mazak Mazatrol Matrix Programming Manual

Download

PROGRAMMING MANUAL

Return to Main Menu

for

MAZATROL MATRIX

(For INTEGREX IV)

MAZATROL Program

MANUAL No. : H740PA0031E

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

10. 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 MAZATROL PROGRAM CONFIGURATION........................................ 1-1

1-1 Program Configuration .......................................................................................1-1

2 PROGRAM COORDINATE SYSTEM .................................................. 2-1

3 PROGRAM CREATION........................................................................ 3-1

3-1 Procedure for Program Creation ........................................................................3-1

3-2 Common Unit .....................................................................................................3-6

3-2-1 Setting unit data (common data)............................................................................. 3-6

3-3 Materials Shape Unit (MATERIAL).....................................................................3-8

3-3-1 Setting unit data...................................................................................................... 3-8

3-3-2 Setting sequence data............................................................................................ 3-8

3-4 Types of the Milling Unit...................................................................................3-12

3-4-1 Planes to be machined and machining methods.................................................. 3-12

3-5 Point Machining Units.......................................................................................3-15

3-5-1 Types of point machining units.............................................................................3-15

3-5-2 Procedure for selecting point machining unit........................................................ 3-16

3-5-3 Unit data and automatic tool development of the point machining unit ................ 3-17

3-5-4 Automatic tool development for carbide drills....................................................... 3-35

3-5-5 New tapping auto-setting scheme ........................................................................ 3-36

3-5-6 Tool sequence data of the point machining unit...................................................3-41

3-5-7 Tool path of the point machining unit.................................................................... 3-47

3-5-8 Shape sequence data of the point machining unit................................................ 3-96

3-6 Line Machining Units......................................................................................3-116

C-1

3-6-1 Types of line machining units ............................................................................. 3-116

3-6-2 Procedure for selecting line machining unit........................................................ 3-117

3-6-3 Unit data, automatic tool development and tool path of the line machining

unit...................................................................................................................... 3-118

3-6-4 Tool sequence data of the line machining unit ................................................... 3-157

3-6-5 Shape sequence data of the line machining unit................................................ 3-160

3-6-6 Precautions in line machining............................................................................. 3-161

3-6-7 Automatic corner override................................................................................... 3-165

3-7 Face Machining Units.....................................................................................3-167

3-7-1 Types of face machining units............................................................................3-167

3-7-2 Procedure for selecting face machining unit....................................................... 3-168

3-7-3 Unit data, automatic tool development and tool path of the face machining

unit...................................................................................................................... 3-169

3-7-4 Tool sequence data of the face machining unit..................................................3-214

3-7-5 Precautions in face machining............................................................................ 3-220

3-7-6 Override in case of the overall width cutting....................................................... 3-230

3-7-7 Shape sequence data of the line/face machining unit........................................3-232

3-8 Turning Units..................................................................................................3-257

3-8-1 Types of turning units ......................................................................................... 3-257

3-8-2 Procedure for selecting turning unit.................................................................... 3-257

3-9 Bar-Materials Machining Unit (BAR)...............................................................3-259

3-9-1 Setting unit data.................................................................................................. 3-259

3-9-2 Setting tool sequence data................................................................................. 3-263

3-9-3 Setting shape sequence data............................................................................. 3-269

3-10 Copy-Machining Unit (CPY) ...........................................................................3-274

C-2

3-10-1 Setting unit data.................................................................................................. 3-274

3-10-2 Setting tool sequence data................................................................................. 3-276

3-10-3 Setting shape sequence data............................................................................. 3-278

3-11 Corner-Machining Unit (CORNER).................................................................3-279

3-11-1 Setting unit data.................................................................................................. 3-279

3-11-2 Setting tool sequence data................................................................................. 3-280

3-11-3 Setting shape sequence data............................................................................. 3-282

3-12 Facing Unit (FACING) ....................................................................................3-283

3-12-1 Setting unit data.................................................................................................. 3-283

3-12-2 Setting tool sequence data................................................................................. 3-284

3-12-3 Setting shape sequence data............................................................................. 3-286

3-13 Threading Unit (THREAD)..............................................................................3-288

3-13-1 Setting unit data.................................................................................................. 3-288

3-13-2 Setting tool sequence data................................................................................. 3-291

3-13-3 Setting sequence data........................................................................................ 3-294

3-14 Grooving Unit (T. GROOVE)..........................................................................3-297

3-14-1 Setting unit data.................................................................................................. 3-297

3-14-2 Setting tool sequence data................................................................................. 3-300

3-14-3 Setting shape sequence data............................................................................. 3-304

3-15 Turning Drilling Unit (T. DRILL) ......................................................................3-308

3-15-1 Setting unit data.................................................................................................. 3-308

3-15-2 Setting tool sequence data................................................................................. 3-309

3-15-3 Setting shape sequence data............................................................................. 3-315

3-16 Turning Tapping Unit (T. TAP) .......................................................................3-316

C-3

3-16-1 Setting unit data.................................................................................................. 3-316

3-16-2 Setting tool sequence data................................................................................. 3-319

3-16-3 Setting shape sequence data............................................................................. 3-321

3-17 Mill-Turning Unit (MILLTURN)........................................................................3-322

3-17-1 Setting unit data.................................................................................................. 3-322

3-17-2 Setting tool sequence data................................................................................. 3-323

3-17-3 Setting shape sequence data............................................................................. 3-325

3-18 Other Units.....................................................................................................3-326

3-19 Manual Program Machining Unit (MANL PRG)..............................................3-327

3-19-1 Setting unit data.................................................................................................. 3-327

3-19-2 Setting sequence data........................................................................................ 3-329

3-20 M-Code Unit (M-CODE) .................................................................................3-331

3-20-1 Setting unit data (M-code) .................................................................................. 3-331

3-21 Head Selection Unit (HEAD) ..........................................................................3-333

3-21-1 Setting unit data.................................................................................................. 3-333

3-22 Workpiece Transfer Unit (TRANSFER)..........................................................3-334

3-22-1 Setting unit data.................................................................................................. 3-334

3-23 Subprogram Unit (SUB PRO).........................................................................3-338

3-23-1 Setting unit data.................................................................................................. 3-338

3-23-2 Setting sequence data........................................................................................ 3-339

3-24 Add-In MAZATROL Unit.................................................................................3-341

3-24-1 Setting unit data.................................................................................................. 3-341

3-24-2 Setting sequence data........................................................................................ 3-341

3-24-3 Help function on Add-in MAZATROL.................................................................. 3-342

C-4

3-25 End Unit (END)...............................................................................................3-346

3-25-1 Setting unit data.................................................................................................. 3-346

3-25-2 Setting sequence data........................................................................................ 3-350

3-26 Simultaneous Machining Unit (SIMULTAN)....................................................3-351

3-26-1 Procedure for calling up the SIMULTAN unit...................................................... 3-351

3-26-2 Setting unit data.................................................................................................. 3-351

3-27 Two-Workpiece Machining Unit (2 WORKPC) ...............................................3-352

3-27-1 Procedure for calling up the 2 WORKPC unit..................................................... 3-352

3-27-2 Setting unit data.................................................................................................. 3-352

3-28 Coordinate Measuring Unit (MMS).................................................................3-353

3-28-1 Procedure for calling up the MMS unit................................................................ 3-353

3-28-2 Setting unit data.................................................................................................. 3-353

3-28-3 Setting sequence data........................................................................................ 3-353

3-28-4 Type of measurement......................................................................................... 3-355

3-29 Workpiece Measuring Unit (WORK MES)......................................................3-358

3-29-1 Procedure for selecting workpiece measuring unit............................................. 3-358

3-29-2 Setting the unit data............................................................................................ 3-358

3-29-3 Setting the sequence data.................................................................................. 3-359

3-29-4 Selection of a measurement type.......................................................................3-360

3-29-5 Offset value and the direction of offset............................................................... 3-369

3-29-6 Offset judgment .................................................................................................. 3-373

3-30 Tool Measuring Unit (TOOL MES)..................................................................3-374

3-30-1 Procedure for selecting tool measuring unit ....................................................... 3-374

3-30-2 Setting the unit data............................................................................................ 3-374

C-5

3-30-3 Setting the sequence data.................................................................................. 3-375

3-30-4 Measuring patterns............................................................................................. 3-376

4 PRIORITY FUNCTION FOR THE SAME TOOL................................... 4-1

4-1 Priority Machining Order.....................................................................................4-1

4-2 Priority Machining Zone......................................................................................4-4

4-3 Editing Function and Input Method of Priority Numbers .....................................4-6

4-3-1 Input of priority numbers......................................................................................... 4-6

4-3-2 Assignment of priority numbers .............................................................................. 4-7

4-3-3 Change of priority numbers .................................................................................... 4-8

4-3-4 Deletion of all the priority numbers.........................................................................4-9

4-3-5 How to use the SUB PROG PROC END function .................................................. 4-9

4-4 Relation between the Subprogram Unit and the Priority Machining

Function............................................................................................................4-11

4-5 Relation between the M-Code Unit and the Priority Machining Function..........4-12

5 LOWER-TURRET CONTROL FUNCTIONS ........................................ 5-1

5-1 Machining with the Lower Turret ........................................................................5-1

5-1-1 Independent machining with the lower turret.......................................................... 5-1

5-1-2 Simultaneous machining with the upper and lower turrets ..................................... 5-2

5-1-3 Balanced cutting with the upper and lower turrets.................................................. 5-6

5-1-4 Simultaneous machining of processes 1 and 2, using the upper and lower

turrets (optional)...................................................................................................... 5-7

5-2 Retraction of the Lower Turret..........................................................................5-10

5-3 Other Setup Items............................................................................................5-12

5-3-1 LTUR DIA in common unit.................................................................................... 5-12

C-6

6 TPC DATA SETTING ........................................................................... 6-1

6-1 Operating Procedure for Setting TPC (Tool-Path Control) Data.........................6-1

6-2 Description of Each TPC Data Item of Turning Unit and Measurement

Unit.....................................................................................................................6-4

7 PROGRAM EDITING............................................................................ 7-1

7-1 Operating Procedures for Editing Programs.......................................................7-1

7-2 Search................................................................................................................7-2

7-3 Insertion..............................................................................................................7-6

7-4 Deletion............................................................................................................7-10

7-5 Copy.................................................................................................................7-14

8 PROGRAM CREATING/EDITING FUNCTIONS.................................. 8-1

8-1 Help Function.....................................................................................................8-1

8-2 Automatic Crossing-Point Calculation Function..................................................8-2

8-2-1 Automatic crossing-point calculation in the line and face machining units............. 8-2

8-2-2 Automatic crossing-point calculation function in the turning unit............................8-6

8-3 Automatic Cutting-Conditions Setting Function................................................8-15

8-4 Desk Calculator Functions................................................................................8-18

8-5 Tool Data Window............................................................................................8-19

8-6 Tool File Window..............................................................................................8-20

9 SAMPLE PROGRAMS......................................................................... 9-1

10 THREE-DIGIT G-FORMAT................................................................. 10-1

10-1 Outline.............................................................................................................. 10-1

C-7

10-2 Detailed Description .........................................................................................10-1

10-3 Three-Digit G-Format of MAZATROL Program................................................10-2

10-4 Various Data Description Using G10..............................................................10-20

C-8

1 MAZATROL PROGRAM CONFIGURATION

1-1 Program Configuration

MAZATROL programs are each made up of a set of data referred to as unit. The following types of units are prepared for this NC equipment:

Common unit Materials shape unit Machining unit Milling unit Point mach ining unit Drilling

MAZATROL PROGRAM CONFIGURATION 1

Counterbore machining Inversed faced hole machining Reaming Tapping Boring Through hole

Non-through hole Stepped through hole

Stepped non-through hole Back boring Circular milling Counterbore-tapping

Line machining unit Central linear machining

Face machining unit Face milling

Turning unit Bar-materials machining Manual program machining unit Copy-machining End unit Corner-machining M-code unit Facing Subprogram unit Threading Coordinate measuring unit Grooving Workpiece measuring unit Drilling (turning) Tool measuring unit Tapping (turning) Head selection unit Mill-turning Workpiece transfer unit Process end unit Simultaneous machining unit Two-workpiece machining unit Add-in MAZATROL unit

Right-hand linear machining Left-hand linear machining Outside linear machining Inside linear machining Right-hand chamfering Left-hand chamfering Outside chamfering Inside chamfering

End milling-top End milling-step Pocket milling Pocket milling-mountain Pocket milling-valley End milling slot

1-1

1 MAZATROL PROGRAM CONFI GURATION

Data to be set in the units listed above is classified into the following four major types:

1. Unit data The data consists of data on the type of machining and the sections to be machined, etc.

2. Tool sequence data The tool sequence data consists of tool names and other data relating to the operation of the tools. This type of data exists for the milling (point, linear, and face machining) and turning units. For other units, data relating to tools exists with the unit data.

3. Shape sequence data The data consists mainly of data used to define machining patterns.

4. TPC data (Tool path control data) TPC data is the auxiliary data to be set on the TPC display. The data consists of tool path/tool change position adjustment data, M-codes, tool offset numbers, etc. Tool paths are automatically generated according to the data set on the PROGRAM display and various parameters. TPC data is intended to eliminate unnecessary paths by changing thus-generated tool paths on an unit-by-unit basis. Machining itself, therefore, will be executed even if TPC data is not set.

Example: PROGRAM display

UNo. MAT. OD-MAX ID-MIN LENGTH WORK FACE ATC MODE RPM LTUR DIA

0 FC 70. 0. 97. 2 0 3000

UNo. UNIT MODE POS-B POS-C DIA DEPTH CHMF

1 DRILLING ZC ! ! 10. 20. 0. SNo.TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M

1 CTR-DR 12. A 10. !! ! 90. SPOT 25 0.1 2 DRILL 10. 10. 20. 0. 100 DRIL T 5. 63 0.1

FIG PTN SPT-R/x SPT-C/y SPT-Z SPT-Y NUM. ANGLE Q R

1 PT 0. 0. 0. 0. ! ! ! 0 UNo. UNIT MODE POS-B POS-C SRV-A SLOT-WID BTM WAL FIN-A FIN-R PAT.

2 SLOT ZY ! 90. 10. 20. 4 4 0. 0. 0 SNo. TOOL NOM-φ No. # APRCH-1 APRCH-2 TYPE AFD DEP-A DEP-R C-SP FR M M M

F1 END MILL 20. A ? ? CW G01 ! ! 120 0.13 FIG PTN SPT-R Z Y R/th I J P CNR RGH

1 LINE 25. 20. 20. 2 LINE ! 20. –20.

A: Unit data B: Tool sequence data C: Shape sequence data

Specific details and setting procedures of each data are described in Chapter 3. Here (Chapter

1), you should understand what types of units and data constitute a program.

Note: Specify tools in program by their tool names, nominal diameters and suffixes.

Specify tools in the tool sequence data. To operate the machine in the automatic operation mode, the tools that have been specified in the program must be registered on the TOOL DATA display.

