mitsubishi M700, M70NAVI Instruction Manual

MELDAS is a registered trademark of Mitsubishi Electric Corporation. Other company and product names that appear in this manual are trademarks or registered trademarks of the respective companies.

Introduction

This manual is an instruction manual for NAVI LATHE for 700/70 (hereafter NAVI LATHE). This manual explains how to operate NAVI LATHE, so read this manual thoroughly before use. Be sure to study "Precautions for Safety" on the next page and use the system safely.

Details described in this manual

CAUTION

For items described as "Restrictions" or "Usable State" in this manual, the instruction manual

issued by the machine tool builder takes precedence over this manual.

Items not described in this manual must be interpreted as "not possible". This manual is written on the assumption that all option functions are added. Confirm with the

specifications issued by the machine tool builder before starting to use.

Refer to the Instruction Manual issued by each machine tool builder for details on each

machine tool.

Some screens and functions may differ depending on the NC system (or its version), and

some functions may not be possible. Please confirm the specifications before use.

Refer to the following documents.

MITSUBISHI CNC 700/70 Series Instruction Manual ....................................IB-1500042

MITSUBISHI CNC 700/70 Series Setup Manual ...........................................IB-1500124

MITSUBISHI CNC 700/70 Series Programming Manual (Lathe System) .....IB-1500057

Precautions for Safety

Always read the specifications issued by the machine tool builder, this manual, related manuals and attached documents before operation or programming to ensure correct use. Understand the NAVI LATHE, safety items and cautions before using the system. This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".

DANGER

When the user may be subject to imminent fatalities or major injuries if handling is mistaken.

WARN ING

When the user may be subject to fatalities or major injuries if handling is mistaken.

CAUTION

When the user may be subject to bodily injury or when property damage may occur if handling is mistaken.

Note that even items ranked as "

CAUTION", may lead to serious consequences depending

on the situation. In any case, important information that must always be observed is described.

DANGER

Not applicable in this manual.

WARNING

1. Items related to operation

If the operation start position is set in a block which is in the middle of the program and

the program is started, the program before the set block is not executed. Please confirm that G and F modal and coordinate values are appropriate. If there are coordinate system shift commands or M, S, T and B commands before the block set as the start position, carry out the required commands using the MDI, etc. If the program is run from the set block without carrying out these operations, there is a danger of interference with the machine or of machine operation at an unexpected speed, which may result in breakage of tools or machine tool or may cause damage to the operators.

Under the constant surface speed control (during G96 modal), if the axis targeted for

the constant surface speed control moves toward the spindle center, the spindle rotation speed will increase and may exceed the allowable speed of the workpiece or chuck, etc. In this case, the workpiece, etc. may jump out during machining, which may result in breakage of tools or machine tool or may cause damage to the operators.

1. Items related to product and manual For items described as "Restrictions" or "Usable State" in this manual, the instruction

manual issued by the machine tool builder takes precedence over this manual.

Items not described in this manual must be interpreted as "not possible". This manual is written on the assumption that all option functions are added. Confirm

with the specifications issued by the machine tool builder before starting use.

Refer to the Instruction Manual issued by each machine tool builder for details on

each machine tool.

Some screens and functions may differ depending on the NC system (or its version),

and some functions may not be possible. Please confirm the specifications before use.

2. Items related to installation and assembly

Ground the signal cables to ensure stable system operation. Also ground the NC unit

main frame, power distribution panel and machine to one point, so they all have the same potential.

3. Items related to preparation before use

Always set the stored stroke limit. Failure to set this could result in collision with the

machine end.

Always turn the power OFF before connecting/disconnecting the I/O device cable.

Failure to do so could damage the I/O device and NC unit.

CAUTION

4. Items related to screen operation

NAVI LATHE uses the following variables in order to operate the NC program.

NC program mode Variables used by NAVI LATHE

User macro mode #150 to #197 MTB macro mode #450 to #497

When NC program mode is user macro mode, do not use common variables (#150 to #197). If those variables are written over, malfunction will be resulted. If mistakenly written them over, turn the NC power OFF after securing your safety. When the power is turned ON again, the system recovers the data. NC program mode is specified on the Preferences screen.

When either "TOOL REG No." or "CYCLE" is input in each machining process screen, the cutting speed and feedrate are automatically determined using the data in the tool file screen and the cutting condition file screen. Note that the cutting speed and feedrate of each process determined once will not be changed by changing the data in the tool file screen and the cutting condition file screen.

(Continued on next page)

5. Items related to operation Stay out of the moveable range of the machine during automatic operation. During

rotation, keep hands, feet and face away from the spindle.

Carry out dry operation before actually machining, and confirm the machining program,

tool offset and workpiece coordinate system offset.

If the operation start position is set from a block in the program and the program is

started, the program before the set block is not executed. If there are coordinate system shift commands or M, S, T, and B commands before the block set as the starting position, carry out the required commands using the MDI, etc. There is a danger of interference with the machine if the operation is started from the set starting position block without carrying out these operations.

Program so the mirror image function is turned ON/OFF at the mirror image center.

The mirror image center will deviate if the function is turned ON/OFF at a position other than the mirror image center.

6. Items related to faults and abnormalities

If the battery low warning is issued, save the machining programs, tool data and

parameters in an input/output device, and then replace the battery. When the battery alarm is issued, the machining programs, tool data and parameters may be destroyed. Reload the data after replacing the battery.

If the axis overruns or emits an abnormal noise, immediately press the emergency

stop button and stop the axis movement.

CAUTION

(Continued from previous page)

(Continued on next page)

7. Items related to maintenance Incorrect connections may damage the devices, so connect the cables to the

specified connectors.

Do not apply voltages other than those indicated according to specification on the

connector. Doing so may lead to destruction or damage.

Do not connect or disconnect the connection cables between each unit while the

power is ON.

Do not connect or disconnect the PCBs while the power is ON.

Do not connect the cable by pulling on the cable wire.

Do not short circuit, charge, overheat, incinerate or disassemble the battery. Dispose the spent battery according to local laws. Dispose the spent cooling fan according to local laws. Do not replace the control unit while the power is ON. Do not replace the operation panel I/O unit while the power is ON. Do not replace the control section power supply PCB while the power is ON. Do not replace the expansion PCB while the power is ON. Do not replace the memory cassette while the power is ON. Do not replace the cooling fan while the power is ON. Do not replace the battery while the power is ON. Be careful that metal cutting chips, etc., do not come into contact with the connector

contacts of the memory cassette.

Do not replace the high-speed program server unit while the power is ON.

CAUTION

(Continued from previous page)

Disposal

(Note) This symbol mark is for EU countries only.

This symbol mark is according to the directive 2006/66/EC Article 20 Information for endusers and Annex II.

Your MITSUBISHI ELECTRIC product is designed and manufactured with high quality materials and components which can be recycled and/or reused. This symbol means that batteries and accumulators, at their end-of-life, should be disposed of separately from your household waste. If a chemical symbol is printed beneath the symbol shown above, this chemical symbol means that the battery or accumulator contains a heavy metal at a certain concentration. This will be indicated as follows: Hg: mercury (0,0005%), Cd: cadmium (0,002%), Pb: lead (0,004%) In the European Union there are separate collection systems for used batteries and accumulators. Please, dispose of batteries and accumulators correctly at your local community waste collection/ recycling centre.

Please, help us to conserve the environment we live in!

1. OUTLINE .....................................................................................................................1

1.1 System Outline............................................................................................................1

1.2 Input Procedures.........................................................................................................3

1.3 Screen Configuration...................................................................................................4

1.4 Starting NAVI LATHE..................................................................................................5

1.5 Setting up NAVI LATHE ..............................................................................................6

2. FUNCTIONS OF DISPLAY AREA...............................................................................8

2.1 LIST VIEW Area..........................................................................................................9

2.2 OPERATION VIEW Area...........................................................................................11

2.3 Setting Area...............................................................................................................12

2.4 Message Area ...........................................................................................................12

2.5 Menu Display Area....................................................................................................12

3. BASIC OPERATIONS................................................................................................13

3.1 Changing Active View................................................................................................13

3.2 Changing Screen.......................................................................................................13

3.3 Setting Data...............................................................................................................15

3.4 Switching Windows....................................................................................................18

3.5 Switching Selection Tags ..........................................................................................18

3.6 Inputting Operations..................................................................................................19

4. SCREEN SPECIFICATIONS.....................................................................................20

4.1 Starting NAVI LATHE................................................................................................20

4.2 Screen Related to the Program.................................................................................21

4.2.1 Program Edit Screen ..................................................................................21

4.3 Screens Related to the Process Edit Functions........................................................26

4.3.1 Process List Screen....................................................................................26

4.3.2 Operating Process......................................................................................27

4.3.3 Process Mode Selection Screen.................................................................33

4.3.4 Initial Condition Setting Screen................................................................... 37

4.3.5 Turning Process..........................................................................................40

4.3.6 Copy Cut Process.......................................................................................46

4.3.7 Threading Screen.......................................................................................49

4.3.8 Grooving Screen.........................................................................................53

4.3.9 Trapezoidal Grooving Screen.....................................................................56

4.3.10 Hole Drilling Screen..................................................................................59

4.3.11 EIA Screen................................................................................................61

4.3.12 Milling Hole Drilling Screen.......................................................................62

4.3.13 Keyway Cutting Screen ............................................................................75

4.3.14 Contour Cutting Screen............................................................................81

4.4 Screens Related to File Editing.................................................................................90

4.4.1 Tool File Screen for Turning.......................................................................90

4.4.2 Tool File Screen for Milling.........................................................................95

4.4.3 Cutting Condition File Screen for Turning...................................................97

4.4.4 Cutting Condition File Screen for Milling...................................................101

4.5 Screen Related to the Parameters..........................................................................103

4.5.1 Parameter Screen.....................................................................................103

4.5.1.1 Parameters for Turning................................................................103

4.5.1.2 Parameters for Milling..................................................................107

4.5.2 PREFERENCE Screen.............................................................................110

4.6 Screen Related to the Version.................................................................................112

4.6.1 Version Screen.........................................................................................112

4.7 Program Checker Screen........................................................................................113

4.8 Guidance Function ..................................................................................................122

4.8.1 Tool Guidance Screen..............................................................................123

4.8.1.1 Tool Guidance for Turning...........................................................123

4.8.1.2 Tool Guidance for Milling.............................................................125

5. PROGRAM SPECIFICATIONS................................................................................126

5.1 NC Program.............................................................................................................127

5.1.1 Output Method for NC Program................................................................127

5.1.2 Restrictions...............................................................................................131

5.2 File Program............................................................................................................133

5.3 Parameter Program.................................................................................................133

5.4 Macro Program........................................................................................................134

6. RESTRICTIONS FOR CNC FUNCTION SPECIFICATIONS...................................135

7. ALARM MESSAGE..................................................................................................139

7.1 Error Message.........................................................................................................139

7.2 Operation Message.................................................................................................142

APPENDIX 1. VARIABLES USED IN NAVI LATHE.....................................................143

APPENDIX 2. PROGRAMMING EXAMPLE 1 (TURNING) .........................................146

Appendix 2.1 Machining Drawing..................................................................................146

Appendix 2.2 Process Table..........................................................................................147

Appendix 2.3 Condition Setting.....................................................................................148

Appendix 2.4 Creating Program....................................................................................149

APPENDIX 3. PROGRAMMING EXAMPLE 2 (MILLING) ...........................................156

Appendix 3.1 Machining Drawing..................................................................................156

Appendix 3.2 Process Table..........................................................................................157

Appendix 3.3 Condition Setting.....................................................................................158

Appendix 3.4 Creating Program....................................................................................159

1. OUTLINE

1.1 System Outline

This manual is an instruction manual for NAVI LATHE for 700/70 (hereafter NAVI LATHE). The part program for the turning center is created with the NAVI LATHE. NAVI LATHE provides the turning function and the milling function.

