Gsk983m Cnc System User Manual

GSK983M Milling CNC System

User Manual (Volume I: Specifications and Programming)

Kenh

新建图章

3

Foreword Dear user,

We are really grateful for your patronage and purchase of GSK983M milling CNC system made by GSK CNC Equipment Co., Ltd.

This manual consists of two volumes. Volume I mainly describes the

specifications and programming of the system while Volume II operations, all

codes, parameters, I/O interfaces and other appendices.

！ This system can only be operated by authorized and qualified personnel as

improper operations may cause accidents. Please carefully read this user

manual before usage.

All specifications and designs herein are subject to change without further notice.

We are full of heartfelt gratitude to you for supporting us in the use of GSK’s products.

Kenh

cover

Kenh

小小空白

Kenh

小小空白

Kenh

xiaoxiaoxiao

3

CONTENTS

1. GENERAL .................................................................................................................................... 1

1.1 Overview............................................................................................................................................ 1

1.2 Introduction to the Manual............................................................................................................. 1

2. SPECIFICATIONS ........................................................................................................................ 2

3. PROGRAMMING........................................................................................................................ 13

3.1 What Is Programming?................................................................................................................. 13

3.2 Program Make-up .......................................................................................................................... 13 3.2.1 Block ........................................................................................................................................................14 3.2.2 Program word ........................................................................................................................................14 3.2.3 Input format ............................................................................................................................................16 3.2.4 Decimal programming .........................................................................................................................18 3.2.5 Maximum instruction value.................................................................................................................19 3.2.6 Program number ...................................................................................................................................20 3.2.7 Sequence number ................................................................................................................................21 3.2.8 To skip over an optional block............................................................................................................21

3.3 Dimension Word ............................................................................................................................ 23 3.3.1 Controllable axis ...................................................................................................................................23 3.3.2 Set unit ....................................................................................................................................................25

3.3.2.1 Minimum set unit and minimum travel unit..............................................................................25 3.3.2.2 Input unit×10 ..................................................................................................................................26

3.3.3 Maximum travel.....................................................................................................................................26 3.3.4 Program origin and coordinate system............................................................................................26 3.3.5 Coordinate system and origin of processing ..................................................................................27 3.3.6 Workpiece coordinate system............................................................................................................27 3.3.7 Reference (position) point ..................................................................................................................28 3.3.8 Absolute value instruction and incremental value instruction .....................................................29

3.4 Feed Function (F function) .......................................................................................................... 30 3.4.1 Rapid traverse (positioning) function ...............................................................................................30 3.4.2 Cutting feedrate ....................................................................................................................................30 3.4.3 To reduce feedrate to 1/10..................................................................................................................31 3.4.4 Synchronous feed (feed per rotation) ..............................................................................................31 3.4.5 F1 digit feed ...........................................................................................................................................32 3.4.6 Automatic acceleration and deceleration ........................................................................................33 3.4.7 Automatic angle adjustment ...............................................................................................................34

3.4.7.1 Automatic adjustment of inner angle ........................................................................................34 3.4.7.2 Switch of inner arc cutting feedrate ..........................................................................................37

3.5 Preparation Function (G function).............................................................................................. 38 3.5.1 Selection of planes (G17, G18, G19)...............................................................................................40 3.5.2 Positioning (G00) ..................................................................................................................................41

3

3.5.3 Unidirectional positioning (G60) ........................................................................................................42 3.5.4 Linear interpolation (G01) ...................................................................................................................42 3.5.5 Arc interpolation (G02, G03) ..............................................................................................................44

3.5.5.1 Arc interpolation without any additional axis...........................................................................44 3.5.5.2 Arc interpolation with an additional axis...................................................................................48

3.5.6 Sine-curve interpolation ......................................................................................................................48 3.5.7 Thread cutting (G33)............................................................................................................................49 3.5.8 Automatic return to reference point (reference positions G27～G30) ......................................51

3.5.8.1 Check of return to reference point (G27).................................................................................51 3.5.8.2 Automatic return to reference point (G28)...............................................................................52 3.5.8.3 Automatic return from reference point (G29) ..........................................................................53 3.5.8.4 Return to the 2nd, 3rd or 4th reference point (G30) .............................................................55

3.5.9 Dwell (G04) ............................................................................................................................................55 3.5.10 Accurate stop detection (G09).........................................................................................................56 3.5.11 Accurate stop detecting mode (G61) and cutting mode (G64) ................................................56 3.5.12 Coordinate system setting (G92) ....................................................................................................56 3.5.13 Workpiece coordinate system (G54～G59) .................................................................................57 3.5.14 To change workpiece coordinate system by program instruction ...........................................59 3.5.15 Automatic setting of a coordinate system .....................................................................................59 3.5.16 To switch between Inch and metric systems (G20, G21)..........................................................59 3.5.17 Storage travel limit (G22, G23) .......................................................................................................60 3.5.18 Skip function (G31) ............................................................................................................................63

3.6 Compensation ................................................................................................................................ 65 3.6.1 Tool length compensation (G43, G44, G49)...................................................................................65 3.6.2 Tool offset (G45～G48) .......................................................................................................................67 3.6.3 Tool radius compensation (G40～G42) ...........................................................................................74

3.6.3.1 Tool radius compensation function............................................................................................74 3.6.3.2 Offset (D codes) ............................................................................................................................74 3.6.3.3 Offset vector ...................................................................................................................................75 3.6.3.4 Plane selection and vector..........................................................................................................75 3.6.3.5 G40, G41 and G42 .......................................................................................................................75 3.6.3.6 Details about tool radius compensation C...............................................................................77

3.6.4 D and H functions ...............................................................................................................................109 3.6.5 External tool offset.............................................................................................................................. 110 3.6.6 To input offset through program (G10)........................................................................................... 110 3.6.7 Zooming function (G50, G51) .......................................................................................................... 110

3.7 Cycle Machining Function ......................................................................................................... 113 3.7.1 External moving function .................................................................................................................. 113 3.7.2 Fixed cycles (G73, G74, G76 and G80～G89)............................................................................ 114

3.7.2.1 Repeating a fixed cycle .............................................................................................................126 3.7.3 Specifying an origin and Point R in a fixed cycle (G98, G99)...................................................132

3.8 Spindle Function (S function), Tool Function (T function), Miscellaneous Function (M function) and Secondary Miscellaneous Function (B function) ......................... 133

3.8.1 Spindle function (S function) ............................................................................................................134 3.8.1.1 S 2 digits .......................................................................................................................................134

3

3.8.1.2 S 4 digits .......................................................................................................................................134 3.8.2 Constant surface speed control ......................................................................................................134

3.8.2.1 Instructed methods .....................................................................................................................135 3.8.2.2 Spindle speed ..............................................................................................................................135 3.8.2.3 Restraint of maximum rotational speed of spindle ..............................................................135 3.8.2.4 Rapid traverse (positioning) (G00)..........................................................................................136

3.8.3 Tool function (T function)...................................................................................................................137 3.8.4 Miscellaneous function (M function)...............................................................................................137 3.8.5 Secondary miscellaneous function (B function) ..........................................................................138

3.9 Subprogram...................................................................................................................................... 138 3.9.1 Creation of a subprogram .................................................................................................................139 3.9.2 Execution of a subprogram ..............................................................................................................139 3.9.3 Special methods of application........................................................................................................140

3.10 User Macro ..................................................................................................................................... 142 3.10.1 General ...............................................................................................................................................142 3.10.2 Variables.............................................................................................................................................144

3.10.2.1 Indication of a variable ............................................................................................................144 3.10.2.2 Introduction of variables ..........................................................................................................144 3.10.2.3 Undefined variables .................................................................................................................145 3.10.2.4 Display and setting of variable...............................................................................................146

3.10.3 Types of variables ............................................................................................................................146 3.10.3.1 Local variables # 1～# 33 .......................................................................................................147 3.10.3.2 Common variables #100～ #149 , #500～ #509 .............................................................147 3.10.3.3 System variables (for user Macro B)....................................................................................147

3.10.4 Operation instructions .....................................................................................................................160 3.10.4.1 Definition and substitution of variable ..................................................................................160 3.10.4.2 Additive operation .....................................................................................................................160 3.10.4.3 Multiply operation (Macro B option) .....................................................................................160 3.10.4.4 Function (Macro B option) ......................................................................................................160 3.10.4.5 Hybrid operation........................................................................................................................161 3.10.4.6 Changing operational order using [ ] .................................................................................162 3.10.4.7 Accuracy .....................................................................................................................................162 3.10.4.8 Cautions regarding deterioration of precision ....................................................................162

3.10.5 Control instruction ............................................................................................................................163 3.10.5.1 Branch (GOTO) .........................................................................................................................163 3.10.5.2 Repeat (how to select Macro B)............................................................................................165

3.10.6 Creation and storage of user macro body ..................................................................................169 3.10.6.1 Creation of user macro body..................................................................................................169 3.10.6.2 Storage of user macro body ...................................................................................................170 3.10.6.3 Macro statement and NC statement ....................................................................................170

3.10.7 Macro call instruction.......................................................................................................................173 3.10.7.1 Simple calling ............................................................................................................................173 3.10.7.2 Modal calling..............................................................................................................................180 3.10.7.3 Multiple calling...........................................................................................................................181 3.10.7.4 Multiple modal calling ..............................................................................................................181 3.10.7.5 Calling a macro with G codes ................................................................................................182

3

3.10.7.6 Calling a subprogram with an M code .................................................................................183 3.10.7.7 Calling macros with M codes .................................................................................................184 3.10.7.8 Calling a subprogram with a T code.....................................................................................185 3.10.7.9 The position of the decimal point of an independent variable ........................................185 3.10.7.10 The difference between M98 (calling a subprogram) and G65 (calling a macro body) ...............................................................................................................................................186 3.10.7.11 The nesting and local variables of user macro ................................................................186

3.10.8 The relationship with other functions ...........................................................................................187 3.10.9 Special codes and words used in user programs .....................................................................189 3.10.10 Restrictions......................................................................................................................................190 3.10.11 Descriptions for P/S alarm ...........................................................................................................191 3.10.12 Examples of user macros ............................................................................................................191

3.10.12.1 Groove machining ..................................................................................................................191 3.10.13 External output instructions .........................................................................................................193

3.10.13.1 OPEN instruction: POPEN ...................................................................................................194 3.10.13.2 Data output instruction BPRNT DPRNT ...........................................................................194 3.10.13.3 Close instruction PCLOS......................................................................................................195 3.10.13.4 Necessary settings for using the function.........................................................................195 3.10.13.5 Cautions ...................................................................................................................................195

3.10.14 Macro interruption function (Macro B).......................................................................................196

3.11 Tool Life Management............................................................................................................... 196 3.11.1 Setting of tool groups.......................................................................................................................196 3.11.2 Setting in machining processes ....................................................................................................198 3.11.3 Performance of tool life administration ........................................................................................200

3.11.3.1 Tool life calculation....................................................................................................................200 3.11.3.2 Tool change signal and tool change reset signal...............................................................200 3.11.3.3 New tool selection signal.........................................................................................................201 3.11.3.4 Tool skip signal ..........................................................................................................................201

3.11.4 The display and input of tool data.................................................................................................201 3.11.4.1 The display and modification of tool group number ..........................................................201 3.11.4.2 The display of tool life data during the execution of machine program ........................201 3.11.4.3 Presetting tool life counter ......................................................................................................202

3.11.5 Other cautions ...................................................................................................................................203

3.12 The Indexing Function of Indexing Worktable ..................................................................... 203 3.12.1 Instructing methods .........................................................................................................................203

3.12.1.1 Input unit .....................................................................................................................................203 3.12.1.2 Absolute / incremental instruction .........................................................................................203 3.12.1.3 Concurrently controlled axes .................................................................................................204

3.12.2 Minimum travel unit: 0.001 degree/pulse....................................................................................204 3.12.3 Feedrate .............................................................................................................................................204 3.12.4 The clamping and release of indexing worktable......................................................................204 3.12.5 Jog/step/handwheel.........................................................................................................................205 3.12.6 Other cautions...................................................................................................................................205

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

1

1. GENERAL

1.1 Overview

As a high-accuracy and high-performance closed-loop CNC system with firmware, GSK983M milling CNC system (hereinafter called “System”) was newly developed and launched by GSK CNC Equipment Co., Ltd. to satisfy the demands of NC market and intended for CNC milling machine and processing center. By employing a high-speed microprocessor, a general large scale integrated circuit (LSI), a semiconductor memory and up-to-date storage elements, the reliability as well as performance-to-price ratio of its control circuit are greatly improved, thereby facilitating the reliability, functions/ performance to price ratio to a large extent.

With a widely applicable advanced servo, GSK983M milling CNC system uses a high-duty pulse encoder as its detecting element, thereby composing a closed-loop CNC system.

This operating manual describes all available functions of the system. However, a real unit may not necessarily be provided with all the optional functions. Should the specifications of the control panel and operating mode of the machine change, the instruction manual supplied with the machine by the manufacturer shall be referred to.

1.2 Introduction to the Manual

The functions of a NC machine system are not only dependent on its NC, but also on its mechanical part. That is to say, its heavy current circuit, servo system, NC and mechanical operation panel jointly determines its performance. The manual only gives a general account from the angle of NC as it is difficult to describe all the functions of an NC machine and programming and operating procedures in detail. As for a specific NC machine, please refer to the instruction manual supplied with the machine by the manufacturer. The contents of the machine instruction manual are more important than those herein.

The performance of a NC machine system is jointly determined by its NC system, mechanical structure, heavy current control and servo system including its mechanical operation panel. The operating manual only describes GSK983M CNC system. To know the performance, programming and operating instructions of the entire NC machine system further, please refer to the machine instruction manual supplied by the manufacturer.

The operating manual describes all matters in detail as much as possible. However, the listing of all matters is unnecessary and impossible as this will complicate the contents of the manual. Therefore, the functions that are not described in this manual may be considered impractical.

The functions that are not described in this manual may be deemed unavailable so far.

Some items are specifically explained in Note sections. Therefore, if any explanation is not available in the current Note section, it is advisable to skip over it, thoroughly read the manual and then return to the part.


2

2. SPECIFICATIONS

Serial No.

Designation Descriptions

1 Controllable axes

Standard: 3 axes, namely axes X, Y and Z (4 or 5 axes are also available upon customer’s request. The address of the 4th axis can be selected from A, B, C, U, V or W. That the 4th axis is linear or rotary may be set by parameters. The address of the 5th axis can be designated as U, V, W, A, B or C. It is possible to specify whether the 5th axis is linear or rotary by parameters.)

2 Number of concurrently

controllable axes

Standard: 3, axis 3, link, (The following configurations are also available upon customer’s request: 4, axis 3, link; 4, axis 4, link; 5, axis 3, link; and 5, axis 4 and link.)

Min. set increment 0.001mm 0.0001 inch 0.001°

Min entered increment 0.001mm 0.0001 inch 0.001° 3 Incremental system

The minimal increment entered in accordance with parameter setting metric system may be 0.01mm.

4 Bit detecting device Pulse encoder

5 Max. instruction value ±99999.999 mm ±9999.9999 inch ±99999.999°

6 Input format Changeable block, character and address formats are employed.

7 Decimal point programming

It is possible to enter numerical values including a decimal point. The addresses that may include a decimal point are X, Y, Z, A, B, C, U, V, W, I, J, K, Q, R and F.

8 Rapid traverse Axial speed can be up to 24,000m/min or 960 inch/min. In addition, rapid traverse speed may be changed to FO，25，50 or 100% using rapid traverse override (optional).

9 Miscellaneous function

(Bit M2)

Feedrate can be set within the following ranges: 1 mm/min～15,000mm/min and 0.01inch/min ～ 600.00 inch/min. It is possible to set the upper speed limit of cutting feed by parameters. A feedrate may be selected from 0 to 200% by setting the override of feedrate to 10% as a step. The unit of feedrate may be changed to 0.01 mm/min, 0.001 mm/min or 0.001 inch/min according to parameter setting.


3

10 Automatic

acceleration/deceleration

Both manual rapid traverse and automatic rapid traverse are performed in linear acceleration/deceleration mode so as to reduce positioning time.

11 Absolute/incremental

value instruction

G codes may be used to select absolute or Incremental programming. G90: Absolute programming G91: Incremental programming

12 Coordinate system

setting (G92)

When the instruction value for subsequent axes of G92 is used to establish a coordinate system, the actual position of cutting tool will become the instruction value for the coordinate system.

13 Positioning (G00)

All axes individually move to the end point rapidly and decelerate until stop through instruction G00, and the machine performs positioning (whether the machine reaches the instructed position) detection by parameters setting.

14 Linear interpolation

(G01) Linear interpolation may be conducted at the feedrate specified by F codes using instruction G01.

15 Buffer register

When executing a block, the unit reads the next one in buffer register in advance. In this way the intermittence of the NC instruction operation caused by the time required for reading may be avoided. While inputting data in buffer register, BUF will appear on the lower right of LCD screen.

16 Dwell (G04) The operation of the next block can be delayed before execution using instruction G04. The delay time must be specified with address P or X.

17 Accurate stop detection

(G09) The block of instruction G09 decelerates and performs positioning detection by the end of the block.

18 Accurate stop detecting

mode/cutting mode (G61, G64)

If G61 is instructed, the travel instructions following G61 decelerate from doubtful points of all blocks and continue to execute the next block when it is positioned. If G64 is instructed, the travel instructions following G64 rather than positioning instruction do not decelerate but execute the following blocks. As a rule, they are applicable for cutting mode.

19 Miscellaneous function

(Bit M2)

The instructions of M2 with 2 digits following may be used to control the ON/OFF signal on machine side. Only one M code can be instructed in one block.

20 Dry run

In dry running mode, feedrate becomes Jog (JOG) feedrate. The rapid traverse speed keeps constant and rapid traverse override (option) is still valid in rapid traverse instruction (G00). However, the dry running of instruction is available when it is set to rapid traverse (positioning) according to parameters.


4

21 Interlock

It is possible for all axes to individually disable the feed of an instructed axis. If any instructed axis in interlocked during traveling, all axes of the machine will decelerate until stop. Once the interlock signal is cancelled, the machine will accelerate and restart.

22 Single block A block instruction can be executed each time.

23 To skip over an optional

block

The block preceded by a “/” (slash) code may be ignored by turning on the OPTIONAL BLOCK SKTP switch on the machine side.

24 External mirroring

The switch may be used to reverse the program instructions of axes X and the 4th axis as well as the travel of MDI. It is possible to set mirroring with the MDI/LCD panel or the switch on the machine side.

25 Manual Absolute Value

ON/OFF

It is possible to determine whether to add the traveling amount through the manual traveling tool to absolute coordinates by switching the manual absolute value switch on the machine side. Manual Absolute Value switch ON: To add; OFF: Not to add.

26 To lock auxiliary function BCD code signal and strobe signal of M, S, T and B are sent to the machine side.

27 To lock the machine The machine keeps still. However, position display is still valid as the machine is moving and machine locking is also valid even in the execution of a block.

28 To cancel the instruction

for axis Z The function is only equivalent to Z-axis locking. It is to be used when NC program is checked by drawing a picture with a pen.

29 To feedrate feed

The function is used to temporarily stop the feed of all axes that can be restarted by pressing Cycle Start button. Before the restart of feed, it is possible to insert manual operation in manual mode.

30 To cancel override The function is used to fix the cutting feedrate at 100% depending on the signals from the machine side.

31 Emergent stop By pressing the Emergent stop button all feed instructions stops (interrupt immediately) and the machine stops running at the same time.

32 External reset, reset

signal

The function is used to reset NC from the outside of NC. The signal stops all feed instruction and the machine decelerates until stop by reset. Additionally, the Reset button on MDI/LCD outputs reset signals to the machine side during emergent stop and external reset.


5

33 Overtravel

The moving parts of the machine receives arriving signal when they come to the end of travel. Then the movement of axis decelerates until stop and overtravel warning is displayed at the same time.

34 NC Ready signal When the power supply is switched on, NC gives the signal in controllable state. It stops sending signals to the machine side once the power supply is cut off or the control unit overheats.

35 Servo Ready signal

When the servo system is ready, the signal is sent to the machine side. For the axis to be braked, it is locked when the signal has not been given off. LCD displays NO READY in the absence of the signal.

36 NC warning signal The signal is sent out when NC is in warning state.

37 Distribution Completed

signal

NC outputs the signal when the motion order ends up. If the functions of M, S, T or B and motion instruction are active in a block, the signal is given after the completion of the execution of traveling instruction and the functions of M, S, T or B can be executed.

38 Cycle Operation signal NC gives the signal in cycle operation.

39 Cycle Operation Start

Indicator signal NC sends out the signal at the start of cycle operation.

40 Feed Hold Indicator

signal NC outputs the signal when it is in holding state through feed hold.

41 Manual continuous feed

(1) JOG feed: For JOG feedrate, the rotary switch may be used for 24-step switching. The ratio of 24-step is geometric progression.

(2) Manual rapid traverse: Rapid traverse may also be achieved by manual means. Rapid traverse override may be used for the rapid traverse speed set by parameters. Rapid traverse override is an optional function.

Manual continuous feed is available for 2 axes at one time.

42 Incremental feed

Since the following increments may exert positioning control, manual positioning can be performed efficiently. Incremental feed is available for 2 axes at one time (incremental feed amount).

43 Sequence number

searching It is possible to search the sequence numbers in the currently selected program with the MDI/LCD panel.

44 Program number

searching It is possible to search the program numbers of 4 digits following O with the MDI/LCD panel.


6

45 Clearance compensation It is this function that compensates the lost amount of movement of the machine. The amount of compensation is set in the minimum amount of movement within 0 ~ 255 by parameters.

46 Program key locking The function disables the display, setting and editing of the program with a program number of 9000～9899 by means of key locking.

47 Environmental

conditions

(1) Ambient temperature 0℃～45 for operation and ℃ -20℃～55 for storage and ℃

shipment. (2) Relative humidity

≤90%(without condensation), ≤95%(40 )℃ (3) Vibration

Less than 0.5G for operation and 1G for storage and shipment

(4) Ambient air To install an NC in an environment with high density of dust, machining fluid and organic solvent, contact the manufacturer.

48 Self-diagnostics

(1) Servo system a. To give an alarm when the error of the error register

goes beyond the setting in halted state. b. To give an alarm when the value of the error register

goes beyond the maximum setting. c. To give an alarm in case of malfunction of positioning

detection system. d. To give an alarm when the drift voltage is excessive. e. To give an alarm in case of malfunction of speed control

unit. (2) NC

a. To give an alarm in case of malfunction of the memory. b. To give an alarm in case of malfunction of ROM and

RAM. c. To give an alarm in case of malfunction of the

microprocessor. (3) Status display

a. To display the status of NC on LCD. b. To display the status of I/O on LCD.

49 S function/T function

(BCD2 bit)

Once the instructions of 2 digits following S and T are instructed, the code signal of BCD2 bit may be sent out while codes S and T ad other codes are individually output. They are reserved until the following S and T are instructed.


7

50

S4 Bit (binary 12-bit output)

A/S4 Bit (analog output) A

The binary 12-bit or analog voltage corresponding to the speed of principal axis is output to the machine side. The analog voltage is up to ±10V, 2mA and the speed (r/min) of principal axis is directly specified by S4 Bit. The speed of principal axis may be regulated in the following range depending on the contact signal on the machine side: 50, 60, 70, 80, 90, 100, 110 and 120%.

51

S4 Bit (binary 12-bit output)

A/S4 Bit (analog output) B

When the speed (r/min) of principal axis is directly specified, the voltage for the current speed of principal axis is output by the presently selected gear numbers 1 to 4.The switching of gear is performed in a heavy-current circuit, resulting that the signal of GRA or GRB is input in NC side. As the judging message for switching gears on the heavy-current side, NC outputs the higher 2 bits or lower 2 bits of S4 bit in BCD codes.

52 Thread cutting

/synchronous feeding

A position coder is installed on the principal axis. It is possible to perform thread cutting using the pulse synchronous speed of the position coder.

53 Position coder

To achieve the feed that is in step with the rotation of the principal axis, a device that may generate pulse voltage of which frequency is proportional to the number of revolutions of the principal axis and generates 1024 pulses in each rotation shall be directly connected.

54 Constant surface speed

control

Generally surface speed is instructed with B codes. In this way the principal axis accordingly changes when the position of the tool changes so that its surface cutting speed is always equal to the linear speed set by S codes.

55 Second auxiliary function

(B3 bit)

Address B is followed by three digits. Once it is instructed, a BCD three-bit code signal will be sent out to position the index table.

56 T-function (BCD4 bit)

Addresses S and T are followed by a 2-digit instruction. Once they are instructed, the code signal of BCD2 bit will likely to be sent out and other codes of the addresses S and T are individually sent out and held until the next S and T are instructed.

57 Code standards ISO codes (ISO840) and EIA codes (EIA RS-244-A) can be used for program code. The identification of ISO codes and EIA codes may be performed automatically.


8

58 Rapid traverse override The automatic or manual rapid traverse speed can be set in 4 levels, i.e. FO, 25, 50 and 100% and FO is likely to be set to a specific speed by parameters.

59 Return to reference point

A

Return to reference point A consists the following procedures: (1) Manual return to the reference point; (2) Examination of the return to the reference point (G27); (3) Automatic return to the reference point (G28).

60 Return to reference point

B

Besides the functions of returning to reference point A, the return to reference point B also includes the return to the 2nd reference point (G30).

61 Return to the 3rd and 4th

reference points

It is possible to set the 3rd and 4th reference points by setting their distances from the 1st reference point and return to these reference points.

62 Storage travel limits 1

and 2

For storage travel limit 1, the area beyond those set by parameters are exclusion areas. For storage travel limit 2, the inside or outside of the area specified by parameters or programs are exclusion areas. The validity or invalidity of storage travel limit 2 is set by G codes. G22: Valid G23: Invalid

63 Memory type pitch error

compensation

The function is designed to compensate the pitch error caused by the mechanical wear of the feed screw so as to maximize processing accuracy and mechanical life. Compensation data is saved in memory, thereby omitting the compensation mechanism such as the stop and the relevant setting operations.

64 The selection of a

workpiece coordinate system

It is possible to preset one of the 6 workpiece coordinate systems using six G codes, i.e. G54～G59 and subsequent programming can be made in the selected coordinate system.

65 Tool offset (G45～G48)

Tools can be offset using instructions G45～G48. Tool offset refers to the side-play mount corresponding to a move instruction’s elongation or reduction of an instruction of D or H codes in axial direction. D or H codes may instruct 1～32 and the maximum offset shall be ±999.999mm or ±99.999 inches. G45: To increase the set value; G46: To reduce the set value; G47: To increase the set value by twice; G48: To reduce the set value by twice.


9

66 Automatic setting of a

coordinate system

To manually return to a reference point, parameters must be preset to establish a coordinate system, namely automatic execution is similar to the condition that the instruction G92 is used at the reference point.

67 Tool length offset (G43,

G44, G49)

Tool length offset (tool length compensation) is possible in the direction of the axis Z using instructions G43 and G44. The offset number must be selected within 01～32 using H codes. The offset shall fall within ±999.999mm or ±99.999 inches.

68 Tool radius

compensation B, C (G40～G42)

Tool radius compensation is possible using instructions G40～G42. The offset number must be specified within 01～32 using D codes. The offset shall fall within ±999.999mm or ±99.999 inches. Cutter compensation B is unavailable for a tool of a medial angle less than 90°. Cutter compensation 0 can be used for the tool of a medial angle less than 90°.

69 Tool length

measurement

Manually position the standard tool to the fixed point of the machine tool. Then manually position the machine tool to be measured to the same mechanical point. The length compensation of the tool will be input as offset once z INPUT is pressed.

70 Tool life management

function

Divide the tools in the cutting tool room into several groups and specify service life for each group of cutting tools. Accumulate the tool processing time or processing number that serves as the evaluation standard for tool life whenever a tool in the groups is used. The next cutting tool in the predetermined sequence is automatically selected in the same group when the tool reaches its service life.

71 Additional offset memory

A The numbers of tool offset and tool radius compensation may be increased to 64.


B The numbers of tool offset and tool radius compensation may be increased to 99.


C The number of cutter compensation is increased to 200.

74 F1- bit feed

Once the number of F followed by one digit of 1~9 is instructed, the feedrate corresponding to the number will be set. The instruction FO is a rapid traverse speed. The feedrate of the currently selected number can be increased or reduced by turning the manual pulse generator when the machine side gives a speed-changing signal.


10

75 External moving function

(G80, G81) Instruction G81 is used to output external movement signals after the positioning of X and Y axes and G80 to cancel it.

76 Fixed cycle A (G80, G81, G82, G84, G85, G86 and

G89)

It is possible to perform 6 fixed cycles including drilling cycle, tapping cycle and boring cycle.

77 Fixed cycle B (G73,

G74, G76, G80～G89)

It is possible to perform 12 fixed cycles including gun drilling cycle, finish boring cycle, tapping cycle and reverse-tapping cycle.

78 Switch between Inch and

metric systems (G20, G21)

Input in Inch or metric system can be selected by switching G codes. G20: Input in Inch system G21: Input in metric system

79 Arc interpolation (G02,

G03)

Using G02 (or G03) may achieve any arc interpolation within 0～360° with the feedrate of F code instruction. G02: Clockwise (CW) G03: Counterclockwise (CCW)

80 Sine-curve interpolation

When an axis in the arc plane does not move (the axis is considered as an imaginary axis) in the spiral-curve interpolation instruction, the other 2 axes may be used for sine-curve interpolation.

81 The arc interpolation using arc radius R for programming

In arc interpolation, directly specifying radius with radius value R rather than I, J and K simplifies programming. An arc over or below 180° can be instructed.

82 External deceleration The mechanical vibration at the end of travel can be minimized and the range of effective travel maximized through the function. External deceleration is not applicable for an additional axis.

83 External workpiece number search A

The function is used to input any program number among 1～31 for NC from the outside such as machine side and to select these programs from the memory of NC.

84 External data input

The function is used to transmit the following data from the outside such as machine side: (1) External workpiece number search C; (2) External cutter compensation C; (3) External warning message; (4) External operation information.

85 Automatic acceleration/ deceleration of cutting

feed

Cutting feed and manual continuous feed can be set by parameters to make power type acceleration/ deceleration in 8ms～4000ms time constant.


11

86 Additional skipping over

selected blocks

9 switches for skipping over selected blocks can be set on machine side by adding a digit (1~9) after the switching instruction”/” of a block. When a switch n for skipping over selected blocks is enabled, the blocks with “/n” will be skipped over.

87 Skip function (G31)

When G31 is followed by X, Y, Z, the 4th or 5th axis instruction as same as G01, it is possible to make line interpolation. If skip signal is input from the outside during the execution of the instruction, the remaining part of the instruction stops executing and the blocks that follow will be executed.

88 Program restart When the sequence number to be restarted is specified, the program will restarts from here.

89 Unidirectional positioning Positioning can only be performed in one direction in order to eliminate clearance and achieve accurate positioning.

90 Addition of the number of

storable programs 96 programs can be added to the standard programs to reach 191 programs in total.

91 Zoom The tool path instructed in a program can be zoomed in a range of 0.001～99.999x.

92 Insertion of a manual

tray

The tool movement overlapping an automatic running instruction can be done only with the pulses of the manual pulse generator without processing interruption.

93 Automatic angle

adjustment

When cutting the inner side of an angle in tool radius compensation mode, adjustment can be automatically added in the set area for processing at low speed.

94 Manual feed at any

angle

The function is used to set the angle of the positive direction of axis X on the dial gauge of the operation panel of the machine and to make Jog feed in the set direction. In the XY plane, this function is only valid for the increment of 5° spacing within 0°～360° range.

95 Sequence number comparison stop

Once the block with the same sequence number as the preset one appears in the execution of a program, a single block will be in stop status when the execution of the program ends. The function is used to check a program.

96 Indication of running time The NC automatic running time can be indicated on LCD in seconds, minutes and hours.

97 Menu switch The ON/OFF can be controlled by using the settings on MDI/LCD rather than the switches on the operation panel on the machine


12

98 User macros

A and B These are the intrinsic functions available for manufacturer and user and types A and B are provided due to functional limits.

99 Graphic display The tracks of cutting tools are traced out on LCD.

100 Manual pulse generator

The manual pulse generator on the operation panel can be used to perform Jog feed of the machine. The manual pulse generator sends out 100 pulses each turn. The travel of each pulse can be switched between 1x, 10x and 100x depending on the signals on the machine side.

101 PLC

PLC MODELS A and B are available.

PLC MODEL-A PLC MODEL-B

Quantity of input points

192 points 192 points

Quantity of output points

128 points 128 points

Program step Up to 2,000

steps Up to 5,000 steps


13

3. PROGRAMMING

3.1 What Is Programming?

NC processing machine operates by developed programs. To process a part on the NC machine,

the route and other processing conditions of cutting feed shall be included in the program. The

program is called “part program”.

The following diagram indicates the processes from preparation of detail drawing to NC’s

execution of the processing program.

Detail drawing Processing plan Part programming NC’s execution of processing program

Part program is an NC instruction for controlling feed route and the auxiliary movement of a machine written according to the rules for NC. The instructions are usually written in a program list.

This chapter will describe how to develop a part program.

3.2 Program Make-up

A program consists of main program and subprogram. As a rule, NC moves by the instructions of a main program. When the main program gives an instruction to switch to a subprogram, NC moves by the subprogram.

When there is an instruction to return to a main program in a subprogram, NC will return to the main program and continue to move by the instructions of the main program.

NC memory can store 95 main programs and subprograms in total. When one of the main programs is selected, NC machine can move by its instructions.

(1) Determine the NC processing range and select an NC machine to be used. (2) Determine the assembling method of the workblank on the machine and select a

necessary clamping device and a tool. (3) Determine the cutting sequence (process type, home point of the cutting tool, the cut

depths of rough cutting and finish cutting and route of cutting feed). (4) Select a cutting tool and a tool clamping device and determine the mounting position on

the machine. (5) Set cutting conditions (spindle rotating speed, feed speed and whether to use cooling

fluid, etc).


14

Main program Subprogram

Note: The number of programs that can be stored will be increased to 191 if the function “Addition of the number of storable programs” (Optional) is selected.

Refer to Chapter 4: Operations for the storage method of program.

3.2.1 Block

A program is composed of a number of instructions. Each instruction unit in a program is called a block. Blocks are distinguished from each other by end code. As described below, end-of-block code is indicated with a “;”.

For example:

XXXX; XXXX; XXXX;

Note 1: The maximum number of characters a block is not limited in.

Note 2: End-of-block code: CR for EIA codes and LF for ISO codes.

3.2.2 Program word

The elements composing a block are program words. The program word below consists of an address and a subsequent figure. A “+” and a “ –“ can also be added before the figure.

X - 1000 Address Figure

Program word

An address is indicated with a letter among A～Z. An address determines the meaning of its subsequent figure. The addresses that can be used in an NC and their meanings are as follows. An address may have different meanings depending on different instructions of preparation

Instruction 1

Instruction 2

┊

┊

┊

┊

[Instruction to switch to a subprogram]

Instruction n

Instruction n+1

┊

┊

┊

┊

┊

Instruction 1

Instruction 2

┊

┊

┊

┊

┊

┊

┊

┊

┊

┊

┊

[Instruction to return to a main program]


15

function in a program.

Name Address Meaning

Program No. : (ISO) /O (EIA) Program number

Sequence No. N Sequence number

Preparatory function

G Instructed move mode (linear, arc, etc)

X, Y, Z Move instruction of coordinate axis

A, B, C, U, V, W Move instruction of additional axis

R Arc radius Coordinate word

I, J, K Coordinates of arc center

Feed function F Designation of feedrate

Spindle function S Designation of spindle rotational speed

Tool function T Designation of tool number and tool offset number

M Designation of ON/OFF control on machine side Auxiliary function B Worktable indexing, etc.

Offset No. H, D Designation of offset number

Dwell P, X Designation of dwell time

Designation of program No.

P Designation of subprogram number

Designation of sequence No.

P Designation of sequence number: Program is repeatedly executed at this sequence number.

Number of repetition

L Numbers of repetition of subprogram and fixed cycles

Parameter P, Q, R Parameters of fixed cycle

For example, these program words may compose the following block.

； N— G— X— Y— F— S— T— M— ；

SequencN

o.


Coordinate N

o.

Feed function

Spindle function

Tool function

Miscellaneous


16

In the following program list, a line indicates a block and a case in the block indicates a program word.

Name S57.10.10 Page/Program No. 0 (: ) 2002

/ N G X Y Z A/B/C

C/V/W

R/I J K F S T M B H/D

L P Q ；

N20 G92 X 100.0

Y 200.0

Z 300.0

；

N21 G00 X 196.0

Y 315.0

Z 500.0

S400

T15

M03 ；

N22 G01 F10.0

；

(Note ) CR(EIA)，LF(ISO)

3.2.3 Input format

All program words composing a block shall be instructed in the formats as specified below. The input format of this system is a variable block format. Therefore, the number of the program words in a block and the number of characters in a program word are variable, which makes programming easier.

(1) Input in metric system

NO4·G02·XL+053·YL053·ZL+053·

RD053 D02 αL+053·βL+053· ·F050· ·

ID053·JD053·KD+053 H02 S02 T02

· ·B03·M02; S04 T04

(2) Input in Inch system

NO4·G02·XL+044·YL+044·ZL+044· RD044 D02

αL+053·βL+053· ·F032· · ID044·JD044·KD044 H02

S02 T02 · ·B03·M02；


17

S04 T04 Note 1: α and β are for any one of A, B, C, U, V and W.

Note 2: The address and digits in the above formats have the following meanings. X L + 0 5 3

The three digits behind decimal point The five digits before decimal point Leading zero may be omitted. With a symbol Absolute value or incremental value Address

J D 0 5 3 The three digits behind decimal point The five digits before decimal point Leading zero may be omitted. Incremental value with a symbol Address

For example: When a cutting tool moves to 50.123mm along X axis, its move instruction is as follows:

G00 X50 123 The three digits behind decimal point

The five digits before decimal point: 00050 The leading zero and T are omitted. G00 must not be omitted even the leading zero may be omitted. (G00 specifies rapid traverse (positioning)).

Note 3: When an address word in a block is instructed twice or more times, the last instruction will be

valid and not give any alarm in principle.

For example: G01 M03 S200 M08;

Now M08 is valid and M03 invalid. For G codes, the lastly specified one in each group of G codes in a block is valid. However, G90/G91 is only valid at the specified location in a block (see Section 3.3.8.).

Example G90 X10.0 G91 Y20.0 ；

Absolute Incremental

If R and I, J or K are concurrently instructed in an arc interpolation instruction, R is always valid and this is not related to instruction sequence.

Note 4:F050 in Inch-system input format may also be changed into F051 through parameter switching. Refer to Section 3.4.3 “To multiply feedrate by 1/10”.

Note 5: Since P and Q have a number of meanings, they are omitted in the above format.

Note 6: Refer to Section 3.2.4 ”Decimal entries”.


18

Note 7: Multiply the value input in metric system of X, Y, Z, A, B, C, U, V, W, I, J, K, Q and R by 10 by means of parameter setting.

RD052

XL+052·YL+052·ZL+052·αL+052·βL+052· ID052·JD052·KD052

(α and β are A, B, C, U, V and W) (Input in metric system) Refer to Section 3.3.2.2 “To multiply an input unit by 10”.

Note 8: Refer to Section 3.3.2.2 “To multiply an input unit by 10”.

3.2.4 Decimal programming

It is possible for this unit to input the numerical values with a decimal point. Decimal point is used in the values in the unit of distance, time or speed. However, some addresses may not use decimal for entry. The location of a decimal point indicates the position of mm, inch, degree or second.

X15.0 X15mm or x15 inches

F10.0 10mm/min for 10 inch/min

G04×1 Feedrate for 1 second

B90.0 B90deg

The addresses that can be entered with decimal point are as follows:

X, Y, Z, A, B, C, I, J, K, R, Q and F.

Note 1: During the dwell of an instruction, X can be input with the decimal point but P cannot (because P is also specified with a sequence number).

Note 2: When G codes are used to change the location of the decimal point, it is necessary to predetermine G codes even in a block. G20; (specify in Inch system ) X1.0G04；X1.0 is considered as a travel distance (in inch) because it does not indicate time. The result is held for 10 seconds in relation to X10000G04.

When G04 is entered, its indication changes from 1.0 to 10.0.

G04X1.0 is treated as G04X1000 and the result is held for 1 second.

Note 3: Take note that the condition with or without a decimal point is quite different. Its programming mode differs from an electronic computer.

G21; (specified in metric system)

X1……X1 mm

X1……X0.001 mm

G20; (specified in Inch system )

X1……X1 inch


19

X1……X0.0001 inch

Note 4: The numerical values with/without a decimal point can be mixed.

X1000 Y23.7；

X10 Y22359；

Note 5: If a specified value is less than the minimum setting, the value will be rounded down. The instruction of X1.23456 is considered as X1.234 when it is entered in metric system and 1.2345 in Inch system . It has cumulative error for an incremental value instruction and has no cumulative error but rounding error for an absolute value instruction. The instructed digits must not exceed the allowable maximum digit.

X1.23456789……There is an error because it has more than 8 digits.

X1.2345678…… There is no error when it is up to 8 digits inclusive.

Note 6: When a figure with a decimal point is entered, the figure will be converted into the integer of the minimum input increment.

(Example)X12.34 12340(entered in metric system)

In addition, it is necessary to perform digit number verification for the converted integer.

(Example)X1234567.8 X1234567800(entered in metric system). It gives an alarm because the number of digits exceeds 8.

3.2.5 Maximum instruction value

The maximum instruction values of all addresses are as listed in the table below. Take note

that what the table lists are the ranges of the maximum specified values for the NC unit rather

than the mechanical moving ranges of the NC machine tool. For instance, the moving range of

X axis is about 100m (entered in metric system) for an NC unit while the travel distance of axis

X is likely to be limited to 2m for a machine tool and so is its feedrate. The cutting feedrate of

an NC unit is up to 15m/min while that of an NC machine tool is likely to be limited to 6m/min.

In actual programming, both this manual and the instruction manual supplied by machine

builder shall be referred to. Programming shall be performed on the basis of full knowledge

about the programming ranges of a specific machine tool.

Table 2.5: Basic addresses and ranges of instruction values (including additional options)

Name Address Input in mm

Output in mmInput in inch

Output in mmInput in mm

Output in inch

Input in inchOutput in

inch

Program No. : (ISO) O (EIA)

1～9999 See the left See the left See the left

Sequence No. N 1～9999 ″ ″ ″


20


G 0～99 ″ ″ ″

Coordinate word

X, Y, Z, I, J, K, Q, R,

A, B, C, U, V, W

±99999.999mm±99999.999°

±3937.0078inch±99999.999°

±99999.999mm ±99999.999°

±937.0078inch±9999.999°

Feed per minute F 1～15000 mm/min

0.01～600.00 inch/min

1～15000 mm/min

0.01～600.00inch/min

Feed per minute (feedrate l/10) (parameter setting)

F 0.1～15000.0

mm/min See the above

0.1～15000.0 mm/min

See the above

Spindle function S 0～30000 See the left See the left See the left Tool function T 0～9999 ″ ″ ″

Miscellaneous function

M 0～99 ″ ″ ″

Dwell X, P 0s～99999.99s ″ ″ ″ Sequence No. setting

P 1～9999 ″ ″ ″

Repeated times L 1～9999 ″ ″ ″

Offset No. S, H 0～200 ″ ″ ″

2nd auxiliary function

B 0～999 ″ ″ ″

3.2.6 Program number

The control unit can store a number of programs in the memory of the NC. Program numbers are added to all programs in order to distinguish them.

Program number

(From 1 to 9999.0 and preceding 0 may be omitted) 4 digits

The program starts from the program number and ends at M02, M30 or M99.

#1111 program #2222 program

M02 and M30 indicate the end of a main program. M99 indicates the end of a subprogram.

01111……………………M02； 02222………………………M30；


21

#5555 subprogram

Note 1: For ISO codes, replace O with a “:”.

Note 2: The block with an optional block skip code such as /M02, /M30 and /M99 shall not be deemed as the end of a program.

Note 3: When a program is not provided with a preceding program number, the first sequence number (N…) other than NO of the program may be used to replace the program number.

Note 4: If a program is not provided with a preceding program number or sequence number, MDI/LCD panel shall be used to specify a program number when storing the program into the memory.

Note 5: For several programs, the second program and the succeeding ones are not necessarily provided with an EOB code skipped wit a mark. However, an EOB code shall be used before the program when the foregoing program ends by ER (EIA) or %(ISO).

Note 6: It is possible to operate without a program number. Subprogram shall be provided with a

program number.

Note 7: In some cases, the program number from 9000 ～ 9899 can only used by machine manufacturer rather than user.

Note 8: When it has a robot option, program numbers 9900～9999 are used as robot data.

Note 9: When there is no M02, M30 or M99 but ER (EIA)%(ISO) at the end of the program, or the next program number is 0, the end of the program shall be set by parameter No.306 BIT3 (NEOP).

3.2.7 Sequence number

A sequence number may be specified with N followed by four or less digits (1~9999) at the start of a block. The order of sequence numbers is random and discontinuous. It is likely that all blocks are provided with sequence numbers or sequence numbers are only added at the necessary locations of a program.

It is recommended to specify sequence number in succession at key locations, e.g. when replacing new tools or change the worktable indexing to a new machined surface.

Note 1: The use of the sequence number NO. is not allowed for the purpose of compatibility with the program formats of other NC units.

Note 2: Since 0 cannot be used as a program number, the sequence number treated as a program number shall not be 0.

3.2.8 To skip over an optional block

When a slash followed by a digit /n(n=1～9) is specified at the beginning of a block and the

05555………………………M99；


22

OPTIONAL BLOCK SKTP switch n is enabled on the operation panel , the block with a /n corresponding to switch number n will be ignored.

When the OPTIONAL BLOCK SKTP switch n is disabled, the block with a /n is valid, namely operator may choose to skip over the block with a /n. The 1 in /1 can be ignored. However, the 1 in /1 must not be ignored when two or more OPTIONAL BLOCK SKTP switches are used.

When an OPTIONAL BLOCK SKTP switch is enabled, the ignored area is as follows:

；/2N123G01X4……………………；N7856 Ignored area

Example: N100X100；

N101/2z100；

N102/2/3X200；

N103/3z200；

In the above example, blocks N101 and N102 will be skipped over when No. 2 switch is enabled and N102 and N103 skipped over when No. 3 switch enabled.

Note 1:Slash (/) shall be specified at the beginning of a block. If it is specified at other places of a block, the information from the slash (/) to EOB code will be ignored but the information before the slash (/) will remain valid.

Note 2: When the OPTIONAL BLOCK SKTP switch is enabled, TH and TV checkouts shall be

performed for the skipped part as the switch is disabled.

Note 3: The block to be skipped over is identified when the memory sends information to the buffer register. When the block preceded by a slash is written in the buffer register, it will not be ignored even if the OPTIONAL BLOCK SKTP switch is enabled.

Note 4: The function remains available during sequence number searching.

Note 5: The function is invalid when saving a program in the memory. That is, the block preceded by a slash (/) will be written in the memory regardless the state of OPTIONIAL BLOCK SKIP.

Note 6: The programs may be completely output from the memory regardless the state of OPTIONIAL BLOCK SKIP.

Note 7: Some OPTIONIAL BLOCK SKIP switches are likely to be unavailable for some machines. Therefore, it is necessary to consult the machine manufacturer for the number of usable switches.

Note 8: For the system with additional function to skip over an optional block, the 1 in /1 must not be omitted if there are two or more marks for skipping over an optional block in one block.

/1 shall be specified as per the above requirements.

Example: Incorrect: //3 G00 X10.0；

Correct: /1/3 G00 X10.0；


23

3.3 Dimension Word

A dimension word prescribes the movement of a tool. It composes a relevant instruction with the address of a kinematical axis and a value indicating the direction and amount of travel. It varies depending on the different absolute and incremental programming modes. (See Section 3.3.8.)

Address of dimension world Meaning

Basic axes X, Y, Z The addresses of all axes in a rectangular coordinate system: To indicate the location of the axis or the distance in axial direction.

Additional axes A, B, C, U, V, W The addresses of the 4th and 5th axes: To indicate the angle of axis of rotation or the location and distance of linear axis.

R To specify the radius of an arc. Arc interpolation parameters

I, J, K To indicate the distance from the home point to the arc center along axis X, Y or Z or an axis parallel to them.

3.3.1 Controllable axis

The kinematical axis of a machine under the control of the NC system is called controllable axis.

Each control shaft is recalled with the dimension word address of the control unit.

The number of axes that can be controlled by the NC system may be 3 (axes X, Y and Z) and can be added to 4 or 5.

An additional axis may use any address among A, B, C, U, V or W. A, B and C are recommended for axis of rotation and U, V and W for linear axis.

2 standard axes can be controlled in a block at the same time. The number of concurrently controllable may be increased to 3 or 4 by means of additional selection. Separate control of additional axis is only used for 3-axis link. The selection of additional axis gang control function enables the link of 2 or 3 additional axes. If 3-axis gang control function is selected, it is not necessary to select additional axis gang control function any more.

Number of concurrently controllable axes

Number of controllable

axes

Number of standard

axes

Selection of concurrently controllable

additional axes

Concurrent selection of 3 axes

Concurrent selection of 3 axes

+ Concurrent control selection of

additional axes

Concurrent selection of

4 axes

3 2 3


24

4 5

2 (Including

additional axes)

X, Y, Z 3 (Including

additional axes)

4

Note 1: The system gives #17 alarm if additional axes (A, B, C, U, V, W) are specified without

additional control function.

Note 2: The number of link axes is always 2 in manual operation.

Note 3: When the system has the 5th axis, the following function control shall be exerted.

① Thread cutting and synchronous feed cannot be performed.

② The capacity of part program is reduced to 75%.

③ Additional S4 digit analog output function is not available.

④ Additional constant surface speed control function is not available.

Coordinate axes and movement symbols

If the machine coordinate axes specified by the machine are not identical with the tool movement symbols, programming is subject to serious disorder. The concerned basic concepts are provided in EIA RS-267-A or ISO841.

However, the following points shall be observed during programming.

a) Program shall be developed on the basis of a standard coordinate system (right-manual rectangular coordinate system).

b) When programming, assume that workpiece does not move and a cutting tool moves around it.


25

3.3.2 Set unit

3.3.2.1 Minimum set unit and minimum travel unit

1) Minimum set unit (input unit)

Minimum unit of tool travel is input by instruction. The minimum unit is given in mm, inch or degree.

2) Minimum travel unit (output unit)

The minimum unit output to the machine is indicated in mm, inch or degree. Any one of the following combinations may be employed.

Input/output Minimum set unit Minimum travel unit Input in mm and output in mm 0.001mm 0.001mm Input in inch and output in mm 0.0001inch 0.001mm Input in mm and output in inch 0.001mm 0.0001inch

Linear axis

Input in inch and output in inch 0.0001inch 0.0001inch Axis of rotation 0.001° 0.001°

Note: The set unit of an axis of rotation cannot be converted between Inch and metric systems. Whether the minimum travel unit is 0.001 mm or 0.0001inch shall be determined by the machine and selected by presetting parameter No.006 BIT0 (SCW).

Whether the minimum travel unit is 0.001 mm or 0.0001inch shall be selected by G codes or by setting parameter through MDI/LCD panel.

G20……The minimum set unit of a linear axis is 0.0001inch.

G21……The minimum set unit of a linear axis is 0.001mm.

The state of G20 and G21 remains unchanged when the system is powered on/off.


26

3.3.2.2 Input unit×10

The minimum set unit in mm may be changed to 0.01mm by parameter No.006 BIT1 setting. The minimum set unit in inch cannot be changed.

Minimum set unit Address

Input in mm Input in inch Dimension word X, Y, Z, Q, R, I, J, K, U, V, W 0.01mm 0.0001inch Revolution axis A, B, C 0.01° 0.01°

X 0.01s 0.001s Dwell time

P 0.01s 0.001s It cannot be changed in the following cases:

a) Inputting differs from the above conditions

b) Display unit

c) Maximum range of instruction value

d) Units of step feed and manual feed

e) Offset input

f) Others

Note 1: In the following descriptions herein, input unit is either 0.0001inch or 0.001mm.

Note 2: Display unit may become 0.01mm or 0.01 degree by parameter No.006 BIT2 (MDL) setting.

3.3.3 Maximum travel

The maximum travels that can be instructed of the device are as listed in the table below:

Input in mm and output in mm

Input in inch and output in mm

Input in mm and output in inch

Input in inch and output in inch

±99999.999mm ±99999.999°

±3937.0078inch ±99999.999°

±99999.999mm ±99999.999°

±9999.9999inch ±99999.999°

Note: The travels listed in the above table change depending on different machines.

3.3.4 Program origin and coordinate system

Program origin and coordinate system shall be determined during programming. Generally a specific point on the workpiece is determined as the program origin.


27

This coordinate system is a workpiece coordinate system.

3.3.5 Coordinate system and origin of processing

A workpiece coordinate system needs to be used when a program is sent to the NC. The cutting tool starts motion from the origin and the program starts from the origin, but the NC always need to know the coordinates of the cutting tool at the origin through G92 instruction (coordinate system setting).

3.3.6 Workpiece coordinate system

Several workpiece coordinate systems are needed when the mounting positions of the several trailing bars for the machine are different. In this case, the 6 coordinate systems preestablished on the machine may be selected with 6 G codes (G54～G59) and the following programs are executed in the selected coordinate system. All coordinate systems shall be determined with the set distance between a reference point (a fixed point on the machine) and their respective origins of coordinate (workpiece origin offset). See the following diagram for details.

Refer to Section 4.4.13 for the setting method of workpiece origin offset.


28

It is not necessary to establish a coordinate system with G92 instruction when the above-mentioned workpiece coordinate system is used. Concurrent use of G54～G59 and G92 may substitute the coordinate system established by G54～G59. Therefore, usually G92 shall not be used in conjunction with G54～G59.

Note: When using the workpiece coordinate system established by G54～G59, make sure to

return to the first reference point after switching on so that G54 will automatically generate a

workpiece system. Hence it is not necessary to set an automatic coordinate system.

3.3.7 Reference (position) point

Reference point is a fixed point on the machine. Reference point return function allows the

cutting tool to return to the reference point. Therefore, a program is likely not to start from one

point on a workpiece coordinate system but from the reference point. In this case, the return of

the tool to the position of the reference point shall always be specified with G92 in the

workpiece coordinate system because the reference point is a specific point on the machine

and the program is developed on the basis of the workpiece coordinate system with a point on

the workpiece as its origin.


29

Note: G92 instruction is not necessary when the workpiece coordinate systems established

with G54～G59 are used.

3.3.8 Absolute value instruction and incremental value instruction

The distance that a cutting tool moves along all axes may be programmed with an incremental

instruction or absolute instruction.

It is possible to directly program a running distance in a block using an incremental instruction

(G91).

When using an absolute instruction (G90), the end position of the cutting tool is indicated with

a coordinates in the block.

In the above diagram, the program will give the following position when an incremental instruction is employed:

G91 X-60.0 Y40.0； In the above diagram, the program will give the following position when an absolute instruction is employed:

G90 X40.0 Y70.0；


30

The instruction mode of G90/G91 must not be changed for all addresses in a block so that the program can be compatible with other NC.

3.4 Feed Function (F function)

3.4.1 Rapid traverse (positioning) function

All axes of the machine operate at the specified rapid traverse speed during rapid traverse.

As a rule, the rapid traverse speed has been set by manufacturer before shipment (set by parameters RPDFX through RPDF4).

