-58

13-7 Tool Offsetting Based on MAZATROL Tool Data...........................................13-67

13-7-1 Selection parameters.......................................................................................... 13-67

13-7-2 Tool length offsetting .......................................................................................... 13-68

13-7-3 Tool diameter offsetting......................................................................................13-70

13-7-4 Tool data update (during automatic operation)................................................... 13-71

14 PROGRAM SUPPORT FUNCTIONS................................................. 14-1

14-1 Fixed Cycles for Turning...................................................................................14-1

14-1-1 Longitudinal turning cycle: G90 [Series M: G290] ................................................ 14-2

14-1-2 Threading cycle: G92 [Series M: G292]................................................................ 14-4

14-1-3 Transverse turning cycle: G94 [Series M: G294].................................................. 14-6

14-2 Compound Fixed Cycles ..................................................................................14-8

14-2-1 Longitudinal roughing cycle : G71 [Series M: G271] ............................................ 14-9

14-2-2 Transverse roughing cycle: G72 [Series M: G272]............................................. 14-14

14-2-3 Contour-parallel roughing cycle: G73 [Series M: G273].....................................14-16

14-2-4 Finishing cycle: G70 [Series M: G270] ............................................................... 14-20

14-2-5 Longitudinal cut-off cycle: G74 [Series M: G274] ............................................... 14-21

14-2-6 Transverse cut-off cycle: G75 [Series M: G275]................................................. 14-24

14-2-7 Compound threading cycle: G76 [Series M: G276] ............................................ 14-27

C-6

14-2-8 Checkpoints for compound fixed cycles: G70 to G76 [Series M: G270 to

Return to Library

G276].................................................................................................................. 14-34

14-3 Hole Machining Fixed Cycles: G80 to G89 [Series M: G80, G283 to

G289]..............................................................................................................14-37

14-3-1 Outline ................................................................................................................ 14-37

14-3-2 Face/Outside deep hole drilling cycle: G83/G87 [Series M: G283/G287]........... 14-40

14-3-3 Face/Outside tapping cycle: G84/G88 [Series M: G284/G288].......................... 14-41

14-3-4 Face/Outside boring cycle: G85/G89 [Series M: G285/G289]............................ 14-42

14-3-5 Face/Outside synchronous tapping cycle: G84.2/G88.2 [Series M:

G284.2/G288.2]..................................................................................................14-42

14-3-6 Hole machining fixed cycle cancel: G80............................................................. 14-44

14-3-7 Checkpoints for using hole machining fixed cycles ............................................ 14-44

14-3-8 Sample programs with fixed cycles for hole machining...................................... 14-46

14-4 Hole Machining Pattern Cycles: G234.1/G235/G236/G237.1 [Series M:

G34.1/G35/G36/G37.1] ..................................................................................14-47

14-4-1 Overview............................................................................................................. 14-47

14-4-2 Holes on a circle: G234.1 [Series M: G34.1] ...................................................... 14-48

14-4-3 Holes on a line: G235 [Series M: G35]...............................................................14-49

14-4-4 Holes on an arc: G236 [Series M: G36].............................................................. 14-50

14-4-5 Holes on a grid: G237.1 [Series M: G37.1]......................................................... 14-51

14-5 Fixed Cycles (Series M) .................................................................................14-53

14-5-1 Outline ................................................................................................................ 14-53

14-5-2 Fixed-cycle machining data format..................................................................... 14-54

14-5-3 G71.1 [Chamfering cutter CW] (Series M).......................................................... 14-57

14-5-4 G72.1 [Chamfering cutter CCW] (Series M) ....................................................... 14-58

14-5-5 G73 [High-speed deep-hole drilling] (Series M).................................................. 14-59

C-7

14-5-6 G74 [Reverse tapping] (Series M)......................................................................14-60

Return to Library

14-5-7 G75 [Boring] (Series M)...................................................................................... 14-61

14-5-8 G76 [Boring] (Series M)...................................................................................... 14-62

14-5-9 G77 [Back spot facing] (Series M)...................................................................... 14-63

14-5-10 G78 [Boring] (Series M)......................................................................................14-64

14-5-11 G79 [Boring] (Series M)......................................................................................14-65

14-5-12 G81 [Spot drilling] (Series M).............................................................................. 14-65

14-5-13 G82 [Drilling] (Series M) ..................................................................................... 14-66

14-5-14 G83 [Deep-hole drilling] (Series M) .................................................................... 14-67

14-5-15 G84 [Tapping] (Series M) ................................................................................... 14-68

14-5-16 G85 [Reaming] (Series M)..................................................................................14-69

14-5-17 G86 [Boring] (Series M)......................................................................................14-69

14-5-18 G87 [Back boring] (Series M) ............................................................................. 14-70

14-5-19 G88 [Boring] (Series M)......................................................................................14-71

14-5-20 G89 [Boring] (Series M)......................................................................................14-71

14-5-21 Synchronous tapping [Option] (Series M)........................................................... 14-72

14-6 Initial Point and R-Point Level Return: G98 and G99 (Series M)....................14-76

14-7 Scaling ON/OFF: G51/G50 (Series M)...........................................................14-77

14-8 Mirror Image ON/OFF: G51.1/G50.1 (Series M).............................................14-90

14-9 Subprogram Control: M98, M99 .....................................................................14-91

14-10 End Processing: M02, M30, M998, M999.....................................................14-100

