mazak Mazatrol Fusion Programming Manual

Download

PROGRAMMING MANUAL

for

MAZATROL FUSION 640M MAZATROL FUSION 640M 5X MAZATROL FUSION 640M NEXUS

MAZATROL PROGRAMMING

MANUAL No. : H735PG0019E

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/Service Center.

IMPORTANT NOTICE

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.

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

required, please contact the nearest Technical/Service Center. 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.

This manual was considered complete and accu rate at the time of public ation, how ever, 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/Service Center.

Always keep this manual near the machinery for immediate use.

If a new manual is required, please order from the nearest Technical/Service Center with the

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

Issued by Manual Publication Section, Yamazaki Mazak Corporation, Japan

03. 2004

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 m achine 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 cont ains the precautions t o b e obs er ve d as to the working methods and s tates usually expected. Of course, however, unexpec ted operations and/or un expected working states may take place at the user site. During daily operation of the machine, therefore, the user must pay extra careful attention to its own working safety as well as to observe the precautions described below.

2. Although this manual c ontains as great an amount of information as it can, since it is not rare for the user to perfor m the operations that ov erstep the manufactur er-assumed ones, not all of “what the user ca nnot perform” or “what the us er must not perform” c an be fully covered in this manual with all such operations taken into consideration beforehand. It is to be understood, therefore, that functions not clearly written as “executable” are “inexecutable” functions.

SAFETY PRECAUTIONS

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

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

DANGER

: Failure to obs erve t hese instructi ons could r esult in ser ious harm to a hum an

life or body.

WARNING

: Failure to obs erve these instructions could result in m inor injuries or serious

machine damage.

CAUTION

HGENPA0029E

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 th e next operations, full y check that correct data has b een 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 m ake 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 b y operating the machine at no load. Also, full y utilize tool path check , solid check, and other functions, if provided.

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

particular machining requirements. Always understand that since the maximum usable feed rate and rotational spe ed are det er mined by the specificat ions of the to ol to b e us ed , th os e of the workpiece to be m achined, and various ot her factors, actual c apabilities diff er from the machine specif ications listed in this manual. If an inappropriate fee d rate or rotationa l speed is designated, the workpiece or the tool may abruptly move out from the machine.

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

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

Param eters are set to the optim um standard m achining conditi ons prior to sh ipping of the

machine from the fac tor y. In princ iple, these settings s houl d not be m odif ied. If it b ecom es absolutely necessary to modify the settings, perform modifications only after thoroughly understanding the func tions of the correspondin g parameters . Modifications us ually aff ect any program. Unexpected oper ation of the machine will resu lt if the settings are modified without a thorough understanding.

Remarks on the cutting conditions recommended by the NC

! Before using the following cutting conditions:

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

WARNING

Determination Function

- Cutting conditions sugg es ted b y the Machini ng Na vig atio n Fu nctio n

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

Function

Confirm that every necessary precaution in regards to safe machine setup has been taken – especially for workpiec e fixt uring /c lamping 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

! Full y check that the s ettings of the c oordinate s ystem s are c orrect. Even if th e des ignated

program data is correct, errors i n the s ystem s ettings m a y cause the m ac hine to operate in unexpected places a nd the work piece to abruptl y m ove out fr om the m achine in the e vent of contact with the tool.

! During surface velocit y hold control, as the current work piece coordinates of the surf ace

velocity hold contr ol axes appr oach zeroes , the spind le speed inc reases signif icantly. F or the lathe, the work piece m ay even c om e off if the chuc k ing forc e decreas es. 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 register ed until that t ime are not c onverted. Full y check these data units before operating the machine. If the machine is oper ated without checks being performed, even exis ting correct programs may cause the machine to oper ate 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 r everse of their origin al meaning, totall y 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-cyc le m ac hini ng, the too l may collide with the work piece or part of the machine since the m otions of the control axes assum ed 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 subse quent machine actions si gnificantly. Use

the mirror image f unction only after th oroughly unders tanding the abo ve. (This pr ecaution 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 ex pectations of the oper ator. Execute the above com mands only af ter making the correspondin g correction functio n invalid. (This precaution a pplies only to NC units provided with EIA functio ns .)

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

tool information that m atches the tools t o be actual ly used. Other wise, the barr ier function will not work correctly. (This precaution applies only to the M640MT/MT 5X/T/T NEXUS/TN and M640M Pro/MT Pro.)

The system of G-code and M-code commands differs between the machines equipped with

M640M Pro (e-Series such as the INTGEREX e-410, e-650 and e-1060) and the machines equipped with M640MT/MT 5X/T/T NEXUS/TN/MT Pro (such as the INTGEREX non eSeries, the SQT Series, the MPX Series and the QTN Series). 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 Machine with M640M Pro

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

Machine with M640MT/MT 5X/T/

T NEXUS/TN/MT Pro

SAFETY PRECAUTIONS

! For the machines equi pped with M640M Pro (e-Ser ies such as the INTGEREX e- 410, e-

650 and e-1060), 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 ex ample, when the B-axis is rota ted 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 fac t, the resulting movement of the tool to unexpected posit ions may incite collisions. To create the progr am with the plus sid e of the X - ax is or ie nted in an upward directio n, us e the mirror function of the WPC shift unit or the mirror imaging function of G-code command (G50.1, G51.1).

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

check function, the so lid check f unction, an d other f unctions , and conf irm that the program operates properly. T he m odification of tool dat a ma y cause even a f ield-pro ven m achining program to change in operational status. If the user operates the machine without be ing aware of an y changes in program status, interference with the workpiece could arise from unexpected operation. For example, if the cutting edge of the tool during the start of automatic operation is present inside the clearance- i nclu din g blank (unmachined wor kpiece) specified in t he c ommon unit of the MAZATROL program, care is required since the tool will directly move from that position to the approac h point because of no obstructions being judged to be pr esent 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.

S-4

CAUTION

SAFETY PRECAUTIONS

! If axis -by-axis independ ent positionin g is selecte d and simultaneous ly rapid f eed selected

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

If the machine employs sl iding surface structure, lubr ication may prove to be insuff icient

during continuous m icrof eed mac hining ( see Note 1 belo w), an d in the worst cas e, se izure of the sliding surface could result. For these reasons, the sliding surface needs to be maintained in a wel l-lubricated con dition during s uch machining by, for exam ple, inserting an oil-film forming program (see Note 2 below).

List of applicable models and intended axes (Models that employ sliding surface structure)

Classification Machine model Axes with sliding surface structure

Lathes INTEGREX 50Y X-axis, Y-axis, Z-axis

INTEGREX 50YB X-axis, Y-axis, Z-axis INTEGREX 70Y X-axis, Y-axis, Z-axis INTEGREX 70YB X-axis, Y-axis, Z-axis SLANT TURN 450 X-axis, Z-axis SLANT TURN 50N X-axis, Z-axis SLANT TURN 60N X-axis, Z-axis SLANT TURN 80N X-axis, Z-axis TURNING CENTER M-4N X-axis, Z-axis TURNING CENTER M-5N X-axis, Z-axis POWER MASTER X-axis, Z-axis QUICK TURN 40 X-axis, Z-axis MEGA TURN series X-axis, Z-axis SUPER QUADREX 200/250 Z2-axis SUPER QUICK TURN 200/250MY Y-axis SUPER QUICK TURN 300MY Y-axis FJV-35/50/60 Z-axisVertical machining

centers

MTV-515/655/815 Z-axis V-40/60 Z-axis

For further details and m ore specific examples, refer to the relevant Machine Operating Manual, Part 4, Section 1-2, “Precautions for Microfeed Machining (Models th at Employ Sliding Surface Structur e) ”.

Note 1: Cont inuous m ic rofeed machining refers to the oper ation in which t he m ovem ent of the

intended feed axis through strokes shorter than those required for lubrication is continuously repeated.

Note 2: T he oil-film form ing program refers to a program that creates an oil f ilm on the slidin g

surface by moving the intended machining axis over a long stroke during machining.

S-5

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

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

function, or other functions ar e execut ed, t he work piece coor dinat e system s will usua ll y be shifted. When making machine restart after manual intervention, machine locking, the mirror image f unction, or other functions , consider the resu lting 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 f unction to check the machine for norm al operation at no load . Since the

feed rate at this tim e becomes a dry run r ate 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 ar ea. As a result, serious machine damage will result.

Do not design ate an incorrect puls e multiplier when performing m anual pulse handle f eed

operations. If the m ultip lier is se t to 100 t im es and the han dle op erated i nadver tent ly, axia l movement will become faster than that expected.

S-6

OPERATIONAL WARRANTY FOR THE NC UNIT

The warranty of the manufacturer does not co ver a n y troub le ar is i ng if the NC un it 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 b y the use of any commercially available computer equipment

Operating Environment

1. Ambient temperature

During machine operation: 5° to 40°C (41° to 104°F) Note: When power is turne d on, if the therm al s ensor de tects an am bient t em perature und er

5°C, the hard disk warm-up status indic ator lamp will ligh t up and the NC un it will not start operating at once. After autom atic heating of the hard disk by its int ernal heater, the lamp will go out and the NC unit will start. It takes about 20 minutes for temperature to increase from 0 to 5° C in order to avoid condensation due to sudden changes in temperature.

2. Relative humidity

During machine operation: 30 to 75 % (without bedewing) Note: As humidity increases, insulation deteriorates causing electrical component parts to

deteriorate quickly.