(1) The following machining processes can be edited.

Turning Processes

• Turning (Outer dia., inner dia., front face)

• Copy cutting (Outer dia., inner dia., front face)

• Threading (Outer dia., inner dia., front face)

• Grooving (Outer dia., inner dia., front face)

• Trapezoidal grooving (Outer dia., inner dia., front face)

• Hole drilling (Drilling, deep-hole drilling, step, tapping)

• EIA

Milling Processes

• Milling hole drilling (Drilling, deep-hole drilling, boring, tapping)

• Keyway cutting (Front face, outer surface, side surface)

• Contour cutting (Front face, outer surface, side surface)

(Note) Milling interporation specifications are required to edit the milling processes.

1.1 System Outline

(2) The tool file and the cutting condition file are provided and the cutting conditions for each process are

determined automatically.

(3) The operation screen consists of the LIST VIEW area and the OPERATION VIEW area. In the LIST

VIEW area, the whole part program can be always viewed. In the OPERATION VIEW area, there are the guide drawings related to the input items, and the data can be easily input by using these guide drawings.

[LIST VIEW area]

The object of the NAVI LATHE is selected.

[OPERATION VIEW area]

The screen is displayed corresponding to the object selected

in the LIST VIEW. [Cutting conditions automatically determined]

Upon tool registration No. entry, the

cutting conditions for each process

are automatically determined based

on the tool file and cutting condition

file.

[Help]

[Guide drawing]

[Menu keys]

- 1 -

1. OUTLINE

1.1 System Outline

(4) Program Checker enables the machining shape of a part program to be graphically traced. With this

function, errors in input data can be detected at an earlier stage. (5) Guidance function provides an operator with error recovery information. (6) Part program is a macro-program-based NC program. Commands can be added between processes

from the edit screen of the standard MITSUBISHI CNC 700/70 Series. (7) The macro program mentioned above can be customized by the machine tool builder.

- 2 -

1. OUTLINE

1.2 Input Procedures

The input procedure for the NAVI LATHE is shown below.

The part is operated on the NAVI LATHE's screen.

Supplements

1.2 Input Procedures

Start

File edition

Tool file Cutting condition file

Parameter setting

Parameter file (The parameter setting is valid even if the parameter is set after editing the NC program)

NC program selection

Newly create Read out

Process editing:

Initial conditions Process mode selection Process data input

Turning / Copy cutting / Threading / Grooving / Trapezoidal grooving / Hole drilling / EIA / Milling hole drilling / Keyway cutting / Contour cutting

Tool file

(Tool registration No. 10 1 -)

No. No.

direction

No.

direction

Tool leng. offset

Tool diam. offset

Spindle rotation

Cut condition file

(Work registration No.1 to 8)

Parameter setting

• M0 output

• Maximum number of spindle rotations

• Clearance

• Tool return position

• Common parameters for threading process

• Common parameters for grooving process

• Common parameters for hole drilling process

Process editing

Material Tool applicable

Material

rotation rate

Tool applicable

rotation rate

Program check

Program Checker is used.

Program check

(Note) Set the tool

compensation amount and workpiece coordinate system offset to perform Program Check. This function is realized by using the 700/70 Series graphic check functio n .

NC program operation

END

- 3 -

1. OUTLINE

1.3 Screen Configuration

The screen configuration for the NAVI LATHE is shown below.

Program

editing screen

Process list

screen

Initial

condition

setting screen

Turning

screen

Copycutting screen

Threading

screen

1.3 Screen Configuration

Process

pattern

screen

Process

File

Process mode

selection

screen

(For a new process, select a process from the process mode.)

Program

checker

Tool file

screen

Cutting

condition

file screen

Grooving

screen

Trapezoidal

grooving

screen

Hole drilling

screen

EIA screen

Milling

hole drilling

screen

Keyway

cutting screen

Contour

cutting screen

Process

pattern

screen

Process

pattern

screen

Parameter

Version

Parameter

screen

Version

screen

Preference

screen

- 4 -

1. OUTLINE

Screen name Details

Program editing screen NC program is newly created and read out, etc. Process list screen Tool information and cutting conditions for each process of a

Process mode selection screen

Initial conditions setting screen

Turning screen Various parameters for turning process are input. Turning pattern screen The machining patterns for turning process are input. Copy cutting screen Various parameters for copy cutting process are input. Copy cutting pattern

screen Threading screen Various parameters for threading process are input. Grooving screen Various parameters for grooving process are input. Trapezoidal grooving

screen Hole drilling screen Various parameters for hole drilling process are input. EIA screen The EIA process is input. Milling hole drilling

screen Milling hole drilling

pattern screen Keyway cutting screen Various parameters for keyway cutting process are input. Contour cutting screen Various parameters for contour cutting process are input. Contour cutting pattern

screen Tool file screen The tool data by each tool is registered.

Cutting condition file screen

Parameter screen The parameters for a NC program are set. Preference screen The system is set up. Version screen The version data of the NAVI LATHE is displayed. Program checker The machining shape of a NC program is graphically

1.4 Starting NAVI LATHE

1.3 Screen Configuration

NC program are listed. The process mode (turning process, etc.) is selected.

The initial conditions for a NC program are set.

Machining patterns for copy cutting process are input.

Various parameters for trapezoidal grooving process are input.

Various parameters for milling hole drilling process are input.

The machining patterns for milling hole drilling process are input.

The machining patterns for contour cutting process are input.

The cutting conditions (cutting speed, feedrate) by each process are input, corresponding to tip material. Also, the cutting conditions (speed rate) by each process are input, corresponding to workpiece material.

displayed.

Select

function, then the lathe menu to display NAVI LATHE screen.

EDIT

Program edit screen is displayed once when the power is turned ON. Then, whatever the screen previously selected with NAVI LATHE is displayed thereafter.

- 5 -

1. OUTLINE

1.5 Setting up NAVI LATHE

Part program output from NAVI LATHE is a macro-program-based NC program. Thus, macro programs have to be registered in the NC system in advance. Also, the destinations where NC programs or NAVI LATHE's reference files are saved, as well as the unit for data input, have to be specified prior to NAVI LATHE operations.

NAVI LATHE setup items

Item Details Standard value

PATH PROGRAM

PATH PARAMETER

MACRO Macro program mode

UNIT Unit for data input

Path to the folder in which NC program is saved. MEM:/

Path to the folder in which tool file, cutting condition file and parameter file are saved.

1: User macro mode 2: MTB macro mode

1: inch 2: mm

In 700 Series:

D:/NCFILE/NAVI

In 70 Series:

MEM:/

1 (User Macro)

2 (mm)

- 6 -

1. OUTLINE

1.5 Setting up NAVI LATHE

NAVI LATHE setup procedures

(1) Open PARAMETER screen.

(2) Set "999 MAINTE" to 1. [PREFERENCE] menu is displayed.

(3) Press [PREFERENCE] menu.

PREFERENCE screen is displayed.

(4) Select the macro type.

(1:Uer macro 2:MTB macro)

(5) Press [MACRO ENTRY] menu.

"OK?(Y/N)" message is displayed.

(6) Press [Y] key. Macro program is registered in NC system.

(7) Enter the program path.

(8) Enter the parameter path.

(9) Select the unit.

(1:inch, 2:mm)

When the unit is changed, turn the power OFF and ON again.

(Addendum)

• Always carry out a macro program registration when setting up NAVI LATHE or switching "MACRO" types.

• Change "PROGRAM PATH" and "PARAMETER PATH" when necessary.

• When "UNIT" is changed, turn the power OFF and ON again.

• If the tool file, cutting condition file and parameter file do not exist in "PARAMETER PATH" folder when the power is turned ON, the system creates them.

- 7 -

2. FUNCTIONS OF DISPLAY AREA

The screen of the NAVI LATHE is divided into the following five areas.

(1) LIST VIEW area (Refer to "2.1 LIST VIEW Area") (2) OPERATION VIEW area (Refer to "2.2 OPERATION VIEW Area") (3) Setting area (Refer to "2.3 Setting Area") (4) Message area (Refer to "2.4 Message Area") (5) Menu display area (Refer to "2.5 Menu Display Area")

(1) LIST VIEW area

(2) OPERATION VIEW area

(4) Message area

(5) Menu display area

(3) Setting area

- 8 -

2. FUNCTIONS OF DISPLAY AREA

2.1 LIST VIEW Area

The object of the NAVI LATHE is selected in this area.

(1) Area bar

(2) Object

(3) Cursor

2.1 LIST VIEW Area

(1) Area bar

When the LIST VIEW area is active, the area bar is highlighted.

(2) Objects

The list of objects that can be selected are displayed. The object is composed of the main object and the sub object, which is a specification of the main object. The details of each object are as follows.

Main object Sub object Details

PROGRAM - Newly creates, reads out, and deletes, etc. the NC program. PROCESS 0 INIT

1 DR :

FILE

PARAMETER - Displays the tool option and the miscellaneous parameter to

VERSION - Displays the version data of the NAVI LATHE.

(Note) If too many processes are registered and all the objects cannot be displayed, a scroll bar will be

displayed. In this case, change display of the list by pressing cursor key or page key down, or by clicking on the scroll bar.

TOOL Displays and changes the tool file. M TOOL Displays and changes the tool file for the milling machining.

CUT CONDTN Displays and changes the cutting conditions for each

M CUT CONDTN

Displays the currently edited process list. The settings of the selected process can be displayed and changed.

(Note) This is valid when the milling interporation

process per tip material or workpiece material. Displays and changes the cutting conditions for each

process per tip material or workpiece material for the milling machining. (Note) This file is valid when the milling interporation

be used in each process. Those can be changed.

specifications are provided.

- 9 -

2. FUNCTIONS OF DISPLAY AREA

2.1 LIST VIEW Area

(3) Cursors

When the LIST VIEW area is active and the object is selected with the cursor, the display in the OPERATION VIEW area and the menu display area will be changed.

<Cursor movement> The cursor is moved using the cursor keys or a pointing device.

Key type Operation of cursor

[↑] Cursor key Moves the cursor one field up regardless of the main object or sub object.

Note that if the ↑ cursor is pressed when the cursor is at the top, the cursor does not move.

[↓] Cursor key Moves the cursor one field down regardless of the main object or sub object.

Note that if the ↓ cursor is pressed when the cursor is at the bottom, the cursor does not move.

[←] Cursor key When the cursor is at the sub object, moves the cursor to the previous main

object.

[→] Cursor key When the cursor is at the sub object, moves the cursor to the next main

object.

[Page Up] key Moves the displayed data toward the top. [Page Down]

key Pointing device Cursor jumps to the spot where clicked with a pointing device. If an object not

Moves the displayed data toward the bottom.

selectable is clicked, cursor does not jump.

