Optimum bell–shaped acceleration/deceleration before interpolation, as mentioned here, refers to bell–shaped acceleration/deceleration before interpolation in which linear acceleration/deceleration not reaching the specified acceleration/deceleration does not occur if T2 > T1. Calculation is performed as described below.
(1) If the bell–shaped acceleration/deceleration before interpolation time constant T2’ is calculated under the condition that the bell–shaped acceleration/deceleration before interpolation must not have a linear portion,
A F2T
2T *
=’
T2: Acceleration change time specified for bell–shaped acceleration/ deceleration before interpolation
F: Acceleration/deceleration reference speed
A: Acceleration for the acceleration/deceleration before interpolation
(2) Setting the speed on the Parameter
(3) Using the speed specified with the F command issued at the start of cutting as the reference speed
� Acceleration/deceleratio n parameter calculation method
PROGRAMMING 19. HIGH SPEED CUTTING
FUNCTIONS B–64124EN/01
402
(2) A proper acceleration is determined under the condition that the acceleration change must be about the same as the setting so that parameter changes do not cause considerable shock to the machine, that is:
Acceleration after change Acceleration before change =
Acceleration change time Acceleration change time after change before change
The acceleration change time is regarded to be the sum of the acceleration change time of bell–shaped acceleration/deceleration and the time constant of acceleration/deceleration after interpolation, and the acceleration A’ for the acceleration/deceleration before interpolation is determined as follows:
TcT
TcT AA
+
+ *=
2
’2 ’
A: Acceleration for the acceleration/deceleration before interpolation
Tc:Time constant of acceleration/deceleration after interpolation
Acceleration/deceleration is performed using T2’ and A’, determined as described above.
PROGRAMMINGB–64124EN/01 20. AXIS CONTROL FUNCTIONS
403
20 AXIS CONTROL FUNCTIONS
PROGRAMMING20. AXIS CONTROL FUNCTIONS B–64124EN/01
404
It is possible to change the operating mode for two or more specified axes to either synchronous operation or normal operation by an input signal from the machine. Synchronous control can be performed for up to four pairs of axes with the Series 16, or up to three pairs with the Series 18, according to the parameter setting (parameter No. 8311). The following operating modes are applicable to machines having two tables driven independently by separate control axes. The following example is of a machine with two tables driven independently by the Y axis and V axis. If the axis names and axis sets that are actually being used differ from those in the example, substitute the actual names for those below.
V
X
Y
Z
Fig. 20.1 Example of axis configuration of the machine operated by simple synchronous control
This mode is used for, for example, machining large workpieces that extend over two tables. While operating one axis with a move command, it is possible to synchronously move the other axis. In the synchronous mode, the axis to which the move command applies is called the master axis, and the axis that moves synchronously with the master axis is called the slave axis. In this example, it is assumed that Y axis is the master axis and V axis is the slave axis. Here, the Y axis and the V axis move synchronously in accordance with program command Yyyyy issued to the Y axis (master axis). Synchronous operation is possible during automatic operation, jog feed, manual handle feed using the manual pulse generator, and incremental feed, but is not possible during manual reference position return.
20.1 SIMPLE SYNCHRONOUS CONTROL
Explanations
� Synchronous operation
PROGRAMMINGB–64124EN/01 20. AXIS CONTROL FUNCTIONS
405
This operating mode is used for machining different workpieces on each table. The operation is the same as in ordinary CNC control, where the movement of the master axis and slave axis is controlled by the independent axis address (Y and V). It is possible to issue the move commands to both the master axis and slave axis in the same block.
(1) The Y axis moves normally according to program command Yyyyy issued to the master axis.
(2) The V axis moves normally according to program command Vvvvv issued to the slave axis.
(3) The Y axis and the V axis move simultaneously according to program command YyyyyVvvvv. Both automatic and manual operations are the same as in ordinary CNC control.
For how to switch between the synchronous operation and normal operation modes, refer to the relevant manual published by the machine tool builder.
When the automatic reference position return command (G28) and the 2nd/3rd/4th reference position return command (G30) are issued during synchronous operation, the V axis follows the same movement as the Y axis returns to the reference position. After the return movement is complete, the reference position return complete signal of the V axis goes on when that of the Y axis goes on. As a rule, commands G28 and G30 must be issued in the normal operating mode.
When the automatic reference position return check command (G27) is issued during synchronous operation, the V axis and Y axis move in tandem. If both the Y axis and the V axis have reached their respective reference positions after the movement is complete, the reference position return complete signals go on. If either axis is not at the reference position, an alarm is issued. As a rule, command G27 must be issued in the normal operating mode.
When a move command is issued to the slave axis during synchronous operation, a P/S alarm (No. 213) is issued.
The axis to be used as the master axis is set in parameter No. 8311. The slave axis is selected by an external signal.
Setting bit 7 (SMF) of parameter No. 3105 to 1 suppresses display of the actual speed of the slave axes.
� Normal operation
� Switching between synchronous operation and normal operation
� Automatic reference position return
� Automatic reference position return check
� Specifying the slave axis
� Master axis and slave axis
� Displaying actual speed for master axis only
PROGRAMMING20. AXIS CONTROL FUNCTIONS B–64124EN/01
406
In synchronous axis control, commands that require no axis motion, such as the workpiece coordinate system setup command (G92) and the local coordinate system setup command (G52), are set to the Y axis by program command Yyyyy issued to the master axis.
For signals such as external deceleration, interlock, and machine lock, only the signals issued to the master axis are valid in the synchronous operating mode. Signals issued to other axes are ignored.
Both the pitch error and backlash are compensated independently for the master axis and the slave axis.
Turn on the manual absolute switch during synchronous operation. If it is off, the slave axis may not move correctly.
The difference between the master axis and slave axis in servo positional deviation is always monitored. If the difference exceeds the parameter– set limit, an P/S alarm (No. 213) is issued.
The difference between the master axis and slave axis in machine coordinates is always monitored. If the difference exceeds the parameter– set limit, an servo alarm (No. 407) is issued.
When the power is turned on, compensation pulses are output for the slave axis to match the machine position of the master axis with the machine position of the slave axis. (This is enabled only when the absolute position detection function is used.)
Compensation for out–of–synchronism (where the difference between the master and slave axes in servo positional deviation is always monitored and the servo motor for the slave axis is compensated to reduce the difference) is not performed.
When the machine is manually returned to the reference position during synchronous operation, both the master axis and the slave axis move synchronously until the acceleration movement is complete. However, grid detection thereafter is carried out independently.
Limitations
� Setting a coordinate system
� Externally–requested deceleration, interlock, and machine lock
� Pitch error compensation
� Manual absolute
� Synchronization error check using positional deviation
� Synchronization error check using machine coordinates
� Synchronization
� Compensation for out–of–synchronism
� Manual reference position return
PROGRAMMINGB–64124EN/01 20. AXIS CONTROL FUNCTIONS
407
The roll–over function prevents coordinates for the rotation axis from overflowing. The roll–over function is enabled by setting bit 0 of parameter ROAx 1008 to 1.
For an incremental command, the tool moves the angle specified in the command. For an absolute command, the coordinates after the tool has moved are values set in parameter No. 1260, and rounded by the angle corresponding to one rotation. The tool moves in the direction in which the final coordinates are closest when bit 1 of parameter RABx No. 1008 is set to 0. Displayed values for relative coordinates are also rounded by the angle corresponding to one rotation when bit 2 of parameter RRLx No. 1008 is set to 1.
Assume that axis A is the rotating axis and that the amount of movement per rotation is 360.000 (parameter No. 1260 = 360000). When the following program is executed using the roll–over function of the rotating axis, the axis moves as shown below.
G90 A0 ; Sequence
number Actual
movement value
Absolute coordinate value after movement
end
N1 G90 A–150.0 ; N1 –150 210
N2 G90 A540.0 ; N2 –30 180
N3 G90 A–620.0 ; N3 –80 100
N4 G91 A380.0 ; N4 +380 120
N5 G91 A–840.0 ; N5 –840 0
Relative coordinate value
–720°
–0°
–360°
–0° –0°
–0° 360°
–0°
N1
N2
N3
N4
N5
210°(Absolute)
180° 100°
120°
Absolute coordinate value
NOTE This function cannot be used together with the indexing function of the index table.
20.2 ROTARY AXIS ROLL–OVER Explanations
� ����
PROGRAMMING20. AXIS CONTROL FUNCTIONS B–64124EN/01
408
When the angular axis makes an angle other than 90° with the perpendicular axis, the angular axis control function controls the distance traveled along each axis according to the inclination angle. A program, when created, assumes that the angular axis and perpendicular axis intersect at right angles. However, the actual distance traveled is controlled according to an inclination angle.
+Y
+Y Coordinate system actually used (Angular axis)
Program coordinate system
+Z (Perpendicular axis)
θ
θ : Inclination angle
When the angular axis is the Y–axis and the perpendicular axis is the Z–axis, the amount of travel along each axis is controlled according to the formulas shown below. The distance traveled along the Y–axis is determined by the following formula: Ya=Yp/cosθ The distance traveled along the Z–axis is corrected by the inclination of the Y–axis, and is determined by the following formula: Za=Zp–Yp*tanθ The speed component along the Y–axis is determined by the following formula:
Fa=Fp/cosθ Ya, Za, Fa : Actual distance and speed Yp, Zp, Fp : Programmed distance and speed
The angular and perpendicular axes for which angular axis control is to be applied must be specified beforehand, using parameters (No. 8211 and 8212). Parameter AAC (No. 8200#0) enables or disables the inclined axis control function. If the function is enabled, the distance traveled along each axis is controlled according to an inclination angle parameter (No. 8210). Parameter AZR (No. 8200#2) enables angular axis manual reference point return only with a distance along the angular axis.
By setting the normal axis/angular axis control invalid signal NOZAGC to 1, slanted axis control only for the angular axis can be available. In this time the angular axis are converted to those along the slanted coordinate system without affecting commands to normal axis.
An absolute and a relative position are indicated in the programmed Cartesian coordinate system.