1-2

2 PROGRAM COORDINATE SYSTEM

In general, machining dimensions on a drawing are indicated as the distances from a specific reference point. Likewise, within a program, a machining pattern is defined by setting the coordinates from a specific reference point. This reference point is referred to as the program origin and the coordinate system based on the program origin is referred to as the program coordinate system. For MAZATROL programs, the following coordinate system is used to define machining patterns:

PROGRAM COORDINATE SYSTEM 2

Program origin

T3P001

The program origin of X-Z-coordinates system can be set anywhere on the center line of the workpiece. Usually, however, the crossing point of the center line of the workpiece and its finishing edge surface should be taken as the program origin. The program origin of C-axis (rotational axis) can be set at any position convenient for programming. For MAZATROL programs, set X-coordinates as diameter data. That is, the workpiece diameter indicated on the drawing must be set as it is.

Example: For the workpiece shape shown in the diagram below:

The coordinates (x, z) of point A are (50, 20), and the coordinates (x, z) of point B (20, 30).

20φ50

T3P008

Note 1: For manual program machining units (MANL PRG) and facing units (FACING), the

direction of Z-axis is opposite to the one shown in the diagram above. See the relevant items in Chapter 3 for further details.

Note 2: Refer to the sections of milling units for details on the C- and Y-axes.

2-1

2 PROGRAM COORDINATE SYSTEM

- NOTE -

2-2

3 PROGRAM CREATION

Both the program data and sequence data within a MAZATROL program must be set on the PROGRAM display, and TPC data must be set on the TPC display. The TPC display is call ed up from the PROGRAM display.

This chapter first describes general procedures and precautions related to creating a MAZATROL program and then describes detailed procedures for setting each type of program data on a unit-by-unit basis.

3-1 Procedure for Program Creation

(1) Select the PROGRAM display.

- Carry out the following operations to call up the PROGRAM display:

1) Press the display selector key. ! You will then see the follo wing main -display selection me nu in the menu di splay area of

your screen:

PROGRAM CREATION 3

POSITION SET UP

INFO

PROGRAM TOOL

DATA

CUTTING

COND.

PARAM DIANOS DATA

IN/OUT

TOOL

LAYOUT

2) Press the [PROGRAM] m enu key. ! The program last selected will be displayed on the PROGRAM display and the current

menu will change over to this one:

WORK No. FIND PROGRAM BARRIER

INFORM.

WPC MSR TOOL

PATH

PROCESS CONTROL

PROGRAM

LAYOUT

HELP PROGRAM

(2) Press the [WORK No.] menu key.

! The display of [WORK No.] becomes highlighted and the work-Nos. listing window will

be displayed.

* The work-Nos. listing window refers to a window that displays a list of work numbers of the

programs that have already been registered in the NC equipment.

(3) Set the work number of the creating program.

- A “work number” refers to a number assigned to each program to distinguish one program

from another. A combination of up to 32 alphanumeric characters: 0 to 9 and A to Z, including the symbols “_”, “.”, “+” and “–”, can be used for a work number.

Note 1: If a work number is composed of figures alone, it should be a natural number

between 1 and 99999999.

DISPLAY

MAP

FILE

Note 2: A program name should not begin with a dot (.).

- If a work number already registered in the NC unit is set, that program will be displayed on

the screen. To create a new MAZATROL program, therefore, you must set a work number not used in other programs. You can check the work-Nos. listing window or the PROGRAM FILE display to see which work numbers are not yet used

3-1

3 PROGRAM CREATION

- If you set a work number not used for the programs that have been registered in the NC

unit, the current menu will change over to this one:

WORK No. EIA/ISO

* The EIA/ISO programming function is optional.

(4) Press the [MAZATROL PROGRAM] menu key.

! The following line will be displayed on the screen:

UNo. MAT. OD-MAX ID-MIN LENGTH WORK FACE ATC MODE RPM LTUR DIA

This line denotes the common unit.

(5) Set data in each item of the common unit.

- See Section 3-2, “Common Unit” for details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

- When you set data in the last item of the common unit, the cursor will move to the starting

position of the next line and then the following menu A will be displayed, and pressing the [ >>> ] menu key changes A → B → C → A → B → C in order.

PROGRAM

Cursor

MAZATROL

PROGRAM

POINT

MACH-ING

SELECT

HEAD

LINE

MACH-ING

TRANSFER WORKPICE

FACE

MACH-ING

PROCESS

END

TURNING MANUAL

PROGRAM

M CODE

SUB

PROGRAM

WPC MSR WORKPICE

MEASURE

END SHAPE

CHECK

TOOL

MEASURE

SIMUL. 2 WORKPC

WORKPIECE

SHAPE

MODE

(6) From the menus A, B and C, select a unit that is to follow the common unit.

! The unit data line of the selected unit will be displayed in the screen. Example: If you have selected the bar-materials machining unit (BAR):

UNo. MAT. OD-MAX ID-MIN LENGTH WORK FACE ATC MOCE RPM LTUR DIA

0 CBN STL 100. 0. 100. 2. 0 3000 120.

UNo. UNIT PART POS-B CPT-X CPT-Z FIN-X FIN-Z

1 BAR

↑

Cursor

This line will be displayed.

If you have selected a unit that consists of only unit data (e. g. M-code unit):

>>>

"""

(7) Set data in each item on the unit data line.

- See the relevant part of this section for further detail of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

- When you set data in the last item, the cursor will move to the beginning of the next line

(unit data line).

3-2

PROGRAM CREATION 3

If you have selected a unit that consists of unit data, tool sequence data, and shape sequence data of only one line (e. g. corner-machining unit):

(7)-1 Set data in each item on the unit data line.

- See the relevant part of this section for further detail of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

- When you set data in the last item, the cursor will move to the beginning of the next line

(tool sequence data line).

(7)-2 Set data in each item on the tool sequence data line.

- See the relevant part of this section for further details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

- When you set data in the last item, the cursor will move to the beginning of the next line

(shape sequence data line).

(7)-3 Set data in each item on the shape sequence data line.

- See the relevant part of this section for further details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

- When you set data in the last item, the cursor will move to the beginning of the next line

(unit data line).

If you have selected a unit that consists of unit data, tool sequence data, and shape sequence data of multiple lines (e. g. bar-materials machining unit):

(7)-1 Set data in each item on the unit data line.

- See the relevant part of this section for further details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

- When you set data in the last item, the cursor will move to the beginning of the next line

(tool sequence data line).

(7)-2 Set data in each item on the tool sequence data line.

- See the relevant part of this section for further details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

- When you set data in the last item, the cursor will move to the beginning of the next line

(shape sequence data line).

(7)-3 Set data in each item on the shape sequence data line.

- See the relevant part of this section for further details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

(7)-4 After you have set the entire shape sequence data, press the [SHAPE END] menu key.

- The line that immediately succeeds the last shape sequence data line will be displayed as

a unit data line.

- For a unit that permits you to set more than one line of shape sequence data, you cannot

select the next unit unless you carry out this operation (pressing the [SHAPED END] menu key).

3-3

3 PROGRAM CREATION

If you have selected a unit that consists of unit data, tool sequence data of multiple lines and shape sequence data of multiple lines (e. g. drilling unit):

(7)-1 Set data in each item on the unit data line.

- See the relevant part of this section for further details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

- When you set data in the last item, the tool sequence data is made automatically and the

cursor will move to the beginning of the tool sequence data line.

(7)-2 Set data in each item on the tool sequence data line.

- See the relevant part of this section for further details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

(7)-3 After you have set the entire tool sequence data, set data in each item on the shape

sequence data line.

- See the relevant part of this section for further details of the data to be set.

- Each time you set data, the cursor moves to the next item automatically.

(7)-4 After you have set the entire shape sequence data, press the [SHAPE END] menu key.

- The line that immediately succeeds the last shape sequence data line will be displayed as

a unit data line.

- For a unit that permits you to set more than one line of shape sequence data, you cannot

select the next unit unless you carry out this operation (pressing the [SHAPED END] menu key).

(8) Select the units required for the intended machining operation by repeating steps (6) and (7)

above (including steps (7)-1, (7)-2, (7)-3 and (7)-4), and then set data in each of the items displayed on the screen.

- A selectable unit differs according to the type of product to be machined. Select a unit in

the most suitable order in accordance with your machining drawing, unit sheet, etc. After unit selection, the program can be generated just by setting data as guided by messages.

(9) Set the end unit at the end of the program.

- Press the [END] menu key.

- Without the end unit, the program will not be regarded as a complete one. Therefore, you

must set the end unit at the last line of the program.

(10) Set data in each item of the end unit.

- See the section “End Unit (END)” for details of the data to be set.

Note 1: One MAZATROL program can contain a maximum of 1000 units, including the

common unit and the end unit. For units that allow you to set multiple lines of sequence data, up to a maximum of 200 lines of shape sequence data can be regi ste red per unit.

Note 2: The shape data that you have set can be checked for errors by calling up the SHAPE

CHECK display while you are creating the program. See the Operating Manual for

details.

3-4

Note 3: For the following units, TPC data can be set as required:

Turning

- BAR unit

- CPY unit

- CORNER unit

- FACING unit

- THREAD unit

- T. GROOVE unit

- T. DRILL unit

- T. TAP unit

- MILLTURN unit

Other units

- MMS unit

- WORK MES unit

- TOOL MES unit

- TRANSFER unit

Milling

- DRILLING unit

- RGH CBOR unit

- RGH BCB unit

- REAMING unit

- TAPPING unit

- BK-CBORE unit

- CIRC MIL unit

- CBOR-TAP unit

- BORE T1 unit

- BORE S1 unit,

- BORE T2 unit

- BORE S2 unit

- LINE CTR unit

- LINE RGT unit

- LINE LFT unit

- LINE OUT unit

- LINE IN unit

- CHMF RGT unit

- CHMF LFT unit,

- CHMF OUT unit

- CHMF IN unit

- FCE MILL unit

- TOP EMIL unit

- STEP unit

- POCKET unit

- PCKT MT unit

- PCKT VLY unit

- SLOT unit

PROGRAM CREATION 3

See “TPC DATA SETTING” for further details of the data to be set.

3-5

3 PROGRAM CREATION

[4]

3-2 Common Unit

The common unit is the first to be placed in a MAZATROL program, and always takes unit number 0. Data that is set in this unit is referred to as common data, which becomes the base data for the entire program. When creating a MAZATROL program, therefore, you must first set data in this unit.

3-2-1 Setting unit data (common data)

UNo. MAT. OD-MAX ID-MIN LENGTH WORK FACE ATC MODE RPM LOW TURR

0 [1] [2] [3] [4] [5] [6] [7] [8]

[1] MAT The following menu will be displayed when the cursor is placed at this item:

CST IRN DUCT IRN CBN STL ALY STL STNLESS ALUMINUM L.C.STL AL CAST

From the menu, select the materials type of the workpiece to be machined. If the workpiece to be machined is of a materials type other than those listed above, pre-register

that materials type on the CUTTING CONDITION - PERCENTAGE display. See the Operating Manual for details. The data of this item is referred to by the system during automatic setting of cutting conditions.

[2] OD-MAX, [3] ID-MIN, [4] LENGTH Set the maximum outside diameter, minimum inside diameter, and maximum length, respectively,

of the workpiece.

[2] OD-MAX

Program

origin

T4P017

[3] ID-MIN

[4] LENGTH

Round bar materials

Program

origin

[3] ID-MIN

LENGTH

Molded materials

- Set the workpiece length, including the edge protrusion (edge section to be cut), in item [4].

3-6

PROGRAM CREATION 3

[5] WORK FACE Set the length of the workpiece edge protrusion in the Z-axis direction.

Protrusion

Program origin

[4] LENGTH

[5] WORK FACE

T4P019

- The workpiece edge protrusion refers to a section to be cut during a facing unit (FACING

FACE). For units other than facing units, the protrusion is not regarded as part of the workpiece. Therefore, if the workpiece edge is to be cut (that is, if a value other than 0 is set for this item), an facing unit must be selected before selecting a unit involving other machining operations.

Either 0 or a plus value must always be set for this item. [6] ATC MODE Specify how to retract the axes before ATC.

- Enter 0 to move the axes one by one from the machining end point to the ATC position.

- Enter 1 to move the axes all together from the machining end point to the ATC position. [7] RPM If the maximum spindle speed is to be limited, set that maximum value. Data does not need be

set if the spindle speed is permitted to reach the maximum value provided for in the specifications. This data has no relation to the milling axial velocity.

Note: For an X-axial tool-tip position over OD-MAX or under ID-MIN (both specified in the

common unit), constant cutting speed control will opportunely be relieved by the constant spindle speed control for extra-workpiece area and the spindle will rotate at the speed calculated for the position of OD-MAX or ID-MIN.

The spindle speed for this area is downwards limited to the value c al culated for OD-MAX.

OD-MAX ID-MIN

The spindle speed for this area is upwards limited to the value c al culated for ID-MIN.

* Constant surface speed control is cancelled for extra-workpiece

area in order to reduce the machining time.

3-7

3 PROGRAM CREATION

[8] LOW TURR For a machine equipped with upper and lower turrets, enter a safe outside -diameter value for the

lower turret. See Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS”, for further details.

3-3 Materials Shape Unit (MATERIAL)

The shapes of cast materials or forged materials cannot be defined using the common unit alone. To machine such molded materials, the materials shape unit must be selected following the common unit and the shape data of the materials to be machined must be set.

Only the outside-diameter shape and inside-diameter shape of the intended workpiece can be defined using the materials shape unit. This unit of base data, therefore, has no relation to units of machining on the front and back faces, since the tool path for such units are created merely on the basis of the settings in the common unit. This unit need not be set for round-bar materials. Press the [WORKPICE SHAPE] menu key to select the materials sha pe unit.

3-3-1 Setting unit data

UNo. UNIT

∗ MATERIAL [1]

[1] UNIT The following menu will be displayed when the cursor is placed at this item.

OUT IN

- Select [OUT] to define the outside-diameter shape of the workpiece.

- Select [IN] to define the inside-diameter shape of the workpiece. Both OUT and IN can be defined using a maximum of 25 sequences.

You must first select [OUT], however, when defining both the outside-diameter and insidediameter shapes of a workpiece. That is, after selecting the materials shape unit a s both units No. 1 and No. 2, define the outside-diameter shape using unit No. 1 and then define the insidediameter shape using unit No. 2.

3-3-2 Setting sequence data

UNo. UNIT

∗ MATERIAL ∗∗∗

FIG PTN SPT-X SPT-Z FPT-X FPT-Z RADIUS

1 [1] [2] [3] [4] [5] [6]

[1] PTN The following menu will be displayed when the cursor is placed at this item.

LIN TPR SHAPE

Select the type of shape from the above menu.

3-8

END

The data of the displayed menu denote the following shapes:

PROGRAM CREATION 3

LIN : Line parallel to the center line of the workpiece

TPR : Line not parallel to the center line of the workpiece (Taper line)

: Convex arc

:Concave arc

Outer diameter

shape

Inner diameter

shape

TPR

LIN

Material shape

T4P021

[2] SPT-X, [3] SPT-Z, [4] FPT-X, [5] FPT-Z, [6] RADIUS Set the coordinates of the intended start point and end point of the shape you selected for item

[1]. Also set the radius of the desired circle if you have selected

or .