- 10 -

2. FUNCTIONS OF DISPLAY AREA

2.2 OPERATION VIEW Area

The various data are displayed in this area. Selecting the object in the LIST VIEW area changes the contents displayed in the OPERATION VIEW area.

(1) Area bar

(2) Help

(3) Guide drawing

(4) Sub cursor

(1) Area bar

When the OPERATION VIEW area is active, the area bar is highlighted. The name of the currently edited program is displayed.

(2) Help

Quick reference on the setting items is displayed.

(3) Guide drawing

When the process is edited, a guide drawing according to the currently edited machining mode is displayed.

(4) Sub cursor

Key type Operation of cursor

[↑] Cursor key Moves the cursor one field up.

Note that if the ↑ cursor is pressed when the cursor is at the top, the cursor does not move.

[↓] Cursor key Moves the cursor one field down.

Note that if the ↓ cursor is pressed when the cursor is at the bottom, the

cursor does not move. [Page Up] key Moves the displayed data toward the top. [Page Down]

key

Moves the displayed data toward the bottom.

- 11 -

2. FUNCTIONS OF DISPLAY AREA

2.3 Setting Area

The value to be set to data is input.

2.4 Message Area

An error message or operation message, etc. during operation is displayed.

2.5 Menu Display Area

The screen operation is selected, and the screen is changed. The different menus are displayed in each screen. (Refer to the chapter 4.)

2.3 Setting Area

- 12 -

3. BASIC OPERATIONS

3.1 Changing Active View

3. BASIC OPERATIONS

3.1 Changing Active View

To operate NAVI LATHE, activate either LIST VIEW area or OPERATION VIEW area. When the VIEW is active, the area bar is highlighted and data can be input. Use menu keys [←] and [→] or a pointing device to switch either one of the VIEWs to be activated.

3.2 Changing Screen

When the object is selected in the LIST VIEW area, the screen (contents in the OPERATION VIEW area) changes. (Refer to the section 2.1 LIST VIEW Area.) Note that the screen cannot be changed while the OPERATION VIEW area is active. In such a case, press the [←] menu key or click "LIST VIEW" with a pointing device to turn the LIST VIEW area active.

Operation example

(1) Open the program edit screen.

The OPERATION VIEW area is active.

Press the [←] menu key. (2)

The LIST VIEW area will turn active.

- 13 -

3. BASIC OPERATIONS

(3) Select the object with the cursor key.

3.2 Changing Screen

The OPERATION VIEW area will change into the screen corresponding to the selected object.

(4) Press the [MODIFY] menu key.

The OPERATION VIEW area will turn active.

- 14 -

3. BASIC OPERATIONS

3.3 Setting Data

After moving the sub cursor, input the data into the setting area and then press the [INPUT] key, and the data will be set. (The sub cursor is displayed only when the OPERATION VIEW area is active.)

Sub cursor

Setting area

- 15 -

3. BASIC OPERATIONS

Operation method

An example for setting the data on the hole drilling screen is shown below.

(1) Screen selection Select the object to be changed from the

LIST VIEW and press [MODIFY] menu key.

(2) Setting item selection Move the sub cursor with cursor keys.

The OPERATION VIEW area will turn active. (Refer to the section 3.2 "Changing screen".)

This is an example of the sub cursor movement on the hole drilling screen.

3.3 Setting Data

(3) Data key input Set data with the numeral keys or

alphabet keys, etc. [1] [8] [.] [0] [0] [0]

The data is set in the data setting area. 18．000

(4) [INPUT] key input Press the [INPUT] key.

Data for the selected setting item is set. The sub cursor moves to the next position.

(Note 1) The contents in the data setting area are only displayed when [INPUT] key is not pressed and

will be invalidated if the screen is changed at this time. Data for the currently selected setting item will be set when [INPUT] key is pressed.

(Note 2) If illegal data is set, an error occurs when [INPUT] is pressed. Set the correct data again.

- 16 -

3. BASIC OPERATIONS

3.3 Setting Data

Operations in the data setting area

The key is input at the position where the cursor is displayed. If a cursor is not displayed, the key input is invalid. When a key is input, the data appears at the cursor position, and the cursor moves one character space to the right.

[→] / [←] keys: Moves the cursor one character to the left or right.

(1) The cursor is at the position shown on

the right.

(2)

Press the [→] key.

[DETETE] key: Deletes the character in front of the cursor.

(1) Move the cursor to the position where

the data is to be deleted.

(2) Press the [DETETE] key.

1 2 3 7 7 7 | 4 5 6

The cursor moves one character space to the right. 1 2 3 7 7 7 4 | 5 6

The cursor in the data setting area moves. 1 2 3 4 | 5 6

The character in front of the cursor is deleted. 1 2 3 | 5 6

- 17 -

3. BASIC OPERATIONS

3.4 Switching Windows

When a shortcut button on the keyboard is pressed, its corresponding window is displayed.

Button Application

LIST

Displays the tool guidance window.

Displays the message guidance window.

Displays the checker window.

3.5 Switching Selection Tags

Menu tag

When a tag button on the keyboard is pressed, the main window and checker window can be switched over.

Button Application

Selects the tag on the left.

Selects the tag on the right.

(Note 1) Depending on the keyboard specifications, tag button may not be available.

- 18 -

3. BASIC OPERATIONS

3.6 Inputting Operations

In addition to the method of directly inputting numeric data for specific data settings, a method to input the operation results using four rules operators and function symbols can be used.

Input method

Numeric values, function symbols, operators and parentheses ( ) are combined and set in the data setting area. The operation results appear when the [INPUT] key is pressed. Data for the currently selected setting item will be set when [INPUT] key is pressed again. The contents in the data setting area are erased.

Examples of operator settings,

and results

Operation

Setting

example

Operation

results

Function symbols, setting examples

and results

Function

symbol

Setting

example

Operation

results

Addition =100+50 150.000 Subtraction =100−50 50.000 Square root SQRT =SQRT (3) 1.732

Multiplication =12.3∗4 49.200 Sine SIN =SIN (30) 0.5 Division =100/3 33.333 Cosine COS =COS (15) 0.966

Function

=1.2∗ (2.5+SQRT(4))

5.400

Circle ratio PAI =PAI*10 31.415 Inch INCH =INCH/10 2.54

Operation examples

(1) Set as shown below, and press the

[INPUT] key. =12∗20 [INPUT]

(2) Press the [INPUT] key again.

Notes for using operators and functions

Division: Zero division causes an error. Square root: If the value in the parentheses is negative, an error occurs. Triangle function: The unit of angle θ is degree (°). Arc tangent: −90 < operation results < 90.

Restrictions

• Always use "=" for the first character.

• Do not use the following characters as the second character or last character.

Invalid as second character: ∗, /, ) Invalid as last character: ∗, /, (, +, -

• Make sure that the left parentheses and right parentheses are balanced.

• The 360° limit does not apply on the angle. SIN (500) is interpreted as SIN (140).

Absolute value

ABS

=ABS (50−60)

10.000

Tangent TAN =TAN (45) 1 Arc tangent ATAN =ATAN (1.3) 52.431

The operation results appear in the data setting area.

240 |

Data for the selected setting item is set. The cursor moves to the next position.

- 19 -

4. SCREEN SPECIFICATIONS

4.1 Starting NAVI LATHE

When NAVI LATHE is started, the program edit screen will be displayed.

Screen layout

4.1 Starting NAVI LATHE

At the initial start up of NAVI LATHE, the cursor is displayed at the position of [PROGRAM] in the LIST VIEW area, and the program edit screen is displayed in the OPERATION VIEW area. The LIST VIEW area is active. The process program is not selected.

- 20 -

4. SCREEN SPECIFICATIONS

4.2 Screen Related to the Program

4.2.1 Program Edit Screen

The NC program is newly created and read out, etc. on this screen. When [PROGRAM] is selected in the LIST VIEW area, this screen is displayed.

Screen layout

The process list of the currently selected program is displayed in the LIST VIEW area.

- 21 -

4. SCREEN SPECIFICATIONS

4.2 Screen Related to the Program

Process name

Turning

Thread

Groove

Trapezoidal grooving

Hole drilling

EIA EIA

OD OPEN TURN-OUT ? OD CLOSE TURN-OUT ? ID OPEN TURN-IN ? ID CLOSE TURN-IN ? FACE OPEN TURN-FACE ? FACE CLOSE TURN-FACE ?

Outer diameter COPY OUT ? Copy cutting Inner diameter COPY-IN ?

Outer diameter THD-OUT ? Inner diameter THD-IN ? Face THD-FACE ?

Outer diameter GRV-OUT Inner diameter GRV-IN Face GRV-FACE

Outer diameter TGRV-OUT ? Inner diameter TGRV-IN ? Face TGRV-FACE ?

Drill DR Deep hole PECK Step STEP Tapping TAP

Display

character

A symbol that indicates the machining type (rough/finishing) is put at ?.

• Rough machining: R

• Finishing machining: F

A symbol that indicates the machining type (rough/finishing) is put at ?.

• Rough machining: R

• Finishing machining: F A symbol that indicates the machining type

(rough/finishing) is put at ?.

• Rough machining: R

• Finishing machining: F

A symbol that indicates the machining type (rough/finishing) is put at ?.

• Rough machining: R

• Finishing machining: F

Remarks

- 22 -

4. SCREEN SPECIFICATIONS

Process name Display

Milling hole drilling

Deep hole

Step M STEP-**** Tapping M TAP-****

Keyway cutting

Outer surface K WAY-OUT ? Side surface K WAY-SIDE ?

Contour cutting

Outer surface CONT-OUT ? Side surface CONT-SIDE ?

Screen display item

No. Display item Details Setting range

Drilling M DR-****

drilling

Front face K WAY-FACE ?

Front face CONT-FACE ?

PROGRAM LIST Displays the program number and comment of the

4.2 Screen Related to the Program

character

Symbols that indicate the machining area (front face/outer surface/side surface) are put at ****.

M PECK-****

NC program that can be currently read out.

・Front face: FACE ・Outer surface: OUT ・Side surface: SIDE

A symbol that indicates machining type (rough/finishing) is put at ?.

・Rough machining: R ・Finishing machining: F

Remarks

- 23 -

4. SCREEN SPECIFICATIONS

Menus

No. Menu Details

← Turns the LIST VIEW area active.

NEW

OPEN

4.2 Screen Related to the Program

Newly creates the NC program. (Note 1) < Display in the setting area when pressing the menu > O( ) COMMENT( )

Reads out the existing NC program. (Note 1) (Note 2) < Display in the setting area when pressing the menu > O( ) When this menu is pressed, the cursor appears at the program list's name section. When the setting area is empty, select a program with the cursor and press the [INPUT] key to read the program.

COPY

Curso

Copies the existing NC program to another program. (Note 1) < Display in the setting area when pressing the menu > O( ) → O( )

COMMENT

Edits the comment in the NC program. (Note 1) < Display in the setting area when pressing the menu > O( ) COMMENT( )

RENAME

Renames the existing NC program. (Note 1) < Display in the setting area when pressing the menu > O( ) → O( )

DELETE Deletes the NC program.

< Display in the setting area when pressing the menu > O( ) to O( )

LIST UPDATE Updates the list display.

(Note 1) 1 to 7999 or 10000 to 99999999 can be set for the O No, and up to 18 alphanumeric

characters can be set for the comment.