20.3 ANGULAR AXIS CONTROL
Explanations
� .����� �� ���
� Invalidity of normal axis
� Absolute and relative position display
PROGRAMMINGB–64124EN/01 20. AXIS CONTROL FUNCTIONS
409
A machine position indication is provided in the machine coordinate system where an actual movement is taking place according to an inclination angle. However, when inch/metric conversion is performed, a position is indicated which incorporates inch/metric conversion applied to the results of inclination angle operation.
WARNING 1 After angular axis control parameter setting, be sure to
perform manual reference position return operation. 2 If once manual reference position return has been
performed along the angular axis, also perform manual reference position return along the perpendicular axis. P/S alarm No.090 is issued when an attempt is made to manually return to the reference position along the perpendicular axis although the angular axis is not on the reference point.
3 Once the tool has been moved along the angular axis when perpendicular/angular axis control disable signal NOZAGC has been set to 1, manual reference position return must be performed.
4 Before attempting to manually move the tool along the angular and perpendicular axes simultaneously, set perpendicular/angular axis control disable signal NOZAGC to 1.
NOTE 1 If an inclination angle close to 0° or ±90° is set, an error can
occur. (A range from ±20° to ±90° should be used.) 2 Before a perpendicular axis reference position return check
(G27) can be made, angular axis reference position return operation must be completed.
� Machine position display
PROGRAMMING20. AXIS CONTROL FUNCTIONS B–64124EN/01
410
When enough torque for driving a large table cannot be produced by only one motor, two motors can be used for movement along a single axis. Positioning is performed by the main motor only. The submotor is used only to produce torque. With this tandem control function, the torque produced can be doubled.
Table
Ball screw
Main motor
Submotor
Fig. 20.4 Example of operation
In general, the NC regards tandem control as being performed for one axis. However, for servo parameter management and servo alarm monitoring, tandem control is regarded as being performed for two axes. For details, refer to the relevant manual published by the machine tool builder.
20.4 TANDEM CONTROL
III. OPERATION
OPERATIONB–64124EN/01 1. GENERAL
413
1 GENERAL
OPERATION1. GENERAL B–64124EN/01
414
The CNC machine tool has a position used to determine the machine position. This position is called the reference position, where the tool is replaced or the coordinate are set. Ordinarily, after the power is turned on, the tool is moved to the reference position. Manual reference position return is to move the tool to the reference position using switches and pushbuttons located on the operator’s panel.
Reference position
Tool
Machine operator’s panel
Fig. 1.1 (a) Manual reference position return
The tool can be moved to the reference position also with program commands. This operation is called automatic reference position return (See Section II–6).
1.1 MANUAL OPERATION
Explanations
� Manual reference position return (See Section III–3.1)
OPERATIONB–64124EN/01 1. GENERAL
415
Using machine operator’s panel switches, pushbuttons, or the manual handle, the tool can be moved along each axis.
Tool
Workpiece
Machine operator’s panel
Manual pulse generator
Fig. 1.1 (b) The tool movement by manual operation
The tool can be moved in the following ways:
(i) Jog feed (See Section III–3.2) The tool moves continuously while a pushbutton remains pressed.
(ii) Incremental feed (See Section III–3.3) The tool moves by the predetermined distance each time a button is pressed.
(iii) Manual handle feed (See Section III–3.4) By rotating the manual handle,the tool moves by the distance corresponding to the degree of handle rotation.
� The tool movement by manual operation
OPERATION1. GENERAL B–64124EN/01
416
Automatic operation is to operate the machine according to the created program. It includes memory, MDI and DNC operations. (See Section III–4).
Program
Tool
01000 ; M_S_T ; G92_X_; G00... ; G01...... ;
.
.
.
.
Fig. 1.2 (a) Tool movement by programming
After the program is once registered in memory of CNC, the machine can be run according to the program instructions. This operation is called memory operation.
CNC Machine
Memory
Fig. 1.2 (b) Memory operation
After the program is entered, as an command group, from the MDI keyboard, the machine can be run according to the program. This operation is called MDI operation.
MDI keyboard CNC
Manual program input
Machine
Fig. 1.2 (c) MDI operation
In this mode of operation, the program is not registered in the CNC memory. It is read from the external input/output devices instead. This is called DNC operation. This mode is useful when the program is too large to fit the CNC memory.
1.2 TOOL MOVEMENT BY PROGRAMMING– AUTOMATIC OPERATION
Explanations � .� ��! ���� ����
� MDI operation
� DNC operation
OPERATIONB–64124EN/01 1. GENERAL
417
Select the program used for the workpiece. Ordinarily, one program is prepared for one workpiece. If two or more programs are in memory, select the program to be used, by searching the program number (Section III–9.3).
G92
O1001 Program number
M30
G92
O1002 G92
M30
Program number Program number search
Automatic operation
O1003 ––––––
M30
––––––
––––––
Work–1 program
Work–2 program
Program number
Work–3 program
In memory or on a tape
Fig. 1.3 (a) Program selection for automatic operation
Pressing the cycle start pushbutton causes automatic operation to start. By pressing the feed hold or reset pushbutton, automatic operation pauses or stops. By specifying the program stop or program termination command in the program, the running will stop during automatic operation. When one process machining is completed, automatic operation stops.
Cycle start
Feed hold Reset
Program stop Program end
Stop caused by program
Start
Stop Automatic operation
Fig. 1.3 (b) Start and stop for automatic operation
1.3 AUTOMATIC OPERATION
Explanations
� Program selection
� Start and stop (See Section III–4)
OPERATION1. GENERAL B–64124EN/01
418
While automatic operation is being executed, tool movement can overlap automatic operation by rotating the manual handle.
�
Programmed depth of cut
Depth of cut by handle interruption
Tool position after handle interruption
Tool position during automatic operation
Fig. 1.3 (c) Handle Interruption for automatic operation
� Handle interruption (See Section III–4.7)
OPERATIONB–64124EN/01 1. GENERAL
419
Before machining is started, the automatic running check can be executed. It checks whether the created program can operate the machine as desired. This check can be accomplished by running the machine actually or viewing the position display change (without running the machine) (See Section III–5).
Remove the workpiece, check only movement of the tool. Select the tool movement rate using the dial on the operator’s panel.
Tool
Table
Fig. 1.4.1 (a) Dry run
Check the program by changing the feedrate specified in the program.
Tool Feed rate specified by program : 100 mm/min.
Feed rate after feed rate override (20%) : 20 mm/min.
Workpiece
Fig. 1.4.1 (b) Feedrate override
1.4 TESTING A PROGRAM
1.4.1 Check by Running the Machine
Explanations
� Dry run (See Section III–5.4)
� Feedrate override (See Section III–5.2)
OPERATION1. GENERAL B–64124EN/01
420
When the cycle start pushbutton is pressed, the tool executes one operation then stops. By pressing the cycle start again, the tool executes the next operation then stops. The program is checked in this manner.
Cycle start
Cycle start
Cycle start
Cycle start
StopStop
Stop
Tool
2���&'���
Fig. 1.4.1 (c) Single block
Tool
MDI
X Y Z
The tool remains stopped, and only the positional displays of the axes change.
Workpiece
Fig. 1.4.2 Machine lock
When automatic running is placed into the auxiliary function lock mode during the machine lock mode, all auxiliary functions (spindle rotation, tool replacement, coolant on/off, etc.) are disabled.
� Single block (See Section III–5.5)
1.4.2 How to View the Position Display Change without Running the Machine
Explanations
� Machine lock (See Sections III–5.1)
� Auxiliary function lock (See Section III–5.1)
OPERATIONB–64124EN/01 1. GENERAL
421
After a created program is once registered in memory, it can be corrected or modified from the MDI panel (See Section III–9). This operation can be executed using the part program storage/edit function.
Program registration
MDI
CNC CNC
Program correction or modification
Tape reader
CNC tape (program)
Fig. 1.5 Part program editing
1.5 EDITING A PART PROGRAM
OPERATION1. GENERAL B–64124EN/01
422
The operator can display or change a value stored in CNC internal memory by key operation on the MDI screen (See III–11).
Data setting
MDI
Data display
Screen Keys
CNC memory
Fig. 1.6 (a) Displaying and setting data
Tool compensation number1 12.3 25.0 Tool compensation number2 20.0 40.0 Tool compensation number3 ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅
Setting
Display
CNC memory
Screen Keys
MDI
Geometry compensation
Wear com- pensation
Fig.1.6 (b) Displaying and setting offset values
The tool has the tool dimension (length, diameter). When a workpiece is machined, the tool movement value depends on the tool dimensions. By setting tool dimension data in CNC memory beforehand, automatically generates tool routes that permit any tool to cut the workpiece specified by the program. Tool dimension data is called the offset value (See Section III–11.4.1).
1.6 DISPLAYING AND SETTING DATA
Explanations
� Offset value
OPERATIONB–64124EN/01 1. GENERAL
423
Machined shape
1st tool path
2nd tool path
Offset value of the 1st tool
Offset value of the 2nd tool
Fig. 1.6 (c) Offset value
Apart from parameters, there is data that is set by the operator in operation. This data causes machine characteristics to change. For example, the following data can be set: Inch/Metric switching Selection of I/O devices Mirror image cutting on/off The above data is called setting data (See Section III–11.4.3).
⋅ ⋅ ⋅
Setting
DisplayingScreen Keys
Setting data
⋅Inch/Metric switching ⋅Selection of I/O device ⋅Mirror image ON/OFF setting
CNC Memory
Program Automatic operation
Operational characteristics
Movement of the machine
Fig. 1.6 (d) Displaying and setting operator’s setting data
� Displaying and setting operator’s setting data
OPERATION1. GENERAL B–64124EN/01
424
The CNC functions have versatility in order to take action in characteristics of various machines. For example, CNC can specify the following: Rapid traverse rate of each axis Whether increment system is based on metric system or inch system. How to set command multiply/detect multiply (CMR/DMR) Data to make the above specification is called parameters (See Section III–11.5.1). Parameters differ depending on machine tool.
MDI
CNC memory
Parameter Rapid traverse rate Position control Reference position return Backlash compensation data Pitch error compensation data ⋅
⋅ ⋅
Program
Operational characteristics
Setting
DisplayScreen Keys
Automatic operation
Movement of the machine
Fig. 1.6 (e) Displaying and setting parameters
A key called the data protection key can be defined. It is used to prevent part programs, offset values, parameters, and setting data from being registered, modified, or deleted erroneously (See Section III–11).
