fanuc TURN MATE i Operators Manual

Download

FANUC TURN MATE

OPERATOR’S MANUAL

B-64254EN/06

• No part of this manual may be reproduced in any form.

• All specifications and designs are subject to change without notice.

The products in this manual are controlled based on Japan’s “Foreign Exchange and

Foreign Trade Law”. The export from Japan may be subject to an export license by the

government of Japan.

Further, re-export to another country may be subject to the license of the government of

the country from where the product is re-exported. Furthermore, the product may also be

controlled by re-export regulations of the United States government.

Should you wish to export or re-export these products, please contact FANUC for advice.

In this manual we have tried as much as possible to describe all the various matters.

However, we cannot describe all the matters which must not be done, or which cannot be

done, because there are so many possibilities.

Therefore, matters which are not especially described as possible in this manual should be

regarded as ”impossible”.

B-64254EN/06 SAFETY PRECAUTIONS

SAFETY PRECAUTIONS

When using a machine equipped with the FANUC TURN MATE i, be sure to observe the following safety precautions.

s-1

SAFETY PRECAUTIONS B-64254EN/06

DEFINITION OF WARNING, CAUTION, AND NOTE

This manual includes safety precautions protecting the user and preventing damage to the machine. Precautions are classified into Warning and Caution according to the degree of the risk or the severity of damage. Also, supplementary information is described as Note. Read the Warning, Caution, and Note thoroughly before attempting to use the machine.

WARNING

Applied when there is a danger to the user being

injured or when there is a risk to the user, being injured, and the equipment, being damaged, if the warning statement is not followed up.

CAUTION

Applied when there is a danger to the equipment

being damaged, if the caution statement is not followed up.

NOTE

The Note is used to indicate supplementary

information other than Warning and Caution.

∗ Read this manual carefully, and store it in a safe place.

s-2

B-64254EN/06 SAFETY PRECAUTIONS

GENERAL WARNINGS AND CAUTIONS

To ensure safety while using a machine featuring the TURN MATE i function, observe the following precautions:

WARNING

1 Confirm, on the screen, that the data has been

entered correctly before proceeding to the next operation. Attempting operation with incorrect data may cause the tool to strike the workpiece or machine, possibly breaking the tool and/or machine and/or injuring the operator.

2 When using constant surface speed control, set the

maximum rotating speed of the spindle to a value that is allowed for the workpiece and workpiece holding unit. Otherwise, the workpiece or holding unit may be removed by centrifugal force damaging the machine or injuring the operator.

3 Set all necessary parameters and data items before

starting TURN MATE i operations. Note that if the cutting conditions are not suitable for the workpiece, the tool may be damaged and/or the operator may be injured.

4 After creating a machining program using TURN

MATE i functions, do no run the machining program immediately on the machine . Before starting production machining, run the machine with no workpiece attached to the machine to make sure that the tool will not strike a workpiece or the machine. If the tool strikes the machine and/or workpiece, the tool and/or machine may be damaged, with possibility to injure the operator.

5 Switching between inch and metric inputs does not

convert the measurement units of data such as the workpiece origin offset, parameter, and current position. Before starting the machine, therefore, determine which measurement units are being used. Attempting to perform an operation with invalid data specified may damage the tool, the machine itself, the workpiece, or cause injury to the user.

CAUTION

After pressing the power-on button, do not touch

any keys on the keyboard until the initial screen appears. Some keys are used for maintenance or special operations such that pressing such a key may cause an unexpected operation.

s-3

SAFETY PRECAUTIONS B-64254EN/06

OVERVIEW OF THIS MANUAL

This manual describes the functions of "TURN MATE i" for the Series 0 i -TC/Mate-TC or Series 0 i -TD/Mate-TD. For other functions, other than TURN MATE i, refer to the operator’s manual for the Series 0 i-TC/Mate-TC or Series 0 i -TD/Mate-TD. The specifications and features of TURN MATE i may differ from the specifications of the operator’s manual supplied by the machine tool builder. Be sure to read the manual provided by the machine tool builder. The functions of the CNC machine tool system are determined not only by the CNC, but by the combination of the machine tool, the power magnetic circuit of the machine tool, the servo system, the CNC, and the operator’s panel. It is impossible to cover all possible combinations of all functions, programming methods, and operations in a single manual. This manual explains only the TURN MATE i operations provided for the CNC. For individual CNC machine tools, refer to applicable manuals supplied by the machine tool builders. This manual explains as many detailed functions as possible. However, it is not possible to describe all the items which cannot be done or which the operator must not do. Therefore, please assume that functions not described in this manual cannot be performed. Detailed information and special conditions are explained in notes. The readers may encounter new technical terms in the notes not previously defined or described. In this case, read this manual through first, and then review the details.

s-4

B-64254EN/06 TABLE OF CONTENTS

SAFETY PRECAUTIONS............................................................................s-1

DEFINITION OF WARNING, CAUTION, AND NOTE .............................................s-2

GENERAL WARNINGS AND CAUTIONS............................................................... s-3

OVERVIEW OF THIS MANUAL .............................................................................. s-4

I. WHAT’S TURN MATE i ?

1 WHAT’S TURN MATE i ? ...................................................................... 3

II. BASIC SCREEN AND OPERATIONS

1 BASE SCREEN....................................................................................... 7

2 BASIC SCREEN OPERATIONS ...........................................................11

2.1 BUTTON OPERATION................................................................................ 12

2.2 CURSOR OPERATION ............................................................................... 13

2.3 TAB OPERATION........................................................................................ 13

2.4 CALCULATOR OPERATION....................................................................... 14

3 SETTING OF COORDINATE SYSTEM ................................................17

4 SETTING OF SPINDLE INFORMATION ..............................................20

4.1 SETTING OF SPINDLE SPEED..................................................................21

4.2 SETTING OF SURFACE SPEED ................................................................22

4.3 SETTING OF GEAR NUMBER.................................................................... 23

4.4 SETTING OF SPINDLE SPEED USING BUTTON ON MACHINE

OPERATOR'S PANEL................................................................................. 24

5 SETTING OF TOOL INFORMATION ....................................................25

5.1 TOOL SELECTION...................................................................................... 26

5.2 INPUT OF TOOL OFFSET .......................................................................... 27

5.2.1 Direct Input of Tool Offset.....................................................................................27

5.2.2 Measurement of Tool Offset ..................................................................................30

6 ALARM CHECK .................................................................................... 33

III. MANUAL CUTTING

1 MANUAL CUTTING .............................................................................. 37

2 MANUAL CUTTING IN LIMITED AREA ...............................................40

c-1

TABLE OF CONTENTS B-64254EN/06

IV. CUTTING CYCLE

1 OUTLINE ...............................................................................................47

1.1 WHAT’S CUTTING CYCLE ? ...................................................................... 48

1.2 CUTTING METHODS.................................................................................. 49

2 OPERATION .........................................................................................51

2.1 WORKFLOW ............................................................................................... 52

2.2 SETTING THE FEEDRATE......................................................................... 54

2.3 CREATING A NEW CUTTING CYCLE........................................................ 55

2.4 EDITING A CUTTING CYCLE..................................................................... 58

2.5 SELECTING A CUTTING CYCLE ............................................................... 59

2.6 DELETING A CUTTING CYCLE.................................................................. 61

2.7 NOTES ........................................................................................................ 63

2.7.1 Inhibition of Operation...........................................................................................63

2.7.2 Manual Intervention during Cutting Cycles ...........................................................63

2.7.3 Tool Nose Radius Compensation ...........................................................................63

3 FACE CYCLE........................................................................................ 64

3.1 OUTLINE ..................................................................................................... 65

3.2 TOOL CUTTING MOTIONS ........................................................................ 66

3.3 INPUT DATA ...............................................................................................69

4 CHAMFER CYCLE................................................................................ 71

4.1 OUTLINE ..................................................................................................... 72

4.2 TOOL CUTTING MOTIONS ........................................................................ 74

4.3 INPUT DATA ...............................................................................................81

5 RECTANGULAR CYCLE...................................................................... 82

5.1 OUTLINE ..................................................................................................... 83

5.2 TOOL CUTTING MOTIONS ........................................................................ 85

5.2.1 Rough Cutting Motions..........................................................................................85

5.2.2 Finish Cutting Motions...........................................................................................93

5.3 INPUT DATA ...............................................................................................98

6 TAPER CYCLE ...................................................................................100

6.1 OUTLINE ................................................................................................... 101

6.2 TOOL CUTTING MOTIONS ...................................................................... 103

6.2.1 Rough Cutting Motions........................................................................................103

6.2.2 Finish Cutting Motions.........................................................................................111

6.3 INPUT DATA .............................................................................................116

c-2

B-64254EN/06 TABLE OF CONTENTS

7 RADIUS CYCLE.................................................................................. 118

7.1 OUTLINE ................................................................................................... 119

7.2 TOOL CUTTING MOTIONS ...................................................................... 121

7.2.1 Rough Cutting Motions........................................................................................121

7.2.2 Finish Cutting Motions.........................................................................................121

7.3 INPUT DATA .............................................................................................122

8 FREE FIGURE CYCLE........................................................................124

8.1 OUTLINE ................................................................................................... 125

8.2 TOOL CUTTING MOTIONS ...................................................................... 126

8.2.1 Rough Cutting Motions........................................................................................126

8.2.2 Finish Cutting Motions.........................................................................................126

8.3 INPUT DATA .............................................................................................127

8.3.1 Details of Input Data ............................................................................................127

8.3.2 Free Figure Input Data Screen..............................................................................129

8.3.3 Creating New Free Figure ....................................................................................134

8.4 NOTES ...................................................................................................... 137

8.4.1 Creation of Figure ................................................................................................137

8.4.2 Cutting Cycle with Manual In-Feeding................................................................138

8.4.3 Pocket Figure Operation.......................................................................................139

9 DRILL CYCLE ..................................................................................... 140

9.1 OUTLINE ................................................................................................... 141

9.2 TOOL CUTTING MOTIONS ...................................................................... 142

9.3 INPUT DATA .............................................................................................148

10 TAP CYCLE ........................................................................................150

10.1 OUTLINE ................................................................................................... 151

10.2 TOOL CUTTING MOTIONS ...................................................................... 152

10.3 INPUT DATA .............................................................................................156

11 GROOVE CYCLE................................................................................ 157

11.1 OUTLINE ................................................................................................... 158

11.2 TOOL CUTTING MOTIONS ...................................................................... 160

11.2.1 Rough Cutting Motions........................................................................................160

11.2.2 Finish Cutting Motions.........................................................................................163

11.3 INPUT DATA .............................................................................................167

12 THREAD CYCLE................................................................................. 169

12.1 OUTLINE ................................................................................................... 170

12.2 TOOL CUTTING MOTIONS ...................................................................... 171

12.2.1 Outer Thread Cycle ..............................................................................................171