(Note 2) NC program mode includes user macro mode and MTB mode. (This is specified in the

preferences screen.) When user macro mode is active and an NC program created with MTB mode is opened, the NC program is converted into user macro mode. When MTB mode is active and an NC program created with user macro mode is opened, the NC program is converted into MTB mode.

- 24 -

4. SCREEN SPECIFICATIONS

Operation example (Opening the existing NC program)

(1) Select the [PROGRAM] in the LIST

VIEW area.

4.2 Screen Related to the Program

The program edit screen will be displayed. The list of the NC program that can be read out will be displayed.

Press the [OPEN] menu key, and input

(2)

the NC program No. to be read out.

Press the [INPUT] key.

(3)

The [OPEN] menu will be highlighted, and the setting area will be displayed.

The highlight of the [OPEN] menu will turn OFF, and the setting area will disappear. The process of the NC program read out will be displayed in the LIST VIEW area. The NC program No. read out will be displayed on the area bar of the OPERATION VIEW area.

- 25 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3 Screens Related to the Process Edit Functions

4.3.1 Process List Screen

The tool information and cutting conditions for each process are displayed on this screen. When [PROCESS] is selected in the LIST VIEW area, this screen is displayed. When the NC program is not selected, this screen is not displayed.

Screen layout

Screen display items

No. Display item Details Setting range

PCS The process name is displayed.

T NAME The name of tool to be used is displayed. -

T The tool No. and compensation No. are displayed.

V The cutting speed is displayed.

F The feedrate is displayed. The feedrate can be

Menus

No. Menu Details

← Turns the LIST VIEW area active.

SAVE Saves changes in the process list.

(Note) This name is same as the name displayed in

the LIST VIEW area.

The tool No. can be changed. T-command will not be output if the tool No. is set to "0". Set the tool No. to "0" unless T-command needs to be output, such as when the same tool is used for the multiple consecutive processes.

The cutting speed can be changed.

changed. When TAP or THREAD process is applied, the pitch (mm/rev) is displayed.

0 to 99999999

1 to 9999 m/min 1 to 9999 feet/min

0.0001 to 999.9999 mm/rev

0.00001 to

99.99999 inch/rev

- 26 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.2 Operating Process

When the cursor is moved to the sub-object of PROCESS in the LIST VIEW area, a menu for editing the process is displayed, and the process can be operated.

Screen layout

Menus

No. Menu Details

MODIFY The OPERATION VIEW area turns active, and the process

parameters can be changed.

NEW Adds a new process.

The process will be inserted into the cursor position.

MOVE Changes the process position.

DELETE Deletes the process at the cursor position.

When performing the deletion, the process under the deleted process will be moved up.

COPY Copies the process at the cursor position.

The copied process will be inserted under the cursor position.

- 27 -

4. SCREEN SPECIFICATIONS

Operation example (Selecting the process)

Validate the LIST VIEW area, select the

(1)

process with the cursor key.

4.3 Screen Related to the Process Edit Functions

The contents of the OPERATION VIEW area will change to those of the selected process.

Press the [MODIFY] menu key. (2)

The OPERATION VIEW area will turn active.

- 28 -

4. SCREEN SPECIFICATIONS

Operation example (Deleting the process)

Validate the LIST VIEW area, select the

(1)

process to be deleted with the cursor key.

4.3 Screen Related to the Process Edit Functions

The contents of the OPERATION VIEW area will change to those of the selected process.

Press the [DELETE] menu key. (2)

Press the [Y] key. (3) When not deleting the process, press

the [N] key

The [DELETE] menu will be highlighted, and a massage confirming the deletion will appear.

The highlight of the [DELETE] menu will turn OFF, and the process at the cursor position will be deleted. The process under the deleted process will be moved up one. The contents in the OPERATION VIEW area will change to those of the process at the cursor position.

- 29 -

4. SCREEN SPECIFICATIONS

Operation example (Copying the process)

Validate the LIST VIEW area, select the

(1)

process of the copy source with the cursor key.

4.3 Screen Related to the Process Edit Functions

The contents of the OPERATION VIEW area will change to those of the selected process.

Press the [COPY] menu key. (2)

The copied process will be inserted under the cursor position.

- 30 -

4. SCREEN SPECIFICATIONS

Operation example (Moving the process)

Validate the LIST VIEW area, select the

(1)

process to be moved with the cursor key.

4.3 Screen Related to the Process Edit Functions

The contents of the OPERATION VIEW area will change to those of the selected process.

Press the [MOVE] menu key. (2)

Select the position of the movement

(3)

destination with the cursor key.

The [MOVE] menu will be highlighted. The mark "M" will be displayed beside the process to be moved.

- 31 -

4. SCREEN SPECIFICATIONS

Press the [INPUT] key.

(4)

If the [MOVE] menu key is pressed again during the movement operation, the movement operation will be canceled.

4.3 Screen Related to the Process Edit Functions

The message to confirm a movement is displayed.

Press the [Y] key. (5)

When not moving the process, press the [N] key

(Note) For the [NEW] menu, refer to the next section.

The process of the movement source will be moved to the cursor position. The highlight of the [MOVE] menu will turn OFF.

- 32 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.3 Process Mode Selection Screen

When a new process is added, the process mode is selected on this screen.

Screen layout

• Turning process

• Milling Process

(Note) Milling process is available only when the milling interporation specifications are provided.

- 33 -

4. SCREEN SPECIFICATIONS

Screen display item

• Turning process

No. Display item Details Setting range

Process mode Displays the process mode that can be selected for

• Milling Process

No. Display item Details Setting range

Process mode Displays the process mode that can be selected for

No. Menu Details

← Cancels adding a new process.

LATHE Displays the process mode for the turning machining.

MILLING Displays the process mode for milling.

4.3 Screen Related to the Process Edit Functions

1: TURN the turning machining. Select the process mode by moving the sub cursor or inputting numerical values.

milling. Select the process mode by moving the sub cursor or inputting numerical values.

The LIST VIEW area will turn active after cancel.

(Note) This is valid when the milling interporation specifications are

provided.

(Note) This is valid when the milling interporation specifications are

provided.

2: COPY

3: GROOVE

4: T GROOVE

5: THREAD

6: HOLE

7: EIA

1: MILL HOLE

2: KEYWAY

3: CONTOUR

- 34 -

4. SCREEN SPECIFICATIONS

Operation example (Adding a new process)

Validate the LIST VIEW area, and select

(1)

the position where the process is added with the cursor key.

4.3 Screen Related to the Process Edit Functions

Press the [NEW] menu key. (2)

Select turning mode or milling mode by pressing [LATHE] or [MILLING] respectively.

Select the process mode with the cursor

(3)

or the numerical value input.

A blank process will be inserted into the cursor position. The process mode selection screen will be displayed in the OPERATION VIEW area, and the OPERATION VIEW area will turn active.

- 35 -

4. SCREEN SPECIFICATIONS

Press the [INPUT] key.

(4)

(Note) If the [←] menu key is pressed during adding the process, the screen will return to the state

before pressing the [NEW] menu key (state of the 1).

4.3 Screen Related to the Process Edit Functions

The contents in the OPERATION VIEW area will change into those of the selected process mode. The selected process mode will be displayed at the cursor position in the LIST VIEW area.

- 36 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.4 Initial Condition Setting Screen

The initial conditions for the program are set on this screen. When the [INIT] is selected in the LIST VIEW area, this screen is displayed.

Screen layout

Screen display items

No. Display item Details Setting range

WORK REG No. Input the registration No. of the workpiece

1 to 8 material to be cut. Specify it with the No. registered in the cutting condition file. (The list of material names set on the cutting condition file screen will be displayed. Input the corresponding No. based on the list.)

WORK ZERO Input the program zero point.

Depending on the program zero point selection,

1 to 2 the program coordinate system is determined.

1: Tailstock side zero point 2: Chuck side zero point

Tail stock side zero point

Chuck side zero point

- 37 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

OUTSIDE DIA Input the workpiece outer diameter. 0.001 to

INSIDE DIA Input the workpiece inner diameter. 0.000 to

+Z Input the workpiece face position looking from the

-Z Input the workpiece backside position looking from

WORK

COORDINATE

4.3 Screen Related to the Process Edit Functions

program zero point.

the program zero point. Specify the workpiece coordinate system to be

used.

54 : G54

59 : G59 P1 : G54.1 P1

99999.999mm

0.0001 to

9999.9999inch

99999.999mm

0.0000 to

9999.9999inch

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch 54 to 59

P1 to P48

P48 : G54.1 P48

COOLANT Select valid/invalid of the coolant.

0: Coolant invalid 1: Coolant valid

TOOL CHANGE

POS

Select the tool change position.

1: X axis: Reference position

Z axis: Tool turning clearance position 2: X axis, Z axis: Tool turning clearance position 3: X axis, Z axis: Tool fixed point return position

FIN TOOL RET Select the tool return type after the program end.

1: Reference position 2: Machining end position 3: Specified position

Reference position X

Tool turning clearance X

Tool turning clearance Z

Tool fixed point return position X

0 to 1

1 to 3

C1 C1 1 to 3

Tool fixed point return

END POS X

END POS Z

position Z

Input the tool return position after the program end by using machine coordinate system. This is valid when end tool return type 3 (specified position) is selected.

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

- 38 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

END M CODE At the program end, select the M command to be

Menus

No. Menu Details

← Turns the LIST VIEW area active.

SAVE Saves the changes in the initial conditions.

output.

1 : M30 2 : M02 3 : M99

4.3 Screen Related to the Process Edit Functions

1 to 3

- 39 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.5 Turning Screen

(1) Turning screen

The parameters for the turning process are input on this screen.

Screen layout

Screen display items

No. Display item Details Setting range

TOOL REG No. Input the registration No. of the tool to be used.

Use the No. registered in the tool file.

CYCLE Input the machining method.

<1: Rough machining>

Cuts into the cutting area gradually. Leaves the finishing allowance for the cutting shape.

<2: Finishing machining>

Machines the cutting shape in one cycle.

101 to 150 601 to 650

1,2

- 40 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

PARTS Input the machining area.

4.3 Screen Related to the Process Edit Functions

<1: OD OPEN>

Machines the outer diameter area from the front face of workpiece.

<2: OD CLOSE>

Machines the outer diameter area from the halfway of workpiece.

<3: ID OPEN>

Machines the inner diameter area from the front face of workpiece.

<4: ID CLOSE>

Machines inner area from the halfway of workpiece.

<5: FACE OPEN>

Machines the front face of workpiece.

<6: FACE CLOSE>

Machines the front face from the halfway of workpiece.

[OPEN type]

pproach point

1 to 6

Pe (Cutting shape end point)

[CLOSE type]

Pe (Cutting shape end point)

When the cutting shape is not incremented or decremented monotonously, CLOSE type is selected.

APPRCH POS X Input the approach point.

After machining, the tool returns to the approach point.

APPRCH POS Z

Cutting start point

pproach point

P1 (Cutting shape start point) Cutting start point

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

- 41 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

No. Display item Details Setting range

FINISH ALLOW X

(FX)

FINISH ALLOW Z

(FZ) CUT AMOUNT Input the cut amount for the rough machining. 0.001 to

RETRACT

AMOUNT TOOL T No. Input the turret No. (or ATC No.) of the tool being

CUT SPEED V Input the cutting speed.