Program Offset value Parameters Setting data
CNC memory
Data Setting
Machine operator’s panel
Screen Keys
Data protection key
MDI
Signal
Protection Key
Registration / modification inhibition
Fig. 1.6 (f) Data protection key
� Displaying and setting parameters
� Data protection key
OPERATIONB–64124EN/01 1. GENERAL
425
The contents of the currently active program are displayed. In addition, the programs scheduled next and the program list are displayed. (See Section III–11.2.1)
*�0���.
MEM STOP * * * * * * 13 : 18 : 14
1100 00005
.#
PRGRM
�� �=� ��7 ��� �>� ?�7 �5��� �55��� �
�� ��� �=���� -�5� �
�� >5��� �
�> ��� 5���� ���5��� 65��� �
�6 ��� =5��� �=���� 65��� �
�7 ��� ��5��� �
�@ �55��� �
�= 7���� �65��� �
��� �5��� �55��� �
��� ��� �>� � �� �
�A$�B �C �� �$ � !D8 �"
Active program number Active sequence number
Currently executed program
The cursor indicates the currently executed location
Program content
N5 G02 X900.0 R–250.0 ;
PROGRAM (NUM.) MEMORY (CHAR.) USED: 60 3321
FREE: 2 429
O0001 (MACRO–GCODE.MAIN) O0002 (MACRO–GCODE.SUB1) O0010 (TEST–PROGRAM.ARTHMETIC NO.1) O0020 (TEST–PROGRAM.F10–MACRO) O0040 (TEST–PROGRAM.OFFSET) O0050 O0100 (INCH/MM CONVERT CHECK NO.1) O0200 (MACRO–MCODE.MAIN)
> _ EDIT **** *** *** 16:05:59 [ PRGRM ] [ DIR+ ] [ ] [ ] [ (OPRT) ]
PROGRAM DIRECTORY O0001 N00010
1.7 DISPLAY
1.7.1 Program Display
OPERATION1. GENERAL B–64124EN/01
426
The current position of the tool is displayed with the coordinate values. The distance from the current position to the target position can also be displayed. (See Section III–11.1.1 to 11.1.3)
Y
E
F
Workpiece coordinate system
� #9�; *0-6#608 ��=-0;9# �
* * * * * * * * * *
O0003 N00003
!D8 �"
X 150.000 Y 300.000 Z 100.000
�$� 19 : 47 : 45
RUN TIME 0H41M CYCLE TIME 0H 0M22S 8� � �DC�� ��
ABS $G �GG
When a trouble occurs during operation, alarm number and alarm message are displayed on the screen. (See Section III–7.1) See APPENDIX G for the list of alarms and their meanings.
�;��.. --��
MEM STOP * * * * * * 19 : 55 : 22
O1000 N00003
.#
ALM
�G� � ��� A:�� �
��� :�8 D8$ �;�D?$
1.7.2 Current Position Display
1.7.3 Alarm Display
OPERATIONB–64124EN/01 1. GENERAL
427
Run time and number of parts are displayed on the screen. (See Section lll–11.4.5)
ACTUAL POSITION (ABSOLUTE)
* * * *
O0003 N00003
!D8 �"
X 150.000 Y 300.000 Z 100.000
�$� �� � 20 : 22 : 23
RUN TIME 0H16M CYCLE TIME 0H 1M 0S 8� � �DC�� �@
ABS $G �GG
FIN
Programmed tool movement can be displayed on the following planes: (See Section III–12) 1) XY plane 2) YZ plane 3) XZ plane 4) Three dimensional display
Z
X
Z
Z
X Y
Y
Y
X
Three dimensional display (isometric)
Display on the XY plane Display on the YZ plane
Display on the XZ plane
(1) (2)
(3) (4)
Fig. 1.7.5 Graphic display
1.7.4 Parts Count Display, Run Time Display
1.7.5 Graphic Display
OPERATION1. GENERAL B–64124EN/01
428
Programs, offset values, parameters, etc. input in CNC memory can be output to paper tape, cassette, or a floppy disk for saving. After once output to a medium, the data can be input into CNC memory.
Memory
Program
Offset
Parameters
Reader/puncher interface
Portable tape reader
CNC Automatic programming system
Floppy disk
FANUC Floppy cassette adaptor
FANUC Floppy Cassette
SYSTEM P
FANUC PPR
Paper tape
.
.
.
Memory card adapter
(incorporated CNC)
Memory card
Fig. 1.8 Data Output
1.8 DATA INPUT / OUTPUT
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
429
2 0* ��#608�; � ?6 - The available operational devices include the setting and display unit attached to the CNC, the machine operator’s panel, and external input/output devices such as a Handy File.
OPERATION2.
Key location of MDI (horizontal type LCD/MDI unit) III–2.1.3. . . Key location of MDI (vertical type LCD/MDI unit) III–2.1.4. . . . .
2.1 SETTING AND DISPLAY UNITS
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
431
2.1.1 7.2″ Monochrome/ 8.4″ Color LCD/MDI Unit (Horizontal Type)
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
432
2.1.2 7.2″ Monochrome/ 8.4″ Color LCD/MDI Unit (Vertical Type)
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
433
Address/numeric keys
Function keys
Cursor keys Page change keys
Shift key
Cancel (CAN) key
Input key
Edit keys
Help key
Reset key
2.1.3 Key Location of MDI (Horizontal Type LCD/MDI Unit)
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
434
Shift key Page change keysCursor keys
Function keys
Input key
Cancel (CAN) keyEdit keys
Address/numeric keys
Reset key Help key
2.1.4 Key Location of MDI (Vertical Type LCD/MDI Unit)
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
435
Table 2.2 Explanation of the MDI keyboard
Number Name Explanation
1 RESET key
RESET
Press this key to reset the CNC, to cancel an alarm, etc.
2 HELP key
HELP
Press this key to display how to operate the machine tool, such as MDI key operation, or the details of an alarm which occurred in the CNC (Help function).
3 Soft keys The soft keys have various functions, according to the Applications. The soft key functions are displayed at the bottom of the screen.
4 Address and numeric keys
…QN 4 [
Press these keys to input alphabetic, numeric, and other characters.
5 SHIFT key
SHIFT
Some keys have two characters on their keytop. Pressing the <SHIFT> key switches the characters. Special character � is displayed on the screen when a character indicated at the bottom right corner on the keytop can be entered.
6 INPUT key
INPUT
When an address or a numerical key is pressed, the data is input to the buffer, and it is displayed on the screen. To copy the data in the key input buffer to the offset reg- ister, etc., press the <INPUT> key. This key is equivalent to the [INPUT] key of the soft keys, and either can be pressed to produce the same result.
7 Cancel key
CAN
Press this key to delete the last character or symbol input to the key input buffer. When the key input buffer displays
>N001X100Z_ and the cancel key is pressed, Z is canceled and >N001X100_ is displayed.
CAN
8 Program edit keys
ALTER INSERT DELETE
Press these keys when editing the program.
: Alteration
: Insertion
: Deletion
ALTER
INSERT
DELETE
9 Function keys
… POS PROG
Press theses keys to switch display screens for each function. See sec. III–2.3 for details of the function keys.
2.2 EXPLANATION OF THE KEYBOARD
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
436
Table 2.2 Explanation of the MDI keyboard
Number ExplanationName
10 Cursor move keys There are four different cursor move keys.
: This key is used to move the cursor to the right or in the forward direction. The cursor is moved in short units in the forward direction.
: This key is used to move the cursor to the left or in the reverse direction. The cursor is moved in short units in the reverse direction.
: This key is used to move the cursor in a downward or forward direction. The cursor is moved in large units in the forward direction.
: This key is used to move the cursor in an upward or reverse direction. The cursor is moved in large units in the reverse direction.
11 Page change keys
PAGE
PAGE
Two kinds of page change keys are described below.
: This key is used to changeover the page on the screen in the forward direction.
: This key is used to changeover the page on the screen in the reverse direction.
PAGE
PAGE
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
437
The function keys are used to select the type of screen (function) to be displayed. When a soft key (section select soft key) is pressed immediately after a function key, the screen (section) corresponding to the selected function can be selected.
1 Press a function key on the MDI panel. The chapter selection soft keys that belong to the selected function appear.
2 Press one of the chapter selection soft keys. The screen for the selected chapter appears. If the soft key for a target chapter is not displayed, press the continuous menu key (next–menu key). In some cases, additional chapters can be selected within a chapter.
3 When the target chapter screen is displayed, press the operation selection key to display data to be manipulated.
4 To redisplay the chapter selection soft keys, press the return menu key.
The general screen display procedure is explained above. However, the actual display procedure varies from one screen to another. For details, see the description of individual operations.
2.3 FUNCTION KEYS AND SOFT KEYS
2.3.1 General Screen Operations
Function keys
(OPRT)
Chapter selection soft keys Operation
selection key
Return menu key Continuous menu key
OFS/SETPROGPOS
SYSTEM CSTM/GRMESSAGE
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
438
Function keys are provided to select the type of screen to be displayed. The following function keys are provided on the MDI panel:
Press this key to display the position screen.
Press this key to display the program screen.
Press this key to display the offset/setting screen.
Press this key to display the system screen.
Press this key to display the message screen.
Press this key to display the custom screen (conversational macro screen) and graphics screen.
2.3.2 Function Keys
POS
PROG
OFS/SET
SYSTEM
MESSAGE
CSTM/GR
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
439
To display a more detailed screen, press a function key followed by a soft key. Soft keys are also used for actual operations. The following illustrates how soft key displays are changed by pressing each function key.
: Indicates a screen that can be displayed by pressing a function key(*1)
: Indicates a green–lettered soft key.(*2)
: Indicates input from the MDI panel.
: Indicates a black–lettered soft key.
: Indicates the continuous menu key (rightmost soft key).
H I
! "
H I
The symbols in the following figures mean as shown below :
: Indicates screens
*1 Press function keys to switch between screens that are used frequently.
*2 Some soft keys are not displayed depending on the option configuration.