S-7

- NOTE -

OPERATIONAL WARRANTY FOR THE NC UNIT

S-8

CONSTRUCTION

Introduction

Part 1 MAZATROL PROGRAMMING PROCEDURES

Chapter 1 MAZATROL PROGRAM Chapter 2 SYSTEM OF COORDINATES Chapter 3 FUNCTION OF KEYS AND SWITCHES Chapter 4 PROCEDURE BEFORE PERFORMING THE MACHINING

Part 2 MAZATROL PROGRAM FUNCTIONS

Chapter 1 CALLING UP AND THE END OF THE PROGRAM DISPLAY Chapter 2 EDITION OF DATA Chapter 3 WINDOW FUNCTIONS Chapter 4 PROGRAM CREATION Chapter 5 PRIORITY FUNCTION FOR THE SAME TOOL Chapter 6 COORDINATES MEASUREMENT FUNCTION

Appendix

Chapter 7 TPC DATA CREATION Chapter 8 BACKGROUND PROGRAMMING Chapter 9 CASE OF APPEARANCE OF ALARM Chapter 10 THREE-DIGIT G-FORMAT

Appendix 1 LIST OF M CODES Appendix 2 PROGRAM EXAMPLES Appendix 3 WHAT TO DO IN SUCH A CASE?

GC-1

- NOTE -

GC-2

Introduction

This manual describes only programming based on the MAZATROL language of the MAZATROL FUSION 640M system. The description given in this manual assumes that the readers have already read the relevant Operating Manual and thoroughly understood its contents.

Programming in the MAZATROL langua ge uses an inter ac ti ve method that allows the system to be operated in accordance with the messages displayed on the CRT monitor. Thus, even a user who is to operate the system for the first time can readily create and edit programs.

Carefully read this manual and the Operating Manual to correctly operate the MAZATROL FUSION 640M system and use its capabilities to their maximum.

H735P0A011E

NOTE:

The MAZATROL FUSIO N 640M controls the m achining center by digital calculat ion, but it is possible that the m achining cannot be perf ormed because of the process ing of a calculation error. Before proceed ing with autom atic operat ion therefore, do not fail to ins pect the path of the tool on the display in order to verify that the machining is being done correctly.

Organization of this manual

The following outlines the organization of this manual:

Part Title

1MAZATROL

PROGRAMMING

PROCEDURES

2MAZATROL

PROGRAM

FUNCTIONS

APPENDIX

Upper row – Directions for using the chapter

Lower row – Contents of the chapter

Those who are going to set up a MAZATROL program for the first time must first read this part. Actually operate the MAZATROL FUSION 640M system from the beginning as directed in Chapter 4, “PROCEDURE BEFORE PERFORMING THE MACHINING.” You will then be able to roughly understand the entire operating procedure from tool registration to creation of a MAZATROL program. Those who already have an experience in creating a program using the MAZATROL M-1, M-2, M-32 or MAZATROL FUSION 640M system will be able to understand the functions and usage of the M640M system just by directly reading Part 2, “MAZATROL PROGRAM FUNCTIONS.”

The program architecture, coordinates systems, and operation keys are discussed here as the basic information required for program creation in MAZATROL language. In addition to the program creation procedures, successive processing procedures up to machining are described in order after the discussion of the basic information.

Use the functions of the MAZATROL FUSION 640M system only after understanding the MAZATROL program architecture and program creation procedures described in Part 1. Also, use this part as a reference whenever required, such as in cases where you have only a slight idea (or have forgotten) how to use a function, as you create a MAZATROL program.

How to call up the details of each function are described here. How to create programs in the background mode, and how to act in the event of alarms are also discussed.

An M-code list, sample programs, and a Q&A (Questions and Answers) list are contained. Read this appendix as appropriate.

PROGRAM

display, how to edit data, how to use a function, and

How to use this manual

Next, how to use this manual is briefly described below.

1. In Part 2, “MAZATROL PROGRAM FUNCTIONS,” where the operating procedures for carrying out the MAZAT RO L la ngu age func t ions are described, the order of s el ect in g menu items is indicated at “Menu selection.” Use the section as quick reference during menu selection.

2. In Part 2, “MAZATROL PROGRAM FUNCTIONS,” where the operating procedures are described, the arrow “!” under the description of each step of the procedure is followed bya description of the results of the particular operation.

Example:

(1) Press the

! The message

menu key.

SEARCH DATA?

will be displayed and the menu will change to the

following address menu:

The section underlined above denotes the results of the operation.

PART 1

MAZATROL PROGRAMMING

PROCEDURES

Part 1 describes the architecture of MAZATROL programs, coordinate systems, the keys to be used for programming, and simplified programming procedures.

H735P10017E

CONTENTS

Page

1 MAZATROL PROGRAM...................................................................... 1-1

2 SYSTEM OF COORDINATES............................................................. 2-1

2-1 Machine Coordinates System............................................................................ 2-1

2-2 Workpiece Coordinates System......................................................................... 2-2

2-3 Machine Coordinates System and Workpiece Coordinates System.................. 2-3

2-4 Basic Coordinates.............................................................................................. 2-3

2-5 Auxiliary Coordinates......................................................................................... 2-4

3 FUNCTION OF KEYS AND SWITCHES..............................................3-1

4 PROCEDURE BEFORE PERFORMING THE MACHINING................4-1

4-1 Diagram of Preparation for the Machining.........................................................4-1

4-2 Part Drawings and Stock Materials.................................................................... 4-3

4-3 Registration of Tools.......................................................................................... 4-5

4-3-1 Calling up the TOOL FILE display .........................................................................4-5

4-3-2 Registration of tools...............................................................................................4-6

4-4 Creation of Simple Programs............................................................................. 4-9

4-4-1 Program structure..................................................................................................4-9

4-4-2 Calling up the PROGRAM display.......................................................................4-10

4-4-3 Assigning workpiece numbers.............................................................................4-11

4-4-4 Creating a program..............................................................................................4-13

4-4-5 Creation of common unit .....................................................................................4-13

4-4-6 Creation of basic coordinates system unit ...........................................................4-15

C-1

4-4-7 Face machining unit ............................................................................................4-17

4-4-8 Line machining unit..............................................................................................4-27

4-4-9 Point machining unit (1).......................................................................................4-37

4-4-10 Point machining unit (2).......................................................................................4-46

4-4-11 End unit...............................................................................................................4-53

4-4-12 End of the program..............................................................................................4-54

4-5 Registration of Tools in a Tool Data File.......................................................... 4-56

4-5-1 Pocket numbers and tool numbers......................................................................4-56

4-5-2 TOOL DATA display............................................................................................4-57

4-5-3 TOOL LAYOUT display .......................................................................................4-59

4-5-4 Registration of tools.............................................................................................4-62

4-6 Check of the Machining Path........................................................................... 4-65

C-2

1 MAZATROL PROGRAM

The machining MAZ ATROL program of a work piece consists in principle of the following four units:

1. Common unit

This concerns a un it which is obligatoril y entered in the pr ogram head . It specifies the comm on data to a program assembly such as the material, the initial point, the machining of several workpieces, etc.

2. Basic coordinates system unit

Use to specify the value of the coordinates (basic coordinates) of the workpiece zero point in the machine coordinates system.

3. Machining unit

Use to specify the data concerning the machining method and the machining form. The machining unit is available in the following three types:

Point machining unit

MAZATROL PROGRAM

-Drilling

- RGH CBOR machining

- RGH BCB machining

- Reaming

- Tapping

-Boring

- Back boring

- Circular milling

- Counterbore-tapping

Line machining un i t

- Central linear machining

- Right-hand linear machining

- Left-hand linear m achining

- Outside linear machining

- Inside linear machining

- Right-hand chamfering

- Left-hand chamfering

- Boring of through hole

- Boring o f stepped through hole

- Boring of non-through hole

- Boring o f stepped n on-through hole

Face machining unit

- Face milling

- End milling-top

- End milling-step

- Pocket milling

- Pocket milling-mountain

- Pocket milling-valley

- End milling-slot

- 3-D (option)

H735P1A010E

- Outside chamfering

- Inside chamfering

Moreover, the necessary data are specified in the following two sequences:

Tool sequence ............... Use to specify the data concerning the name of the tool and the

movement of the tool.

Shape sequence ............ Use to specify the data related to the machining dimensions.

1-1

MAZATROL PROGRAM

4. End unit

Unit created at the end of program. Also, the following units are entered when necessary.

5. Auxiliary coordinates system unit

Use to specify the auxiliary coordinates system (OFFSET).

6. Special mode unit

There are the following special mode units. It is possible that these units marked with an asterisk (*) can not be used or executed in certain machine models.

M code............................ Output of M code

Sub-program................... Calling up a sub-program

Pallet changing*.............. Changing of pallet

Indexing*......................... Use to specify the angle of the indexing table.

Process end.................... Delimits the useful scope of the priority function for the same tool.

7. Manual program mode unit

This unit is entered t o establish a program cor responding to the EIA/I SO program using the G and M codes which permits performing minute movement or a movement other than machining.

8. MMS unit

Automatic measur ement of a basic coordinates s ystem (WPC). MMS unit cann ot be used for certain machines or will not be performed even if programmed.

1-2

2 SYSTEM OF COORDINATES

(

)

–Y–

–

(

)

In the preparation of the pr ogram, a system of c oordinates is used for introduci ng th e pos it ion of the machining and the form of the machining.

The system of coordinat es of the machining cen ter consists of thr ee axes of coordinat es which each cross the reference zero point at right angles.

An arbitrary point found in this system of coordinates can be defined by the value of the coordinates in the 3 axes (X, Y and Z).