FEEDRATE F Input the feedrate.

(Addendum) The tool is retracted as shown below during rough machining.

[OPEN type] [CLOSE type] The tool is retracted in 45˚ direction in

respect to the cutting shape.

Input the finishing allowance for the rough machining. Input both FX and FZ with radius value.

Input the retract amount for the rough machining. 0.0001 to

set, as well as the compensation No. When tool registration No. is specified, tool No. registered in the tool file is automatically set.

When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file and cutting condition file.

When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

The tool is retracted tracing the cutting shape.

pproach point

0.000 to

99999.999mm

0.0000 to

9999.9999inch

99.999mm

9.9999inch 0 to 99999999

1 to 9999 m/min 1 to 9999 feet/min

0.0001 to

999.9999 mm/rev

0.00001 to

99.99999 inch/rev

pproach point

Cutting start point

(Note) Tool path is not provided based on the tool shape (tool nose angle, front edge angle, etc.)

Therefore, when the cutting shape is not incremented or decremented monotonously, take the tool shape into consideration to input the cutting shape.

- 42 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

Menus

No. Menu Details

← Turns the LIST VIEW area active.

PATTERN Machining pattern selection screen is displayed.

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position. If illegal parameters are found in the pattern input screen, the screen name and error will be displayed.

(2) Turning pattern screen

The cutting shapes for the turning process are input on this screen.

Screen layout

Screen display items

No. Display item Details Setting range

No. Shape No. 1 to 50

M Input the shape.

<1> Linear (G01) machining <2> CW circular (G02) machining <3> CCW circular (G03) machining (Note) Not omittable.

- 43 -

1 to 3

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

D Input right turn or left turn in respect to the vector

4.3 Screen Related to the Process Edit Functions

at the end of the previous shape. 1: Left turn 2: Right turn

(Note 1) When nothing is input, it is regarded as

"contacting".

(Note 2) Omittable. However, when the end

point of the previous line, X and Z, is uncertain, always input.

Turn to left Tangent Turn to right

Input the start point of a shape in the line No.1 and the end point of each shape in the line No.2 and after. Specify with diameter value of the program coordinate system for X and with radius value for Z.

1,2

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

(Note 1) Always input the coordinate in the final

line. Omittable except for the line No.1 and the last one.

(Note 2) Always input when the corner shape

dimension is input in the previous line.

R/A • When the shape is arc, input the radius of arc.

Positive value: Arc command smaller than 180° Negative value: Arc command larger than 180°

• When the shape is linear, input the angle.

135°

(Note 1) Always input when the shape is arc. (Note 2) When the shape is linear and the

coordinate X, Z or vector I, K is input, this data is invalid.

Radius:

0.001 to

999999.999mm,

-999999.999 to

-0.001mm Angle:

-359.999 to

360.000°

- 44 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

4.3 Screen Related to the Process Edit Functions

• When the shape is arc, input the arc center coordinate.

• When the shape is linear, input the gradient (vector).

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

I = 40. K = 60.

4060

I = 40. K = 40.

(Note 1) When the shape is arc and only one of

either I or K is input, the other one is regarded as "0".

(Note 2) When the shape is linear and the

coordinate X, Z or angle is input, this data is invalid.

C Input the corner dimension.

Positive value: Corner R Negative value: Corner C

(Note 1) When corner dimension is specified,

input the end point X, Y in the next line in principle.

Menus

No. Menu Details

LINE INSERT Inserts the shape data in front of the cursor position.

(Note) This menu is not available when the cursor is at No.1

(machining start point).

LINE DELETE Deletes the shape data at the cursor position.

(Note) This menu is not available when the cursor is at No.1

(machining start point).

COPY Copies the previous line data at the cursor position.

+INPUT Inputs data at the cursor position with the data in the previous line

added. (Note) This is valid only when inputting the coordinate X and Z.

CLEAR Clears the data at the cursor position.

RETURN Returns to the turning screen.

2060

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

- 45 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.6 Copy Cutting Screen

(1) Copy cutting screen

The parameters for the copy cutting process are input on this screen.

Screen layout

Screen display items

No. Display item Details Setting range

TOOL REG No. Input the registration No. of the tool to be used.

CYCLE Input the machining method.

PARTS Input the machining area.

APPRCH POS X -99999.999 to

APPRCH POS Z

Use the No. registered in the tool file.

<1: Rough machining>

Cuts into the cutting area gradually. Leaves the finishing allowance for the cutting shape.

<2: Finishing machining>

Machines the cutting shape in one cycle.

<1: Outer diameter>

Machine the outer diameter section of the workpiece.

<2: Inner diameter>

Machine the inner diameter section of the workpiece.

Input the approach point. After machining, the tool returns to the approach point.

101 to 150 601 to 650

1,2

1 to 2

99999.999mm

-9999.9999 to

9999.9999inch

- 46 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

MACH ALLOW X

(LX) MACH ALLOW Z

(LZ) FINISH ALLOW X

(FX) FINISH ALLOW

FZ (FZ) NUM OF CUTS Input the number of cuts for the rough

4.3 Screen Related to the Process Edit Functions

Input the allowance in X axis direction with the radius value for the rough machining.

Input the allowance in Z axis direction for the rough machining.

Input the finishing allowance for the rough machining. Input both FX and FZ with radius value.

machining.

0.001 to

99999.999mm

0.0001 to

9999.9999inch

0.000 to

99999.999mm

0.0000 to

9999.9999inch 1 to 99

Menus

TOOL T No. Input the turret No. (or ATC No.) of the tool being

set, as well as the compensation No. When tool registration No. is specified, tool No. registered in the tool file is automatically set.

CUT SPEED V Input the cutting speed.

When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file and cutting condition file.

FEED RATE F Input the feedrate.

When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

No. Menu Details

←

PATTERN Displays the machining pattern selection screen.

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

Turns the LIST VIEW area active.

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position. If illegal parameters are input in the pattern input screen, the screen name and error will be displayed.

1 to 999999

1 to 9999 m/min 1 to 9999 feet/min

0.0001 to

999.9999 mm/rev

0.00001 to

99.99999 inch/rev

- 47 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

(2) Copy cutting pattern screen

The cutting shapes for the turning process are input on this screen.

Screen layout

Screen display items

Refer to the section "4.3.5 Turning Screen (2) Turning pattern screen".

Menus

No. Menu Details

LINE INSERT Inserts the shape data in front of the cursor position.

(Note) This menu is not available when the cursor is at No.1

(machining start point).

LINE DELETE Deletes the shape data at the cursor position.

(Note) This menu is not available when the cursor is at No.1

(machining start point).

COPY Copies the previous line data at the cursor position.

+INPUT Input data at the cursor position with the data in the previous line

added. (Note) This is valid only when inputting the coordinate X and Z.

CLEAR Clears the data at the cursor position.

RETURN Returns to the copy cutting screen.

- 48 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.7 Threading Screen

The parameters for the thread process are input on this screen.

Screen layout

Screen display items

No. Display item Details Setting range

TOOL REG No. Input the registration No. of the tool to be used.

Use the No. registered in the tool file.

CYCLE Input the machining method.

<1: Rough machining>

Cuts into the thread shape gradually. Leaves the finishing allowance for the thread shape.

<2: Finishing machining>

Machines the thread shape in one cycle.

PARTS Input the machining area.

<1: Outer diameter>

Thread the outer diameter area of the workpiece.

<2: Inner diameter>

Thread the inner diameter area of the workpiece.

<3: Face>

Thread the front area of the workpiece.

301 to 350

1,2

1 to 3

- 49 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

CUT METHOD Select the threading cutting pattern for the rough

4.3 Screen Related to the Process Edit Functions

machining.

1: Constant area-normal 2: Constant area-zigzag 3: Constant depth-normal 4: Constant depth-zigzag

[Constant depth-normal] [Constant area-normal]

S in gl e c u tti n g am ou n t S in gl e c u tti n g am ou n t S in gl e c u tti n g am ou n t

[Constant area-z igzag] [Constant depth-zigz ag]

S3 S2 S1

1 to 4

S in gl e c u tti n g am ou n t S in gl e c u tti n g am ou n t

S in gl e c u tti n g am ou n t

S3 S1 S2

ANG OF CUT (A) Input the cutting edge angle for the rough

machining. When the cutting edge angle is set to 0, the zigzag cutting pattern will be invalid.

Cutting edge angle = 0 Cutting edge angle 0

Cutting edge angle

Cutting edge angle 0

PITCH (P) Input the screw pitch. 0.0001 to

HEIGHT (H) Input the thread height.

When selecting a thread type from the menu, thread height can be input automatically based on the pitch.

MET ER

START POS X

(X1) START POS Z

(Z1) END POS X (X2) Input the X coordinate of the threading end point

Input the X coordinate of the threading start point in the diameter value.

Input the Z coordinate of the threading start point.

UNI FY

WIT

PF PT

PIPI NG

NPT

PIPI NG

TRA P.30 °

TRA P.29 °

in the diameter value.

0.000 to

60.000°

999.9999mm

0.00001 to

99.99999inch

0.001 to

999.999mm

0.0001 to

9999.9999mm

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

-99999.999 to

99999.999mm

- 50 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

END POS Z (Z2) Input the Z coordinate of the threading end point. -9999.9999 to

FIN ALLOW Input the threading finishing allowance for the

CUT AMOUNT Input the cutting amount corresponding the

CHM. ANGLE Input the chamfering angle.

CHM. AMOUNT Input the chamfering amount.

TOOL T No. Input the turret No. (or ATC No.) of the tool being

CUT SPEED V Input the cutting speed.

4.3 Screen Related to the Process Edit Functions

rough machining. Chamfered section is machined as continuous thread.

respective methods below for the rough machining.

Maximum cutting amount per cut is input. Cutting amount is calculated according to the

following formula, and the average is taken. Number of cutting cycles =

((Thread height - Threading finishing allowance)/Cutting amount) ↑

↑: Rounded up

Actual cutting amount =

(Thread height – Threading finishing

allowance)/Number of cutting cycles

Initial cutting amount is input. "n" th cutting amount (dn) is calculated according to the following formula. dn = d1( √n - √(n-1) )

d1: Initial cutting amount

0: No chamfering 1: 45

2: 60

Chamfering is not carried out when: Thread angle + chamfering angle > 90°

Chamfered section is machined as continuous thread.

set, as well as the compensation No. When tool registration No. is specified, tool No. registered in the tool file is automatically set.

When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file and cutting condition file.

9999.9999inch

0.000 to

99999.999mm

0.0000 to

9999.9999inch

0.001 to

99999.999mm

0.0001 to

9999.9999inch

0 to 2

0.1 to 9.9 (Number of threads)

1 to 999999

1 to 9999 m/min 1 to 9999 feet/min

- 51 -

4. SCREEN SPECIFICATIONS

Menus

No. Menu Details

← Turns the LIST VIEW area active.

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

4.3 Screen Related to the Process Edit Functions

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position.

- 52 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.8 Grooving Screen

The parameters for the groove process are input on this screen.

Screen layout

Screen display items

No. Display item Details Setting range

TOOL REG No. Input the registration No. of the tool to be used.

201 to 250

Use the No. registered in the tool file.

PARTS Input the machining area.

1 to 3

<1: Outer diameter>

Groove the outer diameter area of the workpiece.

<2: Inner diameter>

Groove the inner diameter area of the workpiece.