LIN

End

point

[4] FPT-X

[5] FPT-Z

End point

[6] RADIUS

Start point

End point

TPR

Start point

[2] SPT-X

[4] FPT-X

[3] SPT-Z

[5] FPT-Z

End point

[6] RADIUS

Start point

T4P023

- If you have selected [LIN] for item [1] above, it is good enough just to designate only the

coordinates of the end point (FPT-X and -Z). This is because the NC unit will then form

automatically two orthogonal lines between the end point of the immediately preceding shape

(or the program origin for an LIN as the first shape) and that end point.

3-9

3 PROGRAM CREATION

End point

Note 1: The Z-coordinates of any points located to the right of the program origin must be set

Start point (The coordinates do not need to be set. )

End point of imm edi at el y preceding shape

T4P022

with a minus sign.

Plus data Minus data

T4P024

Note 2: If the start point of a shape is present in the same position as that of the end point of

the immediately preceding shape, those coordinates can be automatically set by pressing the [NEXT] menu key.

UNo. UNIT

1 MATERIAL OUT

FIG PTN SPT-X SPT-Z FPT-X FPT-Z RADIUS

1 2

LIN TPR

##20. 30. #

Cursor

Pressing the [NEXT] menu key with the cursor at the position shown above sets the following data automatically:

UNo. UNIT

1 MATERIAL OUT

FIG PTN SPT-X SPT-Z FPT-X FPT-Z RADIUS

1 2

LIN TPR

20.#30.

20. 30. #

These values are set automatically.

You can use this function also for BAR and CPY units.

3-10

PROGRAM CREATION 3

Note 1: Although a maximum of 200 lines of shape sequence data can be set in one materials

shape unit or turning unit, the maximum usable number of shape sequence data lines may be less than 200 when corner R/C is defined for a complex shape. In that case, alarm 723 EXCEEDS NUMBER OF SHAPES will be displayed, even before the maximum usable number of shape sequence data lines is reached.

Note 2: If the maximum usable number of shape sequence data lines is exceeded, alarm 723

EXCEEDS NUMBER OF SHAPES will be displayed during tool path checking, shape

checking, shape drawing, or automatic operation.

3-11

3 PROGRAM CREATION

3-4 Types of the Milling Unit

The milling unit is available in the following three types :

- Point machining unit ...... used for drilling of holes (Section 3-5)

- Line machining unit ........ used for a contour machining (Section 3-6)

- Face machining unit ...... used for machining an area and machining form (Section 3-7)

Each milling unit includes tool sequence and shape sequence.

3-4-1 Planes to be machined and machining methods

Data items for setting the plane to be machined and for setting the machining method exist in all point, linear, and face machining unit data. These data items are displayed as MODE, POS-B, and POS-C.

Specify the desired face and method under the MODE, POS-B, and POS-C columns.

UNo. UNIT MODE POS-B POS-C DIA DEPTH CHMF

DRILLING

[1] MODE

[1] [2] [3]

Select the machining method.

Mode Description

Cylindrical sides can be machined into the desired shape as specified in the Z-C coordinate system.

(C-axial machining)

Edges can be machined into the desired shape as specified in the R-C or X-Y coordinate system. (C-axial machining)

If C-axis function for No. 2 spindle is

Note:

available, the line machining can be executed on the No. 2 spindle as well.

Rear plane can be machined into the desired shape as specified in the R-C or X-Y coordinate system.

(C-axial machining)

Note: The line machining is possible only if

the machine has C-axis function for No. 2 spindle.

3-12

Mode Description

Plane of cylinder can be machined into the desired shape as specified in the Z-Y coordinate system.

(Y-axial machining)

PROGRAM CREATION 3

Edges can be machined into the desired shape as specified in the X-Y or R-C coordinate system. (Y-axial machining)

Rear plane can be machined into the desired shape as specified in the X-Y or R-C coordinate system.

(Y-axial machining)

Holes can be machined on an oblique plane at the desired oblique positioning angle as specified in the B-axial direction. (C-axial machining) This mode cannot be selected for the line or plane machining units.

The tool approaches from the edge side. Holes can be machined on an oblique plane at the desired oblique positioning angle as specified

in the B-axial direction. (C-axial machining) This mode cannot be selected for the line or plane machining units.

The tool approaches from the rear side. Holes can be machined on an oblique plane at the desired oblique positioning angle as specified

in the B-axial direction. (Y-axial machining)

The tool approaches from the edge side.

3-13

3 PROGRAM CREATION

Mode Description

The XC , XY , /C , /Y mode can be selected for a machine model capable of back machining.

Holes can be machined on an oblique plane at the desired oblique positioning angle as specified in the B-axial direction. (Y-axial machining)

The tool approaches from the rear side.

Note: For the line machining unit, the /C or /C

/C or /C

Precautions for milling with the lower turret

1. The machine operates in single-workpiece independent machining mo de.

2. The machine operates only in point-machining mode.

Drilling, inverse faced hole machining, reaming, tapping, and boring (see Note 2 below) are possible (see Note 1 below). Counterbore machining, back boring, circular milling, or counterbore-tapping i s impossible.

3. It is possible to use ZC, XC, or XC

It is not possible to use /C, /C

4. The machine does not operate in line- or face-machining mode.

5. The lower turret cannot be used for the M-MANUAL unit that operates the Y-axis.

6. Simultaneous machining with the milling tools mounted in the upper and lower turrets is

impossible.

Note 1: Machining that requires Y-axis operation results in an alarm (for chamfering cycle 2). Note 2: Boring cycle 1 and 2 cannot be used (an alarm occurs for lower-turret milling spindle

orientation).

mode cannot be selected for a face machining unit.

mode. (See Note 1.)

, ZY, XY, XY , /Y, or /Y mode.

mode cannot be selected. The ZC, XC, XC ,

[2] POS-B When machining an oblique plane, specify angle B of the oblique plane with respect to a

reference angle of 0 degrees of the edge. This data item will become valid when the /C, /Y, /C

having a B-axis. [3] POS-C

Specify the position of the C-axis. This data item will become valid when the ZY, XY, XY

3-14

, /Y mode is selected for a machine model

, /Y, /Y mode is selected.

3-5 Point Machining Units

The point machining unit serves to determine the data concerning the machining method and machining form for the drilling of holes.

The unit includes the tool sequence determining the tool data used and the shape sequence determining the data concerning the machining dimensions on the drawing.

3-5-1 Types of point machining units

As shown below 12 types of point machining units are available:

PROGRAM CREATION 3

1. Drilling 2. Counterbore machining

NM210-00532

5. Tapping 6-(1) Boring of through hole

NM210-00533 NM210-00534 NM210-00535

3. Inversed faced hole machining

6 (2) Boring of non-

through hole

4. Reaming

6 (3) Boring of stepped

through hole

NM210-00536

6-(4) Boring of stepped

non-through hole

NM210-00540 NM210-00541 NM210-00542 NM210-00543

Fig. 3-1 Types of point machining units

NM210-00537

7. Back boring 8. Circular milling 9. Counterbore-tapping

NM210-00538

NM210-00539

3-15

3 PROGRAM CREATION

3-5-2 Procedure for selecting point machining unit

(1) Press the menu selector key (key located at the right of the menu keys) to display the

following menu.

POINT

MACH-ING

LINE

MACH-ING

FACE

MACH-ING

TURNING MANUAL

PROGRAM

END SHAPE

CHECK

>>>

(2) Presse the [POINT MACH-ING] menu key.

! The following unit menu will be displayed.

DRILLING RGH CBOR RGH BCB REAMING TAPPING BORING BK CBOR CIRC MIL CBOR TAP HI SPD.

DRL.USE

(3) Press the appropriate menu key of the desired machining unit.

- When the [BORING] menu key is pressed, the menu of the four following machining subunits is displayed.

BORING BORING BORING BORING

Remark: For the function of the [HI SPD. DRL. USE] menu key, refer to the Subsection 3-5-4,

“Automatic tool development for cemented carbide drills”.

3-16

PROGRAM CREATION 3

3-5-3 Unit data and automatic tool development of the point machining unit

1. Drilling unit (DRILLING)

Select this drilling unit for machining of a hole with a drill.

DRILLING unit Tool sequence

DIA

CHMF

DEPTH

Centering drill

M3P085 D740PA030

The tools in parentheses ( ) are developed or not developed depending on the particular case.

Drill (Drill) (Drill)

(Chamfering cutter)

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

entered in the unit. The machining is executed on the basis of the tool sequence data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool.

Tool Development patterns

Centering drill Development is always executed.

A maximum of three tools are developed depending on the diameter of the hole.

Drill

Chamfering cutter

< DIA ≤ D8: Development of one tool D8 < DIA ≤ D9: Development of two tools D9 < DIA ≤ D10: Development of three tools

Development is not executed in the following cases:

DIA + (CHMF × 2) ≤ D2 – D4 CHMF = 0

The bold codes represent parameter addresses.

Note: In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed.

- DEPTH < CHMF

- DIA = 0

- D10 < DIA

3-17

3 PROGRAM CREATION

2. Counterbore machining unit (RGH CBOR)

This unit is selected for machining a hole with a counterbore (faced hole).

RGH CBOR unit Tool sequence

CB-DIA

CB-DEP

CHAMF

DIA

The tools in parentheses ( ) are developed or not developed depending on the particular case.

DEPTH

Centering drill Drill (Drill) (Drill) End mill (Chamfering

cutter)

M3P087 D740PA031

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

A maximum of three tools are developed depending on the diameter of the hole.

0 < DIA

Drill

End mill Development is always executed.

Development is not executed in the following casses:

Chamfering cutter

≤ D8: Development of one tool D8 < DIA ≤ D9: Development of two tools D9 < DIA ≤ D10: Development of three tools

CHMF = 0 DIA + (DEPTH × 2)

≥ CB-DIA + (CHMF × 2) < D13

The bold codes represent parameter addresses.

Note: In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed.

- CB-DIA < DIA

- DEPTH < CB-DEP

- DEPTH < CHMF

3-18

3. Inversed faced hole machining unit (RGH BCB)

This unit is selected for machining a hole with an inversed faced hole.

RGH BCB unit Tool sequence

DIA

PROGRAM CREATION 3

CHMF

CB-DIA

DEPTH

CB-DEP

M3P089 D740PA032

The tools in parentheses ( ) are developed or not developed depending on the particular case.

Centering drill Drill (Drill) Back facing(Drill) (Chamfering

cutter)

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

A maximum of three tools are developed depending on the diameter of the hole.

0 < DIA

Drill

Development is not executed in the following cases:

Chamfering cutter

Back facing tool Development is always executed.

≤ D8: Development of one tool D8 < DIA ≤ D9: Development of two tools D9 < DIA ≤ D10: Development of three tools

DIA + (CHMF × 2) CHMF = 0

≤ D2 – D4

The bold codes represent parameter addresses.

Note: In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed.

- CB-DIA < DIA

- DEPTH < CB-DEP

- DEPTH < CHMF

3-19

3 PROGRAM CREATION

4. Reaming unit (REAMING)

Select this unit for performing finish machining with reamer. In reaming, the content of the tool sequence to be set is different according to the preceding

process.

A. Case of preceding process = drilling

REAMING unit Tool sequence

DIA

CHMF

DEPTH

Centering drill

M3P091 D740PA033

The tools in parentheses ( ) are developed or not developed depending on the particular case.

Drill

(Drill) (Drill)

(Chamfering cutter)

Reamer

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

entered in the unit. The ma chining is executed on th e basis of the tool sequenc e data and the unit data are not used for the machining. If the data developed are inappropriate for the machining, edit by modifying the data or deleting the tool.

Tool Development patterns

Centering drill Development is always executed.

A maximum of three tools are developed depending on the diameter of the hole.

Drill

Chamfering cutter

Reamer Development is always executed.

0 < DIA –

D8 < DIA – D35 ≤ D9: Development of two tools D9 < DIA – D35 ≤ D10: Development of three tools

Development is not executed in the following cases:

DIA + (CHMF × 2) CHMF = 0

D35 ≤ D8: Development of one tool

≤ D2 – D4

The bold codes represent parameter addresses.

Note: In the following case the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed.

- DEPTH < CHMF

3-20

B. Case of preceding process = boring

REAMING unit Tool sequence

DIA

PROGRAM CREATION 3

CHMF

DEPTH

Centering drill

(Chamfering

cutter)

M3P093 D740PA034

The tools in parentheses ( ) are developed or not developed depending on the particular case.

Drill

Reamer

(Drill) (Drill)

Boring

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

A maximum of three tools are developed depending on the diameter of the hole.

Drill

Boring tool Development is always executed.

Chamfering cutter

Reamer Development is always executed.

0 < DIA –

D8 < DIA – D36 ≤ D9: Development of two tools D9 < DIA – D36 ≤ D10: Development of three tools

Development is not executed in the following cases:

DIA + (CHMF × 2) ≤ D2 – D4 CHMF = 0

D36 ≤ D8: Development of one tool

The bold codes represent the parameter addresses.

Note: In the following case the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed.

- DEPTH < CHMF

3-21

3 PROGRAM CREATION

C. Case of preceding process = end mill

REAMING unit Tool sequence

DIA

CHMF

DEPTH

Centering drill Drill (Drill) (Drill) End mill

End mill

M3P095 D740PA035

The tools in parentheses ( ) are developed or not developed depending on the particular case.

(Chamfering cutter)

Reamer

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

A maximum of three tools are developed depending on the diameter of the hole.

Drill

End mill Development of two tools is executed.

Chamfering cutter

Reamer Development is always executed.

0 < DIA –

D8 < DIA – D37 ≤ D9: Development of two tools D9 < DIA – D37 ≤ D10: Development of three tools

Development is not executed in the following cases:

DIA + (CHMF × 2) CHMF = 0

D37 ≤ D8: Development of one tool

≤ D2 – D4

The bold codes represent the parameter addresses.

Note: In the following case the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed.

- DEPTH < CHMF

3-22

5. Tapping unit (TAPPING)

Select this unit for performing tapping. <Setting the nominal diameter of unified thread>

Example 1: For 3/4-16 unified thread:

Press the [Q (1/4) QUARTER] menu key, and then press the keys

3 – 1 6

and

Example 2: For 1 1/8-7 unified thread:

Press the [E (1/8) EIGHTH] menu key, and then press the keys

in this order.

INPUT

<Setting the nominal diameter of pipe thread> Example 1: For PT 3/8 thread:

Press the [E (1/8) EIGHTH] menu key, and then press the keys in this order.

Example 2: For PF 1 thread:

Press the keys

and

in this order.

INPUT

in this order.

INPUT

PROGRAM CREATION 3

9 – 7

and

INPUT

Note 1: The thread depths of PT screws or PS screws are set automatically according to

MAZAK specifications.

Note 2: For planetary tapping, the data to be set for the MAJOR-φ, PITCH, TAP-DEP, and

CHMF, depends on the selected type of tool. Enter the data specified in the

corresponding tool catalogue. For TAP-DEP, enter the cutting edge length specified in the tool catalogue. Also, set the tool data as follows.

- Enter the catalogued nominal diameter in the tool data item ACT-φ.

- Enter the catalogued thread outside diameter in the tool data item DIAMETER.

- Enter the catalogued cutting edge length in the tool data item LENGTH.