12.2.2 Inner Thread Cycle...............................................................................................173

12.2.3 Cutting Methods...................................................................................................175

12.3 INPUT DATA .............................................................................................180

c-3

TABLE OF CONTENTS B-64254EN/06

13 THREAD REPAIR CYCLE .................................................................. 182

13.1 OUTLINE ................................................................................................... 183

13.2 TOOL CUTTING MOTIONS ...................................................................... 184

13.3 INPUT DATA .............................................................................................185

V. SEQUENTIAL EXECUTION OF CUTTING CYCLES

1 OVERVIEW .........................................................................................191

2 CUTTING MOTIONS ........................................................................... 192

3 OPERATIONS ..................................................................................... 194

3.1 OPERATION PROCEDURE...................................................................... 195

3.2 PROCESS CREATION.............................................................................. 202

3.3 PROCESS ALTERATION.......................................................................... 204

3.4 PROCESS DELETION .............................................................................. 205

VI. CONVERSION OF CUTTING CYCLE TO NC STATEMENT (OPTION)

1 OVERVIEW .........................................................................................209

2 OPERATIONS ..................................................................................... 210

2.1 OPERATIONS ON SINGLE EXECUTION SCREEN ................................. 211

2.2 OPERATIONS ON SEQUENTIAL EXECUTION SCREEN........................ 214

3 NOTES ................................................................................................217

VII. DATA INPUT/OUTPUT USING MEMORY CARD

1 OVERVIEW .........................................................................................221

2 CUTTING CYCLE DATA INPUT/OUTPUT ......................................... 222

2.1 CUTTING CYCLE DATA INPUT................................................................ 223

2.2 CUTTING CYCLE DATA OUTPUT............................................................ 227

3 PROGRAM INPUT/OUTPUT...............................................................231

3.1 PROGRAM INPUT ....................................................................................232

3.2 PROGRAM OUTPUT ................................................................................ 236

4 MEMORY CARD FORMATTING ........................................................238

VIII. DATA SETTING

1 OVERVIEW .........................................................................................241

2 LANGUAGE SETTING........................................................................242

3 INCH/METRIC SETTING.....................................................................243

4 FINISHING AMOUNT SETTING .........................................................244

c-4

B-64254EN/06 TABLE OF CONTENTS

IX. MDI KEY OPERATION FUNCTION (OPTION)

1 OVERVIEW .........................................................................................247

2 SINGLE EXECUTION SCREEN (BASE SCREEN) ............................ 248

3 CUTTING CYCLE SELECTION SCREEN .......................................... 249

4 CYCLE INPUT DATA SCREEN ..........................................................250

5 FREE FIGURE INPUT DATA SCREEN .............................................. 251

6 SEQUENTIAL EXECUTION SCREEN................................................ 253

APPENDIX

A WARNINGS......................................................................................... 257

B ALARMS .............................................................................................260

B.1 ALARMS COMMON TO ALL CYCLES...................................................... 261

B.2 RECTANGULAR, TAPER, RADIUS, FREE FIGURE AND FACE CYCLES

................................................................................................................... 261

B.3 THREAD CYCLE ....................................................................................... 261

B.4 GROOVE CYCLE ...................................................................................... 262

B.5 HOLE CYCLE............................................................................................ 262

B.6 SEQUENTIAL EXECUTION ...................................................................... 262

C PARAMETERS.................................................................................... 263

C.1 PARAMETERS RELATED TO BASIC OPERATIONS .............................. 264

C.2 PARAMETERS RELATED TO COLOR PALETTES.................................. 268

C.2.1 Setting Related to Color Palettes for Screen Display ...........................................268

C.2.2 Setting Related to Color Palettes for Icon Display...............................................271

C.2.3 Setting Related to Color Palettes for Guidance Display.......................................273

C.3 PARAMETERS RELATED TO CUTTING CYCLES .................................. 275

C.3.1 Parameters Common to All Cycles ......................................................................275

C.3.2 Turning Cycle.......................................................................................................277

C.3.3 Thread Cycle ........................................................................................................278

C.3.4 Groove Cycle........................................................................................................279

C.3.5 Hole Cycle............................................................................................................280

APPENDIX (FOR MACHINE TOOL BUILDER)

A LADDER PROGRAM CREATION ......................................................283

A.1 TURN MATE i SCREEN SWITCH SIGNAL.............................................. 284

A.2 MODE CHANGE........................................................................................ 285

A.3 CYCLE START .......................................................................................... 286

A.4 REVERSE TAP CYCLE............................................................................. 288

A.5 SPINDLE SPEED ...................................................................................... 291

c-5

TABLE OF CONTENTS B-64254EN/06

B LINKING MACRO CREATED BY MACHINE TOOL BUILDER WITH

TURN MATE i MACRO...................................................................... 293

B.1 LINKING MACRO PROGRAM................................................................... 294

B.1.1 In Case of 0i-TC/Mate-TC ...................................................................................294

B.1.2 In Case of 0i-TD/Mate-TD...................................................................................295

B.2 NOTES ...................................................................................................... 295

C PARAMETER SETTING......................................................................296

C.1 PARAMETERS NEEDED ON NC SIDE .................................................... 297

C.2 PARAMETERS NEEDED ON TURN MATE i SIDE.................................. 299

c-6

I. WHAT’S TURN MATE i ?

1.OVERVIEW OF

B-64254EN/06 OVERVIEW OF TURN MATE i

TURN MATE i

1 WHAT’S TURN MATE i ?

TURN MATE i provides integrated operation guidance functions for CNC lathes that are designed to enable the operator to perform turning without the need to create an NC program.

TURN MATE i screen

It has the following main features:

(1) Integrated display of all information necessary for operation on a

single screen

All information necessary for operation is integrated on a single

screen, so that the operator need not switch between screens.

(2) Simple screen operation using the touch panel or cursor keys By touching an item displayed on the screen or selecting it using

cursor keys, the operator can jump to a related operation screen. This allows intuitive operation.

(3) Easily operable even by operators inexperienced in CNCs It is not necessary to create machining programs in ISO code

format. By entering data in accordance with the guidance drawing displayed on the screen, it is possible to perform turning with ease.

(4) Support of cutting methods for general-purpose lathes It supports two types of cutting methods, manual cutting and

cutting cycles, often used with general-purpose lathes.

- 3 -

1. OVERVIEW OF TURN MATE i

OVERVIEW OF TURN MATE i B-64254EN/06

(a) Manual cutting It is possible to move the tool freely to perform cutting,

using the handle or the JOG switch. It is also possible to move the tool in a limited area.

(b) Cutting cycles A cutting cycle is a series of prescribed cutting motions

collected together. By starting the start button, the series of cutting motions is automatically executed.

Execution

(5) Various cutting cycles containing free figures are available. It provides all cutting cycles necessary for lathes. The following cutting cycles are available:

(a) Rough cutting cycle (pattern figure, free figure) (b) Finish cutting cycle (pattern figure, free figure) (c) Groove cycle (pattern figure, free figure) (d) Thread cycle (general-purpose screw) (e) Re-thread cycle (general-purpose screw) (f) Hole cycle (drill, tap)

- 4 -

II. BASIC SCREEN AND OPERATIONS

B-64254EN/06 BASIC SCREEN AND OPERATIONS 1.BASE SCREEN

1 BASE SCREEN

TURN MATE i has integrated all information necessary for operation on a single screen. This integrated screen is called the Base Screen.

(1) Present position

(2) Spindle speed

(5) Machine status

(3) Feedrate

(4) Tool number

(6) Guidance drawing for cutting cycle

(8)

larm

message

(10) Manual cutting screen

The Base Screen consists of nine sections and four soft keys. In each section, information display and operation functions are integrated together. Either by touching a section on the tough panel or by moving the focus to a section using cursor keys as appropriate and pressing the [INPUT] key, the operator can jump to the related operation screen.

(11) Setting screen

Base Screen

(12) Cutting cycle call

(7) Cutting cycle data

(9) Cutting cycle call number

- 7 -

1.BASE SCREEN BASIC SCREEN AND OPERATIONS B-64254EN/06

Each of the sections and soft keys is described below.

(1) Present position section

In this section, the present position (absolute coordinates) and the

load ratio (load meter) of the servo axis are displayed. Touching this section causes a jump to the workpiece coordinate system setting screen.

"Workpiece coordinate system setting screen": Screen for

setting the workpiece coordinate system.

(2) Spindle speed section

In this section, the actual spindle rotation speed (rpm (min-1)),

the commanded spindle speed (S_set), and the spindle load ratio (load meter) are displayed. In addition, the following states are represented by icons: (a) Spindle direction (CW or CCW) (b) Constant surface speed control (enabled or disabled)

Touching this section causes a jump to the spindle speed setting

screen. "Spindle speed setting screen": Screen for setting a spindle speed, turning constant surface

speed control ON/FF, and setting a gear number.

(3) Feedrate section

In this section, the actual feedrate and the commanded feedrate

(F_set) are displayed. Touching this section causes a jump to the feedrate setting screen. "Feedrate setting screen": Screen for setting the feedrate used in a cutting cycle.

(4) Tool number section

In this section, the currently selected tool number is displayed.

Touching this section causes a jump to the tool selection screen.

"Tool selection screen": Screen for selecting the tool to use and

setting tool data (offset value, radius of the tool nose, and virtual tool tip)

(5) Machine status section

In this section, the machine status is displayed.

MTN : The tool is moving along at least one axis. (The CNC is in MEM mode.) ALM : A CNC or machine alarm has been generated. EMG : Emergency stop state RESET : Reset state HOLD : Automatic operation suspend STOP : Automatic operation stop FIN : Miscellaneous function under execution MSG : An operator message has been generated.

- 8 -

B-64254EN/06 BASIC SCREEN AND OPERATIONS 1.BASE SCREEN

(6) Guidance drawing for cutting cycle section

In this section, the guidance drawing for the currently selected

cutting cycle is displayed. Touching this section causes a jump to the cutting cycle selection screen. "Cutting cycle selection screen": Screen for selecting the cutting cycle to create.

(7) Cutting cycle data section

In this section, the currently selected cutting cycle data (NOTE)

is displayed. Touching this section causes a jump to the cutting cycle input screen. "Cutting cycle input screen": Screen for editing the input data for the currently selected

cutting cycle

NOTE

By enabling the optional function and parameter

below, it is possible to display cutting methods (R+F, DIR, and XA/ZA) and cutting conditions (T, CSS, S, and T) as additional cutting cycle data.

• Optional function: Expansion of Machining

Cycle

• Parameter: Bit 4 (DID) of parameter No. 9103

= 1

Screen example)

(8) Alarm section

In this section, a P/S alarm (38 characters in length) is displayed.

Touching this section causes a jump to the alarm screen. "Alarm screen": Screen for displaying all NC alarm messages and operator

messages.