Since all axes of the machine moves individually, the times for all axes to move from their home positions to end positions are different.

For example, when the rapid traverse speeds of axes X and Y reach 5m/min and 8m/min respectively and movement program is as follows:

G91 X200.0 Y200.0；

The times for axes X and Y of the machine to run from the starting point to the end point are 24s and 15s respectively.

The locus of the cutting tool in the above example is as indicated in the figure below:

The control over the override of the rapid traverse speed can be achieved with the switch on the operation panel of the machine. (FO, 25%, 50%, 100%) FO shall be determined by setting parameter No.113 (SPDFL) and its unit shall not be indicated in percentage (%) but mm/min or inch/min.

3.4.2 Cutting feedrate

The cutting feedrate shall be specified in the form of the distance per minute. The feedrate is


31

specified as follows with F codes:

F1 (1mm/min; 0.01inch/min)

F15000(15000mm/min) or F60000(600.00 inch/min)

The feedrate is restrained to the upper limit.

According to the upper limit, the manufacturer of the machine sets feedrate by parameter No.106 (FEDMX) or exerts override restraint from 0 to 200% (10% each step) with the switch on the operation panel. The control over upper limit speed is also effective for override feedrate. The means of specifying feedrate with F codes is also applicable for the axis of rotation.

Example: To input in metric system F050

To input in Inch system F032

When inputting in metric and Inch system s, decimal point may be used for inputting and it is located in the position of degree/min.

To input in metric system F12 0.12 degree/min

To input in Inch system F12 0.12 degree/min

To input in metric system F12.0 12 degree/min

To input in Inch system F12.0 12 degree/min

Note 1: Except the acceleration and deceleration processes in the row of NC, NC’s calculus error regarding instructed feedrate is kept within ±2%. Moreover, the error is determined by measuring a travel distance over 500mm when NC is in stable running state.

Note 2: The number of the digits of F codes is up to 7. Should the input feedrate is above the upper limit, the feedrate is restrained to the upper limit.

3.4.3 To reduce feedrate to 1/10

The input speed in metric system can be changed to 1/10 of the original speed by parameter No.006 BIT3 (FMIC) setting.

Item Minimum input unit Range

Feed per minute 0.1mm/min F1 to F150,000 (0.1 mm/min to

15000.0mm/min)

3.4.4 Synchronous feed (feed per rotation)

It is possible to specify a feedrate in relation to the feed amount per minute of the spindle. G95 specifies synchronous feed while G94 feed per minute (with travel per minute as the feedrate).


32

Feed per minute Synchronous feed

Meaning Feed amount per minute of

cutting tool Feed amount of cutting tool per

rotation of spindle Address F F G code G94 G95

Input in mm

1mm/min～15000mm/min (F1～F15000)

0.01mm/r～500.00mm/r (F1～F50000)

Range Input in

inch 0.01inch/min～600.0inch/min

(F1～F60000) 0.0001inch/r～50.0000inch/r

Restraining value

Both the feed per minute and synchronous feed at specific feedrate are restrained. The restraining value is set by manufacturer (only the feedrate with override is restrained).

Override The override from 0 to 200% (10% each step) is effective for both feed per minute or synchronous feed.

A restraining value is set in mm/min or inch/min. Synchronous speed is converted to mm/min or inch/min with the following formula:

fm=fr×R

Where fm: the feed per minute in mm/min or inch/min

fr: the synchronous feedrate in mm/r or inch/r

R: the rotational speed of the spindle in r/min

Note 1: Both G94 and G95 are modal. Once they are specified, they will be effective until other G codes appear.

Note 2: The spindle shall be provided with a synchronous feed position coder.

Note 3: When the rotational speed of the position coder is as low as 1 rpm, the feedrate will become irregular. The irregularity has no impact on the machining of the machine. Therefore it is still usable when the rotational speed is as low as 1 rpm. However, the degree of irregularity must not worsen more as the further reduction in rotational speed is subject to deterioration.

3.4.5 F1 digit feed

Specifying a digit (1～9) behind F sets the feedrate of the corresponding number. Feedrate is preset for each number using parameter. Specify FO as the rapid traverse speed and set the F1 digit feedrate switch on the machine panel to ON. Then rotate the manual pulse generator to increase or reduce the feedrate of the currently selected number.

The increase or reduction in feedrate:

F=△X

Fma100

1×/Manual pulse generator per case

Where: Fma×1 is used as the upper limit of feedrates of F1～F4 (set with a parameter).


33

Fma×2: is used as the upper limit of feedrates of F5～F9 (set with a parameter).

X: Any figure between 1 and 127 (set with a parameter).

Set or modified feedrate can be saved even in case of power failure. The current feedrate is displayed on the LCD.

3.4.6 Automatic acceleration and deceleration

During the start or stop of feed, acceleration or deceleration is performed at some time constant so as to prevent the mechanical system from shock. Hence it is possible to consider the problem of acceleration and deceleration during programming.

It is impossible to machine a sharp angle under the influence of automatic acceleration and deceleration. To machine a sharp angle, dwell instruction (G04) must be added between two blocks.

Once the dwell instruction is inserted, the actual tool path tallies with the programmed path. The rapider feedrate is, the greater time constant of acceleration and deceleration and angle error will be.

Note 1: The changes of feedrate between the blocks that have specified different moving modes are as listed in the table below.

Foregoing blocks

New blocks Positioning Cutting feed Not to move

Positioning × × × Cutting feed × ○ × Not to move × × ×

×: The next block will be executed when the instruction speed is reduced to zero.

○: Continue to execute the next block so that the feedrate will not change excessively.

Note 2: Acceleration/deceleration is independently performed on both axes (axes X and Z) and their feedrates changes between blocks, resulting in the discrepancy between the actual path of the tool and programmed path. For example, if the tool only moves along axis X in a block and along axis Z in the next block, the movement in the direction of axis X starts to decelerate near the angle. Meanwhile, it starts accelerated movement in the direction of axis Z. The actual path


34

of the tool is as indicated in the figure below.

In arc interpolation, the actual arc radius is less than the programmed on (see the Appendix). The deviation may be increased by minimizing the time constant of acceleration and deceleration.

3.4.7 Automatic angle adjustment

Tool cutting is subject to overload if the tool performs the rough machining with tool compensation in inner angle and inner arc area at programmed feedrate. The function automatically reduces feedrate so as to lower the tool’s overload in the above machining areas, thereby obtaining a smooth machining surface.

3.4.7.1 Automatic adjustment of inner angle

1) Working conditions

Feedrate can be automatically regulated provided that both the two blocks in succession passing the angle satisfy the following requirements.

a. The G codes of Group 01 are G01, G02 or G03.

b. The offset is not 0 in offset mode.

c. Offsetting shall be performed inside the angle to be processed.

d. The axis moves along the offset surface.

e. Instructions G41 and G42 do not exit in the succeeding block. f. Instructions G41 and G42 do not exist in the preceding block or the block is not started

though it has the two instructions.

g. The inner angle is less than the θ preset by parameter.

The angle judgment with regard to programmed path:


35

(I) Straight line Straight line

(II) Straight line Arc

(III) Arc Straight line

(IV) Arc Arc

The angle may be considered as an inner angle when θ≤θP. The value of θP shall be set by parameter (NO·335) (1°≤θP≤179°). It is subject to error in judgment less than 0.001° provided that θ is nearly equal to θP.

Operation range

When an angle is determined as an inner angle, feedrate is regulated from the range specified by the Lθ in the block on one side of the intersection point of the angle to the range specified by the Ls in the block one the other side of the intersection point. Ls and Lθ are the straight distances from one point on the path of the tool center to the intersection point. Lθand Ls are


36

set by different parameters (N0·355 and 356).

Feedrate is regulated in the range from point a to point b.

Feedrate is regulated within the range from Point a to Point b.

For an arc, the adjustment function is effective for the end point of a block provided that the following requirements are fulfilled.

① Within the range of Lθ;

② The origin and end point of the arc are in the same quadrant or the origin is in the quadrant adjacent to the one in which the end point is. Similarly, the adjustment of the origin of the block is effective when the following conditions are met.

① Within the range of Ls;

② The origin and end point of the arc are in the same quadrant or the origin is in the quadrant adjacent to the one in which the end point is.

(Example) For a disc:

For the program for an② arc, feedrate is regulated from point a to point b and from point c to point d.

Amount of adjustment


37

Amount of adjustment is set by No. 335 parameter.

1≤amount of adjustment (1% each step) ≤100 (%)

This is effective for commissioning and F1 digit instruction. For F4 digit instruction, the actual feedrate will become:

Fx (inner angle adjustment) × (feedrate adjustment)

Whether inner angle adjustment is effective Whether to adjust an inner angle or not may be selected with G codes. The inclusion of G62 in the group 15 in which G61 and G64 are is as shown in the table below. These G codes are related to accurate stop checking mode.

Accurate stop detecting mode Inner angle adjustment

G61 Valid Invalid

G62 Invalid Valid

G64 Invalid Invalid

Note 1: It is in G64 mode when powered on or cleared.

Note 2: It is necessary to specify G09 when you plan to perform accurate stop detection in G62 mode.

Note 3: The switch of inner arc cutting feedrate is always valid as described in Section 4.7.2 and is not subject to the influence of G codes.

3.4.7.2 Switch of inner arc cutting feedrate

For inner arc offset cutting, the feedrate of programmed path shall be specified by F codes while its actual feedrate F×RC/RP (where RC is the radius of the path of tool center and RP the radius of program path.

The switch is also effective for commissioning and F1 digit instruction.

(Example 1)

However, if RC is much less than RP, i.e. RC/RP=0, the tool will stop. Therefore, when

RC/RP≤MDR after the minimum reduction ratio (MDR) is set, the actual feedrate will be FX

(MDR).


38

MDR is set by N0·333 parameter. When 1≤MDR (1% each step)≤100, it is applicable for F1

digit and commissioning. The reduction ratio of automatic inner angle adjustment is not under

the influence of MDR.

Note: If inner arc cutting is overlapped on automatic inner angle adjustment, now the actual

feedrate will be F×RpRc

× (angle adjustment)× (feedrate override).

3.5 Preparation Function (G function)

The two digits following address G determine the meaning that the concerned block involves.

G codes may be divided into the following two types:

Type Meaning Primary valid G codes It is only valid in its instructed block.

Modal G codes After being instructed to be valid, the G codes become invalid only when another G code in the same group is instructed.

(Example) G01 and G00 are modal G codes.

G01 X ;

Y ; G01 is valid in this range.

X ;

G00 Y ;

Table 5.1: G codes list

G codes Group Function G00 Positioning (rapid traverse) G01 Linear interpolation (feed) G02 Arc interpolation CW (clockwise) G03

01

Arc interpolation CCW (counterclockwise) G04 Hold G07 Speed sine-curve control (specified imaginary axis) G09 Accurate stop detection G10

00

Offset setting, workpiece zero offset setting G17 To select XY plane G18 To select ZX plane G19

02 To select YZ plane

G20 Input in inch G21

06 Input in mm

G22 04 Storage travel limit ON


39

G23 Storage travel limit OFF G27 Reference point return check G28 To return to reference point G29 To return from reference point G30 To return to the 2nd, 3rd and 4th reference points G31

00

To skip over cutting G33 01 Thread cutting G40 To cancel tool compensation G41 Tool compensation – left side G42

07 Tool compensation – right side

G43 Forward compensation of tool length G44 Reverse compensation of tool length G49

08 To cancel tool length compensation

G45 To increase tool offset G46 To reduce tool offset G47 To increase tool offset by twice G48

00

To reduce tool offset by twice G50 Zooming OFF G51

11 Zooming ON

G54 14 To select workpiece coordinate system 1 G55 To select workpiece coordinate system 2 G56 To select workpiece coordinate system 3 G57 To select workpiece coordinate system 4 G58 To select workpiece coordinate system 5 G59

14

To select workpiece coordinate system 6 G60 00 unidirectional positioning G61 Accurate stop detecting mode G62 To enable automatic angle adjustment G64

15 Cutting mode

G65 00 Simple recall of a microinstruction G66 Modal recall of microinstruction G67

12 To cancel modal recall of microinstruction

G73 Gun drilling cycle G74 Reverse-tapping cycle G76 Finish boring G80 To disable fixed cycle G81 Drilling cycle, spotter G82 Drilling cycle, counterboring G83 Peck drilling cycle G84 Tapping cycle G85 Boring cycle G86 Boring cycle G87 Reverse boring cycle G88 Boring cycle G89

09

Boring cycle


40

G90 Absolute value programming G91

03 Incremental value programming

G92 Absolute zero programming G94 Feed per minute G95

05 Feed per rotation

G98 To return fixed cycle to the initial point G99

10 To return fixed cycle to point R

G96 G97

B

(Note 1) The G codes marked with are the initial G codes of all groups. That is, these G codes are established when the system parameters specifying initial G codes are validated by powering on or pressing the RESET key. For G22 and G23, G22 is selected when power is switched on and G22 or G23 (one of them is valid before reset) is established after reset.

The selection of the state of the initial G codes such as G00, G01, G43, G44, G49, G90, G91 or G94 and G95 shall be set by parameters ((G00, G43, G44, G90 and G95).

For G20 or G21, the valid one is selected before powering off or pressing the RESET key.

(Note 2) The G codes in group 00 are modal and are only valid in the blocks they belong to.

(Note 3) When a G code not listed in the above table is specified or an optional G code not defined by control unit is specified, (N0.0/0) will give an alarm. (N0.0/0) But G38 and G39 are ignored.

(Note 4) Some G codes may be specified in the same block even they do not belong to the same group. When 2 or more G codes than belong to the same group are specified in a block, the lastly specified G code will be valid.

(Note 5) If any G code in group 01 in fixed cycle mode, the fixed cycle will be automatically disabled and the system will be in G80 state. However, the G codes in group 01 are not subject to the influence of the G codes of fixed cycle.

(Note 6) G70 and G71 replaces G20 and G21 (special G codes) by parameter No.008 BIT5 (GSP) setting.

(Note 7) The G codes of all groups are displayed.

3.5.1 Selection of planes (G17, G18, G19)

A plane is selected with the instruction for arc interpolation and tool compensation.

G17……XY plane

G18……ZX plane

G19……YZ plane

Travel instruction is not related to the selection of planes G17/G18/G19. For example, when G17Z—— is specified, Z will move.


41

3.5.2 Positioning (G00)

Using this code positions the tool at the points programmed by addresses X, Y and Z or A, B, C, U, V and W. Coordinates shall be always specified in absolute instructions while the distance from the origin to the end point in incremental instructions. All axes move the tool at rapid traverse (positioning) rates individually and the tool path is not always straight line during positioning.

2 axes (2 addresses) can be programmed concurrently in a block. But only one can be programmed for the 4th axis.

G00 specifies a position.

G00α——β——:

(α·β=X, Y or Z)

Example: The program shall be as follows when the rapid traverse (positioning)rate is 9.600mm/min in the direction of axis X and 9.600mm/min in the direction of axis Y:

G00 X25.0 Y-10.0

Note 1: The rapid traverse (positioning) rate in G00 instruction is set for all axes respectively by

manufacturer. Therefore rapid traverse (positioning) rate can not be specified through program.

In the positioning mode of G00, the tool start speeding up until it reaches the predetermined speed. Then it rapidly travels and finally slows down to the end point. When it comes to the “proper position”, the next block is executed in sequence (Note 2).

Note 2: The so-called “proper position” means motor feed is within the specified range (The range is determined by manufacturer). The travel instruction in the following format may be specified provided that the system selects three-axis link function.

G00 X——Y——Z——:

In this example, axes X, Y and Z move the tool to designated position in specified rapid traverse.

When the system selects the linked control function with additional axes, not only addresses X, Y and Z, but also the addresses of additional axes may be instructed. If they are instructed in this way, 3 or 4 axes can move at the same time.

Example: X500.0 Y300.0 Z25.0 B20.0:


42

3.5.3 Unidirectional positioning (G60)

For the accurate positioning without offset, final positioning can be achieved in only one direction.

Origin

End point

(The direction for final positioning is from right to left.)

The condition that replaces G00 with G60 is as follows:

G60 α——β——γ——δ——:

(α, β and γ= X, Y and Z or additional axes A, B, C, U, V or W. This is the case of concurrent control of 3 or 4 axes. The situation of concurrent control of 2 or 3 axes includes the selection of one additional axis.

Overshoot and positioning direction are set by parameter. The tool stops once before the end point even the positioning direction of instruction is identical with parameter setting.

Note 1: G60 is an one-off valid G code.

Note 2: Axis Z must not be positioned in a single direction in fixed drilling cycle.

Note 3: The axis whose overshoot has not been set by parameter shall not be positioned in a single direction.

Note 4: When the travel distance instruction is O, unidirectional positioning will not be performed.

Note 5: When mirroring function is used, it is invalid to set its direction by parameter.

Note 6: Unidirectional position does not apply to fixed cycles G76 and G87.

3.5.4 Linear interpolation (G01)

G01α——β——F——:

(α, β and γ=X, Y, Z, A, B, C, U, V and W. Gang control is exerted for 4th and other axes.)

This actually specifies linear interpolation mode. α and β defines the travel distance of the tool. Whether the distance is in absolute or incremental mode depends on the current state of G90/G91. Feedrate shall be specified by F codes, which are modal.


43

Example of program: (G91) G01 X200.0 Y100.0 F200.0

Y End point

0 Origin 200.0 X

The feedrate instructed by F codes is the traveling speed of the tool. If F codes are not specified, the feedrate is considered as 0.

The travel instruction (linear interpolation) with 3-axis gang control function is as follows:

G01 X——Y——Z——F——:

It is possible for the instruction to perform linear interpolation for 3 axes at one time.

When additional gang control function is selected, the addresses (A, B or C) of the fourth axis may be used to replace X, Y or Z. In this way the 3-axis gang control involving the 4th axis can be exerted.

Example: G01 X500.0 Y300.0 B20.0 F10.0:

When the system is provided with optional 4-axis gang control functio0n, the use of the following instruction is allowed.

G01α——β——γ——δ——F——:

Where α, β, γ, δ= X, Y, Z, A, B, C, U, V or W.

Note 1: Axial feedrates are as follows: G01ααββ F f:

The feedrate in the direction of axis α: Fα=Lα

·f

The feedrate in the direction of axis β: Fβ=Lβ

·f

L= βα22

+

Note 2: The feedrate of an axis of rotation shall be instructed in degree/min (input in metric system: F050; input in inch system: F032).

Example: G91 G01 B90.0 F300:


44

Note 3: In the linear interpolation involving the 4th axis (axis of rotation A, B or C), the unit of cutting

feed is changed from degree to inch (or mm) and the cutting feedrate in α—β rectangular coordinate system is controlled so that it keeps identical with the speed specified by F codes. The feedrate of an axis of rotation is determined with the formulas in Note 1 and its unit is changed into degree/min.

E: G91 G01 X20.0 B40.0 F300.0:

When the unit (degree) of B-axis movement instruction is changed into mm or inch, machining time shall be determined as follows:

3004020 22 +

=0.014907 (min)

The feedrate of axis B is:

14907.040

=268.3 °/min

Note 4: For 3- or 4-axis link, the method for calculating the feedrate in rectangular coordinate system is the same as 2-axis control.

Note 5: For inputting in Inch system and inputting in metric system, the upper limit of the feedrate of an axis of rotation is approximately 6000°/min. The speed is fixed at the upper limit even the feedrate of an instruction exceeds the upper limit.

3.5.5 Arc interpolation (G02, G03)

3.5.5.1 Arc interpolation without any additional axis

The instruction below moves the tool along the arc.

The arc in the X——Y plane:

G02 R—— G17 X——Y—— F——;

G03 I——J——


45

The arc in the Z——X plane:

G02 R—— G18 X——Z—— F——: G03 I——K——

The arc in the Y——Z plane:

G02 R—— G19 X——Z—— F——: G03 J——K——

Item Instruction Meaning

G17 The arc in the plane of XY

G18 The arc in the plane of ZX 1 Plane selection

G19 The arc in the plane of YZ

G02 Clockwise (CW) 2 Rotating direction

G03 Counterclockwise (CCW)

G90 mode 2 of axes X, Y and ZThe position of the end point in the workspace coordinate system

3 The position of end point

G91 mode 2 of axes X, Y and ZThe distance from the origin to the end point

The distance from the starting point to the center

2 of axes I, J and K The distance from the origin to the center 4

Arc radius R Arc radius

Once the unit is switched on, G17 is enabled as the initial code for plane selection.

Whether it is in clockwise or counterclockwise direction depends on the left-manual or right-manual coordinate system.

The end point of the arc is determined by address X, Y or Z and its indication in absolute or

incremental value by G90 or G91. In incremental indication, the coordinate of the end point is

specified from the origin of the arc.


46

The center of the arc is determined by the addresses I, J and K corresponding to axes X, Y and Z.

The digit following I, J or K is a coordinate component from the origin to the center of the arc and

they are always specified as an incremental value. The provision has no bearing upon G90 and

G91.

The marks of I, J and K correspond to the specified directions.

Arc interpolation may substitute I and J with R or gives an instruction with K. The instruction is

given in the following format:

G02

X——Y——R——:

G03

There are two types of arc in the arc interpolation with R (specified by radius) – the arc less

than 180° and more than 180°. Its analysis is as indicated in the diagram below.

Example of Instruction:

1． The arc less than 180°:

G02 X6.0 Y2.0 R5.0:

2． The arc over 180°:

G02 X6.0 Y2.0 R-5.0:


47

a) Absolute programming

(1) G92 Ｘ200.0 Y40.0 Z0;

G90 G03 X140.0 Y100.0 I-60.0 F300.0; G02 X120.0 Y60.0 I-50.0;

(2) G92 X200.0 Y40.0 Z0;

G90 G03 X140.0 Y100.0 R60.0 F300; G01 X120.0 Y60.0 R50.0;

b) Increment programming

(I) G91 G03 X-60.0 Y60.0 I-60.0 F300;

G02 X-20.0 Y-40.0 I-50.0; (II) G91 G03 X-60.0 Y60.0 R60.0 F300;

G02 X-20.0 Y-40.0 R50.0; The tangential feedrate of arc interpolation is equal to the cutting feedrate specified by F codes. However, the arc interpolation involving the fourth axis is not allowed.

Note 1: In arc interpolation, I0, J0 or K0 may be omitted.

Note 2: When the end point of an arc coincides with its origin, I, J and K are used to instruct a center of a circle for programming a 360° arc (full circle) and X, Y and Z may be omitted.

Note 3: It will give No. 023 alarm if an arc of radius of 0 is programmed.

Note 4: The deviation of instruction feedrate from actual tool feedrate is less than or equal to ±2%. In tool radius compensation, the actual tool feedrate is the speed of the tool center path.

Note 5: If the addresses I, J, K and R are assigned to the same block, the arc specified by address R is valid and other I, J and K are ignored.


48

3.5.5.2 Arc interpolation with an additional axis

The arc interpolation with an additional axis is allowable. An axis (X, Y or Z) shall be set to parallel with the additional axis by parameter setting. If the additional axis does not parallel with any axis, arc interpolation will be impractical. G code for plane selection shall be specified for arc interpolation. An address of an axis is specified with the G code for plane selection so as to determine the axes performing arc interpolation.

Example: Assuming that additional axes U and W parallel with axes X and Y respectively.

a) G17X-Y-…………………XY plane

b) G17U-Y-…………………UY plane (U parallels with X)

c) G17Y-……………………XY plane

d) G17………………………XY plane

e) G17 X-Y-U-……… …Alarm

f) G18X-W-………………XW plane (W parallels with Z)

Addresses I, J and K may also be used to specify the center of the arc. This is similar to the arc interpolation without any additional axis. The addresses I, J and K are used for the axes parallel to axes X, Y and Z.

The arc interpolation specified with R is also valid.

3.5.6 Sine-curve interpolation

In spiral cutting instruction, sinusoidal interpolation is realized by specifying an arc instruction axis not to move during arc interpolation. The imaginary axis is specified as follows:

G07α0: (Specify α as the imaginary axis)

G07α1: (Specify α as the real axis)

(α= X, Y, Z or additional axes A, B, C, U, V and W)

After instruction G07α0, axis α is deemed as an imaginary axis until G07α1 instruction is given.

For the single-period sine interpolation in Y-Z plane, axis X serves as an imaginary axis.

X2+Y2 = r2 (r: arc radius)

Y = rsin(l

π2)Z( l : the travel distance along axis Z in a single period)


49

N001 G07 X0: N002 G91 G17 G03 X-200 Y0.0 I-10.0 Z20.0 F100: N003 G01 X10.0: N004 G07 X1: Axis X is deemed as an imaginary axis during N002～N003 blocks.

In the N003 block, spiral-curve cutting instruction is given in this way when axis Z is used a linear axis. However, axis Y moves only when axis Z is performing sine interpolation since axis X does not move.

In N003 block, the machine is in suspended state after interpolation because axis X does not move.

Note 1: Imaginary axis is only available for automatic operation but not for manual operation.

Note 2: Interlock, travel limit and external deceleration are also available for imaginary axis.

Note 3: Manual insertion is also valid for imaginary axis. That is, the axis moves by manual insertion.

3.5.7 Thread cutting (G33)

The possibility of cutting determines the threads of screw pitch.

G33Z Z F: f:

Where Z is the length of thread (incremental instruction) or end point of thread (absolute instruction)

f: screw pitch

Minimum input increment Range

Input in mm 0.01mm F1 to F50000 (0.01mm to 500.00mm)

Input in inch 0.0001inch F1 to 500000 (0.0001inch to 50.0000inch)


50

Spindle axis is restricted as follows:

1≤R≤(Maximum feedrate/screw pitch) or allowable rotational speed of the position coder)

Where:

R: Spindle speed (r/min)

Screw pitch: mm or inch

Maximum feedrate: mm/min or inch/min

The instruction signal of maximum feed per minute or the maximum feedrate due to the restriction of motor or machine, whichever is lower;

Allowable rotational speed of position coder: 4,000r/min (position coder A)

6, 000r/min (position coder B)

Note 1: Spindle speed may be read continuously through the position coder installed on the spindle. The coder converts the spindle speed into the cutting feed per minute for purposes of feed.

Note 2: The converted cutting feedrate is not overridden but fixed at 100%.

Note 3: The converted cutting feedrate shall be fixed.

Note 4: Feed hold is invalid during thread cutting.

Example:

N20 G90 G00 X100.0 Y… S45 M03;

N21 Z200.0 ;

N22 G33 Z120.0 F5.0 ;


51

N23 M19;

N24 G00 X105.0 M03;

N25 Z200.0 M00;

N26 X100.0 M03;

N27 G04 X2.0 ;

N28 G33 Z120.0 F5.0 ;

Notes:

N20, N21: To locate the tool at the center of the hole and to clockwise (CW) rotate the spindle.

N22: To perform thread cutting for the first time with screw pitch specified by address F.

N23: M19 orders the spindle to stop in a fixed position on the circumference (M19: Spindle stops in a fixed position).

N24: To withdraw the cutting tool in the direction of axis X.

N25: To move the cutting tool above the hole: M00 orders the program to stop and allows operator to adjust the tool for the thread cutting for the second time.

N26: To align the cutting tool with the center of the hole and to start forward rotation of the spindle.

N27: When the travel instruction in the N26 block is relatively short, it is necessary to add another dwell instruction so that the spindle has adequate time to reach the rated rotational speed.

N28: To perform thread cutting for the second time.

3.5.8 Automatic return to reference point (reference positions G27～G30)

3.5.8.1 Check of return to reference point (G27)

A point fixed on a machined plane is called reference point (reference position). Once a tool is manually returned to a reference point, it is positioned at the point.

G27 instruction function is used to check that the tool is positioned at the reference point.

G27α—β—:

(α, β are selected from address X, Y and Z and additional axes A, B, C, U, V and W) The instruction is used to rapidly position the tool at the reference point.

Once the tool reaches the reference point, the indicator indicating controllable axis’s return to the reference point is lit.

After returning to the reference point, the next block will be executed if M00 or M01 does not exist in M00 or M01. If the return to the reference point is not required in all cycles, optional


52

program skip function can be used.

If the system is provided with 3-axis gang control function, the G27 instruction may be expressed in the following format:

G27α—β— r —:

(The addresses α, β and r shall be selected from X, Y, Z and additional axes A, B, C, U, V and W. However, only one axis can be controlled at one time if concurrent control of additional axes is not selected.)

The use of the following instruction is allowable when 4-axis gang control is selected:

G27α—β—r—δ—:

Where α, β, r, δ= X, Y, Z, A, B, C, U, V or W

Note 1: In tool compensation mode, the position that the tool reaches with G27 is the position with offset. In this case, the tool is also not at the reference point and the indicator for return to the reference point does not illuminate. As a rule, G27 is only used for compensation cancellation mode.

Note 2: In a inch mechanical system that inputs in metric system, the indicator illuminates even the programmed position of the tool offsets from the reference point by 1μ as a result of that the minimum input increment is less than the minimum traveling increment of the mechanical system.

3.5.8.2 Automatic return to reference point (G28)

G28 α—β—:

(The addresses α and β shall be selected from X, Y, Z and additional axes A, B, C, U, V and W. However, additional axes can only be individually controlled without additional axis gang control function.)

The axis specified by the instruction can be automatically positioned at the reference point. As move instructions, α and β shall be specified in absolute/incremental value in G90/G91 mode.

The end point of the instruction is called “intermediate point” and the coordinates specified by this instruction are saved to the NC.

The procedures in the G28 block are as follows:

First all controlled axes are positioned at intermediate points rapidly. Then they move from the intermediate points to the reference points. If now the machine is not locked, the indicator for return to the reference point is lit.

The positioning at the intermediate point and reference point in this way is equivalent to the positioning of G00.

The instruction for 3-axis link is as follows:

G28α—β— r —:


53

(The addresses α, β and r shall be selected from X, Y, Z and additional axes A, B, C, U, V and W.) The following instruction is allowed for 4-axis link function.

G28α—β— r —δ—:

Where α, β, r, δ= X, Y, Z, A, B, C, U, V or W

Generally the G28 instruction is used for automatic tool change (ATC). In principle, tool radius compensation, tool offset compensation and tool length compensation shall be cancelled before executing the instruction.

Note 1: Not only the coordinates of move instruction, but also the coordinates of intermediate point is saved to memory in the blocks of G28. This is, for the axes without instruction in the blocks of G28, the foregoing coordinates in G28 serves as the coordinates of the intermediate point of the axis.

Example: N1 G90 X100.0 Y200.0 Z300.0:

N2 G28 X400.0 Y500.0: N3 G28 Z600.0:

Remarks:

N2: Intermediate point - 400.0, 500.0

N3: Intermediate point - 400.0, 500.0, 600.0

Note 2: After the system is switched on without manual return to the reference point, it moves from the intermediate point when G28 is specified. This is similar to the manual return to the reference point. Now the moving direction from the intermediate point has become the direction of return to the reference point set by parameter.

Note 3: If G28 is instructed for an axis of rotation, the moving direction from the intermediate point to the reference point has become the direction of return to the reference point. Furthermore, the travel is within 360°.

3.5.8.3 Automatic return from reference point (G29)

G29α—β—:

(The addresses α and β shall be selected from X, Y, Z and additional axes A, B, C, U, V and W. However, additional axes can not be interlocked with one the three basic axes if additional axis gang control function is not selected.)

The tool may be positioned at the specified point through an intermediate point using this function. As a rule, the instruction is used after a G28 instruction.

Α and β are specified in absolute/incremental value depending on the current G90/G91 state.

In an incremental instruction, an incremental value relative to the intermediate value shall be specified.

Using the movement of the blocks of G29 allows all instructed axes to pass through the intermediate point previously defined by G28 instruction and to reach the specified point at rapid traverse (positioning) rate.


54

The procedures for positioning at the intermediate point and then the specified point are similar to the positioning with G00.

Example of G28 and G29 application:

For G91:

G28 X1000.0 Y200.0: (From A to B)

M06: G29 X500.0 Y-400.0: (From B to C)

The example shows that programmer needs not to calculate the actual travel distance from the intermediate point to the reference point. The G29 instruction for a system with 3-axis concurrent control function is as follows:

G29α—β— r —:

(The addresses α, β and r shall be selected from X, Y, Z and additional axes A, B, C, U, V and W. However, additional axes can not be interlocked with one the three basic axes if additional axis concurrent control function is not selected.)

The following instruction is allowed for the system with 4-axis link function:

G29α—β— r —δ—:

Where α, β, r, δ = X, Y, Z, A, B, C, U, V and W

Note: After the tool passes through the intermediate point and reaches the reference point under the instruction of G29/30, the intermediate point shall move to a new coordinate system in case of change in the position of workpiece coordinate system. Thereafter the tool shall pass through the intermediate point that has moved to the new coordinate system and reach the specified point when G29 is instructed.


55

3.5.8.4 Return to the 2nd, 3rd or 4th reference point (G30)

The following instruction moves the specified axis to the 2nd, 3rd or 4th reference points (G30).

P2 G30 P3 α—β—; (P2 may be omitted) P4

P2: The 2nd reference point P3: The 3rd reference point P4: The 4th reference point Determining the positions of the 2nd, 3rd and 4th reference points is to preset the distance between the 1st reference points for field adjustment. Except that the tool does not return to the 1st reference point but to the 2nd, 3rd and 4th reference points, the function is similar to G28’s instructions of return to reference point. After the G30 instruction, G29 instruction positions the cutting tool to the specified position through the intermediated established by G30 instruction. Its movement is the same as the situation of specifying G29 instruction after G28 instruction.

When the G30 instruction’s normal position of automatic tool change (ATC) varies from the reference point, the G30 instruction is as follows if 3-axis link function is provided:

G30α—β— r —:

(The addresses α, β and r shall be selected from X, Y, Z and additional axes A, B, C, U, V and W. However, additional axes can not be concurrently controlled along with one the three basic axes if additional axis concurrent control function is not selected.)

The following instruction may be used when 4-axis gang control function is selected.

P2 G30 P3 α—β— r —δ—;

P4 Where α, β, r, δ = X, Y, Z, A, B, C, U, V or W Note: After switching on, it is necessary to manually or automatically return to the reference point once (G28) before executing the G30 instruction.

3.5.9 Dwell (G04)

G04X (t): or

G04P (t):

Either of the above methods may be used for hold. After executing the previous block, It is necessary to wait for (t) seconds before executing the next block.

The maximum instruction time is 99999.999s and time error is about 16ms.

Example: To suspend for 2.5s

G04 X2.5 or G04 P2500:

Note 1: Address P does not program with a decimal point.


56

Note 2: Dwell and time delay are applicable for the two conditions below and are enabled by

parameter setting.

1. After the speed of the foregoing block drops to 0

2. After the tool reaches the instruction value (after the inspection of locating point)

3.5.10 Accurate stop detection (G09)

A block involving G09 reduces its feedrate to 0 at the end point and affirms the state of locating point (Note 2). Then the next block is executed. The function is used to machine a sharp edge or corner. G09 is only valid in its specified block.

Note 1: Locating point detection is automatically performed in the locate modes (G00, G60) without G09.

Note 2 Locating point means that a feed motor is within the range of the specified end point.

3.5.11 Accurate stop detecting mode (G61) and cutting mode (G64)

(1) Accurate stop detecting mode (G61)

The move instructions of all blocks following G61 decelerate to 0 at its end point until G64 instruction. They are determined as being in positioned state and then the next block is executed.

(2) Cutting mode (G64)

The blocks following G64 do not accelerate until the end point of the move instruction of G61 but immediately go to the next block. Even in the G64 mode, feedrate is reduced to 0 and positioning detection is performed under a positioning instruction (G00 or G60) or in the blocks that has determined (G09) accurate stop detection.

3.5.12 Coordinate system setting (G92)

To move the cutting tool to a specific point with absolute instruction, make sure to preset the coordinate system, which is established with the following instruction.

G92X (X) Y (Y) Z (Z) r (r) δ (δ): (r, δ= A, B, C, U, V, W)

The instruction establishes a coordinate system whose origin is located at a point keeping a specified distance from the tool. The following absolute instruction will refer to the coordinates in the workpiece coordinate system.


57

G92 X25.0 Z23.0:

As shown in the above program, G92 is used at the beginning of the block to ensure the nose of the tool coincides with the origin of the program.

G92 X600.0 Z1200.0: As shown in the above diagram, G92 will confirm that the tool point coincides with the origin of the program and execute an absolute instruction. The standard point is positioned at the specified point. To position the nose of the tool to the specified point, the deviation of the nose of the point from the reference point shall be corrected by tool length compensation.

Note 1: In the coordinate system established with G92 instruction in offset mode, the coordinates of the tool in specified position does not include offset.

Note 2: Tool radius compensation is temporarily disabled by G92 instruction.

3.5.13 Workpiece coordinate system (G54～G59)

G92 instruction is not used to establish a workpiece coordinate system. However, the machine’s six exclusive coordinate systems may be preset and selected with G54 and G59.

G54…………………Workpiece coordinate system 1


58






The six coordinate systems are determined by setting all axes’ distances (the offset of the zero

point of workpiece) from the reference point to their respective points.

Example: G55 G00 X100.0 Z20.0:

X15.5 Z25.5:

In the above example, it is positioned in the workpiece coordinate system 2 (X =100.0, Z =20.0)

and (X =15.5, Z =25.5).

Workpiece coordinate systems 1 to 6 are established after switching on and returning from the

reference point. G54 coordinate system is enabled upon switching on.

Note 1: When the range of the workpiece zero point offset of all axes compensated by external data

inputting (optional) is 0～±0.7999mm or 0～±0.7999mm, check the machine instruction

manual for the function.

Note 2:When G54～G59 are used, the coordinate system is not set with G92 but established with G92.

G54～G59 are used to move the coordinate system. G54～G59 must not be incorporated with

G92 except the special situation that G54～G59 are used to move the coordinate system.


59

When the tool is positioned at (200, 160) in G54 mode, G92 X10 Y100; The specified workpiece coordinate system 1 (X’, Y’) is moved by vector A. However, all other workpiece coordinate systems shall concurrently offset vector A.

Note 3: When automatic coordinate system setting is not selected, proper parameter values shall be set (309 APX～AP4).

3.5.14 To change workpiece coordinate system by program instruction

When the number of workpiece coordinate system becomes inadequate (although 6 are ready) or when they are to be moved as required, we move them through programming instructions.

G10L2P P X—Y—Z— r —δ:

Where P=1～6: the 1～6 X, Y, Z, r, δ (r, δ= one of A, B, C, U, V and W) of the corresponding coordinate system: the workpiece zero offsets of all axes.

Note: External workpiece origin offset may be changed by setting P= 0.

3.5.15 Automatic setting of a coordinate system

A coordinate system may be set in the preset parameter number (375PPRTMX～441PPRTI5)

when returning to the reference point for the first time after switching on, namely it functions as

that G92 automatically sets a coordinate system at the reference point.

Note: If workpiece coordinate system setting function is enabled, it is necessary to set No.

375～378 and 400 parameters to 0 or No. 379～382 and 441 parameters to 0. If they are not

set to 0, the workpiece coordinate system (1～6) will offset.

3.5.16 To switch between Inch and metric systems (G20, G21)

Inputting in metric or Inch system may be selected using G codes.


60

System of units G codes Minimum input unit Inch (Inch system ) G20 0.0001inch mm (metric system) G21 0.001mm

Both the G codes must be instructed with a single block before the start of the program and setting of the workpiece coordinate system.

N10 G20:

N20 G92 X—Y—:

The following items changes with the G codes:

(1) The feedrate instructed by F;

(2) Position indication;

(3) Offset

(4) The unit of the scale of the manual pulse generator;

(5) The travel of incremental feed;

(6) A part of parameters

Note 1: Once it is switched on, it enters into the state before power off.

Note 2: Switching between G20 and G21 in the midway of a program is not allowed.

Note 3: When the system of the units of the machine differs from that of the program, the maximum deviation is 1/2 of the minimum traveling unit. The deviation value does not accumulate.

3.5.17 Storage travel limit (G22, G23)

The movable range of the tool may be restricted by the two means below.

(The tool does not enter the shadow area.)

Storage travel limit 1:

The outside of the boundary set by parameter is an exclusion area. As a rule, it shall not change once it is set by manufacturer. Therefore it is set at the maximum travel of the machine and is equivalent to the current so-called software limit.


61

Storage travel limit 2:

The outside or inside of the boundary set by parameter or instruction is an exclusion area. Whether it is inside or outside is determined by parameter No.009 BIT6(RWL).

G22 instruction is used to stop the tool from entering the exclusion area and G23 to cancel the restriction.

The instruction below is used to establish or change an exclusion area.

G22 X—Y—Z—I—J—K—:

X＞I, Y＞J, Z＞K

X－I＞2000 (Minimum instruction increment)

Y－J＞2000 (Minimum instruction increment)

Z－K＞2000 (Minimum instruction increment)

The points A and B in the figure below shall be involved during parameter setting.

X1＞X2, Y1＞Y2, Z1＞Z2

X1－X2＞2000 (Minimum instruction increment)

Y1－Y2＞2000 (Minimum instruction increment)

Z1－Z2＞2000 (Minimum instruction increment)

If the exclusion area is set by parameter, X, Y, Z, I, J and K shall be set by the minimum travel unit (input unit) of the mechanical system with the reference as its origin.

If the exclusion area is set by G22 instruction, X, Y, Z, I, J and K shall be set by the minimum travel unit (input unit) of the mechanical system with the reference as its origin. Then the programming data is changed into the numerical value in the minimum traveling unit and the value is set a parameter.


62

Since it is necessary to detect which part of the tool nose or clamp has entered the exclusion area, the computing methods for X, Y, Z, I, J and K are different.

If point A is detected to enter into the exclusion area, a shall be set. If point B is detected to enter into the exclusion area, b shall be set.

When point A is used to detect the nose of the tool, it is safe without changing the settings of the tool each time if the tool of varied lengths are set to the required length.

Overlapped setting is possible for the area.

Note 1: All limits will become effective after power on and manual return from the reference point or G28 completes automatic return from the reference point.

Note 2: If the reference point is within the exclusion area of all limits, the system immediately gives an alarm when the storage travel limits are valid after power on and manual return from the reference point. (For storage limit 2, only G22 mode is applicable.)

When G23 is changed to G22 and the tool is in the exclusion area, the system will give an alarm in the next block.

Note 3: Pressing the emergent stop switch to cancel the restrictions and move the tool out of the exclusion area in G23 mode when the tool remains still in the exclusion area under the conditions of Note 2. The settings shall be changed if they are set incorrectly. Then the tool returns from the reference point.

Note 4: Since the axis without the function of returning from the reference point, the axis does not give an alarm in the exclusion area.

Note 5: For the setting of the exclusion area, the area is described as follows:

When the exclusion area is beyond the specified area, all the areas are movable.


63

When the exclusion area is within the specified area, all the areas are restricted for movement (in G22 mode).

Note 6: The settings beyond the travel of the machine are not necessary.

Note 7: The tool may reversely move provided that the tool is in the exclusion are and an alarm is given.

Note 8: Even the sequence of the coordinates of the two points In the set area are set incorrectly, the rectangle with the two points as its acmes can also be created into a limit area.

Note 9: G22 and G23 shall be instructed in single blocks.

Note 10: Storage travel limit 2 cannot be used for additional axes.

3.5.18 Skip function (G31)

The G31 followed by a move instruction is capable of instructing linear interpolation as G01. If skip signal is input form the outside in the midway of the instruction, the remaining part of the instruction will be interrupted and the next block will be executed.

G31 instruction is one-off and only valid in the instructed block.

The movement after skip signal depends on whether the next block is incremental or absolute.

1) The next block is an incremental instruction.

To make incremental movement from the break point:

Example: G31 G91 X100.0:

Y50.0:

The next block is an absolute instruction (only one axis)

The axis instructed in one block moves to the instructed position while those not instructed remain in the positions input by skip signal.


Y100.0:


64

2) The next block is an absolute instruction (to instruct 2 axes)

The next block moves to the instructed position wherever skip signal is input.


X300.0 Y100.0:

The feedrate of a block is specified （G31）with No. 306 (SKPF) parameter in the following two ways:

a) Feedrate is specified with F codes (may be specified in the foregoing blocks or G31 block)

b) No. 342 parameter is set by No. 342 parameter.

The coordinates when skip signal is switched on are stored in the system variables #5061 to #5065 of the user macro. Therefore they may be used in macros.

#5061………………………X coordinates

#5062………………………Y coordinates

#5063………………………Z coordinates

#5064………………………The 4th coordinates

#5065………………………The 5th coordinates

The skip function may be used to the situation with unknown travel. Therefore, it is applicable in the following conditions.

a) For the standard-dimension feed of the milling machine;

b) To enable tool contact pick-off to measure

Note 1: Once G31 instruction is performed in the active state of tool compensation C, No. 035 alarm


65

will be given. Tool compensation shall be canceled with G40 before G31 instruction.

Note 2: If the feedrate instructed by G31 is related to the speed set by parameter, it will have a bearing upon parameter setting in no-load operation.

Note 3: If the feedrate instructed by G31 is related to the speed set by parameter, the automatic acceleration/deceleration will be invalid. In this way the accuracy of automatic measurement in skip function applications is improved.

3.6 Compensation

3.6.1 Tool length compensation (G43, G44, G49)

Using G43 Z—H—; or

G44

G43 H—;

G44

The end position of the axis Z move instruction is moved forward or reversely by setting the

offset set in the offset storage. Using this function may set the difference between the tool

length estimated in programming and the actual one in service into the offset storage to

achieve compensation without changing the program. H instructs the offset set into the offset

storage by instructing the offsetting direction with G43 and G44.

Offsetting direction

G43 Offset in + direction

G44 Offset in - direction

Whether in the situation of absolute or incremental instruction, the offset specified by H codes

and saved in the offset storage is added to the coordinates of the end point of the spindle move

instruction for G43 and detracted from it for G44. The calculated coordinates become the end

point of the coordinates. It may be illustrated in the same way when axis Z move instruction is

ignored as follows:

G43 G91 ZOH——; G44

The offset is positive for G43 and negative for G44.

G43 and G44 are modal G codes and, when instructed, are always valid if no G codes in the

same group are coded. G 43 or G44 code is valid upon power on depends on parameter setting.

Offset specification


66

Offset number is specified with H codes. The offset set in the offset storage of the number is

added to or detracted from the programming value of axis Z. Offset number may be specified

with H00 or H200. The number of the D codes using tool radius compensation hits 32 (It is also

possible to choose 64, 99 or 200).

Offset corresponds to offset number and may be preset in the offset storage through MDI/LCD

or communicating operations. The setting range of the offset is as follows:

Input in mm Input in inch Offset 0mm～±999.999mm 0 inch～±999.999inch

The offset of the corresponding offset No.00, i.e. H00 is generally 0. The offset corresponding to H00 shall not be set.

Cancellation of tool length compensation

To cancel tool length compensation, G49 or H00 shall be instructed. Once H00 or G49 is instructed, canceling operation will be performed.

(1) Example of tool length compensation (machining of #1, #2 and #3 holes)

H01= －4.0 (Offset)

N1 G91 G00 X120.0 Y80.0 ; ……………①

N2 G43 Z-32.0 H01 ; ……………②

N3 G01 Z-21.0 F1000 ; ……………③

N4 G04 P2000 ; ……………④

N5 G00 Z21.0 ; ……………⑤


67

N6 X30.0 Y-50.0 ; ……………⑥

N7 G01 Z-41.0 ; ……………⑦

N8 G00 Z41.0 ; ……………⑧

N9 X50.0 Y30.0 ; ……………⑨

N10 G01 Z-25.0 ; ……………⑩

N11 G04 P2000 ; ……………⑪

N12 G00 Z57.0 H00 ; ……………⑫

N13 X-200.0 Y-60.0 ; ……………⑬

Note 1: When offset is changed due to the change of the offset number, the new offset will not be added to the original offset.

H01…………Offset 20.0

H02…………Offset 30.0

G90 G43 Z100.0 H01: ……Z will hit 120.0

G90 G43 Z100.0 H02: ……Z will hit 130.0

Note 2: D codes cannot be used for tool length compensation. Other axes except axis Z may employ tool length compensation.

Which axis will be added with tool length compensation is instructed with axis address α in the same block with G43 and G44

G43

α＿H＿: (α: any axis) G44

Tool length compensation can only be added to an axis at one time. Therefore the system gives an alarm in the following instructions. To switch an axis for tool length compensation, it is necessary to cancel the one-off tool length compensation.

G43 Z＿H＿:

G43 X＿H＿: (Alarm)

3.6.2 Tool offset (G45～G48)

The moving distance of the specified axis may be zoomed in or zoomed out by the numerical values set in the offset storage through instructions G45～G48. G codes and their functions are listed in Table 6.2.


68

Table 6.2: Tool offset and G codes

G codes Function G45 To zoom in an offset G46 To zoom out an offset G47 To zoom in an offset by twice G48 To zoom out an offset by twice

These G codes are modal and only valid in instructed blocks.

These amounts of compensation are instructed by D or H codes and remain unchanged once they selected before selecting other amounts of compensation.

Whether tool offset compensation uses H or D codes is set by parameter No.010 BIT3 (OFSD).

In offset storage, the shape of the workpiece serves as the path of the tool for programming during the setting of the radius of the tool.

Range of offset

Input in metric system Input in Inch system

Offset value 0mm～±999.999mm 0”～±99.9999”

Offset value 00～±999.9990 00～±999.9990

The offset function is valid for an additional axis (the 4th axis).

When the offset number is 00 (H00 or D00), the offset will also be 0.

Zooming is made in the moving direction of the tool of the axis. When the absolute value

instructs, the tool starts to move to the position instructed by the instructions in the blocks of

G45～G48 and makes zooming compensation.

1) G45 instruction (only to lengthen the offset)

～～～～～～～ Move instruction value

Offset


69

Actual travel

a) Move instruction +12.34 offset +5.67 b) Move instruction+12.34 offset

c) Move instruction offset +5.67 d) Move instruction -12.34 offset -5.67

2) G46 instruction (only to reduce by one offset)

If the sign of the offset is reversed in G45 instruction, it will be identical with G46.

a) Move instruction+12.34 offset+5.67(b)～(d) (omitted)

3) G47 instruction (lengthen the offset by twice)

a) Move instruction+12.34 offset+1.23 b) Move instruction+12.34 offset-1.23

c) Move instruction-12.34 offset+1.23 d) Move instruction-12.34 offset-1.23

4) G48 instruction (to reduce the offset by twice)


70

If the sign of the offset is reversed in G47 instruction, it will be identical with G48.

a) Move instruction+12.34 offset +1.23(b)～(d) (omitted)

When offset is moved in the mode of incremental instruction (G91), the instruction for travel will be 0. No movement will be performed if the travel instructed in the mode of absolute instruction (G90).

Offset +12.34 (offset No. 01)

NC instruction G91 G45 X0 D01: G91 G46 X0 D01: G91 G45 X-0 D01 G91 G46 X-0 D01:Equivalent instructions

X12.34 X-12.34 X-12.34 X12.34:

Note 1: If one of G45～G48 is specified for 2-axis gang control, the tool offset is valid for both axes.

For G45

Move instruction X1000.0 Y5000.0

Offset +200.0 Offset No. 02

Programming instruction G45 G01 X1000.0 Y500.0 D02:

Note 2: During bevel machining, it is subject to overcutting or under-cutting if tool offsetting is performed.


71

Note 3: When the offset is higher than the move instruction value, the actual moving direction of the tool will be contrary to the programmed direction.

Example: G46 X2.50; (Incremental instruction) Equivalent to X-1.20: Offset+3.70

Note 4: For arc interpolation (G02, G03), only the tool offset under the conditions of 1/4 and 3/4 circles may be resulted by G45 to G48 instructions. That is, tool compensation is only available for 1/4 and 3/4 arc instructions.

Example 6.21: Offset +20.0, Offset No. 01

G01 X F ； G47 X Y ；

Y ；

G01 G45 X F D ；

X Y ； G45 Y ；


72

Example of programming:

(G91)

G45 G03 X-70.0 Y70.0 I-70.0 D01:

Example 6.22: The tool position offset during arc interpolation

N1 G46 G00 X—Y—D—;

N2 G45 G01 Y—F—;

N3 G45 G03 X—Y—I—;

N4 G01 X—;

Example 6.23: The program with tool offset

Tool radius compensation


73

1. G91 G46 G00 X80.0 Y50.0 D01;

2. G47 G01 X50.0 F120;

3. Y40.0;

4. G48 X40.0;

5. Y-40.0;

6. G45 X30.0;

7. G45 G03 X30.0 Y30.0 J30.0;

8. G45 G01 Y20.0;

9. G46 X0; …… Only to move the offset in the direction of -X

10. G46 G02 X-30.0 Y30.0 J30.0;

11. G45 G01 Y0; …………Only to move the offset in the direction of -Y

12. G47 X-12.0;

13. G47 Y-80.0;

14. G46 G00 X-80.0 Y-50.0;

Note 5: Only axis Z moves an offset if H codes are used in G43 or G44 mode. Therefore, it is recommended not to use H codes but D codes in the offsets of G45～G48 as much as possible.

Note 6: G45～G48 modes are ignored in fixed cycles. Hence G45～G48 shall be programmed before instructing fixed cycles and they must always be cancelled after fixed cycles.


74

Note 7: Tool offset modes (G45～G48) are not allowed in the modes of G41 or G42 (tool compensation); otherwise P/S alarm will be given (alarm no. 36).

3.6.3 Tool radius compensation (G40～G42)

3.6.3.1 Tool radius compensation function

As shown in the figure below, to machine the workpiece indicated by A in the figure with a tool of radius R, the corresponding tool center must always be B path keeping a distance of R away from A. Moving the tool from the workpiece by one distance in this way is called offsetting. The tool compensating function is used to determine the path (i.e. offset) of the tool that has moved for a distance.

Therefore, programmer may use the tool offset mode to program the outline of a workpiece. Furthermore, if tool radius (offset) is measured and set in the NC during machining, the tool path will be offset (path B) regardless the programmed path.

Two types of tool compensation (B and C) are available. This section only describes type C. The difference between B and C is as follows: In the mode of type B tool compensation, inward offsetting cannot be performed for angles equal to or less than 90°. In this condition, make sure to program it into a proper inward arc.

3.6.3.2 Offset (D codes)

At most 32 amounts of offset may be set in the offset storage (64, 99 and 200 are optional) (including 32 amounts of offset for tool length compensation and tool position offsetting). The offset depends upon the D instructed in program and the number of digits is set with MDI/LCD.

The range of programmable offsets is as follows:

Input in mm Input in inch Offset 0mm ~± 999.999mm 0inch ~± 99.9999inch

The offset corresponding to No. 00 or D00 is always 0.

So the offset corresponding to D00 need not be set.


75

3.6.3.3 Offset vector

Two-dimensional offset vector is equal to the vector of the offset specified by D codes. It is determined in the control unit and its direction is duly corrected in accordance with tool feed of all axes. The offset vector (hereafter called “vector”) is generated in the control unit so as to determine the amount of tool offsetting movement and calculate the actual path that the tool radius offsets from the programmed path. The offset vector will be cleared away by reset.

The vector changes with the movement of the tool. It is very important to know the status of the vector during developing a program. Please read the following sections and carefully make certain how the vector is generated.

3.6.3.4 Plane selection and vector

The calculation of offset is performed in the plane established by G17, G18 and G19, which is called offset plane. For instance, (X, Y) or (I, J) is used to calculate the offset as well as vector when XY plane is selected. The coordinates of the axes beyond the offset plane are not under the influence of offset but follows instructed value in the instruction.

In 3-axis gang control, the tool path projected on the offset plane is compensated.