There are two types of systems of coordinates:

- Machine coordinates system

- Workpiece coordinates system

Z axis

SYSTEM OF COORDINATES

X axis

Fig. 2-1 Coordinates system

2-1 Machine Coordinates System

The machine actually m oves in its own system of coordinat es called the machine coordinates system. A point of reference in this system of coordinates is known as machine zero point.

Generally, the machine coordin ates system has the machining zone on the side of the minus (negative) direction from the machine zero point.

Note:

The following figure represents the case of vertical machining center.

Machining zone

Machine coordinates system

Axis of X coordinate

+Y +X

Machine zero point

X0, Y0, Z0

Axis of Z coordinate

Reference point zero

Y axis

M3P001

Axis of Y coordinate

Table

NM210-00510

Fig. 2-2 Machine coordinates system

H735P1B010E

2-1

SYSTEM OF COORDINATES

2-2 Workpiece Coordinates System

If the program is prepared on the bas is of the m achine coordinates system, the entering of the machining position and of the form of machining is very complex, tedious and inflexible.

Consequently, a temporary reference point is taken in the machine coodinates system for preparing the program.

The point thus taken is called the workpiece zero point, and the system of coordinates taking this point as reference is called the workpiece coordinates system.

Example:

Plan of the workpiece

M3P002

100

Zero point of the workpiece to be taken

M8 tapped holes

(4 places)

10-mm diameter drilled hole

100

145 150

- When the dim ensions are entered of the configuration on the basis of the ab ove plan of the

workpiece, the bottom left hand corner is taken as the workpiece zero point.

- In this case, the value of the coordinates of the configuration is the following: Workpiece zero point = ( 0, 0, 0)

P1 = (150, 0, 0) P2 = (150, 100, 0) P3 = ( 0, 100, 0)

The adoption of the work piece zero point facilitates the enter ing of the machining dimensions and therefore the programming.

2-2

SYSTEM OF COORDINATES

2-3 Machine Coordinates System and Workpiece Coordinates System

The relationship bet ween the machine coordinates s ystem and workpiece coord inates system when workpiece has been mounted on the table of a machine is shown below.

Machine coordinates system

Workpiece coordinates system

The above relationship may slightly differ according to the type of machine being used.

Note:

Fig. 2-3 Machine coordinates system and workpiece coordinates system

2-4 Basic Coordinates

The machine moves in the machine coordinates system whilst the program is prepared depending on the workpiece coordinates system.

NM210-00511

NM210-00512

Machine coordinates system

Workpiece coordinates system

NM210-00513

It is necessary therefore to enter in the program, the position relation between the machine coordinates system and the workpiece coordinates system.

The unit of entry is called the basic coordinates unit. The basic coordinates are entered as values of the coordinates of the workpiece zero point in the

machine coordinates system. The unit of the basic coord inates is entered by utilizing the coord inates measurement function

after the workpiece is placed on the machine.

2-3

(

)

SYSTEM OF COORDINATES

Basic coordinate Z

Basic coordinate X

−

Fig. 2-4 Basic coordinates

Workpiece zero point

Example of entering of the basic coordinates unit:

Machine zero point

Machine coordinates system

Basic coordinate Y

−

Workpiece coordinates system

NM210-00514

UNo.

Basic coordinates unit

No. of basic coordinates unit

Basic coordinate X

Example: –500

Basic coordinate Y (Exam pl e: –300)

2-5 Auxiliary Coordinates

The auxiliary coordinates are used for offsetting the workpiece zero point to any position in order to further facilitate the preparation of the program.

The auxiliary coordinates unit (OFFSET) is entered as a value of offsetting in the workpiece zero point.

UNIT

WPC-0

ADD. WPC X

-500.Y-300.

Basic coordinate Z (Example: –200)

ngle formed by the axes X and Y of the machine coordinates system and the axes X and Y of the workpiece coordinates system.

-200.

Coordinate or angle of 4th axis, if there is one.

2-4

1. Example of entering of auxiliary coordinates

Workpiece zero point

In this example, the entering of the position of hole P1 requires a very complicated calculation.

30°

SYSTEM OF COORDINATES

M3P003

P1 = (70 + 50 ×

3 2

, 50 ×

)

However, the use of auxiliary coordinates permits performing this entering easily.

Zero point offset in auxil iary coordinates mode

30°

M3P004

As the figure above s hows, positions P1 and P2 ar e entered as follows by off setting the workpiece zero point to R1.

P1 = (50, 0) P2 = (50, 20)

In this case, the auxiliary coordinates unit to be programmed is as follows:

UNo.

Auxiliary coordinates unit

Offsetting on X axis

UNIT

OFFSET

U (X)

70.

V (Y)

Offsetting on Y axis

D (th)

30.

Offsetting on Z axis

Angle with relation to workpiece coordinates system

2-5

W (Z)

SYSTEM OF COORDINATES

2. Cancellation of auxiliary coordinates

The system of auxiliary coordinates is voided in the following cases: A. The system of aux iliary coordi nates specif ied in a sub- program is void ed at the t ime of the

return on the main program. When the main program contains a system of auxiliary coordinates, th e return is made to this system of auxiliary coordinates.

B. The system of auxiliar y coordinates is voided when a new s ystem of basic coordinates is

introduced. In this case, the state without a system of auxiliary coordinates is assumed. (When the system of basic coordinates was specified in the sub-program as shown in Figure 2-5, the retur n to the main program has the effect of voiding the s ystem of auxiliar y coordinates of the main program.)

Main program

WPC-1 Machining [1]

Subprogram

Machining [2]

WPC is a code that signifies the bas i c coordinates system. Machining [2] is performed under the coordinates system of WPC-2.

Fig. 2-5 Basic coordinates system after execution of subprogram

Sub program

WPC-2

M3P005

2-6

3 FUNCTION OF KEYS AND SWITCHES

A MAZATROL program can be c reated usin g onl y the k eys and switches ind icated i n the d otted portion on the operating panel shown in Fig. 3-1 and Fig. 3-2.

FUNCTION OF KEYS AND SWITCHES

H735P1C017E

3-1

FUNCTION OF KEYS AND SWITCHES

D735P0001

Fig. 3-1 Keys and switches used for creating a MAZATROL program <M640M, M640M-5X> ( portion)

3-2

FUNCTION OF KEYS AND SWITCHES

D735P0001’

Fig. 3-2 Keys and switches used for creating a MAZATROL program <M640M NEXUS> ( portion)

3-3

FUNCTION OF KEYS AND SWITCHES

Table 3-1 Functions of keys and switches

No. Name Description

1 Display selector key

2 Menu selector key Press this key to select menu that is displayed on the bottom of the screen.

3 Menu keys

4 Cursor keys

5 Numeric keys

6 Input key Press this key to register keyed-in data in the data display area.

7 Clear key

8 Data cancellation key

9 Page keys

Press this key to select between displays. Depression of this key causes a display selection menu to be displayed in the menu display area.

A specific key is assigned to each of ten menu data that are displayed in the menu display area. Press the appropriate key to carry out the operation speci fied by the particular display or to input the data specified by the particular display.

Press the apropriate key to move the cursor in the desired direction. If a cursor key is pressed and held down, the cursor will move continuously in the corresponding direction.

Use these keys to key in the numerics 0 to 9, the minus sign ( – ), and/or the decimal point ( . ).

Press this key to cancel the data currently being displayed in the data selection area. This key is also used for erasure of the alarm display.

Press this key to cancel the data that has been displayed in the data display area. Depression of this key causes the data in the cursor position to be erased.

Press the appropriate key to move the cursor unit by unit. Pressing and holding down the key will move the cursor unit by unit continuously.

Note: The numbers in the No. column corresponds to those in Fig. 3-1 and 3-2.

3-4

PROCEDURE BEFORE PERFORMING THE MACHI NING

4 PROCEDURE BEFORE PERFORMING THE MACHINING

4-1 Diagram of Preparation for the Machining

To machine a workpiec e, it is essential to co ordinate the pr ogramming and th e preparations for the tool and the workpiece. The f ollowing diagram shows the ge neral procedure to be foll owed before performing the machining.

Note 1:

Note 2:

It is possible to m onitor the path of the tool even if the tool is not recorded in the tool data. (The path of the tool is laid out by taking the diam eter of the tool = the nominal diameter and the length of the tool = 0).

Automatic operation c an not be perform ed if the tool used is not recorded in the t ool data.

H735P1D011E

4-1

PROCEDURE BEFORE PERFORMING THE MACHINI NG

Preparation of part drawings

Reflection of the mounting workpiece

TOOL FILE

Recording of tools available in the workshop

TOOL DATA

Verification of the tools mounted on the tool magazine

display

PROGRAM

Preparation of machining program op

TOOL LAYOUT

Recording of a tool to be mounted on the tool magazine

TOOL PATH CHECK

Verification of path of tool form

Installation of tool

TOOL DATA

Measurement of length of tool

display

SHAPE CHECK

Verification of the programmed form

display

Installation of workpiece

PROGRAM

Measurement of basic coordinates

Automatic operation

Fig. 4-1 Procedure before performing the machining

display

4-2

M3P006

4-2 Part Drawings and Stock Materials

(

)

The following shows the part drawing for which a program is to be created in Section 4-4.

PROCEDURE BEFORE PERFORMING THE MACHI NING

100 95

100

145

Fig. 4-2 Part drawing example

M8 tapped holes (4 places)

10-mm diameter drilled hole

150

Held by a vise, the part to be machined is shown below.

Material: Carbon steel Finish-machinin

surface:

∇, ∇∇

M3P007

NM210-00516

Machining of this part consists of the following four processes:

4-3

PROCEDURE BEFORE PERFORMING THE MACHINI NG

[1] Milling the top face of the workpiece. [2] End-milling the edges of the workpiece.