- 9 -

1.BASE SCREEN BASIC SCREEN AND OPERATIONS B-64254EN/06

(9) Cutting cycle call number section

TURN MATE i provides 40 areas for storing cutting cycle data.

The serial numbers for these storage areas are used as cutting cycle call numbers. In this section, the currently selected cutting cycle call number is displayed. Touching this section causes a jump to the cutting cycle call selection screen. "Cutting cycle call selection screen": Screen for selecting and deleting cutting cycles.

(10) Manual cutting screen switching soft key: [HANDLE]

This soft key causes a switch to the manual cutting screen. "Manual cutting screen": Screen for performing manual

cutting.

(11) Setting screen switching soft key: [SETTING]

This soft key causes a switch to the setting screen.

"Setting screen": Screen for selecting a language, switching between inch and

metric systems, and setting a default finishing amount.

(12) Cutting cycle call soft keys: [←][→]

Touching the [←] soft key causes selection of the cutting cycle

call number equal to the currently selected cutting cycle call number minus 1. Touching the [→] soft key causes selection of the cutting cycle call number equal to the currently selected cutting cycle call number plus 1.

- 10 -

2.BASIC SCREEN

B-64254EN/06 BASIC SCREEN AND OPERATIONS

OPERATIONS

2 BASIC SCREEN OPERATIONS

This chapter consists of the sections below.

2.1 BUTTON OPERATION ............................................................12

2.2 CURSOR OPERATION.............................................................13

2.3 TAB OPERATION.....................................................................13

2.4 CALCULATOR OPERATION..................................................14

- 11 -

2. BASIC SCREEN OPERATIONS

BASIC SCREEN AND OPERATIONS B-64254EN/06

2.1 BUTTON OPERATION

A section in which information display and operation functions are integrated together appear raised as shown below that does not appear raised provides information display functions only.) Such a raised section is called a button.

There are two methods to button operation: (1) Touch the desired section on the touch panel. (2) Move the focus (button cursor) to the desired section using the

cursor keys (↑, ↓, ←, and →) as appropriate and press the

[INPUT] key Either of the above methods causes a jump to the related operation screen.

Button cursor

(NOTE 2)

NOTE

1 To make a button appear more pronouncedly

raised, change the color settings on the color palette, using parameters Nos. 9156 and 9162.

2 The method of moving the focus to a section using

cursor keys requires the MDI key operation function (option). For details, see Part IX, "MDI Key Operation Function".

(NOTE 1)

. (A section

- 12 -

2.BASIC SCREEN

B-64254EN/06 BASIC SCREEN AND OPERATIONS

OPERATIONS

2.2 CURSOR OPERATION

The cursor can be moved between edit boxes, using the cursor key (↑ and ↓). The edit box on which the cursor is positioned is displayed gray (blue on a color LCD). By entering data in one edit box, the cursor is automatically moved to the next edit box.

Cursor

2.3 TAB OPERATION

On a setting screen such as the cutting cycle input screen, multiple tabs are displayed on top of the data in an edit box. By selecting one of these tabs, it is possible to switch to the corresponding one of the multiple edit boxes hidden behind.

There are two methods to tab selection: (1) Touch a tab on the touch panel. (2) Press the cursor key (← and →) as appropriate.

Either of the methods above causes the edit box of the selected tab to appear.

Tabs

- 13 -

2. BASIC SCREEN OPERATIONS

BASIC SCREEN AND OPERATIONS B-64254EN/06

2.4 CALCULATOR OPERATION

Functions are provided whereby when numeric data is input, expressions for arithmetic operations, trigonometric functions, square root calculations, and so forth can be input for calculation.

These functions can be used in the input of cycle data, input of free figure data, and setting of various data (such as workpiece coordinate system data).

Input example)

Cutting cycle input screen example

The following describes each calculation operation.

• Arithmetic operations

(addition, subtraction, multiplication, and division)

Arithmetic operations are performed by using the key operations

described below. The result of a calculation is displayed at the cursor position of input data. (1) Addition : 100.+200. [INPUT] (2) Subtraction : 100.-200. [INPUT] (3) Multiplication : 100.*200. [INPUT] (4) Division : 100./200. [INPUT]

- 14 -

2.BASIC SCREEN

B-64254EN/06 BASIC SCREEN AND OPERATIONS

• Trigonometric functions

(sine, cosine, tangent, arcsine, arccosine, arctangent)

Trigonometric function calculations are performed by using the

key operations described below. The result of a calculation is displayed at the cursor position of input data. (1) Sine : SIN[45] [INPUT] (2) Cosine : COS[45] [INPUT] (3) Tangent : TAN[45] [INPUT] (4) Arcsine : ASIN[0.5] [INPUT] (5) Arccosine : ACOS[0.5] [INPUT] (6) Arctangent : ATAN[20,2] [INPUT]

(Note that for an arctangent calculation, a special format using

two arguments is required. Enter data according to the format ATAN[a,b]. arctan(a/b) is calculated.)

For a calculation, brackets ( [ ] ) are required at all times.

• Square root

A square root calculation is performed by using the key

operations described below. The result of a calculation is displayed at the cursor position of input data. (1) Square root : SQRT[45] [INPUT]

For a calculation, brackets ( [ ] ) are required at all times.

• Exponential functions

Exponential function calculations are performed by using the key

operations described below. The result of a calculation is displayed at the cursor position of input data. (1) Exponential function 1 (An exponential function of e =

2.718... can be calculated.) : EXP[4] [INPUT] (2) Exponential function 2 ("a" raised to the power of "b" can

be calculated.) :

PWR[4,3] [INPUT]

(Note that for a calculation of exponential function 2, a special

format using two arguments is required. Enter data according to the format PWR[a,b]. "a" raised to the power of "b" is calculated.)

For a calculation, brackets ( [ ] ) are required at all times.

• Logarithmic functions

(common logarithm, natural logarithm)

Logarithmic function calculations are performed by using the key

operations described below. The result of a calculation is displayed at the cursor position of input data. (1) Common logarithm : LOG[45] [INPUT] (2) Natural logarithm : LN[45] [INPUT]

For a calculation, brackets ( [ ] ) are required at all times.

OPERATIONS

- 15 -

2. BASIC SCREEN OPERATIONS

BASIC SCREEN AND OPERATIONS B-64254EN/06

• Absolute value

An absolute value calculation is performed by using the key

operations described below. The result of a calculation is displayed at the cursor position of input data.

(1) Absolute value : ABS[-45] [INPUT]

For a calculation, brackets ( [ ] ) are required at all times.

• Rounding

Rounding operations are performed by using the key operations

described below. The result of a calculation is displayed at the cursor position of input data. (1) Rounding 1 (rounding off to an integer) : RND[1.234] [INPUT] (2) Rounding 2 (rounding off "a" to the decimal places

RND2[1.267,0.01] [INPUT]

(Note that for a calculation of rounding 2, a special format using

two arguments is required. Enter data according to the format RND[a,b]. The value of "a" is rounded off to the decimal places specified by "b". As "b", do not specify a value other than 1,

0.1, 0.01, and so forth.)

For a calculation, brackets ( [ ] ) are required at all times.

• Discarding

This operation discards all decimal places. A discarding

operation is performed by using the key operations described below. The result of a calculation is displayed at the cursor position of input data. (1) Discarding : FIX[1.234] [INPUT]

For a calculation, brackets ( [ ] ) are required at all times.

• Circle ratio

A circle ratio calculation is performed by using the key

operations described below. The circle ratio 3.14... is indicated. (1) Circle ratio : PAI [INPUT]

specified by "b") :

- 16 -

3.SETTING OF

B-64254EN/06 BASIC SCREEN AND OPERATIONS

COORDINATE SYSTEM

3 SETTING OF COORDINATE SYSTEM

TURN MATE i assumes the coordinate system shown below. It is necessary to set the workpiece coordinate system before operating the machine.

-X

-Z

Push the present position screen area on the Base Screen to display the workpiece coordinate system setting screen, shown below. The present position and the active tool number are displayed on the upper left side of the screen. On the right side of the screen, a data input area is displayed, and on the bottom left side of the screen, the guidance drawing for input items is displayed.

[SET] key

Workpiece coordinate system setting screen (X coordinate)

[RET] key

- 17 -

3. SETTING OF

COORDINATE SYSTEM

BASIC SCREEN AND OPERATIONS B-64254EN/06

[SET] key

Workpiece coordinate system setting screen (Z coordinate)

It is possible to decide on the origin of the workpiece coordinate system by following the procedure described below.

(1) To determine a standard plane, cut the side at a low feedrate,

using the handle.

(2) Retract the tool along the Z-axis only, not moving it along the

X-axis, then stop the spindle.

(3) Measure the diameter of the workpiece, assume this value as the

input value for X, and set it for the input item X. (4) Push the [SET] key. (5) The X coordinate of the present position shown on the upper left

side of the screen is replaced with the value entered in <3>.

(1) Bring the tool in contact with the workpiece face side, and

measure the Z coordinate. (2) Set the desired value for the input item Z. (3) Push the [SET] key. (4) The Z coordinate of the present position shown on the upper left

side of the screen is replaced with the value entered in <2>.

Example) If deciding on the origin of the workpiece coordinate system as

shown in the figure below

[RET] key

Workpiece origin

- 18 -

3.SETTING OF

B-64254EN/06 BASIC SCREEN AND OPERATIONS

(1) First cut the side and then retract the tool along the Z-axis.

Stop the spindle and measure the diameter of the workpiece.

(2) Enter the measured value (40.0) in the X coordinate data

COORDINATE SYSTEM

area, and push the [INPUT] (

) key.

(3) Push the [SET] key. (The X coordinate of the present

position is replaced with 40.0.)

(4) Bring the tool in contact with the workpiece side face.

(5) Enter the measured value (10.0) in the Z coordinate data

area, and push the [INPUT] (

) key.

(6) Push the [SET] key. (The Z coordinate of the present

position is replaced with 10.0.)

- 19 -

4. SETTING OF SPINDLE INFORMATION

BASIC SCREEN AND OPERATIONS B-64254EN/06

4 SETTING OF SPINDLE INFORMATION

It is necessary to set a spindle speed before operating the machine. Pushing the spindle speed screen area on the Base Screen causes the spindle speed setting screen to be displayed. There are three operations related to the spindle:

(1) Setting a spindle speed (/MIN). (2) Setting a surface speed (M/MIN or FEET/MIN) and a maximum

spindle speed (/MIN).

(3) Setting a gear number.

Each operation is described below. (Switch to the screen for each operation, with an appropriate tab operation.)

NOTE

If specifying a spindle speed on each cutting cycle

input screen, these operations are not required.

- 20 -

4.SETTING OF SPINDLE

B-64254EN/06 BASIC SCREEN AND OPERATIONS

INFORMATION

4.1 SETTING OF SPINDLE SPEED

Selecting the tab [CSS OFF] causes the screen shown below to appear. This screen is used to set a spindle speed (RPM(MIN constant surface speed control.