Plane selection switching shall be performed in the mode of offset cancellation. No. 027 alarm will be given if plane selection switching is performed in offset mode.

G codes Offset plane G17 X－Y plane G18 Z－X plane G19 Y－Z plane

To set an offset plane with an additional axis, it is necessary to preset which one in axes X, Y and Z that the additional axis parallels with by parameter. When none axis it parallels with, the offset plane cannot be defined.

While setting the offset plane with an additional axis, the additional axis shall be instructed at the same time with the G codes, i.e. G17, G18 and G19. a) G17 X_Y_; ……XY plane

b) G17 U_Y_; ……UY plane (U parallels with axis X)

c) G17 Y_; ………XY plane

d) G17; …………XY plane

e) G17 X_Y_U_; ……Alarm

f) G18 X_W_; ……XW plane (W parallels with axis Z)

3.6.3.5 G40, G41 and G42

G40, G41 and G42 are used to specify the cancellation and generation of a tool radius


76

compensation vector. To determine the direction of an offset vector and the moving direction of the tool, G40, G41 and G42 may be instructed concurrently with G00, G01, G02 or G03.

G codes Function G40 To cancel tool compensation G41 Tool compensation, left G42 Tool compensation, left

G41 or G42 instruction allows the system to enter into offset mode.

G40 instruction allows the system to enter into cancellation mode.

An example of offsetting course will be illustrated in the following figure.

Start-up block ①: Offset cancellation mode becomes offset mode (G41) in this block. The tool center is offset at the end point (P1) of the block by the radius perpendicular to the lower section of program path (from P1~P2). The tool compensating value is specified by D07, i.e. offset No.7. G41 means that the tool offsets to the left.

After workpiece shape P1→P2——→P8→P9→P1 programming and starting, the system automatically performs tool compensation.

In block ①, the tool returns to the point of origin (offset cancellation) through G40. The tool center moves (from P9～P1) normal to the programmed path at the end point of the 10th block.

G 40 instruction (program cancellation) shall be instructed at the end point of the program.

Example of program for tool compensation C:


77

G92 X0 Y0 Z0

① N1 G90 G17 G00 G41 D07 X250.0 Y550.0: (The offset is preset in D07 by MDI)

② N2 G01 Y900.0 F150:

③ N3 X450.0:

④ N4 G03 X500.0 Y1150.0 I-600.0 J250.0:

⑤ N5 G02 X900.0 I200.0 J150.0:

⑥ N6 G03 X950.0 Y900.0 I250.0 J0:

⑦ N7 G01 X1150.0:

⑧ N8 Y550.0:

⑨ N9 X700.0 Y650.0:

⑩ N10 X250.0 Y550.0:

⑪ N11 G00 G40 X0 Y0:

3.6.3.6 Details about tool radius compensation C

The tool radius compensation C is described in detail as follows.


78

(1) Cancellation mode

The system will be in offset cancellation mode after power on, reset or completion of the program by executing M02 and M03.

In cancellation mode, the vector is always 0 and the tool center path coincides with the programmed path. It shall be ended up by means of cancellation at the end of the program.

When the program ends in offset mode, positioning the tool at the end point of the program cannot be performed and the position of the tool will offset from the end position by a vector.

(2) Start-up

When a block satisfying all the following requirements is executed in cancellation mode, the system will be in offset mode. This block is called start-up block.

a) G41or G42 has been instructed and the system is in the state of G41 or G42.

b) Tool compensation number is not D00.

c) Axes (other than axes I, J and K) (even one axis is acceptable) in the offset plane is allowable and their travel is not 0.

In a start-up block, arc instructions (G02, G03) shall not be used; otherwise the NC will gives No. 34 alarm and stops operation. The NC reads in two blocks. The next block enters into the tool compensation buffer register (the contents of the register cannot be displayed) once the first block is read in and executed.

In addition, two blocks in succession are read in when the system is in single block mode. The block is firstly read in stops after execution. As a rule, two blocks are normally read in after that. Hence there are three blocks in the NC, namely the executing block and the next two blocks.

Note: The meaning of the so-called interior angle and other terms are as indicated in the following figure. The intersection angle of the move instructions of two blocks is called “interior angle” when its angular degree on the workpiece side is above 180° and “exterior angle” when it falls within 0°～180°.

(i) To machine along the interior side

Straight line → Straight line


79

Where:

S indicates the dwell point of single block.

L indicates line motion.

C indicates arc motion.

Straight line → Arc

(ii) When the tool machines one side of an obtuse angle, the start-up and cancellation of a

(90°≤α≤180°) tool path have the noses A and B and they are selected by parameter No.011 BIT1 (SUPM).

Type A: (Straight line → Straight line)

(Straight line → Arc)


80

Type B: (Straight line → Straight line)

Intersection point is a point at which the offset paths determined by two blocks in succession intersect.


The intersection point in the above diagram is a point where the offset paths of the r length of two blocks.

(iii) To machine an acute angle (α＜90°＝exterior)

Type A (Straight line → Straight line)



81

Type B (Straight line→ Straight line)

(Straight line→ Arc)

Note: For Type B, compensation shall be performed as follows when the tool moves on one side of a sharp angle less than 10.

(3) Offset mode

In offset mode, arc interpolation may offset even linear interpolation is instructed.

In offset mode, the blocks without move instruction but miscellaneous function, hold, etc cannot be instructed in two blocks in succession; otherwise it is subject to undercutting or overcutting.


82

Offset plane cannot be changed in offset mode; otherwise the system will stop after No. 37 alarm.

(i) Situations of interior angle (180°≤α)

Straight line→ Straight line

Straight line→ Arc

Arc→ Straight line

Arc→ Arc


83

For the condition of straight line to straight line, a narrow and closed angle less than 1° is machined. Now its offset vector becomes extremely big.

User may follow the above procedures for the conditions of arc to straight line, straight line to arc and arc to arc.

(ii) To machine an obtuse angle along the exterior side (90°≤α＜180°)

Straight line →Straight line

Straight line →Arc


84


Arc→ Arc

(iii) To machine an acute angle along the exterior side




85


Arc→ Arc

Note 1: Special cases

When the end point of an arc is not on it


86

If there is a lead on the arc as shown in the diagram, use the arc center connecting to the end point of the arc as the center of a circle to make a imaginary arc. Make a vector for compensation by using the imaginary arc as the arc of tool compensation. Its result varies from the tool center path that uses the arc lead a lead for tool compensation.

Follow the same procedures for the situation of arc → arc.

The situation without an internal intersection point

As shown in the diagram below, arc intersection point exists on compensation path when the offset is small. Increase in the offset eliminates the intersection point. Now the system gives No. 33 alarm and stops at the end point of the previous block.

As shown in the diagram below, arc intersection point P exists on compensation paths of arc A and arc B when the offset is small. Increase in the offset eliminates the intersection point. For that center coincides with the origin or end point, the system gives No. 38 alarm and stops program execution at the end point of the previous block.

(4) Offset cancellation

When executing a block satisfying one of the following requirements in offset mode, the system enters into tool cancellation mode. The function of the block is called offset cancellation.

(a) G40 is instructed (b) D00 is instructed as a tool compensation number.

(G02) and (G03) cannot be instructed when offset cancellation is performed. If they are instructed, No. 34 alarm will be sent out and NC will stop.

When a block is read in offset cancellation mode, two blocks including that stored in the buffer (not display) for tool compensation will be executed. In single block mode, a block is read in

（G41 mode） N5 G01 X1000; N6 G02 X1000 I0 J0; N7 G03 Y-1000 J-1000;


87

and executed before stop. The next block is read in and executed by pressing the START button.

After the control system enters into cancellation mode, the next executed block will be normally saved in the buffer register rather than typed in the tool compensation buffer register.

(a) To machine an interior angle (α≥180°)



(b) To machine an exterior angle (90°≤α＜180°, obtuse angle)

(i) Type A




88

(ii) Type B



(c) To machine the exterior angle of an acute angle (α＜90°)

(i) Type A



89


(ii) Type B



Note: For the situation of type B, compensation is performed as follows when the tool machine an acute angle below 10 by means of straight line to straight line from the exterior side:


90

(5) G codes for tool compensation in offset mode

It is possible set an offset vector in relation to the direction of the foregoing block by individually instructing G codes (G41, G42) for tool compensation in offset mode so as to create a correct angle. It is independent of the inner wall or outer wall to be processed.

Correct arc motion cannot be performed provided that the codes (G41, G42) are included in an arc instruction.

To reverse the direction of compensation through the G codes (G41, G42) for tool compensation, refer to Note 2: To change offsetting direction in offset mode.



Note 2: Change offsetting direction in offset mode.

Offsetting direction is identified with the G codes (G41 and G42) for tool compensation and offset signs as follows:

Offset signs G codes

＋－


91

G41 Offsetting to the left Offsetting to the right

G42 Offsetting to the right Offsetting to the left

In special cases, offsetting direction can be changed by switching between G41 and G42 in offset mode. However, it cannot be changed for the start-up block and the block that follows. In the situation of changing offsetting direction, the concepts of interior side and exterior side are canceled to adapt to all conditions. The amounts of offset are assumed to be positive in all the following examples.

(Straight line →Straight line)

(Straight line →Arc)

(Arc→ Straight line)


92

(Arc→ Arc)

When a path with offset has not intersection point:

If the switch between G41 and G42 is performed and there is no intersection point of offset path from block A to block B, a vector perpendicular to the programmed direction will be established at the point of origin of block B.


93

a) Straight line →Straight line

b) Straight line →Arc

c) Arc→ Arc

The situation in which the length of the tool center path caused by tool compensation:

Generally the above condition will not arise. It is only possible when G41and G42 is switched or G 40 is instructed with address I, J and K.


94

In the above situation, the tool center path does not go around the circle for one turn but only makes arc motion along P1～P2. Its cause will be described in the alarm caused by interference verification. If you want the tool to make movement along the full circumference, make sure to instruct the circumference by sections.

(6) The cancellation of temporary offset and execution of the following instructions in offset mode, “cancellation of temporary offset” will be triggered. Then the system will be automatically restored to offset mode.

Refer to Section 6.3.6 (4) “Offset cancellation” and Section 6.3.6 (2) “Start-up” for the details of the above operations.

(a) G28 Automatic return to reference point

If G28 is instructed in offset mode, offset will be cancelled at the intermediate point. When the reference point is reached, the offset mode will be automatically restored.

If offset vector is maintained at the intermediate point, the NC will zero the vector of all axes returned to reference point.

(b) G29 Automatic return from reference point

If G29 is instructed in offset mode, the offset will be cancelled at the intermediate point and then automatically restored in the next block.

To directly instruct G29 after G28:


95

The situations rather than that G29 is directly instructed after G28:

(7) The instruction for temporary cancellation of an offset vector

In the offset mode, offset vector shall be cancelled and then it will be automatically restored if G92 (absolute zero programming).

In this case, offset cancellation will not be performed. The tool directly moves to the point that is specified to cancel its offset vector from the intersection point, and directly moves to the intersection point when the offset mode is restored.

(G41 mode)

N5 G01 X3000 Y7000:

N6 X－3000 Y6000:

N7 G92 X1000 Y2000:

N8 G01 X4000 Y8000:

Note: SS indicates the points at which tool stops twice in single block mode.

(8) The blocks without tool movement

The following blocks are free from tool movement. The tool does not move even tool radius compensation is valid in these blocks.


96

M05; ……………………………M code input

S21; ………………………….S code input

G04 X1000; ……………….Dwell time

G22 X100000; ………………Machining area setting

G10 P01 X100; ……………Offset setting Not move

(G17) Z2000; ………………….The movement beyond offset plane

G90; ……………………………Only G codes

G91 X0; ………………………Offset is 0

a) The situations in which a block is instructed during start-up

If a block without tool movement is instructed at the origin of the program, it does not generate offset vector.

G04 G91 N6 X1000.0 Y1000.0; N7 G41 X0; N8 Y－1000.0; N9 X1000.0 Y—1000.0;

b) The situations in which a block is instructed in offset mode

When a single block without tool movement is instructed in offset mode, its vector and tool center path are the same as when the block is not instructed (refer to Section 6.3.6 (a): Offset mode). The block is executed at the stop point of the single block.

When the travel is 0, however, the tool movement of the block is identical with when more than a block without tool movement is instructed. It is specifically described as follows:


97

More than 2 blocks without tool movement cannot be specified in succession; otherwise a vector which has a length equal to the offset and direction perpendicular to the moving direction of the tool in the previous block will be generated, thereby causing overcutting.

Note 4: SSS means that the tool operated by a single block stops here for three times.

c) When the block is instructed along with offset cancellation

When a block without tool movement and offset cancellation are specified at one time, its vector whose length is equal to the offset is generated in the direction normal to the tool movement of the previous block. The vector will be cancelled in the next move instruction.

N6 G91 X100.0 Y100.0: N7 G40: N8 X100.0 Y0:

(9) When G40 and the one among I, J and K that is in the offset plane are instructed and the

previous block mode is G41 or G2.

When the above instruction is performed in the offset mode, it will become the following condition with G17 plane as an example. Analogies may be drawn for the situations of other planes.

Now the direction of the vectors (I, J) that start from the end point of the previous block are determined by the above instructions. Its offsetting direction is the same as the previous block.


98

(G42 mode)

G40 X X Y Y I — J --:

Note 5: Take note that in this situation the NC gets a intersection point of tool path independent of the specified machined inner wall or outer wall.

Note 6: When it is impossible to get an intersection point, the tool reaches the position normal to the previous block path at the end of the previous block.

Note 7: When the length of the tool center path is bigger than the circumference:


99

(G41) N5 G01 G91 X10000: N6 G02 J－6000: N7 G40 G01 X5000:

Y5000 I－100 J－100:

In the above situation, the tool center does not go around the circumference but the section of arc between P1 and P2.

The alarm caused by interference verification is related to the following conditions. (If you want the tool to go around the circumference, you need to instruct a circumference by sections.)

(10) Corner movement

When 2 or more vectors are generated at the end point of a block, the tool makes line motion from one vector to the other.

If these vectors almost coincide, corner movement will not be performed and the following vectors will be ignored.

If Vx< V limits or Vy< V limits, the vectors that follow will be ignored. V limit shall be preset by parameter No.069(CRCDL).

If these vectors do not coincide, movement around the angle will be caused. The movement is included in the blocks that follow.


100

Note 8: If the path of the next block is an arc over a semicircle, however, the above-mentioned function cannot be achieved.

The cause is as follows:

If the vector is not ignored, the tool path is as follows:

P0→P1→P2→P3 (Circumference)→P4→P5→P6→P7

If the distance between P2 and P4 is small, P3 will be ignored. Now the tool path is as follows:

P0→P1→P2→P3→P4→P5→P6→P7

The arc cutting instructed by block N6 will be ignored.

(11) General cautions about compensation

a) To specify offset

The D codes that are specified with an offset number instructs offset.

Once they are specified, the D codes will remain valid until another D code is specified or

they are cleared.

Besides that D codes are used for the offset of tool radius compensation, they are also

intended for specifying the offset of tool position offset. If both tool compensation (G41/G42)

and tool offset (G45～G48) are included in a block, No. 36 alarm will be given.


101

b) To change offset

In general, if offset is changed during tool change in offset cancellation mode, the vector of

the end point of the block is fit for the new offset.

c) Positive and negative offsets and tool center path

A negative (-) offset is equivalent to the exchange of G41 and G42 in the program. If

originally the tool center moves along the exterior side of a workpiece, now it will move

along its interior side, vice versa.

The figure below is an example. In general, offset is programmed as a positive value.

When the offset is negative when the tool path is programmed as shown in the Figure (a),

the tool center will move as indicated in (b), vice versa. Therefore machining a female

mould and a male mould may use the same program. The clearance between them may

be adjusted by selecting an offset (it is also applicable if the start-up and cancellation is of

type A.)

d) Overcutting resulting from tool compensation

(i) To machine the inner side of an arc whose radius is less than that of a tool

When the instructed arc radius is less than that of the tool, the system will give No.41

alarm and stop since the offset of the interior side of the tool may lead to overcutting.

During single block operation, however, it is likely to cause overcutting because the tool

only stops when the program ends up. Now the tool movement is similar to the No. 41


102

alarm below.

(ii) To machine a groove smaller than tool diameter

Since that tool compensation forces the tool center path to move in the direction contrary

to the programmed direction may cause overcutting, No. 41 alarm will be given and NC will

stop at the origin of the block.

(iii) To machine a step less than the tool radius

When the program includes a step smaller than the tool radius and it is machined under

circular cutting instruction, the tool center path using normal offset 6.3.6 (3) will become

the reverse programmed direction. Now the first vector will be ignored and the tool moves

the position of the second vector. The tool stops at this point. The program continues to

execute if it is not machining in single block mode.


103

(iv) The startup associated with tool compensation C and the movement in the direction of axis Z

At the beginning of cutting, tool compensation (generally XY plane) shall be preset at a distance from the workpiece and then the tool feed by means of movement along axis Z. Now take note of the following issues if the rapid traverse (positioning) of axis Z shall not be independent of the cutting feed.

Refer to the following program

N1 G91 G00 G41 X50000 Y50000 D1;

N3 G01 Z-30000 F1;

N6 Y100000 F2;

In the above example, N3 and N6 will also be read in buffer register during execution of block N1 and the relationship between them will be properly compensated as shown in the right figure.

Secondly, if N3 (axis Z move instruction) is separated,

N1 G91 G00 G41 X50000 Y50000 D1;

N3 Z-25000;

N5 G01 Z-5000 F1;


104

N6 Y100000 F2;

Since both the move blocks N3 and N5 do not include the XY plane, block N6 cannot enter into the buffer register when N1 starts execution. As a result, the tool center path is calculated by the information N1 in the right figure. In this situation, tool vector will not be generated during start-up, thereby resulting in the overcutting as shown in the right figure.

In this situation, overcutting may be prevented by specifying an instruction of the same moving direction in the blocks before and after axis Z feed instruction using the above rules.

N1 G91 G00 G41 X50000 Y40000 D1;

N2 Y10000;

N3 Z-25000;

N5 G01 Z-5000 F1;

N6 Y100000 F2;

(The moving directions of N2 and N6 are identical)

Blocks N2 and N3 are read in the buffer register and correctly compensated according to the relationship between N1 and N2 during the execution of block N1.

Note 9: Interference verification

Tool overcutting is called “interference”. Interference verification is a function designed to precheck tool overcutting. However, not all overcuts can be checked by the function. There are also some cases that overcutting is not checked.


105

1） The benchmark for overcutting verification

a) In tool compensation, the traveling direction of the tool center path differs from that of sine path (differ by 90°～270°) .

b) During arc machining, the angle difference between the starting point and end point of the tool center path extremely varies from that between those of programmed path except the above state a (more than 180°).

Example of state a:

Example of state b:

(G41)

N5 G01 G91 X8000 Y2000 D01:

N6 G02 X3200 Y-1600 I-2000 J-8000 D02:

N7 G01 X2000 Y-5000:

(Corresponding offset of D01: 1r =2000)

(Corresponding offset of D02: 2r =6000)

In the above example, the arc in block N6 is within a quadrant. However, the arc extends to


106

the four quadrants after tool compensation.

2） Precorrection of interference

(a) Vector travel associated with interference

When tool compensation is performed for blocks A, B and C, the vectors V1, V2, V3 and V4 of blocks A and B as well as the V5, V6, V7 and V8 will be created. The vectors close each other will be first verified. They will be neglected in case of interference. If the vector to be neglected due to interference is a vector at the end of the angle, it will not be neglected.

The interference verification before vectors N4 and N5 →interference→V4 and V5 are neglected.

Verify V2 and V6 → interference → neglect

Verify V2 and V7 → interference → neglect

Verify V1 and V8 → interference → not neglect

If no vector interference is found during verification, the verification will stop.

In case block B is an arc, the arc will make line motion if interference arises.

Example 1: The tool makes line motion from V1 to V8.

Example 2: The line motion of the tool is as follows:

Tool path: V1→V2→V7→V8


107

(b) The tool will stop due to alarm if interference arises after correction (a).

If interference arises at the last vector during correction (a) or there is a pair of vectors at

the beginning of verification and interference arises, the system will give No. 41 alarm and

stop after the completion of the previous block.

Though vectors V2 and V5 are neglected due to interference, interference will arise

between V1 and V6. Now the system gives an alarm and stop.


108

3) Verification is performed even actually no interference arises. See the following examples:

(a) Concave depth less than tool compensation

Though actually no interference occurs, the tool stops due to No. 41 alarm because the

direction of tool path after tool compensation differs from that of programmed path.

(b) Groove depth less than tool compensation

It is similar to (a) and the direction of tool path differs from that of programmed path.

(12) Instructions input through MDI

Compensation is not applicable for the instructions input through MDI. However, the tool path

is as follows after the use of the programmed operations constituted of absolute instructions,

dwell of execution of single block, performing of MDI operations and the restart of automatic

operations.

Under these conditions, the vector at the starting point of the block that follows is translated

while other vectors are created by the next two blocks.

Therefore, compensation is automatically performed from point Pc.


109

When points PA, PB and PC are specified in an absolute instruction, the tool is stopped at the end point of the blocks PA to PB by the single block function. Now the means for translation are

operated by MDI. Vectors 1BV and 2BV are translated to 1BV ′ and 2BV ′ . The 1CV and

2CV between BP —— CP and CP —— DP need to be recalculated.

Since the vector 2BV ′ is not to be calculated, compensation will be accurately performed from

point CP .

(13) Manual inputting interference

Refer to Volume II, Section 4.3.4.3, e), Note 1 for the manual inputting interference during tool compensation.

(14) The tool compensation involving with the 4th axis

Tool compensation cannot be performed for the 4th axis because the offset plane involving with the 4th axis is not provided.

3.6.4 D and H functions

Address D and H are used to specify tool offset and tool compensation. They use the same number and the same compensation value.

Address D differs from H as follows:

D———For tool diameter compensation (tool diameter compensation and tool position offset)

H———For tool length compensation (tool diameter compensation and tool position offset)

The codes and offsets are input in storage through MDI/LCD panel correspondingly so as to specify one two-digit code to perform the relevant compensation. The specified usable value is selected in the following range. No. 30 alarm will be given if a value beyond the range is specified.


110

The compensation specified by H00 and D00 are always 0. H00 and D00 are made certain after power on.

The standard number of tool compensation is 32 (01～32). When options A, B and C are selected for the number of tool compensation, they correspond to 64 (01～64), 99(01～99) and 200 (01～200) respectively.

Note 1: Tool compensation in G40, G41 and G42 modes always use D codes. Tool length compensation (G43, G44, G49) always use H codes. Whether tool offset (G45, G46, G47, and G48) uses D codes or H codes are specified by parameter No.010 BIT3 (OFSD).

Note 2: When an additional tool offset number B is used, make sure to select a part program to save/edit B (40m)～F (1280m).

Note 3: When an additional tool offset number C is used, make sure to select a part program to save/edit C (40m)～F (1280m).

3.6.5 External tool offset

The function is designed for correction of an offset from the outside. For example, using the function on the machine side may input a tool offset and add it to the offset corresponding to the offset number specified by program. In addition, the input value itself may be specified as an offset.

When the machine is provided with an automatic measurement function for tool and workpiece, a difference value in relation to the accurate value may be input in the NC as the amount of correction with the function.

Make sure to operate by following the instruction manual supplied by manufacturer because of machine manufacturers’ difference in programming, operating functions and restrictions.

3.6.6 To input offset through program (G10)

The offsets for tool position offset, tool length compensation and tool radius compensation may be specified by G10 instruction in programming. The instruction has the following format:

G10 P p R r

p: Offset number

r: Offset

Whether the offset is absolute or incremental depends on G90 or G91 mode.

3.6.7 Zooming function (G50, G51)

The zooming of the switch specified in machine program may be performed through instruction. First the zooming scale shall be enabled in No. 64 parameter.

G51 I J K P :

I, J, K: X, Y and Z coordinates in zooming


111

P: Zooming ratio (minimum input incremental: 0.001)

With the instruction, the move instruction that follows is converted by the zooming ratio specified by P and centered on the point specified by I, J and K.

The conversion mode is cancelled by G50.

G50: Zooming mode cancel instruction

G51: Zooming mode

The zooming range that may be instructed is as follows:

0.001x～99.999x (P1～P99999)

P1～P4: The outline of machine program

P1～ P′ 4: The outline after zooming

P0: Zooming center

If P is not specified, the zooming ratio may also be set by MDI/LCD. For the situations that I, J and K are omitted, the point instructed by G51 serves as the zooming center.

The zooming can not be used for offset, e.g. tool radius compensation, tool length compensation and tool position offset.

Note 1: In a single block, G51 shall be specified in G40 mode. G50 may also be specified in offset mode. G51 must always be cancelled by G50.

Note 2: A position is indicated at coordinates after zooming.

Note 3: If a setting is used as a zooming ratio that does not specify P, the setting will be the zooming


112

ratio specified by G51 and it is invalid for any other instruction to specify the setting.

Note 4: Whether the zooming function of all axes is valid may be set by parameter. For G51 mode, the function is always valid for the arc radius instructed by R and is dependent of parameter setting.

Zooming function is always invalid for additional axes.

Note 5: Zooming function is invalid for manual operations, but valid for DNC, automatic operations and MDI operations.

Note 6: Zooming is not applicable for the following movement in the event that axis Z moves in a fixed cycle.

* The cutting depth Q and backing of peck drilling cycle (G83, G73).

* The travel of X and Y in finish boring (G76) and reverse boring (G87) cycles

Note 7: G27, G28, G29, G30 and G92 are specified in G50 mode.

Note 8: Rounding of the zooming result may zero the travel. Now the block is considered as an

unmovable block. Therefore, it may affect the tool movement caused by tool compensation

(see Section 6.3.6 (8)).

Note 9: Reset

(a) Reset in G51 mode changes the original programming coordinate to the current

coordinates or zoomed coordinate. Hence the travel after reset differs depending on

whether the instruction is incremental or absolute.

If it is reset at Point B, Point A in the program shall be regarded as the current B. While

executing the move instruction of Point D, the generation of the following movements

depends on whether they are incremental or absolute.

* Incremental

If the travel from Point A to Point D is incremental, D’ will become the point of destination

on the programmed path and Point D’ is converted to Point E. The tool moves to Point EY

because it is only a move instruction for axis Y.


113

* Absolute

If Point D is absolute, the tool moves to Point E, which is converted from Point D.

(b) When clearance is made by reset by parameter No.007 BIT3 CLER setting.

After switching from G51 to G50, the tool moves to point D’ if the move instruction is incremental (see Fig. A) and to Point D if it is absolute (see Fig. B).

3.7 Cycle Machining Function

3.7.1 External moving function

As instructed by G81X—Y—L—, NC sends out external moving function signal once X—Y— positioning is completed. The machine side performs clamping, drilling and other specific operations and executes cycles according to the signal. Each positioning operation sends out the signal before clearance with G80 instruction. Whether G81 will be reset may be set by parameter No.007 BIT3 (CLER). The system is in G80 mode when it is switched on.

Circular positioning is conducted for L times depending on the numerical value behind the address L and external moving signal is given after each positioning. External moving signal will not be sent out when the blocks excluding X and Y are executed. Besides that G81 is used for external moving function, it can be applied to the following fixed cycles through parameter No.009 BIT5 (MCF) setting.

AD-A＇D＇


114

3.7.2 Fixed cycles (G73, G74, G76 and G80～G89)

In general, a fixed cycle may employ a block including G codes instead of the several blocks

for instructing machining operations in order to simplify programming.

At present, two types (A and B) of fixed cycles are available for your selection. Type A may use

G80, G81, G82, G84, G85, G86 and G89 as listed in the table below while Type B all the G

codes in the table.

Refer to Table 7.2 for the summary of fixed cycles.

G codes Drilling operations

(-Z direction)

Operations in

hole bottom

Backing operations

(＋Z direction) Applications

G73 Intermittent feed —— Rapid traverse

(positioning)

High-speed peck

drilling

G74 Cutting feed Spindle forward

rotation Cutting feed Reverse tapping

G76 Cutting feed Oriented

spindle stop

Rapid traverse

(positioning)

Finished boring cycle

(only for the 2nd group

of fixed cycles)

G80 —— —— —— Cancellation

G81 Cutting feed —— Rapid traverse

(positioning)

Drilling cycle

(fixed-point cycle)

G82 Cutting feed Hold Rapid traverse

(positioning)

Drilling cycle

(counterboring)

G83 Intermittent feed —— Rapid traverse

(positioning) Peck drilling

G84 Cutting feed Spindle reverse

rotation Cutting feed Tapping

G85 Cutting feed —— Cutting feed Boring cycle

G86 Cutting feed Spindle stop Rapid traverse Boring cycle

G87 Cutting feed Spindle stop Manual operation of

rapid running Boring cycle (reverse)

G88 Cutting feed Hold, spindle

stop

Manual operation of

rapid running Boring cycle

G89 Cutting feed Hold Cutting feed Boring cycle

Note 1: Whether the signal [(SRV, SSP) fixed cycle I] output by NC or M codes (fixed cycle II) is used


115

to control the reverse rotation and stop of spindle is determined by parameter No.009 BIT7

(FIX2).

Note 2: In G87 mode, different operations are performed for fixed cycle I and II.

A fixed cycle normally consists of the following six operations.

1. Positioning of axes X and Y

2. Rapidly moving to Point R

Operations 3. Drilling

4. Performing relevant operations at hole bottom

5. Returning to Point R

6. Rapidly moving to initial point

Positioning is performed on XY plane and drilling is conducted in the direction of axis Z. Drilling in other planes or axial directions is not allowed. This is independent of plane selection G instruction.

These fixed cycles are specified in three modes with each specified by a special modal G code.

G90 Absolute!

① Data type

G91 Incremental

G98 Initial-point plane

② Plane of return point

G99 Point-A plane


116

G73 G74 G76

③ G80 See Table 7.2.

G81

G89

Note: Initial-point plane refers to the position of the absolute value in Z direction when fixed cycle cancellation mode changes to fixed cycle mode.

The data indicated in Fig. 7.2.2 depends on G90 or G91 mode.

G90 G91

Figure 7.2.2: Absolute and increment programming （A） During the returning operation, whether the tool returns to Point-R plane or initial-point plane

depends on the setting of G98 or G99. See Fig. 7.2.3.

G98 G99


117

Fig. 7.2.3: Initial-point plane and Point-R plane

The initial point remains constant even touring operations in G99 mode. If the position of previous return is located in Point-R plane, the starting point is Point R. If the position of previous return is in initial-point plane, the initial point is used as the starting point.

（B） After G73, G74, G76 and G81 to G89, specifying the data related to touring may create a block. The data saved in control unit as modal value through the instruction data and related to the machining in a fixed cycle shall be instructed in the following format.

G□□ X———Y———Z———R———Q———P———F———L———:

Hole machining mode Hole position data Hole machining data Cycle times

Hole machining mode:

G□□ (See Table 7.2)

Hole position data X, Y:

Hole position is specified by an absolute or incremental value. Whether the selection of tool path and feedrate will follow group 01 G codes (G02 and G03 are regarded as G01) or unconditionally follow G00 shall be determined by parameter No.009 BIT3 (FCUT).

Hole machining data:

Z: It is necessary to specify the increment of the distance from point R to hole bottom or the absolute coordinates of hole bottom. The feedrate of the operation 3 in Fig. 7.2.1 depends on F codes. Operation 5 feeds at rapid traverse (positioning)rate or the speed specified by F codes depending on different drilling modes.

R: R specifies the incremental value of the distance from the initial-point plane to point R or the absolute coordinates of point R. The feedrate in operations 2 and 6 is a rapid traverse (positioning) rate.

Q: The depth of each machining is specified in G73 or G83 mode and travel value in G76 or G87 (fixed cycle II) mode. (It is always an incremental value.)

P: To specify the dwell time in hole bottom: The relationship between time and specified value is similar to G04 instruction.

F: To specify cutting feedrate

Number of repetitions L: L is used to specify the number of repetitions of fixed cycles (Job 1 to 6). It is considered as 1 when L is omitted.

If L=0 is specified, machining will not be performed though the machining data of hole is saved in the system.

Once a drilling mode (G□□) is specified, it remains constant until other drilling modes or the G codes for fixed cycle cancellation are specified. So it needs not to be specified in each block when the same holes are machined in succession. The G codes for fixed cycle cancellation are the G codes in G80 or Group 01.


118

Once hoe machining data is specified, they remain constant until the data is changed or fixed cycle is disabled. Hence you only need to specify all necessary hole machining holes at the beginning of fixed cycles and change hole coordinate data in fixed cycles.

When necessary, the number of repetitions L shall be specified. The data of L is valid in the specified blocks. The cutting speed specified by F is maintained even fixed cycles are cancelled. Hole machining mode and data remain unchanged, but hole position data and repetitions are cancelled when the control unit is reset during fixed cycles. When the parameter (CLER) for specifying G80 mode for reset is set, however, hole machining data is also cleared.

The example of maintaining and canceling the above data is as follows:

① G00 X—M30:

② G81 X—Y—Z—R—F—L—: The original data Z, R and F of fixed cycles must be specified. Drilling operation is specified by G81 for L times.

③ Y—: When drilling mode and drilling data are the same as block ②, G81, Z, R and F may be omitted. Hole position is moved for Y— distance and drilling is performed once in G81 mode.

④ G82 X—P—L—: Hole position only moves X— in relation to ③. Drilling is performed for L times in G82 mode. Now the drilling data is used as follows.

Z, R and F ………………………Specified in block ②

⑤ G80 X—Y—M05:

Now touring operation will not be performed and all touring data except F codes will be cleared.

⑥ G85 X—Z—R—P—: Since addresses Z and R are cancelled in block ⑤, they shall be specified once again. Now F codes are identical with block ② and may be omitted. Address P is not needed in this block, but it is still saved.

⑦ X—Z—: Hole position has only moved X— and now drilling data is used as follows:

Z…………………Specified in block ⑦

R…………………Specified in block ⑥

F…………………Specified in block ②

⑧ G89 X—Y—: After the positioning movement specified by addresses X and Y, drilling is performed in G89 mode. Now the drilling data is applied as follows:

Z…………………Specified in block ⑦

R…………………Specified in block ⑥

F…………………Specified in block ②

⑨ G01 X—Y—:

Now all hole machining modes and hole machining data (except F) are cancelled.


119

All machining means are described as follows:

（1） G73 (high-speed peck drilling)

G73 (with G98) G73 (with G99)

Backing “α” value is set by parameter No.067 (CYCR).

Drilling may be efficiently performed and cutting easily prevented by axis Z’s discontinuous feed. Backing is carried out at rapid traverse (positioning)rate.

(2) G74 (left-hand tapping cycle)


The instruction specifies that the spindle forward rotate at hole bottom and then perform a left-hand tapping cycle.

Note: If feedrate override is neglected or feed hold occurs during tapping with G74, machining will not stop until the fixed cycle is completed.


120

(3) G76 (Finish boring)


○P Hold

OSS Oriented spindle stop (spindle stops at a fixed point)

Tool motion

Rapid traverse

Cutting feed

Manual feed “d” is set by parameter.

Note 1: G76 can be used only when the output M codes set by parameter No.009 BIT7 (FIX2)


121

are used as the output signals for spindle reverse rotation, spindle forward rotation and spindle

accurate stop.

It is possible to accurately and efficiently perform hole machining and not to damage workpiece

surface by stopping the spindle in oriented position at hole bottom and then removing the tool

bit after it offsets for departing machining. Offset is specified by the address Q (always

positive). The minus sign will be neglected if a negative number is used. An offset direction

shall be preset between (＋X, ＋Y) and (－X,－Y) by parameter No.022 BIT4,5 (PMXY1, 2).

Note that Q value is modal in a fixed cycle mode and indicates the cutting depth in G73 and

G83.

Even at the hole bottom, address I and J may specify offset for the tool. Axes X and Y moves

using linear interpolation according to parameter No.022 BIT6 (SIJ) setting and replace Q with

the incremental value specified by I and J. Hence they may offset upward in any direction.

Feedrate is identical with the speed specified by F codes. I and J are modal in mode of fixed

cycles. Hole machining can not be performed only by specifying I and J. The instructions are

only used to specify I and J again.

(4) G80 (To disable fixed cycles)

The instruction disables fixed cycles (G73, G74, G76, G81～G89). Then NC starts to perform

normal operations. The data of Point R and Point Z is also disabled, namely the tool does not

travel and other machine data is cancelled.

(5) G81 (Drilling cycle, fixed-point drilling)



122

(6) G82 (drilling cycle, boring)

Except that it holds at hole bottom and then retracts, the instruction is similar to G81 (The dwell time is specified by address P). The accuracy of hole depth is improved because it holds at hole bottom. (7) G83 (Peck drilling cycle)


Now the format of the instruction is as follows:

G83 X—Y—Z—Q—R—F—;

Q indicates the cutting depth of each time and always specifies it in incremental value. Rapid traverse (positioning) is changed into cutting feed at a distance of a millimeter or inch from the machined position. Q value is specified in positive number. Minus sign is neglected if it is

G76 (with G98)

G76 (with G99)


123

specified with a negative number. Distance “d” is set by parameter (CYCD).

(8) G84 (Tapping cycle)


Rapid traverse (positioning) Cutting feed

The instruction requires the spindle to counterclockwise rotate at hole bottom and perform a tapping cycle.

Note: Feed override is neglected and it shall not stop until the end of the cycle during the tapping instructed by G84. It will not be affected even Feedrate occurs at this time.

(9) G85 (Boring cycle)


The instruction is similar to G84 except that spindle does not rotate reversely at hole bottom.


124

(10) G86 (Boring cycle)


The instruction is equivalent to G81 except stop at hole bottom and return by rapid traverse.

(11) G87 (Boring cycle/Reverse boring cycle)


Fixed cycle I


125

Fixed cycle II

Not use

Rapid traverse

Cutting feed

Manual feed

Tool offset

Spindle accurate stop

Fixed cycle (boring cycle)

The control system enters into Feedrate mode when the tool reaches the hole bottom and the

spindle stops. In this condition, the tool may travel by manual means. Any manual operation

may be performed. For the purpose of safety, however, the tool shall be withdrawn from the

hole.

To restart machining, it is necessary to switch to DNC or automatic mode and press the

CYCLE START key. The spindle rotates forward after the tool returns to the position of origin or

Point R through G98 and G99. Then the instruction of the next block is executed.

Fixed cycle II (reverse boring cycle)

Once axes X and Y are positioned, the spindle stops and the tool offset in the direction

contrary to the tool nose and is rapidly positioned at the hole bottom (Point R). Here the tool

returns in the original amount of offset. The spindle starts clockwise and performs machining in

the direction of axis Z until Point Z. It does not suspend even under P instruction. After the

spindle stops here again, the tool backs out from the original offset and moves upward. Then

the tool returns to the origin and backs out in the original offset. The spindle rotates forward

and the next block starts. The offsets and directions of axes X and Y are identical with G76

(Refer to G76 and G87 for the setting of direction.)

Note: Fixed cycle I is set by parameter No.009 BIT7(FIX2) and signals SRV and SSP are used

as the output signals for spindle reverse rotation and spindle stop.

Fixed cycle II is set by parameter No.009 BIT7 (FIX2) and M codes are used as the output


126

signals for spindle reverse rotation, spindle stop and spindle oriented stop.

(12) G88 (boring cycle)


Except that the spindle stops rotation after pausing at hole bottom, the instruction is similar to

G87 (fixed cycle I).

(13) G89 (boring cycle)


Though it is similar to G85, the spindle needs to dwell at hole bottom.

3.7.2.1 Repeating a fixed cycle

To repeatedly machine equally spaced holes with the same fixed cycle, it is possible to specify

the number of repetitions with address L, which is up to 9999 and is only valid in some existing


127

block.

G81 X—Y—Z—R—L 5 F—;

X—Y— specifies the first machining position in an incremental value (in G91 mode). If the instruction specifies it in an absolute value (in G90 mode), drilling will be repeatedly performed at the same point.

In a fixed cycle, the time constant of automatic acceleration/deceleration can be automatically switched. It is switched to the time constant of rapid traverse (positioning) or cutting feed depends on all feed motions. After deceleration is completed at the end of the motion, the system switches to the next operation.

In G98 instruction, however, it returns to Point R from hole bottom at rapid traverse (positioning)rate and then to the origin without deceleration.

Notes regarding fixed cycles:

Note 1: Spindle rotation function shall be specified with M codes before specifying a fixed cycle.

ER:

M03: Spindle forward rotation (clockwise)

G□□ ; Correct M05: Spindle stop G□□ ; Incorrect (so specify M03 or M04 before the block)

Note 2: In the mode of fixed cycle, touring operation may be performed provided that the position data corresponding to axes X, Y and Z and the 4th axis are specified in the block.


128

Touring cannot be performed if the position data is not specified. It will not be performed even the dwell instruction (G04 P— ; ) is incorporated. If address X is used to specify the dwell time (G04 X— ; ), touring operation will not be performed.

G00 X— :

G81 X—Y—Z—R—F—P—L— :

; (Not to drill)

F— ; (Not to drill but modify the value of F)

M— ; (Not to drill but perform M function)

G04 P— ; (Not to drill; the P data for drilling will not be modified by the instruction)

Note 3: For the fixed cycles G74, G84 and G86 for controlling spindle rotation, the spindle fails to reach the normal rotational speed before drilling because drilling is continuously performed when the spacing between holes and the distance from the origin to Point R are relatively short. In this case, a G04 (HOLD) shall be instructed to insert between all drilling motions. Therefore, the program below does not specify the number of repetitions with through L.

G00 M—;

G86 X—Y—Z—R—F—;

G04 P—; (Not to drill but to feedrate)

X—Y—; G04 P—; (Not to drill but to feedrate) Whether it is necessary to perform the operation or not depends on the performance of the machine. Refer to the manual supplied by the manufacturer of the machine.

Note 4: The above-mentioned fixed cycles may be deleted with G00, G01, G02 or G03. When G00～G03 is instructed in a fixed cycle, the following motions will be carried out.

# indicates 0, 1, 2 or 3.

G0# indicates G00, G01, G02 or G03.


129

G□□ indicates a fixed cycle.

G0# G□□ X—Y—Z—R—Q—P—F—L—;

(To perform a fixed cycle)

G□□ G0# X—Y—R—Q—P—F—L—;

The tool’s travel along axes X and Y depends on G0# codes. The values of R, P and L will be neglected and F codes saved.

G□□ G0# X—Y—Z—R—Q—P—F—L—;

If 3-axis link function is not provided, the block will cause an alarm.

Note 5: When M codes and a fixed cycle are specified in the same program, M codes and MF signals will be sent out during the first positioning (Operation 1). The machining of the next hole will be performed after receiving the signal FIN at the end of the cycle. The M codes and MF signals are only sent out in the first cycle rather than the cycles that follow provided that the cycles are provided with L instruction for repeated operation.

Note 6: Tool offset instructions (G45～G48) are ignored in the mode of fixed cycles.

Note 7: Tool length compensation (Operation 2 in Fig. 7.2.1) will be performed during the positioning of Point R if it (G43 or G44) is instructed in the mode of fixed cycles.

Note 8: Cautions of operation

(a) Reset

When the control unit is stopped by pressing the RESET key of EMERGENT STOP bottom in a fixed cycle, normally touring mode and touring data will remain unchanged. Fully note this during restarting. Touring mode and touring data may be cancelled by parameter No.007 BIT3 (CLER).

(b) Single block

When a fixed cycle is performed in the single block mode of operation, the control unit will stop at the end points of the operations 1, 2 and 6 in Fig. 7.2.1. As a result, it needs to be started for three times for drilling a hole.

The FEEDRATE lamp illuminates at the end points of Operation 1 and 2. For Operation 6, if repeated cycles do not end up in the block, it will stop in Feedrate mode or other stop mode.

(c) Feedrate

Once the FEEDRATE button is pressed during operations 3 to 5 in G74 or G84, the FEEDRATE lamp will illuminate and the control unit will continue to perform Operation 6 before stop. If Feedrate is available during Operation 6, the operation will immediately stop.

(d) Feedrate override

Feedrate is fixed at 100% during the fixed cycle G74 or G84.


130

(e) Manual absolute value

The MANUAL ABSOLUTE switch is used to switch between the manual operations of G87 (fixed cycle I) and G88 in the two modes below:

ON: Point R and origin are identical with the programming.

OFF: Point R and origin are offset through manual unit.

Note 9: Fixed cycles G74 and G84 may be changed by parameter No.022 BIT2 (FXCD).

The spindle may dwell before forward and reverse rotation using the time instructed by P by setting the parameter.

It is very necessary when using a dedicated tapping device. Thread machining is performed through the forward/backward movement caused by the rotary force of the tap during dwell without the travel of axis Z.

(a) Left-hand tapping cycle G74

G74 X—Y—Z—R—P—F—; G74 (with G98) G74 (with G99)

(b) G84 (Tapping cycle)

G84 X—Y—Z—R—P—F—; G84 (with G98) G84 (with G99)


131

Example 7.2.2: Programming using tool length compensation and fixed cycle.

Example of program

N001 G92 X0 Y0 Z0; Set the coordinate system at the reference point

N002 G90 G00 Z250.0 T11 M06; Tool change

N003 G42 Z0 H11; Origin & tool length compensation

N004 S30 M03; Spindle start

N005 G99 G81 X400.0 Y－350.0 Z－153.0

R－97.0 F120; Drill 1# hole after positioning

N006 Y－550.0; Drill 2# hole after positioning and returning to Point R

N007 G98 Y－750.0; Drill 3# hole after positioning and returning to the origin

N008 G99 X1200.0; Drill 4# hole after positioning and return to the origin


132

N009 Y－550.0; Drill 5# hole after positioning and return to Point R

N010 G98 Y－350.0; Drill 6# hole after positioning and return to the origin

N011 G00 X0 Y0 M05; Return to the reference point and stop the spindle

N012 G49 Z250.0 T15 M06; Tool length compensation and tool change

N013 G43 Z0 H15; Origin, tool length compensation

N014 S20 M03; Spindle starts

N015 G99 G82 X550.0 Y－450.0 Z－130.0

R—97.0 P300 F70; Drill 7# hole after positioning and return to Point R


N017 G99 X1050.0; Drill 9# hole after positioning and return to Point R


N019 G00 X0 Y0 M05; Return to the reference point and stop the spindle

N020 G49 Z250.0 T31 M06; Cancel tool length compensation and change a tool

N021 G43 Z0 H31; Origin, tool length compensation

N022 S10 M03; Spindle starts

N023 G85 G99 X800.0 Y－350.0 Z－153.0 R－47.0 F50;

Drill 11# hole after positioning and return to Point R

N024 G91 Y－200.0 L2; Drill 12# and 13# holes after positioning and return to Point R

N025 G00 G90 X0 Y0 Z0 M05; Return to the reference point and the spindle stops

N026 G49 G91 Z0; Cancel tool length compensation

M02: Program stops

Note: When the number of repetitions L is programmed in G98/G99, the tool returns from the

first drill hole to the origin (G98) or Point R (G99).

3.7.3 Specifying an origin and Point R in a fixed cycle (G98, G99)

G98 and G99 specifies whether the return point in a fixed cycle is the origin or Point R as

shown in Fig. 7.3 respectively. If the return position of the first fixed cycle is the origin, the

starting point of the cycle will be the origin. If it is at point R, the starting point of the cycle will

be Point R. In general, G99 is employed to drill the first hole while G98 the last. To program the

number of repetitions L, G98 shall be specified for the first hole so that the tool may return to


133

the origin.

G98 G99

Fig. 7.3: Origin and Point R

3.8 Spindle Function (S function), Tool Function (T function),

Miscellaneous Function (M function) and Secondary Miscellaneous

Function (B function)

A numerical value is specified behind address S, T, M or B so that BCD signal or strobe pulse

is transmitted to the NC machine. This is mainly used for the switching function of the

numerically controlled machine.

S codes are used for spindle control, T codes for tool change, M codes for switching all the

functions controlling the machine and B codes for swivel table division. Refer to the application

instructions for these addresses and codes supplied by manufacturer.

When a move instruction is specified in the same block as the codes S, T, M or B, the

instruction shall be executed by one of the following two methods.

(i) The move instruction is executed at the same time as S, T, M or B,

(ii) S, T, M or B function is performed after the move function.

(Example): N1 G01 G91 X50.0 Y－50.0 M05: (Spindle stop)


134

Which method shall be selected depends on manufacturer’s setting. In general, both the two methods are available for a numerically controlled machine. Refer to the manual supplied by the manufacture of the machine.

3.8.1 Spindle function (S function)

3.8.1.1 S 2 digits

Spindle speed is controlled by address S and the 2 digits that follow. Refer to the manual supplied by the manufacture of the machine for details.

Note: When S 4 digits are specified after S 2 digits, the last 2 digits will be valid.

3.8.1.2 S 4 digits

Spindle speed (r/min) is directly specified by the 5 digits following address S. The unit of spindle speed (up to 30000r/min) is set by the manufacturer of the machine.

3.8.2 Constant surface speed control

When surface speed (the tool speed relative to workpiece) is specified after S instruction, the

constant speed control function always keeps surface speed unchanged with the change of

the tool position and supplies a control voltage corresponding to the calculated spindle speed

so that the spindle may rotate at correct surface speed.

The units of surface are as listed in the table below:

Input unit Unit of surface speed M (Metric system) m/min Inch (Inch system ) Inch/min

The units of surface speed may vary depending on different manufacturers.


135

3.8.2.1 Instructed methods

The following G codes are specified for the control of constant surface speed.

G code Meaning Unit G96 Constant surface speed control ON m/min or inch/min G97 Constant surface speed control OFF r/min

To exert constant surface speed control, it is necessary to establish a workpiece coordinate system so that the coordinates of center of the rotation axis are 0 (the axis that exerts constant surface speed control).

The axis for constant surface speed control may be selected through programming instruction.

G96P ——;

P1……………………Constant surface speed control is designated to axis X. P2……………………Constant surface speed control is designated to axis Y.

P3……………………Constant surface speed control is designated to axis Z.

P4……………………Constant surface speed control is designated to the 4th axis.

P5……………………Constant surface speed control is designated to 5th axis.

For P0 or that no axis is specified, the present concerned axis is predetermined by No. 315 parameter.

Note 1: To set an axis for constant surface speed control by programming, make sure to specify Pα (α=1, 2, 3, 4 or5). Otherwise the axis set by parameter setting will be under control. Whenever G96 is set again, Pα must be always specified. This is independent of whether G96 Pα is specified before that.

Note 2: The surface speed (S) in G96 is considered as S=0 until M03 or M04 is specified. That is to say, S function cannot be performed before specifying M03 or M04 [only when parameter TCW (the 7th digit of No. 010 parameter) is 1].

3.8.2.2 Spindle speed

The specified surface speed or spindle speed may be overridden in 50, 60, 70, 80, 90, 100, 110 or 120% by the signal from the operation control panel of the machine.

3.8.2.3 Restraint of maximum rotational speed of spindle

During constant surface speed control, the value in rpm following G92 specifies the maximum rotational speed of spindle.

G92 S—:

1234


136

During constant surface speed control, the system will automatically restrain the rotational speed of spindle to the maximum value if the speed is higher than the programmed value.

3.8.2.4 Rapid traverse (positioning) (G00)

In the rapid traverse (positioning) blocks specified by G00, it is impossible to exert constant surface speed control by calculating the surface speed in the position of the tool at all times. However, the control may be achieved by calculating the surface speed from the starting point to the end point of the block. Machining cannot be carried out in the conditions of rapid traverse (positioning).

Note 1: Constant surface speed control is disabled (G97) during power on.

Note 2: Spindle override becomes effective when parameter SOV (the 5th digit of No. 010 parameter) is

preset to 1.

Note 3: The maximum spindle speed cannot be preset (or restrained) during power on.

Note 4: The maximum spindle rotational speed is only restrained in G96 mode. It needs not to be

retrained in G97 mode. However, the spindle motor is restrained by No.136 parameter in G97

mode.

Note 5: G92 S0 means that the spindle speed is restrained to 0 rpm.

Note 6: The S value specified in G96 mode is still saved even after it is switched from G96 mode to

G97 mode. The value will be restored when it is returned from G97 mode to G96 mode.

G96 559: (50m/min or 50 inch/min)

G97 S1000: (1000r/min)

G96 X3000: (50m/min or 50inch/min)

Note 7: When tool length compensation (G43 or G44) was made earlier, programming coordinates

shall be used to calculate the constant surface speed. When tool position offset (G45～G48)

was made, the existing value shall be used to calculate the constant surface speed.

Note 8: When the machine is locked, calculation about constant surface speed shall be made

depending on the change in the coordinates of the axis with constant speed control.

Note 9: Constant surface speed control is also available during thread machining. Therefore, it is

recommended to use G97 instruction to disable constant surface speed control before face

thread and taper thread chasing because servo system does not respond during the change of

spindle rotational speed.

Note 10: Constant surface speed (feed per minute) control mode (G96) is also allowable in G94

mode.

Note 11: When switching from G96 mode to G97 mode, the final spindle rotational speed, in G96

mode, is used as the S codes in G97 mode if S codes (r/min) is predetermined in G97 block.


137

N111 G97 S800: 800r/min

┆

N222 G96 S100: 100m/min ┆

N333 G97: X r/min X the spindle rotational speed X rpm in the blocks before N333, alternatively the spindle speed remains unchanged when the mode has been changed from G96 to G97. ,

The S value newly specified in G96 mode will be enabled when switching from G97 to G96 mode.

If S is not specified, S=0m/min (inch/min).

3.8.3 Tool function (T function)

Tool function is specified by the 2 or 4 digits after address T. The relationship between T codes and the tool is set by the manufacturer of the machine.

3.8.4 Miscellaneous function (M function)

When 2 digits are set after address M, a 2-digit BCD code and strobe signal will be sent out. These signals are designed for the ON/OFF control of the functions of the machine. An M code may be set in a block. When more than two M codes are concurrently set, the last code will be valid. The setting of M codes may vary depending on different manufacturers of machine.

The following M codes have special meanings.

(1) M02, M30: End of program

(i) This indicates the end of the main program and is necessary for recording NC instructions in storage in communication mode.

(ii) Automatic operation stop and reset of NC unit (It is different depending on manufacturers).

(iii) It will return to the starting point of program after the end of the program for M30, and return to the starting point for M02.

(2) M00: Program stops

Automatic operation stops after the end of the block with M00. When the program stops, all modal data remains unchanged as in the operations of a single block. The cycle operation restarts by setting NC start-up (This may vary depending on different manufacturers).

(3) M01: Selection stops

Just like M00, automatic operation stops after the end of the block with M01. The code is valid only when the SELECTION STOP switch on the operation panel of the machine is


138

pressed.

(4) M98: Call of subprogram

The code is intended to call a subprogram. Refer Chapter 9 for details.

(5) M99: End of subprogram

The code indicates the end of a subprogram. It returns to the main program once M99 is executed. See Chapter 9 for details.

Note 1: The block following M00, M01, M02 or M30 cannot be read in the buffer register. Similarly, the next block may set the M codes not to make intermediate conversion through 2 parameters. Refer to the section regarding M codes in the manual supplied by the manufacturer of the machine.

Note 2: Code signal or strobe signal will not be sent out during the execution of M98 or M99.

Note 3: The M codes other than M98 and M99 will be processed by the machine side instead of the NC unit. Refer to the instruction manual supplied by the manufacturer of the machine.

3.8.5 Secondary miscellaneous function (B function)

Worktable indexing is set by address B and the 3 digits that follow. Different manufacturers may have different settings for the division value corresponding to B codes.