Cutting edge length

Thread outside diameter

3-23

3 PROGRAM CREATION

TAPPING unit Tool sequence

MAJOR-

CHMF

PITCH

TAP-

DEP

Centering d rill Drill (Drill) (Drill) (Chamfering cutter) Tap

M3P097 D740PA036

The tools in parentheses ( ) are developed or not developed depending on the particular case.

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

A maximum of three tools are developed depending on the diameter of the hole.

Drill

Chamfering cutter

Tap Development always takes place.

0 < Diameter of pre-hole dr illing

D8 < Diameter of pre-hole drilling ≤ D9: Development of two tools D9 < Diameter of pre-hole drilling ≤ D10: Development of three tools

Development is not executed in the following cases:

Diameter of hole + (CHMF × 2) ≤ D2 – D4 CHMF = 0

≤ D8: Development of one tool

The bold codes represent the parameter addresses.

Note: In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed.

- TAP-DEP < CHMF

- Case of designation of threading other than the JIS standard threading (however, this can be used for forced insertion).

3-24

PROGRAM CREATION 3

6. Boring unit (BORING)

The boring has the four units as the through hole boring, non-through hole boring, stepped through hole boring and stepped non-through hole boring.

A. Through hole boring unit (BORE T1)

Select this unit for performing through-hole boring.

BORE T1 unit Tool sequence

DIA

CHMF

DEPTH

Centering drill Drill

(Chamfering cutter)

M3P099 D740PA037

The tools in parentheses ( ) are developed or not developed depending on the particular case.

(Boring)

(End mill) Boring (Boring)

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

Drill Development is always executed.

End mill

Boring tool

Chamfering cutter

Development is not executed in the following case:

DIA – 6.0 <

Development of a maximum of three tools is executed depending on the wall roughness.

Wall roughness = 1, 2: Development of one tool Wall roughness = 3, 4: Development of two tools Wall roughness = 5, 6, 7, 8, 9: Development of three tools

Development is not executed in the following case:

CHMF = 0

The bold codes represent the parameter addresses.

Note: In the following cases the alarm 416 AUTO PROCESS IMPOSSIBLE will be displayed.

- Diameter of faced hole < DIA

- DEPTH < Depth of faced hole

- DEPTH < CHMF

3-25

3 PROGRAM CREATION

B. Non-through hole boring unit (BORE S1)

Select this unit for performing boring of non-through holes.

BORE S1 unit Tool sequence

DIA

CHMF

PRE-DIA

DEPTH

Centering drill Drill

(Chamfering cutter)

M3P0101 D740PA037

The tools in parentheses ( ) are developed or not developed depending on the particular case.

(Boring)

(End mill) Boring (Boring)

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

Drill Development is always executed.

Development is not executed if the following three conditions are fulfilled:

End mill

Boring tool

Chamfering cutter

DIA – 6.0 <

10.0 < PRE-DIA DIA – PRE-DIA

The development of a maximum of three tools is executed according to the wall roughness.

Wall roughness = 1, 2: Development of one tool Wall roughness = 3, 4: Development of two tools Wall roughness = 5, 6, 7, 8, 9: Development of three tools

Development does not take place in the following case:

CHMF = 0

≤ 6.0

The bold codes represent the parameter addresses.

Note: The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases:

- DIA < PRE-DIA

- DIA ≤ 6.0

- DEPTH < CHMF

- PRE-DIA = 0 → DEPTH < (A/3.328558 – D12)

- PRE-DIA ≠ 0 → DEPTH < (A – PRE-DIA)/3.328558

A: DIA – 6.0 (in case of DIA – 6.0 < D8) or A:

D8 (in case of D8 ≤ DIA – 6.0)

3-26

C. Stepped through hole boring unit (BORE T2)

Select this unit for performing stepped through hole boring.

BORE T2 unit Tool sequence

CB-DIA

CB-DEP

CHMF

PROGRAM CREATION 3

CHMF

DIA

DEPTH

Centering

drill

Boring (Chamfering

M3P0102 D740PA038

The tools in parentheses ( ) are developed or not developed depending on the particular case.

Drill End mill Boring

(Boring) (Boring)

cutter)

(End mill) (Boring)

(Chamfering

cutter)

(Boring)

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

Drill Development is always executed.

Development of a maximum of two tools is executed depending on the diameter of the hole.

End mill

Boring tool

Chamfering cutter

0 < DIA – 6.0 < D8: Development of one tool

D8 < DIA – 6.0 ≤ 999.999: Development of two tools

The development of a maximum of three tools is executed depending on the wall roughness of the hole and depending on the wall roughness of the large hole, respectively.

Wall roughness of hole = 1, 2: Development of one tool Wall roughness of hole = 3, 4: Development of two tools Wall roughness of hole = 5, 6, 7, 8, 9: Development of three tools Wall roughness of large hole = 1, 2: Development of one tool Wall roughness of large hole = 3, 4: Development of two tools Wall roughness of large hole = 5, 6, 7, 8, 9: Development of three tools

Development is not executed when the following two conditions are fulfilled:

CHMF = 0 CHMF (CB) = 0

The bold codes represent the parameter addresses.

Note: The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases:

- CB-DEP < CHMF (CB)

- CB-DIA < DIA

-(CB-DIA – DIA)/2 < CHMF

- DEPTH – CB

-DEP < CHMF

- DIA ≤ 6.0

3-27

3 PROGRAM CREATION

D. Stepped non-through hole boring unit (BORE S2)

Select this unit for performing stepped non-through boring.

CB-DIA

BORE S2 unit Tool sequence

CB-DEP

HMF

CHMF

DIA

DEPTH

Centering

PRE-DIA

M3P0104 D740PA038

The tools in parentheses ( ) are developed or not developed depending on the particular case.

drill

Boring (Chamfering

Drill End mill Boring

(Boring) (Boring)

cutter)

(End mill) (Boring)

(Chamfering

cutter)

(Boring)

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

Drill Development is always executed.

Development of a maximum of two tools is executed depending on the diameter of the hole.

End mill

Boring tool

Chamfering cutter

0 < DIA – 6.0 < D8, 10.0 < PRE-DIA and (DIA – PRE-DIA) ≤ 6.0: Development of one tool

D8 < DIA – 6.0 ≤ 999.999: Development of two tools

The development of a maximum of three tools is executed depending on the wall roughness of the hole and depending on the wall roughness of the large hole, respectively.

Development is not executed when the following two conditions are fulfilled:

CHMF = 0 CHMF (CB) = 0

The bold codes represent the parameter addresses.

3-28

PROGRAM CREATION 3

Note: The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases:

- CB-DIA < DIA

- DIA ≤ PRE-DIA

- DEPTH < CB-DEP

- CB-DEP < CHMF (CB)

-(CB-DIA – DIA)/2 < CHMF

-(DEPTH – CB-DEP) < CHMF

- DIA ≤ 6.0

- DEPTH < CHMF

-B ≤ 0

B: DIA – 6.0 (in case of DIA – 6.0 < D8) or B:

D8 (in case of D8 ≤ DIA – 6.0)

3-29

3 PROGRAM CREATION

7. Back boring unit (BK-CBORE)

Select this unit for performing back boring.

BK-CBOR unit Tool sequence

PRE-DIA

CHMF

DIA

PRE-DEP

DEPTH

M3P106 D740PA039 The tools in parentheses ( ) are developed or not developed depending on the particular case.

drill

(Back

boring)

Drill (End mill) Boring (Back

(Back

boring)

(Back

boring)

(Back

boring)

(Boring)Centering

(Back

boring)

(Chamfering

cutter)

(Boring)

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

Drill Development is always executed.

End mill

Boring tool

Chamfering cutter

Back boring tool

(Semi-finishing,

finishing)

Development is not executed in the following case:

PRE-DIA – 6.0 <

Development of a maximum of three tools is executed depending on the wall roughness.

Wall roughness of pre-hole = 1, 2: Development of one tool (Roughing) Wall roughness of pre-hole = 3, 4: Development of two tools (Roughing, semi-finishing) Wall roughness of pre-hole = 5, 6, 7, 8, 9: Development of three tools (Roughing, semi-

Development is not executed in the following case:

CHMF = 0

The development of a maximum of five tools is executed according to the value of N (See Note below.)

N = 2: Development of two tools N = 3: Development of three tools N = 4: Development of four tools N = 5: Development of five tools

The development of a maximum of two tools is executed depending on the wall roughness.

Wall roughness of hole = 1, 2: No development Wall roughness of hole = 3, 4: Development of one tool (Semi-finishing) Wall roughness of hole = 5, 6, 7, 8, 9: Development of two tools (Semi-finishing, finishing)

finishing, finishing)

The bold codes represent the parameter addresses.

boring)

(Back

boring)

3-30

PROGRAM CREATION 3

Note: The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases:

- DIA < PRE-DIA

- PRE-DEP < DEPTH

- PRE-DEP < CHMF

- PRE-DEP ≤ DIA/2

-5 < N The value N is determined by the roughness and the number of times of back boring.

(DBBL – DP)

N =

Wall roughness of hole DBBL 1, 2 DIA 3, 4 DIA – 1.0 5, 6, 7, 8, 9 DIA – 1.5

Wall roughness of pre-hole DP 1, 2, 3, 4 PRE-DIA 5, 6, 7, 8, 9 PRE-DIA – 1.5

(Decimal fractions are rounded up.)

3-31

3 PROGRAM CREATION

8. Circular milling unit (CIRC MIL)

Select this unit for performing drilling with the end mill. According to the set value in item TORNA., one of the following two machining patterns is

selected.

TORNA.: 0...................Circular milling cycle

1...................Tornado milling cycle

A. Circular milling cycle

CIRC MIL unit Tool sequence

DIA

CHMF

PRE-DIA

The tools in parentheses ( ) are developed or not developed depending on the particular case.

DEPTH

End mill (Chamfering cutter) (Chamfering cutter)

M3P108 D740PA040

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

End mill Development is always executed.

Development is not executed under the following two conditions:

Chamfering cutter

CHMF = 0 CHMF

re-hole) = 0

Note: The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases:

- DIA < PRE-DIA

- DEPTH < CHMF

-(DIA – PRE-DIA)/2 < CHMF (pre-hole)

3-32

PROGRAM CREATION 3

B. Tornado milling cycle

CIRC MIL unit Tool sequence

PITCH1

CHMF

PITCH2

DEPTH

End mill (Thread mill)

D735P0063 D740PA041

The tools in parentheses ( ) are developed or not developed depending on the particular case.

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

End mill Development is always executed.

Note 1: The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases:

- DIA < PRE-DIA

- DEPTH < CHMF

-(DIA – PRE-DIA)/2 < CHMF (pre-hole)

Note 2: Set such a tool diameter in tool data that satisfies “DIA > tool diameter ≥ (DIA/2)”.

3-33

3 PROGRAM CREATION

9. Counterbore-tapping unit (CBOR-TAP)

Select this unit for machining a tapped hole with a counterbore (faced hole).

CBOR-TAP unit Tool sequence

CB-DIA

CHMF

PITCH

MAJOR-

CB-DEP

TAP-DEP

Centering drill Drill (Drill) (Drill) End mill

(Chamfering

cutter)

M3P110 D740PA042

The tools in parentheses ( ) are developed or not developed depending on the particular case.

(Chamfering

cutter)

Tap

Automatic tool development The tools are automatically developed according to different patterns on the basis of the data

Tool Development patterns

Centering drill Development is always executed.

The development of a maximum of three tools is executed depending on the diameter of the hole.

Drill

Chamfering cutter

Tap Development always takes place.

< Hole diameter ≤ D8: Development of one tool D8 < Hole diameter ≤ D9: Development of two tools D9 < Hole diameter ≤ D10: Development of three tools

Development is not executed in the following cases:

CHMF (faced hole) = 0 CHMF (threaded hole) = 0

The bold codes represent the parameter addresses.

Note: The alarm 416 AUTO PROCESS IMPOSSIBLE is given in the following cases:

- CB-DIA < MAJOR-φ

-(CB-DIA – MAJOR-φ)/2 < CHMF (threaded hole)

- PRE-DEP < CHMF (faced hole)

- TAP-DEP < CHMF (threaded hole)

3-34

3-5-4 Automatic tool development for carbide drills

The Subsection 3-5-3 describes automatic tool development for drilling using high speed steel drills. Automatic tool development for cemented carbide drills is described below. This function allows machining time and programming time to be reduced. Before using this function, thoroughly understand its usage, since mis-use causes tool damage.

After point machining unit selection, the following menu is displayed. Press the [HI SPD DRL. USE] menu key to make the function valid (reverse the display status of the menu item) before selecting a unit. Automatic tool development for cemented carbide drills will occur for the tool sequence:

PROGRAM CREATION 3

DRILLING RGH CBOR RGH BCB REAMING TAPPING BORING BK CBOR CIRC MIL CBOR TAP

HI SPD.

DRL.USE

Automatic tool development for drilling with cemented carbide drills is valid for all poit-machining units and described below using a drilling unit as an example.

UNo. UNIT MODE POS-B POS-C DIA DEPTH CHMF

2 DRILLING

SNo. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M

12DRILL

CHAMFER

DRIL

1) Centering drill data for machining a center hole is not developed automatically.

2) Drilling cycle is developed at RGH in the drilling tool sequence, irrespective of the hole depth.

3) Only one drill data is developed automatically, even for a large hole diameter.

4) When the hole diameter is larger than the value of parameter D2 (nominal diameter of a centering drill), chamfering cutter data is developed automatically. Tool data for chamfering with a centering drill is developed automatically for a hole diameter (DIA) smaller than or equal to the value of parameter D2 (nominal diameter of a centering drill).

UNo. UNIT MODE POS-B POS-C DIA DEPTH CHMF

2 DRILLING

SNo. TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M

12DRILL

CTR-DR

DRIL

90°

$ : The data displayed here are automatically determined by automatic tool development

function.

# : Data are not necessary to be set here.

3-35

3 PROGRAM CREATION

3-5-5 New tapping auto-setting scheme

Any given value for tapping with the tapping unit/counterbore-tapping unit can be specified as an auto-set value by editing the required text file within the hard disk. (New tapping auto-setting scheme)

The items corresponding to the new tapping auto-setting scheme are listed below.

Type of thread to be

tapped

Metric thread — — —

Unified thread — — — Pipe thread (PT) Pipe thread (PF) Pipe thread (PS)

1. Tapping for metric thread /unified thread

MAJOR-

φ PITCH TAP-DEP PRE-DIA PRE-DEP

$$$$$

$: New tapping auto-setting scheme applicable

—: New tapping auto-setting scheme inapplicable

Tapping/Counterbore-tapping unit

—

— —

—

In the case of tapping for metric thread/unified thread, the new tapping auto-setting scheme is valid only when parameter D95 is set as follows:

D95 bit 2 = 0: The text file is invalid and tapping for metric thread is subject to the conventional

auto-setting scheme.

= 1: The text file is valid and tapping for metric thread is subject to auto-setting based

on editing.

D95 bit 1 = 0: The text file is invalid and tapping for unified thread is subject to the conventional

auto-setting scheme.

= 1: The text file is valid and tapping for unified thread is subject to auto-setting based

on editing.

The text file format, the text data items, and the editing procedure are shown below.