Tab [CSS OFF]

Tab [CSS ON]

-1

)) and disable

Tab [G-NO]

[SET] key

Spindle speed setting screen (tab [CSS OFF])

[RET] key

The procedure is as described below.

(1) In the S-SET data area, enter the desired spindle speed

-1

(RPM(MIN

)), and push the [INPUT] ( ) key.

(The message “KEY IN NUMERALS. (/MIN)” is displayed in the message space on the bottom left side of the screen).

(2) Push the [SET] key.

Pushing the [SET] key disables constant surface speed control, enabling the input spindle speed. (In the S area, the actual spindle speed in the CNC is displayed.)

- 21 -

4. SETTING OF SPINDLE INFORMATION

BASIC SCREEN AND OPERATIONS B-64254EN/06

4.2 SETTING OF SURFACE SPEED

Selecting the tab [CSS ON] causes the screen below to appear. This screen is used to set a surface speed (m/min) and enable constant surface speed control.

Spindle speed setting screen (tab [CSS ON])

The procedure is as described below.

(1) In the S-CSS data area, enter the desired surface speed (m/min),

Tab [CSS ON]

and push the [INPUT] (

) key. (The message "KEY IN

NUMERALS. M/MIN, FEET/MIN)" is displayed in the message space on the bottom left side of the screen.)

(2) In the S-MAX data area, enter a maximum spindle speed

(RPM(MIN

-1

)), and push the [INPUT] ( ) key.

(The message "KEY IN NUMERALS. M/MIN, FEET/MIN)" is displayed in the message space on the bottom left side of the screen.)

(3) Push the [SET] key.

Pushing the [SET] key enables constant surface speed control, enabling the input surface speed and maximum spindle speed. (In the S area, the actual spindle speed in the CNC is displayed.)

NOTE

Change the surface speed unit to (feet/min), using

inch/metric switching.

- 22 -

4.SETTING OF SPINDLE

B-64254EN/06 BASIC SCREEN AND OPERATIONS

INFORMATION

4.3 SETTING OF GEAR NUMBER

Selecting the tab [G-NO] causes the screen shown below to appear. This screen is used to specify a gear number (1 to 4). Buttons are displayed on the bottom left side of the screen, and by pushing a button (or selecting it with the button cursor), the corresponding gear number is set. Alternatively, a number can be set by entering it from the MDI keyboard.

Tab [G-NO]

Push one of them.

Spindle speed setting screen (tab [G-NO])

NOTE

1 Switch between display and non-display, using bit

6 of parameter No. 9102.

2 When setting a gear number, be sure to set

parameters Nos. 9115 to 9118 (M code to select a gear number).

- 23 -

4. SETTING OF SPINDLE INFORMATION

BASIC SCREEN AND OPERATIONS B-64254EN/06

4.4 SETTING OF SPINDLE SPEED USING BUTTON ON

MACHINE OPERATOR'S PANEL

By setting bit 5 of parameter No. 9103 to 1, it is possible to specify the value specified on the spindle speed setting screen to the CNC when pushing the spindle rotation button on the machine operator's panel. The procedure is as described below.

(1) On the spindle setting screen, enter a value and push the [SET]

key, and the entered value will be stored in memory. This value will be retained even after the power is turned OFF. (At this point, the value is not specified to the CNC.)

(2) Upon pushing the spindle rotation button on the machine

operator's panel, the value retained in (1) is specified to the CNC.

NOTE

This feature requires that the ladder program be

modified. For details, see A.5, "SPINDLE SPEED", in the Appendix (for machine tool builders).

- 24 -

5.SETTING OF TOOL

B-64254EN/06 BASIC SCREEN AND OPERATIONS

INFORMATION

5 SETTING OF TOOL INFORMATION

Pushing the tool number display area on the Base Screen causes the tool selection screen to appear. On the upper side of the screen, the currently selected tool number and tool offset data are displayed.

- 25 -

5. SETTING OF TOOL INFORMATION

BASIC SCREEN AND OPERATIONS B-64254EN/06

5.1 TOOL SELECTION

To enable tool offset, first push the button for the tool number to use and then push the [SET] key at the bottom of the screen. To set tool offset data, first push the button for the tool for which to set tool offset data and then push the [EDIT] key at the bottom of the screen to display the tool offset setting screen. On this screen, set and change tool offset data. To disable tool offset, push the [CAN] key at the bottom of the screen. This causes 0 to be displayed at the tool number on the upper side of the screen, disabling tool offset. To return to the Base Screen, push the [RET] key at the bottom of the screen. Pushing the [EDIT] key causes the tool offset setting screen for setting tool offset values to appear.

Cursor for selection

[SET] key [EDIT] key [CAN] key

Tool selection screen

NOTE

1 Up to 16 tools can be registered. 2 If the [SET] key is pushed, tool offset is

compensated for differently depending on the setting of NC parameter No. 5002.

3 On this screen, tool-nose radius compensation

cannot be applied.

4 This screen can be switched between display and

non-display, using bit 7 of parameter No. 9102.

[RET] key

- 26 -

5.SETTING OF TOOL

B-64254EN/06 BASIC SCREEN AND OPERATIONS

INFORMATION

5.2 INPUT OF TOOL OFFSET

Pushing the [EDIT] key on the tool selection screen causes the tool offset setting screen to appear. There are three tool offset setting operations:

(1) Direct input of tool offset (absolute command). (2) Direct input of tool offset (incremental command). (3) Measurement and input of tool offset.

Each operation is described below. (Switch to the screen for each operation, with an appropriate tab operation.)

5.2.1 Direct Input of Tool Offset

On this screen, the tabs [ABS] and [INC] enable direct input and editing of tool offset (radius of the tool nose, virtual tool tip, and offset).

Tab [ABS]

[SET] key

Tool offset setting screen (tab [ABS])

Tab [INC]

Tab [MES]

[RET] key

- 27 -

5. SETTING OF TOOL INFORMATION

BASIC SCREEN AND OPERATIONS B-64254EN/06

Tab [ABS]

[SET] key

Tool offset setting screen (tab [INC])

The procedure is as described below.

• For input with an absolute command

(1) To enter tool offset data with an absolute command, select

the tab [ABS].

(2) In the OFS_X and OFS_Z data areas, enter offset values,

Tab [INC]

Tab [MES]

[RET] key

and push the [INPUT] (

) key.

(3) Finally, push the [SET] key, and the values will be reflected

in the offset values.

• For input with an incremental command

(1) To enter tool offset data with an incremental command,

select the tab [INC].

(2) In the OFS_X+ and OFS_Z+ data areas, enter offset values,

and push the [INPUT] (

) key.

(3) Finally, push the [SET] key, and the values will be reflected

in the offset values.

NOTE

Offset values are reflected in tool geometry

compensation values.

- 28 -

5.SETTING OF TOOL

B-64254EN/06 BASIC SCREEN AND OPERATIONS

In the R data area, enter the desired radius value, and push the

INFORMATION

[INPUT] (

) key.

Finally, push the [SET] key, and the value is reflected in the

offset values.

[SET] key

Tool offset setting screen (itme "R")

[RET] key

In the TIP data area, enter the desired virtual toop tip position (1

to 9), and push the [INPUT] (

) key. Finally, push the

[SET] key, and the position will be reflected in the offset values.

[SET] key

Tool offset setting screen (item "TIP")

[RET] key

- 29 -

5. SETTING OF TOOL INFORMATION

BASIC SCREEN AND OPERATIONS B-64254EN/06

5.2.2 Measurement of Tool Offset

On this screen, the tab [MES] enables the tool offset values, X and Z coordinates, to be measured with the procedure described below.

[SET] key

Tool offset setting screen (X coordinate in the tab [MES])

[SET] key

Tool offset setting screen (Z coordinate in the tab [MES])

Tab [MES]

[RET] key

- 30 -

5.SETTING OF TOOL

B-64254EN/06 BASIC SCREEN AND OPERATIONS

The tool offset values, X and Z coordinates, can be measured with the procedure described below.

(1) Bring the tool in contact with the workpiece side face. (2) Measure the diameter of the workpiece, and set this value for the

input item X. (3) Push the [SET] key. (4) The X coordinate of tool offset on the bottom left side of the

screen will be updated with the value calculated as described

below. (Present value of the X coordinate in the absolute coordinate

system) - (Value entered in (2))

+ (Present offset value) = (Calculated value)

(1) Bring the tool in contact with the workpiece side face and

measure the Z coordinate. (2) Set the measured value for the input item Z. (3) Push the [SET] key. (4) The Z coordinate of tool offset on the bottom left side of the

screen will be updated with the value calculated as described

below. (Present value of the Z coordinate in the absolute coordinate

system) - (Value entered in (2))

+ (Present offset value) = (Calculated value)

INFORMATION

NOTE

If any of the offset values, the radius of the tool

nose, and the virtual toop tip position of the currently selected tool is changed on the tool offset setting screen, the tool is automatically re-selected. The operator need not, therefore, select the tool again after editing tool data.

Example) If setting tool offset as shown in the figure below

Workpiece origin

Present values : X=45.0 Z=15.0

Offset values : X=30.0 Z=5.0

- 31 -

5. SETTING OF TOOL INFORMATION

BASIC SCREEN AND OPERATIONS B-64254EN/06

(1) Bring the tool in contact with the workpiece side face, and

measure the diameter of the workpiece.

(2) Enter the measured value (40.0) in the X coordinate data

area, and push the [INPUT] (

) key.

(3) Push the [SET] key. Result: (Present value X 45.0) - (Entered value X 40.0) +

(Offset value X 30.0) = (Calculated value X 35.0)

(4) Then, bring the tool in contact with the workpiece side face.

(5) Enter the measured value (10.0) in the Z coordinate data

area, and push the [INPUT] (

) key.

Result: (Present value Z 15.0) - (Entered value Z 10.0) +

(Offset value X 5.0) = (Calculated value Z 10.0)

(6) Push the [SET] key.

- 32 -

B-64254EN/06 BASIC SCREEN AND OPERATIONS 6.ALARM CHECK

]

6 ALARM CHECK

On the Base Screen, pushing the alarm display area causes the alarm screen to appear.

Tab [ALARM]

Selecting the tab [ALARM] causes P/S alarms and external alarm messages to be displayed on the screen. Selecting the tab [MSG] causes operator messages to be displayed on the screen.

Alarm screen

Tab [MSG

[RET] key

- 33 -

III. MANUAL CUTTING

B-64254EN/06 MANUAL CUTTING 1.MANUAL CUTTING

1 MANUAL CUTTING

It is possible to move the tool freely to perform cutting, using the handle or the JOG switch.

The operation procedure is as described below.