3.9 Subprogram

When some areas in fixed sequences or those repeatedly appear are included in a program, these sequences or areas may be saved in storage as subprograms so simplify programming.

A subprogram can be called in automatic mode of operation. A subprogram can also call another subprogram.

That a main program calls a subprogram is called primary call. Secondary call of subprogram is performed as follows.

A call instruction can be used to repeatedly call a subprogram. A call instruction may repeat calling for 9999 times.


139

3.9.1 Creation of a subprogram

Create a subprogram in the following format:

O (: )××××;

; ;

; M99;

Specify a subprogram number after “O” (EIA) or “:” (ISO) at its beginning. M99 is not necessarily set in a single block at the end of a subprogram.

Example:

X M99;

Refer to Sections 5.17 to 5.19 for how to save a subprogram in a register.

Note 1: The subprogram number in the preceding block can also be indicated as “N××××” rather than the (:) following O so that NC program may be compatible with other systems.

The system records the numerical value following N as a subprogram number.

3.9.2 Execution of a subprogram

A subprogram will be executed once it is called by a main program or other subprograms.

A subprogram may be called in the following format:

M98 P— — — — L— — — —: Number of repeated subprogram calls Subprogram number

A subprogram shall be only repeated once in case of omission of L.

Example:

M98 P1002 L5:

The No.1002 subprogram will be called repeatedly for five times when the instruction is executed.

The called subprogram instruction (M98 P—L—) and move instruction may be set in the same block.

Example:

X1000 M98 P1200;

In the above example, No.1200 subprogram is called after the travel in the direction of axis X.


140

Example:

The executing sequence for a main program to call a subprogram is as follows:

The executive process for a subprogram to call another subprogram is similar to the above example.

Note 1: M98 and M99 signals are not sent to the machine.

Note 2: If the subprogram number specified by P is not found, No.78 alarm will be given.

Note 3: The M98 P××××: instruction input through MDI cannot call a subprogram. In this case,

the following program shall be developed in the editing mode and executed with storage.

O××××

M98 P××××:

M02:

Note 4: The blocks or single block containing M98 P—; M99; are invalid. When the blocks of

M98 and M99 contain the addresses other than O, N, L and P, however, the stop of a single

block will be valid.

3.9.3 Special methods of application

The following special methods of application are available.

3.9.3.1 When a sequence number is specified in address P in the last block of a subprogram, control

cannot return to the next block of the called subprogram in a main program, but to the block

specified by the sequence number set by address P. Yet the main program is only valid in the

storage operation mode.

The time required to return to the main program by this means is longer than that in normal

conditions.


141

3.9.3.2

If M99 is executed in a main program, the control will return to its beginning.

If a “/M99;” block is inserted in the proper position in the main program, execution of M99 at this time will enable the control to return to the beginning of the main program and it will be executed again.

“/M99;” will be neglected and the control will go to the next block provided that SKIP OPTIONAL BLOCKS function is enabled.

If “/M99 Pn;” is inserted, the control cannot return to the head of the program but to the blocks of sequence number “n”. The time required for switching to the blocks of sequence number n is longer than that for returning to the starting point of the program.

3.9.3.3

It may be executed in automatic mode as a main program from the beginning of MDI Search subprogram.

In this case, it will return to the beginning of the subprogram if a block containing M99 instruction is executed. When “M99 Pn;” is executed, it will switch to the block of the sequence number “n” and repeatedly execute it.

To stop execution in the above process, it is possible to insert “/M02;” or “/30;” in a proper position if you need to stop the execution. The execution of the above instruction may stop it and disconnect the switch when the SKIP OPTIONAL BLOCKS switch is set to ON.


142

3.9.3.4 M99 Lα Number L of repeated recalls of a subprogram is changed to α in midway when the above instruction is executed.

If the SKIP OPTIONAL BLOCKS switch is set to OFF in the process, the number of repetitions will be changed to zero and the execution of the main program will go on when END OF SUBPROGRAM instruction (M99) is executed.

3.10 User Macro

3.10.1 General

The functions of user macros A and B are basically equivalent. The differences between them are described in section 10.10 (9).

A function is composed of a group of instructions and saved in the storage as a subprogram. The saved function is symbolized by an instruction. Therefore, it is only necessary to specify its symbolic instruction for the function to be executed. The group of saved functions is called “macro body” and is symbolic instruction is called “user macroinstruction”. Macro body may also be called “macro” for short and user instruction called “macro call instruction”.


143

Programmer only needs to memorize macroinstructions in stead of the instructions in macro bodies.

Three points regarding macro: Variables may be used in macro bodies; operations can be performed on the basis of variables; and the variables that may be actually specified in user macroinstructions.

The above shows that annularly distributed screw holes are easy to machine.

Once a macro body for annular holes is programmed and recorded, NC may start machining in it has annular hole machining function.

Programmer may call the annular hole machining function through the following instruction.

G65 P p R r A a B b K k :

p: Macro number of annular holes


144

r: Radius

a: Starting angle of holes

b: Angle between holes

k: Number of holes

In this way user may improve the performance of NC himself. Macro bodies may be supplied by the manufacturer of machine or developed by user.

3.10.2 Variables

In macros, variables are used to replace data of figures. User may define any of their values (in allowable range). The application of macros enables them to more general and flexible.

When using some variables, they are identified by signs.

3.10.2.1 Indication of a variable

As shown in Example 10.2.1, a variable consists of a # followed by a variable number.

#1 (i=1, 2, 3, 4……)

Example 10.2.1: #5

#109

#1005

The format below may also be usable, in which figure is replaced with a formula.

#〔<Formula>〕

Example 10.2.2: #〔#100〕

#〔#1001-1〕

#〔# b/2〕

The variable # i is replaced with #〔<formula>〕hereinafter.

3.10.2.2 Introduction of variables

The values following addresses may be replaced by variables. If a program is <Address># 1 or < Address >-# 1, it means that a variable value or its complement serves as the instruction value of its address.

Example 10.2.3:

F #33 Assuming #33=1.5, it is similar to F1.5.。

Z-#18 Assuming #18=20.0, it is similar to Z-20.0.

G #130 Assuming #130=3.0, it is similar to G3.


145

(1) The addresses prohibited from using variable: 1, :, O and N, namely # 27 or N # 1 or equivalent expressions are not allowed.

The n folds ((n = 1 ～ 9 ) in SKIP OPTIONAL BLOCKS /n cannot be used as a variable.

(2) The method for replacing a variable number with a variable is as follows: When the “5” in # 5 is replaced with “# 30”, it shall not be written as “# #30” but “# (30)

(3) For all addresses, their variable value must not exceed their maximum instruction value. For instance, when #140=120, M #140 exceeds its maximum value (M code shall be less than 99).

(4) Numerical number shall not be used for identification purpose. When #30=02, for instance, F #30 shall be deemed as F2.

(5) – 0 and + 0 are not identifiable, namely when # 4 = - 0, X # 4 is deemed as X 0.

(6) When a variable is used for address data, the numerical value below significant bit shall be rounded (half-adjust)

(7) The numerical value following an address can also be replaced with <Formula>. If < Formula >[< Formula >] or < Formula > - [<Formula >] is used as a program, the value or complement of < Formula> shall be the instruction value of the address.

Caution: For a constant without a decimal point in parentheses, assume there is a decimal point at its end.

Example: 10.2.4:

X [#24+ #18*COS (#1)]

Z- (#18+ #26)

3.10.2.3 Undefined variables

Undefined variable value is called <Empty>. Variable #0 is used for the variable that is always empty.

An undefined variable has the following characteristics:

(1) Introduction of variable

The address itself will be neglected when an undefined variable is introduced.

When #1=<Empty> When #1=0

G90 X100 Y#1 ↓

G90 X100

G90 X100 Y#1

G90 X100

(2) Operational formula

Except <Empty> is used for replacement, it is equivalent to variable O.


146


#2=#1 ↓

#2=<Empty>

#2=#1 ↓

#2=0

#2=#1*5 ↓

#2=0

#2=#1*5 ↓

#2=0

#2=#1+#1 ↓

#2=0

#2=#1+#1 ↓

#2=0

(3) Conditional expression

<Empty> and 0 differ in relation to E Q and N E.


#1EQ#0 ↓

Definite

#1EQ#0 ↓

Indefinite #1 NEO

↓ Definite

#1 NEO ↓

Indefinite #1GE#0

↓ Definite

#1GE#0 ↓

Definite #1GT0

↓ Indefinite

#1GT0 ↓

Indefinite (unestablished)

3.10.2.4 Display and setting of variable

A variable may be displayed on LCD and set by MDI means. See Chapter IV, Section 5.8.2.

3.10.3 Types of variables

Variable may be classified into local variable, common variable and system variable depending on their variable numbers. And these variables have different use and characteristics.


147

3.10.3.1 Local variables # 1～# 33

A local variable is a variable that is locally used in a macro, namely the local variable # 1 for calling a macro at a point of time varies from the # 1 for calling a macro at another point of time (regardless the macros are the same). Therefore, the local variable for Macro A will never be misused for Macro B and damage its variable value as nesting when calling Macro B from A.

Local variable is used for independent variable conversion. See Section 10.7 for the relationship between variable and address. The local variable without independent variable conversion is empty in its original state and user may use them as he like.

3.10.3.2 Common variables #100～ #149 , #500～ #509

Local variable is common in a macro. Common variable is common for all subprograms called by main programs and all macros are common. That is, the # 1 for some macro and the # 1 for another. Therefore, the operation result of the common variable # 1 in a certain macro is usable in another macro.

In this system, no special requirement is made for the use of common variable. They may be used by user.

Common variables #100 to #149 can be cleared by powering off. However, the #500 to #509 common variables cannot be removed by powering off.

3.10.3.3 System variables (for user Macro B)

In this system, the use of system variables is definite.

(1) Interface signals #1000 to #1015 and #1032, #1100 to #1115 and #1132

[Input signal]

The state of interface input signal is determined by the readings of #1000 to #1032 system variables.


148

System variables Interface input signals

#1000 #1001 #1002 #1003 #1004 #1005 #1006 #1007 #1008 #1009 #1010 #1011 #1012 #1013 #1014 #1015

20 UI0 21 UI1 22 UI2 23 UI3 24 UI4 25 UI5 26 UI6 27 UI7 28 UI8 29 UI9

210 UI10 211 UI11 212 UI12 213 UI13 214 UI14 215 UI15

Variable value Input signal

1 Contact ON

0 Contact OFF

Since the reading of variable value 1.0 or 0.0, it is not necessary to take its unit into account. However, unit shall be considered in the development of a macro.

All input signals are read in by reading variable system #1032.

#1032=∑=

+15

02*]1000[#

i

ii

In operational instructions, system variables #1000 to #1032 shall not be used as the item on

the left side [output signal]

Interface output signals may be given by assigning a value to #1100 to1132 system

variables.

System variables Interface input signals


149

#1100

#1101

#1102

#1103

#1104

#1105

#1106

#1107

#1108

#1109

#1110

#1111

#1112

#1113

#1114

#1115

20 UO0

21 UO1

22 UO2

23 UO3

24 UO4

25 UO5

26 UO6

27 UO7

28 UO8

29 UO9

210 UO10

211 UO11

212 UO12

213 UO13

214 UO14

215 UO15

Variable value Output signal

1 Contact ON

0 Contact OFF

All output signals can be output at a time by assigning a value to system variable #1132.

#1132=∑=

+15

0

2*]1100[#i

ii

For #1100 to #1132 system variables, the given final numerical values are stored as 1.0 or

0.0.

Note: When the values of different 1.0 or 0.0 are assigned to #1100 to 1115, <Empty> is

deemed as 0 and all conditions other than <Empty> and 0 are regarded as 1. But the

numerical values less than 0.00000001 are undefined.

Note 1: The figure below indicates the connection for input signals of user macros.


150

Note 2: The figure below indicates the connection for output signals of user macros.

Example 10.3.1 ① The 3-digit BCD data with symbol is read to #100 by changing address.

Composition of DI:

215 214 213 212 211 210 29 28 27 26 25 24 23 22 21 20

Other applications Symbol 102 101 100


151

Composition of D0:

28 27 26 25 24 23 22 21 20

Unused Other applications Addresses

Macro call instruction:

G65 P9100D (address):

The macro body is required as follows:

09100:

#1132=#1132 AND496 OR #7: : To deliver the address

G65 P9101 T60: : Time macroinstruction

#100=BIN [#1032 AND 4095]; : To read 3-digit BCD data

IF [#1012 EQO] GOTO 9100; : With symbol

#100= - #100:

N9100 M99:

② Eight types of 6-digit BCD data (3 digits on the left side of decimal point + 3 digits on the

right of decimal point) with symbol are read to #101 through address change. When D02°=0, 3 digits on the right of decimal point

=1, 3 digits on the left side of decimal point

When D023～21=000, No.1 data

=001, No.2 data

┆

=111, No.8 data


G65 P9102 D (data number):

User macro body is required as follows:

09102:

G65 P9100D [#7*2];

#101=#101+#100/1000;

M99;

(2) Tool offsets #2000～#2200, workpiece offsets #2500～#2906。

Tool offsets use system variables #2001～#2200 while workpeice offsets #2500 and #2906.


152

The offsets are established by reading these variables and changed by assigning values to the system variable #1.

Tool offset No. Tool offset

1 #2001

2 #2002

3 #2003

┆ ┆

┆ ┆

199 #2199

200 #2200

#2000 is readable, but its numerical value is always 0.

Axes Workpiece offset numbers Workpiece offsets

X

External workpiece offset G54 ┆

G59

#2500 #2501 ┆

#2506

Y


G59

#2600 #2601 ┆

#2606

Z


G59

#2700 #2701 ┆

#2706

The fourth


G59

#2800 #2801 ┆

#2806

The fifth


G59

#2900 #2901 ┆

#2906

Example 10, 3, 2 #30=#2005

Substitute the tool offset of the offset number for variable #30.

When the offset is 1.500mm (0.500inch), the value of #30 will change into 1.5 (0.15).


153

#2210=#8

Alter the offset of Offset number 10 so that it is equal to the value of variable #8.

(3) Alarm #3000

When error is found in a macro, an alarm will be given. If the alarm number is specified in system variable #3000, the warning lamp will be lit and NC unit will be in warning state.

#3000=n (ALARM MESSAGE):

Select the alarm number not used in standard specifications and set it in the macro. (n＜200= A warning less than 26 characters may be specified between the note start code and note end code.

(4) Clocks #3001, #3002

It is possible to know the time of the clock by reading the values of system changes #3000 and #3002 for the clock. Time can also be preset by evaluation to the system variable.

Type System variable Unit of time Power on Counting condition

Clock 1 #3001 1ms Reset to 0 Any time

Clock 2 #3002 1hr The same as power off When there is an

STL signal

The accuracies of all clocks fall within 16ms. The accuracy beyond the range of Clock 1 will be reset to 0 at 6536ms. Clock 2 will continue to increase provided that it is not predetermined.

Time cannot be correctly determined in the event that it goes beyond the maximum value 9544hr.

Example 10.3.3: Timing

Macro call instruction

G65 P9101T (wait time)ms;

The macro may be set as follows:

09101;

#3001=0; : Initial setting

WHILE [#3001 LE #20] D01; : Wait for the set time

END1;

M99;

(5) Disable SINGLE BLOCK STOP and wait for end signal of miscellaneous functions

When the following numerical value is assigned to the system variable #3003, SINGLE

BLOCK STOP function will be disabled and the next block will be executed in advance


154

without waiting for the end signal (FIN) of miscellaneous functions (M, S, T and B).

Distribution end signal (DEN) will not be sent without waiting for end signal. Note that a

miscellaneous function

without waiting for end signal will be set after that.

#3003 Single block stop End signal of miscellaneous functions0 Not disable Wait 1 Disable Wait 2 Not disable Not wait 3 Disable Not wait

Example 10.3.4: Drilling cycle (for increment programming) is equivalent to G81.


G65 P9081L (Number of repetitions) R (Point R) Z (Point Z):

The macro body is required as follows:

09081;

#3003=1;

G00 Z#18;

G01 Z#26;

G00Z-[ROUND (#18)+ROUND (#26)];

#3003=0;

M99;

Single block will not stop. #18 corresponds to R and #26 to Z.

(6) Set FEEDRATE, FEEDRATE OVERRIDE and ACCURATE STOP CHECK INVALID in #3004

If the following numerical values are assigned to system variable #3004, the FEEDRATE and

FEEDRATE OVERRIDE of the blocks that follow will become invalid and accurate stop

check will not be performed any more. Press the FEEDRATE key during the execution of

FEEDRATE INVALID block.

① Pressing down and hold the key: FEEDRATE will be executed at the beginning of the

first block of FEEDRATE VALID.

② Pressing and releasing the key: Now the FEEDRATE lamp illuminates. However,

Feedrate is not performed as above, but started at the end point of the first block of


155

FEEDRATE VALID.

#3004 Feedrate Feedrate override Accurate stop

check

0 ○ ○ ○

1 × ○ ○

2 ○ × ○

3 × × ○

4 ○ ○ ×

5 × ○ ×

6 ○ × ×

7 × × ×

○: Valid ×: Invalid

Example 10.3.5: Tapping cycle (for increment programming) (equivalent to G84)


G65 P9084 L (Number of repetitions)R (Point R) Z (Point Z):

The macro body is developed as follows:

09084;

#3003=1; : Disable SINGLE BLOCK STOP

G00Z#18; #3004=7;

G01Z#26; M05; FEEDRATE, FEEDRATE OVERRIDE and ACCURATE STOP CHECK

M04;

Z-#26;

#3004=0;

M05;

M03;

G00Z-#18;

#3003=0;

M99;

Note: “M05” may be omitted for some machines.


156

(7) Variable corresponding to the setting data #3005

Setting data is established by assigning a value to the system variable #3005. Its digits correspond to all setting data when the system variable #3005 is expressed as a binary number.

#3005= X MIRROR IMAGE

Y MIRROR IMAGE A MIRROR IMAGE

TV CHECK PUNCH CODE INPUT UNIT INPUT DEVICE1

INPUT DEVICE2

Example: If #3005=55: instruction is executed, the setting data is established as follows:

X MIRROR IMAGE (X mirror image)=1

Y MIRROR IMAGE (Y mirror image)=1

A MIRROR IMAGE (A mirror image)=1

TV CHECK (vertical check)=0

PUNCH CODE (code standard)=1

INPUT UNIT (input unit)=1

INPUT DEVICE1 (input device 1)=0

INPUT DEVICE2 (input device 2)=0

(8) Modal messages #4001～#4120

The present value instructed by a modal message may be determined by readable system variables #4001 to #4120. Its unit is the unit during instruction

System variables Modal messages #4001 ┆

#40021 #4102 #4107 #4109 #4111 #4113 #4114 #4115 #4119 #4120

G codes (Group 01) ┆

G codes (Group 21) B codes D codes F codes H codes M codes

Sequence numbers Program numbers

S codes T codes


157

Example 10.3.6: Boring cycle (equivalent to G86) during incremental value/absolute value mixed programming


G65 P9086L (Number of repetitions) R (Point R) Z (Point Z):

The macro is developed as follows:

09086;

#1=#4003; : Save Group 03 G codes

#3003=1; : Disable SINGLE BLOCK STOP

G00 G91 Z#18;

G01 Z#26;

M05;

G00 Z-[#18+#26];

M03;

#3003=0;

G#1 M99; : Restore Group 03 G codes

System variables #4001 to #4120 cannot be used for the left item on the left side of the operational instruction.

(9) Position messages #5001～#5105

Position messages may be determined by readable system variables #5001 to 5015. Whether its unit is mm or inch depends on the input system.

System variables #5001# to #5105 cannot be used for the left item on the left side of the operational instruction

System variables Position messages Reading in during

travel #5001 #5002 #5003 #5004 #5005

End position of Axis X block (ABSIO) End position of Axis Y block (ABSIO) End position of Axis Z block (ABSIO)

End position of the 4th axis block (ABSIO)End position of the 5th axis block (ABSIO)

Applicable

#5021 #5022 #5023 #5024 #5025

Actual position of Axis X (ABSMT) Actual position of Axis Y (ABSMT) Actual position of Axis Z (ABSMT)

Actual position of the 4th axis (ABSMT) Actual position of the 5th axis (ABSMT)

Not applicable

#5041 #5042 #5043

Actual position of Axis X (ABSMT) Actual position of Axis Y (ABSMT) Actual position of Axis Z (ABSMT)

Not applicable


158

#5044 #5045

Actual position of the 4th axis (ABSMT) Actual position of the 5th axis (ABSMT)

#5061 #5062 #5063 #5064 #5065

Axis X SKIP position (ABSKP) Axis Y SKIP position (ABSKP) Axis Z SKIP position (ABSKP)

The 4th axis X SKIP position (ABSKP) The 5th axis X SKIP position (ABSKP)

Applicable

#5083 Tool length offset Not applicable

#5101 #5102 #5103 #5104 #5105

Axis X servo position deviation Axis Y servo position deviation Axis Z servo position deviation The 4th servo position deviation The 5th servo position deviation

Not applicable

Abbreviation ABSIO ABSMT ABSOT ABSKP

Meaning

The end position of

the previous block

The actual position of an instruction (identical with

indication POS, MACHINE)

The actual position of an instruction (identical with

indication POS, MACHINE)

The position of the ON SKIP signal in G31

block

Coordinate system

Workpiece coordinate

system

Workpiece coordinate system

Workpiece coordinate system

Workpiece coordinate

system

Tool position Tool length

N/A Applicable Applicable Applicable

Tool compensation

Tool position Tool calibrating spot Tool calibrating spot Tool calibrating

spot

Note: The tool length offset is not valid just between the blocks to be executed, but in the executing blocks. If SKIP signal is not switched on in G31 block, its position is at the end point of the block.

Example 10.3.7:

The tool moves to a fixed point (The distances from XP, YP and ZP to the reference point) and returns to the original position after treatment by programming an intermediate point.


G65 P9300X (Intermediate point) Y (Intermediate point) Z (Intermediate point):

The macro body is developed as follows:

0 9300;

#1=#5001;

#2=#5002;


159

#3=#5003;

G00 Z#26;

X#24 Y#25;

G04; Stop travel because of reading #5021～#5023.

G91 X[XP-#5021]Y[yp-#5022]Z[ZP-#5023]:

(Treatment)┆

X#24 Y#25 Z#26;

X#1 Y#2;

Z#3;

M99;

(10) The setting and display of variable names

The names consisting of up to 8 characters may be assigned to variables #500 to #511 through the following instructions.

SETVNn[α1α2…………α8, β1, β2, …………β8…………]:

n is a starting number of the variable numbers with names.

α1, α2…………α8 are the names of variable number n.

β1, β2, …………β8 are the names of variable number n+1; the same applies below.

All character strings are separated by “, ”. All characters except NOTE END, NOTE START, [, ], EOB, EOR, : (colon for program number) can be used for valid messages. Variable names will not be cleared after power off.

LCD displays in the sequence of NO., NAME and DATA.

Note: Since the function is not available for some devices, #510 and #511 may not be used.

Example 10.3.8

SETVN 500[ABCDEFGH, COUNTER, POINTER];

MACRO VAL： 06： 01234 N3456 NO。 NAME DATA 0500 ABCDEFGH -1234。5678 0501 COUNTER 00020。000 0502 POINTER 0503 1st -0000。4025 0504 2nd -00004。500 0505 124000。00] 0506 0507 0508 START 0509 0510 TOOL-PT 000045。00 0511

P LSK


160

3.10.4 Operation instructions

All types of operations may be carried out between variables. Operation instruction is equivalent to general arithmetically developed program.

#i=＜Formula＞

The right ＜Formula＞ of an operation instruction is the combination of constant, variable, function and operator. Constant replaces #j and #k. The constant with a decimal point in ＜Formula＞ may be deemed that there is a decimal point at its end.

3.10.4.1 Definition and substitution of variable

#i=#j Definition and substitution

3.10.4.2 Additive operation

#i=#j+#k Summation

#i=#j-#k Subtraction

#i=#joR#k Logical sum (for each one of 32 digits)

#i=#jXOR#K Exclusive or (for each one of 32 digits)

3.10.4.3 Multiply operation (Macro B option)

#i=#j*#k Arithmetic product

#i=#j/#k Quotient

#i=# JAND#K Logical multiply (for each one of 32 digits)

3.10.4.4 Function (Macro B option)

#i=SIN[#j] Sine (unit: degree)

#i=COS[#j] Cosine (unit: degree)

#i=TAN[#j] Tangent (unit: degree)

#i=ATAN[#j]/ [#k] Arc tangent (unit: degree)

#i=SQRT[#j] Square root (unit: degree)

#i=ABS[#j] Absolute value

#i=BIN[#j] Switching from BCD to BIN

#i=BCD[#j] Switching from BIN to BCD

#i=ROUND[#j] Rounding


161

#i=FIX[#j] Rounding off the part below decimal point

#i=FUR[#j] Rounding the decimal part to integer part

Note: How to use ROUND function

(1) If function ROUND is used in an operation instruction or in IF or WHILE conditions, the original data with a decimal point shall be rounded off.

Example: #1=ROUND [1.2345];

#1 changes to 1.0.

IF [#1 LEROUND (#2)]GOTO 10:

When #2=3.567, ROUND[#2]=4.0

(2) When the function ROUND is used in an address instruction, it shall be rounded off in its minimum setting unit.

Example: G01 X[ROUND (#1)];

If #1 is 1.4567 and the minimum input increment of X is 0.001, the block will change to G01 X1.457;

This instruction is equivalent to G01 X#1: in the instruction.

The function ROUND in an address instruction mainly applies to the following conditions.

Example: [It is only moved by #1 and #2 in increment and then return to the initial point.]

N1 #1=1.2345;

N2 #2=2.3456;

N3 G01 X#1 F100; : X moves by 1.235

N4 X#2; : X moves by 2.346

N5 X-[#1+#2]; : X moves (because #1+#2=3.5801)

Since 1.235+2.346=3.581, the program cannot return to the starting point through N5.

With N5X-[ROUND[#1]+ROUND[#2] ];

This is equivalent to N5x-1.235+2.346] and the program may return to the starting point.

3.10.4.5 Hybrid operation

The above operations and functions may be combined. The precedence order of operation is function, multiply operation and then additive operation.

Example 10.4.1 #i #j+#K*SIN [#l ]

——①——Operational order

——②——

——③——


162

3.10.4.6 Changing operational order using [ ]

The part that is to be preferred may be put in [ ]. [ ] may be nested for 5 times (including the parenthesis in a function).

Example 10.4.2:

#i=SIN [ [ [ #j+#K ] *#l +#m ] *n ] (triple nesting)

—①——

——②——

————③——

—————④——

———————⑤————

3.10.4.7 Accuracy

To arrange an order with macro order, make sure it has an adequate accuracy.

(1) Data format

The floating point format of the data processed by macro is as follows:

M*2E

Where: M: 1 sign bit +31 binary numbers

E: 1 sign bit +7 binary numbers

(2) Operational precision

Executing an operation once generates the following error. These errors are totalized in repeated operations.

Operational format Average error Maximum error Error type a=b*c 1.55×10-10 4.66×10-10 Relative error a=b/c 4.66×10-10 1.86×10-9

a= b 1.24×10-9 3.73×10-9 │

aε│

a=b+c a=b-c

2.33×10-10 5.32×10-10 min (bε

,cε

)

a=SiNb a=comb

5.0×10-9 1.0×10-9

a=ATANb/c 1.8×10-6 3.6×10-6

Absolute error │ε│ degree

Note: Function TAN executes SIN/COS.

3.10.4.8 Cautions regarding deterioration of precision

(1) Add-subtract operation


163

Note that when absolute values operate subtraction in addition or subtraction, the relative error will not be maintained below 10-8. For example, assuming the actual values of #1and #2 are as follows:

#1=9876543210123.456

#2=9876543277777.777

Execute the operation of #2-#1:

#2-#1=67654.321

The above numerical value cannot be achieved. Since a macro has only a decimal 8-bit precision, the precision of #1and #2 numerical values is degraded and approximates:

#1=9876543200000.000

#2=9876543300000.000

Strictly speaking, the above value differs from internal value because they are binary.

#2-#1=100000.000

Causing a bigger error.

(2) Logic operation

EQ, NE, GT, LT, GE and LE are basically equivalent to add-subtract operation. Hence note the error and make sure that the #1 and #2 are equal in the above example. For instance, IF[#IEQ#2] always fails to make correct judgment.

If IF[ABS[#1-#2]LT50000] is used to make error judgment, #1and #2 are considered equal when the difference between #1and #2 falls within its error range.

(3) Trigonometric function

Absolute may be well guaranteed in trigonometric functions. Since they are not below 10-8, note the conditions of multiplication and division after an operation of trigonometric function.

3.10.5 Control instruction

The control of a program is achieved by using the following instructions.

3.10.5.1 Branch (GOTO)

IF [＜Conditions＞]＝GOTOn

If ＜Conditions＞ is satisfied, the next operation will go to the block with a sequence number n in the program. The sequence number n may be substituted by a variable or [＜Formula＞].

If the condition is not satisfied, it will continue to execute the next block.

IF[＜Conditions＞= can also be omitted, and the program is unconditionally forwarded to block n in this case.


164

＜Conditions＞ is of the following types:

#JEQ#K=

#JNE#K≠

#JGT#K＞

#JLT#K＜

#JGE#K≥

#JLE#K≤

#j and #k may also be substituted with ＜Formula＞ and n with a variable or＜Formula＞.

Note 1: The blocks with a sequence number following n are executed after GOTOn and block shall be preceded by the sequence number n.

Note 2: When executing GOTON, the more distant Nn block is in the same direction, the longer executing time will be.

In the above figure, the executing time increases in the order of . The GOTOn that ①②③④

has been executed for more times only keeps a short distance from Nn block. When the contents of a variable are used for measurement as well as warning, it is recommended not to use the warning program to approach GOTOn statement. The warning program departs from GOTOn. Example 10.5.1: When #1≥10, No.150 alarm will be given.

┆

IF [#1GE10]GOTO150;

The conditions in which no alarm will be given:

M99;

┆

N150 #3000=150;

M99;

(If NEOP (NO.306) is set by parameter, the program will be saved in storage and M99 will not be used as the end of program.)

Note3: During the execution of GOTO, alarm may be given in the following events:


165

① When a macro operation cannot be properly executed in an address。

If GOTO is executed when #1=-1,

No. 119 alarm will be given in the block X[SQRT[#1]];.

② When the conditions specified by WHILE cannot be correctly executed

If GOTO is executed when #1=0,

No. 112 alarm will be given in the block WHILE [10/#1 GE2]D0 1.

In this case, change the following program:

① #2=SQRT[#1];

x#2;

② #2=10/#1

WHILE[#2 GE 2]D0 1; ┆

#2=10/#1;

END 1; Operation instruction does not give an alarm even GOTO is executed.

3.10.5.2 Repeat (how to select Macro B)

WHILE[＜Conditions＞］＝DOm (m=1,2,3)

ENDm

When ＜Conditions＞ is satisfied, the block from DOm to ENDm will be repeatedly executed. That is, when the conditional expression ＜Conditions＞ for judging DOm block is satisfied, the program will go to the next block. When the conditional expression is not satisfied, the blocks following ENDm will be executed. When WHILE[＜Conditions＞＝is equivalent to IF, it may also be omitted. If it is omitted, the program will repeatedly executed from DOom to ENDm.。 WHILE[＜Conditions＞＝DOm and ENDm shall be used in pair and identification number m be used for mutual identification.

Example 10.5.2

#120=1;

N1 WHILE [#120LE10] DO1; Repeat for 10 times

Repeat when #30=1

N2 WHILE [ #30EQ1 ] DO2;

N3 END 2;


166

#120=#120+1;

N4 END1;

Note 1: REPEAT (pay attention to the following points during REPEAT programming)

① DOm shall always be set before ENDm.

┆

END1;

(N/A)┆

DO1;

┆

② In the same program, DOm shall correspond to ENDm one by one.

┆

DO1;

┆

DO1; (N/A)

┆

END1;

┆

DO1;

┆

END1 (N/A)

┆

END1;

┆

③ The same identification number may be used for many times.

┆

DO1;

┆

END1;

┆ (Applicable)

DO1;

┆


167

END1;

┆

④ DO statement may be nested for 3 times.

┆

DO1;

┆

DO2;

┆

DO3;

┆

END3;

┆

END2;

┆

END1;

┆

⑤ DO area must not be crossed.

┆

DO1;

┆

DO2;

┆

END1;

┆

END2;

┆

⑥ It is possible to transfer from the inside to the outside of DO area.

┆

DO1;

┆

GOTO 9000;


168

(Applicable)┆ END1;

┆ N9000….;

┆ ⑦ Transferring from the outside to the inside of the DO area is not allowed.

┆ GOTO 9000;

┆ DO1; (N/A) ┆

N9000…..;

┆

END1;

┆

DO1;

┆

N9000…..;

(N/A)┆

END1;

┆

GOTO 9000;

⑧ It is possible to call a macro and subprograms from the inside of the DO area. DO statement may be nested for three times in a macro body or a subprogram.

┆

DO1;

┆

G65…..; (Applicable)

┆

G66…..; (Applicable)

┆

G67 ; (Applicable)

┆

END 1;


169

┆;

DO1 ;

┆

M98….. ; (Applicable)

┆

END1;

┆

Note 2: As a rule, the time required for TRANSFER is shorter than that for REPEAT.

Example 10.5.3: Wait for the cyclic program whose signal (#10000) is 1

┆

N 10 I F[#1000 EQ 0]GOTO 10;

┆

If

┆

WHILE [#1000 EQ 0] DO 1

END1

Is used for programming, the executing time will be shorter.

3.10.6 Creation and storage of user macro body

3.10.6.1 Creation of user macro body

Macro and subprogram have the same format. O (Program number ):

M99;

Program number is prescribed as follows:

(1) O 1～ O 7999

The numbers are applicable for the programs that can be freely saved, cleared and edited.

(2) O 8000～ O 8999

The numbers cannot be used for the programs for saving and clearing way edition without the setting of relevant devices.

Instruction


170

(3) O 9000～ O 9019

The numbers are applicable for calling type special macros.

(4) O 9020～ O 9899

The numbers cannot be used for the programs for saving and clearing way edition without the setting of the parameters. (5) O 9900～ O 9999

The numbers are applicable for robot operational programs.

Fictitious variable (the variable that macro calls in instruction to receive data) are fixed, namely the addresses of the specified parameters correspond to macro body number through macro call instruction.

Example 10.6.1:

O 9081;

G 00 X#24;

Z#18;

G 01 Z#26;

G00 Z-[ROUND[#18]＋ROUND[#26]];

M99;

Z #24

#18

#26 X

3.10.6.2 Storage of user macro body

A macro is a subprogram and is stored and edited in the same way as a subprogram. Its storage capacity is set with that is combined with a subprogram.

3.10.6.3 Macro statement and NC statement

The following block is called macro statement.

(i) Operation instruction (including =block)

(ii) Control instruction (including block GOTO, DO or END)

(iii) Macro call instruction (including the blocks of the macros called by G65, G66, G67 and G codes)


171

The block other than macro statement is called NC statement.

Macro state differs from NC statement in the following aspects:

(i) Single block does not stop in general single block mode.

(ii) Tool radius compensation C does not serve as “block without travel”.

(iii) The executing time may vary depending on different statements.

(a) If a macro statement are provided after a block without buffer (the M codes without buffer and the blocks of G31), the statement will be executed after the block.

Example 3.1:

N1 X1000 M00; Executing block

N2 #1100=1; Macro statement

Execution of Macro statement N2

N1 Execution of NC statement

Time (b) When a block with buffer is followed by macro statements,

(i) When tool radius compensation C is not used,

The current block will be executed, and at the same time, the next macro statement will be executed until the next NC statement.

Example 3.2

N 1 G01 X1000; Executing block

N2 #1100＝1; Executed macro statement

N3 #1=10; Executed macro statement N4 X2000; Next NC statement Execution of Macro statement N2 N3

N1 Execution of NC statement


172

(ii) Tool radius compensation C mode

(2－1) The first NC statement following the currently executing block is not a block without travel (no block without move instruction in the tool radius compensation plane).

(2－1－1) The 2nd NC statement is also not a block without travel.

The statements after the first NC statement following the executing block are executed.

Example 3.3:

N1 X1000; Executing block


N3 Y1000; The first NC statement

N4 #11001; Executed macro statement


N6 X－1000; The 2nd NC statement

Execution of N4 N5 Macro statement N1 Execution of NC statement (2－1－2) The 2nd NC statement after the executing block is a “block without travel”.

The statements after the 2nd NC statement (i.e. block without travel) following the executing block are executed.

Example 3.4

N1 X 1000; Executing block


N3 Y 1000; The 1st NC statement



N6 Z 1000; The 2nd NC statement

N7 #1101＝1; Executed macro statement N8 #2＝20; Executed macro statement N9 X－1000: The 3rd NC statement

Execution of N4 N5 N7 N8

Macro statement N1 Execution of NC statement


173

(2－2) The first NC statement following the currently executing block is a block without travel. The macro statement cannot be executed.

Example 3.5

N1 Y1000; Executing block

N2 1100＝1; Executed macro statement


N4 # Z 1000; The 1st NC statement (the block without travel)



N7 X－1000; The 2nd NC statement

Execution of NC statement N1

3.10.7 Macro call instruction

Macro may be easily called from a single block or modally from each block by means of calling.

3.10.7.1 Simple calling

The macro body specified by P (programmer) is called during the execution of the following

instruction.

G 65 P (program number)L (Number of repetitions) <independent variable assignment>:

When an independent variable is required to change to macro, it is set by < independent

variable assignment >. The following two types of <independent variable assignment> may

be set. The independent variable herein is the actual numerical value assigned to a variable.

(Note) G65 shall be always specified before independent variable in a block. Minus sigma

and decimal are usable and independent of the address in <independent variable

assignment>.

(1) Independent variable assignment I

A B C D Z

An independent variable other than G, L, N, O and P may be assigned to other addresses.

An address needs not to be assigned alphabetically but specified in the format of words. The


174

addresses that do not need to be specified may be neglected.

The use of I, J and K shall always be assigned alphabetically.

B A D I K True

B A D J I False

The coincidence relation between the addresses assigned to variable assignment I and the

variable number in macro body is as follows:

Addresses of independent variable assignment I

The variables in macro body

A B C D E F H I J K M Q R S T U V W X Y Z

#1 #2 #3 #7 #8 #9 #11 #4 #5 #6

#13 #17 #18 #19 #20 #21 #22 #23 #24 #25 #26

(2) Independent variable assignment II

A B C I J K I J K

Besides that independent variable may be assigned to addresses A, B and C, up to ten

groups of independent variables can be specified with addresses I, J and K. When several

numerical values need to be assigned to the same address, they shall be assigned in the

specified sequence. Unnecessary addresses may be omitted.

The addresses allocated as per independent variable assignment II correspond to the


175

variable numbers of macro as follows:

Addresses of independent assignment I Variables in macro A #1 B #2 C #3 I1 #4 J1 #5 K1 #6 I2 #7 J2 #8 K2 #9 I3 #10 J3 #11 K3 #12 I4 #13 J4 #14 K4 #15 I5 #16 J5 #17 K5 #18 I6 #19 J6 #20 K6 #21 I7 #22 J7 #23 K7 #24 I8 #25 J8 #26 K8 #27 I9 #28 J9 #29 K9 #30 I10 #31 J10 #32 K10 #33

The subscripts 1 to 10 of I, J and K indicate the order of the assigned group.

(3) Concurrently existing independent variable assignments I and II

Alarm will not be given even the independent variables of assignments I and II are within the same block with G65 instruction.


176

If Type I and II independent variables correspond to the same variable, the latterly specified independent variable will be valid. G 65 A1.0 B2.0 I－3.0 I4.0 D5.0 P1000: <Variable> #1: 1.0 #2: 2.0 #3: #4: －3.0 #5: #6: #7 5.0

In the example, the D5.0 that follows is valid though independent variables I 4.0 and D5.0 are set to variable #7.

Example 10.7.1: Reference point setting

Before instructing hole-group machining, the reference point of the hole group shall be set.

X 0 The X coordinate of hole-group reference point

Y 0 The Y coordinate of hole-group reference point


G 65 P9200 Xx Yy;

Shall use the following variables:

#100: hole counting

#101: the X coordinate of the reference point for hole-group macro

#102: the Y coordinate of the reference point for hole-group macro

#24: the X coordinate of the reference point is assigned with a macro call instruction

#25: the Y coordinate of the reference point is assigned with a macro call instruction

Macro body is developed as follows:

09200;

#101＝#24; Notify the reference point to hole-group macro

#102＝#25;

#100＝0; : Reset of hole counting

M99;

Example 10.7.2 Bolt-hole ring

The reference point set with the reference-point setting macro is used as the center of the circular ring. The h holes to be machined distribute on the circular ring at equal spacing. The


177

1st hole is located on the straight line of “a” angle (see the figure below).

The coordinates of the ring reference point for XO and YO bolt-holes

R: radius

A: starting angle

H: number of holes


G65 P9207 Rr Aa Hh;

When h＜0, however, workpiece will be machined clockwise in –h counting.

The following variables shall be used.

#100 hole counting

#101 the X coordinate of reference point

#102 the Y coordinate of reference point

#18 radius r

#1 starting angle a

#11 number of holes h

#30 the storage of the X coordinate of reference point

#31 the storage of the Y coordinate of reference point

#32 Counting shows that the No.1 hole is being machined.

#33 the angle of No.1 hole

Macro body is developed as follows (for absolute programming)

09207;

#30=#101; : Storage of reference point


178

#31=#102; #32=1; WHILE[#32LEABS[#11]]DO1; : Repeat depending on number of holes

#33=#1+360*[#32-1]/#11;

#101=#30+#18*COS [#33]; : Hole position

#102=#31+#18*SIN [#33];

X#101 Y#102;

#100=#100+1; : Hole count plus 1

#32=#32+1;

END1;

#101=#30; ; Return to reference point

#102=#31;

M99;

Example 10.7.3: Unequally spaced oblique line

The point established by the reference point setting macro is used as the reference point. The holes to be machined are arranged by different spacing (1, 12……) in the direction forming an a angle with axis X

Coordinates of X0, Y0

A Angle

I Spacing between holes

K Number of holes set by equal spacing (to be assigned with decimal point)



179

G65 P9203 Aa, I1, Kn1, I12, Kn2…………; When n=1, Kn may be omitted. Using the following variables:

#100 : hole counter

#101 : X coordinate of reference point

#102 : Y coordinate of reference point

#1 : angle a

#4 : No.1 spacing 11

#6 : number of holes n1 of the 1st spacing group 11

#7 : No. 2 spacing 12

#9 : number of holes n2 of the 2nd spacing group 12

┋

#2 : the X coordinate of storage reference point

#3 : the Y coordinate of storage reference point

#5 : Take out hole spacing I1 count

#8 : the distance from reference point to the current hole

The macro is developed as follows (for absolute programming)

09203;

#2=#101; : Storage reference point

#2=#102;

#5=4;

#8=0;

WHILE[#5 LE 31]D01; : Hole spacing assignment I is limited to 10.

IF[#[#5]EQ#0]GOTO 9001; : If the assignment I is＜＞, it will ends.

D02;

#8=#8+#[#5];

#101=#2+#8*COS [#1]; : Hole position

#102=#3+#8*SIN [#1];

X#101 Y#102;

#100=#100+1; : Hole count plus 1

#[#5+2]=#[#5+2]-1;


180

IF[#[#5+2]LEO]GOTO 9002; : Repeat for k times

END2;

N9002 #5=#5+3; : Move to the next assignment I

END1;

N9001 #101=#2; : Return to the reference point

#102=#3;

M99;

3.10.7.2 Modal calling

When executing the following instruction, the macro calling mode may be instructed. During the execution of macro calling mode, calling the specified macro each time executes a move instruction.

G66P (Program number)L (Number of repetitions)＜Independent variable assignment＞:

＜Independent variable assignment＞ is equivalent to the condition of simple calling.

Macro calling mode will be cleared when the following instruction is executed.

G67;

(Note): In G66 block, G66 shall be instructed before all independent variables.

The addresses for＜Independent variable assignment＞ may use minus sign and decimal point.

Example 10.7.4 Drilling cycle

Drilling cycle is performed at all locating points.

G66 P9082 R (Point R)X (Point Z)X (Dwell time):

X ;

M ;

Y Some move block performs drilling cycle within the area.

┋

G67 ;

The macro is as follows (for incremental programming)


181

G9082;

G00 Z#18;

G01 Z#26;

G04 X#24;

G00 Z-[ROUND[#18]+ROUND[#26]];

M99;

Example 10.7.5 Combined type hole group

For a drilling process with the bolt-hole ring as described in 10.7.2 and a unequally spaced hole group on an oblique line as described in the above example 10.7.3, it is necessary to perform it with macro and fixed cycle. The program is as follows:

G81…………;

G65 P9200 X (coordinate of reference point) Y (coordinate of reference point);

G66 P9207 R (radius) A (starting angle) K (number of holes);

G65 P9203 A (angle) I (spacing) K (number) I (spacing);

G67;

3.10.7.3 Multiple calling

It is equivalent to calling a subprogram from another one. It is also possible to call a macro from another one. Multiple calling includes single calling and modal calling. Its number of repetitions is up to 4.

3.10.7.4 Multiple modal calling

In modal calling mode, move instruction is executed whenever the specified macro is called. When several modal macros are specified, the move instruction of the previous macro will be executed whenever the next macro is called. Macros are called by the following specified instructions continuously.


182

Example 10.7.6

G66 P9100; Z10000; (1-1)

G66 P9200;

Z15000; (1-2)

G67; : P9200 Cancelled

G67; : P9100 Cancelled

Z-25000; (1-3)

09100;

X5000; (2-1)

M99;

09200;

Z6000; (3-1)

Z7000; (3-2)

M99;

Executing order (the blocks without instruction are omitted)

(1-1) (1-2) (1-3)

(2-1) (3-1) (3-2)

(2-1) (2-1)

(Note): Since (1-3) is not followed by macro calling mode, modal macro is not called.

3.10.7.5 Calling a macro with G codes

A G code for calling macro may be set by parameter, namely substituted by N G65 P <Independent△△△△ variable assignment>. The same motion may use the following simple instruction.

N G××<Independent variable assignment>

The correspondence between calling macro with G code xx and calling the program number may be set by parameter.△△△△


183

The program number for calling G code xx and calling macro is set in parameters.△△△△

Except G00, up to 10 of G01 to G255 can be selected to call macro. These G codes cannot be specified through MDI panel like G65 instruction. The G codes cannot be set in the macro calling instructions for G codes and used in the subprogram calling instructions with M codes.

Set the following parameters: 0323 The G code for calling macro: 9010

0324 The G code for calling macro: 9011

┋

0332 The G code for calling macro: 9019 Example 10.7.7 : Clockwise machining with G02

G02 I (Radius)D (Offset number);

(1) Set the following parameter

Macro body: 9010 calls G code=12

(2) Record the following macro body

09010;

#1-ABS[#4]-#[2000+#7];

IF[#1 LEO]GOTO 1;

#2=#1/2;

#3003=3;

G01 X[#1-ROUND[#2]]Y#2;

G17 G02 X#2 Y-#2R-#2;

I-#1;

X-#2 Y-#2 R#2;

G01 X[#-ROUND[#2]]Y#2];

#3003=0;

N1 M99;

3.10.7.6 Calling a subprogram with an M code

The M code set by parameter may be used to call a subprogram. The instruction of N G X Y ……M98P : may be substituted by the following simple instruction.△△△△

N G X Y ……M××:


184

For M98, a subprogram is indicated on COMND page, but MF and M codes are not sent.

The correspondence between calling macro with M code xx and calling the program number may be set by parameter.△△△△

Except the No. 35 and 36 M30 parameters MBUF1 and MBUF2, at most 3 of M03 to M97 can be used for macro calling.

Instruction may be specified through MDI keypad. In the macros called by the means that a G code calls a macro or in the subprogram called by the means that a T code calls a subprogram, the subprograms of the specified M codes cannot be called like common M codes. Set the following parameters: 0320 The M code for calling macro: 9001

0321 The M code for calling macro: 9002

0322 The M code for calling macro: 9003

Example 10.7.8 : Through the ATC fixed cycle of M06

(1) Set the following parameter

Subprogram: the M code called by 9001=06。

(2) Record the following macro bodies:

09001;

#1=#4001;

#3=#4003;

G28 G91 Z0 M20;

G28 Y0;

M21;

G00 Z10000;

M22;

G28 Z0;

M23;

G#1 G#3 M99;

3.10.7.7 Calling macros with M codes

The M codes set by parameter may call a macro, i.e. N—G65 P <Spe△△△△ cified variable>

Operation is performed when using the following instruction instead.

N—M××<Specified variable>

The calling of the program number of macro is set by relevant parameter.△△△△


185

Except a part of specified M codes, up to 10 of M06 to M255 can call macro. However, this type of M code cannot be input through MDI like G65 or used in the subprograms called with G code, M code and T code.

Set the parameters as follows:

043

052

3.10.7.8 Calling a subprogram with a T code

The T codes set by parameter may call a subprogram.

N G X Y ………………………Tt;

Operation is performed when using the following two instructions of the program instead.

#149 = t;

N G X Y ………………………M98 P90000;

The t in T codes is saved as the independent variable in variable #149. T codes are displayed on COMND page, but TF and T codes are not sent. They may be specified through MDI but cannot be instructed in the blocks with the M codes for calling a subprogram.

In the macro called by the means for G codes to call a macro as well as in the subprogram called by the means for M or T codes to call a subprogram, these T codes does not call a subprogram but are treated like common T codes when instructed.

Set the following parameter:

0306

3.10.7.9 The position of the decimal point of an independent variable

Independent variable is usually specified with a decimal point. If a decimal point is not specified, the position of the decimal point is assumed as follows:

Addresses Input in mm Input in inch A, C 3 (2) 3 B (B 3-digit is not selected) 3 (2) 3 B (B 3-digit is selected) 0 0 D, H 0 0 E, F (in G94 mode) 0 (1) 2 E, F (in G95 mode) 2 (3) 4 I, J, K 3 (2) 4 M, S, T 0 0 Q, R 3 (2) 4

User macro body: 9020 calls M mode

User macro body: 9029 calls M mode

TMCR


186

U, V, W 3 (2) 4 X, Y, Z 3 (2) 4

The positions of the decimal point are calculated from the least significant bit for the numerical values listed in the above table.

The numerical values in () indicate the number of the digits on the right side of the decimal point. For addresses E and F, parameter FMIC=1.For other addresses, MIC=1.

3.10.7.10 The difference between M98 (calling a subprogram) and G65 (calling a macro body)

(1) G65 may contain an independent variable, but M98 not.

(2) After executing an instruction other than M, P or L in M98 block, the use of M98 goes to a subprogram but G65 only transfers.

(3) When M98 block contains an address other than O, N, P and L, a single block stops execution, but G65 block not.

(4) G65 may change the level of a local variable, but M98 cannot. That is to say, the #1 specified before G65 is different from the #1 in a macro. The #1 specified before M98 is identical to the #1 in a calling subprogram.

(5) It is possible to call a nesting for 4 times when G65 is combined with G66. M98 can also call for 4 times (when Macro A or B is selected).

(6) During automatic operation, M98 can achieve 4 calls at most in TAPE mode or MEMORY mode when an operation is inserted through MDI. One or two codes may achieve 4 calls in MDI mode. G65 can achieve up to 4 calls in all modes.

3.10.7.11 The nesting and local variables of user macro

When G65, G66 and G codes are used to call a macro, the nesting degree (level) of its macro increases by 1 and the level of its local variable also increases by 1.

The relationship between macro calling and local variable is as follows:

Local variables


187

① Note that local variables (Level 0) #1 to #33 are provided in a main program.

② When a macro (Level 1) is called by G65, the local variable (Level 0) of the main program is saved, the local variables #1～#33 (Level 1) of the new macro (Level 1) are prepared and the substitution of the independent variables are possible (the same for

).③

③ Each group of local variables (Levels 1, 2 and 3) are saved ant new local variables (Levels 2, 3 and 4) are prepared whenever a macro (Levels 2, 3 and 4) is called.

④ When using M99 to return from each macro, the local variables (Levels 0, 1, 2 and 3) saved in and are restored as they are saved. ② ③

3.10.8 The relationship with other functions

(1) MDI operation

Macro call instruction, operation instruction and control instruction cannot be specified with MDI.

During the execution of a macro and the stop of a single block, the MDI instructions other than those are related to macros may be executed.

In macro calling mode (G66), inputting a move instruction by MDI cannot perform macro calling.

(2) Sequence number retrieving

The sequence numbers in a macro body cannot be retrieved.

(3) Single block

The blocks other than macro call instruction, operation instruction, control instruction sometimes may be processed in single block stop mode in a macro.

The blocks of macro call instruction (G65, G66, and G67), operation instruction and control instruction do not stop in the workpiece with single block.

However, the blocks other than macro call instruction may perform single block stop and be set through the following settings and parameters.

For the check of a macro body

0318

0319

MCS9

MCS8 MCS7


188

When MCS7 = 1, single block stop will be performed in the macro statements in 01 to 07999 and 09900～09999.

When MCS8 = 1, single block stops in the macro statements in 08000～8999.

When MCS9 = 1, single block stops in the macro statements in 09000～9899.

However, when single block stops in a macro in offset compensation mode C, it is assumed that it does not to move. Sometimes wrong compensation is also performed (strictly speaking, instructing movement is similar to that the amount of movement is zero). The assumption is preferential for the single block stop restraint of #3003. In a word, when MCS7, 8 and 9 are equal to 1, #3003 will be equal to 1 (also called 3) in the programs in all program sequence numbers. All single blocks will be restrained. Here MCS7, 8 and 9 are the parameters for the inspection of macros. Therefore, the parameter shall be set to 0 at the end of macro inspection.

(4) Skip optional blocks

When / code appears in <Expression> (on the right side of working equation or in [ ]), it may be deemed as a division operator rather than an optional block.

(5) Operation in EDIT mode

In order to prevent damage caused by misoperation, the recorded macro bodies and subprograms may be set as follows.

0318

0319 Here PRG8 = 1 corresponds to the user macros and subprograms of program numbers 8000～8999 while PRG9 = 1 to those of 9000～9899. Recording, clearance and edition are not allowed. However, clearance of all blocks and output of single programs can be carried out upon tenderization.

(6) Indication of the program numbers other than EDIT mode

As a rule, the called programs will be displayed when calling a user macro and a subprogram. The following setting may be used to maintain the foregoing programs.

0318

0319 MPD8 = 1 corresponds to the user macros and subprograms of program numbers 8000～8999 while MPD9 = 1 to those of 9000～9899. These programs are not displayed in the PROGRAM page for the modes other than EDIT.

(7) Reset

When reset function is used for clearance, all local variables and public variables #100 to #149 are in <Empty> mode and system variables #10000 through #1132 cannot be cleared.

PRG9

PRG8

MPD9

MPD8


189

The calling mode of user macro and subprogram as well as the state of D0 will be cleared and the main program be returned to in the cases other than the clearance in MDI mode. For the clearance in MDI mode, only the calling state in MDI mode is cleared.

(8) Macro statements and NC statements

The following blocks indicate the statements of a macro.

① Operation instruction (= is also included in the block)

② Control instruction (G0T0, D0 and END are included in the block)

③ Macro call instruction (G65, G66, G67 and the G codes for calling a macro are included in the block).

The blocks other than macro statements are NC statements.

(9) MDI’s interference in automatic operation

When the MDI in automatic operation is used to insert a macro, up to 4 levels of the nesting degree called by macros and that of D0 can be continuously called from the beginning of automatic operation.