2.3.3 Soft Keys
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
440
Monitor screen
[(OPRT)] [PTSPRE] [EXEC]
[RUNPRE] [EXEC]
[ABS]
Absolute coordinate display
[(OPRT)][REL] !�E'� �� (+����"
HORIGINI
[PRESET]
[ALLEXE]
(Axis name) [EXEC]
[PTSPRE] [EXEC]
[RUNPRE] [EXEC]
[ALL]
[HNDL]
[MONI]
��� ��F �� �' '� �'**���% �F )� �( � '� ��FPOSITION SCREEN
Relative coordinate display
Current position display
Handle interruption
[(OPRT)] !�E'� �� (+����"
HORIGINI
[PRESET]
[ALLEXE]
(Axis name) [EXEC]
[PTSPRE] [EXEC]
[RUNPRE] [EXEC]
[WRK–CD] [ALLEXE] [EXEC](Axis name, 0)
[(OPRT)] [PTSPRE] [EXEC]
[RUNPRE] [EXEC]
[(OPRT)] [PTSPRE] [EXEC]
[RUNPRE] [EXEC]
POS
POS
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
441
[ABS]
[(OPRT)] [BG–EDT] [O SRH]
[PRGRM]
Program display screen
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
' )� �$� +�%�
[N SRH] [REWIND]
See “When the soft key [BG–EDT] is pressed”
[(OPRT)][CHECK]
Program check display screen
[REL]
Current block display screen
[(OPRT)] [BG–EDT][CURRNT]
Next block display screen
[(OPRT)] [BG–EDT][NEXT]
Program restart display screen
[(OPRT)] [BG–EDT][RSTR]
!�"
(O number) (N number)
PROGRAM SCREEN
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
[F SRH]
[P TYPE] [Q TYPE]
[CAN] [EXEC]
[BG–EDT] [O SRH] [N SRH]
[REWIND]
See “When the soft key [BG–EDT] is pressed” (O number) (N number)
[F SRH]
[P TYPE] [Q TYPE]
[CAN] [EXEC]
(2)(Continued on the next page)
1/2
(N number)
(N number)
PROG
PROG
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
442
[FL.SDL] [PRGRM]
File directory display screen
[(OPRT)][DIR] [SELECT] [EXEC] (File No. ) [F SET]
Schedule operation display screen
[(OPRT)][SCHDUL] [CLEAR]
(Schedule data)
[CAN] [EXEC]
[INPUT]
Return to !�" (Program display)
(2) 2/2
[(OPRT)] [BG–EDT] [O SRH]
[DIR]
Program directory screen
���J2)� )� ��� ��F H��;$?�I '� &�����%K
(O number) � (� � )� &��*��+
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
443
1/2
[(OPRT)] [BG–EDT] (O number) [O SRH]
[PRGRM]
Program display
(Address) [SRH↓]
[REWIND] (Address) [SRH↑]
[F SRH] [CAN] (N number) [EXEC]
[READ] [CHAIN] [STOP] [CAN]
[EXEC] [PUNCH] [STOP]
[CAN] [EXEC]
[DELETE] [CAN] [EXEC]
[EX–EDT] [COPY] [CRSR∼] [∼CRSR] [∼BTTM] [ALL]
[MOVE] [CRSR∼] [∼CRSR] [∼BTTM] [ALL]
[MERGE] [∼CRSR] [∼BTTM]
[CHANGE] (Address) [BEFORE]
(Address) [AFTER] [SKIP] [1–EXEC] [EXEC]
(1)(Continued on the next page)
(The cursor moves to the end of a program.)
(O number)
(O number)
(N number)
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
' )� $?:� +�%� PROGRAM SCREEN
(O number) [EXEC]
(O number) [EXEC]
(O number) [EXEC]
���K2)� )� ��� ��F H��;$?�I '� &�����%K
PROG
PROG
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
444
(1)
[C.A.P.]
Graphic Conversational Programming
[PRGRM] [G.MENU]
(G number) [BLOCK] (Data) [INPUT] When a G number is omitted, the standard screen appears.
[(OPRT)] [INPUT]
2/2
� (� � )� &��*��+
[(OPRT)] [BG–EDT] (O number) [O SRH]
[DIR]
Program directory display
[READ] [CHAIN] [STOP] [CAN]
[EXEC] [PUNCH] [STOP]
[CAN] [EXEC]
(O number)
(O number)
� (� � )� &��*��+
���K2)� )� ��� ��F H��;$?�I '� &�����%K
[F SRH] [CAN] [EXEC]
[READ]
[STOP] [CAN]
[PUNCH]
[F SET]
[F SET]
[EXEC]
[O SET]
[STOP] [CAN]
[F SET]
[EXEC]
[O SET]
[DELETE] [CAN]
[F SET]
Floppy directory display
[FLOPPY] [DIR] ( number)
(O number)
(number) (O number)
[PRGRM] [(OPRT)]
� (� � )� &��*��+
(number)
(number)
[EXEC]
[(OPRT)] INSERT
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
445
[(OPRT)] [BG–EDT][PRGRM]
Program display
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
' )� �?: +�%� PROGRAM SCREEN
[(OPRT)] [BG–EDT][MDI]
Program input screen
(Address) (Address)
[SRH↓] [SRH↑]
Current block display screen
[(OPRT)] [BG–EDT][CURRNT]
Next block display screen
[(OPRT)] [BG–EDT][NEXT]
Program restart display screen
[(OPRT)] [BG–EDT][RSTR]
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
[REWIND]
PROG
PROG
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
446
[(OPRT)] [BG–EDT][PRGRM]
Program display
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
' )� A�?G0 <D�0 �� $- +�%� PROGRAM SCREEN
Current block display screen
[(OPRT)] [BG–EDT][CURRNT]
Next block display screen
[(OPRT)] [BG–EDT][NEXT]
Program restart display screen
[(OPRT)] [BG–EDT][RSTR]
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
[(OPRT)] [BG–EDT][DIR]
Program directory display
See “When the soft key [BG–EDT] is pressed”
PROG
PROG
Program display
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
' )� �<D� �� �A?G +�%� PROGRAM SCREEN
[(OPRT)] [BG–EDT][PRGRM]
(Address) (Address)
[SRH↓] [SRH↑]
(O number)
[REWIND]
[(OPRT)] [BG–EDT] (O number) [O SRH]
[DIR]
Program directory display
� (� � )� &��*��+
See “When the soft key [BG–EDT] is pressed”
See “When the soft key [BG–EDT] is pressed”
[O SRH] � (� � )� &��*��+
PROG
PROG
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
447
1/2
[(OPRT)] [BG–END] (O number) [O SRH]
[PRGRM]
Program display
(Address) [SRH↓]
[REWIND] (Address) [SRH↑]
[F SRH] [CAN] (N number) [EXEC]
[READ] [CHAIN] [STOP] [CAN]
[EXEC] [PUNCH] [STOP]
[CAN] [EXEC]
[DELETE] [CAN] [EXEC]
[EX–EDT] [COPY] [CRSR∼] [∼CRSR] [∼BTTM] [ALL]
[MOVE] [CRSR∼] [∼CRSR] [∼BTTM] [ALL]
[MERGE] [∼CRSR] [∼BTTM]
[CHANGE] (Address) [BEFORE]
(Address) [AFTER] [SKIP] [1–EXEC] [EXEC]
(1)(Continued on the next page)
(The cursor moves to the end of a program.)
(O number)
(O number)
(N number)
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
!2)� )� ��� ��F H��;$?�I '� &�����% ' ��� +�%��"
PROGRAM SCREEN
(O number) [EXEC]
(O number) [EXEC]
(O number) [EXEC]
PROG
PROG
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
448
[(OPRT)] [BG–EDT] (O number) [O SRH]
[DIR]
Program directory display
[READ] [CHAIN] [STOP] [CAN]
[EXEC] [PUNCH] [STOP]
[CAN] [EXEC]
(1)
(O number)
(O number)
[C.A.P.]
Graphic Conversational Programming
[PRGRM] [G.MENU]
(G number) [BLOCK] (Data) When a G number is omitted, the standard screen appears.
[F SRH] [CAN] [EXEC]
[READ]
[STOP] [CAN]
[PUNCH]
[F SET]
[F SET]
[EXEC]
[O SET]
[STOP] [CAN]
[F SET]
[EXEC]
[O SET]
[DELETE] [CAN]
[F SET]
[EXEC]
Floppy directory display
[FLOPPY] [DIR]
2/2
� (� � )� &��*��+
� (� � )� &��*��+
(number)
(number) (O number)
(number) (O number)
(number)
[PRGRM] [(OPRT)]
� (� � )� &��*��+
[(OPRT)] [INPUT]
[INPUT][(OPRT)] INSERT
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
449
[(OPRT)][OFFSET]
Tool offset screen
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
(Number) (Axis name) (Numeral) (Numeral)
[NO SRH] [INP.C.]
[+INPUT] [INPUT]
[(OPRT)][SETING]
Setting screen
(Numeral) (Numeral)
[NO SRH]
[+INPUT] [INPUT]
[ON:1] [OFF:0]
[(OPRT)][WORK]
Work coordinate system setting screen
(Numeral) (Numeral)
[NO SRH] [+INPUT] [INPUT]
(Number)
(Number)
OFFSET/SETTING SCREEN
[(OPRT)][MACRO]
Macro variables display screen
(Numeral)
[NO SRH]
[INPUT]
(Number) (Axis name) [INP.C.]
[CLEAR] [ALL] [WEAR] [GEOM]
[READ] [CAN] [WEAR]
[PUNCH] [CAN] [EXEC]
(1)
1/2
(Numeral) [INPUT]
[PUNCH] [CAN] [EXEC]
OFS/SET
OFS/SET
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
450
[(OPRT)][MENU]
Pattern data input screen
[SELECT](Number)
[OPR]
Software operator’s panel screen
[(OPRT)][TOOLLF]
Tool life management setting screen
(Numeral)
[NO SRH]
[INPUT]
(Number) [CAN] [EXEC]
[CLEAR]
2/2 (1)
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
451
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
[(OPRT)][PARAM]
Parameter screen
(Numeral) (Numeral)
[NO SRH]
[+INPUT] [INPUT]
[ON:1] [OFF:0]
(Number)
[READ] [CAN] [EXEC]
[PUNCH] [CAN] [EXEC]
[(OPRT)][DGNOS]
Diagnosis screen
[NO SRH](Number)
[PMC]
PMC screen
1/2
SYSTEM SCREEN
Note) Search for the start of the file using the PRGRM screen for read/punch.