Set the workpiece coordinate

system

Set a spindle speed

Select a tool

(Set an offset value)

Switch to the manual cutting

screen

Set a JOG feedrate (NOTE)

Operate with handle/JOG

switch

NOTE

1 By setting bits 2 and 1 of parameter No. 9103 to 1,

it is possible to set a JOG feedrate.

2 For cutting with the handle, it is not necessary to

set a JOG feedrate.

- 37 -

1.MANUAL CUTTING MANUAL CUTTING B-64254EN/06

Each operation is described below.

(1) Set the workpiece coordinate system

For details, see Chapter 3, "SETTING OF COORDINATE

SYSTEM", in Part II.

(2) Set a spindle speed

For details, see Chapter 4, "SETTING OF SPINDLE

INFORMATION", in Part II.

(3) Set a tool

Set a tool if required.

For details, see Chapter 5, "SETTING OF TOOL INFORMATION", in Part II.

(4) Switch to the manual cutting screen

On the Base Screen, push the soft key [HANDLE] to switch to

the manual cutting screen, shown below.

[RET] key

Manual cutting screen

- 38 -

B-64254EN/06 MANUAL CUTTING 1.MANUAL CUTTING

(5) Set a JOG feedrate

On the manual cutting screen, perform the following operation to

set a JOG feedrate: (1) Move the cursor to the input item "UNIT", and the buttons

[MIN (feed per minute)] and [REV (feed per revolution)] will be displayed and JOG feed mode will become selectable.

(2) If selecting [MIN (feed per minute)], enter the desired JOG

feedrate (mm/min or inch/min) in the "F-JOG" data area,

and push the [INPUT] (

be effective.

(3) Similarly, if selecting [REV (feed per revolution)], enter the

desired JOG feedrate (mm/rev or inch/rev) in the "F-JOG"

data area, and push the [INPUT] (

data will be effective.

Note that the data last entered is effective. If it is to be used, it

need not be set again.

) key. The entered data will

) key. The entered

CAUTION

To set a JOG feedrate, bit 4 of JOG feedrate

parameter No. 1402 and parameter No. 1423 are used. Thus, any previously specified value will be invalid on this screen. Screens other than this screen return to the original value, so that the existing JOG feedrate can be used.

(6) Cutting with the handle/JOG switch

On the manual cutting screen, move the tool to perform cutting,

using the handle or the JOG switch.

- 39 -

2. MANUAL CUTTING IN A LIMITED AREA

MANUAL CUTTING B-64254EN/06

2 MANUAL CUTTING IN LIMITED AREA

It is possible to move the tool in a limited area, using the handle or the JOG switch.

Prohibited area

The operation procedure is as described below.

Set the workpiece coordinate

system

Setting a spindle speed

Switch to the manual cutting

screen

Set a JOG feedrate (NOTE)

Set a limit area

(Set an offset value)

Select a tool

Operate with the handle/JOG

switch

NOTE

1 By setting bits 2 and 1 of parameter No. 9103 to 1,

it is possible to set a JOG feedrate.

2 For cutting with the handle, it is not necessary to

set a JOG feedrate.

- 40 -

2.MANUAL CUTTING IN

B-64254EN/06 MANUAL CUTTING

Each operation is described below.

(1) Set the workpiece coordinate system

For details, see Chapter 3, "SETTING OF COORDINATE

SYSTEM", in Part II.

(2) Set a spindle speed

For details, see Chapter 4, "SETTING OF SPINDLE

INFORMATION", in Part II.

(3) Set a tool

Set a tool if required.

For details, see Chapter 5, "SETTING OF TOOL INFORMATION", in Part II.

(4) Switch to the manual cutting screen

On the Base Screen, push the soft key [HANDLE] to switch to

the manual cutting screen, shown below.

(5) Set a JOG feedrate

Same as "Set a JOG feedrate" in the preceding chapter, Chapter 1,

"MANUAL CUTTING".

(6) Set a limit area

On the manual cutting screen, a tool movement range (rectangle)

can be set using the handle or the JOG switch. Depending on the settings of bits 2 and 1 of parameter No. 9103, either of the two operation procedures on the subsequent pages is possible.

LIMITED ARE

- 41 -

2. MANUAL CUTTING IN A LIMITED AREA

MANUAL CUTTING B-64254EN/06

Manual cutting screen (1)

It is possible to set a tool movement range with the procedure below.

(1) Move the cursor to the input item "LIMT", and the buttons [ON

(enable)] and [OFF (disable)] will be displayed on the left side of the screen, so that a prohibited area can be enabled or disabled.

(2) Enter the tool movement range on the X-axis (X coordinate) in

[RET] key

the input item [-X] or [+X] and push the [INPUT] (

) key,

and the input data will be reflected in the prohibited area. If the tool attempts to move into the prohibited area, an alarm will be displayed and a deceleration stop is made. If the tool enters the prohibited area, causing an alarm, the tool can move only in the direction opposite to the direction in which it has been moved.

(3) Similarly, enter the tool movement range on the Z-axis (Z

coordinate) in the input item [-Z] or [+Z] and push the [INPUT]

) key, and the input data will be reflected in the prohibited

(

area.

(4) Pressing the [RET] key returns the system to the Base Screen,

canceling the prohibited area.

Note that on this screen, the data last entered is effective. If it is to be used, it need not be set again.

- 42 -

2.MANUAL CUTTING IN

B-64254EN/06 MANUAL CUTTING

[CLR] key

Manual cutting screen (2)

[SET] key

It is possible to set a tool movement range with the procedure below.

(1) Enter the tool movement range on the X-axis (X coordinates) in

the input items [-X] and [+X] and the tool movement range on the Z-axis (Z coordinates) in the input items [-Z] and [+Z].

(2) Push the [SET] key, and the entered data will be set on the

bottom left side of the screen and the prohibited area will be enabled.

If the tool attempts to move into the prohibited area, an alarm

will be displayed and a deceleration stop is made. If the tool enters the prohibited area, causing an alarm, the tool can move only in the direction opposite to the direction in which it has been moved.

(3) Pushing the [CLR] key causes the entered data, shown on the

bottom left side of the screen to be cleared (replaced with blanks), disabling the prohibited area.

(4) Pushing the [RET] key causes the entered data to be initialized,

returning the system to the Base Screen and canceling the prohibited area.

LIMITED ARE

[RET] key

CAUTION

To set a limited area, stored stroke limit 2 (bit 0 of

parameter No. 1300, bit 0 of parameter No. 1310, parameter No. 1322, and parameter No. 1323) is used. Thus, any previously specified value will be invalid on the manual cutting screen. Screens other than the manual cutting screen return to the original value, so that existing stored stroke limit 2 can be used.

- 43 -

2. MANUAL CUTTING IN A LIMITED AREA

MANUAL CUTTING B-64254EN/06

(7) Cutting with the handle/JOG switch

On the manual cutting screen, move the tool to perform cutting,

using the handle or a JOG switch.

- 44 -

IV. CUTTING CYCLE

B-64254EN/06 CUTTING CYCLE 1.OUTLINE

1 OUTLINE

This chapter consists of the following sections.

1.1 WHAT’S CUTTING CYCLE ? .................................................47

1.2 CUTTING METHODS ..............................................................49

- 47 -

1.OUTLINE CUTTING CYCLE B-64254EN/06

1.1 WHAT’S CUTTING CYCLE ?

A "cutting cycle" is a predefined group of tool cutting motions for workpiece machining. By pressing the start button, you can have TURN MATE i execute a series of tool cutting motions.

TURN MATE i uses patterns of machining profiles that frequently appear in drawings in order to reduce the workload involved in figure input. The following cutting cycles are available.

(1) Rectangular cycle (2) Chamfer cycle (3) Taper cycle (4) Radius cycle (5) Face cycle (6) Free figure cycle (7) Thread cycle (thread/thread repair) (8) Groove cycle (9) Hole cycle (drill/tap)

(4)

(1)

(2)

(3)

(5)

Cutting cycle selection screen

(6)

(7)

(8)

(9)

- 48 -

B-64254EN/06 CUTTING CYCLE 1.OUTLINE

1.2 CUTTING METHODS

The following two types of cutting cycles are available - cutting cycle with automatic in-feeding and cutting cycle with manual in-feeding one of which may be chosen depending on the cutting depth "D-CUT" value.

(1) Cutting cycle with automatic in-feeding (D-CUT > 0)

This method enables automatic execution of a cutting cycle

(rough cutting/finish cutting) from the cutting start position. In rough cutting, the area to be cut differs depending on the position of the tool. (a) Entire area cutting cycle with automatic in-feeding (rough

cutting)

The entire area of the workpiece is cut.

(b) Partial area cutting cycle with automatic in-feeding (rough

cutting)

If the tool is positioned halfway through the cutting area,

the cutting starts at the current tool position.

Cutting start point

Execution

Cutting start point

Execution

Cutting start point

Execution

- 49 -

1.OUTLINE CUTTING CYCLE B-64254EN/06

(2) Cutting cycle with manual in-feeding (D-CUT=0)

A single in-feed cutting can be executed. This methos allows the

operator to control the cutting depth manually for each cutting motion.

Cutting start point

Execution

- 50 -

B-64254EN/06 CUTTING CYCLE 2.OPERATION

2 OPERATION

This chapter consists of the following sections.

2.1 WORKFLOW.............................................................................52

2.2 SETTING THE FEEDRATE .....................................................54

2.3 CREATING NEW CUTTING CYCLE .....................................55

2.4 EDITING CUTTING CYCLE ...................................................58

2.5 SELECTING CUTTING CYCLE..............................................59

2.6 DELETING CUTTING CYCLE................................................61

2.7 NOTES .......................................................................................63

2.7.1 Inhibition of Operation........................................................63

2.7.2 Manual Intervention during Cutting Cycles........................63

2.7.3 Tool Nose Radius Compensation ........................................63

- 51 -

2.OPERATION CUTTING CYCLE B-64254EN/06

2.1 WORKFLOW

The workflow of a cutting cycle is as follows.

Setting of workpiece

coordinate system

Setting of spindle speed

Setting of feedrate

Selection of tool

(Setting of offset)

Input of cutting cycle data

Pressing of cycle start

button

D-CUT>0

Yes

Cutting cycle with

automatic in-feeding

Cutting cycle with manual

in-feeding

- 52 -

B-64254EN/06 CUTTING CYCLE 2.OPERATION

Each step of the workflow is described below.

(1) Setting of workpiece coordinate system

For details, see Part II, Chapter 3, "SETTING OF

COORDINATE SYSTEM".

(2) Setting of spindle speed

For details, see Part II, Chapter 4, " SETTING OF SPINDLE

INFORMATION".

(3) Setting of feedrate

For details, see Section 2.2, "SETTING THE FEEDRATE".

(4) Selection of tool

If necessary, set the tool.

For details, see Part II, Chapter 5, " SETTING OF TOOL INFORMATION".