[3] Drilling a 10-mm diameter through-hole. [4] Drilling four M8 tapped holes.

NM210-00517 NM210-00518

NM210-00519 NM210-00520

4-4

4-3 Registration of Tools

First, turn on the power to return the axes to the zero point. Next, turn the reprogramming switch to the ENABLE position using the key.

Fig. 4-3 Reprogramming switch

PROCEDURE BEFORE PERFORMING THE MACHI NING

Turn

NM210-00521

Before creating the program, information on the tools located in the workshop must be registered in a tool file. Unregistered tools cannot be used for programming or automatic run.

4-3-1 Calling up the TOOL FILE display

Call the

TOOL DATA

. Then press the menu key

display by pressing firs tly the disp lay selector k ey and then t he menu k ey

TOOL FILE

to call the following

TOOL FILE

display.

4-5

D735P0002E

PROCEDURE BEFORE PERFORMING THE MACHINI NG

End mill Face mill Chamfering cutter Ball-end mill

NM210-00522 NM210-00523 NM210-00524 NM210-00525

Tools other than these f our types do not nee d to be registered. T ool selection is automatically made by the NC unit during programming.

4-3-2 Registration of tools

In this chapter, programming is to be carried out by using the two types of tools shown below.

TOOL FILE

display. The tools to be registered here are as follows:

End mill

Tool material:

Cemented carbide

Number of teeth: 2

NM210-00522

Fig. 4-4 Registered tools example

Face mill

Tool material:

Cemented carbide

Number of teeth: 6

NM210-00523

4-6

PROCEDURE BEFORE PERFORMING THE MACHI NING

1. Registering the end mill

Using the page keys, search the display for the tool indicated as E-MILL 10. A. Up to 256 tools can be registered. If the tool is found, this indicates that the tool has been

registered; therefore, proceed to the procedure described in “Registering the face mill.”

(1) Press the cursor key

The message

display area.

(2) Press the input key

The message

(3) Input an approximate tool-diameter value (in this example, input 10 by pressing numeric

keys

The message

(4) Input a specific code th at identifies the p articular tool ( in this example, input A b y pressing

menu key A).

and

NOMINAL DIAMETER?

and then pressing the input key ).

TOOL ID CODE <MENU>?

and position the cursor on an unregistered tool number.

to register the tool.

will be displayed.

will then be displayed in the message

will be displayed.

D735P0003E

D735P0004E

The message

(5) Select the tool material from the tool material menu. Material names registered in the

CUTTING CONDITION

carbide by pressing menu ke y

The message

(6) Input the maximum depth to which the work piece can be cut in the axial directio n by one

cutting operation ( in this example, input 30 by press ing numeric keys then pressing the input key

The message

TOOL MATERIAL <MENU>?

display are disp layed as menu (in this exam ple, select cemented

CARBIDE

MAX DEPTH OF CUT?

NUMBER OF TEETH?

will be displayed.

4-7

will be displayed.

and

PROCEDURE BEFORE PERFORMING THE MACHINI NG

(7) Input the number of teeth of the t ool ( in this ex am ple, input 2 b y pressing n um eric ke y

and then pressing the input key ).

Registration of the 10-mm diameter end mill will be completed as shown below.

2. Registering the face mill

The operations to be carried out are similar to those required for registering the 10-mm diameter end mill. For brevity of description, the displayed message and key(s) to be pressed are noted to the right and left respectively as shown below.

(1) Press the menu key

Check if the tool indica ted as 80. A is inc luded in the the tool is found, then t his indicates th at the t ool has been reg istered. Thus , the oper ations shown below are not required.

(2) Position the cursor on an unregistered tool number.

(3)

NOMINAL DIAMETER?

(4)

TOOL ID CODE <MENU>

(5)

TOOL MATERIAL <MENU>

(6)

MAX DEPTH OF CUT?

(7)

FACE MILL

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

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

TOOL FILE (FACE MILL)

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

?............................................................

? ........................................................

8 0

CARBIDE

D735P0005E

display. If

4-8

PROCEDURE BEFORE PERFORMING THE MACHI NING

NUMBER OF TEETH?

(8)

This completes registration of the 80-mm diameter face mill as shown below.

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

4-4 Creation of Simple Programs

4-4-1 Program structure

The structure of MAZATROL program is described before creating a program. Each MAZATROL program consists of units. Conversely, a combination of program units forms a program. The name of each part of a program is described below using part of the program to be created.

D735P0006E

4-9

PROCEDURE BEFORE PERFORMING THE MACHINI NG

[1]

[2]

[3]

[4]

D735P0007E

[1] Common unit

Basic data rel a ted to the en tire prog ra m, su c h as the ma teria l of th e workpiece, is to be input to this unit.

[2] Basic coordinates system unit

The coordi nat e values of the workpi ece zero poin t in the mach ine coo rdin ates s ystem are to be input to this unit.

[3] Machining units

Various types of machining units are provided. Data related to selection of a machining method an d to machining di m e ns ions are to be input to these units.

Tool sequence ................consists of data inputs related to the operation of a tool.

Shape sequence............. consists of data inputs related to the machining shape on

a drawing.

[4] End unit

Denotes the end of a program (i.e., the completion of machining).

Fig. 4-5 Program structure

4-4-2 Calling up the PROGRAM display

First, the

FILE

display:

PROGRAM

display is to be presented as previously done when displaying the

TOOL

(1) Press the display selector key. (2) Press the menu key

The

PROGRAM

display will be presented then as shown belo w.

4-10

PROCEDURE BEFORE PERFORMING THE MACHI NING

Note:

The above display status is referred to as the listing mode. The listing mode is a program-contents check mode. For details, see Part 2, Section 1-1, “Listing Mode and Creating Mode.”

4-4-3 Assigning workpiece numbers

Number the individual pro grams to be created. T hese numbers identif y the individua l programs just as part number in a part drawing identif ies the indi vidual parts . These num bers are r eferred to as workpiece num bers , and the desired number f r om 1 to 9999 999 9 c an be se lec ted for each program. Here, workpiece No. 1234 is to be set.

(1) Press the menu key

WORK No.

(2)

The message

If either one of the t wo displays [1] and [2] sho wn below is displayed inste ad of this message, then this indicat es that workpiece No. 1 234 has already been used. In that case, input a different workpiece number.

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

WORK No.

NEW PROGRAM <MENU>?

1 2 3 4

will be displayed.

D735P0008E

4-11

PROCEDURE BEFORE PERFORMING THE MACHINI NG

[1] MAZATROL program

[2] EIA/ISO program

D735P0009E

4-12

D735P0010E

PROCEDURE BEFORE PERFORMING THE MACHI NING

Note:

In M640M, two different programs can be created. The program [1] above is referred to as a MAZATROL program, and the one [2], as an EIA/ISO program.

4-4-4 Creating a program

Let us create a program.

(1) After setting the workpiece number, press the menu key

The display shown in Figure 4-6 will be presented. T he program creation will become

possible. This status is referred to as the creating mode. If the EIA/ISO prog ramming function (optio n) is provided in the s ystem, the following menu will be displayed.

WORK No. EIA/ISO

PROGRAM

(2) The following display will be presented. The program creation will become possible.

MAZATROL

PROGRAM

MAZATROL PROGRAM

Fig. 4-6 PROGRAM display (edit mode)

4-4-5 Creation of common unit

The common unit is the program unit that must be created a t the head position of a pr ogram. Basic data on the entire program is to be input to this unit.

The help window is described here before the creation of comm on unit. Prior t o input of data to the unit, full details of the data to inp ut c an be dis p layed on the screen for ease of pr ogramming. This display is referred to as the help window display. Carry out the following operation to display the help window display:

D735P0011E

4-13

PROCEDURE BEFORE PERFORMING THE MACHINI NG

(1) Press the menu key

HELP

The following help window display will be presented.

D735P0012E

Now, start creating the common unit. The data for the article MAT, INITIAL-Z and ATC MODE will be specified here.

MAT Specify the material of the workpiece. INITIAL-Z Specify the initial he ight of the t oo l where it c om es close to th e work piece

for machining purposes (see figure below).

From this level up, the t ool is kept clear of the workpiec e or jigs.

Initial point

Workpiece

oint

zero

M3P018

Fig. 4-7 Tool path

4-14

PROCEDURE BEFORE PERFORMING THE MACHI NING

ATC MODE Specify the manner in whic h the too l is to be returned to the ATC pos iti on

for tool change.

MULTI MODE Use this function when m ore than one work piece of the sam e type are to

be arranged on the table for successive machining. Do not use this function here.

MATEIRAL <MENU>?

(2)

INITIAL POINT Z (CLEARANCE)?

(3)

ZERO RETURN <Z. X+Y: 0, X+Y+Z: 1>?

(4)

MULTI MODE <MENU>?

(5)

The common unit will be created as shown below. When the unit is created, the help windo w will be closed and the program wil l a wait dat a i nput to

the next unit.

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

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

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

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

S45C

2 0 1

MULTI OFF

4-4-6 Creation of basic coordinates system unit

Let us set the basic coordinates (the coordinate values of the workpiece zero point in the machine coordinate s ystem). This data is to be input using the coor dinates measuring func iton (refer to Part 2) af ter workpiec e has been m ounted on th e machine. Her e, inpu t the data o n the assumption that workpiece has been mounted in the position shown below.