(10) The display of PROGRAM RESTART page

The M and T codes used for calling a subprogram are not displayed like M98.

(11) Feedrate

When Feedrate is set to ON, the execution of macro statement stops (also stops during alarm clearance).

3.10.9 Special codes and words used in user programs

Besides those for common programs, the codes used in user macros include the following codes:

(1) ISO

Meaning Binary encoding Symbol [ ] # * = 0 +

1 1 0 1 1 ° 0 1 1 1 1 0 1 1 ° 1 0 1 1 0 1 0 0 ° 0 1 1 1 0 1 0 1 ° 0 1 0 1 0 1 1 1 ° 1 0 1 1 1 0 0 1 ° 1 1 1 0 0 1 0 1 ° 0 1 1

[ ] # * = 0 +

(2) EIA Meaning Binary encoding Symbol

[ ] # *

0 0 0 1 1 ° 1 0 0 0 1 0 0 1 ° 1 0 0

Parameter setting 0 0 0 0 1 ° 1 1 0

&


190

= +

0 0 1 1 1 ° 0 1 1 0 1 1 1 0 ° 0 0 0

, +

0: The 0 code similar to the 0 of program number shall be used.

The # of EIA codes and code format shall be set by parameter.

However, Chinese characters cannot be used. Latin letters are usable. If # is used, note that its original meaning is not applicable.

Parameter No.

0317 The special characters used by Macro A are as follows: OR, XOR, IF, GOTO, EQ, GT, LTT, GE, LE.

The special characters used by Macro B are as follows:

AND, SIN, COS, TAN, ATANN, SQRT, ABS, BIN, RCD, ROUND, FIX, FUP, WHILE, DO, END.

3.10.10 Restrictions

(1) Usable variables

#0, #1～#33, #100～#149, #500～#509 and system variables

(2) Usable variable value

Maximum ±1047, minimum ±10－39

(3) Rated numerical value used in <Expression>

Maximum ±99999999, minimum ±0.0000001

Decimal point: usable

(4) Operational precision: decimal 8 digits

(5) Nesting degree of macro calling: up to 4 levels

(6) Repetition Identification number: 1～3

(7) Nesting of [ ]: up to 5 levels

(8) Nesting degree of subprogram calling: up to 4 levels

(9) The above-mentioned functions: User Macro B may perform all of them while A can only perform the following operations.

(i) The variables beyond the amount are applicable.

(ii) The following operations may be performed between variables:＋, －, OR, XOR.


191

(iii) IF [ <Conditions> ] GOTO n is applicable.

(iv) Simple calling and modal calling are possible.

3.10.11 Descriptions for P/S alarm

① Alarm No.004

Addresses are not found in proper positions

(Example): X1*1:

No.004 alarm will be given when “*” instead of the next address appears after X1.

② Alarm No.114

The formats other than <Formula> are incorrect. This type of alarm indicators up a lamp in the following conditions:

(a) The characters following an address shall not be numerical values, • , －, #, [, ＋

(Example): XF1000:

XSIN [ 10 ]: (b) The formats other than IF (also called WHILE)[ <Formula>ΔΔ<Formula> ]

(Example) IF [ #1 EQ #2 ] GOTO 10:

WHILE [ #1 SIN#2 ] DO1:

3.10.12 Examples of user macros

3.10.12.1 Groove machining

User macro performs fixed cycles of groove in the range of the figure below, where Z is the machining range of certain depth and z the cutting amount of the machining range.

(1) User macro call instruction


192

G65 P9802 X x Y y Z z R r Q q I I J j K k T t D d F f E e *

The meaning of all addresses

xy: Absolute coordinates of the axes X and Y (Left bottom corner of the groove) at the origin.

zr: Absolute coordinates of Point Z and Point R (See the figure)

g: The cutting amount of each machining (positive)

ij: The lengths (positive) in the directions of X and Y in machining area (see the figure) (the machining efficiency will be higher when i> j.

k: Allowable amount at the end

t: The machining width shall not exceed the tool radius xt%

d: Tool radius compensation number (01～99)

f: The feedrate in xy plane

e: The feedrate during cutting in, the feed is at 8Xe feedrate 1mm before cutting in.

(2) User macro body 0 9802;

#27＝#[2000＋＝#7];

#28=#6+#27;

#29=#5-2*#28;

#30=2*#27*#23/100;

#31=FUP[#29/#30];

#32=#29/#31;

#10=#24+#28;

#11=#25+#28;

#12=#24+#4-#28;

#13=#26+#26+#6;

G00 X#10 Y#11;

Z#18;

#14=18;

D01;

#14=#14－#17;

IF[#14GE13]GOTO 1;

#14=#13;


193

N1 G01 Z#14 F#8;

X#12 F#9;

#15=1;

WHILE[#15 LE #31] D02;

Y[#11+#15*#32];

IF[#15 AND 1 EQO]GOTO02;

X#10;

GOTO 3;

N2 X#12;

N3 #15=#15+1;

END2;

G00 Z #18;

X#10 Y#11;

IF[#14 LE#13]GOTO 4;

G01 Z[#14+1F[8*#8];

END1;

N4 M99;

3.10.13 External output instructions

Besides typical user macro instructions, the following macro instructions (external output instructions) may be executed.

(a) BPRNT

(b) DPRNT

(c) POPEN

(d) POLOS

These instructions are for the purpose of outputting values and texts of variable through RS232 interface.

These instructions shall be instructed in the following order:

① OPEN instruction: POPEN

Get external I/O equipment interface ready before outputting a series of data instructions.

② Data output instruction: BPRNT and DPRNT


194

Execute the necessary data output instructions.

③ Close instruction: POLOS

The instruction shall be used at the end of all data output instructions to disable external I/O devices and interfaces.

3.10.13.1 OPEN instruction: POPEN

POPEN: While an external I/O device and its interface is executing an instruction, the instruction shall be executed to output DC2 control code from the NC side before outputting a series of data instructions.

3.10.13.2 Data output instruction BPRNT DPRNT

(1) BPRNT [ a #b [o] －－－－ ]

Character Variable Number of effective digits after decimal point

The output of characters and binary output of variables are performed during the execution of BPRNT instruction.

(a) Characters: Instructed characters output as ISO codes. The characters that can be instructed include:

Latin letters (A～Z)

Numerical values

Special characters (*,/,+,-)

“*” is output as a space code.

(b) Since all variables with a decimal point will be saved. The number of the valid digits after decimal point is indicated with the parentheses following a variable instruction. The variable value that takes the digits after decimal point into account is indicated with a 2-character data (32bit) and starts from high byte outputting in binary data.

(c) EOB codes outputs with ISO codes after outputting instruction data.

(d) The variables of <Empty> cannot be output (with 114#p/s alarm)

(2) DPRNT [ a #b [ c d ] Number of the digits after decimal point Number of the digits before decimal point Variable Character

The output of characters and digits of numerical values may be performed with ISO codes during the execution of DPRNT.

(a) Refer to the descriptions for the points (a), (c) and (d) of BPRNT instruction.


195

(b) During the output of a variable value, the variable number is specified after character #. Here the numbers of the digits before and after decimal point are specified in parentheses.

The number of digits of a variable value starts from high-byte valid digit. Each digit and its decimal point are output through ISO codes.

A variable value consists of up to eight digits. If its high-byte digit is 0, then no code will be output when No. 315 parameter PRT=1 and space code is output when PRT=0.

Whenever no decimal is output, + code outputs space code when No.315 parameter PRT=0 in the situation of its sign is positive (+). No code will be output when PRT=1.

3.10.13.3 Close instruction PCLOS

PCLOS

To release the machining link of external I/O unit, the instruction is specified at the end of all data output instructions. DC4 control codes are output through NC.

3.10.13.4 Necessary settings for using the function

(1) Set No.341 parameter so as to use the output unit RS232C for communication outputting.

(2) Set all data (baud rate, etc) of the RS232C interface for one of No. 310 to 313 parameters according to the above output unit predetermined for No.341 parameter.

(3) Set the ISO codes as output codes.

(4) Set No.315 parameter so as to determine whether to put space for the preceding 0 when outputting data with DPRNT instruction.

7 6 5 4 3 2 1 0 The leading zero is treated by PRT DPRNT instruction as follows during the output of data.

0: Output space 1: Not output

3.10.13.5 Cautions

(1) It is unnecessary to continuously set the open instruction (POPEN), data output instruction (BPRENT, DPRNT) and close instruction (PCLOS). After setting the open instruction at the beginning of a program, it is not necessary to set the open instruction until the close instruction is set.

(2) Open instruction and close instruction shall be set in pair without omission.

That is, close instruction shall be given at the end of a program. It is impossible to individually set the close instruction without the open instruction.

(3) Reset the data output instruction in the execution of stop program and cancel the data

0 PRT 5 1 3


196

that follows.

If the reset process is instructed by with M30 or a similar instruction at the end of a data output program, you need to specify the close instruction at the end of the program and to wait until all data is output before the start of M30 or other reset process.

(4) It is necessary to select Macro B and I/O interface for the function.

3.10.14 Macro interruption function (Macro B)

If a interruption is input for NC between M96 PX X X X; and M97; blocks, control will go to PX X X X program.

Setting M99; program returns from the original program. The sequence number of the original program returned to may be set with address P.

(Note 1): Refer to Appendix 11 for the details of the functions of macro.

(Note 2): Make sure to refer to the operation manual supplied by the manufacture of the machine when using this function.

3.11 Tool Life Management Tools are divided into serial groups. Specific tool life (in time or number of cycles) is specified for each group. The so-called tool life management function refers to the capability of totalizing the tool life of all groups in service and replacing a tool in the predetermined order in the same group.

3.11.1 Setting of tool groups

The order of the tools in each group and the life of each tool are preset in the NC device in the following format.

Format Meaning O □□□□ G 1 0 L 3 P □□□ LΔΔΔ

Program number To set the beginning of tool groups What follows P is the group number of N01~128


197

TΔΔΔΔH O O D □□ TΔΔΔΔH O O D □□

┆ TΔΔΔΔH O O D □□; P □□□ LΔΔΔ; TΔΔΔΔH O O D □□;

┆ G11: M02(M30):

What follows L is the tool life of No.1～9999 tools (Note 1) (1) What follows T is a tool number (2) What follows H is a tool length offset number

What follows D is a tool offset number （N） Tool selecting order: (1), (2) till (N)

The data of the next group

To set the end of tool group End of program

The setting procedures are as follows:

(i) Like the general DNC functions, press ENTER in “EDIT” mode after activating the DNC

communication interface. Programs will be loaded into the part program storage and get

ready for display and edition.

(ii) In storage mode, perform a cycle starting operation so as to run the programs. Data will

be saved in the tool life data area. At the same time, the tool life data of all tool groups

saved earlier will be deleted and the tool life counter cleared. Once data is saved, it will

not lose even after power failure.

(iii) In the operation of Step (i), perform a cycle starting operation in DNC mode and save the

contents of the program directly into the tool life data area through RS232. Now display

and edition cannot be performed as Step (i).

(Note 1) Whether tool life will be indicated in time (min) or frequency (number of cycles) shall

be set by parameter (309－LOTM).

(Note 2) One of the following four groups may be selected for tool group number and tool

numbers (309－GST1,GST2)

In any type of combination, up to 256 tools can be saved. At most 16 groups can be selected

for group , each group having 16 tools. Gr① oup may have 32 groups at most and each ②

group may have 8 tools, and so on. A type of combination may be changed by modifying its

parameters and then switching off and on the power supply.

Group No. Tool No.

①

②

③

④

16

32

64

128

16

8

4

2

(Note 3) H codes and D codes can be omitted when they are not to be used.


198

(Note 4) The same tool number may appear for many times or appear in any position in set

data. The following is an example of program format.

Data of No.1 group

Data of No.2 group

Data of No.3 group

(Note 5) The tool group numbers specified by P are not necessarily continuous and all savable tool groups need not to be set.

3.11.2 Setting in machining processes

Tool groups are set by T codes as follows in machining processes.

Program format Meaning

00001; G10L3; P001 L0150; T0011 H02 D13; T0132 H05 D08; T0068 H14 D16;

P002 L1400; T0061 H15 D07; T0241 H25 D04; T0134 H17 D03; T0074 H08 D21; P003 L0700; T0012 H14 D08; T0202 H22 D02; G11; M02;


199

T▽▽▽▽ M O 6 T □ □ □ □; H□□; D 0 0 T△△△△ ; M O 6 T▽▽▽▽; M 0 2 ( M 3 0 );

To use tool group number + tool life administration invalidation number (Note 1) at the beginning of the next M06 instruction. The tools specified by □□□□ (Note 2) are concluded and those specified by are s▽▽▽▽ tarted.

99 : The tool offset specified by valid group number 00 : Cancellation of tool length offset 99 : The tool compensation specified by valid group number. 00: Cancellation of tool compensation To use the tools set by after the next △△△△ M06 instruction. Tool end number and tool start number ▽▽▽▽ △△△△ End of machine program

(Note 1) It is set by tool life administration invalidation number from T 0 0 0 0 to △△△△

T as common T code instructions without tool life administration. When T△△△△ tool code plus group number is specified, the tool life administration of the concerned group △△△△

is administrated. Tool life administration invalidation number is set by parameter.

For example, when the value is 100, T0000 through T0100 will be output as common T codes. When T0101 is specified, the T codes of the tools in No.1 group that have not reached their service life will be output.

(Note 2) The above program format is used for tool return number instruction mode. Tool return instruction is required for tool change. It is not required for other instructions. After that, the T codes of M06 can be neglected. Now the similar tool change operation is performed as above.

The following is an example of the program format whose tool life administration invalidation number is 100 in a tool return number instructing method.

Program format Meaning


200

…………… T 0 1 0 1; …………… M 0 6 T 0 0 0 3; …………… G 4 3 H 9 9; …………… G 4 1 D 9 9; ………… D 0 0; ………… H 0 0; …………… T 0 0 0 5; ………………… M 0 6 T 0 1 0 1;

What follows the next M06 instruction is No.1 group of the used tools.

End of the currently used No.0003 tool and start of using No.1 group of tools The setting of the tool length offset number used in No. 1 group The setting of tool offset number used in No. 1 group Cancellation of tool compensation Cancellation of tool length compensation To use No.0005 tool after the next M06 instruction End of No.1 group of tools and start of No.0005 tool

3.11.3 Performance of tool life administration

3.11.3.1 Tool life calculation

(1) When tool life is determined in time (min)

Now, T (△△△△ △△△△＝tool life administration invalidation number＋tool group number) and M06 are instructed in succession. M06 is specified in machine program again. In cutting method, the actual time of tool usage is calculated by specified time interval (4s). The time for single block stop, Feedrate, rapid traverse (positioning), dwell, etc is not included. The maximum set life value is 4300min.

(2) When tool life is determined in number of cycles

Whenever a cycle starting operation is performed, it operates until M02 or M30 is instructed and NC reset. Then the counter for the used tool group increases by 1. The counter increases by 1 even a group is instructed for several times in the same program. Life value is up to 9999. Each group of calculated life and contents of counter will not lose after power failure.

(Note) For specifying life in number of cycles, EXTERNAL RESET (ERS) or RESET AND REWIND (RRW) signal is input in NC when M02 or M30 is executed.

3.11.3.2 Tool change signal and tool change reset signal

Another tool will be selected in the predetermined order after the end of tool life. When the last tool in the same tool group has reached its service life, a tool change signal will be given. The tool to be changed is displayed on LCD. Then the relevant group number is specified


201

and tool change reset signal input or MDI panel (see 3.11.4.3) operated. All data such as life counter *,@, etc (see 3.11.4.2) are cleared. All tool groups are changed and reset when tool change signal is automatically released at the end of tool life. After machining is restored, the group starts selection from the first tool.

(Note) For specifying tool life in time, tool change signal is output once it has reached service life and machining goes on until the end of program. For specifying tool life in number of cycles, tool change signal is output in case of M02 or M30 reset at the end of tool life.

3.11.3.3 New tool selection signal

When a new tool is selected from a group, tool T code and new tool selection signal are output at the same time. When a new tool is selected, the signal may be used for the automatic measurement of tool compensation.

3.11.3.4 Tool skip signal

It is possible to forcibly change a tool even it has not reached its service life.

(I) Set the group where the tool is and input tool skip signal. Use the next T code instruction to select the next tool in the group.

(II) Input tool skip signal without specifying a group number but assuming the selected tool is specified. Follow (i) for other issues.

Following (I) or (II) shall be set by parameter. Service life starts from 0 no matter which method is followed. However, output a tool change signal when the tool skip signal inputs the last tool.

(Note) When STL or SPL or both of them are lit, it indicates that what is input is neither tool

change signal nor tool skip signal.

3.11.4 The display and input of tool data

3.11.4.1 The display and modification of tool group number

In the part program storage and edition area, tool group data may be displayed and modified like the edition of common programs. As described in Section 11.1, modified program shall be executed; otherwise it cannot be saved in the tool life data area.

3.11.4.2 The display of tool life data during the execution of machine program

Pressing the DIAGNOSIS button twice in any mode displays the first page of tool life data in the following format on the screen of LCD.


202

Group No. Service life

T 0 0L L I F F DA TA 01 : 0 0 0 0 1 N 0 0 1 2

SELECTED GRP 0 0 1

GRP 0 0 1 : LIFE 9800 COUNT 6501 Life counter

* 0 0 3 4 * 0 0 7 8 * 0 0 1 2 * 0 0 5 6

* 0 0 9 0 @0 0 7 6 0 0 3 2 0 0 9 8 The tools in Group 1

0 0 5 4 0 0 1 0 0 0 9 9 0 0 8 7

0 0 7 7 0 0 6 6 0 0 5 5 0 0 2 4 (a): The tool in service

GRP 0 0 2: LIFE 0 5 0 0 COUNT 0112 #: The skipped tool

* 0 0 1 1 *0 0 2 2 *0 2 0 1 *0 1 4 4

* 0 1 5 5 *0 0 6 6 *0 1 7 6 *0 1 8 8

# 0 0 1 9 0 2 3 4 0 0 0 7 0 1 1 2

0 1 5 6 0 0 9 0 0 0 1 6 0 2 3 2

GRP T O BE CHANGED :

0 0 3 0 0 6 0 1 2 0 1 3 0 1 4

N LSK INC

Two groups of data are displayed on each page. Pressing the page turning button ↓ displays all data groups in sequence. Tool change signal may be given to up to 5 groups, which are displayed at the bottom of each page. For 6 or more groups, an arrow will be indicated in the diagram. To review the data, select address N, enter the group number and press the INPUT button, or pressure press the CURSOR ↓ button to move the cursor to the GRP of the next group and to display its data.

3.11.4.3 Presetting tool life counter

To modify the tool life counter, select the MDI mode.

(I) P□□□□ and press the INPUT button.

Now the group counter that is identified by the cursor is preset □□□□ while other data in the group remains unchanged.

(II) Type in P－9999 and press the INPUT button.

All the executed data in the group identified by the cursor including * are cleared. It

*: The tool whose life has come to an end

The tool number in Group 2

The tool group number to be changed


203

functions as the reset of the tools in the group (see Section 3.11.3.2).

3.11.5 Other cautions

Part program storage and edition area will reduce the storage area in the last part for the purpose of tool life data area. When data is saved in the part program and edition area in EDIT mode as described in Section 11.1, more area will be occupied.

3.12 The Indexing Function of Indexing Worktable

The 4th axis (e.g. Axis B) may be used for the indexing of indexing work. Indexing instruction only employees the angle specified by Address B. The process becomes simple as it is unnecessary to set the M codes for worktable tensioning and releasing.

3.12.1 Instructing methods

3.12.1.1 Input unit

Decimal point, B 1…1° shall not be used.

Note: When a decimal is used, PS alarm will be given one the digits after it are instructed. (N O 180) means that the value less than 1° cannot be instructed.

3.12.1.2 Absolute / incremental instruction

Absolute / incremental instruction can be instructed by G90/G91.

Absolute instruction G90 B45; Indexing of 45° position

Incremental instruction G 91 B－45; Indexing of negative rotation 45°

The point A in the above figure is the actual position. The mentioned instruction moves as shown in the above figure.


204

3.12.1.3 Concurrently controlled axes

Axis B shall be individually specified. PS alarm will be given when X, Y, Z or the 5th axis is instructed along with Axis B (NO181).

3.12.2 Minimum travel unit: 0.001 degree/pulse

3.12.3 Feedrate

As a rule, the feedrate of axis B is a rapid one regardless the state of Group 01 G codes (G 00, G01, G02 and G03). When Axis B is instructed in G 00, G01, G02 or G03 mode, the G 00, G01, G02 and G03 in the blocks regarding other axes are still valid, and hence it is not necessary to specify G 00, G01, G02 and G03 again.

G01 X10 F5; Axis X operates at cutting feedrate.

B45 ; Axis B operates at cutting feedrate.

X29 ; Axis X operates at cutting feedrate.

(G01 is still valid.)

No-load operation is invalid.

3.12.4 The clamping and release of indexing worktable

The clamping and release of indexing worktable is automatically performed before and after the movement of Axis B.

(1) Indexing sequence A


205

(2) Indexing sequence B

Positioning check is always performed at the Point A when the above indexing sequence A/B is selected by parameter setting.

Note 1: Clamping or releasing signals are cleared when the NC is reset in the waiting state after clamping or release. NC unit then completes the waiting state and enters into reset state.

Note 2: In clamping or releasing mode, these states remain unchanged even the unit is reset, namely the sequence of release or clamping cannot be automatically executed through reset, but clamping are releasing signals are cleared.

Note 3: The waiting state after clamping or releasing is displayed in diagnosis mode display state (DGN701-BCNT).

3.12.5 Jog/step/handwheel

Operations in Jog/step/handwheel mode cannot be performed for Axis B. However it may return to the reference point in Jog mode. Travel stops once the axis selection signal becomes “0” when manually returning to the reference point. Clamping instruction is not performed. In order to avoid the problem, set the sequence program on the machine side so that the axis selection signal will not become “0” before returning to the reference point.

3.12.6 Other cautions

(1) The indication of the actual position on the screen of LCD, indication of external position and the indication on the screen of COMND have a decimal point.

Example: B180.000

(2) Whether the internal absolute coordinates of NC for Axis B use 360° full circle is set by parameter (314－IRND).

(i) when IRND＝0, absolute coordinate is rounded to 360° and starts from 0° position. If G90 B720; is specified, Axis B rotates by 720° (2 turns) and the actual position


206

indication and absolute coordinate is 720°.

(ii) When IRND＝1, absolute coordinate and the actual position are rounded to 360°. However the rounding of absolute coordinates is performed after the travel for increment determination. That is, if G90 B720; is specified from 0° position, Axis B will rotate by 720° (2 turns) and absolute coordinate will be 0°. Now the actual position changes as follows:

0° 90° 180° 270° 0° 90° 180° 270° 0°.

The result of 360° rounding, absolute coordinates and actual position are displayed between 0° and 359°.

For the RELATIVE in the display of the actual position (ABSOLUTE RELATIVE), rounding is only performed when parameter No. 007 PPD＝1.

No matter it is in the condition of (i) or (ii), the mechanical coordinate system often uses 360° for rounding. When automatic return to the reference point is specified, (G28) calculates the amount of movement with the mechanical coordinate system. The movement between the intermediate point and reference point is less than 360° (on turn).

(3) The following requirements are made through parameter setting (314－IM15):

When IM15＝1:

(i) Axis-B instruction shall be always considered as absolute instruction regardless the G90 or G91 mode.

(ii) The rotating direction is positive.

(iii) When M15 is pacified in the same block as the Axis-B instruction, the rotating direction is negative.

(Note) Though M15 is processed inside the NC, FIN signal returns to the NC because MF and M codes are sent to the machine side.

(4) During the movement of Axis B, Feedrate, reset and emergent stop are valid. Proper workpiece shall be done on the machine side in order to prevent stop in midway.

(5) When the option is adopted, the additional axis servo ON signal (*8VF4) will become invalid.


207

(6) Standard additional axis still applies to the requirements, parameters and inter-unit connection that are not described in the instruction manual.

Add: No.52, 1st . Street, Luochong North Road, Luochongwei, Guangzhou, 510165, China

Website: http://www.gsk.com.cn E-mail: [email protected] Tel: 86-20-81796410/81797922 Fax: 86-20-81993683

All specification and designs are subject to change without notice. Aug. 2007/Edition 4

Aug. 2007/Printing 4

Kenh

新建图章

GSK983M Milling CNC System

User Manual (Volume II: Operations)

Kenh

新建图章

3

Foreword Dear user,

We are really grateful for your patronage and purchase of GSK983M milling CNC system made by

GSK CNC Equipment Co., Ltd.

This manual consists of two volumes. Volume I mainly describes the specifications

and programming of the system while Volume II operations, all codes, parameters,

I/O interfaces and other appendices.

！ This system can only be operated by authorized and qualified personnel as

improper operations may cause accidents. Please carefully read this user

manual before usage. All specifications and designs herein are subject to change without further notice.

We are full of heartfelt gratitude to you for supporting us in the use of GSK’s

products.

Kenh

cover

Kenh

xiaoxiaoxiao

Kenh

小空白

Kenh

xiaoxiaoxiao

Kenh

小小空白

GSK983M Milling CNC System Operation Manual (Volume II: Operations)

III

CONTENTS

4. OPERATIONS......................................................................................................................................1

4.1 Power On/off .................................................................................................................................1 4.1.1 Power on ..................................................................................................................................1 4.1.2 Power off ..................................................................................................................................1

4.2 Key Switch.....................................................................................................................................1

4.3 Operations Involving with the Operation Panel .........................................................................1 4.3.1 Operation panel........................................................................................................................1 4.3.2 Emergency stop (red)...............................................................................................................2 4.3.3 Selection mode.........................................................................................................................3 4.3.4 Operations involving with manual operation.............................................................................3

4.3.4.1 Jog feed.............................................................................................................................3 4.3.4.2 MPG feed...........................................................................................................................4 4.3.4.3 Manual absolute ................................................................................................................5

4.3.5 Manually returning to reference point (reference position) .......................................................9 4.3.6 Operations on automatic running ...........................................................................................10

4.3.6.1 Start of automatic operation .............................................................................................10 4.3.6.2 Suspension of automatic operation..................................................................................10 4.3.6.3 Single block .....................................................................................................................10 4.3.6.4 Restart after feed hold or stop .........................................................................................11 4.3.6.5 The manual operations in automatic run..........................................................................11 4.3.6.6 The MDI operations in automatic run...............................................................................11 4.3.6.7 Skipping over optional blocks ..........................................................................................12 4.3.6.8 Feedrate override ............................................................................................................12 4.3.6.9 Dry run.............................................................................................................................12 4.3.6.10 Machine lock..................................................................................................................12 4.3.6.11 Display lock....................................................................................................................12 4.3.6.12 Mirror image...................................................................................................................12 4.3.6.13 Rapid traverse override .................................................................................................13 4.3.6.14 External workpiece number search function ..................................................................13

4.3.7 JOG feed at any angle ...........................................................................................................14 4.3.8 Manual insertion .....................................................................................................................15

4.3.8.1 Inserting operations by MPG(manual pulse generator/handwheel) .................................15 4.3.8.2 Manual inserting movement by MPG...............................................................................16

4.4 The Display and Operations of the MDI/LCD Panel with LCD Characters .............................17 4.4.1 Status display .........................................................................................................................18 4.4.2 Key input ................................................................................................................................18 4.4.3 Display of program numbers and sequence numbers ............................................................19 4.4.4 Alarm display (function button ALARM)..................................................................................20 4.4.5 Operator information ..............................................................................................................21 4.4.6 Display of actual position and reset (function key POSITION) ...............................................21 4.4.7 Indication of instruction value (function button COMMAND) ..................................................22 4.4.8 Setting (function button SETTING) ........................................................................................24

4.4.8.1 Display and setting of input, output, etc ...........................................................................24 4.4.8.2 Display and setting of user macro variables ....................................................................26

4.4.9 Operating through MDI (function key COMMAND) ................................................................27 4.4.10 Start of MDI motion...............................................................................................................28 4.4.11 Reset ....................................................................................................................................28 4.4.12 Tool position offset................................................................................................................29 4.4.13 Setting and display of workpiece origin offset (Optional) ......................................................30 4.4.14 Measurement of tool length..................................................................................................31 4.4.15 Program display (function button PROGRAM).....................................................................31 4.4.16 Program number search (function key PROGRAM) ............................................................33 4.4.17 Inputting a program with keys...............................................................................................33


IV

4.4.18 Deletion of a program...........................................................................................................35 4.4.19 Deletion of all programs .......................................................................................................35 4.4.20 Sequence number search ....................................................................................................35 4.4.21 Restart of a program ............................................................................................................36 4.4.22 Program number comparison stop function..........................................................................39 4.4.23 Display of parameters (function button: PARAMETER) .......................................................40 4.4.24 Program edit.........................................................................................................................40

4.4.24.1 Word scanning...............................................................................................................41 4.4.24.2 Word search ..................................................................................................................42 4.4.24.3 Address search ..............................................................................................................42 4.4.24.4 Methods for returning to the beginning of a program .....................................................42 4.4.24.5 Word insertion (active when the program protection lock is disabled) ...........................43 4.4.24.6 Word modification (active when the program protection lock is disabled)......................44 4.4.24.7 Insertion and modification of several words, blocks and strings ....................................44 4.4.24.8 Word deletion (active when the program protection lock is disabled) ............................45 4.4.24.9 The deletion of the part before EOB ..............................................................................45 4.4.24.10 Deletion of blocks (active as program protection lock is disabled)...............................45 4.4.24.11 Storage sorting.............................................................................................................46 4.4.24.12 The indication of all stored program numbers..............................................................46 4.4.24.13 Edit of user macro (active as the program protection lock is disabled) ........................46

4.4.25 Indication of run time ............................................................................................................48 4.4.26 Menu switching function .......................................................................................................48 4.4.27 Operations of LCD soft function keys ...................................................................................50

4.4.27.1 General ..........................................................................................................................50 4.4.27.2 Display...........................................................................................................................50 4.4.27.3 Direct entry of measured workpiece origin offset ...........................................................57

4.5 Position Indication through Position Display Unit (Available upon Customer’s Request) ..58 Appendix 1 Codes for Programming ........................................................................................59 Appendix 2 G Codes List ...........................................................................................................62 Appendix 3 Ranges of Instruction Values ................................................................................64 Appendix 4 Calculating Chart....................................................................................................65 Appendix 5 Parameters..............................................................................................................69 Appendix 6 Alarms List ............................................................................................................108 Appendix 7 List of the States during Switching On, Reset and Clearance..........................117 Appendix 8 Memory Type Pitch Error Compensation ...........................................................119 Appendix 9 Operations List .....................................................................................................125 Appendix 10 Lock of Program Key .........................................................................................127 Appendix 11 The Interrupt Function of User Macro...............................................................129


1

4. OPERATIONS

4.1 Power On/off

4.1.1 Power on

1) Make sure all parts of the machine are properly wired and secured.

2) Switch on the machine by following its manual.

3) Pictures appear on the LCD several seconds after switching on the machine.

4.1.2 Power off

1) The indicator of the cycle start button on the operation panel of the machine goes out.

2) All moving parts of the machine stop.

3) Make sure the above operations are performed well and then press down and hold the POWER OFF button for 1 or 2 seconds.

4) Disconnect the power supply of the machine by following its manual.

Note: Never use the keys on the MDI keypad to power on/off the machine.

4.2 Key Switch

A key switch for program protection may be set with the operation panel of the machine. The key switch offers two modes of protection:

1) Relevant operations cannot be performed unless the key switch is actuated. However, the concerned data is still displayed on the LCD.

2) Operations can or cannot be performed without actuating the key switch. It is possible to switch between the two modes by parameter.

The Section 4.4 herein will describe in detail which functions are under the protection of 1) or 2) mode.

4.3 Operations Involving with the Operation Panel

4.3.1 Operation panel

The functions of the operation panel and the layout of switches on it vary depending on different machine types. The following is a typical operation panel. Refer to the relevant parts of the manual supplied with the machine for details. This chapter only describes the operation panel of 3-axis control system (The operation panels of 4-axis and 5-axis control systems are primarily similar to that of a 3-axis control system).


2

进给倍率 % 主轴倍率 %

电源关电源开

急停

Z 4

X Y

4.3.2 Emergency stop (red)

In an emergency, press the EMERGENCY STOP button to stop the movements of all the axes of

the machine. At the same time, the button is locked in the stop position.

The release mode of the button varies with different manufacturers. In general, it is released by

pushing down and clockwise turning the button.

Note 1: The power supply of the motor is switched off when the button is pressed.

Note 2: The control unit is in reset state.

Note 3: Make sure to eliminate all troubles before releasing the button.

Note 4: Return to the reference point by through manual operations or G28 instruction.


3

4.3.3 Selection mode

Modes Functions EDIT Perform the following operations:

(1) Saving programs in storage; (2) Modifying, inserting and deleting programs; (3) Outputting the programs in storage and editing other programs

AUTO (MEMORY)

(1) Executing the programs saved in storage; (2) Search the sequence numbers of the programs in storage

MDI (1) Manual data entry may be performed through MDI and the operation panel of the machine.

JOG (1) It is possible to perform Jog feed. MPG(HANDLE) (1) It is possible to perform manual feed.

MACHINE ZERO (HOME)

Return to the machine zero.

4.3.4 Operations involving with manual operation

Except the automatic operations that can be performed with programs, it is possible to conduct the following manual operations with switches.

4.3.4.1 Jog feed

Jog feed enables the machine to move.

1) Set the selection mode switch to JOG position.

2) Select a motion axis so that the machine travels in the selected direction.

Note 1 2 axes may be concurrently controlled by manual operation.

Note 2 After power on, the selected axis of the machine will not immediately move even the SELECTION MODE switch is set to JOG position. Now it is necessary to reselect an axis.

3) Selecting Jog feedrate

Feedrate Lead screw for feed in metric system Lead screw for feed in Inch system

Position of switch

mm/min inch/min inch/min mm/min 0 0 0 0 0 1 1.0 0.04 0.02 0.508 2 1.4 0.055 0.208 0.711 3 2.0 0.079 0.04 1.02 4 2.7 0.106 0.054 1.37 5 3.7 0.146 0.074 1.88 6 5.2 0.205 0.104 2.64 7 7.2 0.283 0.144 3.66 8 10 0.394 0.2 5.08 9 14 0.551 0.28 7.11 10 20 0.787 0.40 10.2 11 27 1.06 0.54 13.7


4

12 37 1.46 0.74 18.8 13 52 2.05 1.04 26.4 14 72 2.83 1.44 36.6 15 100 3.94 2.00 50.8 16 140 5.51 2.80 71.1 17 200 7.87 4.00 102 18 270 10.6 5.40 137 19 370 14.6 7.40 188 20 520 20.5 10.40 264 21 720 28.3 14.40 366 22 1000 39.4 20.00 508 23 1400 55.1 28.00 711 24 2000 78.7 40.00 1016

Note 1: The numerical values listed in the above table vary with different machines.

Note 2: The allowable deviation of the feedrates listed in the above table is approximately ±3%.

4) Rapid traverse

An axis rapidly traverses in the selected direction when the button is pressed.

Note 1: The feedrate, time constant and acceleration/deceleration mode for manual rapid traverse are the same as the rapid traverse under G00 program instruction.

Note 2: When the machine has a memory type travel limit selecting function, it shall be provided with an axis with the function of returning to the reference point. When the RAPID button is pressed after power on or emergency stop, its feedrate will not change into rapid feed but maintain at Jog feedrate provided that the function of returning to the reference point is not executed.

This is because memory type travel limit dose not function before the manual return to the reference point, thereby preventing the machine from quickly reaching the end of run.

4.3.4.2 MPG feed

Make accurate adjustment for the feed of the machine with a manual impulse generator as follows.

(1) Set the SELECTION MODE switch to MPG position.

(2) Select a motion axis.

(3) Turn the handwheel of manual impulse generator.

Clockwise…………………..+ direction

Counterclockwise……… - direction

(The rotating direction depends on the settings of manufacturers)

(4) Amount of travel: Some of the operation panels are provided with the following selector switches: ×10 means multiplying amount of travel by 10 while ×100 by 100.

The amount of travel each step Input system ×1 ×10 ×100

Input in metric system 0.001mm 0.01mm 0.1mm Input in inch system 0.0001inch 0.001inch 0.01inch

Note 1: If the handwheel rotates at a speed over 5 turns per second, the amount of the rotation of the


5

handwheel will differ from the travel distance of the machine. Hence do not rotate the handwheel

too quickly.

Note 2: When ×100 override is selected and the handwheel is turned at quick speed or the workbench

moves at “rapid traverse” rate, the machine will be subject to impact if it is stopped abruptly. The

selection automatic acceleration/deceleration function is also valid for manual feed, thereby

reducing mechanical shock.

4.3.4.3 Manual absolute

If the switch is set to ON, the manual-operated travel amount will be added to the coordinate axes.

(1) MANUAL ABSOLUTE switch ON: Coordinates change with manual operation.

(2) MANUAL ABSOLUTE switch OFF: Coordinates do not change.

(Example) For example, in the following blocks:

…

G01 G90 X100.0 Y100.0 F010；①

X200.0 Y150.0 ；②

X300.0 Y200.0 ；③

…

a) The above block has been executed while block is only executed after manual ① ②

operation (travel by 20.0 in X direction and 100.0 in Y direction).


6

b) Press the FEED HOLD button in the execution of the block . After manual operation ②(Y+75.0), press the CYCLE START button so as to cancel the hold mode and continue the execution.

c) Press the FEED HOLD button in the execution of the block . Reset the machine after ②manual operation (Y+75.0). The block restarts inputting. ②

d) When manual operation is followed by a single-axis instruction, then only the instructed axis

returns to the programmed absolute position of the axis.

N1 G01 G90 X100.0 Y100.0 F5000； N2 X200.0； N3 Y160.0；

e) When manual operation is followed by an incremental instruction, then the position that the


7

axis moves to is identical with that is instructed while the MANUAL ABSOLUTE switch is set to OFF.

Note 1: Insert manual operations when tool radius compensation C offsets. Now the actual motion path

of the tool is as follows:

(1) MANUAL ABSOLUTE switch OFF

When tool radius compensation C is enabled：If MANUAL ABSOLUTE switch is switched off for

manual operation when tool radius compensation C is enabled, the path of the automatic tool

motion will translate in parallel by the offset of the inserted manual operation.

(2) MANUAL ABSOLUTE switch ON

When tool radius compensation C is enabled：If MANUAL ABSOLUTE switch is switched on for

manual operation when tool radius compensation C is enabled, the path of the tool under

absolute instruction after restart is as follows. The tool path for the blocks after manual operation

runs parallel to the vectors of the origin of the next block.

Tool path is determined by the vectors between the next block and the block that follow. For the angle

machining with the intervention of manual operation, its tool path is identical with the above.

If a program consists of incremental instructions rather than absolute instructions, its tool path is

identical with that when the MANUAL ABSOLUTE switch is set to OFF.

(a) Performing manual operations during execution of a block

Example 1: In the following programmed path (PA→PB→PC→PD), assuming the point PH

between PA and PB is moved to point PH′ by manual operation after pressing the FEED

HOLD button, the end point PB of the current block translates to point PB’ due to the offset

as a result of manual operation and the vectors VB1 and VB2 of the original point PB also

translate to V’B1 and V’B2.


8

The vectors between the next block (tool path from PB to PC) and the one that follows (from

PC to PD) do not need compensation. The new vectors (VC1′, VC2′) with compensation

results from the relationship between the two blocks (programmed paths from PB′ and PC to

PD and from PC to PD). Since vector VB2′ coincides with VB2, however, the section of path

between PB’ and PC as a result of tool offset is not accurately performed. But for the block

after point PC, tool offset can be precisely performed.

Example 2: If manual operation is inserted in angle machining in the case of tool radius

compensation, the feed path after manual operation will be determined by the same method

as Example 1. That is, the vectors VA2′, VB1′ and VB2′ in the figure below are determined by

translating the vectors VA2, VB1 and VB2 by an amount of manual travel and the new

vectors result from VC1′ and VC2′. The block after point PC will be precisely performed by the

tool offset compensation C.


9

(b) If manual operation is inserted after the execution of single block function, the vectors VB1 and VB2 for the end points of the current block will be moved in parallel and the method for determining the following feed path will be identical with (a). MDI operation may be inserted after the execution of a block with single block function. The feed path after MDI operation coincides with tat after the insertion of a manual operation.

4.3.5 Manually returning to reference point (reference position)

The machine may return to the reference point by manual operations:

1) Set the SELECTION MODE to JOG.

2) Press the MACHINE ZERO key.

3) Move all axes toward the reference point by Jog feed.

The machine rapidly traverses to the deceleration point and then to the reference point at FL


10

speed. Rapid traverse override is still active during traversing.

4) The machine stops at the reference point and the indicator indicating the end of the return to the reference point is lit.

Note 1: The indicator is lit after the return to the reference point. If the switch for returning to the reference point is set to ON position, the machine cannot translate in Jog mode.

Note 2: The following procedures may extinguish the indicator: (1) Move the machine away from the reference point; (2) Press the EMERGENCY STOP button.

Note 3: For the distance to the reference point, refer to the manual supplied by the manufacturer of the machine.

4.3.6 Operations on automatic running

The machine may automatically run by programs.

4.3.6.1 Start of automatic operation

Procedures for starting the program stored in memory:

(a) Select the program number. See Section 4.4.16 “Program number search”.

(b) Select AUTO mode.

(c) Press the CYCLE START button. Automatic operation starts once the CYCLE START button is pressed and at the same time the CYCLE START indicator is lit.

Note 1: The programs read in are loaded when the CYCLE START button is pressed in EDIT mode. The loading mode is the same as that when the INPUT button is pressed for parameter setting.

Note 2: The CYCLE START button is inactive in the following conditions：

(a) When the FEED HOLD button is pressed;

(b) When the EMERGENCY STOP button is pressed;

(c) When the RESET signal is enabled (contact the manufacturer of the machine for details);

(d) When the SELECTION MODE switch is set to a wrong position (other than AUTO or EDIT mode);

(e) When it is search a sequence number;

(f) When an alarm is given;

(g) When automatic operation is selected;

(h) When the NC system is not ready

4.3.6.2 Suspension of automatic operation

Press the FEED HOLD button The FEED HOLD indicator illuminates and the CYCLE START indicator goes out when the FEED HOLD button is pressed. And now, (a) If the machine is moving, the feed slows down and stops; (b) If the machine is in hold state, the hold state will interrupt even in FEED HOLD mode; (c) The machine stops after the performance of M, S, T or B function.

4.3.6.3 Single block

If the SINGLE switch is turned to ON position, the control only executes a block each time and


11

stops when the CYCLE START button is pressed. The control only executes a block each time and stops when the SINGLE switch is turned on. When the CYCLE START button is pressed, the control stops after the execution of the next block.

Note 1: In G28, G29 or G30 mode, the tool stops at the intermediate point if the SINGLE function is used. Note 2: For fixed circular processing, the tool stops at the end point of the circular path ①, or of the ② ⑥

fixed cycle (see the figure below) if the SINGLE function is active.

When the result of the fixed circular calculation is not 1, the FEED HOLD indicator illuminates except the block of the final cycle. The FEED HOLD indicator illuminates whenever block ⑥ ①or stops.②

Note 3: For the blocks of M98P—, M99 and G65, G66 or G67, the stop of the single block is invalid. However, it is valid if the instructions in M98 or M99 block are of the addresses other than O, N, L and P.

4.3.6.4 Restart after feed hold or stop

(1) Select the AUTO mode;

(2) Press the CYCLE START button. The FEED HOLD indicator goes out when the CYCLE START button is pressed.

4.3.6.5 The manual operations in automatic run

(1) In automatic run, suspend the operation by pressing the FEED HOLD button on the operation panel or bring the SINGLE switch to ON position.

(2) Record the coordinates of the stop position displayed by the location display unit.

(3) Perform JOG operation (see Section 4.3.4.3).

(4) Return the tool to the recorded coordinates (the origin of JOG operation).

(5) Set the SELECTION MODE switch to the position before JOG operation so as to restart automatic run.

(6) Press the CYCLE START button.

4.3.6.6 The MDI operations in automatic run

(1) Set the SINGLE switch to ON position.

(2) Select MDI operation mode.

(3) Perform MDI operation.

(4) To restart automatic operation, return to the original operation mode and press the CYCLE START button on the operation panel.

Note 1: The modal data reserved in cycle movement is under influence when MDI instruction is used.

Note 2: The modal data instructed by MDI is still valid for automatic MDI operation.


12

Note 3: Too radius compensation C is not performed during MDI operation.

Note 4: MDI operation is disabled in feed hold state.

4.3.6.7 Skipping over optional blocks

When some block contains “/n”(n=1 to 9), the function allows the control to skip over the block. Switches correspond to the 19 numbers respectively.

Note: While blocks are being read in the buffer from storage, the validity of function of skipping over optional blocks is judged. Therefore the function is invalid for the blocks read in buffer register.

4.3.6.8 Feedrate override

For the feedrate set by F function, it is possible to set an override in the range of 10% to 200%. An override of 10% increment is recommended.

4.3.6.9 Dry run

If the switch is set to ON position in the cycle operation instructed by storage or MDI, the F function does not work and the machine travels at the following speeds.

RAPID button ON/OFF In rapid traverse In cutting feed RAPID button ON Rapid traverse Maximum Jog feedrate RAPID button OFF Jog feedrate (see Note) Jog feedrate

Note: The dry run of rapid traverse may be disabled or enabled by parameter setting.

4.3.6.10 Machine lock

When the MACHINE LOCK switch is set to ON, the movement instruction pulse is inhibited. Therefore the position indication for circular feed start or JOG operation is continuously updated according to input instructions. But the machine does not move itself. The function is used to check procedures.

Note 1: When G27, G28 or G30 instruction is set, the machine will not return to the reference point. Hence the indicator for returning to the reference point is not lit.

Note 2: M, S, T and B functions are performed.

4.3.6.11 Display lock

When the DISPLAY LOCK switch is activated, the coordinates indicated by the location display unit are locked. For instance, when the coordinate system is moved as a result of JOG operation, the use of this switch prevents the indicated values from changing by manual movement.

Note: The function is optional.

4.3.6.12 Mirror image

Once the mirror image switches of axes X and Y as well as the 4th axis are activated in automatic operation, the axes move reversely. The reference point is returned to by JOG or automatic operation, the movement between the intermediate point and the reference point does not inverse and position display depends on the actual movement of the tool. This may be achieved by setting parameters with MDI unit (see Section 4.4.7).


13

4.3.6.13 Rapid traverse override

It is possible to set the rapid traverse override switch of optional overrides 100%, 50%, 20% and F0 on the operation panel of the machine.

When the feed speed is 10m/min and the switch is set to 50% position, the actual feed speed will be 5m/min.

F0 is a fixed speed (feedrate) provided by the manufacturer of the machine. The function applies to the following conditions:

(1) The rapid traverse specified by G00;

(2) The rapid traverse in fixed cycles;

(3) The rapid traverse in G27, G28, G29 and G30 modes;

(4) JOG rapid traverse;

(5) The rapid traverse for manually returning to the reference point.

4.3.6.14 External workpiece number search function

Select a workpiece number to be processed with the switch on the operation panel of the machine (No example of the operation panel is given in this user manual). (Machining programs are pre-stored in the part program storage.) Press the START button. Now the system automatically executes the program corresponding to the workpiece number. By using the function, operator does not need to search the stored program numbers so as to reduce dry run time and errors.

(1) Preparation for the program: In the situations using the function, the numbers assigned to programs shall correspond to the workpieces to be processed. That is, a number among 01 to 31 shall be designated for each workpiece to be processed. The relevant program number is expressed as follows:

0(:) 0 0 □ □ (0 for EIA and : for ISO)

Workpiece number (01 to 31) Optional workpiece number

They are stored in the part program memory. As shown in the following examples, each program shall be started by the address 0 followed by a program number and ended by M02, M30 or M99.

In addition, the storage of the programs irrespective of workpiece number is allowable.

0 0001； N 0001 G00…； The program corresponding to workpiece No. 01 …………………… …………………… N 120 M02； 0 0002； N 0001 G00…； The program corresponding to workpiece No. 02 …………………… …………………… N 300 M30； 0 0004； N 001 G00……… ………………………

The program corresponding to workpiece No. 04 ………………………


14

N 080 M02； 0 6247； N 001 G00……… ……………………… Programs irrespective of workpiece number ……………………… N 034 M99；

Note 1: Each program shall be started by the address 0 followed by a program number and ended by M02, M30 or M99. However, M02, M30 and M99 cannot be specified in the middle of the program. If one of them is specified in the middle section, the program that follows will regarded as another program segment (the block following M02, M30 or M99 is immediately numbered as a program when the program is stored in memory).

Note 2: The allowable quantity of workpiece numbers depends on factory setting (see the manual of the machine).

Note 3: For the machine system provided with external workpiece number search function A, the allowable maximum workpiece number is 31. Now the first two digits of the program number corresponding to a workpiece number must be 00.

(1) Operating procedures

Operating procedures vary with different manufacturers of machine. The operating procedures described below are general. Refer to the manual supplied by manufacturer of the machine for specific operating procedures.

Note 1: Select the automatic mode and then set the program (01 to 31) corresponding to the workpiece number with the rotary switch on the operation panel on the machine side. When the START button is pressed, the program corresponding to the set workpiece number will be searched out and machining performed with the start of the program.

Note 2: When a workpiece number is set to 00, the corresponding program will not be searched if the START button is pressed. The execution starts from executable section of the current program. For the situations that starts in the midway of the program or that the executing program is independent of workpiece number, it is necessary to set the workpiece number to 00 and press the START button after sequence number search or program number search.

Note 3: The function does not apply to MDI operation but automatic operation.

Note 4: If a program number corresponding to the workpiece number is not stored in the memory, an alarm (No. 59) will be given once the START button is pressed.

Note 5: It is not always necessary to select the relevant program even a workpiece number is selected with the dial. Refer to the manual supplied with the machine for the procedures for selecting a program. When workpiece number search function A is selected, program search is performed after the NC system starts automatic operation in reset mode.

4.3.7 JOG feed at any angle

Set an angle and feedrate in the plane of X and Y and then press the START button. In this way the machine may feed at any set angle by JOG operation.

(1) Set the SELECTION MODE switch to the mode of JOG feed at any angle

(2) Set an angle with the angle setting dial. The position of an angle is selected among 0-71 with a 2-digit BCD code. 0 ~71 correspond to 0 ~360° respectively (in 5° increment).


15

For angle setting, make sure to switch on angle strobe pulse. If angle strobe pulse is switched on, the formerly set angle will remain valid.

As shown in the above figure, the + direction of Axis X is 0° and that of Axis Y is 90°.

(3) Select a feedrate (speed in tangential direction) with the Jog feed dial.

(4) Press the START button in the mode of JOG feed at any angle. Then the machine moves at the selected feedrate in the set direction.

If the JOG RAPID button is pressed, the machine will feed at the maximum Jog feedrate. The machine feeds when the JOG RAPID TRAVERSE button is switched off and stops feed when it is switched off.

Note 1: If axes X and Y are interlocked, both axes will slow down and stop. They will restart once the interlocking is disabled.

Note 2: In automatic operation, it is possible to insert JOG feed at any angle when the machine is stop in feed hold mode.

Note 3: For the situation with external deceleration selection, JOG feed at any angle is also active. Now the tangential feed is equal to the external decelerating rate.

Note 4: The automatic acceleration and deceleration for cutting feed also apply to the JOG feed at any angle.

Note 5: JOG feedrate at any angle does not change with Jog feedrate even during the switching between metric and inch systems.

4.3.8 Manual insertion

For the specific axis (fixed by parameter) in automatic operation, the movements operated with handwheel may be performed in addition to the self-motion of the axis.

4.3.8.1 Inserting operations by MPG(manual pulse generator/handwheel)

Manual insertion is possible by turning the manual pulse generator in the following conditions. (1) Mode: automatic mode or MDI mode (2) Operating state: Manual insertion is possible during linear interpolation, arc interpolation, spiral

interpolation or sine-curve interpolation. However, the following conditions are excluded: (I) When an alarm is given; (II) When any axis does not move; (III) When positioning is valid; (IV) When interlocking is active; (V) In the absence of travel instruction.


16

(3) Manual axis selection signal Manual axis selection signals (HX, HY, HZ, H4 and H5) are switched on (contacts close) for the axes to perform manual insertion.

4.3.8.2 Manual inserting movement by MPG

(1) Amount of travel: The amount of travel to be inserted by manual shall be identical with that during JOG feed. The amount of travel depends on the scale of the manual pulse generator and JOG feed overrides (X1, X10 and X100) and is added to that of automatic operation.

(2) Traverse speed: The axial speed for JOG insertion is the result of the addition of the travel speed of automatic operation to that inserted by manual. Therefore, axial speed is limited to rapid traverse speed (Parameter HR) in the event that axial speed exceeds rapid traverse speed. Displacement mismatches the indicated value of the manual pulse generator.

(3) The correspondence between manual-inserted travel and all signals is as follows:

Signal Travel Machine is locked Affected: The tool does not move when MACHINE LOCK is enabled.

Display is locked. Affected: Relative coordinates remain unchanged when display is locked.

Mirror image of Axis X

Not affected: The machine moves forward when the handwheel is turned clockwise.

(4) The correspondence between manual-inserted travel and position indications is as follows:

Indication Travel Absolute coordinates Not affected: Manual-inserted pulse is not added to absolute coordinates

Relative coordinates Affected: Manual-inserted pulse is added to relative coordinates

Mechanical coordinates Affected: Manual-inserted pulse is not added to mechanical coordinates

(5) Indication of amount of travel: Manual-inserted amount of travel may be displayed in diagnosis

message (Diagnosis No. 805 to 809). To display a diagnosis message, press the function key DIAGNOSIS on the MDI panel.

Diagnosis data numbering

8 0 5 Manual-inserted amount of travel of Axis X

8 0 6 Manual-inserted amount of travel of Axis Y

8 0 7 Manual-inserted amount of travel of Axis Z

8 0 8 Manual-inserted amount of travel of the 4th axis

8 0 9 Manual-inserted amount of travel of the 5th axis

Unit: 0.001mm (input in metric system)

0.0001 inch (input in inch system)

Note: Only the removable amounts of travel are cleared.


17

4.4 The Display and Operations of the MDI/LCD Panel with LCD Characters

The MDI/LCD panel is usually mounted on the upper front side of the control cabinet. It consists of an LCD and buttons as follows.

Function buttons: The large number of items displayed with the function buttons is just like the chapters of a book. When a function button is pressed for the second time and third time, the chapter 2 or 3 of the corresponding display functions (if the function button for the chapter is provided). Each chapter includes several pages and each page is selected with the page button.

5TH

4TH

The names and meanings of all function buttons are listed below.

POSITION Pressing once Display of actual position and reset

Pressing once Display and setting of set data Pressing twice Display and setting of user macro variables SETTING Pressing for the third time Display and setting JOG switch

Pressing once

Display of the information regarding a program in EDIT mode Display of the executing or executed blocks and the blocks that follow in a mode other than EDIT PROGRAM

Pressing twice Display of the list of program numbers (See Section 4.4.24.12) (The chapter 2 may also be omitted depending on the conditions of the system.)