(5) Input of cutting cycle data

For details, see Sections 2.3 to 2.6.

(6) Pressing of cycle start

Press the cycle start button on the machine operator's panel.

The created cutting cycle is executed to cut the workpiece.

- 53 -

2.OPERATION CUTTING CYCLE B-64254EN/06

2.2 SETTING THE FEEDRATE

It is necessary to set the feedrate before executing any cutting cycle. If you push the feedrate display area on the base screen, the feedrate setting screen is displayed.

[SET] key

Feedrate setting screen

The operation method is as follows.

(1) Input the desired federate of the cutting cycle (mm/rev or

inch/rev) into the data area of F-SET, then push the [INPUT]

[RET] key

) key.

(

(2) Push the [SET] key. (3) When the setting is done, the specified value of the feedrate

appears in the display area in the upper left side of the screen.

(The value displayed next to F in the upper left side represents

the CNC-specified feedrate modal data.)

NOTE

1 The unit of the federate can be in mm/rev or

inch/rev.

2 If the feedrate is specified in the input data screen

of each cutting cycle, then it is not necessary to set the feedrate on the feedrate setting screen.

- 54 -

B-64254EN/06 CUTTING CYCLE 2.OPERATION

2.3 CREATING A NEW CUTTING CYCLE

The workflow to create a new cutting cycle is described below.

(1) Push the guidance drawing on the base screen to display the

cutting cycle selection screen.

(2) To select the desired cycle menu, push the corresponding

drawing on the cutting cycle selection screen (CYCLE tab).

(3) To select the desired cycle, push the corresponding drawing on

the cutting cycle selection screen (DETAIL tab).

(4) When the cycle input data screen (NOTE) is displayed, fill in the

necessary data.

(5) Push the [SAVE] key to save the data and to return to the base

screen.

NOTE

The layout of the cycle input data screen is as

follows.

- 55 -

2.OPERATION CUTTING CYCLE B-64254EN/06

(1) Current

position

(2) Guidance

drawing

(7) [CLEAR] key for data

initialization

(3) [FIG.] tab

(5) [SAVE] key for data

saving

Cycle input data screen

[METH.] tab

[COND.] tab

(4) Cycle data

(6) [CAN] key for data

cancellation

(1) Current position The current position is indicated in the same way as in the base

screen.

(2) Guidance drawing In this area of the screen, the guidance drawing of the selected

cutting cycle is displayed. A selection button may be presented depending on the input data item. When a button is displayed, press the button on the touch panel or select it with the button cursor, and then input data.

(3) Tabs The following 3 tabs - [FIG.], [METH.], and [COND.] - are

provided. Each tab has its own input data items for the cutting cycle. [FIG.] : Input data items related to geometry (positions,

dimenstions, etc.)

[METH.] : Input data items related to the cutting method

(cutting direction, finishing amount, etc.)

[COND.] : Input data items related to the cutting conditions

(spindle speed, feedrate, etc.)

(4) Cycle data This area of the screen displays the data items you need to input

to execute the cutting cycle and the fields for inputting the data. An unnecessary item has an asterisk (*) to the right of its data input field.

- 56 -

B-64254EN/06 CUTTING CYCLE 2.OPERATION

(5) Soft key for data saving [SAVE] If you enter necessary data in the data input field and push the

[INPUT] (

) key, the input of the data is confirmed. After

that, push the [SAVE] key to save the input data to memory and to return to the base screen.

(6) Soft key for data cancellation [CAN] Push the [CAN] key to cancel the input of the data and to return

to the base screen.

(7) Soft key for data initialization [CLEAR] Push the [CLEAR] key to clear the input data and to return to the

base screen.

- 57 -

2.OPERATION CUTTING CYCLE B-64254EN/06

2.4 EDITING A CUTTING CYCLE

The workflow to edit a cutting cycle is described below.

(1) Push the cycle data area on the base screen to display the input

data screen for the cutting cycle.

(2) In the cycle input data screen, edit the data as necessary.

(3) Push the [SAVE] key to save the data and to return to the base

screen.

- 58 -

B-64254EN/06 CUTTING CYCLE 2.OPERATION

2.5 SELECTING A CUTTING CYCLE

The workflow to select a cutting cycle is described below.

(1) Push the cycle memory position number display area on the base

screen to display the cycle memory position screen (NOTE).

(2) Select a cycle memory position number by pushing the cycle

memory position button or moving the cursor with the [↑][↓][←][→] keys.

(In the example at the left, cycle memory position number 9, thread cutting, is selected.)

The content of the selected cutting cycle is displayed at the

bottom of the screen.

(3) Push the [SELECT] key to return to the base screen, where the

cutting cycle you select in (2) will be selected.

Remark) You can also select a cutting cycle by using the cycle memory

position soft keys [←] and [→] on the base screen.

NOTE

The layout of the cycle memory position screen is

as shown on the next page.

- 59 -

2.OPERATION CUTTING CYCLE B-64254EN/06

(1) Cycle memory

position button

(2) Cycle name

and cutting condition

(3) Input buffer

(4) [SELECT] key for

cycle selection

Cycle memory position screen

(1) Cycle memory position button There are 40 buttons. If you push a desired button, the specified

(2) Cycle name and cutting condition display This area displays the cycle name and cutting condition of the

The cycle name and cutting condition are not displayed if there is

(3) Input buffer This area displays the numerical values that are input with the

(4) Cycle selection soft key Push the [SELECT] key to select the specified cutting cycle and

(5) Cycle deletion soft key Push the [DEL] key to delete the specified cutting cycle and to

(6) Return soft key Push the [RET] key to return to the base screen.

(5) [DEL] key for cycle

deletion

(6) [RET] key for

returning

cutting cycle is called and the base screen is displayed. The icon which represents the type of the stored cycle is displayed on the button. The icon is not displayed on the button if there is no cycle.

cycle highlighted by the cursor.

no cycle.

MDI key. This area is used to delete multiple cutting cycles.

to return to the base screen.

clear the icon from the cycle memory position button.

- 60 -

B-64254EN/06 CUTTING CYCLE 2.OPERATION

2.6 DELETING A CUTTING CYCLE

The workflow to delete a cutting cycle is described below.

(1) Push the cycle memory position number display area on the base

screen to display the cycle memory position screen.

(2) Specify the cutting cycle you want to delete. There are two

methods to specify a cutting cycle, as described below. (The example at the left uses the method of (b).) (a) Pressing the cycle memory position button of the cycle to

be deleted The cutting cycle corresponding to the pressed button is specified. No more than one cycle can be specified.

(b) Inputting the cycle memory position number of the cycle to

be deleted, by using the MDI keys (NOTE) One or more cutting cycles can be specified. Using the MDI keys, input the cycle memory position number of each cycle to be deleted in the input buffer field.

(3) Pushing the [DEL] soft key displays the deletion confirmation

window. In addition, the buttons of the specified cycle memory position numbers are displayed in dark gray.

(4) If the [YES] soft key is pressed, the deletion confirmation

window closes and the data of the specified cycles are deleted, clearing the icons from the cycle memory position buttons.

(Pushing the [NO] soft key closes the deletion confirmation

window without deleting any cutting cycle data.)

- 61 -

2.OPERATION CUTTING CYCLE B-64254EN/06

NOTE

When you input cycle numbers in the input buffer

field using the MDI keys, the input format is as follows.

(1) No input If nothing is input in the input buffer, then the cycle on

which the cursor is currently positioned is selected.

(2) Specification of one cycle number Format : X If a number (X) is input, the cycle at position "X" is

selected.

(3) Specification of multiple cycles Format : X1, X2, ... If two or more numbers (X1, X2, ...) are input, each

delimited by a comma, the cycles at positions "X1", "X2", etc. are selected.

(4) Range specification Format : XS-XE If two numbers are input, concatenated with a hyphen, the

cycles from positions "XS" to "XE" are selected.

(5) Combination of multiple specification and range

specification Format : X1, X2, XS-XE It is also possible to combine the selection of multiple

cycles with the selection of a range of cycles.

(6) Input other than the above mentioned If any invalid characters, such as non-alphabetic letters,

numbers outside the 1-40 range, and signs other than

commas and hyphens, are input, the message "INPUT

VALUE IS NOT CORRECT" is displayed.

- 62 -

B-64254EN/06 CUTTING CYCLE 2.OPERATION

2.7 NOTES

Before operating TURN MATE i, carefully read the following notes on cutting cycles.

2.7.1 Inhibition of Operation

If a program is running on the NC side when you switch to the TURN MATE i screen, you cannot set data for TURN MATE i or execute a cutting cycle. For safety reasons, the operation of TURN MATE i is prohibited in any of the following conditions:

(1) PMC signal OP is on. (2) PMC signal SPL is on. (3) PMC signal AL is on. (4) An operator message is displayed.

2.7.2 Manual Intervention during Cutting Cycles

You cannot stop an ongoing cutting cycle and execute manual intervention.

WARNING

Executing manual intervention during a cutting

cycle can lead to unexpected behavior of the system. That may cause the tool to collide with the workpiece or machine, potentially injuring the user and/or damaging the equipment.

2.7.3 Tool Nose Radius Compensation

The tool path of TURN MATE i is generated based on a compensated value (tool nose radius) that takes into account the roundness of the tool nose. Therefore, the tool nose radius compensation command (G41 or G42) cannot be executed during a cutting cycle.

WARNING

If the tool nose radius compensation command

(G41 or G42) is specified before a cutting cycle, TURN MATE i cancels it automatically (G40) when the cycle begins.

- 63 -

3.FACE CYCLE CUTTING CYCLE B-64254EN/06

3 FACE CYCLE

This chapter consists of the following sections.

3.1 OUTLINE...................................................................................65

3.2 TOOL CUTTING MOTIONS....................................................66

3.3 INPUT DATA ............................................................................69

- 64 -

B-64254EN/06 CUTTING CYCLE 3.FACE CYCLE

3.1 OUTLINE

The face cycle is characterized by the following properties.

(1) Rough cutting where turning is done on a face figure in the -X

axis direction

(2) The face area to cut is defined by an cutting end point (X and Z),

cutting start point (X), and cutting clearance.

(3) When the input value of D-CUT is 0, it is possible to machine by

manual in-feeding (a single in-feed machining by the tool).

(4) When the input value of D-CUT is larger than 0, it is possible to

machine by automatic in-feeding (the cutting cycle begins at the cutting start point).

(5) It is possible to change the tool number, feedrate, and spindle

speed, which are set in the spindle speed setting screen, feedrate setting screen, and tool selection screen, respectively.

Clearance

Cutting end point

Workpiece

Cutting area

Cutting start point X coordinate

- 65 -

3.FACE CYCLE CUTTING CYCLE B-64254EN/06

3.2 TOOL CUTTING MOTIONS

1. Determining the Cutting Cycle Based on the Tool Position

Shown below is the relationship between the tool cutting motions and the figure and the tool position at the time cycle start is pressed.