<3: Face>

Groove the front area of the workpiece.

WIDTH (W) Input the groove width. 0.001 to

99999.999mm

0.0001 to

9999.9999inch

LEFT CORNER

(LC)

Input the dimension of the left groove corner. Positive value: Corner R Negative value: Corner C

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

Corner R/C cannot be specified for taper grooving.

- 53 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

RIGHT CORNER

(RC)

START POS X

(X1) START POS Z

(Z1) END POS X (X2) Input the X coordinate of the grooving end point

END POS Z (Z2) Input the Z coordinate of the grooving end point.

4.3 Screen Related to the Process Edit Functions

Input the dimension of the right groove corner. Positive value: Corner R Negative value: Corner C Corner R/C cannot be specified for taper

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

grooving. Input the X coordinate of the grooving start point

in the diameter value.

-99999.999 to

99999.999mm

Input the Z coordinate of the grooving start point. -9999.9999 to

9999.9999inch

in the diameter value.

Groove

width

Star t point X1,Z1

Outer

dia.

groove

End point X2,Z2

End point X2,Z 2

Inner

dia.

groove

Start point X1,Z1

Front

face

groove

Start point X1,Z1

NUM OF GRV Input the number of grooves to be machined. 1 to 99

PITCH

Groove pitch

Gr oove pitch direct ion

+ -

Outer

dia.

groove

Front face

groove

Inner

dia.

groove

CUT AMOUNT Input the cut amount. 0.001 to

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

99999.999mm

0.0001 to

9999.9999inch

- 54 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

SHIFT BEFORE

RETR

TOOL T No. Input the turret No. (or ATC No.) of the tool being

TOOL WIDTH Input the tool width of the respective tool.

CUT SPEED V Input the cutting speed.

FEED RATE F Input the feedrate.

Menus

No. Menu Details

← Turns the LIST VIEW area active.

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

4.3 Screen Related to the Process Edit Functions

Specify whether to shift the tool with cutting feed toward the machined area after reaching the groove bottom second or more time. 0: Not shifted 1: Shifted

set, as well as the compensation No. When tool registration No. is specified, tool No. registered in the tool file is automatically set.

When tool registration No. is specified, tool width registered in the tool file is automatically set.

When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file and cutting condition file.

When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position.

0 to 1

1 to 999999

0.001 to

999.999mm

0.0001 to

99.9999 inch 1 to 9999 m/min

1 to 9999 feet/min

0.0001 to

999.9999 mm/rev

0.00001 to

99.99999 inch/rev

- 55 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.9 Trapezoidal Grooving Screen

The parameters for the trapezoidal groove process are input on this screen.

Screen layout

Screen display items

No. Display item Details Setting range

TOOL REG No. Input the registration No. of the tool to be used.

Use the No. registered in the tool file.

CYCLE Input the machining method.

<1: Rough machining>

Cuts into the trapezoidal groove shape gradually. Leaves the finishing allowance for the trapezoidal groove shape.

<2: Finishing machining>

Machines the trapezoidal groove shape in one cycle.

PARTS Input the machining area.

<1: Outer diameter>

Groove the outer diameter area of the workpiece.

<2: Inner diameter>

Groove the inner diameter area of the workpiece.

<3: Face>

Groove the front area of the workpiece.

BASE POS X Input the X coordinate, basic point of the

trapezoidal groove (the bottom center of the trapezoidal groove), in the diameter value.

201 to 250

1,2

1 to 3

-99999.999 to

99999.999mm

- 56 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

BASE POS Z Input the Z coordinate, basic point of the

WIDTH (W) Input the groove width.

DEPTH 1 (H1) Input the left-side depth of the groove. 0.0001 to

DEPTH 2 (H2) Input the right-side depth of the groove.

GRV ANG 1 (A1) Input the angle between the bottom and left-side

GRV ANG 2 (A2) Input the angle between the bottom and

GRV ANG 3 (A3) Input the angle between the left-side of the

GRV ANG 4 (A4) Input the angle between the right-side of the

4.3 Screen Related to the Process Edit Functions

trapezoidal groove (the bottom center of the trapezoidal groove), in the diameter value.

surface of the groove.

right-side surface of the groove.

groove and the workpiece surface.

A3 A4

-9999.9999 to

9999.9999inch

0.001 to

99999.999mm

9999.9999inch

0.000 to 89.999°

-89.999 to 89.999°

E1 E2

A1 A2

H1 H

ENTR L-COR

(E1)

X,Z

B1 B2

Input the left corner amount of trapezoidal groove entrance.

Positive value: Corner R Negative value: Corner C

ENTR R-COR

(E2)

Input the right corner amount of trapezoidal groove entrance.

Positive value: Corner R Negative value: Corner C

BOT L-COR (B1) Input the left corner amount of trapezoidal

groove bottom.

Positive value: Corner R Negative value: Corner C

BOT R-COR (B2) Input the right corner amount of trapezoidal

groove bottom.

Positive value: Corner R Negative value: Corner C

FIN ALLOW Input the finishing allowance of the groove for

the rough machining.

CUT AMOUNT Input the cut amount. 0.001 to

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

0.000 to

99999.999mm

0.0000 to

9999.9999inch

99999.999mm

0.0001 to

9999.9999inch

- 57 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

TOOL T No. Input the turret No. (or ATC No.) of the tool being

TOOL WIDTH Input the tool width of the respective tool.

CUT SPEED V Input the cutting speed.

FEED RATE F Input the feedrate.

Menus

No. Menu Details

← Turns the LIST VIEW area active.

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

4.3 Screen Related to the Process Edit Functions

1 to 999999 set, as well as the compensation No. When tool registration No. is specified, tool No. registered in the tool file is automatically set.

0.001 to When tool registration No. is specified, tool width registered in the tool file is automatically set.

When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file and cutting condition file.

When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position.

999.999mm

0.0001 to

99.9999inch

1 to 9999 m/min 1 to 9999 feet/min

0.0001 to

999.9999 mm/rev

0.00001 to

99.99999 inch/rev

- 58 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.10 Hole Drilling Screen

Miscellaneous parameters related to the hole drilling process patterns are input on this screen. This is displayed when PATTERN menu is pressed on the hole drilling screen.

Screen layout

Screen display items

No. Display item Details Setting range

TOOL REG No. Input the registration No. of the tool to be used.

Use the No. registered in the tool file.

HOLE CYCLE Input the type of hole machining cycle.

<1: Drill> (G83)

The machining is performed as far as the hole bottom at a stretch, and the tool is lifted up after the hole bottom dwell has been executed.

<2: Deep hole> (G83)

The machining is performed halfway of the hole, and the tool is returned to the higher than the hole top position each time. The machining is performed as far as the hole bottom by repeating such operations.

<3: Boring cycle> (G85)

The machining is performed as far as the hole bottom at a stretch, and the tool is lifted up with the cutting feedrate after the hole bottom dwell has been executed.

<4: Tapping> (G84,G84.1)

The tap machining is performed as far as the hole bottom, and the tool is lifted up with the reversed rotation after the hole bottom dwell has been executed.

401 to 450 501 to 550

1 to 4

- 59 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

SURFACE Z (ZF) Input the top surface position of the hole. -99999.999 to

DEPTH (H) Input the hole depth from the workpiece top

NOSE DEPTH (B) Input the nose depth from the workpiece top

SPOT

DIAMETER (D)

CUT AMOUNT When selecting the hole cycle type C=2(deep

DWELL Input the dwell time at the bottom of the hole. 0.0 to 99.999sec

TOOL T No. Input the turret No. (or ATC No.) of the tool being

TOOL DIA Input the tool radius of the respective tool.

CUT SPEED V Input the cutting speed.

FEED RATE F Input the feedrate.

Menus

No. Menu Details

← Turns the LIST VIEW area active.

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

4.3 Screen Related to the Process Edit Functions

99999.999mm

-99999.999 to surface with the addition input method. When the hole depth is changed, tool nose depth will be automatically updated. If the calculated nose depth is 0 or below, the data range will be over.

surface with the addition input method. When the nose depth is changed, hole depth will be automatically updated.

Input the spot diameter. When inputting the spot diameter, hole depth and nose depth are automatically changed.

hole), input the cut amount per cut.

set, as well as the compensation No. When tool registration No. is specified, tool No. registered in the tool file is automatically set.

When tool registration No. is specified, tool radius registered in the tool file is automatically set.

When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file and cutting condition file.

When the type of hole machining cycle is TAP, the pitch (mm/rev) is displayed. When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position.

99999.999mm

-9999.9999 to

9999.9999inch

0.001 to

99999.999mm

0.001 to

Tool diameter

0.001 to

99999.999mm

1 to 999999

0.001 to

999.999mm

0.0001 to

99.9999inch

1 to 9999 m/min 1 to 9999 feet/min

0.0001 to

999.9999 mm/rev

0.00001 to

99.99999 inch/rev

- 60 -

4. SCREEN SPECIFICATIONS

4.3.11 EIA Screen

The EIA process is input on this screen.

Screen layout

4.3 Screen Related to the Process Edit Functions

Screen display item

No. Display item Details Setting range

EIA BLOCK The current contents of the EIA block are displayed.

Menus

No. Menu Details

← Turns the LIST VIEW area active.

INSERT Inserts a blank block before the block where the cursor exists.

DELETE Deletes the data of the block where the cursor exists.

SAVE Saves the changes in the process.

• Characters that can be input into the EIA block are up to 50 characters.

EIA code Max. 10 blocks

- 61 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.12 Milling Hole Drilling Screen

(1) Milling hole drilling screen

The parameters for the milling hole drilling are input on this screen.

Screen layout

Screen display items

No. Display item Details Setting range

TOOL REG

No. PARTS Input the machining area.

Input the registration No. of the tool to be used. Use the No. registered in the tool file.

<1: FACE>

Machines the front face of workpiece.

<2: OUT>

Machines the outer surface of workpiece.

<3: SIDE>

Machines the side surface of workpiece.

Y-axis specifications are required for the side cutting.

Side surface

Front face

701 to 799

1 to 3

Outer surface

- 62 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

HOLE CYCLE Input the type of hole machining cycle.

BASE PLANE

BZ BASE PLANE BR BASE PLANE BA

DEPTH H Input the hole depth from the workpiece top surface

NOSE

DEPTH B

4.3 Screen Related to the Process Edit Functions

<1: DRILL>(G83,G87)

The machining is performed as far as the hole bottom at a stretch, and the tool is lifted up after the hole bottom dwell has been executed.

<2: PECK>(G83, G87)

The machining is performed as far as the middle of the hole, and the tool is returned to the higher position than the hole top each time. The machining is performed as far as the hole bottom with such operation repeatedly executed.

<3: BORE>(G85, G89)

The machining is performed as far as the hole bottom at a stretch, and the tool is lifted up with cutting feed after the hole bottom dwell has been executed.

<4: TAP>(G84, G84.1, G88, G88.1)

The tap machining is performed as far as the hole bottom, and the tool is lifted up with reversed rotation after the hole bottom dwell has been executed.

Set the hole top position in respect to the machining area.

[Front face]

[Side surface]

[Outer surface]

BASE PLANE BZ/BR are switched according to the machining area. BASE PLANE BA is set only for the side cutting.

with an addition input method. When the hole depth is changed, nose depth is automatically updated. If the calculated nose depth is 0 or below, the data is out of the range.