[SYSTEM]
System configuration screen
(4) (Continued on the next page)
SYSTEM
SYSTEM
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
452
[W.DGNS]
Waveform diagnosis screen
(4)
[W.PRM] [W.GRPH] [STSRT]
[TIME→] [←TIME] [H–DOBL] [H–HALF]
[STSRT] [CH–1↑]
[V–DOBL] [V–HALF]
[CH–1↓]
[STSRT] [CH–2↑]
[V–DOBL] [V–HALF]
[CH–2↓]
2/2
[(OPRT)] [SV.PRM]
Servo parameter screen
[ON:1] [OFF:0]
[SV.SET] [SV.TUN]
Spindle parameter screen
[(OPRT)] [SP.PRM]
[INPUT]
[ON:1] [OFF:0]
[SP.SET] [SP.TUN] [SP.MON]
(Numeral) [INPUT]
[SV.TRC] [(OPRT)] [TRACE] [TRNSF]
[(OPRT)][PITCH]
Pitch error compensation screen
(Numeral) (Numeral)
[NO SRH]
[+INPUT] [INPUT]
[ON:1] [OFF:0]
(No.)
[READ] [CAN] [EXEC]
[PUNCH] [CAN] [EXEC]
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
453
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
[ALARM]
Alarm display screen
[MSG]
Message display screen
[HISTRY]
Alarm history screen
[(OPRT)] [CLEAR]
. --�� - � 8 MESSAGE
MESSAGE
[ALAM]
��� ��F �� �' '� �'**���% �F )� �( � '� ��F
Alarm detail screen
[OPR]
Operation method screen
[PARA]
Parameter table screen
[(OPRT)] [SELECT]
A ;* - � 8
[(OPRT)] [SELECT]
HELP
HELP
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
454
��� ��F �� �' '� �'**���% �F )� �( � '� ��FGRAPHIC SCREEN
Tool path graphics
[(OPRT)]
[PARAM]
Tool path graphics
[EXEC] [AUTO] [STSRT] [STOP] [REWIND] [CLEAR]
[(OPRT)][ZOOM] [EXEC] [←] [→] [↑] [↓]
[POS]
CSTM/GR
CSTM/GR
Soft key transition triggered by the function key
CUSTOM screen
CUSTOM screen
CUSTOM screen
The layout of the CUSTOM screen is customized by the machine tool builder. For details of the screen, refer to the manual issued by the machine tool builder. To switch from the CUSTOM screen to another screen, press the desired function key.
CUSTOM SCREEN CSTM/GR
CSTM/GR
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
455
When an address and a numerical key are pressed, the character corresponding to that key is input once into the key input buffer. The contents of the key input buffer is displayed at the bottom of the screen. In order to indicate that it is key input data, a “>” symbol is displayed immediately in front of it. A “_” is displayed at the end of the key input data indicating the input position of the next character.
Key input buffer display
[ ] [ ] [ ] [ ] [ ]
$?:� �G� ����5�>5
. ���� ����#
Fig. 2.3.4 Key input buffer display
To input the lower character of the keys that have two characters inscribed
on them, first press the SHIFT
key and then the key in question.
When the SHIFT
key is pressed, “_” indicating the next character input
position changes to “~”. Now lowercase characters can be entered (shift state). When a character is input in shift status the shift status is canceled.
Furthermore, if the SHIFT
key is pressed in shift status, the shift status is
canceled. It is possible to input up to 32 characters at a time in the key input buffer.
Press the CAN
key to cancel a character or symbol input in the key input
buffer.
(Example) When the key input buffer displays >N001X100Z_
and the cancel CAN
key is pressed, Z is canceled and
>N001X100_ is displayed.
2.3.4 Key Input and Input Buffer
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
456
After a character or number has been input from the MDI panel, a data
check is executed when INPUT
key or a soft key is pressed. In the case of
incorrect input data or the wrong operation a flashing warning message will be displayed on the status display line.
Warning message display
Display of key input buffer
Soft key display
Status display [ ] [ ] [ ] [ ] [ ]
$?:� 2 D�� �D?$
. #
Fig. 2.3.5 Warning message display
Table 2.3.5 Warning Messages
Warning message Content
FORMAT ERROR The format is incorrect.
WRITE PROTECT Key input is invalid because of data protect key or the parameter is not write enabled.
DATA IS OUT OF RANGE The input value exceeds the permitted range.
TOO MANY DIGITS The input value exceeds the permitted number of digits.
WRONG MODE Parameter input is not possible in any mode other than MDI mode.
EDIT REJECTED It is not possible to edit in the current CNC status.
2.3.5 Warning Messages
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
457
Handy File of external input/output device is available. For detail on Handy File, refer to the corresponding manual listed below.
Table 2.4 External I/O device
Device name Usage Max. storage capacity
Reference manual
FANUC Handy File Easy–to–use, multi function input/output device. It is de- signed for FA equipment and uses floppy disks.
3600m B–61834E
The following data can be input/output to or from external input/output devices: 1. Programs 2. Offset data 3. Parameters 4. Custom macro common variables 5. Pitch error compensation data For an explanation of data input/output and how to use a memory card to input and output data, see Chapter III–8.
2.4 EXTERNAL I/O DEVICES
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
458
Before an external input/output device can be used, parameters must be set as follows.
CNC
MAIN CPU BOARD
Channel 1 Channel 2
JD36A JD36B
RS–232–CRS–232–C
Reader/ puncher
Reader/ puncher
I/O CHANNEL=0 or I/O CHANNEL=1
I/O CHANNEL=2
CNC has two channels of reader/punch interfaces. The CNC has a memory card interface as well. The input/output device to be used is specified by setting the channel (interface) connected to that device in setting parameter I/O CHANNEL. The specified data, such as a baud rate and the number of stop bits, of an input/output device connected to a specific channel must be set in parameters for that channel in advance. (No data need be set for the memory card interface.) For channel 1, two combinations of parameters to specify the input/output device data are provided. The following shows the interrelation between the reader/punch interface parameters for the channels.
0020 I/O CHANNEL
Specify a channel for an input/output device.
I/O CHANNEL = 0 : Channel 1 = 1 : Channel 1 = 2 : Channel 2 = 4 : Memory card
Interface
I/O CHANNEL=0 (channel 1)
0101 Stop bit and other data
0102 Number specified forthe input/output device
0103 Baud rate
I/O CHANNEL=1 (channel 1)
0111 Stop bit and other data
0112 Number specified for the input/output device
0113 Baud rate
I/O CHANNEL=2 (channel 2)
0121
0122
0123
Input/output channel number (parameter 0020)
Parameter Number
Stop bit and other data
Number specified for the input/output device Baud rate
Memory card = 4 interface
* � ����
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
459
The Handy File is an easy–to–use, multi function floppy disk input/output device designed for FA equipment. By operating the Handy File directly or remotely from a unit connected to the Handy File, programs can be transferred and edited. The Handy File uses 3.5–inch floppy disks, which do not have the problems of paper tape (i.e., noisy during input/output, easily broken, and bulky). One or more programs (up to 1.44M bytes, which is equivalent to the memory capacity of 3600–m paper tape) can be stored on one floppy disk.
RS–232–C or RS–422 Interface (Punch panel, etc.)
FANUC Handy File
RS–232–C Interface
RS–422 Interface
2.4.1 FANUC Handy File
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
460
Procedure of turning on the power
1 Check that the appearance of the CNC machine tool is normal. (For example, check that front door and rear door are closed.)
2 Turn on the power according to the manual issued by the machine tool builder.
3 After the power is turned on, check that the position screen is displayed. An alarm screen is displayed if an alarm occurs upon power–on. If the screen shown in Section III–2.5.2 is displayed, a system failure may have occurred.
MEM STRT MTN *** 09:06:35 [ ABS ] [ REL ] [ ALL ] [ HNDL ] [ OPRT ]
ACTUAL POSITION(ABSOLUTE) O1000 N00010
PART COUNT 5 RUN TIME 0H15M CYCLE TIME 0H 0M38S ACT.F 3000 MM/M S 0 T0000
X 123.456 Y 363.233 Z 0.000
4 Check that the fan motor is rotating.
WARNING Until the positional or alarm screen is displayed at the power on, do not touch them. Some keys are used for the maintenance or special operation purpose. When they are pressed, unexpected operation may be caused.
2.5 POWER ON/OFF
2.5.1 Turning on the Power
Procedure
Position display screen
OPERATIONB–64124EN/01 2. OPERATIONAL DEVICES
461
If a hardware failure or installation error occurs, the system displays one of the following three types of screens then stops. Information such as the type of printed circuit board installed in each slot is indicated. This information and the LED states are useful for failure recovery.
SLOT CONFIGURATION DISPLAY
0 : 003E4000 1 : 30464202 2 : 00504303 3 : 4 : 5 :
0 : 1 : 2 : 3 : 4 : 5 :
Physical slot number (secondary)
Information such as the module ID of an installed printed circuit board
Physical slot number (primary)
Internally–assigned slot number
Module functionTypes of printed circuit boards
For more information about the types of printed circuit boards and module functions, refer to the MAINTENANCE MANUAL (B–64115EN).
2.5.2 Screen Displayed at Power–on
Slot status display
OPERATION2. OPERATIONAL DEVICES B–64124EN/01
462
D4B1 – 01 SLOT 01 (3046) : END SLOT 02 (3050) : Blank: Setting not completed
Module ID
Slot number
END: Setting completed
D4B1 – 01 CNC control software OMM : yyyy–yy PMC : zzzz–zz
Order–made macro/macro compiler PMC
The software configuration can be displayed on the system configuration screen also. Refer to the MAINTENANCE MANUAL (B–64115EN) for the system configuration screen.
Power Disconnection
1 Check that the LED indicating the cycle start is off on the operator’s panel.
2 Check that all movable parts of the CNC machine tool is stopping.
3 If an external input/output device such as the Handy File is connected to the CNC, turn off the external input/output device.