4-15

D735P0013E

)

–

PROCEDURE BEFORE PERFORMING THE MACHINI NG

Machine zero point

–200 (Basic coordinate y)

–X

(Basic coordinate z

Fig. 4-8 Workpiece mounting position

(1) While the message (2) Press the menu key

The following help window will be presented. “WPC” is the abbreviation of the

workpiece coordinates.

–Z

–300

100

(Basic coordinate x

Workpiece zero point

MACHINING UNIT <MENU>?

HELP

–Y

NM210-00526

is displayed, press the menu key

WPC

D735P0014E

WPC NUMBER?

(3)

WORKPIECE COORDINATE, WPC-X?

(4)

WORKPIECE COORDINATE, WPC-Y?

(5)

WORKPIECE COORDINATE, WPC-th?

(6)

................................................................... 1

.............................. 3

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

............................. 0

0 0

2 0 0

4-16

PROCEDURE BEFORE PERFORMING THE MACHI NING

WORKPIECE COORDINATE, WPC-Z?

(7)

WORKPIECE COORDINATE, WPC-4?

(8)

The basic coordinates system unit will be created as shown below. When the unit is created, the help windo w will be closed and the program wil l a wait dat a i nput to

the next unit.

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

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

1 0 0

4-4-7 Face machining unit

Let us program a unit that mills the top face of a particular material. This machining unit is referred to as a face milling unit.

D735P0015E

NM210-00517

4-17

PROCEDURE BEFORE PERFORMING THE MACHINI NG

1. Creation of face machining unit

(1) W hile the m ess age

MACH-ING . MACHINING UNIT <MENU>?

(2) (3) Press the menu key

The following help window is presented.

MACHINING UNIT <MENU>?

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

HELP

is displayed, pr ess the m enu key

FACE MIL

FACE

D735P0016E

Now, start creating the fac e machining unit. T he data for the article DEPT H, SRV-Z, BT M, and FIN-Z will be specified here.

DEPTH ..........Input the distance from the workpiece zero point of the Z axis to the surface to

be finished. Here, the depth is 0 because the workpiece zero point is on the finishing surface.

4-18

PROCEDURE BEFORE PERFORMING THE MACHI NING

Workpiece zero point

+XPosition of

WPC-Z = 0

Fig. 4-9 DEPTH and SRV-Z

Chamfering area

Allowance Z (SRV-Z)

Surface to be finished

M3P023

SRV-Z .............Input the chamfer ing thick ness of the work piece. An appr oxim ate value ma y

be input because the workpiece surface is not plane.

BTM.................Input an appropriate finishing code that designates the roughness of the

workpiece surface to be finished.

FIN-Z ...............Input the finish milling thickness. This data will be automatically set if the

roughness of the bottom is specified using a finishing code of the menu.

DIST: WPC Z0 TO FIN. SURFACE?

(4)

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

Z AXIS STOCK REMOVAL?

(5)

BOTTOM FACE ROUGHNESS <MENU>?

(6)

FINISH ALLOWANCE Z?

(7)

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

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

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

(When the bottom roughness is input, the FIN-Z value will be set automatically. Thus , the operator can proceed directly to the next data item using the appropriate cursor key.)

A machining unit such as that s ho wn belo w is n o w com p leted . Us ua lly, a tool appropriate f or the particular tool sequenc e is autom atic ally s elected on t he basis of the data of the m achini ng uni t. Here, a face mill has been selected.

4-19

PROCEDURE BEFORE PERFORMING THE MACHINI NG

2. Creation of tool sequence

(1) W hile the mes sage

(2) Pr ess the menu ke y

that the previously registered tool is included in the display.

The following

mill is registered.

TOOL FILE (FACEMILL)

WHICH TYPE OF TOOL <MENU>?

TOOL FILE

to call the

TOOL FILE

display shows that the 80 mm diameter face

D735P0017E

is displayed, press the curs or key

display on the screen, a nd check

4-20

PROCEDURE BEFORE PERFORMING THE MACHI NING

(3) Press the menu key

programming.

NOMINAL DIAMETER?

(4)

TOOL FILE CODE

(5)

MACHINING PRIORITY No.?

(6)

(Skip to the next item s inc e the id ent ic al-tool priority function is n o t use d h er e. R efer to Part 2, Chapter 5.)

APPROACH POINT X, AUTO

(7)

APPROACH POINT Y, AUTO

(8)

CUTTING DIRECTION <MENU>?

(9)

The possible directions of cutting are shown below.

PROGRAM

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

?........................................................................

to return to the

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

<MENU>?

→→→→

<MENU>?

→→→→

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

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

PROGRAM

AUTO SET AUTO SET X BI-DIR

display and continue

8 0

D735P0018E

4-21

PROCEDURE BEFORE PERFORMING THE MACHINI NG

Cutting feed Rapid feed

<BI-DIR>

<BI-DIR SHORT>

DEPTH OF CUT?

(10)

WIDTH OF CUT?

(11)

CUTTING SPEED, AUTO

(12)

FEEDRATE, AUTO

(13) (14) (15)

M CODE?

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

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

<BI-DIRARCSHORT>

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

<MENU>?

→→→→

<MENU>?

→→→→

<UNI-DIR>

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

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

M3P026

AUTO SET

AUTO SET AUTO SET AUTO SET

A tool sequence such as that s hown below is now completed. F or most of the data items, the optimal data is set b y depressing the m enu key

AUTO S ET

. The data of the artic le APRCH-X, APRCH-Y, however, m aintains ? since the necessary dat a is autom atically set u pon com pletion of the tool path check.

4-22

D735P0019E

PROCEDURE BEFORE PERFORMING THE MACHI NING

3. Cutting parameters

The cutting parameters that have been automatically set in procedural step (12) and (13) of creation of tool sequence above are described here.

The speed at wh ich a too l revolves (circ umfer ential speed) a nd the rat e at which the tool is fed (feed rate) are referred to as cutting parameters.

Circumferential speed (C-SP): Speed (m/min) at whic h a tool m oves on th e outer circ umf erence. T he relations hip betwee n the

revolutions per minute and circumferential speed is given by the following equation.

Circumferential speed (m/min)

Feedrate (FR): The distance (mm /rev) through which workpiece is cut during one revolution of the tool. This

feedrate is called synchronous feedrate.

4. Creation of shape sequence

Tool diameter (mm) × Revolutions per minute (rpm) × 3.14

1000

Circumferential speed

Feedrate

NM210-00527

Next, let us program a shape sequence. Read the machining area from the drawing, and input the coordinate values necessary for the

machining shape. For face milling, the top face of workpiece is to be machined. Thus, input the dimensions of a shape such as that shown below.

4-23

)

PROCEDURE BEFORE PERFORMING THE MACHINI NG

100 (Y coordinate of

onal point

dia

Start point

150 (X coordinate of diagonal point)

Diagonal point

Corner 2 Corner 3

Corner 1 Corner 4

M3P028

Note:

(1) (2) (3)

(4) (5)

(6) (7)

The X- and Y-coordinates of the start point are those of the workpiece zero point.

PATTERN OF FIGURE <MENU>? CORNER 1 COORDINATE X? CORNER 1 COORDINATE Y?

CORNER 3 COORDINATE X? CORNER 3 COORDINATE Y?

CORNER 1 CHAMFER?

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

PATTERN OF FIGURE <MENU>?

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

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

............................................ 0

............................................ 1

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

A shape sequence such as that shown below is now completed.

SQUARE

5 0 0 0

SHAPE END

D735P0020E

4-24

5. Shape check

PROCEDURE BEFORE PERFORMING THE MACHI NING

Check the Of the varioius functions available with the

display of shapes, for erasure of shapes, and for step display of shapes are described here. See Section 6-3, “SHAPE CHECK Display” of the Operating Manual for details of other functions.

(1) Press the menu key

SHAPE CHECK

The following

display to ensure that no errors are included in the inp ut data.

SHAPE CHECK

display will be displa yed.

display, onl y those for continuous

(2) Press the menu key

Shapes will be displayed continuously. The shapes displayed on the screen will be

those of the portions which are chamfered by machining.

SHAPE CONTINUE

4-25

D735P0021E

to display shapes continuously.

PROCEDURE BEFORE PERFORMING THE MACHINI NG

(3) Press the menu key (4) Repe ated ly press the menu key

the screen.

The reverse display state of the menu will be cleared when the final group of shapes is

displayed.

SHAPE ERASE

to erase the shape.

SHAPE STEP

D735P0022E

several times to call shapes step by step on

4-26

PROCEDURE BEFORE PERFORMING THE MACHI NING

(5) Press the menu key

This completes a face milling unit for use in face machining.

4-4-8 Line machining unit

Let us create a unit that steps the edges of a material by contour machining. This machining unit is referred to as an outside linear machining.

PROGRAM

to resume the

PROGRAM

D735P0023E

display.

1. Creation of line machining unit

(1) W hile the mess age

MACH-ING

MACHINING UNIT <MENU>?

4-27

NM210-00518

is displayed, pr ess the menu key

LINE

PROCEDURE BEFORE PERFORMING THE MACHINI NG

MACHINING UNIT <MENU>?

(2) (3) Press the menu key

The help window will be presented.

HELP

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

LINE OUT

D735P0024E

Now, start creating the l ine m achining un it. T he data for the artic le D EPT H, SRV-Z, SR V-R and RGH will be specified here.

DEPTH............... Input a depth value of 10.

SRV-Z ................Input the wall thickness of the workpiece through which it is to be

chamfered in the Z ax ial direct ion f rom the f ace m ille d surf ace (s ee f igure below).

SRV-R................ Input the wall thickness of the workpiece through which it is to be

chamfered in the radial direction (see figure below).