14-11 Chamfering and Corner Rounding at Right Angle Corner ............................14-102

14-12 Chamfering and Corner Rounding at Arbitrary Angle Corner Function......... 14-105

14-12-1 Chamfering at arbitrary angle corner: , C_ ....................................................... 14-105

C-8

14-12-2 Rounding at arbitrary angle corner: , R_........................................................... 14-106

Return to Library

14-13 Linear Angle Commands..............................................................................14-107

14-14 Macro Call Function: G65, G66, G66.1, G67................................................14-108

14-14-1 User macros ..................................................................................................... 14-108

14-14-2 Macro call instructions ...................................................................................... 14-109

14-14-3 Variables........................................................................................................... 14-118

14-14-4 Types of variables............................................................................................. 14-120

14-14-5 Arithmetic operation commands ....................................................................... 14-141

14-14-6 Control commands............................................................................................ 14-145

14-14-7 External output commands (Output via RS-232C)............................................ 14-149

14-14-8 External output command (Output onto the hard disk).....................................14-151

14-14-9 Precautions....................................................................................................... 14-153

14-14-10 Specific examples of programming using user macros ................................. 14-155

14-15 Geometric Commads (Option)......................................................................14-159

15 COORDINATE SYSTEM SETTING FUNCTIONS.............................. 15-1

15-1 Coordinate System Setting Function: G50 [Series M: G92]..............................15-1

15-2 MAZATROL Coordinate System Cancellation: G52.5 (Series T) .....................15-5

15-3 Selection of MAZATROL Coordinate System: G53.5 (Series T) ......................15-7

15-4 Selection of Workpiece Coordinate System: G54 to G59.................................15-9

15-5 Workpiece Coordinate System Shift...............................................................15-10

15-6 Change of Workpiece Coordinate System by Program Command.................15-10

15-7 Selection of Machine Coordinate System: G53..............................................15-11

15-8 Selection of Local Coordinate System: G52...................................................15-12

C-9

15-9 Automatic Return to Reference Point (Zero Point): G28, G29........................15-13

Return to Library

15-10 Return to Second Reference Point (Zero Point): G30 ....................................15-15

15-11 Return to Reference Point Check Command: G27.........................................15-17

15-12 Programmed Coordinate Conversion ON/OFF: G68.5/G69.5 [Series M:

G68/G69]........................................................................................................15-18

15-13 Workpiece Coordinate System Rotation (Series M) .......................................15-22

16 MEASUREMENT SUPPORT FUNCTIONS........................................ 16-1

16-1 Skip Function: G31...........................................................................................16-1

16-1-1 Function description.............................................................................................. 16-1

16-1-2 Amount of coasting............................................................................................... 16-3

16-1-3 Skip coordinate reading error ............................................................................... 16-4

17 PROTECTIVE FUNCTIONS............................................................... 17-1

17-1 Stored Stroke Limit ON/OFF: G22/G23............................................................17-1

18 TWO-SYSTEM CONTROL FUNCTION ............................................. 18-1

18-1 Two-Process Control by One Program: G109..................................................18-1

18-2 Specifying/Cancelling Cross Machining Control Axis: G110/G111...................18-2

18-3 M, S, T, B Output Function to Counterpart: G112 ............................................18-7

19 COMPOUND MACHINING FUNCTIONS........................................... 19-1

19-1 Programming for Compound Machining...........................................................19-1

19-2 Waiting Command: M950 to M997, P1 to P99999999......................................19-2

19-3 Balanced Cutting..............................................................................................19-4

19-4 Milling with the Lower Turret.............................................................................19-6

C-10

19-5 Compound Machining Patterns ........................................................................19-8

Return to Library

20 POLYGONAL MACHINING AND HOBBING (OPTION)..................... 20-1

20-1 Polygonal Machining ON/OFF: G51.2/G50.2 ...................................................20-1

20-2 Selection/Cancellation of Hob Milling Mode: G114.3/G113..............................20-3

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

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

23 AUTOMATIC TOOL LENGTH MEASUREMENT: G37 (OPTION

FOR SERIES M)................................................................................. 23-1

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

(OPTION FOR SERIES M)................................................................. 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-11

- NOTE -

Return to Library

C-12

1 INTRODUCTION

Return to Library

EIA/ISO programs executed by the CNC unit include two modes: One is based on the G-code series T (designed for turning machines), and the other is based on the G-code series M (designed for machining centers). Depending on the types of machines, the G-code series T and M are used as follows:

G-code series T for the INTEGREX-IV machines, and G-code series M for the INTEGREX-e machines.

This manual gives descriptions in general with respect to the G-code series T designed for turning machines.

INTRODUCTION 1

1-1

1 INTRODUCTION

Return to Library

- NOTE -

1-2

2 UNITS OF PROGRAM DATA INPUT

Return to Library

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 cann ot 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)Control axis

2-1

Program

applicability

(A) → (B)

2 UNITS OF PROGRAM DATA INPUT

Return to Library

- NOTE -

2-2

3 DATA FORMATS

Return to Library

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

Return to Library

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

2DE

LCI

MEP003

Example of ISO Code

OBG0 X–850 0 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

Return to Library

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

Return to Library

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,

Return to Library

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 processed 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.)/min,

0.00001 in./min

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)

T1 or T2

T4 or T6

P4 Q5 L4

3-5

+ 501 hidden pages