Cutting not possible

[A]

Cutting not possible

[D]

Clearance

Cutting possible

[G]

2. Cutting Cycle with Manual In-Feeding (D-CUT=0) (When the Tool Is Positioned in [H])

(1) The tool moves from the current position in cutting feedrate in

the X axis direction until the edge of the programmed figure is reached.

(2) The tool retracts in cutting feedrate in the XZ axis direction by

the escape amount (specified in parameter No. 9212).

(3) The tool returns to the initial position in rapid traverse in the X

axis direction and then stops.

Cutting not possible

[B]

Possible only with the cutting cycle with manual in-feeding

[E]

Cutting possible

[H]

Cutting possible

[C]

Cutting possible

[F]

Cutting possible

[I]

Final fi

ure

Current tool position

- 66 -

B-64254EN/06 CUTTING CYCLE 3.FACE CYCLE

3. Entire Area Cutting Cycle with Automatic In-Feeding (D-CUT>0) (When the Tool Is Positioned in [C], [F], [G], or [I])

(1) The tool moves to the cutting start point in rapid traverse, first in

the X axis direction and then in the Z axis direction.

Steps (2) and (3) are the same as the cutting cycle with manual

in-feeding.

(4) The tool moves in the axis direction in rapid traverse by the

depth of cut (D-CUT). (5) Steps (2) to (4) are repeated until the final cut surface is reached. After the final in-feed machining, the tool retracts in the XZ axis

direction by the escape amount (specified in parameter No. 9212)

and then moves in rapid traverse by the Z_max+Z axis clearance. (6) The tool returns to the initial position in rapid traverse, first in

the X axis direction and then in the Z axis direction, and then

stops.

Z axis direction clearance

X axis direction clearance

D-CUTD-CUT

- 67 -

3.FACE CYCLE CUTTING CYCLE B-64254EN/06

4. Partial Area Cutting Cycle with Automatic In-Feeding (D-CUT>0) (When the Tool Is Positioned in [H])

(1) The tool moves to the cutting start point in rapid traverse in the X

axis direction. Steps (2) to (6) are the same as the cutting cycle with automatic in-feeding.

X axis direction clearance

Z axis direction clearance

D-CUT

- 68 -

B-64254EN/06 CUTTING CYCLE 3.FACE CYCLE

3.3 INPUT DATA

If face cycle is selected in the cutting cycle selection screen, the cycle input data screen is displayed as follows.

The items to input are listed below.

Item Meaning Tab Mandatory Note

X0 X coordinate of the cutting

start point

X X coordinate of the cutting

end point

Z Z coordinate of the cutting

end point

E Width of the area to cut FIG.

D-CUT Depth of cut FIG.

XA X coordinate of the approach

position

ZA Z coordinate of the approach

position T Tool number COND. F Feedrate COND.

CSS Specify constant surface

speed with the button on the

touch panel.

[ON] : Disable (1)

[OFF] : Enable (2) S Spindle speed COND.

S-MAX Maximum spindle speed COND.

S-DIR Spindle rotation direction

[NORMAL] : Normal (1)

[REVERSE] : Reverse (2) G Specify the gear number with

the button on the touch panel.

FIG.

METH.

COND.

○

○ ○ ×

× × ×

× ×

Absolute coordinate

Absolute coordinate (NOTE)

Absolute coordinate

Displayed only when parameter No. 9202#2 = 1.

There is no default. There is no default. There is no default.

There is no default. Displayed only when CCS = 1. There is no default. The default is 1 (NORMAL). Displayed only when parameter No. 9202#1 = 1. Refer to parameter Nos. 9213, 9214, and 9215. The value range is 1 to 4; there is no default.

- 69 -

3.FACE CYCLE CUTTING CYCLE B-64254EN/06

NOTE

By enabling the optional function and the

parameter shown below, you can input a negative value for the cutting end point (X).

• Optional function: Cutting cycle extension

• Parameter: No. 9203 #1 (SFC) = 1

When the above optional function and parameter

are enabled, 0 is always assumed for the virtual tool nose position and radius when generating the tool path. Since the X coordinate range check is not made, make sure that the negative value you input is smaller than the tool nose radius.

- 70 -

B-64254EN/06 CUTTING CYCLE 4.CHAMFER CYCLE

4 CHAMFER CYCLE

This chapter consists of the following sections.

4.1 OUTLINE...................................................................................72

4.2 TOOL CUTTING MOTIONS....................................................74

4.3 INPUT DATA ............................................................................81

- 71 -

4.CHAMFER CYCLE CUTTING CYCLE B-64254EN/06

4.1 OUTLINE

There are three types of chamfer cycle - outer face chamfer, outer back chamfer, and inner chamfer. The chamfer cycle is characterized by the following properties.

(1) Cutting where the tool is turned along the outside of the figure

that can be defined by the corner coordinates and the corner

rounding (arc) or corner chamfering (2) Either rounding (arc) or chamfering can be set for the corner. (3) Rough cutting can be done along the final figure (corner

rounding or chamfering). (4) When the input value of D-CUT is 0, it is possible to machine by

manual in-feeding (a single in-feed machining by the tool). (5) When the input value of D-CUT is larger than 0, it is possible to

machine by automatic in-feeding (the cutting cycle begins at the

cutting start point). (6) It is possible to change the tool number, feedrate, and spindle

speed, which are set in the spindle speed setting screen, feedrate

setting screen, and tool selection screen, respectively.

- 72 -

B-64254EN/06 CUTTING CYCLE 4.CHAMFER CYCLE

Outer face chamfer R/chamfer C

Workpiece

R/C

45°

Corner coordinates

Outer back chamfer R/chamfer C

Inner chamfer R/chamfer C

R/C

Corner coordinates

Workpiece

45°

Workpiece

Corner coordinates

45°

R/C

- 73 -

4.CHAMFER CYCLE CUTTING CYCLE B-64254EN/06

4.2 TOOL CUTTING MOTIONS

There are six types of chamfer cutting. However, since the tool cutting motion of each cycle is identical except that the cutting area is symmetrical horizontally (outer face chamfer and outer back chamfer) or vertically (outer face chamfer and inner chamfer), this section describes the outer chamfer C cycle as an example.

1. Determining the Cutting Cycle Based on the Tool Position

Shown below is the relationship between the tool cutting motions and the figure and the tool position at the time cycle start is pressed. In the case of a cutting cycle with manual in-feeding, 0 is specified for the depth of cut and the tool moves to [C] or [F] before the cycle starts. If the cycle starts with a value specified for the depth of cut and the tool moved to [F], automatic cutting is performed from the current position (halfway through the cutting area).

Cutting not

ossible

[A]

Cutting not

Cutting

ossible

[B]

Cutting

ossible

[C]

[D]

Cutting not

possible

Cutting

ossible

[G]

Cutting not

ossible

Cutting

ossible

[H]

Cutting

ossible

[F]

[E]

Cutting

ossible

[I]

- 74 -

B-64254EN/06 CUTTING CYCLE 4.CHAMFER CYCLE

2. Cutting Cycle with Manual In-Feeding (D-CUT=0) (When the Tool Is Positioned in [E] or [F])

(1) The tool moves from the cutting start point in cutting feedrate in

the Z axis direction until position (XS, Z) is reached.

(2) The tool moves in cutting feedrate along the input figure until

position (X, Zn) is reached.

(3) The tool moves in cutting feedrate in the X axis direction over

the distance equal to clearance.

(4) The tool returns to the initial position in rapid traverse, first in

the Z axis direction and then in the X axis direction, and then stops.

Clearance

(2)

(X, Zn)

(3)

(X, Zn) (X, Z)

(3)

Clearance

(X, Z)

Clearance

(2)

(1)

(4)

(1)

(4)

(XS, ZS)

(4)

(XS, ZS)

(4)

- 75 -

4.CHAMFER CYCLE CUTTING CYCLE B-64254EN/06

3. Cutting Cycle with Manual In-Feeding (D-CUT=0)

(When the Tool Is Positioned in [C])

(1) The tool moves from the cutting start point in rapid traverse until

position (Xm, ZS) is reached.

(2) The tool moves in cutting feedrate in the Z axis direction until

position (Xm, Z) is reached.

(3) The tool moves in cutting feedrate along the input final figure

until position (X, Zm) is reached. In the case of corner rounding, overcutting is done in the -Z axis direction.

(4) The tool moves in cutting feedrate in the X axis direction over

the distance equal to clearance.

(5) The tool returns to the initial position in rapid traverse, first in

the Z axis direction and then in the X axis direction, and then stops.

(3)

Clearance

(X, Zm)

(4)

(3)

Clearance

(4)

Overcut

(XS, ZS)

(1)

(Xm, Z)

(2)

(5)

(X, Z)

(5)

(XS,ZS)

(1)

(2)

(5)

(3)

(X, Z) (X, Zm)

(5)

- 76 -

B-64254EN/06 CUTTING CYCLE 4.CHAMFER CYCLE

4. Entire Area Cutting Cycle with Automatic In-Feeding (D-CUT>0) (When the Tool Is Positioned in [C], [G], [H], or [I])

(1) The tool moves from the cutting start point in rapid traverse, first

in the Z axis direction and then in the X axis direction, until position (XS, ZS) is reached.

(2) The tool moves in cutting feedrate in the Z axis direction until

position (XS, Z) is reached.

(3) The tool moves in cutting feedrate along the input figure until

position (X, Zn) is reached.

(4) The tool moves in cutting feedrate in the X axis direction over

the distance equal to clearance.

(5) The tool moves in rapid traverse in the Z axis direction until

position ZS is reached and then in the X axis direction until position XS is reached.

(6) Then, the tool moves in cutting feedrate in the X axis direction

by the depth of cut (D-CUT).

(7) Then, steps (2) to (6) are repeated until one of the following

points is reached: In the case of corner chamfer: (X-C, Z-C) In the case of corner rounding: (X-R, Z-R); overcut when the final figure is cut (the depth of overcut is specified by parameter No. 9212).

- 77 -

4.CHAMFER CYCLE CUTTING CYCLE B-64254EN/06

(1)

(8) The tool returns to the initial position in rapid traverse, first in

the Z axis direction and then in the X axis direction, and then stops.

Clearance

(X, Zn)

Clearance

(8)

(X, Zn)

Clearance

(X, Z)

(4)

(5)

Clearance

(X, Z)

(4)

(5)

(6)

(XS, ZS) (2) (3)

(1)

(5)

(6)

(XS, ZS) (2) (3)

(5)

(7)

(1)

(7)

(1)

D-CUT

(8)

D-CUT

(8)

Overcut

(8)

- 78 -

B-64254EN/06 CUTTING CYCLE 4.CHAMFER CYCLE

5. Partial Area Cutting Cycle with Automatic In-Feeding (D-CUT>0)

(When the Tool Is Positioned in [F])

(1) The tool moves from the cutting start point in rapid traverse in

the Z axis direction until position (XS, ZS) is reached.