4-28

(

)

Depth = Allowance Z

SRV-Z

Fig. 4-10 SRV-Z and SRV-R

PROCEDURE BEFORE PERFORMING THE MACHI NING

llowance R (SRV-R

M3P034

DIST: WPC Z0 TO FIN. SURFACE?

(4)

Z AXIS STOCK REMOVAL?

(5)

X/Y AXIS STOCK REMOVAL?

(6)

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

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

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

1 0 1 0 5

SURFACE ROUGHNESS <MENU>?

(7)

FINISH ALLOWANCE Z?

(8)

FINISH ALLOWANCE R?

(9)

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

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

A line machining unit s uch as that shown below is no w completed. This displ ay shows that an end mill has been automatically selected for the particular tool sequence that is to be programmed.

4-29

PROCEDURE BEFORE PERFORMING THE MACHINI NG

2. Creation of tool sequence

(1) W hile the mes sage

(2) Pr ess the menu ke y

that the previously registered tools ar e inclu ded in the dis play.

The following

is registered.

(3) Press the menu key

programming.

NOMINAL DIAMETER?

(4)

TOOL FILE (ENDMILL)

WHICH TYPE OF TOOL <MENU>?

TOOL FILE

PROGRAM

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

to call the

to return to the

TOOL FILE

display shows that the 10-m m diameter end mill

D735P0025E

is displayed, press the curs or key

display on the screen, a nd check

D735P0026E

PROGRAM

display and continue

1 0

TOOL FILE CODE <MENU>?

(5)

MACHINING PRIORITY No.?

(6)

(Skip to the next article since the priority funct ion for the same tool is not to be used here. See Part 2, Chapter 5.)

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

4-30

PROCEDURE BEFORE PERFORMING THE MACHI NING

APPROACH POINT X, AUTO

(7)

[APPROACH POINT Y, AUTO

(8)

CUTTING DIRECTION <MENU>?

(9)

(Specify the directi on in which the circumf erence is to be cut. The possible d irections of cutting are clockwise (CW) and counterclockwise (CCW).)

FEEDRATE Z, <MENU>/DATA <INPUT>?

(10)

DEPTH OF CUT?

(11)

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

<MENU>?

→→→→

<MENU>?

→→→→

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

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

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

CCW

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

AUTO SET AUTO SET CW CUT

NM210-00528

AUTO SET

CUTTING SPEED, AUTO

(12)

FEED RATE, AUTO

(13)

M CODE?

(14)

M CODE?

(15)

A tool sequence such as that shown below is now completed.

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

→→→→

<MENU>?

→→→→

<MENU>?

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

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

AUTO SET

4-31

)

PROCEDURE BEFORE PERFORMING THE MACHINI NG

3. Creation of shape sequence

Next, let us program a s hape sequence. For outside linear machining, the edges of a material are to be machined. Set the dimensions of a shape such as that shown below.

145 (X coordinate of diagonal point)

Corner 2

(Y coordinate of

onal point

dia

(Y coordinate of the start point)

(1) W hile the message

SQUARE

Corner 1

5 (X coordinate of the start point)

PATTERN OF FIGURE <MENU>?

Corner 3

Corner 4

M3P037

is displayed, press th e menu key

D735P0027E

CORNER 1 COORDINATE X?

(2)

CORNER 1 COORDINATE Y?

(3)

CORNER 3 COORDINATE X?

(4)

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

5 5 1 4 5

4-32

PROCEDURE BEFORE PERFORMING THE MACHI NING

CORNER 3 COORDINATE Y?

(5)

CORNER 1 CHAMFER?

(6)

CORNER 2 CHAMFER?

(7)

CORNER 3 CHAMFER?

(8)

CORNER 4 CHAMFER?

(9)

PATTERN OF FIGURE <MENU>?

(10)

A shape sequence such as that shown below is now completed.

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

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

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

9 5

SHAPE END

4. Shape check

Here, let us call the

(1) Press the menu key (2) Press the menu key

SHAPE CHECK

SHAPE CHECK SHAPE CONTINUE

display on the screen.

to call the

4-33

SHAPE CHECK

D735P0028E

display.

PROCEDURE BEFORE PERFORMING THE MACHINI NG

D735P0029E

The PLANE CHANGE f unciton is desc ribe d here. The s hape be ing d ispla yed in pr oce dura l step (2) is that of the workpiece as seen from above. With this function, it becomes possible to display shapes as seen from the side or from an oblique angle.

The selectable pla ne is one of the f our types sho wn below. It is also possib le to display one of two plane pairs (either XY-XZ (XY plane and XZ plane) or XY-YZ (XY plane and YZ plane)) at the same time. See Section 6-3, “SHAPE CHECK Display” of the Operating Manual for the details.

4-34

XZ plane

PROCEDURE BEFORE PERFORMING THE MACHI NING

Stereographic

view

XY plane

YZ plane

Fig. 4-11 Plane selection

Let us now display shapes of various planes.

XY-XZ plane

(3) Press the menu key (4) Press the menu key

Shapes as seen from above and from the side are selected.

(5) Press the menu key

As shown below, a shape as seen from above ( XY plane) a nd a shape as s een from

PLANE CHANGE XY-XZ

SHAPE CONTINUE

the side (XZ plane) are displayed at the same time.

M3P040

to display shapes continuously.

4-35

PROCEDURE BEFORE PERFORMING THE MACHINI NG

Three-dimens ional pla n

(6) Press the menu key (7) Press the menu key

A shape as seen obliquely from above is selected.

(8) Press the menu key

The shape will be displayed in stereographic form as shown below.

PLANE CHANGE 3-D

SHAPE CONTINUE

D735P0030E

to display shapes continuously.

4-36

PROCEDURE BEFORE PERFORMING THE MACHI NING

(9) Press the menu key (10) Press the menu key XY to change the display to that of XY plan.

Note:

(11) Press the menu key

This completes an outside linear machining unit.

The selected plane maintains its shape until another plane has been selected.

4-4-9 Point machining unit (1)

Let us create a program unit that is us e d to dr ill a 10- mm diameter through-ho le. This machining unit is referred to as a drilling unit.

PLANE CHANGE

PROGRAM

. The

PROGRAM

D735P0031E

display is resumed.

4-37

NM210-00519

PROCEDURE BEFORE PERFORMING THE MACHINI NG

1. Creation of point machining unit (1)

(1) W hile message

MACH-ING MACHINING UNIT <MENU>?

(2) (3) Press the menu key

The following help window will be presented.

MACHINING UNIT <MENU>?

HELP

is displayed, press the menu key

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

POINT

DRILLING

D735P0032E

Now, start creating the point m achining unit. The d ata for the item DIA, DEPTH and CHMF will be specified here.

HOLE DIAMETER?

(4)

HOLE DEPTH?

(5)

CHAMFER WIDTH?

(6)

A machining program unit such as that shown b elow is now com pleted. This shows t hat a spot and a drill have been automatically selected for the tool sequence that is to be programmed.

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

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

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

1 0 2 0 0

4-38

PROCEDURE BEFORE PERFORMING THE MACHI NING

2. Creation of tool sequence

For the point m achining unit, it is necessar y just to set the c utting parameters (c ircumferential speed and feedrate) since most of the tool sequence data are set automatically.

(1) While the message

position under the article C-SP by pressing the cursor key

CUTTING SPEED, AUTO

(2)

FEEDRATE, AUTO

(3)

M CODE?

(4)

M CODE?

(5) (6) Press the cursor key

the article C-SP.

CUTTING SPEED, AUTO

(7)

FEEDRATE, AUTO

(8)

M CODE?

(9)

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

WHICH TYPE OF TOOL <MENU>?

<MENU>?

→→→→

<MENU>?

→→→→

eight times in succession to move the cursor to the position under

<MENU>?

→→→→

<MENU>?

→→→→

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

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

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

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

is displayed, move the cursor to the

six times in successi on.

HSS AUTO HSS AUTO

HSS AUTO

D735P0033E

M CODE?

(10)

A tool sequence such as that shown below is now completed.

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

4-39

)

PROCEDURE BEFORE PERFORMING THE MACHINI NG

3. Creation of shape sequence

Next, create a shape s equence. For drillin g, input the coord inates of the ho le center as sho wn below.

(Y coordinate of hole center

(1) W hile the mes sage

POINT

key

100

(X coordinate of hol e ce nter)

M3P046

POINT CUTTING PATTERN <MENU>?

is displayed, press the menu

D735P0034E

Z VALUE OF WORK SURFACE?

(2)

HOLE POSITION X?

(3)

HOLE POSITION Y?

(4)

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

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

0 1 0 0 2 0

4-40

PROCEDURE BEFORE PERFORMING THE MACHI NING

PATH <XY:0, Y

(5)

(The tool path to the next hole is to be selected from the three types shown below. If, however, the hole to which the tool is to be fed does not exis t, input 0 since the selected function is unavailab le.)

If 0, both the X and Y axes move simultaneousl

Fig. 4-12 Tool path

OMIT SPT MACHINING <Y:1, N:0>?

(6)

→→→→

X:1, X

Y:2>?

→→→→

If 1, the X axis starts moving after the Y axis has moved.

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

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

If 2, the Y axis starts moving after the X axis has moved.

M3P047

(If 0, drilling occurs. If 1, positioning only occurs.)

RETURN POSITION <INIT:0, R:1>?

(7)

The height of the tool path to the next hole is to be selected from the two types shown below. (If however, the hole to wh ich the t ool is to be fed does not ex ist, inpu t 0 since th e sel ected function is unavailab le.)