A. Text file format

[M] PRE_DIA_1=8000 ;<M1> Diameter of Prehole(1/10000mm) ← Pre-hole diameter PRE_DIA_2=9000 ;<M1.1> Diameter of Prehole(1/10000mm) ← Pre-hole diameter

[UN] PRE_DIA_1=15000;<No.1-64UN> Diameter of Prehole(1/10000mm) ← Pre-hole diameter PRE_DIA_2=18000;<No.2-56UN> Diameter of Prehole(1/10000mm) ← Pre-hole diameter

B. Text data items

- Pre-hole diameter (Setting unit: 1/10000 mm) This item denotes the auto-setting values for NOM-φ and HOLE-φ in the last drill tool sequence whose automatic tool development will be conducted for the tapping unit/counterbore-tapping unit.

3-36

PROGRAM CREATION 3

C. Editing procedure

(1) Click the Start button and select “Programs” from the Start menu option. Then click

“Explorer”.

(2) After copying “TapPrDia.org” (an auto-setting model file for metric thread/unified thread

tapping) within the “C:\nm64tdata” directory into this directory, change the file name to

“TapPrDia.txt”.

(3) Open “TapPrDia.txt” using a commercially available editor. (4) Edit the file seeing the above description of “Text file format” and “Text data items” and

taking notice of each data unit. An example of editing is shown below.

Note 1: If data is not entered correctly, alarm 494 AUTO TAP PROCESS IMPOSSIBLE

will be displayed when auto-setting is executed. Enter data within the following range:

Item Keyword Input unit Minimum value Maximum value

Pre-hole diameter PRE_DIA 1/10000 mm 1000 9999000

Enter integral decimal numbers. For this item always enter “0” as the least two significant digits (that is, the la st two digits).

Note 2: Even within the above data range, the particular combination of data settings in

each item may display an asterisk (∗) to indicate that the amount of chamfering cannot be calculated. In such a case, to ensure that the amount of chamfering will be calculated properly, enter data in each item so that the calculation results in the following calculation expressions range from “0” to “99.9”: [If parameter D44 is set to “0”] (Chamfering) = {(Tap outside diameter) + (Thread pitch) × 2 – (Prehole diameter)}/2 [If parameter D44 is set to “1”] (Chamfering) = {(Tap outside diameter) – (Prehole diameter)}/2

Note 3: Even when data within the above data range is entered, alarm 416 AUTO

PROCESS IMPOSSIBLE may be displayed during automatic development of the

tool data.

Note 4: Entered prehole diameter value has its respective last two digits cut away.

(5) After editing the file, execute “Overwrite & Save”. (6) Close “Explorer”.

D. Example of editing

For “M1 tapping”, proceed as follows to auto-set 0.7 mm as the prehole diameter: (1) Open the text file “TapPrDia.txt”. (2) Move the cursor to the masked item

shown below and then edit data in the

required units. Do not edit other items.

[M] PRE_DIA_1= PRE_DIA_2=9000 ;<M1.1> Diameter of Prehole(1/10000mm)

7000 ;<M1> Diameter of Prehole(1/10000mm)

3-37

3 PROGRAM CREATION

Note 1: Since the default settings of the text file data conform to the conventional scheme,

auto-set data cannot be modified by merely changing the value of bit 1 or bit 2 in the

D95 parameter.

Note 2: When modifying the metric thread/unified thread tapping auto-set data, the user itself

needs to edit and manage the text file.

Note 3: After text file editing, the new data is incorporated into the auto-set data immediately. Note 4: Even for inch specifications, assign data in units of 1/10000 mm to the text file. Note 5: Since auto-set data having an assigned decimal point and exceeding the minimum

allowable number of digits cannot be displayed, text file modifications may not be displayed as auto-settings intact.

Example: Even if the value of PRE_DIA_1 is changed to 8600, a nominal drill

2. Tapping for pipe thread

In the case of tapping for pipe thread, the new tapping auto-setting scheme is valid only when parameter D95 is set as follows:

D95 bit 0 = 0: The text file is invalid and tapping for pipe thread is subject to the conventional

diameter of 0.9 may be displayed as its auto-set value.

auto-setting scheme.

= 1: The text file is valid and tapping for pipe thread is subject to auto-setting based

on editing.

The text file format, the text data items, and the editing procedure are shown below.

A. Text file format

[PT] ;PT 1/8 DIAMETER_1=97280 ;Diameter(1/10000mm) ← Tap outside diameter THREAD_1=280 ;Number of Thread(1/10Thread) ← Total threads DEPTH_1=156000 ;Depth(1/10000mm) ← Thread depth PRE_DIA_1=82000 ;Diameter of Prehole(1/10000mm) ← Pre-hole diameter PRE_DEP_1=184100 ;Depth of Prehole(1/10000mm) ← Pre-hole depth

[PF] ;PF 1/8 DIAMETER_1=97280 ;Diameter(1/10000mm) ← Tap outside diameter THREAD_1=280 ;Number of Thread(1/10Thread) ← Total threads PRE_DIA_1=88600 ;Diameter of Prehole(1/10000mm) ← Pre-hole diameter

[PS] ;PS1/8 DIAMETER_1=97280 ;Diameter(1/10000mm) ← Tap outside diameter THREAD_1=280 ;Number of Thread(1/10Thread) ← Total threads DEPTH_1=155000 ;Depth(1/10000mm) ← Thread depth PRE_DIA_1=85000 ;Diameter of Prehole(1/10000mm) ← Pre-hole diameter PRE_DEP_1=183100 ;Depth of Prehole(1/10000mm) ← Pre-hole depth

3-38

PROGRAM CREATION 3

B. Text data items

- Tap outside diameter (Setting unit: 1/10000 mm)

This item denotes the auto-setting values for MAJOR-φ of the tapping unit/counterbore-tapping unit and HOLE-φ in the tool sequence for the tap. (PT, PF, and PS pipe threads)

- Total threads (Setting unit: 1/10 threads)

This item refers to the total number of threads per inch of a tap, and this value is used for auto-setting PITCH of the tapping unit/counterbore-tapping unit. (PT, PF, and PS pipe threads)

- Thread depth (Setting unit: 1/10000 mm)

This item denotes the auto-setting value for TAP-DEP of the tapping unit/counterbore-tapping unit. (PT and PS pipe threads)

- Pre-hole diameter (Setting unit: 1/10000 mm)

This item denotes the auto-setting values for NOM-φ and HOLE-φ in the last drill tool sequence whose automatic tool development will be conducted for the tapping unit/counterbore-tapping unit. (PT, PF, and PS pipe threads)

- Pre-hole depth (Setting unit: 1/10000 mm)

This item denotes the auto-setting value for HOLE-DEP in the last drilling tool sequence for which automatic tool development will be conducted for the tapping unit/counterbore-tapping unit. (PT and PS pipe threads)

C. Editing procedure

(1) Click the Start button and select “Programs” from the Start menu option. Then click

“Explorer”.

(2) After copying “Pipescdt.org” (an auto-setting model file for pipe thread tapping) within the

“C:\nm64mdata” directory into this directory, change the file name to “Pipescdt.txt”.

(3) Open “Pipescdt.txt” using a commercially available editor. (4) Edit the file seeing the above description of “Text file format” and “Text data items” and

taking notice of each data unit. An example of editing is shown below.

Note 1: If data is not entered correctly, alarm 494 AUTO TAP PROCESS IMPOSSIBLE

will be displayed when auto-setting is executed. Enter data within the following range:

Item Keyword Input unit Minimum value Maximum value Tap outside diameter* DIAMETER 1/10000 mm 10 999990 Total threads THREAD 1/10 threads 26 2147483647 Thread depth* DEPTH 1/10000 mm 10 9999990 Pre-hole diameter* PRE_DIA 1/10000 mm 100 9999000 Pre-hole depth* PRE_DEP 1/10000 mm 100 9999000

Enter integral decimal numbers. * For these items always enter “0” as the least significant digit (that is, the last

digit).

3-39

3 PROGRAM CREATION

Note 2: Even within the above data range, the particular combination of data settings in

Note 3: Even when data within the above data range is entered, alarm 416 AUTO

Note 4: Entered prehole diameter and depth values have their respective last two digits

(5) After editing the file, execute “Overwrite & Save”. (6) Close “Explorer”.

D. Example of editing

PROCESS IMPOSSIBLE may be displayed during automatic development of the tool data.

cut away.

For “PT1/8”, proceed as follows to auto-set 10.117 mm as the tap outside diameter, 27 as the number of threads, 11 mm as the thread depth, 8.43 mm as the prehole diameter, and 17 mm as the prehole depth:

(1) Open the text file “Pipescdt.txt” and move the cursor to “PT1/8”. (2) Move the cursor to each masked item

shown below and then edit data in the

required units. Do not edit other items.

[PT] ;PT 1/8 DIAMETER_1= THREAD_1= DEPTH_1= PRE_DIA_1= PRE_DEP_1=

101170 ;Diameter(1/10000mm)

270 ;Number of Thread(1/10Thread)

110000 ;Depth(1/10000mm)

84300 ;Diameter of Prehole(1/10000mm) 170000 ;Depth of Prehole(1/10000mm)

Note 1: Since the default settings of the text file data conform to the conventional scheme,

auto-set data cannot be modified by merely changing the value of bit 0 in the D95 parameter.

Note 2: When modifying the thread tapping auto-set data, the user itself needs to edit and

manage the text file.

allowable number of digits cannot be displayed, text file modifications may not be displayed as auto-settings intact.

Example: Even if the value of PRE_DIA_1 is changed to 62500, a nominal drill

diameter of 6.3 may be displayed as its auto-set value.

3-40

3-5-6 Tool sequence data of the point machining unit

The tool sequence data are automatically developed by entering the machining unit. However, certain data must be set by means of menu keys or numeric keys on the basis of the

tool used or the machining procedure.

Table 3-1 Tool sequence data

TOOL NOM-φ No. # HOLE-φ HOLE-DEP PRE-DIA PRE-DEP RGH DEPTH C-SP FR M M M CTR DR DRILL CHAMFER END MILL BCK FACE REAMER TAP BOR BAR B-B BAR

Reference

$ $$$$$ $ # # # $ # $ $$$$

$ $$$$$ $ $ $ $ $ $ $ $ $$$

$ $$$$$ $ $ $ $ # $ $ $ $$$

$ $$$$$ $ $ $ $ $ $ $ $ $$$

$$$$$$$ $ # $ ##$$$$$

$ $$$$$ $ $ # # $ $ $ $ $$$

$ $$$$$ $ $ $ $ $ $ $ $ $$$

123456 7 8 9 10 11 12 1314151515

Remark 1: For setting of each data item refer to 1 to 15 below.

PROGRAM CREATION 3

$ : Setting possible. # : Not necessary to be set here.

Remark 2: If [TAPPING CYCLE] menu item is selected for PRE-DIA, there is no need to set

data in PRE-DEP.

1. TOOL

Used to specify the name of the tool to be used for machining. The tool designation can be changed by means of menu keys.

CENTER

DRILL

DRILL CHAMFER

CUTTER

ENDMILL BACKSPOT

FACER

REAMER TAP BORING

BAR

BACK

BOR.BAR

2. NOM-φ (Nominal diameter)

Used to specify the nominal diameter of the tool by means of numeric keys. Note: The alarm 434 NO ASSIGNED TOOL IN TOOL FILE is given if the tool entered has

not been previously recorded in the TOOL FILE display.

3. NOM-φ (Tool identification code)

A code should be selected out of the menu to identify those tools which are of identical type (having an identical name) and have an identical nominal diameter.

ABCDEFGH

HEAVY

TOOL

>>>

In order to designate a heavy tool, first of all press the [HEAVY TOOL] menu key to reverse the menu display and then select the desired menu key in the menu thus displayed.

3-41

3 PROGRAM CREATION

4. NOM-φ (Turret selection)

For the machine with the lower turret, select the turret in which the tool to be used is mounted. The following menu is displayed (if [SET UPPER TURRET] is selected, the column will remain blank, and if [SET LOWER TURRET] is selected, “ TURRET CONTROL FUNCTIONS, for further details:

” will be displayed). See Section 5, LOWER-

SET

UPPER

TURRET

SET

LOWER

TURRET

5. No. (Priority No.)

Assign priority levels in the order of machining. The following menu is displayed. A press of a menu key displays the menu item in reverse mode, allowing a priority number to be assigned.

DELAY

PRIORITY

(a) (b) (c) (d) (e)

PRI.No.

CHANGE

PRI.No.

ASSIGN

PRI.No.

ALL ERAS

SUB PROG PROC END

The function of menu item (a) to (e) is described below:

Menu item Function

(a) Select to conduct subsequent-machining. (b) Select to change the priority number for the tool within the particular process. If the cursor is

present at a blank space, assign a new number in a usual manner. Entry of an existing priority number displays alarm

420 SAME DATA EXISTS will be displayed if the assigned priority number has already been set

on any other unit line.

(d) Selection of this item displays message ALL ERASE (PROC:0, PROG:1)?. Setting 0 will erase

the priority numbers preassigned to the tool to be used repeatedly in the process. Setting 1 will erase the priority numbers preassigned to the tool to be used repeatedly in the program.

(e) Select to terminate the process with the subprogram unit.

420 SAME DATA EXISTS.

For details see Chapter 4, “PRIORITY FUNCTION FOR THE SAME TOOL.”

6. # (Retraction position of the lower turret)

For a machine having upper and lower turrets, it is possible to specify the position to which the lower turret is to be retracted when machining workpieces using only the upper turret. The following menu is displayed. For details see Chapter 5, “LOWER-TURRET CONTROL FUNCTIONS.”

LOWER

TURRET

POS.1

LOWER

TURRET

POS.2

3-42

PROGRAM CREATION 3

7. HOLE-φ (Diameter of machining hole)

Used to specify the diameter of the hole to be machined. The data fo r this article can be modified by means of numeric keys.

Note: For the chamfering cutter, this concerns a value equal to twice the distance from the

centerline of the hole to an interference. Enter 999 if there is no interference.

Charmfering if there is interference Chamfering if there is no interference

Hole-φ = 40

Hole-φ = 999

M3P112

Fig. 3-2 Specification of diameter of machining hole for chamfering cutter

8. HOLE-DEP (Depth of machining hole)

Used to specify the depth of the hole to be machined. The data for this article can be modified by means of numeric keys.

Note 1: For the chamfering cutter, this article is specified as illustrated below.

[1]

[2]

[1] Depth of machining hole = 0 [2] Depth of machining hole = 20

[3]

[3] Depth of machining hole = 0

M3P113

Fig. 3-3 Specification of depth of machining hole

Note 2: For planetary tapping, the appropriate data for the selected type of tool must be set.

Enter the data specified in the corresponding tool catalogue. Enter the catalogued cutting edge length in HOLE-DEP.

Cutting edge length

D735P0072

3-43

3 PROGRAM CREATION

9. PRE-DIA (Diameter of pre-hole)

Used to specify the diameter of the pre-hole for the final hole to be machined. The data for this article can be modified by means of numeric keys. Note 1: In the case of boring, the boring cycle can be selected from the menu. [CYCLE 1] is

selected at the time of automatic tool development.

CYCLE1CYCLE2CYCLE

For details, refer to Subsection 3-5-7 “Tool path of the point machininig unit”, “8. Boring tool”.