4 Continue to press the POWER OFF pushbutton for about 5 seconds.
5 Refer to the machine tool builder’s manual for turning off the power to the machine.
Screen indicating module setting status
Display of software configuration
2.5.3 Power Disconnection
Procedure
OPERATIONB–64124EN/01 3. MANUAL OPERATION
463
3 MANUAL OPERATION MANUAL OPERATION are six kinds as follows :
3.1 MANUAL REFERENCE POSITION RETURN 3.2 JOG FEED 3.3 INCREMENTAL FEED 3.4 MANUAL HANDLE FEED 3.5 MANUAL ABSOLUTE ON AND OFF
OPERATION3. MANUAL OPERATION B–64124EN/01
464
The tool is returned to the reference position as follows : The tool is moved in the direction specified in parameter ZMI (bit 5 of No. 1006) for each axis with the reference position return switch on the machine operator’s panel. The tool moves to the deceleration point at the rapid traverse rate, then moves to the reference position at the FL speed. The rapid traverse rate and FL speed are specified in parameters (No. 1420,1421, and 1425). Fourstep rapid traverse override is effective during rapid traverse. When the tool has returned to the reference position, the reference position return completion LED goes on. The tool generally moves along only a single axis, but can move along three axes simultane ously when specified so in parameter JAX(bit 0 of No.1002).
ÇÇ ÇÇ ÇÇ
Rapid traverse rate (rapid traverse override is effective)
Rapid traverse motion Decelerated motion FL speed
ÇÇ ÇÇ ÇÇ
Reference position
Deceleration point
Procedure for Manual Reference Position Return
1 Press the reference position return switch, one of the mode selection swithces.
2 To decerease the feedrate, press a rapid traverse override switch. When the tool has returned to the reference position, the reference position return completion LED goes on.
3 Press the feed axis and direction selection switch corresponding to the axis and direction for reference position return. Continue pressing the switch until the tool returns to the reference position. The tool can be moved along three axes simultaneously when specified so in an appropriate parameter setting. The tool moves to the deceleration point at the rapid traverse rate, then moves to the reference position at the FL speed set in a parameter.
4 Perform the same operations for other axes, if necessary. The above is an example. Refer to the appropriate manual provided by the machine tool builder for the actual operations.
X
MIRRROR IMAGE
Y Z C X Y Z
PROGRAM STOP
M02/ M30
MANU ABS
SPINDLE ORI TAP
ATC READY NC? MC?
 MANUAL OPERATION
465
The coordinate system is automatically determined when manual reference position return is performed. When �, � and � are set in workpiece zero point offset values, the workpiece coordinate system is determined so that reference point on the tool holder or the position of the tip of the reference tool is X= �, Y = �, Z = � when reference position return is performed. This has the same effect as specifying the following command for reference position return:
G92X�Y�Z�;
Once the REFERENCE POSITION RETURN COMPLETION LED lights at the completion of reference position return, the tool does not move unless the REFERENCE POSITION RETURN switch is turned off.
The REFERENCE POSITION RETURN COMPLETION LED is extinguished by either of the following operations: – Moving from the reference position. – Entering an emergency stop state.
For the distance (Not in the deceleration condition) to return the tool to the reference position, refer to the manual issued by the machine tool builder.
Explanations
� Automatically setting the coordinate system
������������
� .����" ��� ���� " ��
� ��������� �������� ������
�� ������� ; �
� #�� ���� ��� �� ������ ��
��������� ��������
OPERATION3. MANUAL OPERATION B–64124EN/01
466
In the jog mode, pressing a feed axis and direction selection switch on the machine operator’s panel continuously moves the tool along the selected axis in the selected direction. The jog feedrate is specified in a parameter (No.1423) The jog feedrate can be adjusted with the jog feedrate override dial. Pressing the rapid traverse switch moves the tool at the rapid traverse feedrate (No. 1424) regardless of the postiotion of the jog feedrate override dial. This function is called the manual rapid traverse. Manual operation is allowed for one axis at a time. 3 axes can be selected at a time by parameter JAX (No.1002#0).
ÇÇ ÇÇ ÇÇ
While a switch is pressed, the tool moves in the direction specified by the switch.
Z
Y
X
Procedure for JOG feed
1 Press the jog switch, one of the mode selection switches.
2 Press the feed axis and direction selection switch corresponding to the axis and direction the tool is to be moved. While the switch is pressed, the tool moves at the feedrate specified in a parameter (No. 1423). The tool stops when the switch is released.
3 The jog feedrate can be adjusted with the jog feedrate override dial.
4 Pressing the rapid traverse switch while pressing a feed axis and direction selection switch moves the tool at the rapid traverse rate while the rapid traverse switch is pressed. Rapid traverse override by the rapid traverse override switches is effective during rapid traverse.
The above is an example. Refer to the appropriate manual provided by the machine tool builder for the actual operations.
3.2 JOG FEED
MEMORY
ÂÂ ÂÂ
REMOTE MDIEDIT
ZERO RETURN
JOGHANDLE
MODE
TEACH
+C +Z +Y
+X–X
–C–Y –Z
RAPID
AXIS DIRECTION Procedure
0 2000
JOG FEED RATE DL$ :?$
F0 50 10025
RAPID TRAVERSE
OVERRIDE (%)
OPERATIONB–64124EN/01 3. MANUAL OPERATION
467
Feedrate, time constant and method of automatic acceleration/ deceleration for manual rapid traverse are the same as G00 in programmed command.
Changing the mode to the jog mode while pressing a feed axis and direction selection switch does not enable jog feed. To enable jog feed, enter the jog mode first, then press a feed axis and direction selection switch.
If reference position return is not performed after power–on, pushing RAPID TRAVERSE button does not actuate the rapid traverse but the remains at the JOG feedrate. This function can be disabled by setting parameter RPD (No.1401#01).
Limitations
� ������� ����@������� 1
���� ��� � ��� �� �����
� � �"� �� ����
� � ��� �� ����� ����� ��
��������� �������� ������
OPERATION3. MANUAL OPERATION B–64124EN/01
468
In the incremental (INC) mode, pressing a feed axis and direction selection switch on the machine operator’s panel moves the tool one step along the selected axis in the selected direction. The minimum distance the tool is moved is the least input increment. Each step can be 10, 100, or 1000 times the least input increment. This mode is effective when a manual pulse generator is not connected.
Tool Each time a switch is pressed, the tool moves one step in the direction specified by the switch.
Z
X
Y
Procedure for Incremental Feed
1 Press the INC switch, one of the mode selection switches.
2 Select the distance to be moved for each step with the magnification dial�
3 Press the feed axis and direction selection switch corresponding to the axis and direction the tool is to be moved. Each time a switch is pressed, the tool moves one step. The feedrate is the same as the jog feedrate.
4 Pressing the rapid traverse switch while pressing a feed axis and direction selection switch moves the tool at the rapid traverse rate. Rapid traverse override by the rapid traverse override switch is effective during rapid traverse.
The above is an example. Refer to the appropriate manual provided by the machine tool builder for the actual operations.
3.3 INCREMENTAL FEED
X10 X100
X1 X1000
+C +Z +Y
+X–X
–C–Y –Z
RAPID
AXIS DIRECTION
OPERATIONB–64124EN/01 3. MANUAL OPERATION
469
In the handle mode, the tool can be minutely moved by rotating the manual pulse generator on the machine operator’s panel. Select the axis along which the tool is to be moved with the handle feed axis selection switches. The minimum distance the tool is moved when the manual pulse generator is rotated by one graduation is equal to the least input increment. Or the distance the tool is moved when the manual pulse generator is rotated by one graduation can be magnified by 1 times, 10 times, or by one of the two magnifications (total four magnifications) specified by parameters (No. 7113 and 7114). In addition to using parameters No. 7113 and No. 7114 to set arbitrary magnifications common to all axes, the user can use parameters No. 12350 and No. 12351 to set arbitrary magnifications independently for individual axes. When parameter No. 12350 has no value, parameter No. 7113 is used; when parameter No. 12351 has no value, parameter No. 7114 is used. These parameters are also valid for manual handle interruption.
Manual pulse generator
ÇÇ ÇÇ ÇÇ
Z
X
Y
Procedure for Manual Handle Feed
1 Press the HANDLE switch, one of the mode selection switches.
2 Select the axis along which the tool is to be moved by pressing a handle feed axis selection switch.
3 Select the magnification for the distance the tool is to be moved by pressing a handle feed magnification switch. The distance the tool is moved when the manual pulse generator is rotated by one graduation is: Least input increment multiplied by magnification.
4 Move the tool along the selected axis by rotating the handle. Rotating the handle 360 degrees moves the tool the distance equivalent to 100 graduations. The above is an example. Refer to the appropriate manual provided by the machine tool builder for the actual operations.
3.4 MANUAL HANDLE FEED
TEACHJOGHANDLE
MDIMEMORY REMOTE
ZERO RETURN
MODE
EDIT
Manual pulse generator
OPERATION3. MANUAL OPERATION B–64124EN/01
470
Parameter JHD (bit 0 of No. 7100) enables or disables the manual handle feed in the JOG mode. When the parameter JHD( bit 0 of No. 7100) is set 1,both manual handle feed and incremental feed are enabled.
Parameter THD (bit 1 of No. 7100) enables or disables the manual handle feed in the TEACH IN JOG mode.
Parameter HPF (bit 4 of No. 7100) or (No. 7117) specifies as follows:
� Parameter HPF (bit 4 of No. 7100)
Set value 0 : The feedrate is clamped at the rapid traverse rate and generated pulses exceeding the rapid traverse rate are ignored. (The distance the tool is moved may not match the graduations on the manual pulse generator.)
Set value 1 : The feedrate is clamped at the rapid traverse rate and generated pulses exceeding the rapid traverse rate are not ignored but accumulated in the CNC. (No longer rotating the handle does not immediately stop the tool. The tool is moved by the pulses accumulated in the CNC before it stops.)
� Parameter HPF (No. 7177) (It is available when parameter HPF is 0.)
Set value 0 : The feedrate is clamped at the rapid traverse rate and generated pulses exceeding the rapid traverse rate are ignored. (The distance the tool is moved may not match the graduations on the manual pulse generator.)
Other than 0 : The feedrate is clamped at the rapid traverse rate and generated pulses exceeding the rapid traverse rate are not ignored but accumulated in the CNC until the limit specified in parameter No. 7117 is reached. (No longer rotating the handle does not immediately stop the tool. The tool is moved by the pulses accumulated in the CNC before it stops.)