[1]

[6]

Initial point

[5]

[2]

R point

[3] [4]

If 0, the tool moves to the next hole at the hei

ht of initial point.

Fig. 4-13 Return position

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

[1]

[2]

Initial point

[5]

[3]

[4]

Cutting Positionin

If 1, the tool moves to the next hole at the hei

R point

ht of R point.

M3P048

POINT CUTTING PATTERN <MENU>?

(8)

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

SHAPE END

A shape sequence such as that shown below is now completed.

4-41

PROCEDURE BEFORE PERFORMING THE MACHINI NG

4. Shape check

Let us call the

(1) Press the menu key (2) Press the menu key

SHAPE CHECK

SHAPE CHECK SHAPE CONTINUE

display on the screen to check the shapes.

to call the

SHAPE CHECK

display.

D735P0035E

4-42

PROCEDURE BEFORE PERFORMING THE MACHI NING

D735P0036E

The SCALE CHANG E func tion is ex plained h ere. T his func tion a llows en largem ent/reductio n of shapes, as well as changing of the shape display position.

Enlargement of shapes

Let us display a 10 mm diameter hole in enlarged form using the SCALE CHANGE function.

(3) Press the menu key (4) Us ing the curs or keys

shown below.

SCALE CHANGE

, place the cursor on th e 10 mm diameter hole position as

4-43

PROCEDURE BEFORE PERFORMING THE MACHINI NG

SCALE <INPUT>?

(5)

(The size of the shap e is changed so that the line in the center on the top of the scr een becomes 20 mm in length.)

(6) Press the menu key

As shown below, the s hape has been en larged with its c enter in the 10 mm diam eter

hole position.

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

SHAPE CONTINUE

2 0

D735P0037E

4-44

PROCEDURE BEFORE PERFORMING THE MACHI NING

Reduction of shapes

(7) Press the menu key

SCALE <INPUT>?

(8)

(The size of the shap e is changed so that the line in the center on the top of the scr een becomes 100 mm in length.)

(9) Press the menu key

As shown below, the shape has been reduced in size.

SCALE CHANGE

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

SHAPE CONTINUE

1 0 0

D735P0038E

4-45

PROCEDURE BEFORE PERFORMING THE MACHINI NG

(10) Press the menu key

This completes the creation of a point machining unit.

4-4-10 Point machining unit (2)

Let us create a unit th at is used to dr ill four M8 tapped through-ho les. This m achining pro gram unit is referred to as a tapping unit.

PROGRAM

to resume the

PROGRAM

D735P0039E

display.

1. Creation of point machining unit (2)

(1) While the message

MACH-ING MACHINING UNIT <MENU>?

(2)

MACHINING UNIT <MENU>?

is displayed, press the m enu key

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

4-46

NM210-00520

POINT

TAPPING

PROCEDURE BEFORE PERFORMING THE MACHI NING

(3) Press the menu key

HELP

D735P0040E

Now, start creating the point m achining unit. The data for the ar ticle NOM-φ, TAP-DEP will be specified here.

TYPE OF TAP?

(4)

ACTUAL DIAMETER OF TAP?

(5)

(Setting of the nom inal diameter causes autom atic setting of the outer diameter, the pitch and the amount of chamfering.)

TAPPING DEPTH?

(6)

CHAMFER WIDTH?

(7)

CHIP VAC. CLEANER <Y:1, N:0>?

(8)

A point machining un it such as that shown belo w is now completed. This s hows that after the data input for the point machining unit, a spot, a drill and a tap ha ve bee n automatically selec ted for the tool sequence that is to be programmed.

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

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

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

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

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

METRIC THRD (M)

2 0

4-47

PROCEDURE BEFORE PERFORMING THE MACHINI NG

2. Creation of tool sequence

(1) Pr ess the cursor k ey

the article C-SP.

CUTTING SPEED, AUTO

(2)

FEEDRATE, AUTO

(3)

M CODE?

(4)

M CODE?

(5) (6) Press the cursor key

the article C-SP.

CUTTING SPEED, AUTO

(7)

FEEDRATE, AUTO

(8)

M CODE?

(9)

M CODE?

(10) (11) Press the cursor key

the article C-SP.

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

six times in succession to move the cursor to the position under

<MENU>?

→→→→

<MENU>?

→→→→

eight times in succession to move the cursor to the position under

<MENU>?

→→→→

<MENU>?

→→→→

eight times in succession to move the cursor to the position under

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

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

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

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

HSS AUTO HSS AUTO

D735P0041E

CUTTING SPEED, AUTO

(12)

FEEDRATE, AUTO

(13)

M CODE?

(14)

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

→→→→

<MENU>?

→→→→

<MENU>?

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

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

4-48

HSS AUTO HSS AUTO

PROCEDURE BEFORE PERFORMING THE MACHI NING

M CODE?

(15)

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

A tool sequence such as that shown below is now completed.

3. Creation of shape sequence

Next, create a shape sequence. For ta pping, four holes are to be drilled . These holes are to be set as one shape, as shown below.

25 (Radius of circle - R)

(Y coordinate of

circle center)

(X coordinate of circle center)

(1) W hile the mes sage

CIRCLE

key

POINT CUTTING PATTERN <MENU>?

Start point

M3P057

is displayed, press the menu

D735P0042E

Z VALUE OF WORK SURFACE?

(2)

CIRCLE CENTER X?

(3)

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

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

4-49

0 5 0

PROCEDURE BEFORE PERFORMING THE MACHINI NG

CIRCLE CENTER Y?

(4)

ANGLE OF START PT FROM X AXIS?

(5)

(

Input the angle of the line co nnect ing the center of the c ircle an d the f irst hol e to be drille d

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

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

6 0 0

with respect to the X axis.)

Example 1: Example 2:

Start point

Center

45°

2 5

0°

M3P058

CIRCLE RADIUS R?

(6)

270°

Start point

Center

0°

–90°

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

NUMBER OF HOLES?

(7)

RETURN POSITION <INIT:0, R:1>?

(8)

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

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

(For Return position see Fig. 4-13.)

POINT CUTTING PATTERN <MENU>?

(9)

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

A shape sequence such as that shown below is now completed.

4 1

SHAPE END

4-50

PROCEDURE BEFORE PERFORMING THE MACHI NING

4. Shape check

Let us call shapes on the

(1) Press the menu key (2) Press the menu key

SHAPE CHECK

SHAPE CHECK. SHAPE CONTINUE.

display.

D735P0043E

4-51

PROCEDURE BEFORE PERFORMING THE MACHINI NG

(3) Press the menu key (4) Press the menu key

The reverse-display status of displayed.

The following display shows the unit number 4 shape of point machining unit (1).

SHAPE ERASE SHAPE UNIT

several times to display shapes on a unit basis.

SHAPE UNIT

to erase the shape.

is cleared when the final shape has been

D735P0044E

4-52

PROCEDURE BEFORE PERFORMING THE MACHI NING

(5) Press the menu key

This completes the creation of a point machining (tapping) unit.

4-4-11 End unit

Let us create an end unit that indicates the end of the program.

(1) While the message

CONTINUE <Y:1, N:0>?

(2)

(Specify whether or not the m achining program is to be repeated. If 0, the pr ogram ends with the particular step. If 1, the program returns to its beginning and returns to machine the next workpiece.)

PARTS COUNTER <Y:1, N:0>?

(3)

(Specify whether or not the number of times that the machining operation has been repeated is to be counted. If 0, counting does not occur. If 1, counting occurs and the results are displayed on the

An end unit such as that shown below is now completed, which m eans that the creation of the program is to be ended.

PROGRAM

MACHINING UNIT <MENU>?

POSITION

to resume the

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

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

display of the screen.)

PROGRAM

is displayed, press the menu key

display.

D735P0045E

END

4-53

PROCEDURE BEFORE PERFORMING THE MACHINI NG

4-4-12 End of the program

(1) Press the menu selector key. (2) Press the menu key

Display of the created program Let us trace the create d program back to its beginning. R epeated depress ion of the cursor k ey

causes the screen to scr oll up c ont inu ous ly to display the part of the program that precedes

the existing part. Depressing of the cursor key In addition, the program can also be checked using the page keys

however, the cursor moves on a unit basis. The following shows the entire program (actuate the cursor keys to check the program):

PROGRAM COMPLETE

causes the program to advance.

D735P0046E

. In this case,

4-54

PROCEDURE BEFORE PERFORMING THE MACHI NING

UNo. MAT INITIAL-Z ATC MODE MULTI MODE MULTI FLAG PITCH-X PITCH-Y

0 S45C 20. 1 OFF

UNo. UNIT ADD. WPC X Y th Z 4

1 WPC-1 -300. -200. 0. -100. 0.

UNo. UNIT DEPTH SRV-Z BTM WAL FIN-Z FIN-R

2 FACE MIL 0. 3. 2

SNo. TOOL NOM-φ No. APRCH-X APRCH-Y TYPE ZFD DEP-Z WID-R C-SP FR M M

R1 F-MILL 80.A ? ? XBI

FIG PTN P1X/CX P1Y/CY P3X/R P3Y CN1 CN2 CN3 CN4

1 SQR 0. 0. 150. 100.

UNo. UNIT DEPTH SRV-Z SRV-R RGH CHMF FIN-Z FIN-R

3 LINE OUT 10. 10. 5. 3

SNo. TOOL NOM-φ No. APRCH-X APRCH-Y TYPE ZFD DEP-Z WID-R C-SP FR M M

R1 E-MILL 10.A ? ? CW G01 10.