Note 2: For back boring, enter the diameter of the through hole. Note 3: In the case of tapping, the tapping cycle can be selected from the menu. [TAPPING

CYCLE] is selected at the time of automatic tool development.

TAPPING

CYCLE

PECKING

CYCLE

PLANET

CYCLE

[TAPPING CYCLE] Conventional tappping cycle [PECKING CYCLE] Pecking cycle using a synchronous tap [PLANET CYCLE] Machining cycle using a planetary tapping tool (only for

machines with the Y-axis)

For details, refer to Subsection 3-5-7 “Tool path of the point machininig unit”, “7. Tap”.

10. PRE-DEP (Depth of the pre-hole)

Used to specify the depth of the pre-hole for the final hole to be machined. The data for this article can be modified by means of numeric keys.

Note 1: Enter the depth of the through hole in the case of back facing or back boring for this

article.

Note 2: Enter the depth of the faced hole in the case of boring for this article. Consequently,

preset data of 0 is displayed for through hole boring and non-through hole boring.

Note 3: Enter the interference depth in the case of chamfering for this article. Note 4: For the end mill, the direction of cutting can be selected from the menu. [CCW CUT] is

selected at the time of automatic tool development.

CW CUT CCW CUT

For the tornado cycle of the circular milling unit, the direction of cutting can be selected from the following menu:

CW CUT CCW CUT

For details, refer to Subsection 3-5-7 “Tool path of the point machininig unit”, “4. End mill”.

Note 5: Data setting is not required for [TAPPING CYCLE]. Set “Cutting depth per peck” for

[PECKING CYCLE]. The value of the D50 parameter “Pre-hole machining feed” is set

for [PLANET CYCLE] automatically.

3-44

11. RGH (Cutting surface roughness)

Enter the cutting surface roughness by means of numeric keys or menu keys.

PROGRAM CREATION 3

▼

▼▼

▼▼▼5▼▼▼6▼▼▼7▼▼▼▼8▼▼▼▼

Note 1: For the centering drill, the angle of tool tip can be selected from the menu.

In automatic tool development mode, 90° is selected.

118

Note 2: For the drill, the drilling cycle can be selected from the menu. In automatic tool

development mode, these data are automatically determined on the basis of the machining depth, the drill diameter and the parameters concerned.

DRILLING

CYCLE

PECKING CYCLE 1

PECKING CYCLE 2

PECKING CYCLE 3

AUTOPECK

CYCLE

DECREME

PECKING CYCLE 1

DECREME

PECKING CYCLE 2

DECREME

PECKING CYCLE 3

For details, refer to Subsection 3-5-7 “Tool path of the point machininig unit”, “2. Drill”.

Note 3: Enter the duration of the dwell time for the tapping (invalid for synchronous tapping).

In automatic tool development mode, FIX is selected. In this case, the dwell time is set by parameter D22.

Note 4: For end mill (Tornado cycle)

During automatic tool development, the system sets the same value as for the BTM item of the circular milling unit. If the BTM item value of the circular milling unit is 0, bottom finishing will not occur. Unless the BTM item value is 0, bottom finishing will occur.

12. DEPTH (Cutting depth)

Used to specify the cutting depth or the amount of chamfering at the time of the machining according to the type of tool:

- Cutting depth on Z-axis per pass in the case of drill.

- Amount of chamfering in the case of chamfering cutter.

- Radial cutting depth or amount of chamfering in the case of circular milling cycle or tornado milling cycle of the end mill, respectively.

- In the case of boring with a reamer, specify the return speed of the reamer (as feed per minute) by means of menu keys or numeric keys. In tool automatic development mode [CUT G01] (cutting feed) is selected.

CUT G01

RAPID

G00

Cutting feed speed is selected by parameter D18.

- Thread pitch in the case of tap.

- Cutting depth in the radial direction in the case of boring bar and back boring tool.

3-45

3 PROGRAM CREATION

13. C-SP (Surface speed)

To auto-set a surface speed (m/min) and feedrate (mm/rev), select the corresponding tool material type from the menu.

The tool material types in the menu are the same as those which have been set on the CUTTING CONDITION - W. MAT./T. MAT. display.

To register new tool material types, refer to Section of “CUTTING CONDITION - W. MAT./T. MAT. Display”, of the relevant Operating Manual.

HSS

AUTO

Data can also be set using the numeric keys.

14. FR (Feedrate)

Used to specify the feedrate of the tool. Same as the surface speed, the entry of data is done by means of menu keys or numeric keys.

15. M (M-code)

Set the required M-code(s) to be output immediately after mounting the tool onto the spindle in the ATC mode. A maximum of up to three M-codes may be entered. It is also possible, moreover, to select and enter a general M-code out of the menu.

CARBIDE

AUTO

3-46

3-5-7 Tool path of the point machining unit

This section shows the path of each tool used during execution of a point machining unit. The initial and reference points in each tool path are as shown below.

- When the selected mode is ZC or ZY

PROGRAM CREATION 3

TC37

Initial point

Reference point

TC37

D734P0006

- When the selected mode is XC or XY

- When the selected mode is

Initial point Reference point

TC40

Reference point Initial point

TC39

D734P0007

TC40

D734P0008

3-47

3 PROGRAM CREATION

- When the selected mode is /C or /Y

TC39

Reference point

- When the selected mode is

Initial point

Reference point

Initial point

D734P0009 D734P0010

TC40

Reference point

TC39

Initial point

D734P0011

3-48

1. Centering drill

The cycle of machining with a centering drill is available in the following three types.

PROGRAM CREATION 3

A Drilling cycle

Rapid feed Cutting feed

Chamfering cycle

B Cycle 1 C Cycle 2

Rapid feed Cutting feed

D735P0130

Remark: Two types of chamfering cycles are provided: “Cycle 1”, which only moves the tool in

the Z-axial direction during machining, and “Cycle 2”, which moves the tool in X- and Y-axial directions in addition to the Z-axial direction. Which of the two cycles is to be used for actual machining is automatically selected during operation.

For details of the tool paths in the two cycles, see Items A to C below.

3-49

3 PROGRAM CREATION

A. Centering drilling cycle

[1] Movement to the inti al poi nt

Clearance

Machining After machining

above center of hole to be machi ned

[2] Movement to the R-point

[3] Machining by cutting f eed

Movement to the point R or to the initial

Case of return to the initial poi nt

Case of return to the R-point

[5]

oint

Rapid feed Cutting feed

Clearance

[4] Delayed stop at bottom of hole

The bold codes represent the parameter addresses.

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz h: Depth of the hole to be calculated by the data HOLE-φ and RGH (angle of tool tip) entered

in the tool sequence and also the data LENG COMP. (tool correction) on the TOOL DATA display

Diameter of machining hole

h =

tan (

Angle of cutting tool tip

+ Tool correction

)

Note: The time of delayed stop of the axial feed at bottom of hole is set by the parameter D3.

M3P114

3-50

B. Cycle 1 of chamfering cycle

Machining After machining

PROGRAM CREATION 3

Clearance

Pi: Initial point

Rapid feed Cutting feed

[1] Movement to the initial point

above center of hole

[2] Movement to the R-point

[3] Chamfering

[4]

Delayed stop at bottom of hole

Case of return to the initial poi nt

Movement to the point R or to the initial point

The bold codes represent the parameter addresses.

Rapid feed

Case of return to the R-point

[5]

Clearance

D735P0131

Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz h: Optimum distance to be automatically calculated by the data PRE-DIA and RGH in the tool

sequence and also the data CHMF in the point machining unit.

Note: The time of delayed stop of the axial feed at bottom of hole is set by the parameter

D16.

3-51

3 PROGRAM CREATION

C. Cycle 2 of chamfering cycle

Machining After machining

Rapid feed Cutting feed

[1] Movement to the initial point

above center of hole to be

machined

[2] Movement to the R-point

[3] Chamfering

[4]

Circular milling

along the hole

Case of return to the initial poi nt

Case of return to the R-point

[5]

Movement to the R-

point or to the initial

oint

The bold codes represent the parameter addresses.

Rapid feed

Clearance

D735P0132

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz

Note: When the following condition is fulfilled, R before machining will be equaled to the

parameter D42. However, R after machining is always equaled to the (safety) clearance.

- Case where the bit 7 of parameter D91 is 1.

h: The optimum distance is automatically calculated by the data PRE-DIA and RGH of the tool

sequence and also the data CHMF in the point machining unit.

Note: For the circular milling, refer to the paragraph dealing with 4. End mill, C. Cycle 3.

3-52

2. Drill

The cycle of machining with drill is available in the following eight types.

PROGRAM CREATION 3

A. DRILLING CYCLE B. Deep-hole drilling cycle

(PECKING CYCLE 2)

D. Very deep-hole drilling cycle (PECKING CYCLE 3) E. Auto-pecking cycle of the cutting load detection type

(AUTOPECK CYCLE) The cutting load torque of the drill is continually monitored

during the auto-pecking cycle of the cutting load detection type. This pecking cycle will be performed only when required, which prevents tool breakage and reduces machining time.

F. Deep-hole drilling cycle for gradual depth reduction

(DECREME. PECKING CYCLE 2) In this machining cycle, the cutting depth is decremented

with respect to a normal deep-hole drilling cycle each time the workpiece is cut.

G. High speed deep-hole drilling cycle for gradual depth

reduction (DECREME. PECKING CYCLE 1) In this machining cycle, the cutting depth is decremented

with respect to a high deep-hole drilling cycle each time the workpiece is cut.

H. Very deep-hole drilling cycle for gradual depth reduction

(DECREME. PECKING CYCLE 3)

In this machining cycle, the cutting depth is decremented with respect to a very deep-hole drilling cycle each time the workpiece is cut.

C. High speed deep-hole driilling cycle

(PECKING CYCLE 1)

Rapide feed Cutting feed

D734P0012

Remark 1: See Items A to H for the tool paths in each cycle. Remark 2: Specify the decremental cutting depth in parameter D45, and the minimum cutting

depth, in parameter D46.

Remark 3: For both “Very deep-hole drilling cycle” and “Very deep-hole drilling cycle for

gradual depth reduction”, three types of machining cycle are available: Very deep-hole drilling cycle, Very deep stop-hole drilling cycle and Very deep through-hole drlling cycle.

3-53

3 PROGRAM CREATION

A. Drilling cycle

[1] Movement to the inti al point above

Machining After machining

center of hole to be machi ned

[2] Movement to the R-point

Case of return to the initial poi nt

Case of return to the R-point

Rapid feed Cutting feed

Clearance

oint

[6]

Clearance

[3] Machining by first

cutting feed f

[4] Machining by second

cutting feed f

[5]

Movement to the R-point or to the initial

The bold codes represent the parameter addresses.

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz

Note: When the following two conditions are fulfilled, R before machining will be equaled

to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance.

- Case where the bit 6 of parameter D91 is 1.

- Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.

M3P116

h: Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also

the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction

hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to

be set for the tool sequence

: Feedrate (FR) to be set for the tool sequence

Feedrate to be modified by the data PRE-DEP (feedrate updating rate)

= f1 × Feedrate updating rate

3-54

B. Deep-hole drilling cycle (PECKING CYCLE 2)

[1]

[2]

Clearance

[4]

[1]Movement to the initial

point above the center of

hole to be machined [2]Movement t o the R-point [3]Machining by first cutting

feed f [4]Movement t o the R-point

[3]

Machining After machining

[7]

[5]

F13

[6]

[5] Movement to the position

determined by

[6]Machining by first cutting

feed f

[7]Movement t o the R-point

F13

[8]

F13

[8]Movement to the position

determined by

[9]Repetition of [5] to [7] to

bottom of hole

]Machining by second

[

cutting feed f

[9]

[

]

F13

The bold codes represent the parameter addresses.

PROGRAM CREATION 3

Rapid feed Cutting feed

Case of return to the initial point

Case of return to the R-

[11]

[11]Movement to the R-point

or to the initial point

oint

R Pz

Clearance

M3P117

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz

Note: When the following two conditions are fulfilled, R before machining will be equaled

to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance.

- Case where the bit 6 of parameter D91 is 1.

- Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.

h: Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also

the data LENG COMP. (tool correction) on the TOOL DATA display

h = Depth of machining hole + Tool correction q: Cutting depth (DEPTH) to be entered in the tool sequence data hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to

be set for the tool sequence f

: Feedrate (FR) to be set for the tool sequence

: Feedrate to be modified by the data PRE-DEP (feedrate updating rate)

= f1 × Feedrate updating rate

3-55

3 PROGRAM CREATION

C. High-speed hole drilling cycle (PECKING CYCLE 1)

[1]

[2]

Clearance

[1] Movement to the initial point

above center of hole [2] Movement to the R-point [3] Machining by f irst cutting

feed f [4] Movement to the point

[3]

Machining After machining

F12

[4]

[5] Machinin g t o the position

determined by q

[6] Movement to the position

F12

[5]

F12

[6]

[7] Repetit i on of [5] and [6]

down to bottom of hole

[8] Machining by second

cutting feed f

Rapid feed Cutting feed

Case of return to the initial point

Case of return to the R-point

[9]

[7]

[8]

[9] Movement to the R-point o

to the initial point

R Pz

Clearance

M3P118

The bold codes represent the parameter addresses.

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz

Note: When the following two conditions are fulfilled, R before machining will be equaled

to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance.

- Case where the bit 6 of parameter D91 is 1.

- Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.

h: Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also

the data LENG COMP. (tool correction) on the TOOL DATA display

be set for the tool sequence f

: Feedrate (FR) to be set for the tool sequence

: Feedrate to be modified by the data PRE-DEP (feedrate updating rate)

= f1 × Feedrate updating rate

Note: The feed speed on the paths [4] and [6] is 9999 mm/min or 999.9 inch/min for

millimeter or inch specification respectively.

3-56

D. Very deep-hole drilling cycle (PECKING CYCLE 3)

[14]

[3]

[12]

Machining After machining

PROGRAM CREATION 3

[1]

Clearance

[1] Move men t to th e init ial

point [2] Movement to the R-point [3] Machining of “a” at feed

rate f

q at feedrate f [4] Movement by D55 to the

retraction position at

feed rate f [5] Movement by q at

feedrate f

[2]

and movement by

D55

[4]

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz

Note: When the following two conditions are fulfilled, R before machining will be equaled

Rapid feed Cutting feed

Case of return to the initial point

Dwell D56

[5]

D55

[6]

[6] Movement by D55 to

the retraction position at feedrate f

[7] Movement by q at

feedrate f

[8] After D53 times

peckings, move ment to the chip ejection position and wait for D56 rotations

[7]

[9]

[8]

D55

[10]

[11]

[13] Dwell D56

[9] Movement by D55 to

the advanced position from the previous machining end position

[

]Movement by q at feed

rate f

[11]Movement by

the retraction position at feedrate f

D55

[12]Repetition of [7]

[

The bold codes represent the parameter addresses.

and [9] down to bottom of hole

]After movement

to bottom of hole, wait for D56 rotations

[14]Movement to the R-

point or to the initial point

to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance.

- Case where the bit 6 of parameter D91 is 1.