Parameter HNGx (No. 7102 #0) switches the direction of MPG in which the tool moves along an axis, corresponding to the direction in which the handle of the manual pulse generator is rotated.
��� � �����
� Availability of manual pulse generator in Jog mode (JHD)
� Availability of manual pulse generator in TEACH IN JOG mode (THD)
� A command to the MPG exceeding rapid traverse rate (HPF)
� Movement direction of an axis to the rotation of MPG (HNGX)
OPERATIONB–64124EN/01 3. MANUAL OPERATION
471
Up to three manual pulse generators can be connected, one for each axis. The three manual pulse generators can be simultaneously operated.
WARNING Rotating the handle quickly with a large magnification such as x100 moves the tool too fast. The feedrate is clamped at the rapid traverse feedrate.
NOTE Rotate the manual pulse generator at a rate of five rotations per second or lower. If the manual pulse generator is rotated at a rate higher than five rotations per second, the tool may not stop immediately after the handle is no longer rotated or the distance the tool moves may not match the graduations on the manual pulse generator.
������������
� Number of MPGs
OPERATION3. MANUAL OPERATION B–64124EN/01
472
Whether the distance the tool is moved by manual operation is added to the coordinates can be selected by turning the manual absolute switch on or off on the machine operator’s panel. When the switch is turned on, the distance the tool is moved by manual operation is added to the coordinates. When the switch is turned off, the distance the tool is moved by manual operation is not added to the coordinates.
O P1
P2
Y axis
X axis
Manual operation
The coordinates values change by the amount of manual operation.
Fig. 3.5 (a) Coordinates with the switch ON
X2
X1
Y1 Y2
P1
P2
O1
O2
The coordinates do not change.
 MANUAL OPERATION
473
The following describes the relation between manual operation and coordinates when the manual absolute switch is turned on or off, using a program example.
G01G90
X200.0Y150.0
X100.0Y100.0F010
X300.0Y200.0
; �
;
;
The subsequent figures use the following notation:
Movement of the tool when the switch is on Movement of the tool when the switch is off
The coordinates after manual operation include the distance the tool is moved by the manual operation. When the switch is off, therefore, subtract the distance the tool is moved by the manual operation.
Coordinates when block has been executed after manual operation (X–axis +20.0, Y–axis +100.0) at the end of movement of block �.
Y
X
(120.0 , 200.0) (220.0 , 250.0)
(200.0 , 150.0)
Switch OFF
Switch ON
(1��.0 , �00.0)
Manual operation
Coordinates when the feed hold button is pressed while block is being executed, manual operation (Y–axis + 75.0) is performed, and the cycle start button is pressed and released.
(300.0 , 275.0)
(300.0 , 200.0)(200.0 , 150.0) (150.0 , 125.0)
(150.0 , 200.0)
(200.0 , 225.0)
Y
X
Switch OFF
Switch ON
Manual operation
Explanation
� Manual operation after the end of block
� . �� � ���� ���� ����
���� ����
OPERATION3. MANUAL OPERATION B–64124EN/01
474
Coordinates when the feed hold button is pressed while block is being executed, manual operation (Y–axis +75.0) is performed, the control unit is reset with the RESET button, and block is read again
(300.0 , 275.0)
(200.0,150.0) (300.0 , 200.0)
(150.0 , 200.0) (200.0,225.0)
(150.0 , 125.0)(100.0 , 100.0)
Y
X Switch OFF
Switch ON
Manual operation
When there is only one axis in the following command, only the commanded axis returns.
Manual operation
N2
N1
N3
N1G01X100.0Y100.0F500; N2X200.0; N3Y150.0;
Y
X (100.0 , 100.0)
(200.0 , 100.0)
(200.0 , 150.0)
Switch OFF
Switch ON
When the following commands are incremental commands, operation is the same as when the switch is OFF.
When the switch is OFF After manual operation is performed with the switch OFF during cutter compensation, automatic operation is restarted then the tool moves parallel to the movement that would have been performed if manual movement had not been performed. The amount of separation equals to the amount that was performed manually.
Manual operation
Cutter path
Programmed path
Cutter path after manual operation
� When reset after a manual operation following a feed hold
� When a movement command in the next block is only one axis
� When the next move block is an incremental
� Manual operation during cutter compensation
OPERATIONB–64124EN/01 3. MANUAL OPERATION
475
When the switch is ON during cutter compensation Operation of the machine upon return to automatic operation after manual intervention with the switch is ON during execution with an absolute command program in the cutter compensation mode will be described. The vector created from the remaining part of the current block and the beginning of the next block is shifted in parallel. A new vector is created based on the next block, the block following the next block and the amount of manual movement. This also applies when manual operation is performed during cornering.
Manual operation performed in other than cornering Assume that the feed hold was applied at point PH while moving from PA to PB of programmed path PA, PB, and PC and that the tool was manually moved to PH’. The block end point PB moves to the point PB’ by the amount of manual movement, and vectors VB1 and VB2 at PB also move to VB1’ and VB2’. Vectors VC1 and VC2 between the next two blocks PB – PC and PC – PD are discarded and new vectors VC1’ and VC2’ (VC2’ = VC2 in this example) are produced from the relation between PB’ – PC and PC – PD. However, since VB2’ is not a newly calculated vector, correct offset is not performed at block PB’ – PC. Offset is correctly performed after PC.
VC1
VC2
PA
PD
PC
PH’
PB
VB2
VB1
VB2’
VC1’
PH
VB1’ Cutter path after manual operation
Programmed path (absolute command)
Manual operation
P’B
Cutter path before manual operation
OPERATION3. MANUAL OPERATION B–64124EN/01
476
Manual operation during cornering This is an example when manual operation is performed during cornering. VA2’, VB1’, and VB2’ are vectors moved in parallel with VA2, VB1 and VB2 by the amount of manual movement. The new vectors are calculated from VC1 and VC2. Then correct cutter compensation is performed for the blocks following Pc.
VB2
VB1
VC1
VC2
PA’
PCPB
VC1’
VA1VA2
VA2’ VA1’PH’
PH
PA
VB1’
VB2’
Cutter path after manual operation
Programmed path (absolute command)
Cutter path before manual operation
Manual operation
Manual operation after single block stop Manual operation was performed when execution of a block was terminated by single block stop. Vectors VB1 and VB2 are shifted by the amount of manual operation. Sub–sequent processing is the same as case a described above. An MDI operation can also be interveneted as well as manual operation. The movement is the same as that by manual operation.
VB2
VB1
VC1
VC2PC
PB’
VC1’
VB2’
VB1’
PB
PA
Cutter path after manual operation
Manual operation
Programmed path (absolute command)
Cutter path before manual operation
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
477
4 AUTOMATIC OPERATION Programmed operation of a CNC machine tool is referred to as automatic operation. This chapter explains the following types of automatic operation:
• MEMORY OPERATION Operation by executing a program registered in CNC memory
• MDI OPERATION Operation by executing a program entered from the MDI panel
DNC OPERATION Operation while reading a program from an input/output device
• PROGRAM RESTART Restarting a program for automatic operation from an intermediate point
• SCHEDULING FUNCTION Scheduled operation by executing programs (files) registered in an external input/output device (such as Handy File)
• SUBPROGRAM CALL FUNCTION Function for calling and executing subprograms (files) registered in an external input/output device (such as Handy File) during memory operation
• MANUAL HANDLE INTERRUPTION Function for performing manual feed during movement executed by automatic operation
• MIRROR IMAGE Function for enabling mirror–image movement along an axis during automatic operation
• MANUAL INTERVENTION AND RETURN Function restarting automatic operation by returning the tool to the position where manual intervention was started during automatic operation
• MEMORY CARD–BASED DNC OPERATION Automatic operation by a program written to a memory card
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
478
Programs are registered in memory in advance. When one of these programs is selected and the cycle start switch on the machine operator’s panel is pressed, automatic operation starts, and the cycle start LED goes on. When the feed hold switch on the machine operator’s panel is pressed during automatic operation, automatic operation is stopped temporarily. When the cycle start switch is pressed again, automatic operation is restarted.
When the RESET key on the MDI panel is pressed, automatic operation
terminates and the reset state is entered. The following procedure is given as an example. For actual operation, refer to the manual supplied by the machine tool builder.
Procedure for Memory Operation
1 Press the MEMORY mode selection switch.
2 Select a program from the registered programs. To do this, follow the steps below.
2–1 Press PROG to display the program screen.
2–2 Press address O .
2–3 Enter a program number using the numeric keys.
2–4 Press the [O SRH] soft key.
3 Press the cycle start switch on the machine operator’s panel. Automatic operation starts, and the cycle start LED goes on. When automatic operation terminates, the cycle start LED goes off.
4 To stop or cancel memory operation midway through, follow the steps below.
a. Stopping memory operation Press the feed hold switch on the machine operator’s panel. The feed hold LED goes on and the cycle start LED goes off. The machine responds as follows:
(i) When the machine was moving, feed operation decelerates and stops.
(ii) When dwell was being performed, dwell is stopped.
(iii) When M, S, or T was being executed, the operation is stopped after M, S, or T is finished.
When the cycle start switch on the machine operator’s panel is pressed while the feed hold LED is on, machine operation restarts.
4.1 MEMORY OPERATION
Procedure
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
479
b. Terminating memory operation
Press the RESET key on the MDI panel.
Automatic operation is terminated and the reset state is entered. When a reset is applied during movement, movement decelerates then stops.
After memory operation is started, the following are executed: (1) A one–block command is read from the specified program. (2) The block command is decoded. (3) The command execution is started. (4) The command in the next block is read. (5) Buffering is executed. That is, the command is decoded to allow
immediate execution. (6) Immediately after the preceding block is executed, execution of the
next block can be started. This is because buffering has been executed.
(7) Hereafter, memory operation can be executed by repeating the steps (4) to.(6)
Memory operation can be stopped using one of two methods: Specify a stop command, or press a key on the machine operator’s panel.
– The stop commands include M00 (program stop), M01 (optional stop), and M02 and M30 (program end).
– There are two keys to stop memory operation: The feed hold key and reset key.