FIG PTN P1X/CX P1Y/CY P3X/R P3Y CN1 CN2 CN3 CN4

1 SQR 5. 5. 145. 95. R5. R5.

UNo. UNIT DIA DEPTH CHMF

4 DRILLING 10. 20. 0.

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

12CTR-DR

DRILL

FIGPTN ZXYAN1AN2T1T2FMNPQR

1 PT 0. 100. 20.

UNo. UNIT NOM-φ MAJOR-φ PITCH TAP-DEP CHMF CHP

5 TAPPING M8. 8. 1.25 20. 1.8 0

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

CTR-DR

DRILL

TAP

FIGPTN ZXYAN1AN2T1T2FMNPQR

1 CIR 0. 50. 60. 0.

UNo. UNIT CONTI. NUMBER ATC XYZ4ANGLE

6 END 0 0

20.

10.

20.

6.9

M8.

10.

"""""""

10.517

6.9

20.

24.75

20.

25.

100.

0. 0.

100

"""

3. 56. 121 1.079

54 0.027

90°

DRIL"T5.6355

90°

PCK1

FIX

"""

000

T3.45 P1.25

63 55 13

0.1

0.205

0.1

0.134

1.25

Fig. 4-14 Sample program

4-55

PROCEDURE BEFORE PERFORMING THE MACHINI NG

4-5

Registration of Tools in a Tool Data File

During creation of a program, the names and nominal diameters of the tools required for machining should have already been input. To m achine a workpiece by automatic run, those tools must be mounted in a tool maga zine in adva nce. In addit ion, the tools t o be m ounted in a tool magazine must be registered in a tool data file. Reg istration of tools in a tool data file is referred to as assignment of pocket numbers to the tools.

4-5-1 Pocket numbers and tool numbers

The pocket number refers to the number inscribed on the side face of the pocket of a tool magazine. The tool that h as been mounted in the pock et is s pec if ied by the pocket number . T he identification number of the pocket which accommodates a tool is called tool number.

Tool magazine model V

Tool magazine model H

This tool is referred to as the tool having tool No. 4.

These numbers are referred to as pocket numbers.

Note:

NM210-00529

The design of the tool m agazine slightl y differs according to the t ype of m achine to be used.

4-56

4-5-2 TOOL DATA display

PROCEDURE BEFORE PERFORMING THE MACHI NING

Carry out the following key operations to call the

(1) Press the display selelctor key. (2) Press the menu key

The

Function of

TOOL DATA

The tools are displa yed in order of pocket num ber; the pocket numbers being displayed on the left end of the screen.

If no tool types are being displayed on the s c reen, this ind ic ates that no tools are mounted in the tool magazine. The pocket numbers on the numbers of the tool magazine. The relationship between these two types of pocket numbers can be represented as shown below.

TOOL DATA

display shows the t ypes of tools mounted in the tool magazine. T he types of

TOOL DATA

display will then be presented as shown below.

display

TOOL DATA

display:

display correspond to the pocket

Fig. 4-15 Correspondence to the pocket numbers

4-57

D735P0047ED735P0047ENM210-00530

PROCEDURE BEFORE PERFORMING THE MACHINI NG

- NOTE -

4-58

4-5-3 TOOL LAYOUT display

PROCEDURE BEFORE PERFORMING THE MACHI NING

Carry out the following key operation to call the

(1) Press the display selector key. (2) Press the menu key

The following

TOOL LAYOUT

display will be presented.

TOOL LAYOUT

display:

D735P0048E

Function of

TOOL LAYOUT

The are to be registered in a tool data file. This display consists of two sections:

NEXT display on the right side, and CURRENT display on the left side. On the CURRENT display, tool nam es and pocket numbers ar e indicated in the sam e state as that of the

DATA

tools that have been set o n the program and ass ignment of pocket num bers to them . W hen the setup operations are completed, the tools on the NEXT display will be registered on the CURRENT display (tool data).

The following figure shows the relationship between the display and

TOOL LAYOUT

display is the display on which the tools that have been set on the program

display. The NEXT display is used to carry out set up operations such as displa y of the

TOOL LAYOUT

display

display:

PROGRAM

display,

TOOL

TOOL DATA

4-59

PROCEDURE BEFORE PERFORMING THE MACHINI NG

The CURRENT display and the display always possess the same contents . Thus, the tool data als o changes when new tools have been registered on the CURRENT display.

TOOL DATA

D735P0049E

D735P0050LE

4-60

PROCEDURE BEFORE PERFORMING THE MACHI NING

Registration of new tools

The tools that have been set on the program are displayed.

D735P0051E

4-61

D835P0050RE

PROCEDURE BEFORE PERFORMING THE MACHINI NG

4-5-4 Registration of tools

The display of m enu data

NUMBER?

which has been previously created in Section 4-4. See Section 5-1, “ TOO L LAYOUT Dis play” of the Oper ating Manual f or detai ls of registrat ion of

tools.

(1)

is displayed on the

WORKPIECE PROGRAM NUMBER?

WORK No.

TOOL LAYOUT

is reversed, and the m essage

display. Input the work number of the program

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

WORKPIECE PROGRAM

1 2 3 4

D735P0052E

The tools that have been set on the program having work No. 1234 will t hen be displayed as shown on the NEXT display. Let us assign pocket numbers to the displayed tools.

Three modes are available for assigning pocket numbers: automatic, manual, and shift. Automatic assignment, the simplest of these three modes, is described below.

Note:

(2) (3)

If automatic assignment is performed, data of the registered tools will be erased entirely. To prevent this data erasure, eit her the m anual assignment m ode or the s hift mode must be used.

PKNo. SHIFT OR ASSIGN <MENU>?

POCKET NUMBER ASSIGN <INPUT>?

Pocket numbers will then be assigned to the tools as shown below.

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

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

4-62

PKNo. ASSIGN

PROCEDURE BEFORE PERFORMING THE MACHI NING

D735P0053E

Next, carry out the fol lowing key operations to r egister the tools on t he NEXT display onto the CURRENT display.

LAYOUT FINISH <MENU>?

(4)

LAYOUT FINISH <INPUT>?

(5)

LAYOUT FINISH

(6)

The tools will be registered on the CURRENT display as shown below.

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

LAYOUT FINISH

4-63

PROCEDURE BEFORE PERFORMING THE MACHINI NG

Let us recall the

(7) Press the display selector key. (8) Press the menu key

The tools th at h av e b een registered in the

the

TOOL DATA

display on the screen.

TOOL DATA

display, as shown below.

D735P0054E

TOOL LAYOUT

display will be pres e nted in

4-64

PROCEDURE BEFORE PERFORMING THE MACHI NING

4-6 Check of the Machining Path

Let us return the

(1) Press the display selector key. (2) Press the menu key

The program with work No. 1234 will be displayed as shown below.

Next, let us call the display. See Section 6-2, “TOOL PATH CHECK Display” of the Operating Manual for details.

PROGRAM

TOOL PATH

display.

D735P0055E

display on the screen and check the machining path on that

4-65

PROCEDURE BEFORE PERFORMING THE MACHINI NG

(3) Press the menu key

The following

TOOL PATH

D735P0051E

display will be presented.

4-66

D7350056E

PROCEDURE BEFORE PERFORMING THE MACHI NING

(4) Press the menu key (5) Next, press the menu key

through to the end.

PART SHAPE

to display shapes continuously.

PATH CONTINUE

to display the machining path of the tool

(6) Press the menu key (7) Pr es s the menu key

reverse-display state of the menu continues until the entire machining path appeared.

PATH ERASE

PATH STEP

to erase the machining path of the tool.

several times to displa y the mac hining pat h in steps . The

D735P0057E

4-67

PROCEDURE BEFORE PERFORMING THE MACHINI NG

D735P0058E

(8) To check the machining path in further details, use the PLANE CHANGE function (see

Subsection 4-4-8) or the SCALE CHANGE function (see Subsection 4-4-9).

(9) W hen the all operatio n has been com pleted, press th e display selector key and the m enu

POSITION

key

to resume the

POSITION

display.

4-68

PART 2

MAZATROL PROGRAM FUNCTIONS

Part 2 describes all the functions of the MAZATROL program.

H735P20019E

mazak Mazatrol Fusion 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

OPERATIONAL WARRANTY FOR THE NC UNIT

Operating Environment

Introduction

1 MAZATROL PROGRAM

2 SYSTEM OF COORDINATES

2-1 Machine Coordinates System

2-2 Workpiece Coordinates System

2-3 Machine Coordinates System and Workpiece Coordinates System

2-4 Basic Coordinates

2-5 Auxiliary Coordinates

3 FUNCTION OF KEYS AND SWITCHES

4 PROCEDURE BEFORE PERFORMING THE MACHINING

4-1 Diagram of Preparation for the Machining

4-2 Part Drawings and Stock Materials

4-3 Registration of Tools

4-3-1 Calling up the TOOL FILE display

4-3-2 Registration of tools

4-4 Creation of Simple Programs

4-4-1 Program structure

4-4-2 Calling up the PROGRAM display

4-4-3 Assigning workpiece numbers

4-4-4 Creating a program

4-4-5 Creation of common unit

4-4-6 Creation of basic coordinates system unit

4-4-7 Face machining unit

4-4-8 Line machining unit

4-4-9 Point machining unit (1)

4-4-10 Point machining unit (2)

4-4-11 End unit

4-4-12 End of the program

Registration of Tools in a Tool Data File

4-5-1 Pocket numbers and tool numbers

4-5-2 TOOL DATA display

4-5-3 TOOL LAYOUT display

4-5-4 Registration of tools

4-6 Check of the Machining Path