Rapid feed

Pi Case of return to the R-point

Clearance

D734P0013'

- Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.

h: Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also

the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction

a: Cutting area (Note 3) q: Cutting depth (DEPTH) to be entered in the tool sequence data

: Feedrate (infeed rate) obtained by multiplying “f2” by the “reduction ratio of the starting

speed of cutting” specified in parameter D54 where, if D54 = 0 or if D54 > 100, then D54 = 100.

D54

= f2 ×

: Feedrate (FR) to be set for the tool sequence

: Pecking retraction speed (= setting of parameter D57)

100

where, if D57 = 0, then D57 = 1000.

3-57

3 PROGRAM CREATION

L: Chip ejection distance calculated from the data ACT-φ (tool diameter: D) and data LENG

COMP. (tool correction) on the TOOL DATA display L = Data LENG COMP.–

Note 1: During the “n”th cutting operation, if (q × n) < D55, retraction through the D55-specified

Note 2: The feedrate on the path [8] is “G0 speed × D52/100”. (If the input value of D52 is 0,

Note 3: Cutting area

R-point

Start point

(D: Tool diameter)

distance does not occur. During machining on the path [3], if the first cutting depth of “q” is greater than or equal to (Clearance at R-point + Cutting area “a” ), machining at feedrate “f

” will occur on the path [3] until (Clearance at R-point + Cutting area “a” ) is

reached, then retraction through the D55-specified distance from that position will occur on the path [4], and the workpiece will be cut to the next cutting position (next cutting depth) on the path [5].

then D52 = 100.)

Machining pattern: Very deep hole drilling cycle a = K + R Where K is LENG COMP. (tool correction) on the TOOL DATA display and R is the clearance.

Machining pattern: Very deep stop-hole or very deep through-hole drilling cycle a = D ×

D58

100 Where D is the tool diameter and D58 (parameter) is the feedrate updating distance rate at the start of cutting. If D58 > 300, D58 is taken to be 100. If a < R, a is taken to be equal to R. Under the conditions shown below, alarm 748 CANNOT MAKE T-PATH (CHK DEPTH) will be issued.

[1] If a > r and a ≥ 2q: [2] If a ≤ r and r ≥ q:

R-point

Start point

End point

R-point

Start point

End point

Fig. 3-4

[3] If a ≥ c and c ≥ q

End point

a: Cutting area

Note: As for a gradual depth reduction cycle, the

q: 1st cutting depth r: Clearance hb: Deceleration distance c: Cutting distance before deceleration

constant cutting depth (before gradual depth reduction) is compared to the values concerned.

D740PA146

3-58

PROGRAM CREATION 3

Note 4: For very deep stop-hole or very deep through-hole drilling cycles, the feedrate or the

surface speed can be changed in some cases within the feedrate updating distance from the hole bottom (hb specified under PRE-DIA of the tool sequence).

Machining pattern: Very deep stop-hole drilling cycle When hb (feedrate updating distance from the hole bottom) is reached, machining by

second cutting feed f The surface speed is kept at the speed (S

starts.

) set as C-SP in the tool sequence. (Fig. 3-5)

Let Q represent the feedrate updating rate (specified under PRE-DEP of the tool sequence). Then second cutting feed f

can be calculated from feed f2 set as FR in the

tool sequence, using the following equation.

= f2 ×

100 If Q = 0, Q is taken to be 100. If Q > 200, alarm 402 ILLEGAL NUMBE R INPUT will be

issued.

Distance to the

hole bottom h

Surfa ce speed: S Feedrate: f

Fig. 3-5

Machining pattern: Very deep through-hole drilling cycle When hb (feedrate updating distance from the hole bottom) is reached, machining by

second surface speed S On the return path (G0/G1) after reaching hb, the tool operates at second surface

speed S returns to first surface speed S

Second surface speed S sequence and the surface speed updating rate (set with the parameter D59), using the following equation.

= S1 ×

If D59 = 0 or D59 > 100, D59 is taken to be 100. Let Q represent the feedrate updating rate (specified under PRE-DEP of the tool

sequence). Then, second cutting feed f sequence, using the following equation.

= f2 ×

. After the tool has finished machining and returned to its initial point, its speed

D59

100

D740PA147

and second cutting feed f4 starts.

is calculated from surface speed (S2) set as C-SP in the tool

can be calculated from feed f2 set for the tool

If Q = 0, Q is taken to be 100. If Q > 200, alarm 402 ILLEGAL NUMBE R INPUT will be issued.

3-59

3 PROGRAM CREATION

Distance to the

hole bottom h

Surface speed: S Feedrate: f

Fig. 3-6

If hb > h (PRE-DEP of the tool sequence), hb is taken to be equal to h. If the cutting area (a) and the feedrate updating distance from the hole bottom (hb)

overlap each other:

1) If a and hp overlap between the R-point and the start point:

R-point

Start point

D740PA148

Between the R-point and the start point, feedrate f and surface speed S point and the end point, however, feedrate f

set as C-SP in the tool sequence is used. Between the start

specified for the feedrate updating

distance (hb) is valid. (Fig. 3-7)

for the cutting area (a) is valid

End point

Fig. 3-7

D740PA149

2) If a and hb overlap between the start point and the end point:

Feedrate f speed S

R-point

Start point

End point

Fig. 3-8

for the feedrate updating distance (hb) is valid and second surface

is used. (Fig. 3-8)

D740PA150

3-60

PROGRAM CREATION 3

Figures below show the relationship between feedrate updating distance from the hole bottom (hb) and each cutting depth (q)/last cutting depth (qn).

[1] If feedrate updating distance (hb) < last cutting depth

(qn):

D55

[3] If (qn + D55) < feedrate override distance (hb):

D55

[2] If last cutting depth (qn) ≤ feedrate updating distance

≤ (qn + D55):

(hb)

D55

D740PA150

Fig. 3-9

Note 5: Hole bottom dwell [13] in the figure of tool path for “D. Very deep-hold drilling cycle

(PECKING CYCLE 3)” is executed when the deceleration distance is zero, but not when it is more than zero (for very deep stop-hole or very deep through-hole drilling cycles or very deep stop-hole or very deep through-hole drilling cycles with a gradual depth reduction).

3-61

3 PROGRAM CREATION

[10]

E. Auto-pecking cycle of the cutting load detection type (Option) (AUTOPECK CYCLE)

The cutting load torque of the drill is continually monitored during the auto-pecking cycle of the cutting load detection type. This pecking cycle will be performed only if the cutting load exceeds its reference value.

Clearance

[3]

[1]

[2]

[4]

Machining After machining

Rapid feed

F13

Cutting feed

[7]

[5]

[8]

[6]

F13

[9]

Case of return to the initial poi nt

[

Case of return to the R-point

]

Rapid feed

Clearance

[1] Movement to the initial point

above center of hole [2] Movement to the R-point [3] Machining by f irst cutting

feed f [4] Movement to the R-point

occurs if the cutting load

exceeds its reference value

Pi: Initial point Pz: Start point to be entered in the shape sequence P

, P2: The positions where autonomous pecking will occur if the cutting load exceeds its

reference value

R: Safety clearance above the point Pz

Note: When the following two conditions are fulfilled, R before machining will be equaled

h: Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also

the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction

hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to

be set for the tool sequence

: Feedrate (FR) to be set for the tool sequence

: Feedrate to be modified by the data PRE-DEP (feedrate updating rate)

= f1 × Feedrate updating rate

Note: Cutting load reference value (pecking threshold value) must be set using the DRILL

MONITOR function of the MACHIN. MONITOR display mode.

[5] Movement to the position

F13

[6] Machining by f irst cutting

feed f

[7] Movement to the R-point

occurs if the cutting load exceeds its reference value

[8] Movement to the position of

F13

[9] Repetit i on of [5] to [7] to

bottom of hole

]Machining by second cutting

[

feed f

The bold codes represent the parameter addresses.

[11] Movement to the R-point

or to the initial point

D735P0073

to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance.

- Case where the bit 6 of parameter D91 is 1.

- Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.

3-62

PROGRAM CREATION 3

F. Deep-hole drilling cycle for gradual depth reduction cycle (DECREME PECKING CYCLE 2)

Machining After machining

Rapid feed Cutting feed

Rapid feed

[1]

[2]

Clearance

[1]Movement to t he i ni tial point

above the center of hole [2]Movement t o the R-point [3]Machining by first cutting

feed f [4]Movement t o the R-point

[3] [4]

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz

Note: When the following two conditions are fulfilled, R before machining will be equaled

Case of return to the in itia l p o in

Case of return to the R-

[5]

F13

[6]

[5]Movement t o t he position

determined by

[6]Machining by first cutting

feed f

[7] Movement to the R-point

F13

[7]

F13

[8] Movement to the position

determined by

[9] Repetition of [5] and [7] to

bottom of hole

[

] Machining by second cutting

feed f

[8]

[9]

[10]

F13

The bold codes represent the parameter addresses.

[11] Movement to the R-point

[11]

or to the initial point

to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance.

oint

R Pz

Clearance

D735P0074

- Case where the bit 6 of parameter D91 is 1.

- Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.

h: Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also

the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction

: Cutting depth to be entered in the tool sequence data (first cutting depth)

: i-th cutting depth

The i-th cutting depth q

is calculated by the value of the D45 parameter for drilling gradual

reduction depth and of the D46 parameter for minimum drilling depth as follows.

3-63

3 PROGRAM CREATION

hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to

be set for the tool sequence

: Feedrate (FR) to be set for the tool sequence

: Feedrate to be modified by the data PRE-DEP (feedrate updating rate)

= f1 × Feedrate updating rate

G. High speed deep-hole drilling cycle for gradual depth reduction (DECREME PECKING

CYCLE 1)

[2]

F12

[3]

[1]

[4]

F12

Clearance

[1]Movement t o the initial point above

the center of hole [2]Movement t o the R-point [3]Machining by first cutting feed f [4]Movement t o t he position

determined by

[5]

F12

1st cut

D: Drilling depth q

: 1st cutting depth

: i-th cutting depth

= q1 –

i-th cut

[6]

× (i – 1) (q

D45

D46

F12

[7] Repetition of [5] and [6] to

bottom of hole

[8] Machining by second cutting

feed f

The bold codes represent the parameter addresses.

)

≥

D46

)

D46

Rapid feed Cutting feed

[7]

[8]

D735P0075

Case of return to the

[9] Movement to the R-point

or to the initial point

Machining After machining

[5] Machining up to the

position determined by q

[6]Movement t o t he position

determined by

Rapid feed

initial point

Case of return to the R-

[9]

oint

Clearance

D735P0076

Pi: Initial point Pz: Start point to be entered in the shape sequence

3-64

PROGRAM CREATION 3

R: Safety clearance above the point Pz

Note: When the following two conditions are fulfilled, R before machining will be equaled

to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance.

- Case where the bit 6 of parameter D91 is 1.

- Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.

h: Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also

the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction

: Cutting depth to be entered in the tool sequence data (first cutting depth)

: i-th cutting depth

The i-th cutting depth q

is calculated by the value of the D45 parameter for drilling gradual

reduction depth and of the D46 parameter for minimum drilling depth as follows.

1st cut

D: Drilling depth

: 1st cutting depth

: ith cutting depth

= q1 –

i-th cut

D46

× (i – 1) (q

D45

(qi <

)

≥

D46

)

D46

D735P0075

hb: Feedrate override distance from the hole bottom to be determined by the data PRE-DIA to

be set for the tool sequence

: Feedrate (FR) to be set for the tool sequence

: Feedrate to be modified by the data PRE-DEP (feedrate updating rate)

= f1 × Feedrate updating rate

Note: The feed speed on the paths [4] and [6] is 9999 mm/min or 99 9.9 inch/min for milimeter

or inch specification respectively.

3-65

3 PROGRAM CREATION

[14]

H. Very deep-hole drilling cycle for gradual depth reduction

[1]

Clearance

[2]

[3]

D55

[4]

[1] Movement to the initial

point [2] Movement to the R-poin [3] Machining of “a” at feed

rate f

and movement by

q at feedrate f [4] Movement by

D55

to the retraction position at feedrate f

[5] Movement by q at

feedrate f

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz

Note: When the following two conditions are fulfilled, R before machining will be equaled

(DECREME PECKING CYCLE 3)

Machining After machining

Rapid feed Cutting feed

Case of return to the initial point

Dwell

[5]

D55

[6]

[6] Movement by

D55

the retraction position at feedrate f

[7] Movement by q at

feedrate f

[8] After

D53

times

peckings, mo v ement to the chip ejection position and wait for

rotations

D56

[7]

[8]

D55

[9] Movement by

D55

the advanced position from the previous machining end position

[

]Movement by q at

feedrate f

[11]Movement by

D55

the retraction position at feedrate f

[

[9]

]

D55

[11]

[

] Dwell

[12]Repetiti on of [7]

[

[12]

D56

and [9] down to bottom of hole

]After movement

to bottom of hole, wait for

rotations

D56

[14]Movement to the R-

point or to the initial point

The bold codes represent the parameter addresses.

to the parameter D1 or D42. However, R after machining is always equaled to the (safety) clearance.

- Case where the bit 6 of parameter D91 is 1.

Rapid feed

Pi Case of return to the R-point

Clearance

D734P0013'

- Case where the respective tool sequence contains a centering drill (D1) or a drill (D42) as pre-machining tool.

h: Hole depth to be calculated by the data HOLE-DEP entered in the tool sequence and also

the data LENG COMP. (tool correction) on the TOOL DATA display h = Depth of machining hole + Tool correction

a: Cutting area

Machining pattern: Very deep hole drilling cycle with a gradual depth reduction a = K + R Where K is LENG COMP. (tool correction) on the TOOL DATA display and R is the clearance.

3-66

PROGRAM CREATION 3

Machining pattern: Very deep stop-hole or very deep through-hole drilling cycle with a gradual depth reduction

D58

a = D ×

100 Where D is the tool diameter and D58 (parameter) is the feedrate updating distance rate at the start of cutting.

If D58 > 300, D58 is taken to be 100. If a < R, a is taken to be equal to R. Alarm 748 CANNOT MAKE T-PATH (CHK DEPTH) will be issued under some conditions.

For details, see Fig. 3-4 in Note 3 of “D. Very deep-hold drilling cycle (PECKING CYCLE 3).”

: Cutting depth (DEPTH) to be entered in the tool sequence data

: i-th cutting depth

The i-th cutting depth q

is calculated by the value of the D45 parameter for drilling gradual

reduction depth and of the D46 parameter for minimum drilling depth as follows. Note: If the setting of parameter D46 is 0 (zero), the minimum allowable cutting depth is

1 mm (or in inch units, 0.04 inches).

1st cut

D: Drilling depth q

: 1st cutting depth

: ith cutting depth

= q1 –

i-th cut

D46

× (i – 1) (q

D45

(qi <

)

≥

D46

)

D46

D735P0075

f1: Feedrate (infeed rate) obtained by multiplying “f2” by the “reduction ratio of the starting

speed of cutting” specified in parameter D54 where, if D54 = 0 or if D54 > 100, then D54 = 100.

D54

= f2 ×

: Feedrate (FR) to be set for the tool sequence

: Pecking retraction speed (= setting of parameter D57)

100

where, if D57 = 0, then D57 = 1000.