Input the tool nose depth from the workpiece top surface with an addition input method. When the nose depth is changed, hole depth is automatically updated.

1 to 4

Base plane BZ

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch Base plane BR

0.001 to

99999.999mm

0.0001 to

9999.9999inch Base plane BA

-359.999 to

360.000°

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

0.001 to

99999.999mm

0.0001 to

9999.9999inch

- 63 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

SPOT

DIAMETER D

CUT

AMOUNT

DWELL Input the dwell time at the bottom of the hole. 0.0 to

RETURN

POINT

4.3 Screen Related to the Process Edit Functions

Input the spot diameter. When inputting the spot diameter, hole depth and nose depth are automatically changed.

Input the cutting amount per cut when the hole cycle type C=2 (PECK) is selected.

When machining multiple holes, select the height of the tool movement to the next hole position. 1：Initial point level return

2：R point level return

Initial point level return -OUT-

R point level return -OUT-

0.001 to Tool diameter (mm)

0.0001 to Tool diameter (inch)

0.001 to

99999.999mm

0.0001 to

9999.9999inch

99.999sec 1,2

Safe profile clearance

Hole clearance

C-AXIS CLAMP

Initial point level return -FACE-

Safe profile clearance

Select whether to clamp C axis or not in the machining. Select “Clamp C axis” for heavy load machining.

R point level return -FACE-

Hole clearance

0,1

0：Invalid 1：Valid

PATTERN The machining pattern is displayed.

RANDOM LINE ARC CIRCLE SQUARE GRID Change the machining pattern on the machining pattern screen.

TOOL T No. Input the turret No. (or ATC No.) of the tool being set,

0 to 99999999 as well as the compensation No. When tool registration No. is specified, the tool No. registered in the tool file is automatically set.

DIA Input the tool diameter.

When tool registration No. is specified, the tool diameter registered in the tool file is automatically set.

0.001 to

999.999mm

0.0001 to

99.9999inch

- 64 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

CUT SPEED V Input the cutting speed.

FEED RATE F Input the feedrate.

Menus

No. Menu Details

←

PATTERN The machining pattern selection screen is displayed.

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

4.3 Screen Related to the Process Edit Functions

When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file and cutting condition file.

When the type of the hole machining cycle is TAP, the pitch (mm/rev) is displayed. When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

Turns the LIST VIEW area active.

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position.

1 to 9999

m/min

1 to 9999

feet/min

0.0001 to

999.9999

mm/rev

0.00001 to

99.99999

inch/rev

- 65 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

(2) Hole Drilling Pattern Screen

Various parameters for hole drilling patterns are input on this screen. When the [PATTERN] menu is pressed on the hole drilling screen, this screen is displayed.

Screen layout

Machining area and hole machining pattern

The hole machining patterns selectable for each machining area are as follows.

Pattern

Machining area

Front face Outer surface Side surface

Random Line Arc Circle Square Grid

{

{: Selectable, ×: Not selectable

{

- 66 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

Screen display items

No. Display item Details Setting range

PATTERN Input the type of hole machining pattern.

<1: RANDOM>

The machining points are randomly arranged.

<2: LINE>

The machining points are equally spaced on a line.

<3: ARC>

The machining points are equally spaced on an arc.

<4: CIRCLE>

The machining points are equally spaced on a circle.

<5: SQUARE>

The machining points are squarely arranged.

<6: GRID>

The machining points are arranged in grid.

(Note) If the pattern entered is not selectable for the

machining area, the message “E002 Data range over” will appear.

(Note) Display items No.2 and later differ according to each pattern.

1 to 6

- 67 -

4. SCREEN SPECIFICATIONS

・Parameters for RANDOM

Front face Outer surface Side surface

4.3 Screen Related to the Process Edit Functions

No. Display

Details Setting range

item

HOLE No. Input the hole No. 1 to 35

2 3

FACE:

POS X POS Y

OUT:

POS C POS Z

SIDE:

POS Y POS Z

Input the hole position.

[Front face]

[Side face]

y z

[Outer circumference]

180

270

360

X,Y,Z:

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

-359.999 to

360.000

- 68 -

4. SCREEN SPECIFICATIONS

・Parameters for LINE

Front face Outer surface Side surface

No. Display item Details Setting range

FACE:

BASE POS X BASE POS Y

OUT:

BASE POS C BASE POS Z

SIDE:

BASE POS Y BASE POS Z

4.3 Screen Related to the Process Edit Functions

Set the first hole position for the machining area. X,Y,Z:

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch C:

-359.999° to

360.000°

ANGLE (A)

PITCH (A)

Front face:

Input the angle formed with the machining direction and the positive direction of the X axis.

Outer surface:

Input the pitch angle in respect to the machining direction.

Side surface:

Input the angle formed with the machining direction and the positive direction of the Y axis.

PITCH (K) Input the space from the machining point to the

next machining point.

NUM OF

Input the number of holes. 2 to 999

HOLES OMIT 1 to 4 Specify the hole No. to be omitted (deleted).

Maximum hole No. that can be specified is 127.

-359.999° to

360.000°

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

1 to number of holes

- 69 -

4. SCREEN SPECIFICATIONS

・Parameters for ARC

Front face Side surface

4.3 Screen Related to the Process Edit Functions

No. Display item Details Setting range

FACE:

SIDE:

BASE POS X BASE POS Y

BASE POS Y

Input the arc center position. X,Y,Z:

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

BASE POS Z

RADIUS R Input the arc radius. 0.001 to

99999.999mm

0.0001 to

9999.9999inch

START

ANGLE A

Front face:

Input the angle formed with the first

-359.999° to

360.000° machining point and the positive direction of the X axis.

Side surface:

Input the angle formed with the first machining point and the positive direction of the Y axis.

PITCH K Input the angle from the previous machining point

to the next machining point.

NUM OF

Input the number of holes. 2 to 999

-359.999° to

360.000°

HOLES OMIT 1 to 4 Specify the hole No. to be omitted (deleted).

Maximum hole No. that can be specified is 127.

1 to number of holes

- 70 -

4. SCREEN SPECIFICATIONS

・Parameters for CIRCLE

Front face Side surface

4.3 Screen Related to the Process Edit Functions

No. Display item Details Setting range

FACE:

SIDE:

BASE POS X BASE POS Y

BASE POS Y

Input the circular center position. X,Y,Z:

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

BASE POS Z

DIAMETER

Input the circular diameter. 0.001 to

99999.999mm

0.0001 to

9999.9999inch

START

ANGLE A

Front face:

Input the angle formed with the first

-359.999° to

360.000°

machining point and the positive direction of the X axis.

Side surface:

Input the angle formed with the first machining point and the positive direction of the Y axis.

NUM OF

Input the number of holes. 1 to 999

HOLES OMIT 1 to 4 Specify the hole No. to be omitted (deleted).

Maximum hole No. that can be specified is 127.

1 to number of holes

- 71 -

4. SCREEN SPECIFICATIONS

・Parameters for SQUARE

Front face Side surface

4.3 Screen Related to the Process Edit Functions

No. Display item Details Setting range

FACE:

SIDE:

BASE POS X BASE POS Y

BASE POS Y

Input the position of the machining start point. X,Y,Z:

-99999.999mm to

99999.999mm

-9999.9999 to

9999.9999inch

BASE POS Z

X WIDTH I Input the width of the machining point in the X

axis direction.

-99999.999mm to

99999.999mm

-9999.9999 to

9999.9999inch

X NUM OF

HOLES Y WIDTH J Input the width of the machining point in the Y

Input the number of machining points in the X axis direction.

axis direction.

2 to 999

-99999.999mm to

99999.999mm

-9999.9999 to

9999.9999inch

Y NUM OF

HOLES ANGLE A Front face:

Input the number of machining points in the Y axis direction.

Input the angle formed with the machining

2 to999

-359.999° to

360.000°

start direction and the X axis.

Side surface:

Input the angle formed with the machining start direction and the Y axis.

ANGLE B Input the interior angle.

Default value is 90°.

OMIT 1 to 4 Specify the hole No. to be omitted (deleted).

Maximum hole No. that can be specified is 127.

0.001° to

179.999°

1 to number of holes

- 72 -

4. SCREEN SPECIFICATIONS

・Parameters for GRID

Front face Side surface

No. Display item Details Setting range

FACE:

BASE POS X BASE POS Y

SIDE:

BASE POS

BASE POS Z

X WIDTH I Input the width of the machining point in the X axis

X NUM OF

HOLES Y WIDTH J Input the width of the machining point in the Y axis

Y NUM OF

HOLES ANGLE A Front face:

ANGLE B Input the interior angle.

OMIT 1 to 4 Specify the hole No. to be omitted (deleted).

4.3 Screen Related to the Process Edit Functions

Input the position of the machining start point. X,Y,Z:

-99999.999mm to

99999.999mm

-9999.9999 to

9999.9999inch

-99999.999mm to

direction.

99999.999mm

-9999.9999 to

9999.9999inch

Input the number of machining points in the X axis

2 to 999

direction.

-99999.999mm to

direction.

99999.999mm

-9999.9999 to

9999.9999inch

Input the number of machining points in the Y axis

2 to 999

direction.

-359.999° to

Input the angle formed with the machining

360.000°

start direction and the X axis.

Side surface:

Input the angle formed with the machining start direction and the Y axis.

0.001° to

Default value is 90°.

179.999°

1 to number of

Maximum hole No. that can be specified is 127.

holes

- 73 -

4. SCREEN SPECIFICATIONS

Menus

No. Menu Details

LINE INSERT Inserts the hole position in front of the cursor position.

LINE DELETE Deletes the hole position at the cursor position.

COPY Copies the previous line data above cursor to the setting area.

+INPUT Adds the previous line data above cursor to the setting data and inputs

RETURN Returns to the hole drilling screen.

4.3 Screen Related to the Process Edit Functions

This is available only for the RANDOM pattern.

the value to the setting area. This is available only for the RANDOM pattern.

- 74 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.13 Keyway Cutting Screen

(1) Keyway Cutting Screen

The parameters for the keyway cutting are input on this screen.

Screen layout

- 75 -

4. SCREEN SPECIFICATIONS

Screen display items

No. Display item Details Setting range

TOOL REG

No. CYCLE Input the machining method.

4.3 Screen Related to the Process Edit Functions

Input the registration No. of the tool to be used. Use the No. registered in the tool file.

<1: Rough machining>

Cuts into the keyway shape gradually. Leaves the finishing allowance in respect to the keyway shape.

<2: Finishing machining>

Machines the keyway shape in one cycle.

[Rough machining]

Safe profile clearance positon

Keyway clearance

Finishing allowance

701 to 799

1,2

[Finishing machining]

PARTS Input the machining area.

<1: FACE>

Machines the front face of workpiece.

<2: OUT>

Machines the outer surface of workpiece.

<3: SIDE>

Machines the side surface of workpiece.

Y-axis specifications are required for the side cutting.

Side surface

Safe profile clearance position

Keyway clearance + Finishing allowance

1 to 3

Front face

Outer surface

- 76 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

BASE

PLANE BZ BASE PLANE BR BASE PLANE BA

WIDTH W

DEPTH H

4.3 Screen Related to the Process Edit Functions

Set the machining base plane in respect to the machining area.