(2) The tool moves in cutting feedrate in the Z axis direction until

position (XS, Z) is reached.

(3) The tool moves in cutting feedrate along the input figure until

position (X, Zn) is reached.

(4) The tool moves in cutting feedrate in the X axis direction over

the distance equal to clearance.

(5) The tool moves in rapid traverse in the Z axis direction until

position ZS is reached and then in the X axis direction until position XS is reached.

(6) Then, the tool moves in cutting feedrate in the X axis direction

by the depth of cut (D-CUT).

(7) Then, steps (2) to (6) are repeated until one of the following

points is reached: In the case of corner chamfer: (X-C, Z-C) In the case of corner rounding: (X-R, Z-R); overcut when the final figure is cut.

- 79 -

4.CHAMFER CYCLE CUTTING CYCLE B-64254EN/06

(8) The tool returns to the initial position in rapid traverse, first in

the Z axis direction and then in the X axis direction, and then stops.

Clearance

(X, Zn) (X, Z)

(4) (5)

(8)

Clearance

(3)

Clearance

(6)

(2)

(XS, ZS)

(5)

(6)

(2)

(XS, ZS)

(7)

D-CUT

(1)

(8)

(7)

D-CUT

(1)

Clearance

Overcut

(3)

(X, Zn) (X, Z)

(4)

(8)

(5)

(8)

- 80 -

B-64254EN/06 CUTTING CYCLE 4.CHAMFER CYCLE

4.3 INPUT DATA

There are six types of chamfer cutting. However, since the input data screen of each cycle is identical except for the guidance drawings, this section describes the input data screen for the outer chamfer C cycle as an example.

The items to input are listed below.

Item Meaning Tab Mandatory Note

X X coordinate of the corner FIG. Z Z coordinate of the corner FIG.

R/C Corner rounding radius/amount

of chamfering

D-CUT Depth of cut FIG.

XA X coordinate of the approach

position

ZA Z coordinate of the approach

position T Tool number COND. F Feedrate COND.

CSS Specify constant surface speed

with the button on the touch

panel.

[ON]: Disable (1)

[OFF]: Enable (2) S Spindle speed COND.

S-MAX Maximum spindle speed COND.

S-DIR Spindle rotation direction

[NORMAL] : Normal (1)

[REVERSE] : Reverse (2)

G Specify the gear number with

the button on the touch panel.

FIG.

METH.

COND.

○ ○ ○

○ ×

× × ×

× ×

Absolute coordinate Absolute coordinate There is no default.

Displayed only when parameter No. 9202#2 = 1.

There is no default. There is no default. There is no default.

- 81 -

5.RECTANGULAR CYCLE CUTTING CYCLE B-64254EN/06

5 RECTANGULAR CYCLE

This chapter consists of the following sections.

5.1 OUTLINE...................................................................................83

5.2 TOOL CUTTING MOTIONS....................................................85

5.2.1 Rough Cutting Motions.......................................................85

5.2.2 Finish Cutting Motions........................................................93

5.3 INPUT DATA ............................................................................98

- 82 -

B-64254EN/06 CUTTING CYCLE 5.RECTANGULAR CYCLE

5.1 OUTLINE

There are three types of rectangular cycle - outer, inner, and outer back. The rectangular cycle is characterized by the following properties.

(1) Cutting where the tool is turned along the inside of the rectangle

(specified by the coordinate values of 2 points) (2) Either rounding (arc) or chamfering can be set for the corner. (3) The turning direction can be selected from -Z, +Z, +X, and -X. (4) Rough cutting is possible allowing the tool to move in parallel

with the Z axis (X axis). (5) Finishing cutting is possible allowing the tool to move

counterclockwise along the final figure. (6) When the input value of D-CUT is 0, it is possible to machine by

manual in-feeding (a single in-feed machining by the tool). (7) When the input value of D-CUT is larger than 0, it is possible to

machine by automatic in-feeding (the cutting cycle including

rough or finishing cutting begins at the cutting start point). (8) It is possible to change the tool number, feedrate, and spindle

speed, which are set in the spindle speed setting screen, feedrate

setting screen, and tool selection screen.

CAIUTION

For the outer rectangular cycle, the figure must be

increasing monotonously. For the outer back or inner rectangular cycle, the figure must be decreasing monotonously.

- 83 -

5.RECTANGULAR CYCLE CUTTING CYCLE B-64254EN/06

Outer rectangular/rectangular R/rectangular C

Workpiece

Corner

2nd point

Cutting area

Outer back rectangular/rectangular R/rectangular C

Workpiece

1st point

Cutting area

Corner

2nd point

Inner rectangular/rectangular R/rectangular C

2nd point

1st point

Corner

Workpiece

Cutting area

1st point

- 84 -

B-64254EN/06 CUTTING CYCLE 5.RECTANGULAR CYCLE

5.2 TOOL CUTTING MOTIONS

There are nine types of rectangular cutting. However, since the tool cutting motion of each cycle is identical except that the cutting area is symmetrical horizontally (outer and outer back) or vertically (outer and inner), this section describes the outer rectangular C cycle as an example.

5.2.1 Rough Cutting Motions

1. Determining the Cutting Cycle Based on the Tool Position

NOTE

If a cutting cycle with manual in-feeding starts from

[C], [G], or [I], only the final figure is cut once.

Z direction cutting

Clearance

Cutting not

ossible

[A]

Cutting not

ossible

[D] [F]

Cutting possible

[G]

Cutting not

ossible

[B]

Possible only with the cutting cycle with manual in-feeding

[E]

Cutting possible

[H]

Cutting possible

[C]

Cutting possible

[I]

- 85 -

5.RECTANGULAR CYCLE CUTTING CYCLE B-64254EN/06

X direction cutting

Cutting not possible

[A]

Cutting not possible

[B]

Cutting possible

[C]

Cutting possible

Clearance

Cutting not

ossible

[D] [F]

Possible only with the cutting cycle with manual in-feeding

[E]

Cutting possible

[I]

[G]

Cutting possible

[H]

2. Cutting Cycle with Manual In-Feeding (D-CUT=0) in the Z Direction (When the Tool Is Positioned in [E] or [F])

(1) The tool moves from the current position (cutting start point) in

cutting feedrate, with the finishing amount left, until the input figure position is reached.

(2) Then, the tool immediately retracts in the XZ axis direction by

the escape amount (specified in parameter No. 9212) and then moves in rapid traverse in the Z axis direction until the cutting start point is reached.

(3) The tool returns to the initial position in rapid traverse in the X

axis direction and then stops.

Cutting start point

- 86 -

B-64254EN/06 CUTTING CYCLE 5.RECTANGULAR CYCLE

3. Cutting Cycle with Manual In-Feeding (D-CUT=0) in the Z Direction (When the Tool Is Positioned in [C], [G], [H], or [I])

(1) The tool moves in rapid traverse from the initial position, first

along the Z axis and then the X axis direction, goes at the Z axis

direction clearance distance (No.9211) from the workpiece. (2) Cutting is done along the input figure until the end. (3) The tool moves in cutting feedrate in the X axis direction over

the distance equal to the X axis direction clearance. (4) The tool returns to the initial position in rapid traverse, first

along the Z axis and then the X axis.

Initial tool position

- 87 -

5.RECTANGULAR CYCLE CUTTING CYCLE B-64254EN/06

4. Entire Area Cutting Cycle with Automatic In-Feeding (D-CUT>0) in the Z Direction (When the Tool Is Positioned in [C], [G], [H], or [I])

(1) The tool moves in rapid traverse, first in the Z axis direction and

then in the X axis direction, until the cutting start point is

reached. Steps (2) and (3) are the same as the cycle with manual in-feeding. (4) The tool moves in rapid traverse in the X axis direction by the

depth of cut (D-CUT). (5) Steps (2) to (4) are repeated until the bottom end of the X axis is

reached. After the final in-feed machining, the tool retracts in the XZ axis

direction by the escape amount (specified in parameter No. 9212)

and then goes at the X axis direction clearance distance

(No.9210) from the workpiece. (6) When performing only rough cutting, the tool returns to the

initial position in rapid traverse, first in the Z axis direction and

then in the X axis direction, and then stops. When doing both

rough and finishing cutting, the tool performs finishing cutting.

X axis direction clearance

Z axis direction clearance

D-CUT

- 88 -

fanuc TURN MATE i Operators Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

B-64254EN/06

SAFETY PRECAUTIONS

DEFINITION OF WARNING, CAUTION, AND NOTE

GENERAL WARNINGS AND CAUTIONS

OVERVIEW OF THIS MANUAL

TABLE OF CONTENTS

I. WHAT’S TURN MATE i ?

1 WHAT’S TURN MATE i ?

II. BASIC SCREEN AND OPERATIONS

1 BASE SCREEN

2 BASIC SCREEN OPERATIONS

2.1 BUTTON OPERATION

2.2 CURSOR OPERATION

2.3 TAB OPERATION

2.4 CALCULATOR OPERATION

3 SETTING OF COORDINATE SYSTEM

4 SETTING OF SPINDLE INFORMATION

4.1 SETTING OF SPINDLE SPEED

4.2 SETTING OF SURFACE SPEED

4.3 SETTING OF GEAR NUMBER

5 SETTING OF TOOL INFORMATION

5.1 TOOL SELECTION

5.2 INPUT OF TOOL OFFSET

5.2.1 Direct Input of Tool Offset

5.2.2 Measurement of Tool Offset

6 ALARM CHECK

III. MANUAL CUTTING

1 MANUAL CUTTING

2 MANUAL CUTTING IN LIMITED AREA

IV. CUTTING CYCLE

1 OUTLINE

1.1 WHAT’S CUTTING CYCLE ?

1.2 CUTTING METHODS

2 OPERATION

2.1 WORKFLOW

2.2 SETTING THE FEEDRATE

2.3 CREATING A NEW CUTTING CYCLE

2.4 EDITING A CUTTING CYCLE

2.5 SELECTING A CUTTING CYCLE

2.6 DELETING A CUTTING CYCLE

2.7 NOTES

2.7.1 Inhibition of Operation

2.7.2 Manual Intervention during Cutting Cycles

2.7.3 Tool Nose Radius Compensation

3 FACE CYCLE

3.1 OUTLINE

3.2 TOOL CUTTING MOTIONS

3.3 INPUT DATA

4 CHAMFER CYCLE

4.1 OUTLINE

4.2 TOOL CUTTING MOTIONS

4.3 INPUT DATA

5 RECTANGULAR CYCLE

5.1 OUTLINE

5.2 TOOL CUTTING MOTIONS

5.2.1 Rough Cutting Motions