Pressing once Display and setting of parameters PARAMETER Pressing twice Display and setting of PC parameters Pressing once Display and setting of offset

OFFSET Pressing twice Display and setting of origin offset in a workpiece coordinate system

Pressing once Display of the information of an alarm ALARM Pressing twice Display of an external alarm and external information

Pressing once Display of instruction value and the instructions input through MDI COMMAND

Pressing twice Display of the information regarding program restart


18

Pressing once Display of system diagnostic data DIAGNOSIS Pressing twice Display of the information regarding tool life management

Note: Clear the displayed screen by concurrently pressing a function key and CANCEL button. The corresponding screen is displayed when the function button is pressed again.

4.4.1 Status display

The status indication of the system is displayed on the lower right part of the screen:

The displayed indications are as follows:

NOT READY indicates that the control or servo system fails to operate. LSK indicate the LABEL

SKIP mode created after power on or reset of control rather than in MDI mode. BUF indicates

that a block is read in but not executed. The block not executed still does not disappear after

reset in rather than MDI mode. ABS indicates that MDI instruction is absolute and INC state will

be entered into when the SHIFT button is pressed. INC indicates that MDI instruction is

incremental ABS state will be entered into when the SHIFT button is pressed. ALM indicates that

an alarm is given. The alarm type will be displayed (the symbol blinks) when the ALARM button

is pressed. EDIT indicates that the editing function is being executed (the symbol blinks). The

stopping operation of edition shall be performed when the symbol exits. SRCH indicates that

sequence search is being performed (the symbol blinks). RESTR indicates that the period from

program restart to the return to the final axis (the symbol blinks).

4.4.2 Key input

The entries input with address keys or numerical keys are displayed at the bottom of the screen.

Status indication


19

Data cannot be typed in any more when the POSITION or and ALARM button among the function buttons is pressed to display a screen.

Press D/H to enter D and again to enter H.

Only a word consisting of one address and a figure can be typed in when Program edit is not being performed. Pressing CANCEL once clear a word.

One or more words, a block or any character string of up to 32 characters can be entered with the keys during Program edit.

The last entered character is cleared by pressing the CANCEL key. If the CANCEL key is pressed continuously, the typed characters will be cleared in succession.

Note: In EDIT mode, Program edit is possible when the PROGRAM button is pressed.

4.4.3 Display of program numbers and sequence numbers

Program numbers and sequence numbers are displayed at the top of the screen as shown in the following picture.


20

The meanings of the displayed sequence numbers and program numbers are as follows:

Mode Operation Indication

In the mode other than EDIT To display the last displayed sequence number Mode other than

EDIT When search a sequence number

To always display the sequence number during search

Auto mode (MEMORY)

Pressing the cursor ↑ key when the function button is in PROGRAM mode

To return to the start of a block To display the block

Pressing the cursor ↓ key when the function button is in PRG mode

To review programs in + direction from the actual position of the storage; To display the firstly found N value

Pressing the cursor ↑ key when the function button is in PRG mode

To review programs in - direction from the actual position of the storage; To display the firstly found N value

Edit mode

Entering reset state by pressing the RESET button

To return to the switch of the block and display the block

Auto mode (MEMORY) Program number search To display the program numbers

searched

4.4.4 Alarm display (function button ALARM)

When ALM is indicated at right bottom of the screen in case of alarm, clear warning messages through the following procedures Press the ALARM button. When the information about operator is displayed, press the ALARM button again to display alarm message.

Refer to Appendix 6 for the meanings of all alarm numbers

Note: As a rule, alarm message appear on the screen in the event of alarm.


21

4.4.5 Operator information

Once the machine sends out operator information, the information will be automatically displayed on the screen.

When operator information appears after some other page is displayed, press the ALARM button. When alarm message appears, press it again.

4.4.6 Display of actual position and reset (function key POSITION)

(1) Press the POSITION button. (2) Press the Page button. Data is displayed in one of the following three modes.

(I) Position display in a relative coordinate system

Relative position is displayed once operator resets a position to zero.

Reset: When the X , Y , Z or 4TH/5TH button is pressed, the pressed address characters will continuously blink. The relative position of the blinking address will be set for 0 when the SHIFT button is pressed again.

(II) Position display in a workpiece coordinate system

The current value of program coordinate system is set by G92, automatic coordinate system or reset and displayed. For Axis T, the currently selected tool number is displayed. Reset


22

(program protection unlocking)

For resetting, the X , Y , Z or 4TH/5TH button is pressed. The pressed address characters will continuously blink. The coordinate position of the blinking address when the SHIFT button is pressed again. The actual position of the blinking address is reset.

Note: Reset operation can only be performed in automatic stop status.

(III) Display of comprehensive position

The actual position is displayed in the following coordinate systems at the same time:

(a) The position in relative coordinate system (RELATIVE)

(b) The position in absolute coordinate system (ABSOLUTE)

(c) The position in machine coordinate system (MACHINE)

(d) The distance to be traveled (DISTANCE TO GO)

DISTANCE TO GO indicates the remaining distance of a block. The positions of all coordinate systems cannot be reset when displaying the comprehensive position. The unit of machine coordinate system is identical with that of the machine system.

4.4.7 Indication of instruction value (function button COMMAND)


23

(1) Press the COMMAND button.

(2) Press the PAGE button. Data is displayed in the following two modes.

(I) Display the formerly set modal values while executing an instruction value.

As shown in the above figure, the figure following character % stands for feedrate.

(II) Display the instruction value input by MDI or the instruction value to be executed next time.

(III) Display the instruction value of the next block to be executed during the tool offset of tool radius compensation C.


24

4.4.8 Setting (function button SETTING)

4.4.8.1 Display and setting of input, output, etc

(1) Press the SETTING button.

(2) Press the PAGE button. Setting and display may be performed in the following two modes.

(I) Setting of input and output

Setting (active when the program protection lock is disabled and inactive when it is locked,

which can be switched by parameter)

(a) Set the SELECTION MODE switch to MDI mode.

(b) Press the cursor button to move the cursor to the position of the item to be changed. The

cursor cannot be moved with the address key N.

(c) Enter 1 or 0 with the P key as shown in the following table.


25

0 1 X MIRROR IMAGE MIRROR IMAGE OFF MIRROR IMAGE ON Y MIRROR IMAGE MIRROR IMAGE OFF MIRROR IMAGE ON 4th AXIS MIRROR IMAGE MIRROR IMAGE OFF MIRROR IMAGE ON TV CHECK NO YES PUNCH CODE EIA ISO INPUT UNIT mm inch INPUT DEVICE1 DNC (can only be set to 0) INPUT DEVICE2 Unused RS232C input

Press P , O or 1 , INPUT to proceed.

Note 1: Unselected selection function cannot be set. For example, INPUT UNIT=1 cannot be used for a metric-system machine when metric/inch system selection function is not available. PUNCH CODE=1 cannot be set when ISO code input selection function is not available.

Note 2: INPUT UNIT is automatically rewritten when executing G20 (input in inch system and G21 (input in metric system).

Note 3: The ISO or EIA specified by PUNCH CODE is independent of input during data output. ISO or EIA code can be automatically identified.

Note 4: The output device for data output is set with data No. 341.

(II) Other settings and indications

The displayed numbers and their meanings are as follows:

Data No. Meaning 057 Run time (Unit: hr) (TMHOR) 058 Run time (Unit: min) (TMMIN) 059 Run time (Unit: sec) (TMSEC) 067 The retraction (CYCR) in fixed cycle G73 (depth high-speed Jog touring cycle) 068 The cutting origin in fixed cycle G83 (depth Jog touring cycle) 141 Run time (TIMDE1) 151 X value of Acme 1 of storage type travel limit 2 152 Y value of Acme 1 of storage type travel limit 2 153 Z value of Acme 1 of storage type travel limit 2 155 X value of Acme 2 of storage type travel limit 2 156 Y value of Acme 2 of storage type travel limit 2 157 Z value of Acme 2 of storage type travel limit 2 180 The sequence number whose execution has stopped 319 Settings (PRG8.MSBL)


26

340 Input device for selecting data storage (IDVICE) 341 Output device for selecting data for output (ODVICE) 355 Decelerating distance (automatic angle override) of the end point of block 356 Decelerating distance (automatic angle override) of the origin of block 407 Scaling override

Note 1: The data numbers other than those listed in the above table are not displayed.

Note 2: It is also possible to set the data number identical with the above table as a reference number.

Note 3: Refer to Appendix 5 for the details about data numbering.

Note 4: The details of data No. 340 and 341 are as follows: 3 4 0 I DVICE 3 4 1 O DVICE

IDVICE is used to select an input device for storing data in memory. When the set input device (INPUT DEVICE)2=1(Interface RS232), the setting is valid.

ODVICE is used to select an output device for data output.

Setting I/O 0 Input: paper tape reader; output: FACIT PUNCHER

1 Common for input and output: ASR33/ASR43; Set baud rate and other parameters to 310.

2 Common for input and output: reader/puncher; Set baud rate and other parameters to 311.



It is also possible to set them by parameters.

Setting (active when the program protection lock is disabled and inactive when it is locked, which can be switched by parameter)

(a) Set the SELECTION MODE switch to MDI mode.

(b) Press the cursor button to move the cursor to the position of the item to be changed. The cursor cannot be moved with the address key N.

(c) Press P , numerical keys and INPUT in succession to proceed.

4.4.8.2 Display and setting of user macro variables

It is possible to display general variable values and the local variable values of the currently called user macro body on LCD.

When a variable value is <Empty>, the display will be blank. When an absolute value exceeds 99999999, it displays OVER FLOW. When an absolute value is not 0 but less than 0.0000001, it displays UNDER FLOW.


27

Display

(1) Select a set chapter 2 Press the SETTING button for SETTING DISPLAY and press it again.

(2) Since the display covers 6 pages, you need to press the PAGE button to display the required page. Page 1——The currently called local variables #1-#20 for nesting Page 2——The currently called local variables #21-#33 for nesting Page 3——General variables #100-#119 Page 4——General variables #120-#139 Page 5——General variables #140-#149 Page 6——General variables #500-#509

(3) Move the cursor to the variable number to be displayed. Method 1: Press the cursor button and move the cursor in succession. The next page will be switched to once the cursor goes beyond the current page. Method 2: Set by typing with N, variable number and INPUT (active when the program protection lock is disabled). (a) Select MDI mode; (b) Type with P, variable number and INPUT when the variable is displayed and the cursor is

moved to the variable number to be changed.

4.4.9 Operating through MDI (function key COMMAND)

A program instruction to be executed may be input through MDI&DPL panel. (1) Example: X 10.5 Y200.5

(a) Set the selector switch to MDI position. (b) Press the COMMAND button. (c) Press the PAGE button. “Next block (command data input)” appears on the upper left of the

screen.


28

(d) Press the X , 1 , 0 , • and 5 keys and the INPUT button in succession. If the

numeral entered before pressing the INPUT button is incorrect, press the CANCEL button and enter the correct numeral again. If an error is found after pressing the INPUT button, it is necessary to enter the numeral again.

(e) Press the Y , 2 , 0 , 0 , • and 5 keys and the INPUT button. If the typed numeral is found incorrect, proceed in the same way as inputting X.

(f) Press the CYCLE START button on the control panel of the machine.

(2) Delete Y200.5 from X10.5 Y200.5 before pressing the CYCLE START button.

(a) Press the Y , CANCEL and INPUT in succession.

(b) Press the CYCLE START button on the control panel.

(3) Delete modal data.

Since G code and F, D and H data cannot be deleted, it is necessary to input correct modal data again for modification.

4.4.10 Start of MDI motion

Press the CYCLE START button to execute the instruction input through MDI.

4.4.11 Reset

As a rule, pressing the RESET button cancels alarm state.

Once the RESET button is pressed, the NC system is set to the following states:


29

State before reset State after reset In execution of a move instruction

The tool slows down and stops and the remaining travel disappears.

M, S, T or B In transfer

The transfer sequence stops. Refer to the manual supplied with the machine for the state of the machine now.

MDI mode The contents of the buffer memory are not eliminated. Storage 1 of buffer memory, block

Mode other than MDI mode

The contents of the buffer memory are eliminated and the BUF label disappears.

In any case, pressing the RESET button sets the NC system to reset state. In the modes other than MDI, the NC system is set to the LABEL SKIP mode.

4.4.12 Tool position offset

The setting display of tool radius compensation (function button: OFFSET)

(1) Press the OFFSET button.

(2) Press the PAGE button and display the required page.

Position offset No. 1-12 of page 1;

Position offset No. 13-24 of page 2;

Position offset No. 25-32 or 25-36 (optional) of page 3;

Position offset No. 37-48 (optional) of page 4;

┋ ┋

Position offset No. 97-99 or 97-108 (optional) of page 9;

┋ ┋

Position offset No. 193-200 (optional) of page 17;

The indication of page 1 of position offset

(3) Move the cursor to the offset number to be changed.

Method 1: Press the cursor button and move the cursor in succession. The next page will be switched to once the cursor goes beyond the current page.

Method 2: Set by typing with N , variable number and INPUT.

(4) Set the SELECTION MODE switch to a mode other than EDIT.


30

(5) Type P and POSITION OFFSET and then press the INPUT button.

The figure below is the page after P , 1 , 5 , • , 4 and INPUT is pressed when the position offset number is 19.

Note 1: When offset is changed in automatic operation, the new offset is not valid until its number is specified as D or H code.

Note 2: 0-9999 INPUT is used to reset all offsets to zero.

4.4.13 Setting and display of workpiece origin offset (Optional)

(1) Press OFFSET twice to display the WORKPIECE OFFSET page.

(2) Press the PAGE button to display the required page. Each page indicates as follows:

(i) Page 1(Workpiece coordinate offset 01)

00: Workpiece coordinate offset

01: The origin offset of the workpiece in workpiece coordinate system 1 (G54)



(ii) Page 2(Workpiece coordinate offset 02)




31


(3) Move the cursor to the number to be changed.

Method 1: Press the cursor button ↑ or ↓ and move the cursor in succession. The next page will be switched to once the cursor goes beyond the current page.

Method 2: Set by typing with N , NUMBER and INPUT.

(4) Set the SELECTION MODE switch to a mode other than EDIT.

(5) Type X , Y , Z or 4TH/5TH and the offset to be changed or set. Then press the INPUT button.

The setting range of the workpiece coordinates is 0 mm to ±7.999 mm or 0 inch to ±7.999 inch.

4.4.14 Measurement of tool length

(1) Press the OFFSET button to select the page of offset.

(2) Select a standard tool and manually move it until it contacts the fixed point of the machine (or fixed point of workpiece).

(3) Press the Z and SHIFT buttons so that the relative coordinates of Axis Z is reset to zero.

(4) Then select the tool to be measured and manually move it until it contacts the same fixed point. Now the difference between the standard tool and that to be measured is indicated in the display of relative position.

(5) Just like the setting of offset, move the cursor to the offset number and press the Z and INPUT keys but do not type in any numeral. The measured difference now is the offset to be input.

4.4.15 Program display (function button PROGRAM)

(1) When in EDIT mode, press the PROGRAM key to display the page of the selected character in the current selection program.


32

See the program number in Section 4.16 for which program is displayed. Pressing the cursor ↓ or ↑ key displays the contents of the program in sequence. When the cursor ↓ key is pressed, the page is displayed in forward direction. When the cursor ↑ key is pressed, it is displayed in reverse direction.

(Note 1) Set the SELECTION MODE switch to EDIT and press the PROGRAM button to display the contents of the program at the beginning of an executing or executed block. However, the beginning of the program will be displayed when it is returned to (see 4.4.24.4).

(2) In automatic operation

Press the PROGRAM button to display the current executing block.

Indications of the cursor (in automatic operation)

(a) When the cursor blinks, it indicates the block to be executed next time.

(b) When the cursor does not blink, it indicates the currently executing or executed block.

(3) Note 1: Strictly speaking, when the buffer register becomes empty neither in automatic operating state nor in feed hold state, the blinking of the cursor indicates the next block is going to read in the buffer register so as to continue to execute a program.

Note 2: When the PAGE button or cursor button is pressed in EDIT mode to move the cursor and the program is started in memory mode, the block at the cursor in EDIT mode is read in the buffer register.

(4) EDIT mode and the other modes except automatic mode

When the PROGRAM button is pressed, the executing and executed blocks are displayed on the left side of the page and the blocks to be executed next time on the right side.


33

Note: When an angle moves in G28, G29, a fixed cycle and tool radius compensation, the contents on the left and right of the page are the same for the situation in which a block causes the cycle movement of several blocks.

4.4.16 Program number search (function key PROGRAM)

When several programs are stored in memory, it is possible to search one of them.

0 1001 0 3054 0 1972

Search a program number

(1) Method 1

(a) Select a mode (EDIT or AUTO).

(b) Press the PROGRAM key.

(c) Enter O and the program number to be searched and then press the cursor ↓ key.

The switching page of the program is displayed after search.

(2) Method 2

(a) Select the AUTO mode.


(c) Press O , CANCEL and the cursor ↓ in sequence. The next stored program is

displayed.

(3) Method 3

(a) Select the EDIT mode


(c) Press O and the cursor ↓ to display the next stored program. In addition, the stored

programs are displayed in sequence for reviewing the stored program numbers when the

cursor ↓ key is pressed continuously.

Note 1: The start position is returned to when the stored program numbers are displayed.

Note 2: The contents in the buffer register are deleted when search a program number.

4.4.17 Inputting a program with keys

A program may be directly stored in memory with the MDI keys.

(a) Select the EDIT mode.

(b) Press the PROGRAM button to display the current program.

(c) Enter the program number to be stored. A new page appears when the O , the program

number and INSERT keys are pressed.


34

(d) Type in a block

[Example] When typing in G92 X500.0 Y200.0 M12,

(e) If a typed character is incorrect, press the CANCEL key to delete the lastly typed word.

Pressing the CANCEL key continuously deletes the typed words one by one from the last

typed one. If the number of the characters of a block exceeds 32, the program cannot be

entered. Now it is possible to divide the block with proper breakpoint.

(f) If the typed program is correct, press the INSERT key.

G 9 2 X 5 0 0 . 0 Y

2 0 0 . 0 M 1 2 EOB


35

(g) Enter blocks in succession by this means.

(h) For correcting a typed block, proceed as indicated in the section of Program edit.

(i) For restart, continuously move the cursor to the lastly typed character. The procedure is the same as insertion.

(j) When all programs are input and at the end of the procedures, press the RESET key if you want to return to the start position.

4.4.18 Deletion of a program

(Program protection lock is active; function button PROGRAM) Deleting a program stored in memory:


(b) Press the PROGRAM button.

(c) Press O , the program number and DELETE. The program whose number is entered is deleted.

4.4.19 Deletion of all programs

(Program protection lock is active; function button PROGRAM) Deleting all programs stored in memory:



(c) Press O , - , 9 , 9 , 9 , 9 and DELETE.

4.4.20 Sequence number search

(Function button PROGRAM)

Sequence number search is usually used to search a sequence number in the midway of a program and start or restart the program from the block whose sequence number is searched. Its skipping over blocks exerts no influence on the NC system. Namely when skipping over blocks, the coordinates of the blocks who are skipped over, M, S, T or G codes do not change the coordinates and modal values of the NC. When a macro is supplied, sequence number will not be displayed in search. Therefore, necessary M, S, T, G codes and coordinate system shall be set for the blocks to be started or restarted according to sequence number. If the block needs to restart search during machining, MDI must be used to assume M, S, T, G codes and coordinate system so that the


36

present state of the machine and NC system can be searched. (a) Select the AUTO mode.

(b) Select the program number where the sequence number to be searched belongs to.

0………………

Selected program

Search range To search the sequence number on the block, follow (c). When the sequence number to be searched does not exist on the block, however, the program number with a pre-search sequence number shall be selected for sequence number search.

(c) Press the PROGRAM button.

(d) Type in N and the sequence number to be searched. Then press the cursor ↓ to find the sequence number.

Note 1: Coordinates and modal data do not update during search. These data are set through MDI after search.

Note 2: The following items are checked during search.

TH check

TV check

Skipping over optional blocks

Alarm check (03, 04, 05 and 10)

Note 3: M98P×××× (calling a subprogram) is not executed during sequence number search. Therefore, when the sequence numbers in the subprogram called by the current selected program for search in AUTO mode, No. 060 alarm will be given.

In the following example, alarm will be given when N8888 is searched.

4.4.21 Restart of a program

When the machine restarts after the damage of the tool and stop of machining, the restart function starts the machine from a block to be restarted according to the specified sequence number.

(1) The tool is damaged (method P)

(a) Press the FEED HOLD button, retract the tool and replace a new tool. Change the offset when necessary.

(b) Set the PROGRAM RESTART button on the operation panel to ON.

(c) Press the PROGRAM button to display the present program.

(d) Press the cursor ↑ button to return to the starting point of the program.


37

(e) Press the P, the sequence number and the cursor ↓ to search the block to be restarted. If the same sequence number appears for many times, e.g. when sequence number search calls a subprogram for many times, the higher four digits are specified as the number of times of block appearance and the lower four digits as its sequence number.

P 1 2 3 4 0 1 2 3 Cursor ↓

Number of times Sequence number

The number of times is 1, the higher four digits can be omitted. The preceding zero can also be omitted when the number of times is established.

(f) After search, LCD changes to display the page for program restart.

The TARGET POSITION indicates the restarting position of machining.

The DISTANCE TO GO indicates the distance from the current tool position to the restarting position of machining.

M indicates the M codes instructed in the last 35 times.

T indicates the T codes instructed in the last 2 times.

S indicates the last instructed S code.

B indicates the last instructed B codes.

The first instructed code is indicated.

The program restart instruction or the CYCLE START instruction for eliminating each code in reset state is also indicated.

(g) Set the program restart switch to OFF.

(h) Observe the page. Output by the MDI panel in MDI mode if the M, S, T and B codes to be output exist. In this case, the M, S, T and B codes to be output no longer appear on the program restart page.

(i) When the tool moves to the machining restarting position in AUTO mode, check the distance indicated by DISTANCE TO GO is correct and the tool does not contact workpiece. Press the CYCLE START button after manually moves the tool to the position that does not contact the workpiece. Now the tool moves to the restarting position in the sequence of the 4th axis, axis X, axis Y and axis Z and restart machining.

(2) Restart machining (Q type) after the occurrence of the following conditions.

(a) Disconnect the power supply.

(b) Press the EMERGENCY STOP button


38

(c) The machine immediately stops due to storage type travel limit alarm.

(d) The coordinate system changes after the last automatic operation.

Example: (i) Specify G92 instruction through MDI. (ii) Move the coordinate system. (iii) Set the automatic coordinate system after returning to the reference point. (iv) Press the SHIFT button. (v) Owing to reset, the change of coordinate system, etc. (a) After switching on or the release of emergency stop and travel limit alarm, the machine

returns to the reference point before restart (see the Notes below) (b) The tool is moved to the programmed starting point of machining by manual and the set

modal data and coordinate system is identical with the restart of the machine. (c) If necessary, set or change the offset. (d) Set the PROGRAM RESTART button on the operation panel of the machine to ON. (e) Display the program by pressing the PROGRAM button. Search the required program when

it is not available. (f) Return the program to the origin point. Press the cursor ↓ button in automatic operating

mode. (g) Search the sequence number that the block restarts by pressing the Q and cursor ↓

button and typing in the sequence number. When the same sequence number appears for many times during search, the higher four digits are specified as the number of times of sequence number appearance and the lower four digits as its sequence number.

(h) After search, LCD turns to display the page for program restart.

(i) Set the program restart switch to OFF.

(j) Observe the page. Output by the MDI panel in MDI mode if the M, S, T and B codes to be output exist. In this case, they no longer appear on the program restart page.

(k) When the tool moves to the machining restarting position, check that the tool does not contact workpiece. If necessary, manually move the tool to the position that does not contact the workpiece.

(l) Check that the distance indicated by the DISTANCE TO GO is adequate.

(m) Return to the AUTO mode and press the CYCLE START button. Now the tool moves to the restarting position in the sequence of the 4th axis, axis X, axis Y and axis Z and restart machining.

Note 1: The following conditions, pressing the P button, the sequence number and the cursor ↓ button do not restart the program.

(a) After switching on, no automatic operation is performed.

(b) Automatic operation is performed after the release of emergency stop or storage type travel limit alarm.

(c) The coordinate system is established, changed or moved (the change in the offset of the origin of the external workpiece). The automatic operation is performed.

The above (a), (b) or 94—97 alarm reset causes P/S 97 alarm.

P/S 94 alarm caused by the establishment of a coordinate system;

P/S 95 alarm caused by the travel of a coordinate system;

P/S 96 alarm caused by the change of a coordinate system.

The block for the restartable machining is one of the many blocks. The block follows the block


39

when the coordinate system is last set of changed before the interruption of machinating.

Note 2: In P mode or Q mode, the tool moves to the machining restarting position by traveling by one axis each time. The stop of a single block is possible after the motion of the axis. However, JOG operation rather than MDI operation can be inserted. The returned axes cannot move.

Note 3: When move signal, offset and other conditions are different from the past, the tool cannot return to the machining restarting position identical with the past. The single block switch is set to ON or AUTO mode is switched to for continuous search operation.

Note 4: When feed hold is active during search or reset operation is performed after search, make sure to carry out program restarting operation from the beginning. After the end of search, however, the parameter No.007 “CLEAR Pos” shall be changed to reset state in MDI mode. Note 5: CYCLE START can be ignored provided that the automatic restart switch of program is set to ON position.

Note 6: Always bring the JOG absolute switch for ON position for JOG operation no matter it is before or after machining.

When a program restarting operation instead of resetting is performed after JOG operation or when JOG operation is performed along the axis that has not returned to the machining restarting position, the concerned motion is performed once the manual absolute switch is set to ON position regardless that the manual absolute switch is in ON or OFF position.

Note 7: In principle, the tool cannot return to the correct position in the following cases:

(a) The manual absolute switch is brought to OFF position for JOG operation.

(b) The tool is moved in the lock state of the machine or after the cancellation of axis Z instruction.

(c) Mirror image function is used.

(d) The coordinate system is not set at the beginning of incremental Program edit.

(e) JOG operation is inserted during the return of an axis.

(f) Machine lock is disabled after the program restart is instructed.

(g) Program restart instruction is given during the execution of the cutting program with skip or the blocks of an absolute instruction.

(h) A coordinate system is established after search. Nevertheless, in the condition of (c) the return of the tool in P mode in the block executed by setting the mirror image machining switch to OFF position as well as the blocks that follow. In this case, the mirror image machining state is the same as interruption. No alarm is given in any case.

Note 8: When the specified block only includes M98, M99, macro calling instruction (M65, G66 and G67) or macro statement, or no specified block is searched, No.60 alarm will be given.

Note 9: When program restarting operation is instructed and G28 is detected without returning to the reference point after power on or cancellation of emergency stop or travel limit alarm (immediate stop), P/S alarm (98) will be resulted in.

Note 10: After the end of search, P/S alarm (99) is given when a move instruction is executed through MDI operations before axis motion.

Note 11: After the program restart is instructed, “RESTR blinks at the button of the LCD screen before the return of the last axis (Z).

Note 12: When the block before the restart block has G28, G30, an instruction or incremental instruction, the absolute position of the 4th axis can be displayed in the range of 360°. In this case, the 4th axis is an axis of rotation and the direction of returning to the reference point is negative.

4.4.22 Program number comparison stop function

The function is used to stop machining after an instruction is executed to the preset sequence number.


40

(a) Select the MDI mode.

(b) Press the SETTING button to display the SET page. Move the cursor to the set number 180 by pressing the cursor ↑ or ↓ key. The cursor cannot be moved with address N.

(c) Type the instruction in the sequence of P , the sequence number to be stopped and INPUT.

(d) Select the AUTO mode and get ready for operation by setting the machine.

(e) Press the CYCLE START button.

The machine stops after the data in the block whose sequence number has been predetermined in step (c).

The predetermined sequence number is cleared while the machine is stopping.

To perform another comparison stop, repeat the above procedures from (a).

Note 1: Sequence number O cannot be used for comparison stop

Note 2: The predetermined sequence number is cleared by setting.

4.4.23 Display of parameters (function button: PARAMETER)

Press the PARAMETER button to display the parameters, which are laid out in several pages. Find the desired parameter by pressing the PAGE button (see Appendix 5 for the meanings of parameters).

4.4.24 Program edit

(Function button: PROGRAM)

The function is used to modify the stored programs.

(1) Set the SELECTION MODE switch to EDIT.

(2) Press the PROGRAM button.

(3) Select a program. Proceed with (4) if the program has been selected; otherwise perform program number search.

(4) Search the words to be modified by scanning or word search.

(5) Modify, insert or delete the words.

Note 1: Definition and edit unit

A word comprises an address and the numeral that follows. For user macro, however, the concept of word is indefinite. Hence the concept of “edit unit” is adopted. Edit unit serves as the object of modification and deletion in a single operation and moves the cursor to its beginning in a single pass. For data insertion, the data is inserted behind the edit unit.

Definition of edit unit

① From one address to the next one;

② An address is a letter symbol: WHILE, GOTO, END, DO, =, or ; (EOB)

According to the definition, a word is also an edit unit. On the basis of the following explanations about edit, strictly speaking, word shall be called “edit unit”.

Note 2: During program execution, machining is temporarily suspended by single block skipping, feed hold and other functions. Nevertheless, continuing to execute a program is not allowed after program modification, insertion and deletion; otherwise the program cannot be correctly executed as required by program data. Program is displayed on the LCD after subsequent machining.

To modify stored data in part program edit mode, they must be modified in reset condition before program execution or when resetting operation is performed after edit.


41

4.4.24.1 Word scanning

(1) Press the cursor ↓ button.

The cursor moves forward word by word on the screen. The cursor is displayed underneath the address character of the selected word.

(2) Press the cursor ↑ button.

The cursor returns word by word on the screen. The cursor is displayed underneath the address character of the selected word.

Example:

(3) Continuous search can be conducted by pressing down and holding the cursor ↓ or ↑

button.

(4) The next page is displayed and search starts from the beginning of the page by pressing the page ↓ button.

(5) The previous page is displayed and search starts from the beginning of the page by pressing the page ↑ button.


42

(6) Displaying page by page is possible by pressing down and holding the cursor ↓ or ↑ button.

4.4.24.2 Word search

Search a specified word from the present position forward.

Current word X1234 is the object of search. Search direction

(1) Enter X , 1 , 2 , 3 and 4 with the keypad.

Note 1: The search that only enters X123 and X1234 with the keypad can not be performed.

Note 2: The search that only enters X9 and X009 with the keypad can not be performed. 009 shall be entered with the keypad for the search of X009.

(2) Search starts when the cursor ↓ is pressed. The cursor is displayed underneath X in X1234 after the search.

4.4.24.3 Address search

Search a specified address from the present position forward.

Current word M03 is the object of search.

(1) Type in M .

(2) Search starts when the cursor ↓ is pressed. The cursor is displayed underneath M after the search.

Note 1: Pressing the CANCEL button after typing in a numeral deletes the latter and displays a blank space. Pressing the CANCEL button only indicates CAN.

Note 2: Both word search and address search do not start by pressing the cursor ↑ button.

4.4.24.4 Methods for returning to the beginning of a program

Beginning Current word

(1) Method 1

A program is displayed from its beginning when the RESET button is pressed in EDIT mode.

(2) Method 2

Perform sequence number search.

(3) Method 3

(a) Set the SELECTION MODE button to AUTO.

N1234×1000 Y1250：X1234：N5678 M03：

01100 N0001 X12.34: Z15.67: G01×12.5: M04

N1234×100.0 Y1250：X1234：N5678, M03：


43


(c) Press the cursor ↑ button to return to the EDIT mode for editing a part program.

4.4.24.5 Word insertion (active when the program protection lock is disabled)

Insert T105

Object of search

(1) Quickly search and scan the word preceding the position where a word is to be inserted.

(a) Scan. See 4.24.1.

(b) See 4.24.2 for word search. When Y1250 is in front of the currently indicated position, first move the cursor to the beginning of the program.

(2) Type in T , 1 , 0 and 5 and press the INSERT button.

Before insertion

After insertion

Note 1: When what is inserted is not an address but a numeral, the inserted number is added to

the word indicated by the cursor. (Edit unit: In the above example, the insertion of 2.5 will create

N1234×100.0 Y1250：X1234：N5678, M03：


44

Y12502.5 when the cursor is underneath Y in Y1250.

Note 2: A numeral can also be added to all addresses.

E.g. EOB, IF, etc. When the cursor is underneath “;”, the insertion of 23 will create “; 23”.

However, it makes no sense in programming.

4.4.24.6 Word modification (active when the program protection lock is disabled)

To be changed to M15

(1) Search and scan the word to be modified.

(2) Type in M , 1 and 5 and press the ALTER button.

The program is to be modified.

4.4.24.7 Insertion and modification of several words, blocks and strings

Word, block, character string and other information can be inserted (up to 32 characters). In the

example above, to insert T105 M20, type in T105 M20 and press the INSERT button.

Before insertion

N1234×100.0 Y1250：T105： S1234：

N1234×100.0 Y1250：M15： S1234：


45

After insertion

A word indicated by the cursor can be changed to a word, block or a string, etc.

Note 1: When the cursor is underneath Y in Y1250, the insertion of 25 M20 will become Y1250 2.5 M20.

Note 2: When the cursor is underneath Y in Y1250 T105, the insertion of 2.5 M20 will become Y1250 2.5 M20.

4.4.24.8 Word deletion (active when the program protection lock is disabled)

To delete Y1250 (1) Search and scan the word to be deleted.

(2) Press the DELETE button.

The program after deletion

4.4.24.9 The deletion of the part before EOB

Current word

Range of deletion

Press the EOB and DELETE buttons to delete the part before EOB and move the cursor to the underneath of the address character of the next word.

4.4.24.10 Deletion of blocks (active as program protection lock is disabled)

The range of deletion covers from the currently dedicated word to the block whose sequence number is specified.

N1234 ×100.0 Y1250 T105： X1234：

N1234 ×100.0 T105： X1234：

N1234 ×100.0 Y1250 T105 M13： X1234：


46

Current word Enter N2233 with the keypad

Range of deletion

(1) Type in the sequence number of the last block to be deleted. Type in N , 2 , 2 , 3 and 3 in this example.

(2) Press the DELETE button.

4.4.24.11 Storage sorting

The frequent edit of part program sometimes prevents the storage from economic usage, resulting in the failure to store the program data whose length is specified. Hence it is necessary to regularly clean up the storage.

Press the CANCEL and SHIFT buttons in succession in the EDIT mode. After sorting, the admissible number of characters is indicated at the bottom of the screen.

Note 1: For one program, the storage stores the specified length of the program. For many programs, some storage areas are used to identify these programs.

Note 2: The storage areas to be modified or inserted that exceed the actual length are wasted in quick part program edit. Storage sorting may eliminate the waste.

4.4.24.12 The indication of all stored program numbers

Once the contents of the storage described in 4.24.11 are sorted, all stored program numbers are displayed.

4.4.24.13 Edit of user macro (active as the program protection lock is disabled)

User macro may be edited using the SHIFT key. Operate the key in EDIT mode and when the program protection switch is released. The following points shall be observed.

(a) SHIFT key

Once the SHIFT key is pressed, the cursor (the cursor for keyboard entry: the cursor is in the position of the character whose data is last input) changes from “—” to “∧”. Press the key with a character in the lower right angle of the key top in this state. The character in the lower right angle can be entered.

After entering a character, the cursor restores to the initial “—”. If the SHIFT key is pressed

N1234 M10；M15×100.0……T0122；N2233 T1200；N3344 Y10.0：


47

twice, the cursor also restores the initial “—”.

(Example)

(b) Deletion, insertion and modification of a program

While editing an entered user macro, the cursor moves at the following locations:

(i) At an address

(ii) At the / of an optional block skipped over

(iii) At the left beginning # of a substitution statement

(iv) At (·=)OR;

(v) At the leading character of IF, WHILE, GOTO, END or DO

On the LCD screen, there is a blank space for a character before the above characters. Deletion, modification and insertion may be performed between the front and rear cursor positions.

(Example) Cursor position

N001x-#100: #1=123； N002 / 2x[12/#3]: N003x-SQRT[#3/3*[#4+1]]: N004x-# 2 Y#1: N005#5=1+2-#10； IF[#1 NE 0]GOTO 10: WHILE[#2LE·B]D01: #[2000+#2]=#2*10: #2=#2+1: END1:

(Note 1) The cursor cannot be stopped in ( ).

Control OUT/IN

(Example)(#1=100):

The cursor cannot stop here.

(Note 2) The position of the cursor can change with the changed program.

(Example) X100 Y200: before program modification:

If Y200 is changed into 100 with the ALTER key, it will become X100 100:

(c) Abbreviations of macro word

To change or insert a macro word, it can be abbreviated to its first two characters. The underlined part can alternate the word as an abbreviation.

WHILE, GOTO, END, XOR, AND, SIN, COS, TAN,


48

ATAN, SQRT, ABS, BCD, BIX, FUP, ROUND.

(Example): When WH[TA[#1*AB[#2]]LERO[#3]] is entered as data of keyboard entry, the actual entry will be:

WHILE[TAN[#1*ABS[#2]]LEROUND[#3]]

4.4.25 Indication of run time

Automatic operating time can be accumulated and displayed in hour, minute and second (increment of 2sec) on the screen.

Time is displayed as indicated in the picture below when the SETTING button is pressed. Press the PAGE button for other pages.

Note 1: The accumulated time includes automatic operating time but not the single block offtime, feed hold offtime, etc.

Note 2: If the power supply is switched off immediately after the stop of automatic operation, a time error up to 6min may be caused after power on again.

Note 3: When necessary, time can be preset through setting operations. The data number is 57, 58 or 59.

4.4.26 Menu switching function

It is possible to enable or disable the switching function of the NC storage using the LCD instead of the operation panel of the machine.

With this function, the number of switches on the operation panel can be reduced. The following signals may be switched on or off through the LCD.

(1) Single block (SBK)

(2) Machine lock (MLK)

(3) Dry run (DRN)

(4) Optional block skip 1 to 9(BDT1—9)

(5) Mirror image (MIX, MIY, M14 and M15)

(6) Display lock (DLK)

(7) Auxiliary function lock (AFL)


49

(8) Axis Z neglected (ZNG)

(9) JOG absolute (ABS)

After the signal data is stored in memory, the switching of these data displayed on the LCD remains unchanged even the NC power is disconnected.

These signals are not completely replaced by those displayed on the LCD. These signals are deemed to be switched on no matter whether the machine signals or the signals set on the LCD are switched on. Accordingly, these signals can be switched on or off through the LCD by disconnecting the above listed optional signals through the operation panel.

Setting and display: The LCD state of the above signals may be displayed through the following operations.

Display

(i) Select the set chapter 3

For setting display, press the SETTING button and then press it twice again.

(ii) Press the PAGE button to select the desired page from the two pages than can be displayed.

Page 1: The part other than optional blocks skipping

Page 2: Optional block skipping 1~9.

Setting

Proceed as follows after the above procedures.

(iii) Move the cursor to the page number to be changed.

Move the cursor to the page number to be changed by pressing the cursor ↑ or ↓ key.

(iv) When the address P is pressed, enter 1 for switching on and 0 for switching off. Press the keys in the sequence of (P) (entry).

1 2


50

4.4.27 Operations of LCD soft function keys

4.4.27.1 General

Here function buttons (POSITION, PROGRAM, OFFSET etc) are used as soft function keys. Their meanings may be displayed on the LCD. All the pages abstained by pressing the soft function keys are described below.

4.4.27.2 Display

(1) Display of actual position

The actual position of relative coordinate system is displayed on the LCD when the soft function key REL is pressed.


51

Press the page ↓ key the update display as shown above. The positions of workpiece coordinate system and relative coordinate system are exchangeable on the screen.

(2) Display of a program

Press the PROGRAM soft function key to display a program. It is possible to make background edit (edit the programs other than the currently running programs) using B. EDIT.

Press the PROGRAM soft function key again to display program list. The program list is displayed as follows.


52

(3) Display of offsets

When the OFT soft function key is pressed, the offset corresponding to each tool number is indicated on the LCD. Press the page ↑ or ↓ key and cursor ↑ or ↓ key to select the desired data. At the same time, the actual position of relative coordinate system is displayed on the lower part of the LCD.

(4) Display of an instruction


53

Press the COMMAND soft key. The data displayed on three pages of the LCD appears on the screen as shown in the above figure. The screen changes as follows when the page ↓ key is pressed.

(5) Setting


54

Press the SET soft function key. Now all set data is displayed on the screen. Run time is

displayed in the page of SET DATA 01.


55

Press the MACRO key. Now the local variable and common variable of user macro are

displayed on the LCD screen.

Press the ON-OFF key. The menu switch window is displayed as shown as shown in Section

4.26 (menu switch function).

(6) Display of alarm and operation information

Pressing the ALM soft function key displays the alarm messages as shown in the above figure.

Pressing the OUTMESS soft function key displays the external information as shown in the

above figure.


56

(7) Parameter display

Pressing the NC PARA and PC PARA soft function keys to display the relevant parameters on the LCD.

Pressing the page ↑ or ↓ and cursor ↑ or ↓ to display the desired parameters.

(8) Display of diagnostic data


57

Pressing the DGN soft function key displays 64 diagnostic data.

Pressing the page ↑ or ↓ and cursor ↑ or ↓ to display the desired diagnostic data.

4.4.27.3 Direct entry of measured workpiece origin offset

The coordinates of the relative coordinate system that offsets at the workpiece origin and is

indicated by the LCD screen may be set as workpiece origin offset. With the function the

relative coordinate system is cleared away at the reference point and the machine is moved to

the workpiece origin by JOG. Now the coordinates of the relative coordinate system may be set

as workpiece origin offset. In this way it is easy to set the workpiece origin offset.

(1) Operating procedures

The relative coordinate system may be cleared away and workpiece origin offset set on the

workpiece origin offset page of the LCD through the following procedures.

(a) Delete the relative coordinate system

Pressing the X and SHIFT keys deletes the relative coordinate system of axis X (this

operation accordingly applies to axes Y and Z as well as the 4th and 5th axes).

(b) Set workpiece origin offset

Press the X and INPUT keys after moving the cursor to the required workpiece offset

number. Then the coordinates of the axis X in the corresponding coordinate system is set

as the axis-X workpiece origin offset of the selected workpiece offset number.

(This operation accordingly applies to axes Y and Z as well as the 4th and 5th axes

Note: When the X key is pressed in steps (a) and (b), the X of the relative coordinate

system blinks.


58

4.5 Position Indication through Position Display Unit (Available upon Customer’s Request)

The position display unit indicates the actual position. The position display reset buttons are

connected to the position display unit. Each button corresponds to one axis. The position

display of the relevant axis is cleared when any one of the buttons is pressed.

After the absolute origin (G92) is programmed and established, it is indicated on the display unit

through parameter setting (PPD) coordinates.

Note 1: Position pulse cannot be sent to the position display unit when the DISPLAY LOCK

switch is set to ON position. The switch may used to prevent writing offset in position indication

by manually moving the coordinate system.

Note 2: Position is indicated in Inch-system format in the event of entry in inch system.

Position is indicated in metric format in the event of entry in metric system. The RESET button

shall be pressed so that the position indication is zero when the input system is switched from

inch system to metric system, vice versa.

Note 3: Machine compensation data, e.g. amount of clearance compensation cannot be

indicated on the position display unit.

GSK983M Milling CNC System Operating Manual (Volume II: Operations)

59

Appendix 1 Codes for Programming

ISO Code EIN Code Character 8 7 6 5 4 3 2 1 Character 8 7 6 5 4 3 2 1 Meaning

0 ○ ○ 0 0 ○ ○ Numeral “0” 1 ○ ○ ○ 0 ○ 1 ○ ○ "1 2 ○ ○ ○ ○ ○ 2 ○ ○ "2 3 ○ ○ ○ ○ ○ 3 ○ ○ ○ ○ ○ "3 4 ○ ○ ○ ○ ○ 4 ○ ○ "4 5 ○ ○ ○ ○ ○ 5 ○ ○ ○ ○ "5 6 ○ ○ ○ ○ ○ 6 ○ ○ ○ ○ "6 7 ○ ○ ○ ○ ○ ○ ○ 7 ○ ○ ○ ○ "7 8 ○ ○ ○ ○ ○ 8 ○ ○ "8 9 ○ ○ ○ ○ ○ 9 ○ ○ ○ ○ "9 A ○ ○ ○ a ○ ○ ○ ○ Address A B ○ ○ ○ b ○ ○ ○ ○ ? "B C ○ ○ ○ ○ ○ c ○ ○ ○ ○ ○ ○ ? "C D ○ ○ ○ d ○ ○ ○ ○ "D E ○ ○ ○ ○ ○ e ○ ○ ○ ○ ○ ○ "E F ○ ○ ○ ○ ○ f ○ ○ ○ ○ ○ ○ "F G ○ ○ ○ ○ ○ g ○ ○ ○ ○ ○ ○ "G H ○ ○ ○ h ○ ○ ○ ○ ? "H I ○ ○ ○ ○ ○ i ○ ○ ○ ○ ○ ○ "I J ○ ○ ○ ○ ○ j ○ ○ ○ ○ ? "J K ○ ○ ○ ○ ○ k ○ ○ ○ ○ "K L ○ ○ ○ ○ ○ l ○ ○ ○ ○ "L M ○ ○ ○ ○ ○ m ○ ○ ○ ○ "M N ○ ○ ○ ○ ○ n ○ ○ ○ ○ "N O ○ ○ ○ ○ ○ ○ ○ o ○ ○ ○ ○ "O P ○ ○ ○ p ○ ○ ○ ○ ○ ○ "P Q ○ ○ ○ ○ ○ q ○ ○ ○ ○ "Q R ○ ○ ○ ○ ○ r ○ ○ ○ ○ "R S ○ ○ ○ ○ ○ s ○ ○ ○ ○ "S T ○ ○ ○ ○ ○ t ○ ○ ○ ○ "T U ○ ○ ○ ○ ○ u ○ ○ ○ ○ "U V ○ ○ ○ ○ ○ v ○ ○ ○ ○ ？ "V W ○ ○ ○ ○ ○ ○ ○ w ○ ○ ○ ○ "W X ○ ○ ○ ○ ○ x ○ ○ ○ ○ ○ ○ "X Y ○ ○ ○ ○ ○ y ○ ○ ○ ○ ？ "Y Z ○ ○ ○ ○ ○ z ○ ○ ○ ○ "Z

DEL

○ ○ ○ ○ ○ ○ ○ ○ ○

DEL

○ ○ ○ ○ ○ ○ ○ ○

*

Delete (cancellation of an incorrect hole)


60

ISO Code EIN Code Meaning Character 8 7 6 5 4 3 2 1 Charact

er 8 7 6 5 4 3 2 1

NUL

0

Blank

0 *

No-hole and EIA codes are not used in effective-value information area

BS ○ ○ 0 BS ○ ○ 0 ○ * Rewind ( backspace )

HT ○ 0 ○ Tab ○ ○ ○ 0 ○ ○ * Separator LForNL ○ 0 ○ CRorEO

B ○ 0 End of block

CR ○ ○ 0 ○ ○

0 *

Return of printer base

SP ○ ○ 0 SP ○ 0 * Blank space % ○ ○ 0 ○ ○ ER ○ 0 ○ ○ End of rewinding ( ○ ○ 0 (2-4-3) ○ ○ 0 ○ Control OUT (start

of note) ) ○ ○ ○ 0 ○ (2-4-7) ○ ○ 0 ○ Control IN (end of

note) + ○ ○ 0 ○ ○ + ○ ○ ○ 0 * Positive sign － ○ ○ 0 ○ ○ － ○ 0 Negative sign

: ○ ○ ○ 0 ○

0

As a program number of ISO codes

/ ○ ○ ○ 0 ○ ○ ○ / ○ ○ 0 ○ Stop of block selection

· ○ ○ 0 ○ ○ · ○ ○ ○ 0 ○ ○ Full stop (decimal point)

# ○ ○ 0 ○ ○ 0 * Well number $ ○ 0 ○ 0 * Unit number & ○ ○ 0 ○ ○ & ○ 0 ○ ○ * & (and) ’ ○ 0 ○ ○ ○ 0 * Apostrophe * ○ ○ ○ 0 ○ 0 * Asterisk , ○ ○ ○ 0 ○ , ○ ○ ○ 0 ○ ○ * Comma ； ○ ○ ○ ○ 0 ○ ○ 0 * Semicolon

＜ ○ ○ ○ 0 ○ 0 * Left angular bracket

= ○ ○ ○ ○ 0 ○ ○ 0 * Equal sign ＞ ○ ○ ○ ○ 0 ○ ○ 0 * Right angular

bracket ？ ○ ○ ○ 0 ○ ○ ○ 0 * Question mark

@ ○ ○ 0 0 * @ sign ” ○ 0 ○ 0 * Quotation mark [ ○ ○ ○ ○ 0 ○ ○ 0 * Left brace ] ○ ○ ○ ○ 0 ○ ○ 0 * Right brace


61

(Note 1) “*” code is read in memory only it appears in a note and is invalid in other information areas.

(Note 2) “?” code is read in memory only it appears in a note and causes alarm when it appears

in other information areas.

(Note 3) When a user macro is selected, the following codes are usable in the effective

information areas.

For ISO: +, [, ], #, *, =, B, C, H, J, V, Y.

For EIA: +, [, ], &, the codes set by parameter and B, C, H, J, V, Y.

(Note 4) The codes not listed in the table are ineffective even its parity is correct.

(Note 5) The use of a code with incorrect parity may cause TH alarm. But it is ignored in notes

and does not cause TH alarm.

(Note 6) The output of all the eight digits does not cause alarm for EIA code.


62

Appendix 2 G Codes List

G Codes Group No. Function G00* Positioning (quick) G01* Linear interpolation (cutting feed) G02 Arc interpolation CW (clockwise circle) G03

01

Arc interpolation CCW(counterclockwise circle) G04 Suspension G07 imaginary axis designation G09 Accurate stop check G10

00

Offset, work zero offset setting G17* To select XY plane G18 To select ZX plane G19

02 To select YZ plane

G20 To input in inch system G21 06 To input in metric system G22 Storage travel limit ON G23 04 Storage travel limit OFF G27 Reference point return check G28 To return to reference point G29 To return from reference point G30 To return to the 2nd, 3rd and 4th reference points G31

00

To skip over cutting G33 01 Thread cutting G40* To cancel tool compensation G41 Tool compensation – left side G42

Tool compensation – right side

G43* Tool radius compensation, + G44* Tool radius compensation, - G49*

08 To cancel tool length compensation

G45 To increase tool offset G46 To reduce tool offset G47 To increase tool offset by twice G48

00

To reduce tool offset by twice G50* Zooming OFF G51 11 Zooming ON G54* To select workpiece coordinate system 1 G55 To select workpiece coordinate system 2 G56 To select workpiece coordinate system 3 G57 To select workpiece coordinate system 4 G58 To select workpiece coordinate system 5 G59

14

To select workpiece coordinate system 6 G60 00 One-way positioning G61 Accurate stop detecting mode G62 To enable automatic angle adjustment G64*

15 Continuous cutting mode

G65 00 Simple recall of a user macro G66 Modal recall of microinstruction G67* 2 To cancel modal recall of microinstruction G73 Gun drilling cycle G74 Left-handed tapping cycle G76

09

Finish boring


63

G80* To disable fixed cycle G81 Drilling cycle, spotter G82 Drilling cycle, counter boring G83 Depth drilling cycle G84 Tapping cycle G85 Boring cycle G86 Boring cycle G87 Reverse boring cycle G88 Boring cycle G89 Boring cycle G90* Absolute-value programming G91* 03 Incremental-value programming G92 00 Coordinate system setting G94* Feed per minute G95 05 Feed per rotation G96 Feed at constant speed G97* 13 To cancel constant speed control G98* To return fixed cycle to the initial point G99 10 To return fixed cycle to point R

(Note 1) The G codes marked with * are the initial G codes of all groups. That is, these G codes are established when power on or pressing the RESET key (the system parameters specifying initial G codes are validate).

The selection of the state of the initial G codes such as G00, G01, G43, G44, G49, G90, G91 or G94 and G95 shall be set by parameters (G00, G43, G44, G90 and G95).

For G20 or G21, it becomes the state before power off.

(Note 2) The G codes in group 00 are modal and are only valid in the blocks they belong to.

(Note 3) When a G code not listed in the above table is specified or an optional G code not defined by control unit is specified, (N0.010) will give an alarm. (N0.010) But G38 and G39 are ignored.

(Note 4) Some G codes may be specified in the same block even they do not belong to the same group. When 2 or more G codes than belong to the same group are specified in a block, the lastly specified G code will be valid.

(Note 5) If any G code in group 01 in fixed cycle mode, the fixed cycle will be automatically disabled and the system will be in G80 state. However, the G codes in group 01 are not subject to the influence of the G codes of fixed cycle.

(Note 6) G70 and G71 replaces G20 and G21 (special G codes) by parameter setting (GSP).

(Note 7) The G codes of all groups are displayed.


64

Appendix 3 Ranges of Instruction Values

Input in mm Output in mm

Input in inch Output in mm

Input in mm Output in inch

Input in inch Output in inch

Minimum setting unit 0.001mm 0.001°

0.0001inch 0.001°

0.001mm 0.001°

0.0001inch 0.001°

Maximum travel (the value starts from reference point) ±99999.999mm ±99999.999mm ±3937.0078inch ±99999.999inch

Max. instruction value ±99999.999mm ±99999.999°

±3937.0078inch±99999.999°

±99999.999mm ±99999.999°

±99999.999inch±99999.999°

When adjusting cutting feed by 100%

Feed per minute 1 mm/min to 15000 mm/min

0.01 inch/min to 600.00

inch/min

1 mm/min to 15000

mm/min

0.01 inch/min to 600.00

inch/min

Feedrate at high speed (all axes are independent)

30 mm/min to 15000

mm/min

30 mm/min to 15000

mm/min

3.0 inch/min to 600.0

inch/min


inch/min

Upper limit of cutting feedrate

Manual feedrate

F0

6 mm/min to 15000

mm/min

6 mm/min to 15000

mm/min


inch/min


inch/min

JOG feedrate 1 mm/min to

2000 mm/min


inch/min

0.5 mm/min to 1016

mm/min

0.02 inch/min to 40

inch/min

Coordinates of 2nd reference point (the value starts from reference point)

0 mm to ± 99999.999mm

0 mm to ± 99999.999mm

0 inch to ±3937.0078inch


Tool offset 0 mm to ± 99999.999mm

0 inch to ± 99999.999inch

0 mm to ±99999.999mm


Minimum value of incremental feed 0.001mm 0.0001inch 0.001mm 0.0001inch

Clearance compensation 0mm to 0.255mm 0 mm to 0.255mm

0 inch to 0.255inch

0 inch to 0.255inch

Compensation of screw pitch error

0mm to ±0.007mm

0mm to ±0.007mm

0inch to ±0.007inch 0inch±0.007inch

Setting range of storage travel limit (the value starts from reference point)

0mm to ± 99999.999mm

0mm to ± 99999.999mm

0inch to ±3937.0078inch

0inch to ±99999.999inch

Pause 0s to 99999.999s 0s to 99999.999s 0s to 99999.999s 0s to

99999.999s


65

Appendix 4 Calculating Chart

A4.1 The tool path in a turning angle section

(1 ) Summary

Due to the delay of servo system (as a result of exponential deceleration/acceleration during

cutting or the use of the positioning system of a DC servo motor), a minor deviation exists

between the tool path (tool center path) and instructed path as shown in Fig. 4.1 (a). In this

center, the time constant T1 of exponential deceleration/acceleration is fixed to 0.