[Front face]

[Outer surface]

[Side surface]

SZ EZ

BASE PLANE BZ/BR are changed each other according to the machining area. BASE PLANE BA is set only for the side cutting. Input the width and depth of the keyway. An error will occur when the keyway width is smaller than the tool width. Machining path is determined as follows depending on whether Y-axis specifications are provided or not.

Y-axis specifications provided:

When the keyway width exceeds the tool width, cutting is performed with shifting the tool on Y axis.

No Y-axis specifications provided:

Cutting is only executed on the center line of the keyway.

WidthDepth

Base plane BZ

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch Base plane BR

0.001 to

99999.999mm

0.0001 to

9999.9999inch Base plane BA

-359.999 to

360.000°

0.001 to

999.999mm

0.0001 to

99.9999inch

FIN ALLOW Set the finishing allowance in the depth of the keyway.

Rough machining leaves the finishing allowance in respect to the bottom of the keyway.

0.000 to

999.999mm

0.0000 to

99.9999inch

CUT AMOUNT

Input the cutting depth amount of the keyway for the rough machining.

0.001 to

99999.999mm

0.0001 to

9999.9999inch

- 77 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

START

ANGLE SA SHIFT POS SY START RAD

SR START POS SZ END RAD

ER END POS EZ

NUM OF

KEYWAY

4.3 Screen Related to the Process Edit Functions

Refer to the figure of base plane. START ANGLE SA and SHIFT POS SY are switched each other according to the machining area. START RAD SR and START POS SZ are switched each other according to the machining area. END RADIUS ER and END POS EZ are switched each other according to the machining area.

Input the number of keyways.

Start position BZ, end position EZ

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch Start radius SR,

end radius ER, shift position SY

0.001 to

99999.999mm

0.0001 to

9999.9999inch Start angle SA

-359.999 to

360.000° 1 to 9

PITCH Input the pitch if the number of keyways is 2 or more.

RETURN POINT

When the number of keyways is 2 or more, select the height of the tool movement to the next hole position.

1: Initial point level return 2: R point level return

Initial point level return

R point level return

Safe profile clearance

Front face, outer surface

-359.999 to

360.000° Side surface

0.001 to

99999.999mm

0.0001 to

9999.9999inch 1,2

Keyway clearance

- 78 -

4. SCREEN SPECIFICATIONS

No. Display item Details Setting range

C-AXIS

CLAMP

APPROACH

IN AXIS DIR

4.3 Screen Related to the Process Edit Functions

Select whether to clamp C axis or not in the machining. Select “Clamp C axis” for heavy load machining.

0: Not clamp C axis 1: Clamp C axis

When the positioning is performed, the tool moves to the position set in the K-WAY CLEARANCE with rapid traverse. Set “rapid traverse” or “cutting feed” to be performed in the cutting from that set position to the axis direction.

1: RAPID (G00) 2: CUT (G01)

[Rough machining ]

Keyway clearance

pproach in the axis

direction G0/G1

0,1

1,2

[Finishing ma c hining]

Keyway clearance +

finishing allowance

pproach in the axis

direction G0/G1

TOOL T No. Input the turret No. (or ATC No.) of the tool being set,

0 to 99999999 as well as the compensation No. When tool registration No. is specified, the tool No. registered in the tool file is automatically set.

DIA Input the tool diameter.

When tool registration No. is specified, the tool diameter registered in the tool file is automatically set.

0.001 to

999.999mm

0.0001 to

99.9999inch

CUT SPEED V Input the cutting speed.

When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file

1 to9999 m/min

1 to 9999

feet/min and cutting condition file.

FEED RATE

Input the feedrate in the width direction of the keyway. When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

0.0001 to

999.9999

mm/rev

0.00001 to

99.99999

inch/rev

FEED RATE

Input the feedrate in the depth direction of the keyway. When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

0.0001 to

999.9999

mm/rev

0.00001 to

99.99999

inch/rev

- 79 -

4. SCREEN SPECIFICATIONS

Menus

No. Menu Details

←

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

4.3 Screen Related to the Process Edit Functions

Turns the LIST VIEW area active.

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position.

- 80 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

4.3.14 Contour Cutting Screen

(1) Contour Cutting Screen

The parameters for the contour cutting are input on this screen.

Screen layout

Screen display items

No. Display

item

TOOL

REG No.

Details Setting

Input the registration No. of the tool to be used. Use the No. registered in the tool file.

(Continued to the next page)

range

701 to 799

- 81 -

4. SCREEN SPECIFICATIONS

(Continued from the last page)

No. Display

item

CYCLE Input the machining method.

<1: Rough machining>

<2: Finishing machining>

[Finishing the bottom]

[Finishing the side surface]

PARTS Input the machining area.

<1: FACE> Machines the front face of workpiece. <2: OUT> Machines the outer surface of workpiece. <3: SIDE> Machines the side surface of workpiece.

Y-axis specifications are required for the side cutting.

4.3 Screen Related to the Process Edit Functions

Details Setting

In the axis direction: Machines with the tool cutting into the shape. FIN ALLOW FV is left. In the diameter direction: Machines with shifting the tool. FIN ALLOW FH is left.

Finishes the bottom first and then the side surface.

FIN ALLOW FH

Finishing of side surface

ALLOW FV

Finishing of bottom

In the axis direction:

Machines the FIN ALLOW FV in one cycle.

In the diameter direction:

Machines with shifting the tool. FIN ALLOW FH is left.

Finishing of bottom is not executed when FIN ALLOW FV

is set to 0.

In the axis direction:

Machines with the tool cutting into the FIN ALLOW FH.

In the diameter direction:

Machines the FIN ALLOW FH in one cycle.

Finishing of side surface cannot be executed when FIN

ALLOW FH is set to 0

Side surface

Front face

range

1,2

1 to 3

Outer surface

- 82 -

4. SCREEN SPECIFICATIONS

No. Display

item

BASE

PLANE BZ BASE PLANE BR BASE PLANE BA

Set the machining base plane in respect to the machining area.

[Front face] [Outer surface]

[Side surface]

BASE PLANE BZ/BR are switched according to the machining area. BASE PLANE BA is set only for the side cutting.

4.3 Screen Related to the Process Edit Functions

Details Setting range

Base plane BZ

-99999.999 to

99999.999mm

-9999.9999 to

9999.9999inch

Base plane BR

0.001 to

99999.999mm

0.0001 to

9999.9999inch

Base plane BA

-359.999 to

360.000°

TOOL PATH

Input the tool path of the contour shape.

<1: CENTER>

1 to 3

Machines the center of the contour shape.

<2: RIGHT>

Machines the right side of the contour shape.

<3: LEFT>

Machines the left side of the contour shape.

WIDTH W

DEPTH D

Input the machining width and depth of the contour shape. An error occurs when the machining width is smaller than the tool width.

0.001 to

999.999mm

0.0001 to

99.9999inch Machining width cannot be input when CENTER is set as tool path.

FIN ALLOW

FH FIN ALLOW FV

CUT

AMOUNT

Set the finishing allowance in the tool diameter direction and in the tool axis direction. FIN ALLOW FH cannot be input when CENTER is set as tool path.

Input the cutting amount to the tool axis direction. This is not available when CENTER is set as tool path for finishing machining.

0.000 to

999.999mm

0.0000 to

99.9999inch

0.001 to

99999.999mm

0.0001 to

9999.9999inch

- 83 -

4. SCREEN SPECIFICATIONS

No. Display

item

APPROAC H IN AXIS DIR

When the positioning is performed, the tool moves to the position set in the E-ML CLEARANCE with rapid traverse. Set “rapid traverse” or “cutting feed” to be performed in the cutting from that set position to the axis direction.

1: RAPID (G00) 2: CUT (G01)

[Rough machining]

[Finishing machining]

4.3 Screen Related to the Process Edit Functions

Details Setting

range

1,2

Milling clearance

pproach in axis

direction G0/G1

Milling clearance +finishing allowance

TOOL T No. Input the turret No. (or ATC No.) of the tool being set, as

pproach in axis

direction G0/G1

well as the compensation No. When tool registration No. is specified, the tool No. registered in the tool file is automatically set.

DIA Input the tool diameter.

When tool registration No. is specified, the tool diameter registered in the tool file is automatically set.

CUT SPEED V

Input the cutting speed. When tool registration No. is specified, cutting speed is automatically set based on the contents in the tool file and cutting condition file.

FEED RATE

Input the feedrate in the width direction of the groove. When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

FEED RATE

Input the feedrate in the depth direction of the groove. When tool registration No. is specified, feedrate is automatically set based on the contents in the tool file and cutting condition file.

0 to 99999999

0.001 to

999.999mm

0.0001 to

99.9999inch 1 to 9999

m/min 1 to 9999 feet/min

0.0001 to

999.9999 mm/rev

0.00001 to

99.99999 inch/rev

0.0001 to

999.9999 mm/rev

0.00001 to

99.99999 inch/rev

- 84 -

4. SCREEN SPECIFICATIONS

4.3 Screen Related to the Process Edit Functions

Menus

No. Menu Details

← Turns the LIST VIEW area active.

PATTERN Displays the machining pattern selection screen.

CHECKER Displays the checker screen. Select this to check the set data.

SAVE Saves the changes in the process.

If illegal parameters are found in saving, an error will be displayed. When a parameter is incorrectly input, the cursor moves to that parameter position.

(2) Contour cutting pattern screen

The parameters for the contour cutting pattern are input on this screen. When the [PATTERN] menu is pressed on the contour cutting screen, this screen is displayed.

Screen layout

- 85 -

4. SCREEN SPECIFICATIONS

X X

4.3 Screen Related to the Process Edit Functions

Input coordinate system of contour machining shape

Machining area Input coordinate system Remarks

Front face X-Y Outer surface C-Z, Y-Z The input coordinate system can be changed with

Side surface Y-Z

[Front face] [Outer surface]

menu keys.

[Side surface]

z c

- 86 -

mitsubishi M700, M70NAVI Instruction Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Introduction

Precautions for Safety

Disposal

Contents

1. OUTLINE

1.1 System Outline

1.2 Input Procedures

1.3 Screen Configuration

1.4 Starting NAVI LATHE

1.5 Setting up NAVI LATHE

2. FUNCTIONS OF DISPLAY AREA

2.1 LIST VIEW Area

2.2 OPERATION VIEW Area

2.3 Setting Area

2.4 Message Area

2.5 Menu Display Area

3. BASIC OPERATIONS

3.1 Changing Active View

3.2 Changing Screen

3.3 Setting Data

3.4 Switching Windows

3.5 Switching Selection Tags

3.6 Inputting Operations

4. SCREEN SPECIFICATIONS

4.1 Starting NAVI LATHE

4.2 Screen Related to the Program

4.2.1 Program Edit Screen

4.3 Screens Related to the Process Edit Functions

4.3.1 Process List Screen

4.3.2 Operating Process

4.3.3 Process Mode Selection Screen

4.3.4 Initial Condition Setting Screen

4.3.5 Turning Screen

4.3.6 Copy Cutting Screen

4.3.7 Threading Screen

4.3.8 Grooving Screen

4.3.9 Trapezoidal Grooving Screen

4.3.10 Hole Drilling Screen

4.3.11 EIA Screen

4.3.12 Milling Hole Drilling Screen

4.3.13 Keyway Cutting Screen

4.3.14 Contour Cutting Screen