L: Chip ejection distance calculated from the data ACT-φ (tool diameter: D) and data LENG

COMP. (tool correction) on the TOOL DATA display

L = Data LENG COMP.–

(D: Tool diameter)

3-67

3 PROGRAM CREATION

Note 1: During the “n”th cutting operation, if (q × n) < D55, retraction through the D55-specified

Note 2: The feedrate on the path [8] is “G0 speed × D52/100”. (If the input value of D52 is 0,

Note 3: For very deep stop-hole and very deep through-hole drilling cycle s with a gradual depth

3. Chamfering cutter

Chamfering is classified into two types: Chamfering performed by the tool which only moves on the Z-axis (Cycle 1) and chamfering performed by the tool which moves on the X-, Y- and Z-axes (Cycle 2).

distance does not occur. During machining on the path [3], if the first cutting depth of “q” is greater than or equal to (Clearance at R-point + Cutting area “a” ), machining at feedrate “f

” will occur on the path [3] until (Clearance at R-point + Cutting area “a” ) is

then D52 = 100.)

reduction, the feedrate or the surface speed can be changed in some cases within the feedrate updating distance from the hole bottom (hb specified under the PRE-DIA in the tool sequence). For details, refer to Note 4 of “D. Very deep-hold drilling cycle (PECKING CYCLE 3).”

The cycle used is selected automatically.

. Cycle 1 B. Cycle 2

Fig. 3-10 Cycle 1 and cycle 2

NM210-00544

Feedrates that are automatically determined vary according to the machining cycle selected. The feedrate in cycle 1 is the feedrate calculated by multiplying the automatically determined feed rate for cycle 2 by the setting of the parameter D60 (%). The feed rate in cycle 1 is displayed yellow.

Parameter D60: Automatic setting ratio of axial cutting feed rate during chamfering in the point

machining

The following shows the tool path of the chamfering cutter in each cycle.

3-68

A. Cycle 1

PROGRAM CREATION 3

Machining After machining

[1]Movement t o t he i ni tial point

above center of hole

[2]Movement t o the R-point

Case of return to the initial poi nt

Case of return to the R-point

Rapid feed Cutting feed

Clearance

[3]Chamfering

[4]

Delayed stop at bottom of hole

Movement to the point

[5]

R or to the initial point

Clearance

The bold codes represent the parameter addresses.

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz h: Optimum distance to be automatically calculated by the data HOLE-φ and HOLE-DEP in

the tool sequence and also the data ANG on the TOOL FILE display

Note: The time of delayed stop of the axial feed at bottom of hole is set by the parameter

D16.

M3P119

3-69

3 PROGRAM CREATION

B. Cycle 2

Machining After machining

[1] Movement to the initial point

above center of hole to be machined

[2] Movement to the R-point

[3] Chamfering

Clearance

Movement to the point R or to the initial point

Case of return to the initial poi nt

Case of return to the R-point

[5]

Rapid feed Cutting feed

Clearance

[4]

Circle milling along the hole

The bold codes represent the parameter addresses.

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz

Note: When the following condition is fulfilled, R before machining will be equaled to the

parameter D42. However, R after machining is always equaled to (safety clearan ce).

- Case where the bit 7 of parameter D91 is 1.

h: The optimum distance is automatically calculated by the data HOLE-φ and HOLE-DEP of

the tool sequence and also the data ANG on the TOOL FILE display.

Note 1: The time of delayed stop of the axial feed at bottom of hole is set by the parameter

D16.

M3P120

Note 2: For the circular milling, refer to the paragraph dealing with 4. End mill, C. Cycle 3.

3-70

PROGRAM CREATION 3

4. End mill

According to the set value in item TORNA., one of the following three machining patterns is selected.

TORNA.: 0 ..................circular milling cycle

1 ..................circular tornado milling cycle

2 ..................precision rapid boring tornado cycle

For tool path of each machining pattern refer to the relevant description below. <In case of circular milling cycle>

End milling is divided into the following three types according to the machining hole diameter, the pre-hole diameter and the nominal diameter entered in the tool sequence.

At the time of operation, the appropriate cycle is automatically selected.

1. For RGH CBOR and CBOR-TAP units

- Diameter of machining hole = Nominal diameter (Cycle 1)

- “Diameter of machining hole > Nominal diameter” and “Diameter of pre-hole > (Tool

diameter + Safety clearance)” (Cycle 2)

- “Diameter of machining hole > Nominal diameter” and “Diameter of pre-hole ≤ (Tool

diameter + Safety clearance)” (Cycle 3)

2. For units other than those mentioned above

- Diameter of machining hole = Tool diameter (Cycle 1)

- “Diameter of machining hole > Tool diameter” and “Diameter of pre-hole > (Tool diameter

+ Safety clearance)” (Cycle 2)

- “Diameter of machining hole > Tool diameter” and “Diameter of pre-hole ≤ (Tool diameter

+ Safety clearance)” (Cycle 3)

Note: The safety clearance is determined by the parameter D23.

A. Cycle 1

B. Cycle 2

C. Cycle 3

Fig. 3-11 Circular milling cycles 1, 2 and 3

The following shows the tool path of the end mill in each cycle.

3-71

NM210-00545

3 PROGRAM CREATION

A. Cycle 1

Clearance

Machining After machining

[1]Movement t o t he i ni tial point

above center of machining hol e

[2]Movement t o the R-point

[3]Machining to bot t om

of hole

Movement to the R-point

or to the initial

Case of return to the initial point

Case of return to the R-point

[5]

oint

Rapid feed Cutting feed

Clearance

[4]Delayed stop at bottom of hole

The bold codes represent the parameter addresses.

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz h: Depth of machining hole (HOLE-DEP) to be entered in the tool sequence

Note: The time of delayed stop of the axial feed at bottom of hole is set by the parameter

D19.

M3P121

3-72

Clearance

B. Cycle 2

PROGRAM CREATION 3

Machining After machining

[1]Movement t o t he i ni tial point

above center of machining hol e

[2]Movement t o the R-point

[3]Movement to the

machining position

Case of return to the initial poi nt

Case of return to the R-point

Rapid feed Cutting feed

Clearance

Circular milling

[4]

(Repetition of circular milling to bottom of the hole)

Circular milling

The bold codes represent the parameter addresses.

[5] Movement to the

point R or to the initial point

M3P122

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz h: Optimum distance to be automatically calculated by the data HOLE-φ and HOLE-DEP in

the tool sequence and also the data ANG on the TOOL FILE display

hf: Bottom finishing allowance to be determined by the data RGH entered in the tool sequence

and also by the parameter D21

q: Cutting depth in the axial direction per pass to be determined by:

h – hf

(Whole part of

h – hf

cmx

) + 1

(cmx = Data DEPTH entered in TOOL FILE display)

Note: For the circular milling, see Cycle 3 below.

3-73

3 PROGRAM CREATION

C. Cycle 3

Clearance

Machining After machining

[1]Movement t o t he i ni tial point

above center of machining hol e

[2]Movement t o the R-point

[3]Movement t o the

machining position

Case of return to the initial poi nt

Case of return to the R-point

Rapid feed Cutting feed

Clearance

[4]

Circular milling (Repetition of circular milling to bottom of the hole)

Circular milling

[5]

Movement to the R-point or to the initial point

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz h: Optimum distance to be automatically calculated by the data HOLE-φ and HOLE-DEP in

the tool sequence and also the data ANG on the TOOL FILE display

hf: Bottom finishing allowance to be determined by the data RGH entered in the tool sequence

and also by the parameter D21

q: Cutting depth in the axial direction per pass to be determined by:

h – hf

( Whole part of

h – hf

cmx

) + 1

(cmx = Data DEPTH entered in TOOL FILE display)

M3P123

Note: The feed speed on the tool paths [3] and [4] is equaled to the parameter E17, if bit 0 of

parameter D92 is set at 1.

3-74

PROGRAM CREATION 3

[2]

[3]

Circular milling Circular milling is automatically selected according to the diameter of the machining hole, the

diameter of the pre-hole and the cutting depth entered in the tool sequence of the program.

Start

Cutting de

Diameter of pre-hole after m ac hining = Diameter of pre-hole + (2 × a mount o cutting depth)

Fig. 3-12 Circular milling

(Hole dia. – Pre-hole dia.)

Yes

Circular milling - A

Circular milling - B

End

M3P124

Note: In the Cycle 3, the pre-hole diameter (data entered in tool sequence) is equal to the tool

diameter (data entered in the TOOL DATA display).

1. Circular milling-A The movement of circular milling-A is as shown below.

Cutting feed

End mill

Cutting depth

[1]

Pre-hole diameter

Fig. 3-13 Circular milling-A

Machining hole diameter

M3P125

- The cutting direction (CW or CCW) can be designated in the program.

Note: The cutting direction designated for the spindle No. 2 is opposite to that for the spindle

No. 1.

- The movement is done in the order [1]→[2]→[3].

- The movement of [1] starts with the end point of the preceding circular milling-A.

3-75

3 PROGRAM CREATION

2. Circular milling-B The movement of circular milling-B is as shown below.

Cutting feed

Fig. 3-14 Circular milling-B

End mill

[4]

[2]

Pre-hole diameter

[1]

[5]

[3]

Cutting depth

Machining hole diameter

M3P126

- The movement is done in the order [1]→[2]→[3]→[4]→[5].

- The cutting direction is set to the left.

- The movement of [1] starts with the end point of the preceding circular milling-A.

Note: However, when bit 4 (bit 5 in the case of chamfering) of parameter D91 is 1, the

movement of [2] and [5] is done by the following shortened (rapid access) method.

Rapid feed Cutting feed

End mill

[3]

Cutting depth

Diameter of machinin

hole

[2]

[6]

[5]

[1][4]

Diameter of pre-hole

Fig. 3-15 Circular milling-B (case of shortening in chamfering)

- Case of shortening (rapid access) in chamfering is shown above

- The cutting direction (CW or CCW) can be designated in the program.

- The movement is done in the order [1]→[2]→[3]→[4]→[5]→[6].

M3P127

3-76

Machining After machining

[1] Movement to the ini tial point

above center of machini ng hol e

PROGRAM CREATION 3

D735P0065

Rapid feed Cutting feed

Clearance

[2] Movement to the R-point

[3]

After movement to the machining position helical milling is performed.

[4]

Helical milling (repetition of herical milling to bottom of the hole)

Helical milling

Pi: Initial point Pz: Start point to be entered in the shape sequence

Case of return to the initial point

Case of return to the R-point

Clearance

[5]

Movement to the R-point or to the initial point

The bold codes represent the parameter addresses.

D735P0066

R: Safety clearance above the point Pz h: Optimum distance to be automatically calculated by the data HOLE-φ and HOLE-DEP in

the tool sequence and also the data ANG on the TOOL FILE display q: PITCH 2 to be entered in the CIRC MIL unit. s: PITCH 1 to be entered in the CIRC MIL unit.

3-77

3 PROGRAM CREATION

Circular milling (1) With bottom finishing

The operation of the machine when it is programmed to perform bottom finishing operations is shown in Fig. 3-16.

Fig. 3-16 Circular helical processing (with bottom finishing)

Rapid feed Cutting feed

D735P0067

After helical interpolation down to the bottom of the hole, one entire circumference of arc interpolation occurs. Next, the tool moves to the center of the hole and then moves in the rapid feed rate to its initial point or to R-point in the axial direction.

(2) Without bottom finishing

The operation of the machine when it is not programmed to perform bottom finishing operations is shown in the Fig. 3-17.

Rapid feed Cutting feed

Returning throug h a quarter pitch in the axial direction

D735P0068

Fig. 3-17 Circular helical processing (without bottom finishing) After helical interpolation down to the bottom of the hole, the tool moves to the center of the

hole by returning through a quarter pitch in the axial direction and then moves in rapid feed rate to its initial point or to R-point in the axial direction.

The bottom of the hole does not undergo arc interpolation.

3-78

The tool path of end mill is as shown below.

Machining After machining

Rapid feed Cutting feed

[1] Movement to the initial poi nt

above center of machining hol e

Clearance

[2] Movement t o t he R-point

[3] After movement to the

machining position heli cal milling is performed

PROGRAM CREATION 3

D735P0077

Rapid feed

Case of return to the initial poi nt

Case of return to the R-point

Clearance

[4]Helical milling

(repetition of helical milling to bottom of the hole)

[5] Circular inter-

polation at botom of the hole

[6] Relief to the cente

of the arc

[7] Movement to

the R-point or to the initial point

D735P0078

Pi: Initial point Pz: Start point to be entered in the shape sequence R: Safety clearance above the point Pz h: HOLE-DEP in the tool sequence q: Pitch 2 to be entered in the CIRC MIL unit.

The cutting depth on Z per pass “q” should not be greater than the data entered at DEPTH in TOOL FILE display.

Note 1: The precision rapid boring tornado cycle (setting 2 at item TORNA.) requires the shape

correction option.

Note 2: The precision rapid boring tornado cycle (setting 2 at item TORNA.) is valid only on the

G17 plane.

3-79

3 PROGRAM CREATION

Circular milling The movement of circular milling is as shown below.

End mill

[1]

[2]

[3]

[4]

Cutting depth

Rapid feed Cutting feed

[1] Posit i oni ng on t he helical inter-

polation path at rapid feedrate

[2] Helical interpolation to bottom of

the hole

[3] One round of circular interpolation

at bottom of the hole

[4] Relief of t he tool on half round of

circular interpolation to the center

Pre-hole diameter

Fig. 3-18 Circular milling

Machining hole diameter

D735P0079

- The movement is done in the order [1]→[2]→[3]→[4].

- The cutting direction (CW or CCW) can be designated in the program.

- The single block function is invalid during the sequence of [2]→[3]→[4].

If the single block function is specified, the program will come to a single-block stop at the ending point of [4]. The feed hold function, however, is valid.

Note: However, when bit 4 of parameter D91 is 1, the movement of [4] is done by the

following shortened (rapid access) method.

Rapid feed Cutting feed

[2][3]

End mill

[5]

[1]

[4]

Cutting depth

Pre-hole diameter

Fig. 3-19 Circular milling (case of shortening in chamfering)

Machining hole diameter

- The cutting direction (CW or CCW) can be designated in the program.

- The movement is done in the order [1]→[2]→[3]→[4]→[5].

3-80

D735P0080

mazak Mazatrol Matrix Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTIONS

Preface

Rule

Basics

Remarks on the cutting conditions recommended by the NC

Programming

Operations

BEFORE USING THE NC UNIT

Limited Warranty

Operating Environment

Keeping the Backup Data

1 MAZATROL PROGRAM CONFIGURATION

1-1 Program Configuration

2 PROGRAM COORDINATE SYSTEM

3 PROGRAM CREATION

3-1 Procedure for Program Creation

3-2 Common Unit

3-2-1 Setting unit data (common data)

3-3 Materials Shape Unit (MATERIAL)

3-3-1 Setting unit data

3-3-2 Setting sequence data

3-4 Types of the Milling Unit

3-4-1 Planes to be machined and machining methods

3-5 Point Machining Units

3-5-1 Types of point machining units

3-5-2 Procedure for selecting point machining unit

3-5-3 Unit data and automatic tool development of the point machining unit

3-5-4 Automatic tool development for carbide drills

3-5-5 New tapping auto-setting scheme

3-5-6 Tool sequence data of the point machining unit

3-5-7 Tool path of the point machining unit