Fig. 4.1 (a): The tool path regarding a turning angle section

The tool path depends on the following parameters:

(a) Feedrate (V1, V2)

(b) Degree of the turning angle (θ)

(c) Time constant (T1)(T1 = 0) of exponential deceleration/acceleration during cutting

(d) Loop gain of positioning system

(e) Existence of buffer

This document makes theoretical analysis of tool path with the above parameters. The tool path

of temporarily set parameters is displayed in graph.

The above notes shall be observed for programming. Note whether the machining shape is

within the desired accuracy range.

That is, when it is possible to reach the theoretical accuracy, hold for a proper time using the

suspension function until the instruction speed drops to zero before reading in the next block.

(2) Analysis

In the following conditions, make analysis of the tool path as shown in Fig. 4.1(b).

(a) Feedrate remains constant in the blocks before and after the turning angle.

(b) The control is provided with a buffer (error changes with the reading rate of the input

equipment and the number of characters of the next block).


66

VX1 = V·cosφ1

VY1 = V·sinφ1

VX2 = V·cosφ2

VY2 = V·sinφ2

π－(φ1-φ2)=θ

[Explanations for the symbols]

V: Feedrate in the blocks before and after turning angle

VX1: X component of the feedrate in the previous block

VY1: Y component of the feedrate in the previous block

VX2: X component of the feedrate in the next block

VY2: Y component of the feedrate in the next block

θ: Angle of the turning angle

φ1: The included angle between the direction of the instruction path in the previous block and

axis X

φ2: The included angle between the direction of the instruction path in the next block and axis

X


67

Calculation of initial value

The initial value at the beginning of a turning angle, i.e. the X and Y coordinates at the end of

the distribution of the control unit are determined by the time constant of the positioning system

of the used DC motor.

X0 = Vx1(T1+T2)………(1) Y0 = Vy1(T1+T2)………(2)

T1: Time constant (T1 = 0) of exponential deceleration/acceleration

T2: Time constant (reciprocal of position loop gain) of positioning system

Analysis of tool path

The feedrates in the directions of axis X and Y in the turning angle are expressed in the

following formulas.

Vx(t)=(Vx2－Vx1)[1－ { } Vx1]expexpVx1

22

11

21+⎟⎟

⎠

⎞⎜⎜⎝

⎛−×−⎟⎟

⎠

⎞⎜⎜⎝

⎛−×

− TtT

TtT

TT

= Vx2⎥⎥⎦

⎤

⎢⎢⎣

⎡

⎪⎭

⎪⎬⎫

⎪⎩

⎪⎨⎧

⎟⎟⎠

⎞⎜⎜⎝

⎛−×−⎟⎟

⎠

⎞⎜⎜⎝

⎛−×

+−

22

11

21expexp

TVx11

TtT

TtT

T ……………………(3)

Vy(t)= 22

21

121

21 VyexpexpT

VyVy+

⎪⎭

⎪⎬⎫

⎪⎩

⎪⎨⎧

⎟⎟⎠

⎞⎜⎜⎝

⎛−×−⎟⎟

⎠

⎞⎜⎜⎝

⎛−×

−−

TtT

TtT

T ……………………(4)

The coordinates of the tool path at time t are calculated with the following formula.

X(t)= 00)( XdttVxt

−∫

= ( )tTTVxTtT

TtT

TTVxVx

−+−⎪⎭

⎪⎬⎫

⎪⎩

⎪⎨⎧

⎟⎟⎠

⎞⎜⎜⎝

⎛−×−⎟⎟

⎠

⎞⎜⎜⎝

⎛−×

−−

2122

22

1

21

21

12 expexp ……………(5)

Y(t)= 00)( YdttVyt

−∫

= ( )tTTVyTtT

TtT

TTVyVy

−+−⎪⎭

⎪⎬⎫

⎪⎩

⎪⎨⎧

⎟⎟⎠

⎞⎜⎜⎝

⎛−×−⎟⎟

⎠

⎞⎜⎜⎝

⎛−×

−−

2122

22

1

21

21

12 expexp ……………(6)

A4.2 Error of radius direction during arc cutting

When using a DC servo motor, a delay is produced between the input and output axes due to

the factors of the positioning system. The linear interpolation on instruction path does not cause

any error. Arc interpolation, especially the arc cutting at high speed may cause a deviation in

the direction of radius, which is determined with the following formula.

Y: Maximum radius error (mm)△

V: Feedrate (mm/sec)


68

r: Arc radius (mm)

T1: Time constant (sec) (T1 = 0) of exponential deceleration/acceleration during cutting

T2: Time constant (sec) (reciprocal of position loop gain) of positioning system

△ r = ( )r

VTT 22

22

121

×+ ……………………………………………… (1)

The radius r(mm) and permissible error △r(mm) of a workpiece are given in actual machining. Permissible speed limit V(mm/sec) can be calculated with the formula (1).

The Time constant of deceleration/acceleration during cutting set by the unit varies with machine types. Refer to the user manual supplied with the machine.


69

Appendix 5 Parameters

Display and setting procedures of parameters When the NC is connected to a servo motor or the machine, the specifications and functions of the machine shall be set to maximize the performance of the servo motor. Since its contents vary with machine types, please refer to the additional parameters of the machine. End user is not allowed to change the parameters.

A5.1 Display of parameter (a) Press the PARAMETER key.

(b) Select the desired page with the PAGE key, or N , parameter number and INPUT

A5.2 Setting of parameter Setting in MDI mode

(a) Switch the PRM.WT switch on the main unit to ENABLE (ON) to activate the warning indicator on the panel.

(b) Set the MDI mode.

(c) Press the PARAMETER key.

(d) Press the N , the parameter number to be set and INPUT. The cursor will appear underneath the number provided that the page of the parameter number to be set is selected. (This may also be done with the PAGE button and cursor ↓ or ↑ button. )

(e) Set with P , set data and INPUT.

In the event of error during typing in, press the CANCEL key.

(f) Make sure the setting is correct.

(g) After the setting of all parameters and end of confirmation, return the switch on the main PCB to DISABLE (OFF).

(h) To terminate the alarm state (No. 100), press the RESET button.

A5.3 Parameters list Parameter No.

0 0 6

ORWD: Retention parameter

SCTO 1: Perform detection of speed reaching signal during instruction and changing from quick speed to cutting feed.

0: Not perform detection of speed reaching signal.

EENB 1: Servo OFF signal is active.

0: Servo OFF signal is inactive.

OTCE 1: Stop once the travel switch of hardware is pressed.

(Mechanical position is lost)

0: Slow down and stop once the travel switch of hardware is pressed. (Mechanical position is not lost)

FMIC 1: When inputting in metric system, the unit of feedrate is 1/10.

0: Not 1/10

MDL 1: The minimum unit of the indication on the position display unit is 0.01mm or input in metric system and 0.001inch for input in inch system.

ORWD SCTO EENB OTCS FMIC MDL MIC SCW 7 6 5 4 3 2 1 0


70

0: The minimum setting unit of the indication on the position display unit is 0.001mm or input in metric system and 0.001inch for input in inch system.

MIC 1: The minimum setting unit of the indication on the position display unit is 0.01mm or input in metric system and 0.0001inch for input in inch system.

0: The minimum setting unit of the indication on the position display unit is 0.001mm or input in metric system and 0.0001inch for input in inch system.

SCW 1: The minimum travel unit is 0.0001inch (machine in inch system)

0: The minimum travel unit is 0.001mm (machine in metric system)

0 0 7

ADET 1: Perform automatic drift compensation

0: Not perform automatic drift compensation.

EOM 1: If M30 is sent to the machine side and FIN returns when M30 is instructed, it is continuously executed from the preceding block of the program, or the machine side does not send back FIN signal but external reset signal. The program returns to the beginning to enter into reset state (in automatic mode).

0: When M30 is instructed, only M30 is sent out to the machine side and the program does not return to the beginning unless reset and rewinding signal is used (in automatic mode).

CINP 1: Instruction speed reduces to 0 between two non-cutting blocks. The next block is not continued until the machine confirms that the designated position is reached (the confirmation is called positioning detection).

0 The next block is executed once the instruction speed reduces to 0 between two non-cutting blocks (not perform positioning detection).

DCS 1: The start button on the MDI panel does not pass through the machine side, but directly is switched on the NC side (only for MDI mode).

0: The start button on the MDI panel is sent to the machine side, and then the start button on the machine side returns for start.

CLER 1: The NC is brought into clearing state (see Appendix 7 for clearing state) using the RESET button, external reset signal, reset and rewinding signal.

0: The NC is brought into reset state using the RESET button, external reset signal, and reset and rewinding signal.

TVC 1: Not perform TV check in the control output section (note section)

0: Perform TV check in the control output section (note section)

PPD 1: Preset the position display unit by setting a coordinate system.

0: Not preset the position display unit during the setting of a coordinate system.

RDRN 1: Dry run is also valid for rapid feed instruction.

0: Dry run is not valid for rapid feed instruction.

0 0 8

ADFT EOM CINP DCS CLER TVC PPD RDRN

ICR GSP G44 G90 G95 G43 G00

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


71

ICR 1: When ISO code is used for output, EOB will be output by LF.

0: When ISO code is used for output, EOB will be output by LFCR CR.

GSP 1: Use a special G code.

0: Use a standard G code.

G90 1: Enter into G90 mode when in power on and clearing state.

0: Enter into G91 mode when in power on and clearing state.





G44, G43

G44 G43 Initial state

1 0 Enter into G44 mode when in power on and clearing state.



0 0 9

FIX2 1: Output the M code in a fixed cycle (fixed cycle II).

0: Not output the M code but SSP and SRV in a fixed cycle (fixed cycle II)

RWL 1: Store the outside of the travel limit 2 as a prohibited area.

0: Store the inside of the travel limit 2 as a prohibited area.

MCF 1: Output EF at the end of the positioning of G81 (axis Z does not move).

0: Output EF at the end of the positioning of G81 (axis Z moves).

FMFS 1: Output FMF signal twice in a fixed cycle.

0: Output FMF signal once in a fixed cycle.

FCUT 1: The travel of the axes X and Y in a fixed cycle uses the G codes in Group 01.

0: The travel of the axes X and Y in a fixed cycle usually uses rapid feed.

ILVL 1: Change the initial plane points with the RESET button.

0: Not change the initial plane points even using the RESET button.

EFRI 1: Output EF with a photoelectric coupler

0: Output EF with a relay.

TDRN 1: Also valid for dry run of thread cutting.

0: Invalid for dry run of thread cutting.

0 1 0

FIX2 RWL MCF FMFS FCUT ILVL EFR1 TDRN

TCW CWM SOV SLCC OFSD SOVC ISOT 7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


72

Signs for TCW, CWM and S4-digit output

TCW CWM Sign 0 0 M03 M04 are all positive. 0 1 M03 M04 are all negative. 1 0 M03 is positive while M04 is negative. 1 1 M03 is negative while M04 is positive.

SOV 1: Enable main axis adjustment.

0: Disable main axis adjustment.

TLCC 1: The change of offset in G43 and G44 modes starts to take effect from the next block.

0: The change of offset in G43 and G44 modes starts to take effect from the following H and D codes.

OFSD 1: Tool position offset (G45 to G48) uses D code.

0: Tool position offset (G45 to G48) uses H code.

SOVS 1: Spindle adjustment is clamped at 100% in tapping.

0: Spindle adjustment is not clamped at 100% even in tapping.

ISOT 1: With the storage type travel limit selection, JOG rapid feed is valid even returning to the reference point is not performed.

0: With the storage type travel limit selection, JOG rapid feed is valid unless returning to the reference point is performed.

0 1 1

DGNE 1: Enable data output in diagnosis.

0: Disable data output in diagnosis.

SETE 1: Input setting is possible when the lock key is closed.

0: Input setting is not possible when the lock key is closed.

DECI 1: Decelerate when the decelerating signal is “1” during the return to reference point.

0: Decelerate when the decelerating signal is “0” during the return to reference point.

SSPB 1: Spindle stops when the spindle stop input signal (SSP) is “o”.

0: Spindle stops when the spindle stop input signal (SSP) is “1”.

VCT 1: It is possible to specify tool compensation vector with I, J and K.

0: It is impossible to specify (general automatically calculate).

SUPM 1: Start and cancel type B in tool radius compensation C.

0: Start and cancel type A in tool radius compensation C. (See this document for type A/B.)

ADLN 1: The 4th axis is used as a linear axis.

0: The 4th axis is used as an axis of revolution.

0 1 2

ZGMX, ZGMY, ZGMZ and ZGM4 are the return-to-reference-point modes for axes X, Y and Z and the 4th axis respectively.

DGNE SETE DECI SSPB VCT SUPM ADLN

ZGM4 ZGGMZ ZGMY ZGMX ZM4 ZMZ ZMY ZMX

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


73

1: magnetic switch mode 0: grid mode

ZMX, ZMY, ZMZ and ZM4 are the return-to-reference-point directions as well as the initial directions of clearance when power on for axes X, Y and Z and the 4th axis respectively.

1: The return-to-reference-point direction as well as the initial direction of clearance is negative.

0: The return-to-reference-point direction as well as the initial direction of clearance is positive.

(Note 1) For an axis with return-to-reference-point function, the return-to-reference-point direction is identical with the initial direction of clearance. For an axis without return-to-reference-point function, the parameter only has the meaning of initial direction of clearance.

(Note 2) After power on, clearance compensation is made when moving in the direction set by this parameter.

0 1 3

PSG2, PSG The tooth to spindle ratio of spindle and position coder Override PSG2 PSG1

X1 0 0 X2 0 1 X4 1 0 X5 1 1

Override=

When in PHS and PSCG modes (rotary transformer and inductosyn), the initial setting of relative offset:

1: does not automatically set phase deviation

0: automatically sets phase deviation. PHS automatically changes to “1” after the setting is performed once.

0 1 4

0 1 5

0 1 6

PSG2 PSG1 PHS

DMR X GRD X

DMR Y GRD Y

DMR Z GRD Z

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


74

0 1 7

4 1 0

DMRX, DMRY, DMRZ, DMR4 and DMR5 are the measuring override ratio for axes X, Y, Z and the 4th axis respectively.

Overrides Setting codes Pulse coder Rotary transformer and inductosyn0 0 0 1/2 1/8 0 0 1 1 1/4 0 1 0 1 1/4 0 1 1 2 1/2 1 0 0 3/2 3/8 1 0 1 3 3/4 1 1 0 2 1/2 1 1 1 4 1

GRDX, GRDY, GRDZ, GRD4 and GRD5 are the capacities of the reference counters for axes X, Y, Z and the 4th axis respectively.

Setting codes Capacity of a cycle 0 0 0 1 2000 0 0 1 0 3000 0 0 1 1 4000 0 1 0 0 5000 0 1 0 1 6000 0 1 1 1 8000 1 0 0 1 10000

(Note) The codes other than those listed in the above table are treated as 8000 capacity.

0 1 8

Pulse frequency (holoaxial calling) for CPF2 and CPF1 clearance compensations.

(Must be set to 256KHZ)

0 1 9

TMF The time from the send-out of M, S, T and B codes to that of MF, SF, SF and TFBF: 16—126ms (16ms interval).

TFIN The time of FIN signal receiving width: 16—265ms (16ms interval).

DMR 4 GRD 4

DMR 5 GRD 5

CPF2 CPF1

Frequency, KHZ CPF2 CPF1 32 0 0 64 0 1

128 1 0 256 1 1

TMF TFIN

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0

3 2 1 0


75

T M F T F I N Setting 15m sec 32m sec 48m sec 64m sec 80m sec 96m sec 112m sec 128m sec 144m sec 160m sec 176m sec 192m sec 208m sec 224m sec 240m sec 256m sec

>15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec >15m sec

0 0 0 0 0 0 0 0 1 1 1 1 1 1 1 1

0 0 0 0 1 1 1 1 0 0 0 0 1 1 1 1

0 0 1 1 0 0 1 1 0 0 1 1 0 0 1 1

0 1 0 1 0 1 0 1 0 1 0 1 0 1 0 1

CLSI 1: Not detect servo position circuit LSI.

0: Detect servo position circuit LSI.

ZTNX, Y, Z, 4 and 5 are the availability of return-to-reference-point function for axes X, Y and Z as well as the 4th and 5th axis respectively.

1: With return-to-reference-point function

0: Without return-to-reference-point function

0 2 1

0 2 0 CLSI ZTN5 ZTN4 ZTNZ ZTNY ZTNX

G84S SFOU EDMZ EDMY EDMX EDPZ EDPY EDPX

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


76

G84S 1: When S 12-digit output A and S analog output A are used in fixed cycles G74 and G84, method B is valid.

0: When S 12-digit output A and S analog output A are used in fixed cycles G74 and G84, method A is valid (see connection guides for method A/B) .

SFOU For 12-digit outputs A and B as well as analog output A, SF setting is not output in the output without gear switching.

1: Output SF.

0: Not output SF.

EDMX, EDMY and EDMZ correspond to the negative instructions of axes X, Y and Z respectively.

1: Valid for rapid feed and external deceleration of cutting feed

0: Only valid for rapid feed.

EDPC, EDPY and EDPZ correspond to the positive instructions of axes X, Y and Z respectively.

1: Valid for rapid feed and external deceleration of cutting feed

0: Only valid for rapid feed.

0 2 2

SIJ Setting of tool returning method in fixed cycle G76 or G87

1: Set direction and amount of travel with address I and J.

0: The amount of travel uses address Q as instruction and its direction is determined by parameters PMXY1 and PMXY2

PMXY2, 1 Setting of tool returning direction in fixed cycle G76 or G87(only valid when SIJ =0)

PMXY2 PMXY1 Returning direction 0 0 ＋X 0 1 －X 1 0 ＋Y 1 1 －Y

RS43 1: The offset vectors of G43 and G44 are retained after reset.

0: The offset vectors of G43 and G44 are cleared after reset.

FXCD 1: Dwell instruction is valid in fixed cycles G74 and G84.

0: Dwell instruction is invalid in fixed cycles G74 and G84.

TAPSG 1: Output tapping signal in fixed cycles G74 and G84.

(Valid only when FLX2 = 1).

0: Not output tapping signal.

FXCS 1: M05 is not output and spindle rotates reversely or forward in fixed cycles G74 and G84 (Valid only when FIX2 = 1)

0: M05 is output and spindle rotates reversely or forward in fixed cycles G74 and G84

0 2 3

SIJ PMXY2 PMXY1 RS43 FXCD TAPSG FXCS

EXIOD

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


77

EXIOD 1: To multiply the unit of external origin offset by 10.

0: Not to multiply it by10.

0 2 4

PMC2, 1 Screw pitch error compensation override

The set compensation is output after it is multiplied by the override.

FMT 1: Perform software parity check for part program edit area.

0: Not perform the check.

When it is ready for the check, the parameter is automatically set to 1. It cannot be externally switched on or off.

PML2 PML1 Override 0 0 ×1 0 1 ×2 1 0 ×4 1 1 ×8

DLME 1: All programs stored before are automatically cleared when storing programs in

memory.

0: Not automatically clear.

RDAL 1: Generally all programs are stored when storing programs in memory.

0: When storing programs in memory, storing a program or all programs is determined by MDI operations.

ADW2, 1, 0 Select the name for the 4th axis in the even of data output or display on LCD.

ADW2 ADW1 ADW0 Address 0 0 0 A 0 0 1 B 0 1 0 C 0 1 1 U 1 0 0 V 1 0 1 W

0 2 5

MSUB 1: Subprogram type user macro terminates.

0: Macro type user

MURS 1: Use user macro look-at-me function

0: Not use.

MCYL 1: User macro terminates in cycle operations.

0: User macro does not terminate in cycle operations

(Note) The local variable for a macro terminated and called by subprogram type user macro does not change. The local variable for a macro terminated and called by macro type user macro differs from that is used in the current program.

MPRM 1: That a user macro terminates and controls M codes is set by parameter.

0: The look-at-me of a user macro is controlled by M96 and M97.

TSE 1: The look-at-me of a user macro adopts state triggering mode.

PML2 PML1 DLME RDAL ADW2 ADW1 ADW0 FMT

MUSR MCYL MSUB MPRM TSE

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


78

0: Adopt fringe triggering mode.

0 2 6

MGMP The amounts of travel of manual pulse generator are as follows.

NGMP MP2 MP1 Amounts of travel 0 0 0 0.001mm/0.0001inch 0 0 1 0.01mm/0.001inch 0 1 0 0.1mm/0.01inch 0 1 1 0.1mm/0.01inch 1 0 0 0.01mm/0.001inch 1 0 1 0.001mm/0.0001inch 1 1 0 0.1mm/0.01inch 1 1 1 0.1mm/0.01inch

OFFVY 1: Servo alarm is not given even when VRDY is ON before PRDY output.

0: Servo alarm is not given when VRDY is ON before PRDY output.

CKIM 1: Ignore the switching of signal during automatic operation (the state of during CYCLE START is valid).

0: Immediately enable machine lock signal.

(Note) Machine lock is always active in JOG mode. 1: Storage sorting is not performed during program search.

0: Storage sorting is performed during program search.

0 2 7

0 2 8

0 2 9

0 3 0

4 1 4

CMRX, CMRY, CMRZ, CMR4 and CMR5 are the instruction multiplying powers for axes X, Y and Z as well as the 4th and 5th axes respectively.

1 0.5 2 1 4 2

10 5 20 10

0 3 1

0 3 2

0 3 3

0 3 4

4 1 5

VLOCX, Y, Z, 4 and 5 are the minimum values of speed instruction for axes X, Y and Z as well as the 4th and 5th axes respectively.

NGMP OFFVY OGE CKIM

CMRX

CMRY

CMRZ

CMR4

CMR5

VLOCX

VLOCY

VLOCZ

VLOC4

VLOC5

7 6 5 4 3 2 1 0


79

0 3 5

0 3 6

MBUF1, MBUF2 Up to 2 settings between 00 and 97 may be set for the M codes without buffer.

0 3 7

SPGST The setting between 0 and 255 for the number of revolutions of spindle motor (S12 or S analog output A/B) during the shifting of spindle gear.

Setting=

0 3 8

SPSOR Number of revolutions during accurate stop of spindle (S12 or S analog output A/B)

Settings 0 to 255 Unit: rpm

0 3 9

0 4 0

0 4 1

0 4 2

4 1 6

PECZRX to 5 are the settings of pitch error origin for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to 127

Set some points corresponding to the reference point. For example, assuming that the pitch error origin is set to 0 and the set point 1 is located at +8.000mm, then the compensation range of the set point 127 at 1016.000mm is 0 mm to 1016.000mm.

MBUF1

MBUF2

SPGST

SPSOR

PECZRX

PECZRY

PECZRZ

PECZR4

PECZR5


80

This is the occasion that pitch error compensating clearance (parameters 163 to 166) is 8000.

0 4 3

0 4 4

0 4 5

0 4 6

0 4 7

0 4 8

0 4 9

0 5 0

0 5 1

0 5 2

UMMCD4 to UMMCD13 Up to 10 M codes for calling user macros can be set (assignment of independent variable is also possible).

Settings 01 to 97

0 5 3

MACINTON: The code for a user macro to terminate its active state.

Settings 03 to 97

The parameters are only valid when the parameter 025—MPRM = 1.

0 5 4

MACINTON: The code for a user macro to terminate its inactive state.

Settings 03 to 97

The parameters are only valid when the parameter 025—MPRM = 1.

0 5 7

0 5 8

0 5 9

TMHOR Display in hour: 0 to 255 (increment: 1 hr)

TMMIN Display in minute: 0 to 59 (increment: 1min) Display during machining time

UMMCD4

UMMCD5

UMMCD6

UMMCD7

UMMCD8

UMMCD9

UMMCD10

UMMCD11

UMMCD12

UMMCD13

MACINTON

MACINTOF

TMHOR (hr)

TMMIN (min)

TMSEC (sec)


81

TMSEC Display in sec: 0 to 58 (increment: 2 sec)

Machining time (when the STL indicator is lit) is displayed in hour, minute or sec by setting.

Machining time is saved in nonvolatile memory even in the event of power failure.

To preset it to zero, proceed as the setting operations for switching on (also for settings).

0 6 0

IDXUNT Minimum indexing angle of rotary workbench

Settings 1 to 255 Unit: deg(degree)

It is only valid when it is used in junction with the parameter 3/4—5(IFIX)= 1. Now P/S alarm (No. 180) will be given if the travel other than the integral multiples of IDXUNT setting is specified.

In addition, P/S alarm (No. 180) will be given if the instructed value of coordinate setting (G92), the parameter value of automatic coordinate system setting and the parameter value of workpiece origin offset are beyond the integral multiples set in IDXUNT.

0 6 1

FIND The constant of change in feedrate when the pulse generator is moved for one division by JOG under F1-digit instruction.

△ F = 100n

¡maxF (i=1.2)

Set the n in the above formula, namely the feedrate hits Fmax i when the pulse generator is rotated for n turns by JOG.

Settings 1 to 12

The Fmax i in the above formula is the upper limit of the feedrate of F1-digit instruction and is set by parameter No.065, 066.

Fmax1 Upper limit of the feedrate of F1 to F4 (065)

Fmax2 Upper limit of the feedrate of F5 to F9 (066)

0 6 2

SCTTIM The delay time setting of the spindle speed reaching signal detection; the setting of the time from the start of execution of S function to the end of spindle speed reaching signal detection.

Settings 0 to 255 Unit: msec

0 6 3

ADL5 1: The 5th axis is a linear axis.

0: The 5th axis is an axis of rotation

HIR5 1: Enable the look-at-me of the 5th axis handwheel.

IDXUNT

FIDN

SCTTIM

ZDL5 EX5NG HIRS AP5 G605 7 6 5 4 3 2 1 0


82

0: Disable the look-at-me of the 5th axis handwheel.

EX5NG 1: Enable the 5th axis neglecting signal.

0: Disable the 5th axis neglecting signal.

AP5 1: Enable the automatic coordinate system setting for the 5th axis.

0: Disable.

G605 1: The approaching direction of the single-directional positioning for the 5th axis is negative.

0: The approaching direction is positive.

0 6 4

SCLX, SCLY and SCLZ are the settings of availability of the zooming functions of axes X, Y and Z respectively.

1: Enable the zooming function.

0: Disable the zooming function.

0 6 5

0 6 6

FIDMAX1 , FIDMAX2 The upper limit of the feedrate of F1-digit instruction

FIDMAX1 The upper limit of the feedrate of F1 to F4

FIDMAX2 The upper limit of the feedrate of F5 to F9

Settings 0 to 15000 Unit: mm/min (output in metric system)

0 to 6000 Unit: 0.1 inch/min(output in inch system)

See parameter No.061 for details.

0 6 7

CYCR The setting of return in fixed cycle G73 (high-speed depth drilling cycle)

Settings : Input 0 to 32767 in metric system, unit: 0.001mm.

Input 0 to 32767 in inch system, unit 0.0001inch.

It is also to set with specified values.

0 6 8

0 6 9

CRCDL The neglecting limit of the minor amount of travel while the tool is machining on the exterior side of the turning angle near 90° during tool radius compensation.

Settings: Input 0 to 16383 in metric system, unit: 0.001mm

Input 0 to 16383 in inch system, unit: 0.0001inch

SCLZ SCLY SCLX

FIDMAX1

FIDMAX2

CYCR

CYCD

CRCDL

7 6 5 4 3 2 1 0


83

When X△ ＜CRCDL and Y△ ＜CRCDL, minor travel is neglected. In this way the influence as a result of workpiece’s stop on workpiece may be prevented.

0 7 0

0 7 1

0 7 2

0 7 3

4 2 5

INPX, INPY, INPZ, INP4 and INP5 are the positioning width settings for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to 32767 measurement units 0 7 4

0 7 5

0 7 6

0 7 7

4 2 6

STPEX, STPEY, STPEZ, STPE4 and STPE5 are position deviation limits for axes X, Y and Z as well as the 4th and 5th axes respectively.

Setting units: 0 to 32767 measurement units

0 7 8

0 7 9

0 8 0

0 8 1

4 2 7

SERRX, Y, Z, 4 and 5 are position deviation limits for axes X, Y and Z as well as the 4th and 5th axes respectively.

INPX

INPY

INPZ

INP4

INP5

STPEX

STPEY

STPEZ

STPE4

STPE5

SERRX

SERRY

SERRZ

SERR4

SERR5


84

Settings 0 to 32767measurement units

0 8 2

0 8 3

0 8 4

0 8 5

4 2 1

GRDSX, Y, Z, 4 and 5 are grid drifts for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to ±32767measurement units

The setting is a + (-) value when the reference point is the drift in the + (-) direction.

0 8 6

0 8 7

0 8 8

0 8 9

4 2 2

LPGMX, Y, Z, 4 and 5 are the settings of servo loop gain multiplier for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings = 10002048 ××× γLE

E = 7V (motor: 7V/1000rpm)

3.5V(motor: 7V/2000rpm)

L = Mechanical travel in mm or inch equivalent to one rotation of motor

γ= Measurement unit (mm or inch)

Example: Servo motor: 2mm travel each rotation, 7V/1000r/min

Measurement unit: for 1/1000mm

Setting 716810001000

1272048 =×××

The digits behind the decimal point are rounded off.

0 9 0

LPGIN The setting of loop gain for position control

Settings 1 to 9999, unit: 0.01s-1

0 9 1

JOGF The JOG feedrate when the rotary switch is set to 10.

Settings 1 to 150, unit: mm/min, deg/min (output in mm)

1 to 60, unit: 0.1inch/min, 0.1deg/min(output in inch) or 1deg/min(output in inch)

(Note) For the input in inch system, the unit for additional axis is 0.1deg/min or 1deg/min is set

GRDSX

GRDSY

GRDSZ

GRDS4

GRDS5

LPGMX

LPGMY

LPGMZ

LPGM4

LPGM5

LPGIN

JOGF


85

by parameter ROT10(No.306). Also see parameters ADNW(No.318) and JOGFAD(348)

0 9 2

0 9 3

0 9 4

0 9 5

4 2 8

RPDFX, Y, Z, 4 and 5 are the quick speeds of for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 30 to 15000 unit: mm/min (output in metric system)

30 to 6000 unit: 0.1inch (output in inch system)

0 9 6

0 9 7

0 9 8

0 9 9

4 2 9

LINTX, Y, Z, 4 and 5 are the time constant (for quick speed) of linear acceleration/deceleration for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 8 to 4000, unit: msec.

1 0 0

1 0 1

1 0 2

1 0 3

4 3 0

EXPTZ, Y, Z, 4 and 5 are exponential acceleration/deceleration time constant for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 8 to 4000 unit: m.s

1 0 5

FEEDT: The exponential acceleration/deceleration time constant for cutting feed Settings 8 to 4000, unit: m.s.

1 0 6

FEDMX The upper-limit rate of cutting feed, valid for all axes

(a) For parameter No. 318 (ADNW = 0) (type A)

It is applicable for all axes and sets a tangential speed limit, which shall not be exceeded; otherwise it is subject to clamping.

RPDFX

RPDFY

RPDFZ

RPDF4

RPDF5

LINTX

LINTZ

LINT4

LINT5

EXPTX

EXPTY

EXPTZ

EXPT4

EXPT5

FEEDT

FEDMX

LINTY


86

Settings 6 to 15000, unit: mm/min, output in deg/min metric system

6 to 6000, unit: 0.1inch/min, 0.1deg/min or 1deg/min (output in inch system)

(Note) For output in Inch, the unit for an additional axis is 0.1deg/min or 1deg/min depends on parameter ROT10 (No.306).

(b) For parameter No. 318 (ADNW = 1) (type B)

It is applicable for axes X, Y and Z. the speeds of all axes in linear interpolation and tangential speeds in arc interpolation shall not be exceeded; otherwise they will be restricted.

Settings 6 to 15000 unit: mm/min (output in metric system)

6 to 6000 unit: 0.1inch/min (output in inch system)

(See parameter No. 366 for additional axes)

1 0 7

EXDEC Speed of external deceleration (common for all axes)

Settings 6 to 15000, unit: mm/min (output in metric system)

6 to 6000, unit: 0.1inch/min( output in inch system)

1 0 8

FEDFL The lower-limit (FL) rate of exponential acceleration/deceleration for cutting feed

Settings 6 to 15000, unit: mm/min or

6 to 6000 unit 0.1inch/min

The value is generally 0.

1 0 9

1 1 0

1 1 1

1 1 2

4 3 1

JGFLX, Y, Z, 4 and 5 are lower limit (FL) of exponential acceleration/deceleration for continuous JOG feed for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 6 to 15000, unit: mm/min.

6 to 6000, unit: 0.1inch/min

1 1 3

SPDFL The lowest speed (F0) for quick adjustment (common for all axes)

Settings 6 to 15000, unit: mm/min, deg/min(output in metric system).

6 to 6000 unit: 0.1inch/min

0.1deg/min (output in inch system)

6 to 6000 unit: 1deg/min(output in inch system).

(Note) For output in inch system, the unit for an additional axis is 0.1deg/min or 1deg/min depends on parameter ROT10 (306).

1 1 4

ZRNFL Low-speed feedrate (FL) for return to the reference point (common for all axes)

EXDEC

FEDFL

JGFLX

JGFLY

JGFLZ

JGFL4

JGFL5

SPDFL

ZRNFL


87

Settings 6 to 15000, unit: mm/min, deg/min (output in metric system)

6 to 6000, unit: 0.1inch/min

0.1deg/min or 1deg/min (output in inch system).

(Note) For output in inch system, the unit for an additional axis is 0.1deg/min or 1deg/min depends on parameter ROT10 (No.306).

1 1 5

1 1 6

1 1 7

1 1 8

4 3 2

BKLX, Y, Z, 4 and 5 are lower limit (FL) of reverse clearances for axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to 255unit 0.001mm(output in metric system)

0 to 255unit 0.0001inch(output in inch system)

1 1 9

SPDLC Spindle speed offset compensation, i.e. the compensation for setting the zero offset of spindle speed instruction voltage (for S analog output A/B)

Settings 0 to ±8191unit VELO.

1 2 1

TLCNEG Tool life management negligence number

Settings 1 to 255

1 2 4

1 2 5

1 2 6

1 2 7

4 2 3

DRFTX, Y, Z, 4 and 5 are the compensation of the drift occurred inside the servo ring of axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to ±5000 unit: VELO

The value automatically changes after the parameter setting (007-ADFT) of automatic drift compensation.

1 2 8

1 2 9

1 3 0

1 3 1

BKLX

BKLY

BKLZ

BKL4

BKL5

SPDLC

TLCNEG

DRFTX

DRFTY

DRFTZ

DRFT4

DRFT5

PRAZX

PRAZY

PRAZZ

PRAZ4


88

4 2 4

PHAZX, Y, Z, 4 and 5 are the servo phase deviation of axes X, Y and Z as well as the 4th and 5th axes respectively. The value corresponding to the signal phase fed back from phase detector is automatically set (for rotary transformer and inductosyn).

Settings 0 to 500

1 3 2

GRLMAX The setting of maximum number of spindle revolutions for low-speed gear (S12-digit outputs A, for S analog output A)

The setting of number of spindle revolutions when speed instruction voltage is 10V. Settings 1 to 9999 unit: r/min

1 3 3

GRHMAX The setting of maximum number of spindle revolutions for high-speed gear (S12-digit outputs A, for S analog output A)

The setting of number of spindle revolutions when speed instruction voltage is 10V.

Settings 1 to 9999 unit r/min

1 3 4

GRHMIN The setting of lower limit of spindle revolutions for high-speed gear (S12-digit outputs A, for S analog output A)

Settings 1 to 9999 unit r/min.

(Note) It becomes a low-speed gear when a value identical with the setting is instructed.

1 3 5

SPDMIN The setting of lower limit of spindle motor output (S12-digit outputs A/B, for S analog output A/B)

Settings =

Settings 1 to 4095

1 3 6

SPDMAX The setting of upper limit of spindle motor output (S12-digit outputs A/B, for S analog output A/B)

Settings =

Settings 1 to 4095

1 4 0

PSANGN Setting of the gain calling data of S analog output A/B

Setting range: 700 to 1250

Standard setting: 1000

[Adjusting procedures]

(1) Set it to standard setting “1000”.

(2) Specify the maximum value of S analog quantity (10V).

PRAZ5

GRLMAX

GRHMAX

GRHMIN

SPDMIN

SPDMAX

PSANGN


89

(3) Measure the output voltage.

(4) Set PSANGN according to the following formula.

(5) Set the parameter and then instruct the maximum (10V) confirming output voltage of S

analog quantity as 10V.

1 4 1

TIME1 Set the preset quantity of service time.

It is also possible to preset with setting.

Settings 0 to 32767 unit: 0.1hr

1 4 2

TIME2 Set the preset quantity of service time.

Settings 0 to 99999999 unit: 0.1hr

1 4 3

1 4 4

1 4 5

1 4 6

4 3 3

1 4 7

1 4 8

1 4 9

1 5 0

4 3 4

1 5 1

1 5 2

1 5 3

1 5 5

1 5 6

1 5 7

TIME1

TIME2

LT1X1

LT1Y1

LT1Z1

LT141

LTI51

LT1X2

LT1Y2

LTIZ2

LT142

LT152

LT2X1

LT2Y1

LT2Z1

LT2X2

LT2Y2

LT2Z2


90

LT □ □ □

Indicate the No. n acme in the quadrangular area.

Indicate an axis (4 for the 4th axis and 5 for the 5th ) 1 No. n travel limit

Set the above travel limit. 2

Settings 0 to ±99999999 unit: 0.001mm (output in metric system)

0 to ±99999999 unit: 0.0001inch(output in inch system)

151 to 157 can also be set with setting values.

1 5 9

1 6 0

1 6 1

1 6 2

4 3 5

REF2X, Y, Z, 4 and 5 are the distance from the 2nd reference points to the 1st one of axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to ±99999999, unit: 0.001mm(output in metric system).

0 to ±99999999, unit: 0.0001inch(output in inch system).

0 to ±99999999, unit: 0.001°(axis of rotation).

1 6 3

1 6 4

1 6 5

1 6 6

4 3 6

PECINTX to 5 are the settings of pitch error compensation spacing of axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 8000 to 20000000, unit: 0.001mm (output in metric system).

4000 to 20000000, unit: 0.0001inch (output in inch system).

6000 Unit: 0.001°(axis of rotation)

(Note) The setting to 0 does not compensate.

1 6 7

ATCLZV The setting of travel limit of axis Z in negative direction

Settings 0 to ±99999999, unit: 0.001mm (output in metric system).

0 to ±99999999, unit: 0.0001inch (output in inch system).

1 6 8

MASKA Store a password before using key lock for a program.

REF2X

REF2Y

REF2Z

REF24

REF25

PECINTX

PECINTY

PECINTZ

PECINT4

PECINT5

ATCLZV

Password


91

Settings 1 to 99999999

1 7 1

1 7 2

1 7 3

1 7 4

1 7 5

1 7 6

1 7 7

1 7 8

1 7 9

FIDF1, 2, 3, 4, 5, 6, 7, 8 and 9 are the feedrates corresponding to F1 instructions F1 to F9.

Settings 0 to 15000 unit: 0.1mm/min (output in metric system).

0 to 6000, unit: 0.01inch/min (output in inch system).

The setting with set values is also possible.

In addition: For F1 instructions, the parameter value changes when feedrate is changed with a manual pulse generator. 3 0 5

G60X, Y, Z and 4 are the approaching directions of the single-directional positioning of axes X, Y and Z and the 4th axis.

1. Approaching direction is negative.

0. Approaching direction is positive.

For FLX, Y, Z, 4, NC/TC, whether the axes X, Y and Z and the 4th axis are parallel to the 5th axis (NC/TC)

1. parallel

0. not parallel

3 0 6

SKPF 1. For skip instruction (G31), the feedrate becomes the FL speed (No.342) set by parameter.

0. For skip instruction (031), feedrate is specified by F code.

FIDF1

FIDF2

FIDF3

FIDF4

FIDF5

FIDF6

FIDF7

FIDF8

FIDF9

FL4 FLZ FLY FLX G604 G60Z G60Y G60X

SKPF CHR SFRV NEOP ROT10 TMCR SALM

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


92

CHR 1. For the look-at-me function of handwheel, the feedrate is limited to quick speed.

0. Not limited to quick speed.

SFRV 1. In G84 and G74, SRV can be used to change the polarity of analog voltage.

0. Cannot change

(Note) The parameter is valid only when the parameter NO.010 Bit7 TCW is “1”.

NEOP 1. When storing programs in memory, M02, M30 and M99 are not used for the end of program.

0. May be used for the end of program.

ROT10 1. For output in inch system, the unit of feedrate parameters(No.091, 106, 113 and 114) is 1deg/min.

0. The unit is 0.1deg/min.

(The parameter is valid only when the additional axis is an axis of rotation.)

TMCR 0. T code cannot be used for calling

1. T code is used for calling a user macro.

SALM 1. Alarm is given when the S code instructed in S4 binary 12-digit output A/analog output A goes beyond the lower limit or upper limit of the value output to the spindle.

0. No give any alarm but be restrained to the lower limit or upper limit.

Refer to parameters No.135 and 136.

3 0 7

EX4NG 1. Additional-axis neglecting signal 4NG is valid.

0. Additional-axis neglecting signal 4NG is invalid.

Whether SFOB outputs SF in S12-digit output B or S analogy output B:

1. Not output SF.

0. Output SF.

SCDB 1. The last 2 digits of S4-digit is output to B21 through B38 for S12-digit output B or analogy output B. If B3-digit function is required, the digit can not be set to 1.

0. Not output

GRSR 1. All executive data in all groups are cleared during the input of tool change reset signal.

0. Only the executive data that tool life times out are cleared during the input of tool change reset signal.

TLCD 1. Tool length compensation is added to an instructed axis.

0. Tool length compensation is usually added to axis Z.

3 0 8

DIOM 1. It is possible to read and write DI and DO using macro variables.

0. Impossible.

MSFT 1. If user macro selection is provided, SHIFT key is active when typing in through MDI.

0. SHIFT key is active when typing in through MDI.

LGCM 1. The number of rotations for switching between low-speed and high-speed gears depends on the value of parameter SPDMXL(NO·365) (type A).

EX4NG SFOB SCDB GRST TLCD

DIOM MSFT LGCM RSTB CFMF

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


93

0. The number of rotations for switching is the maximum value at low speed (type A).

Note: The parameter is valid for S12-digit output A and S analog output A.

RSTB 1. In-reset signal is not output when the system is reset by with emergency stop,


94

external reset, reset and rewinding.

0. Output in-reset signal.

CFMF 1. For G84 and G74 in the fixed cycle II, output signal FMF is switched OFF by the FIN of M05.

0. For G84 and G74 in the fixed cycle II, output signal FMF is output until R-point plane.

3 0 9

TLCK 1. Input group number during tool skip.

0. Not input group number.

GST1, GST2 GST2 GST1 Group No.

0 0 1 to 16 0 1 1 to 32 1 0 1 to 64 1 1 1 to 128

LCTM 1. Specify tool life in time.

0. Specify tool life in number of cycles.

APX, Y, Z and 4 are the settings of availability of automatic coordinate setting of axes X, Y and Z and the 4th axis respectively.

1. Enable automatic coordinate setting

0. Disable.

See parameters No.375 ～ 382.

3 1 0

3 1 1

3 1 2

3 1 3

When NFED1, 2, 3 and 4 use I/Os 1, 2, 3 and 4 respectively, whether the blank space between the first and last guide holes and program is output or not:

1. Not output guide space

0. Output. RSCB1, 2, 3, 4 When RSCB 1, 2, 3 and 4 use I/Os 1, 2, 3 and 4 respectively, whether the control codes (DC1 to DC4) are used or not:

1. Not use the control codes.

0. Use the control codes.

TLSK GST2 GST1 LCTM AP4 APZ APY APX

NFED1 RSCR1 STP21 RAD1




7 6 5 4 3 2 1 0


95

When STP21, 2, 3 and 4 use I/Os 1, 2, 3 and 4 respectively, the number of stop bit(s) is set to 2 or 1:

1. 2 stop bits

0. 1 stop bit

RAD1, 2, 3 and 4 are the baud rate settings for I/Os 1, 2, 3 and 4.

(Note) If ROBOT interface selection is provided, the baud rate for the data transmission between NC and ROBOT is set to BAD4.

Baud rate RAD1, 2, 3, 4 50 0 0 0 0 100 0 0 0 1 110 0 0 1 0 150 0 0 1 1 200 0 1 0 0 300 0 1 0 1 600 0 1 1 0

1200 0 1 1 1 2400 1 0 0 0 4800 1 0 0 1 9600 1 0 1 0

(Note) See parameters No.340 and 341.

3 1 4

IM15 1. For the instructions for axis B, its rotating direction is positive despite that G90/G91 mode must be regarded as an absolute instruction.

In addition: M15 is instructed to rotate in negative direction.

0. The instruction for axis B is an absolute/incremental instruction depending on G90/G91 and its rotating direction is positive or negative. M15 has no special meaning.

MINT 1. Start to execute interrupt program (user macro interrupt type II) at the end of the execution of the current block.

0. Immediately execute the interrupt program (user macro interrupt type I)

IFIX 1. Give P/S alarm for the instructions other than integral multiple of the indexing angle of

indexing workbench (parameter No.060 shall be also be set).

0. The instructions for axis B may instruct the instructions independent of the minimum angle of the indexing workbench.

IRND 1. It is possible to round the absolute coordinates of axis B to 360.

0. It is impossible to round them to 360.

HX, Y, Z and 4 are the setting of interrupts of the handwheels of axes X, Y and Z as well as the 4th axis.

1. Enable.

IM15 MINT IFIX IRND H4 HZ HY HX 7 6 5 4 3 2 1 0


96

0. Disable.

3 1 5

PRT 1. Leading zero outputs nothing while DPRNT instruction is used for data input.

0. Leading zero outputs blank spaces while DPRNT instruction is used for data input.

SLOW 1. The parameter setting of the clamping value for the minimum number of spindle rotations in the constant control of surface speed is applicable for all gears. (No. 347)

0. Set for all gears respectively (No. 343, 344, 345 and 346)

BDEG 1. Input unit: 0. 001°(B1=0．001°).

0. Input unit of axis B: 1°(B1=1°).

IDXB 1. Indexing sequence B of indexing workbench.

0. Indexing sequence A of indexing workbench.

SSCR 1. In the blocks of rapid feed, surface speed is calculated in accordance with the coordinates of the end point of the current block.

0. In the blocks of rapid feed, surface speed is calculated in accordance with the actual position of the tool.

SSCA2, SSCA1 and SSCA0 are settings for the axis as the calculation basis in the constant control of surface speed.

SSCA2 SSCA1 SSCA0 Axis 0 0 0 X 0 0 1 Y 0 1 0 Z 0 1 1 4 1 0 0 5

3 1 6

CDSCG 1. Not perform frequency detection of DSCG feedback (rotary transformer and

inductosyn).

0. Perform detection

(The parameter is always preset to 0 after original adjustment.)

ACMR 1. It is possible to make special CMR setting (disabled).

0. It is impossible to set special CMR.

DSCGX, Y, Z, 4 and 5 are the position detection system type settings of axes X, Y and Z as well as the 4th and 5th axes respectively.

1. Position detection system is a rotary transformer or inductosyn.

0. Position detection system is a pulse coder.

(Note) Combination of pulse coder and rotary transformer or inductosyn in axes X, Y and Z is not allowed. The mixture of the 4th and 5th axes is also not allowed.

3 1 7

UM#1 to 8 For EIA code, store and use the codes corresponding to “#” used in macro.

Example: UM#8 to UM#1=01001001

PRT BLOW BDEG IDXB SSCR SSCA2 SSCA1 SSCA0

CDSCG ACMR DSCG5 DSCG4 DSCGZ DSCGY DSCGX

UM#8 UM#7 UM#6 UM#5 UM#4 UM#3 UM#2 UM#1

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


97

The codes with holes on passage 1, 4 and 7 are regarded as the “#” of EIA. The used address codes cannot be set.

UM#8 to UM#1=00000000 indicates that “#” will not be used.

3 1 8

PRG9 1. The programs of numbers 9000 to 9899 cannot be edited.

0. The programs of numbers 9000 to 9899 can be edited.

MSC9 1. When executing the programs of numbers 9000 to 9899, single block stops while executing a macroinstruction in user macro if it is single block mode.

0. Not execute.

MPD9 1. The contents of program are not displayed when executing the programs of numbers 9000 to 9899.

0. The contents of program are displayed when executing the programs of numbers 9000 to 9899.

MSRH 1. “OP” signal is not output during sequence number search.

0. “OP” signal is output during sequence number search.

RSTL 1. STL signal is not output when using CYCLE START to store messages in memory in EDIT mode.

0. STL signal is output.

ADNW 1. Feedrate is of type B.

0. Feedrate is of type A.

[Type B]

(1) JOG feedrate

The JOG feedrate of additional axis (axis of rotation) is set by parameter No.348. When the additional axis is interlocked with another axis or it is a linear axis (for parameter No. 11 BIT0 ANLN=1), however, the JOG feedrate of the additional axis is identical with other axes (parameter No. 091 JOGF).

(2) Upper-limit rate of cutting feed

When instructing linear interpolation (G01), the value that speeds of all axes exceed parameter setting by is clamped.

The clamped value is set for axes X, Y and Z and additional axis individually. For arc interpolation, the value that tangential speed exceeds parameter setting by is clamped.

[Type A]

(1) JOG feedrate

The feedrate of additional axis is set along with other axes in parameter No.091.

(2) Upper-limit rate of cutting feed

That the tangential speeds of all axes exceed parameter value is limited by parameter.

3 1 9

It is also possible to set with set values.

PRG8 1. It is impossible to edit the programs of program numbers 8000 to 8999

0. Possible

MCS8 1. If the programs of program numbers 8000 to 8999 are executed in SINGLE

PRG9 MSC9 MPD9 NSRH RSTL ADNW

PRG8 MCS8 MPD8 MCS7

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


98

mode, the execution of the macroinstruction of a user macro stops at a single block.

0. Not stop at a single block.

MPD8 1. The contents of program is not displayed when executing the programs of program numbers 8000 to 8999.

0. The contents of program is displayed

MCS7 1. If the programs of program numbers 0001 to 1999 are executed in SINGLE

mode, the execution of macro stops at a single block.

0. Not stop at a single block.

3 2 0

3 2 1

3 2 2

UMMCD 1, 2, 3 Up to 3 M codes for calling user macro are set.

Settings 01 to 91.

(User macro cannot be called with M00. The setting of 00 is equivalent to no setting.)

3 2 3

3 2 4

3 2 5

3 2 6

3 2 7

3 2 8

3 2 9

3 3 0

3 3 1

3 3 2

UMGCD0．1……9 Up to 10 G codes for calling user macro are set.

Settings 001 to 255.

(User macro cannot be called with G00. The setting of 00 is equivalent to no setting.)

3 3 3

AOVMDR The minimum reduction ratio of interior arc cutting rate Range: 1 to 100%, standard setting: 1 3 3 4

AOVOR The minimum reduction ratio of automatic adjustment for interior turning angle section

Range: 1 to 100%, standard setting: 50

UMMCD1

UMMCD2

UMMCD3

UMGCD0

UMGCD1

UMGCD2

UMGCD3

UMGCD4

UMGCD5

UMGCD6

UMGCD7

UMGCD8

UMGCD9

AOVMDR

AOVOR


99

Set the adjusting value of inner turning angle.

3 3 5

AOVTH Interior reference angle for automatic adjustment for interior turning angle.

Range: 1 to 179°, standard setting: 91°

3 3 6

3 3 7

3 3 8

3 3 9

POSTN X, Y, Z, 4 and 5 are the approaching amount of negative positioning of axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to 255; unit: 0.01mm (output in mm).

0 to 255; unit: 0.001 inch (output in inch).

3 4 0

3 4 1

IDVICE: Select an input device (INPUT DEVICE2=1(RS232) interface for setting; this setting is valid) for storing programs in memory.

ODVICE: Select an output device for data output.

Settings I/O 0 Paper tape reader for input and FACIT and PUNCHER for output

1 ASR33/ASR43 is used to set baud rate and other data (No.310) for both input and output.

2 Reader/puncher interface for I/O. Set baud rate and other data in parameter No.311.



3 4 2

PSKPFL FL speed of skipping cutting (common for all axes)

Settings 6 to 150000 unit: 1mm/min (output in metric system).

6 to 6000 unit: 0.1 inch/min (output in inch system).

3 4 3

3 4 4

3 4 5

3 4 6

GRMIN1 to GRMIN4 Minimum number of spindle revolutions in surface speed constant control (G96) mode

AOVTR

POSTNX

POSTNY

POSTNZ

POSTN4

POSTN5 4 1 7

IDVICE

ODVICE

PSKPFL

GRMIN1

GRMIN2

GRMIN3

GRMIN4


100

Settings 0 to 9999 Unit: RPM.

Valid only when parameter No. 3/5 - SLOW=0

3 4 7

LOWSP Minimum number of spindle revolutions in surface speed constant control (G96) mode (for constant control selection)

Settings 0 to 9999 unit RPM

Valid only when parameter No. 315 - SLOW=1

3 4 8

The JOG feedrate when the rotary switch is set to 10 with the existence of an additional axis (axis of rotation) (type B).

Settings 1 to 150 unit: deg/min

See parameter No.091 (JOGF)

(Note) Refer to parameter No.318 ADNW for type B.

3 5 5

AOVLE The decelerating distance Le at the end point of the automatic adjustment of interior turning angle section

Range: 0 to 3999 unit: 0.1mm(input in metric system).

Unit 0.01 inch(input in inch system).

The parameter may be operated and set with set values.

3 5 6

AOVLS The decelerating distance Ls at the end point of the automatic adjustment of interior

turning angle section

Range 0 to 3999; unit: 0.1mm (input in metric system).

Unit: 0.01 inch (input in inch system).

The parameter may be operated and set with set values.

3 5 7

3 5 8

3 5 9

3 6 0

4 4 2

EXOFS X, Y, Z, 4 and 5 are external workpiece origin offset of axes X, Y and Z as well as the 4th and 5th axes.

Settings 0 to ±7999 unit: 0.001mm (input in metric system).

0 to ±7999 unit: 0.0001 inch(input in inch system).

Typically the parameter is automatically set by the input on the machine side.

(External data input function).

3 6 1

LOWSP

JOGFAD

AOVLE

AOVLS

EXOFSX

EXOFSY

EXOFSZ

EXOFS4

EXOF5

PGMAX1


101

3 6 2

3 6 3

3 6 4

PGMAX1, 2, 3 and 4 select the maximum set numbers of rotations of gears 1, 2, 3 and 4 (For S12-digit output B and S analog output B).

Set the number of spindle rotations at 10V speed instruction voltage.

Settings 1 to 9999rpm.

3 6 5

SPDMXL Settings =


Valid only when parameter NO. 308－5 LGCM =1

3 6 6

FEDMXAD Upper-limit rate of the cutting feed of additional axis

Valid only when parameter No.318 (ADNW=1)

Settings 6 to 15000; unit deg/min (axis of rotation)

6 to 15000; unit: mm/min (output in metric system)

6 to 6000; unit: inch/min (output in inch system)

3 6 7

3 6 8

3 6 9

3 7 0

4 3 8

REF3X, Y, Z, 4 and 5 are the distances from the 3rd reference point to the 1st reference point of axes X, Y and Z as well as the 4th and 5th axes respectively.


0 to ±99999999 unit: 0.0001inch (output in inch system)

3 7 1

3 7 2

3 7 3

3 7 4

PGMAX2

PGMAX3

PGMAX4

SPDMXL

FEDMXAD

REF3X

REF3Y

REF3Z

REF34

REF35

REF4X

REF4Y

REF4Z

REF44

REF45


102

4 3 9

REF4X, Y, Z, 4 and 5 are the distances from the 4th reference point to the 1st reference point of axes X, Y and Z as well as the 4th and 5th axes respectively.


0 to ±99999999 unit: 0.0001inch (output in inch system)

3 7 5

3 7 6

3 7 7

3 7 8

4 4 0

PPRTMX, Y, Z, 4 and 5 are settings of automatic coordinate system input in metric system of axes X, Y and Z as well as the 4th and 5th axes respectively. The distance from the origin of coordinate system to the first reference point is set in metric system.

Settings 0 to 99999999 unit: 0.001mm

If Inch/metric switching option is provided, parameter No.379 to 382 and 411 shall also be set.

It is only valid for the axes that are set active in the automatic coordinate system set in parameter No.309.

3 7 9

3 8 0

3 8 1

3 8 2

4 4 1

PPRTIX, Y, Z, 4 and 5 are settings of automatic coordinate system input in inch system of axes X, Y and Z as well as the 4th and 5th axes respectively.

The distance from the origin of coordinate system to the first reference point is set in inch system.

When settings 0 to 99999999 (unit 0. 0001inch) are provided with Inch/metric switching option, parameters No. 375 to 378 and 440 shall be set. This is only valid for the axes that are set active in the automatic coordinate system set in parameter No.309.

3 8 3

3 8 4

3 8 5

3 8 6

4 4 3

ZOFSIX, Y, Z, 4 and 5 are the first workpiece origin offsets (G54) of axes X, Y and Z as well as the 4th and 5th axes respectively.

PPRTMX

PPRTMY

PPRTMZ

PPRTM4

PPRTM5

PPRTIX

PPRTIY

PPRTIZ

PPRTI4

PPRTI5

ZOFSIX

ZOFSIY

ZOFSIZ

ZOFSI4

ZOFSI5


103

Settings 0 to 99999999 unit: 0.001mm (input in metric system)

0 to 99999999 unit: 0.0001inch (input in inch system)

The OST function key is usually selected for input.

3 8 7

3 8 8

3 8 9

3 9 0

4 4 4

ZOFS2X, Y, Z, 4 and 5 are the 2nd workpiece origin offsets (G55) of axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to 99999999 unit: 0.001mm(input in metric system)

0 to 99999999 unit: 0.000inch(input in inch system)


3 9 1

3 9 2

3 9 3

3 9 4

4 4 5

ZOFS3X, Y, Z, 4 and 5 are the 3rd workpiece origin offsets (G56) of axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to 99999999 unit 0. 001mm(input in metric system).

0 to 99999999 unit 0. 0001inch(input in inch system).


3 9 5

3 9 6

3 9 7

3 9 8

4 4 6

ZOFS4X, Y, Z, 4 and 5 are the 4th workpiece origin offsets (G57) of axes X, Y and Z as well as the 4th and 5th axes respectively.

Settings 0 to 99999999 unit 0.001mm (input in metric system).

0 to 99999999 unit 0.0001inch(input in inch system).


3 9 9

ZOFS2 X

ZOFS2 Y

ZOFS2 Z

ZOFS2 4

ZOFS2 5

ZOFS3 X

ZOFS3 Y

ZOFS3 Z

ZOFS3 4

ZOFS3 5

ZOFS4 X

ZOFS4 Y

ZOFS4 Z

ZOFS4 4

ZOFS4 5

ZOFS5 X


104

4 0 0

4 0 1

4 0 2

4 4 7





4 0 3

4 0 4

4 0 5

4 0 6

4 4 8





4 0 7

SCRATE Scaling rate

Settings: 0 to 99999999; unit: 0.001 time.

It is a value whose P has not been instructed in the blocks of G51.

4 0 8

Typing will not be locked when a value identical with that of No.168 is input. It is locked in the event of input of different values.

4 1 1

ZGM5 The return-to-reference point mode of the 5th axis

1. Magnetic switch mode

0. Grid mode

ZM5 1. The returning direction to reference point and the initial direction of clearance of the 5th axis are negative.

0. The returning direction to reference point and the initial direction of clearance of the 5th axis are positive.

4 1 2

ZOFS5 Y

ZOFS5 Z

ZOFS5 4

ZOFS5 5

ZOFS6 X

ZOFS6 Y

ZOFS6 Z

ZOFS6 4

ZOFS6 5

SCRATE

LOCK/UNLOCK

ZGM5 ZM5

ADW52 ADW51 ADW50 AD5B AD5A AD4B AD4A

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


105

The name selection of the 5th axis when ADW52, 1 and 0 have the 5th axis.

ADW52 ADW51 ADW50 Letter 0 0 0 A 0 0 1 B 0 1 0 C 0 1 1 U 1 0 0 V 1 0 1 W

AD4A, AD4B, AD5A, AD5B Setting of which axis the 4th and 5th axes parallel

The 5th axis The 4th axis AD5B AD5A AD4B AD4A

The basic axis that parallels the 4th and 5th axes

0 0 0 0 Axis X 0 1 0 1 Axis Y 1 0 1 0 Axis Z 1 1 1 1 Which axis it does not parallel

4 1 3

CLCL 1. Local coordinate system is cleared after the JOG return to reference point

0. Not cleared.

WNSAA 1. External workpiece number search function is used to search the programs of a program number whose first digits are 00 and last two digits are identical with the search number.

0. External workpiece number search function is used to search the programs of a program number whose last two digits are identical with the search number.

6 3 3

ROTR 1. The R value of angle instruction is absolute or incremental depends on G90/G91 mode.

0. The R value of angle instruction is absolute.

7 1 6

(The set value may also be set).

RTANGL The angle that the coordinate system rotates by

Settings: 0 to 360000; unit: 0. 001deg.

The value is valid when it is not specified in the blocks of G68.

Setting of pitch error compensation of axis X

Settings 0 to ±7

Setting of pitch error compensation of axis Y

Settings 0 to ±7

Setting of pitch error compensation of axis Z

CLCL WNSAA

ROTR

RTANGL

1 0 0 0

1 1 2 7

2 0 0 0

2 1 2 7

3 0 0 0

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0

7 6 5 4 3 2 1 0


106

Settings 0 to ±7

Setting of pitch error compensation of the 4th axis

Settings 0 to ±7 Setting of pitch error compensation of the 5th axis

Settings 0 to ±7

3 1 2 7

4 0 0 0

4 1 2 7

5 0 0 0

5 1 2 7


107

The items set and displayed using set values.

Data No. Item

000 The settings related to I/O (DNC, RMT, INCH, ISO, TVON, REV4, REVY and REVX)

057* Machining time (unit: hr) (TMHOR) 058* Machining time (unit: min) (TMMIN) 059* Machining time (unit: sec) (TMSEC) 067* The returning amount in fixed cycle G83 (high-speed depth drilling cycle) (CYCR) 068* The cutting origin in fixed cycle G83 (high-speed depth drilling cycle) (CYCD) 141* Machining time (TIME1) 151* Storage type travel limit 2, X value of the 1st acme 152* Storage type travel limit 2, Y value of the 1st acme 153* Storage type travel limit 2, Z value of the 1st acme 155* Storage type travel limit 2, X value of the 2nd acme 156* Storage type travel limit 2, Y value of the 2nd acme 157* Storage type travel limit 2, Z value of the 2nd acme 180* The program number of the program whose execution is stopped 319* All settings (PRG8 and MSBL). 340* Select an input device for data storage (IDVICE) 341* Select an output device for data output (ODVICE)

355* The decelerating distance at the end point of a block (automatic adjustment of turning angle)

356* The decelerating distance at the starting point of a block (automatic adjustment of turning angle)

407* Scaling factor

Select address SET.

The data numbers other than other listed in the table above are displayed as blank.

The data number with a “*” can be set with address PARAM in the same data number.

See the parameter explanations regarding the same data numbers for the contents.


108

Appendix 6 Alarms List

No. Descriptions Remarks

000 N O power supply must be disconnected once and reconnected after parameter setting (parameter No. 012 to 018, 027 to 034, 082 to 090 and 124 to 131, 316).

001 TH alarm (A character with incorrect parity is input in valid information area)

002 TV alarm (the number of characters in a block is odd). ON is possible only when TV detection is set.

003 A data with impermissible number of digits is input (see the item of “Maximum instruction value”)

004 Numeral, character (-) or decimal point is entered without address at the beginning of a block (refer to the descriptions for P/S alarm in the items III, 10 and 11 when it is provided with user macro option).

005 There is not data but address or EOB code following an address.

006 Sign “-“ is input incorrectly (“-“ is entered behind an address that allows no negative sign, or two or more “-“ signs are entered.)

007 Decimal point is entered incorrectly (“·“ is entered behind an address that allows no negative sign, or two or more “·“symbols are entered.)

008 Device setting is entered incorrectly.

009 A prohibited character is entered in the valid information area. (E)

010 A prohibited G code is used (the alarm is also given when an instruction similar to the unselected G code is instructed).

011 Feedrate is not instructed or instructed improperly during cutting feed.

014 Synchronous feed is instructed when thread cutting/synchronous feed option is not provided.

015 Permissible number of concurrently controllable axes is exceeded.

017 The move instruction of additional axis is instructed without additional control option.

018 Concurrent motion of additional axis and other axes is instructed without additional control select function for additional axis.

021 An axis beyond plane assignments (G17, G18 and G19) is instructed in arc instruction.

022 3R is instructed without radius R instruction option in arc instruction.

023 R is instructed as 0 or negative when radius R instruction is used in arc instruction.


109

027 For an axis, tool length compensation is applied without cancellation of the foregoing tool length compensation.

028 An instruction of more than 2 axes is instructed for the axis in the same direction in an arc instruction.

029 Compensation is modified when the stored offset is of more than 6 digits.

030 The compensation number instructed with the D and H codes for tool radius compensation, tool length compensation and tool position compensation is excessive.

031 The P value of an instructed offset number is excessive or P is not instructed in the input of offset (using G10 or user macro input command).

032 The offset instructed by P is excessive in the input of offset (using G10 or user macro input command).

033 Intersection point cannot be determined using the intersection-point method of calculation for tool radius compensation C, or intersection point calculation of a turning angle less than 90° is instructed in tool radius compensation B.

034 Compensation “start” or “cancel” is executed in G02/03 mode during tool radius compensation.

035 Skipping cutting (G31) is instructed in tool radius compensation.

036 G45 to G48 (tool offset) are instructed in tool radius compensation.

037 Switching between compensation planes (G17, G18 and G19) is conducted in tool radius compensation.

038 Overcutting is caused as the radius of arc is 0 at its origin and end point in tool radius compensation.

041 Overcutting is caused in tool radius compensation.

044 G27 through G30 and ATC cycle (M06) are instructed in fixed cycle mode.

045 ATC cycle (M06) is instructed in a device without return-to-reference-point selection function.

046 An instruction other than P2, P3 and P4 is instructed in the 2nd, 3rd and 4th return-to-reference-point instructions.

047 G27 to G30 are instructed for an axis without reference point.

048 G30 is instructed without returning to reference point after switching on or emergency stop. When a storage type travel limit option is provided, a move instruction is executed without returning to reference point after switching on or emergency stop.

058 An instruction beyond the maximum or minimum number of spindle rotations is instructed in S4-digit binary 12-bit/analog output A.

059 The block of the selected workpiece number is not found (external workpiece number selection A function).

060 The specified sequence number is not found during sequence number search or restart of program.

065 A value of a scaling rate beyond 1 to 99999 is instructed.

066 After the application of scaling, traveling amount, coordinates and arc radius exceed the maximum instruction value.


110

067 G51 (scaling ON) is instructed in tool radius compensation.

070 The capacity of memory is inadequate.

071 The address searched is not found.

072 The number of stored programs exceeds 95 or 191.

073 A stored program number is used.

074 The program number is beyond 1 to 9999.

075 Neither program number nor sequence number is entered in the first paragraph of the program.

076 Address P is not instructed in the blocks containing M98, G65 and G66.

077 A subprogram is called for 3 times (or 5 times with a user macro option).

078 The program number (the program number instructed when G, M and T calling are used) specified by address P, sequence number or serial number specified by GOTO statement is not found in the blocks containing M98, M99, G65 and G66.

079 A communicated program is not identical with the original one (program comparison).

084 Program edit is impossible as a result of improperly instructed origin, end point or travel end point in expanded edit function.

085 The number of bits or baud rate of input data is not correct during reading in with RS232 and DNC connectors.

086 Transmission or I/O device is abnormal during input and output with RS232 connector.

087 A data with more than 10 characters is input after sending DC3 stop code when RS232 and DNC connectors are used for reading in.

090 The one-revolution signal from pulse coder (basic origin signal for linear graduation) is not input or reference point is not correctly returned to during the return to reference point in grid mode.

091 The one-revolution signal from pulse coder (basic origin signal for linear graduation) is not in step with basic counter and reference point is not correctly returned to during the return to reference point in grid mode.

092 The axes instructed by G27 cannot return to reference point.

094 The restart of program cannot instruct type P (because coordinate system setting, clearing and other operations are performed after program interrupt).

095 The restart of program cannot instruct type P (because external workpiece origin offset is changed after program interrupt).

096 The restart of program cannot instruct type P (because workpiece origin offset is changed after program interrupt).

097 The restart of program cannot instruct type P (because automatic operation has been never performed after power on or emergency stop and termination of storage limit alarm (emergency stop)).


111

098 Reference point is not returned to after switching on or emergency stop and termination of storage type limit alarm (instant stop) and G28 is found in program search using program restart instruction.

099 Move instruction in MDI mode is executed after the end of the search using program restart.

100 The RESET button is pressed for reset by switching the parameter writing switch from ON to OFF.

101 Power is disconnected when storing and editing a part program or rewriting the memory. In the event of alarm, the memory is completely cleared by concurrently pressing the DELETE and RESET buttons to switch on the power.

102 Power is disconnected when writing in data of tool life management.

110 The absolute value of data indicated by fixed point goes beyond the allowable range.

111 The data displayed by floating point goes beyond the upper limit.

112 The divisor is 0.

113 A function that cannot be used for macro A is used.

114 A format other than FOMAT is incorrect.

115 A value that cannot be defined by variable is instructed.

116 The left of the assignment statement is a prohibited variable.

118 The number of layers of brackets goes beyond the upper limit (5).

119 The independent of SQRT or BCD is negative, or a numeral other than 0 to 9 serves as a digit.

122 The number of calling layers of macro goes beyond the permissible range (1-4).

123 Macro control instruction is used in DNC mode.

124 DO－END do not correspond one to one.

125 The format of (FORMUCA) is incorrect.

126 In DON, the value of N does not fall within 1≤N≤3.

127 NC instructions are mixed with macro instructions.

128 In GOTON, the value of N does not fall within 0≤N≤9999.

129 A prohibited address is used in (independent variable assignment).

130 The data of a big address is incorrect during the input of external data.

131 5 or more alarm numbers appear in the external alarm information area.

132 There is no corresponding alarm number in the clearance of external alarm information.

133 The data of a minor address is external alarm information and external operating information.

134 The rotary plane of coordinate system or the plane of arc or tool radius compensation C is incorrect.

140 Tool group number goes beyond the upper limit (one of 16, 32, 64 and128).


112

141 The tool group number instructed in machining program is not set.

142 The number of tools in a group goes beyond the upper limit of storable number.

143 T code is not stored in the block for setting tool group.

144 H99 or D99 is specified when the tool in group is not used.

145 The T code following M06 in program execution does not match the relevant T code in tool group in service.

146 There is not P and L instructions at the beginning of the program for setting tool group.

147 The set number of tool groups goes beyond the upper limit.

148 The values of parameter No.333, 334 and 335 are beyond the setting range.

160 An executing program is edited or a program to be edited is not selected. Sequence number is searched before edit.

170 The programs of program number 8000 to 8999 and 9000 to 9899 are edited. However, these programs are prohibited from edit, resulting in the alarm (see parameters No.318 for PRG9 and 319 for PRG8)

180 A value below the decimal point is specified when a decimal point is used in B-axis instruction and a value beyond the integral multiple of the minimum indexing angle of the indexing workbench is instructed.

Indexing job

Indexing function.

181 One of the axes X, Y and Z is instructed at the same time with axis B.

190 Axis is specified incorrectly in the control of surface constant speed.

210 The moving part of the machine contacts the travel limit switch in + direction of axis X.

211 The movable part of the machine contacts the travel limit switch in - direction of axis X.

212 Tool enters the exclusion area of storage type travel limit 1 when axis X moves in the positive direction.

213 Tool enters the exclusion area of storage type travel limit 1 when axis X moves in the negative direction.

214 Tool enters the exclusion area of storage type travel limit 2 when axis X moves in the positive direction.

215 Tool enters the exclusion area of storage type travel limit 2 when axis X moves in the negative direction.

220 The movable part of the machine contacts the travel limit switch on the positive side of axis Y.

221 The movable part of the machine contacts the travel limit switch on the negative side of axis Y.

222 Tool enters the exclusion area of storage type travel limit 1 when axis Y moves in the positive direction.

223 Tool enters the exclusion area of storage type travel limit 1 when axis Y moves in the negative direction.

224 Tool enters the exclusion area of storage type travel limit 2 when axis Y moves in the positive direction.

225 Tool enters the exclusion area of storage type travel limit 2 when axis Y moves in the negative direction.

230 The movable part of the machine contacts the travel limit switch on the positive side of axis Z.


113

231 The movable part of the machine contacts the travel limit switch on the negative side of axis Z.

232 Tool enters the exclusion area of storage type travel limit 1 when axis Z moves in the positive direction.

233 Tool enters the exclusion area of storage type travel limit 1 when axis Z moves in the negative direction.

234 Tool enters the exclusion area of storage type travel limit 2 when axis Z moves in the positive direction.

235 Tool enters the exclusion area of storage type travel limit 2 when axis Z moves in the negative direction.

240 The movable part of the machine contacts the travel limit switch on the positive side of the 4th axis.

241 The movable part of the machine contacts the travel limit switch on the negative side of the 4th axis.

242 Tool enters the exclusion area of storage type travel limit 1 when the 4th axis moves in the positive direction.

243 Tool enters the exclusion area of storage type travel limit 1 when the 4th axis moves in the negative direction.

250 The movable part of the machine contacts the travel limit switch on the positive side of the 5th axis.

251 The movable part of the machine contacts the travel limit switch on the negative side of the 5th axis.

252 Tool enters the exclusion area of storage type travel limit 1 when the 5th axis moves in the positive direction.

253 Tool enters the exclusion area of storage type travel limit 1 when the 5th axis moves in the negative direction.

400 Axes X, Y and Z are overloaded.

401 The speed ready signal (VRDY) of axes X, Y and Z are disconnected.

402 Additional axis is overloaded.

403 The speed ready signal (VRDY) of additional axis is disconnected.

404 Though the position ready signal (PRDY) is switched off, the speed ready signal (VRDY) is not OFF. When the power is switched on again, the ready signal (PRDY) is not ON, so the speed ready signal (VRDY) will be ON.

405 The malfunction in NC or servo system may prevent returning to reference point.

407 The position ready signal (VRDY) of the 5th axis is switched off.

410 The position offset during the stop of axis X exceeds the setting.

411 The position offset during the travel of axis X exceeds the setting.

412 Axis X drifts excessively (above 500VELO).

413 The position offset of axis X exceeds ±32767 or the speed instruction value of DA converter is beyond +8191 to -8192. The alarm is often caused by wrong setting.

414 The detecting device of the rotary transformer and inductosyn of axis X malfunctions.

415 A speed above that in unit/sec detected by 511875 is instructed in axis X. The alarm is the result of incorrect CMR setting.

416 The detecting device for the pulse coder of axis X is out of order (disconnection alarm).


114

417 The servo position LSI of axis X is incorrect.

420 Position offset exceeds the setting when axis Y stops.

421 Position offset exceeds the setting when axis Y travels.

422 Axis Y drifts excessively (over 500VELO).

423 The position offset of axis Y exceeds ±32767 or the speed instruction value of DA converter goes beyond the range of +8191 to -8192. The alarm is usually a result of incorrect settings.

424 The detecting device of rotary transformer and inductosyn of axis Y malfunctions.

425 A speed above that in unit/sec detected by 511875 is instructed in axis Y. The alarm is the result of incorrect CMR setting.

426 The position detector for the pulse coder of axis Y is out of order.

427 The servo position LSI of axis Y is incorrect.

430 Position offset exceeds the setting when axis Z stops.

431 Position offset exceeds the setting when axis Z travels.

432 Axis Z drifts excessively (more than 500VELO).

433 The position offset of axis Z exceeds ±32767 or the speed instruction value of DA converter goes beyond the range of +8191 to -8192. The alarm is usually a result of incorrect settings.

434 The detecting device of the rotary transformer and inductosyn of axis Z malfunctions.

435 A speed above that in unit/sec detected by 511875 is instructed in axis Z. The alarm is the result of incorrect CMR setting.

436 The detecting device for the pulse coder of axis Z is out of order (disconnection alarm).

437 The servo position LSI of axis A is incorrect.

440 Position offset exceeds the setting when the 4th axis stops.

441 Position offset exceeds the setting when the 4th axis travels.

442 The 4th axis drifts excessively (more than 500VELO).

443 The position offset of the 4th axis exceeds ±32767 or the speed instruction value of DA converter goes beyond the range of +8191 to -8192. The alarm is usually a result of incorrect settings.

444 The detecting device of the rotary transformer and inductosyn of the 4th axis malfunctions.

445 A speed above that in unit/sec detected by 511875 is instructed in the 4th axis. The alarm is the result of incorrect CMR setting.

446 The detecting device for the pulse coder of the 4th axis is out of order (disconnection alarm).

447 The servo position LSI of the 4th axis is incorrect.


115

450 Position offset exceeds the setting when the 5th axis stops.

451 Position offset exceeds the setting when the 5th axis travels.

452 The 5th axis drifts excessively (more than 500VELO).

453 The position offset of the 5th axis Y exceeds ±32767 or the speed instruction value of DA converter goes beyond the range of +8191 to -8192. The alarm is usually a result of incorrect settings.

454 The detecting device of the rotary transformer and inductosyn of the 5th axis malfunctions.

455 A speed above that in unit/sec detected by 511875 is instructed in the 5th axis. The alarm is the result of incorrect CMR setting.

456 The position detecting device for the pulse coder of the 5th axis is out of order (disconnection alarm).

457 The servo position LSI of the 5th axis is defective.

600 Data transfer error of the connection unit.

601 Ready signal is cut off.

602 PC program is not loaded (only PC-Model A)

603 The communication between the NC and PC is improper or interrupted.

604 The MPU of PC-B cannot be held or the PCGREADY or PC-GR cannot be switched ON.

605 System alarm is given in the MPU or PC-B or G (monitor alarm).

606 RAM/ROM parity error occurs in the MPU or PC-B or G.

607 The data transfer error of MDI/LCD.

700 The main PCB is overheated.

701 The additional PCB is overheated.

702 The DC motors of axes X, Y and Z are overheated.

703 The motor of the 4th axis is overheated.

704 The motor of the 5th axis is overheated.

900 Non-volatile memory circuit 1 malfunctions.



903 Non-volatile memory circuit 4malfunctions.



116






910 RAM parity error (lower byte)

911 RAM parity error (higher byte)

912 Non-volatile memory circuit 11 malfunctions. NO alarm

920 System alarm (fault of monitoring timer).

930 CPU malfunctions (Class 0, 3 and 4 interrupts). NO alarm

940 Offset memory alarm (excessive offset is set): Set correct offset in the specified offset number.

950 Clock malfunctions (the clock of main PCB malfunctions).

960 The temporary storage area for system control commands becomes inadequate (overflow).

961 CPU alarm (execution of INT instruction)

996 Necessary option of additional RAM is added, but RAM is not really installed.

997 ROM parity error (PC ROM).

998 ROM parity error (primary ROM).

999 ROM matching error (height mismatching)


117

Appendix 7 List of the States during Switching On, Reset and Clearance

O. A state remains unchanged or a movement is kept on.

X. A state is cancelled or a movement is interrupted.

Items When switching on Clearing state Reset state

Offset ○ ○ ○

Setting data ○ ○ ○ Setting data

Parameter ○ ○ ○

Programs in memory ○ ○ ○

Information in memory × × In MDI mode ○

Other than in MDI mode ×

Indication of sequence numbers

× ○(Note 1) ○(Note 2)

One-off G codes × × ×

Modal G codes

Initial value G20/G21 remains constant as before

power failure

Initial values G20/G21 and

G22/G23 remain unchanged.

All remain unchanged.

F Zero Zero ○

S·T·M·B × ○ ○

Data

L × × In MDI mode ○ Other than in MDI mode ×

Coordinate system

Workpiece coordinates Zero ○ ○

Travel × × ×

Dwell × × ×

M·S·T·B code is sent. × × × Executing

motions

Tool length compensation × Depending on

“RS43”

MDI mode ○; a mode other than MDI depends

on “RS43”


118

(Note 1) Program number is displayed from the beginning of the program.

Items When switching on Clearing state Reset state

Tool radius compensation × × In MDI mode ○

Other than in MDI mode ×

The storage of the called subprogram numbers

× × (Note 2) In MDI mode ○

Other than in MDI mode × (Note 2)

Executing motions

ALM

The indicator goes out in the

absence of alarm.

See the left. See the left.

NOT READY × × (The indicator is

lit in case of emergency stop.)

×(The indicator is lit in case of emergency stop.)

LSK The indicator is lit. The indicator is lit.

MDI mode: 〇 A mode other than MDI:

the he indicator goes out.

BUF The indicator goes out.

The indicator goes out.

MDI mode: 〇 A mode other than MDI:

the he indicator goes out. Return to reference point × 〇(emergency

stop×) 〇(emergency stop ×)

S·T·B codes × 〇〇 M codes × × × M·S·T·B strobe signal × × ×

Spindle rotation signal (S12-digit /S analog signal)

〇〇〇

NC ready signal (MA, MB) ON 〇〇

Servo ready signal ON (in the absence of

servo alarm) See the left. See the left.

Signal indicator in CYCLE START × × ×

Indicators and output

signals

Signal indicator in feed hold × × ×

Note 2: When the NC is reset in the execution of a subprogram, the next block of the called subprogram during the return of the control to the main program cannot be executed in midway due to the subprogram. Therefore control returns to the start of the program.


119

Appendix 8 Memory Type Pitch Error Compensation

A8.1 Feature Pitch error compensation is applicable for the minimum instruction units for all axes. The function is valid after returning to reference point.

A8.2 Specifications The tool position after returning to reference point is called compensation origin. The compensations of the concerned axes are set in parameters.

i) Compensable axes: axes X, Y and Z as well as the 4th and 5th axes.

ii) Number of compensation points:

Linear axis – 128 points

Rotary axis – 61 points

iii) Range of compensation

0 to ± 7X compensation scaling rate/compensation point (minimum instruction unit)

Compensation scaling rate X1, X2, X4 and X8 (common for all axes)

iv) Compensation interval

Travel unit Minimum set interval Maximum set interval unit Metric system 8000 20000000 0. 001mm inch system 4000 20000000 0.0001inch

(Maximum compensation range = set interval ×128)

Actual compensation interval shall be set depending on the optimal value between the maximum compensation distance and mechanical travel in the ranges as listed in the above table. When the 4th or 5th axis is used as an axis of rotation, compensation interval is set within 360000.

In this case, a value less than 110,000deg/min (31.2rpm) shall be used for the feedrate of an axis of rotation.

When the set interval is less than the above minimal set interval, compensation is impossible for a linear axis.

Now it is necessary to reduce the rapid feedrate.

A8.3 Parameter setting Parameters concerning pitch error shall be set in the following parameter numbers in MDI mode or emergency stop mode.

(1) Pitch error compensation scaling rate

0 2 4 PML2 PML1 ※ ※ ※ ※ ※ ※ The scaling rate is multiplied by the set compensation for output.

PML2 PML1 Scaling rate 0 0 X 1 0 10 X 2 1 0 X 4 1 1 X 8

(Common for all axes) (2) Pitch error origins

0 3 9 P E C Z R X


120

0 4 0 P E C Z R Y

0 4 1 P E C Z R Z

0 4 2 P E C Z R 4

4 1 6 P E C Z R 5

Pitch error origins PECZRX, Y, Z, 4 and 5 specify the origin values in the pitch error compensations list.

The setting ranges of all axes are any value between 0 and 127 depending on machine type.

(3) The setting of compensation interval

1 6 3 PECINTX

1 6 4 PECINTY

1 6 5 PECINTZ

1 6 6 P E C I N T 4

4 3 6 P E C I N T 6

Pitch error compensation intervals PECINT X, Y, Z, 4 and 5 specify pitch error compensation intervals.

Except setting the positive values of 8000 or above (metric system) and 4000 or above (Inch) (for the value that the axis of rotation is 3), the setting of 0 is not compensated.

(4) Compensation setting

The pitch error compensation for all axes is set in the following parameters:

Axis name Parameter number Axis X 1000 to 1127 Axis Y 2000 to 2127 Axis Z 3000 to 3127

The 4th axis 4000 to 4127 The 5th axis 5000 to 5127

Compensation cannot be set for the parameter numbers other than listed in the above table. The set compensation rage is 0±7. The setting beyond the range is invalid.

(Example)

1 1 2 0 —— 7

In the above example, a compensation of ——7 is set at the set point No.120 of axis X. The value of the set point is added or reduced by 1 using the cursor ↑ or ↓ . The compensation values at adjacent points are displayed.

7 6 5 4 3 2 1 0


121

A8. 4 Examples of all parameter settings (1) Example 1: Pitch error origin =○, compensation interval =10000

The beginning of the compensation list corresponds to the reference point while compensation point 1 corresponds to the point moving by 10000 in the positive direction from the reference point. After that, every 1000 corresponds to a compensation point. As a result, the compensation point128 is set at 1270000. The compensation for the travel from 0 to 10000 is set at compensation point 1 while that from 1000 to 2000 is set at compensation point 2 and that from (n－1)× (compensation interval) corresponds to n×(compensation interval) is set at compensation point n.

In the above example

Interval Compensation data

0 to 10000 －7

10000 to 20000 + 6

20000 to 30000 －4

When the real machine move from the reference point to the position at +30000, the total pitch error compensation is as follows:

(+7) + (-6) + (+4) = 5

(2) Example 2: Pitch error origin =60, compensation interval =10000

The set point 60 corresponds to the reference point. The set point 61 is located in the position of +10000. After that, every 10000 corresponds to a compensation point. The set point 59 is located in the position of -10000. After that, every -10000 corresponds to a compensation point and compensation point 0 is located at -600000. That is, the compensation for the travel from (n-61) × (compensation interval) to (n-60)×(compensation interval) is set at compensation point n.

In the above example, in the interval

-30000 to -20000: A compensation of +7 is set.

-20000 to 10000: A compensation of +7 is set.

-10000 to 0: A compensation of -6 is set.

0 to 10000: A compensation of -4 is set.

In the above example, the total compensation for pitch error when the machine moves from -30000 to +10000 is:

(-7)+(-7)+(+6)+(+4)=(-4)

(3) Example 3: Pitch error origin =127, compensation interval =10000


122

The end of the compensation list corresponds to the reference point. The set point 126 is located in the position of -10000. After that, every -10000 corresponds to a compensation point. The compensation for the travel from -10000 to 0 is set at compensation point 127 while that from -20000to -10000 is set at compensation point 126. The compensation for the travel from (n-128) × (compensation interval) to (n-127)×(compensation interval) is set at compensation point n.

In the above example, compensation data is as follows:

in the interval -40000 to -30000: -3

-30000 to -20000: +7

-20000 to 10000: 0

-10000 to 0: -2

The total compensation for pitch error when the real machine moves from -40000 to the reference point is:

(+3)+(-7)+(0)+(2)=(-2)

A8. 5 Compensation setting method The relationship between the compensation as shown in the above item and the reference point as well as compensation origin

The traveling direction of the machine

Compensation interval

They are not directly related. The compensation at the compensation point n (n=0, 1, 2……127) is determined by the mechanical error (the remaining travel for a move instruction) in the interval ｛ n-(compensation origin +1) ｝ ×compensation interval to (n － compensation origin)×(compensation interval).

(1) Method for inputting compensation

The input of compensation is possible by the identical means of the common parameter input.

(a) Cancellation of compensation

For an axis eliminated of compensation, all the compensations of the axis are “○” after a compensation of -9999 is input in any parameter number.

(b) Output of compensation

All compensations can be output in the sequence identical with that of common parameter output. However, -9998 rather than -9999 shall be typed now. This type of output is impossible for some specific axes.

(2) Precautions for setting

(a) When the setting of compensation interval for the setting (parameters No.163 to 166 and 436) is a positive value, the value will be used for compensation.

When it is a negative value, its absolute value will be used for compensation.

When it is 0, the axis will not be compensated.

(The indication is positive even a negative compensation interval is input)

(b) Pitch error compensation is valid at the end of return to reference point. If compensation is not made after parameter setting at the end of return to reference point, parameter setting shall be made before returning to reference point after switching on. If pitch error


123

compensation is changed after returning to reference point, the reference point shall be returned to again.

(c) Pitch error compensation (parameters No.1000 to 5127)

The following restrictions are made for pitch error compensation:

The value of (Valid compensation of pitch error)×(pitch error compensation scaling rate)×CMR must fall within ±127. If the setting of the value goes exceeds ±127, correct compensation cannot be made. If it is necessary to set a value beyond ±127, divide the compensation and then make compensation at adjacent points. Note: CMR: Command multiplying rate

Refer to parameters No.27, 28, 29 and 30.

A8.6 Pitch error compensation for an axis of rotation For pitch error compensation for the 4th axis as an axis of rotation, its parameters are set as follows:

Parameter No. Descriptions Parameter setting 42 Compensation zero 0 166 Compensation interval 6000

That is, pitch compensation error origin =0 and compensation interval=6000 shall be used. Now a circumference is divided into 60 parts and compensation is made for every 6 degrees.

Compensation is set as the following 61 points.

Parameter No. Parameter setting 4000 -6 to 0 deg compensation 4001 0 to 6 deg compensation 4002 6 to 12 deg compensation ┆ ┆

4059 348 to 354 deg compensation 4060 354 to 360 deg compensation

In special cases, parameters 4000 and 4060 may be set to the same value. The pitch error compensation for an axis of rotation uses rapid feedrate 110000deg/min (31.2rpm) or the following speeds.

The sign of the pitch error compensation is based on its moving direction.

Namely for positive compensation, the amount of travel is only increased by one quantity of compensation.

For negative compensation, the amount of travel is only reduced by one quantity of compensation. When mechanical travel has negative and positive errors opposite to the move instruction, negative and positive compensations are set.

When the error (excessive travel) is positive (+), the compensation will be negative (-).

When the error (excessive travel) is negative (-), the compensation will be positive (+).

(Example of setting)

For travel in positive direction, +3 (-5) shall be compensated by the arrival of the compensation point.

For travel in negative direction, -3 (+5) shall be compensated by the arrival of the compensation point.


124

For travel in positive direction, +3 (-5) shall be compensated by the arrival of the compensation point.

For travel in negative direction, -3 (+5) shall be compensated by the arrival of the compensation point.

(Note) Thus it can be seen that the sign of compensation is only related to the traveling direction during compensation instead of the position of origin.


125

Appendix 9 Operations List

Item Function Program protection OFF

Parameter writing ON/OF Mode Function key Operating procedures

To clear memory ○ Power ON － Concurrently press the O and DELETE buttons to switch on the power.

To clear parameters ○ Power ON － Concurrently press the CANCEL and DELETE buttons. To clear programs Power ON － Concurrently press the RESET and DELETE buttons.

Clear

To input parameters ○ Emergency stop ON PARAMETER P → - 9999 - INPUT

To store a program ○ EDIT mode ( O → program number →INPUT

To add programs ○ EDIT mode － O → CANCEL →INPUT To store all programs EDIT mode － O → - 9999 - INPUT Parameters for pitch error compensation ○ Emergency stop

ON PARAMETER P → - 9999 - INPUT

Communication input

To input parameters ○ MDI mode PARAMETER N →parameter number→ INPUT → P →data→INPUT parameter writing switch OFF→ RESET (Note 2)

To input an offset ○ Any mode (Except EDIT) OFFSET N →offset No.→ INPUT → P →offset data→INPUT

To input setting data ○ MDI mode SETTING Move the cursor to the setting number to changed→ P → data→INPUT

MDI input

To output parameters EDIT mode PARAMETER P → - 9999 - OUTPUT To output an offset EDIT mode OFFSET P → - 9999 - OUTPUT

Communication output

To output the parameters for pitch error compensation

EDIT mode PARAMETER P → - 9999 - OUTPUT


126

To output all programs EDIT mode － O → - 9999 - OUTPUT Output a program. EDIT mode － O → program No. - OUTPUT Program number search (stored in memory) EDIT mode PARAMETER ① O →program No→ ↓ (cursor ② O → CANCEL →

↓(cursor) Sequence number search (stored in memory) AUTO mode PARAMETER Program number search→ N →sequence number→↓(cursor)

Word search (stored in memory) EDIT mode PARAMETER Input the address and data to be searched→ ↓(cursor)

Address search (stored in memory) EDIT mode PARAMETER Input the address to be searched→↓(cursor)

Search

To delete all programs ○ EDIT mode PARAMETER O → - 9999 - DELETE

To delete a programs ○ EDIT mode PARAMETER O →program number - DELETE

To delete several programs ○ EDIT mode PARAMETER N →sequence number - DELETE

To delete a single program ○ EDIT mode PARAMETER Search to the beginning of the block to be deleted→ EOB →DELETE

To delete a word ○ EDIT mode PARAMETER Search to the word to be deleted→ DELETE To change a word ○ EDIT mode PARAMETER Search to the word to be changed→ address → data— ALTER

To insert a word ○ EDIT mode PARAMETER Search to the word preceding the one to be inserted→ address →data→ INSERT

Memory sorting ○ EDIT mode PARAMETER CANCEL → SHIFT

Edit


127

Appendix 10 Lock of Program Key

A10.1 General Program numbers 9000 to 9899 are locked with keys. In key lock mode, the programs of program numbers 9000 to 9899 cannot be displayed, edited and output. The function may be used to protect the special programs developed with manufacturer’s user macros and prevents them from accidental deletion.

A10. 2 Program number It is possible to lock the programs of program numbers 9000 to 9899 with keys. Other programs cannot be locked with keys. Once they are locked with keys, all the programs of program numbers 9000 to 9899 are automatically locked. Therefore, the programs that do not need key lock shall use the numbers other than 9000 to 9899.

A10. 3 The state after key lock In key lock mode (see Section 4 below), the programs of program numbers 9000 to 9899 are as follows:

(1) Their information is not displayed even in execution.

(2) Program number search (alarm No.071) is impossible in EDIT mode (AUTO mode). Therefore they cannot be edited.

(3) The memory cannot be cleaned up.

(4) The numbers are not included in the display of all program numbers.

(5) Program output is impossible (not output even when all programs are output).

(6) Program deletion is impossible (not deleted even when all programs are deleted).

(7) Program storage is impossible (alarm No.170).

A10. 4 Key locking and unlocking procedures (1) Preset a secret number (1 to 99999999) in parameter No.168. Do not to

forget the number since the contents of the parameter is not displayed. A program cannot be unlocked if it is set to 0.

(Note 1) The setting of the parameter is active in unlock state.

(Note 2) The parameter is not deleted even in complete clearing state.

(Note 3) The parameter becomes 0 after complete clearance of memory, i.e. the key is disabled.

(2) To disable the key, set the same information in parameter No.408 and 168.

The key is disabled only when it has the same value with parameter No.168.

(Note 1) The settings of the parameter are not displayed.

(Note 2) The parameter cannot be stored in non-volatile memory.

(3) Method of key lock after unlock

(a) Set a different value in parameter No.408 than in parameter No.168.

(b) Switch off the NC power and then switch on it again.

Parameter No.


128

1 6 8 Secret No.

Store the secret number to be locked.


4 0 8 Lock/unlock The key lock is disabled by entering the same value as No.168.

The key lock is active when a different value is entered.

(Note 1) When the value of parameter No.168 is set to 0, the key lock is disabled and is inactive even the power lock is switched OFF. Note that parameter No.168 must be set to 0 when key lock is not necessary.

A10. 5 Cautions (1) Proceed as follows if the set secret code is forgotten:

(a) Completely clear the memory (disable key lock).

(b) Input all parameters (except parameter No.168)

(c) Save secret programs in the memory.

(d) Set a secret code in parameter No.168 (with key lock).

(2) The PROGRAM page is displayed as follows if a program with key lock is switched to EDIT mode. The settings of the program are hidden. The display or edit of other programs shall be performed by reset (now continuous operation is impossible due to reset). The initial page will be returned to once the system is reset. To continue to execute a program, switch the mode to AUTO or DNC mode. Machining is performed using CYCLE START.

(3) Once programs ○90000 to ○9899 are stored and edited, please apply key

lock for the programs other than ○9000 to ○9899. When programs ○9000 to ○9899 are displayed, the above page is displayed in EDI mode and programs are displayed by reset.


129

Appendix 11 The Interrupt Function of User Macro

A11.1 General During the execution of a program, it is possible to call another program by inputting interrupt signal on the machine side. This function is called interrupt function of user macro.

The interrupt instruction in a program is as follows:

M96, P××××；user macro interrupt ON

M97, P××××；user macro interrupt OFF

By using this function it is possible to call other programs on any executing block of program and start program operations in ever-changing conditions.

(Example of application)

(1) Start tool abnormality detection with external signal.

(2) Stop the currently performing machining and insert other machining in the continuous machining.

(3) The current machining information is read regularly.

Fig.1: Schematic diagram of user macro interrupt

It is also applicable for the applications of adaptive control.

After instructing M96P×××× in program, the currently executing program is interrupted once interrupt signal (UINT) is input.

Programs instructed by P××××

The interrupt signal during the execution of program and after M97 is invalid (marked “*” in the figure).

A11.2 Method of instruction A11.2.1 Significant conditions

User macro INTERRUPT is only effective during the execution of a program.


130

Namely the significant conditions are:

(1) MEMORY, TAPE or MDI mode is selected.

(2) STL (start indicator) is set to ON.

(3) User macro INTERRUPT is still not being executed. User macro INTERRUPT cannot be executed during JOG (JOG, STEP, HANDLE etc) operation.

A11.2. 2 Instruction types User macro interrupt function disables or enables interrupt signal (UINT) using M96 and M97 in principle.

That is, when M96 is instructed, interrupt signal (UINT) may be used to start user macro INTERRUPT until M97 is instructed or NC is reset. Also, INTERRUPT (UINT) is invalid without the instruction of M96. User macro INTERRUPT cannot be started even by inputting interrupt signal (UINT) after M979 is instructed or reset.

(Format)

M96 P××××; User macro INTERRUPT ON

Instructing a program number to be interrupted

M97； User macro INTERRUPT OFF

Interrupt signal (UINT) is valid after the input of M96.

Once M97 is instructed, interrupt signal will be invalid. The signal input after instructing M97 is kept until the input of M96. Once M96 is instructed, user macro INTERRUPT can be started.

A11.3 Detailed descriptions A11.3. 1 The ENABLE/MASK of user macro INTERRUPT

Even user macro INTERRUPT is not used, it is not necessary to change the program. For this purpose, parameter ENABLE/MASK (parameter No.025——MSUR) is provided for selecting user macro INTERRUPT.

If user macro INTERRUPT is set to MASK in the parameter, M96 and M97 will be output to the outside as common M codes. If it is set to ENABLE, they are processed inside the parameter without inputting to the outside.

A11.3. 2 Subprogram type interrupt and macro type interrupt


131

The modes of user macro interrupt include subprogram type interrupt and macro type interrupt. Therefore, the parameter No.025——MSUB is designed for an interrupt mode.

Subprogram type interrupt

Interrupt program is called by a subprogram.

That is, the values of local variables remain unchanged before and after interrupt. In addition, the interrupt is not counted as the number of calls.

Macro type interrupt

Interrupt program is called as a macro.

That is, the values of local variables change before and after interrupt.

In addition, the interrupt is not counted as the number of calls. The number of calls of programs and macros executed in interrupt program are accumulated to their numbers respectively.

Variables cannot be obtained from the executing programs even a user macro interrupt is a macro interrupt.

A11.3.3 M codes for control of user macro interrupt

In principle, M96 and M97 are used for the control of user macro interrupt. However, they may be used for other purposes upon manufacturer’s requirements (M function and macro call). Therefore, whether these M codes are valid or not depends on the setting of parameter No.025——MPRM.

When the M codes for control of user macro interrupt are set as a parameter:

User macro is set to ON and the M codes are set in #053.

User macro is set to OFF and the M codes are set in #054.

When the parameter MPRM is 0, M96 and M97 become the M codes for control of user macro interrupt as well as #053 and #054.

It is recommended not to use the M codes other than M96 and M97 for the control of macro interrupt in consideration of the interchangeability of program.

A11.3.4 User macro interrupt and NC instruction

User macro interrupt is of two types: interrupting the executing NC instruction and waiting for the end of the currently executing program. For this purpose, parameter No.314——MINT is designed for switching between interrupting in the midway/at the end of block.

If interrupting in the midway (type I) is selected in the parameter.

(1) Once interrupt signal (UINT) is input, the executing travel or suspension is interrupted and the interrupt program is executed.


132

(2) When there is an NC statement in the interrupt program, the interrupted program instruction disappears and the NC instruction in the interrupt program is executed. In case of return, the next block of the original program is executed.

(3) If there is no NC instruction in the interrupt program, the interrupted block is continuously executed when M99 is used to return to the original block.

If the parameter is selected, it is interrupted (type U) at the end of a block:

(1) Once interrupt signal (UINT) is input, the interrupt program instead of the instruction of the currently executing block is interrupted.

(2) When there is an NC instruction in the interrupt program, it is executed at the end of the executing program.

In any case, the control switches to the interrupt control program once interrupt signal is input.

The relationship between the interrupt in the midway of program (Fig.3.4 – a) and the interrupt at the end of program (Fig.3.4 – b) are as indicated in the figure. Interrupt will be executed whichever interrupt signal is input.

A11.3. 5 Reception of user macro interrupt signal (UINT)

There are two modes of reception of user macro interrupt signal (UINT): state triggering and edge triggering. The so-called state triggering is that it is valid in the ON state of signal. Edge triggering is that the signal on the edge is active when the signal is switched from OFF to ON. The use of a mode shall be determined by parameter No.025——TSE. If this parameter is set to state triggering mode, user macro interrupt occurs when the interrupt is active, i.e. the interrupt signal (UINT) is ON (1). Therefore, interrupt program can be repeatedly executed when the interrupt signal (UINT) is continuously ON. In addition, when the parameter is set to edge triggering mode, interrupt program is completed in an instant (only the program instructed by macro, etc) because it is only valid during the rise of the interrupt signal (UINT). Therefore, it is only applicable for the occasions that is not suitable for state triggering mode and only one user macro interrupt is performed in the whole program (interrupt signal is kept ON in this case).


133

Except special purposes, the actual effects of the two modes are the same (there is not difference in the time from the input of signal to the interrupt of actual execution).

State triggering performs user macro interrupt in the ON state of signal. Edge triggering performs user macro interrupt in the rise of signal. Therefore, in the above example state triggering performs 4 interrupts while edge triggering only one.

A11.3.6 Return from user macro interrupt

The instruction for returning from user macro to the original program is M99. The sequence number in the returned program is also specified with address “P”. In this case, search starts from the relevant program switch and returns to the initially appeared program number (the same as “98”).

Other interrupts cannot be performed in the execution of user macro interrupt program. M99 may be used to clear the state. The conditions individually* instructed with M99 are executed before the end of the execution of the foregoing programs. Therefore user program interrupt is also valid for the last instruction of interrupt program. If it is not applicable, user program interrupt may be controlled with M96/M97.

*: The single block of M99, which only includes address For O, N, P, L and M, the block is considered as the same block as the previous one of the program. Thus even a signal block does not stop. The program is: G×× X××× ; M99 is actually identical with

G×× X××× ; M99.

(They vary in whether G×× executes or not before M99.)


134

Fig. 3.6 Return from user macro

Overlapping is not allowed in the execution of user macro interrupt. That is, other interrupts are automatically shielded in case of interrupt. If M99 is executed, user macro interrupt will be active again. Here M99 is executed before the end of the previous program as a separate block. In the above example, the interrupt in the Gxx block of program 0 1234 is also valid. 0 1234 is executed after signal input.

In addition, 0 5678 is under the control of M96/M97. Hence the interrupt is valid only after returning to 0 1000.

A11.3.7 User macro interrupt and modal information

User macro is different from general program calls. It is started by interrupt signal (UINT) in program execution. As a rule, change of the modal information in an interrupt program has a negative impact on the original program. Therefore, modal information restores the state before interrupt when it returns to the original program with M99 even the modal information is changed in an interrupt program.

When M99 P×××× is used to return to the original program from an interrupt program, the modal information in a program is controllable. Hence the modal information changed in the reception of interrupt program. (On the contrary, when it is to receive the modal information in the original program, the return to the following travel is changeable depending on the modal data during interrupt.)

Therefore, in this case: 1) Modal information is given in the interrupt program.

2) Necessary modal information is instructed at return point. Application is taken into account like this.


135

Fig. 3.7 User macro interrupt and modal information

Modal information shall be changed in interrupt program.

1) During the return of M99, the reception of modal information before interrupt is valid while the modal information changed in interrupt program is invalid.

2) During the return with M99 and P0000, the modal information changed in interrupt program is also valid after the return of modal information (the same as M98).

A11.4 Parameters 7 6 5 4 3 2 1 0 0 2 5 MUSR MSUB MPRM TSE

MUSR 1. Use macro interrupt function

0. Not use macro interrupt function

MSUB 1. Subprogram type user macro interrupt

0. Macro type user macro interrupt

MPRM 1. The M code for the control of user macro interrupt is set by parameter.

0. User macro interrupt is under the control of M96 and M97.

Note) User macro interrupt is a part of User macro B function. That is, user macro interrupt cannot be used without the selection of user macro B.

The settings of parameters No.053 and 054 are valid only when MPRM=1 (user macro B must be selected).

TSE 1. User macro interrupt is of state triggering type.

0. User macro interrupt is of edge triggering type.

Note) State triggering state is valid in signal input state.

Edge triggering is active in the rise of signal.


136

0 5 3 MACINTON

MACINTON: The M code when user macro interrupt is active.

Settings 03 to 97

0 5 4 MACINTOF

MACINTOF: The M code when user macro interrupt is inactive.

Settings 03 to 97

Note) Parameters No. 053 and 054 are valid only when MPRM (025Bit4)=1.

7 6 5 4 3 2 1 0 3 1 4 MINT

MINT 1. The NC instruction that starts to execute interrupt program until the

end of block (user macro interrupt type II)

0. The NC instruction that starts to execute interrupt program before the end of block (user macro interrupt type I)

Note) Once user macro interrupt signal (UINT) type I is input, the currently executing program is interrupted and the interrupt program is executed. The motion after the return varies with the availability of NC instruction in interrupt program.

i) With NC instruction

The remaining instructions (amount of travel and suspension time) disappear in the interrupted blocks.

ii) Without NC instruction

The remaining instruction in an interrupted block continues to execute. However, the sending auxiliary function can be correctly output in the both cases.

Type II: The current block is not interrupted and the interrupt program executed even interrupt signal is input. If the interrupt program has an NC instruction, it starts to execute after the execution of the interrupted program.

A11.5 Diagnosis 7 6 5 4 3 2 1 0 1 2 0 UINT

UINT 1. User macro interrupt ON.

0. User macro interrupt OFF.

The signal is the external signal for user macro interrupt. Intended for the applications have requirements for high speed, the signal may be detected through not only the signal generated by strong power, but also external signal. Therefore, the manufacturer needs to connect the external signal to the position of the signal as shown below. The position is not applicable for other purposes.

7 6 5 4 3 2 1 0 0 4 4 UINT

The diagnosis numbers to be observed are #044 and #120.

A11.6 Internal wiring diagram


137

A11.7 Example of application A11.7.1 Procedures for starting tool fault detection using external signal

(Specifications)

Malfunction restoration is immediately executed even in cycle movement.

(Parameter setting)

TSE=0: Edge triggering mode

MUSR=1: Enable user macro interrupt function

MSUB=*: Subprogram type/macro type user macro interrupt

MPRM=*: Setting of the M code for the control of user macro interrupt MINT=0: Interrupt program is executed before the end of block. (Explanations)

User macro interrupt signal is ON during fault detection. It is kept on unless special operations are performed. Only one interrupt is performed if the edge triggering mode is selected. Whether the execution is interrupted or not is detected with diagnosis No.#120.

Parameters are set for the selection of subprogram type, macro type and control M code depending on programming.

A11.7.2 Inserting other job in continuous machining without interrupting the current program

(Specifications)

A short job is inserted in the program execution with longer machining time. General single block stops when the original program restarts. It is hard to execute the intervention in MDI mode.

(Parameter setting)

TSE=*: Selection of a triggering mode for user macro interrupt


MSUB=0: Macro type user program interrupt

MPRM=*: Setting of the M code for the control of user macro interrupt

MINT=0: Interrupt program is executed after the end of block.


138

(Explanations)

Parameters are set for the triggering mode of user macro interrupt and the selection of M code as required.

For user macro interrupt, interrupt is prohibited in the execution of block and macro type interrupt is used to prevent the affection of the instruction segments in machining. The modal information, mechanical position, etc in case of interrupt in an interrupt program are restored during the return to the original program so that any program can by executed. To fix it, instruction M96 P×××× may be directly used. The program is called from the interrupt program with M98 P#100 if it is not fixed.

A11.7. 3 Reading machining information in fixed intervals (Specifications)

To manage machining status, machining information is sent out on a regular basis. This exerts no impact on machining sequence.

(Parameter setting)

TSE=0: Edge triggering mode


MSUB=0: Subprogram type user macro interrupt


MINT=0: Interrupt program is executed before the end of block

(Explanations)

Assuming that an interrupt program does not include any NC statement, the interrupt program is started only once in edge triggering mode on an regular basis depending on the ON/OFF of interrupt signal (because interrupt program is repeated when the signal is ON in state triggering mode). Since block may interrupt in the midway, the rise corresponding to the interrupt signal immediately interrupts.

The external output of machining information adopts user macro DO, output modal information and position information.

An interrupt program may execute in parallel with the original block. However, the machining will stop for a period of time at the end of the original block and before the end of the interrupt program.

A11.7. 4 Using the same program for general cutting and special cutting

(Specifications)

Each executive program is provided with special travel. But the instruction is not easy to be executed in general program.

(Parameter setting)

TSE=1: State triggering mode


MSUB=*: Subprogram type/macro type user macro interrupt


MINT=1: Interrupt program is executed after the end of block.

(Explanations)


139

The interrupt program shall be instructed as follows

O×××× M97； Disable interrupt

M96； Enable interrupt

M99；

The interrupt signal is kept ON in state triggering mode.

Therefore, user macro interrupt is executed at the end of each block in the original program. The special travel to be executed is instructed in an interrupt program. The program part that needs no user macro interrupt is disabled using M97.

Add: No.52, 1st . Street, Luochong North Road, Luochongwei, Guangzhou, 510165, China

Website: http://www.gsk.com.cn E-mail: [email protected] Tel: 86-20-81796410/81797922 Fax: 86-20-81993683

All specification and designs are subject to change without notice. Aug. 2007/Edition 4 Aug. 2007/Printing 4

Kenh

新建图章

Gsk983m Cnc System User Manual

Documents

Transcript of Gsk983m Cnc System User Manual