Memory operation is stopped after a block containing M00 is executed. When the program is stopped, all existing modal information remains unchanged as in single block operation. The memory operation can be restarted by pressing the cycle start button. Operation may vary depending on the machine tool builder. Refer to the manual supplied by the machine tool builder.
Similarly to M00, memory operation is stopped after a block containing M01 is executed. This code is only effective when the Optional Stop switch on the machine operator’s panel is set to ON. Operation may vary depending on the machine tool builder. Refer to the manual supplied by the machine tool builder.
When M02 or M30 (specified at the end of the main program) is read, memory operation is terminated and the reset state is entered. In some machines, M30 returns control to the top of the program. For details, refer to the manual supplied by the machine tool builder.
When Feed Hold button on the operator’s panel is pressed during memory operation, the tool decelerates to a stop at a time.
Automatic operation can be stopped and the system can be made to the
reset state by using RESET key on the MDI panel or external reset signal.
When reset operation is applied to the system during a tool moving status, the motion is slowed down then stops.
Explanation
Memory operation
Stopping and terminating memory operation
� *��"� ���� (.)))
� 0����� � ���� (.)�)
� *��"� ���
�.)&/ .())
� ���� ����
� �����
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
480
When the optional block skip switch on the machine operator’s panel is turned on, blocks containing a slash (/) are ignored.
A file (subprogram) in an external input/output device such as a Floppy Cassette can be called and executed during memory operation. For details, see Section 4.6.
� Optional block skip
Calling a subprogram stored in an external input/output device
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
481
In the MDI mode, a program consisting of up to 10 lines can be created in the same format as normal programs and executed from the MDI panel. MDI operation is used for simple test operations. The following procedure is given as an example. For actual operation, refer to the manual supplied by the machine tool builder.
Procedure for MDI Operation
1 Press the MDI mode selection switch.
2 Press the PROG function key on the MDI panel to select the program
screen. The following screen appears:
PROGRAM ( MDI )
MDI * * * * * * * * * * 20 : 40 : 05
0010 00002
PRGRM CURRNT NEXT (OPRT)
O0000;
G00 G90 G94 G40 G80 G50 G54 G69 G17 G22 G21 G49 G98 G67 G64 G15
B H M T D F S
>_
MDI
Program number O0000 is entered automatically.
3 Prepare a program to be executed by an operation similar to normal program editing. M99 specified in the last block can return control to the beginning of the program after operation ends. Word insertion, modification, deletion, word search, address search, and program search are available for programs created in the MDI mode. For program editing, see III–9.
4 To entirely erase a program created in MDI mode,use one of the following methods:
a. Enter address O , then press the DELETE key on the MDI panel.
b. Alternatively, press the RESET key. In this case, set bit 7 of
parameter MCL No. 3203 to 1 in advance.
4.2 MDI OPERATION
Procedure
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
482
5 To execute a program, set the cursor on the head of the program. (Start from an intermediate point is possible.) Push Cycle Start button on the operator’s panel. By this action, the prepared program will start. When the program end (M02, M30) or ER(%) is executed, the prepared program will be automatically erased and the operation will end. By command of M99, control returns to the head of the prepared program.
O0001 N00003
MDI * * * * * * * * * * 12 : 42 : 39
PRGRM CURRNT NEXT (OPRT)
PROGRAM ( MDI ) G00 X100.0 Y200. ;
M03 ; G01 Z120.0 F500 ; M93 P9010 ; G00 Z0.0 ; %
G00 G90 G94 G40 G80 G50 G54 G69 G17 G22 G21 G49 G98 G67 G64 G15
B H M T D F S
>_
O0000
MDI
6 To stop or terminate MDI operation in midway through, follow the steps below.
a. Stopping MDI operation Press the feed hold switch on the machine operator’s panel. The feed hold LED goes on and the cycle start LED goes off. The machine responds as follows:
(i) When the machine was moving, feed operation decelerates and stops.
(ii) When dwell was being performed, dwell is stopped.
(iii) When M, S, or T was being executed, the operation is stopped after M, S, or T is finished.
When the cycle start switch on the machine operator’s panel is pressed, machine operation restarts.
b. Terminating MDI operation
Press the RESET key on the MDI panel.
Automatic operation is terminated and the reset state is entered. When a reset is applied during movement, movement decelerates then stops.
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
483
The previous explanation of how to execute and stop memory operation also applies to MDI operation, except that in MDI operation, M30 does not return control to the beginning of the program (M99 performs this function).
Programs prepared in the MDI mode will be erased in the following cases:
In MDI operation, if M02, M30 or ER(%) is executed. (If bit 6 (MER) of parameter No. 3203 is set to 1, however, the program is erased when execution of the last block of the program is completed by single–block operation.)
In MEMORY mode, if memory operation is performed. In EDIT mode, if any editing is performed. Background editing is performed.
When the O and DELETE keys were pressed.
Upon reset when bit 7 (MCL) of parameter No. 3203 is set to 1
After the editing operation during the stop of MDI operation was done, operation starts from the current cursor position.
A program can be edited during MDI operation. The editing of a program, however, is disabled until the CNC is reset, when bit 5 (MIE) of parameter No. 3203 is set accordingly.
Programs created in MDI mode cannot be registered.
A program can have as many lines as can fit on one page of the screen. A program consisting of up to six lines can be created. When parameter MDL (No. 3107 #7) is set to 0 to specify a mode that suppresses the display of continuous–state information, a program of up to 10 lines can be created. If the created program exceeds the specified number of lines, % (ER) is deleted (prevents insertion and modification).
Calls to subprograms (M98) can be specified in a program created in the MDI mode. This means that a program registered in memory can be called and executed during MDI operation. In addition to the main program executed by automatic operation, up to four levels of subprogram nesting are allowed.
Main program Subprogram
One–level nesting Two–level nesting
O0000;
M98P 1000;
M30;
O1000; O2000;
M98P M98P2000; 3000;
M99; M99;
Subprogram
Fig. 4.2 Nesting level of subprograms called from the MDI program
Explanation
� � ���" ��� ���"�
� ���� ��
� Editing a program during MDI operation
Limitations
� Program registration
� Number of lines in a program
� Subprogram nesting
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
484
Macro programs can also be created, called, and executed in the MDI mode. However, macro call commands cannot be executed when the mode is changed to MDI mode after memory operation is stopped during execution of a subprogram.
When a program is created in the MDI mode, an empty area in program memory is used. If program memory is full, no programs can be created in the MDI mode.
� . ��� � ��
� .� ��! ��
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
485
By activating automatic operation during the DNC operation mode (RMT), it is possible to perform machining (DNC operation) while a program is being read in via reader/puncher interface, or remote buffer. It is possible to select files (programs) saved in an external input/output unit of a floppy format (such as Handy File) and specify (schedule) the sequence and frequency of execution for automatic operation. (see III–4.5) To use the DNC operation function, it is necessary to set the parameters related to the reader/punch interface, and remote buffer in advance.
DNC OPERATION
1 Search for the program (file) to be executed.
2 Press the REMOTE switch on the machine operator’s panel to set RMT mode, then press the cycle start switch. The selected file is executed. For details of the use of the REMOTE switch, refer to the relevant manual supplied by the machine tool builder.
PROGRAM CHECK O0001 N00020
O0010 ; G92 G90 X100 Y200 Z50 ; G00 X0 Y0 Z0 ; G01 Z250 F1000 (RELATIVE) (DIST TO GO) G00 G94 G80 X 100.000 X 0.000 G17 G21 G98 Y 100.000 Y 0.000 G90 G49 G80 Z 0.000 Z 0.000 G22 G49 G67 A 0.000 A 0.000 B C 0.000 C 0.000 H M HD.T NX.T D M F S M ACT.F SACT REPEAT RMT STRT MTN *** *** 21:20:05 [ ABS ] [ REL ] [ ] [ ] [ (OPRT) ]
� Program check screen
PROGRAM O0001 N00020
N020 X100.0 Z100.0 (DNC–PROG) ; N030 X200.0 Z200.0 ; N040 X300.0 Z300.0 ; N050 X400.0 Z400.0 ; N060 X500.0 Z500.0 ; N070 X600.0 Z600.0 ; N080 X700.0 Z400.0 ; N090 X800.0 Z400.0 ; N100 x900.0 z400.0 ; N110 x1000.0 z1000.0 ; N120 x800.0 z800.0 ;
RMT STRT MTN *** *** 21:20:05 [ PRGRM ] [ CHECK ] [ ] [ ] [ (OPRT) ]
� Program screen
4.3 DNC OPERATION
*��������
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
486
During DNC operation, the program currently being executed is displayed on the program check screen and program screen. The number of displayed program blocks depends on the program being executed. Any comment enclosed between a control–out mark “(” and control–in mark “)” within a block is also displayed.
� During DNC operation, programs stored in memory can be called.
� During DNC operation, macro programs stored in memory can be called.
In program display, no more than 256 characters can be displayed. Accordingly, character display may be truncated in the middle of a block.
In DNC operation, M198 cannot be executed. If M198 is executed, P/S alarm No. 210 is issued.
In DNC operation, custom macros can be specified, but no repeat instruction and branch instruction can be programmed. If a repeat instruction or branch instruction is executed, P/S alarm No. 123 is issued. When reserved words (such as IF, WHILE, COS, and NE) used with custom macros in DNC operation are displayed during program display, a blank is inserted between adjacent characters.
Example [During DNC operation]
#102=SIN[#100] ; → #102 = S I N[#100] ; IF[#100NE0]GOTO5 ; → I F[#100NE0] G O T O 5 ;
When control is returned from a subprogram or macro program to the calling program during DNC operation, it becomes impossible to use a return command (M99P****) for which a sequence number is specified.
Number Message Contents
086 DR SIGNAL OFF When entering data in the memory by using Reader / Puncher interface, the ready signal (DR) of reader / puncher was turned off. Power supply of I/O unit is off or cable is not connected or a P.C.B. is defective.
123 CAN NOT USE MACRO COMMAND IN DNC
Macro control command is used during DNC operation. Modify the program.
210 CAN NOT COMAND M198/M199
Or M198 is executed in the DNC opera- tion. Modify the program.
Explanations
Limitations
� Limit on number of characters
� M198 (command for calling a program from within an external input/output unit)
� Custom macro
� M99
Alarm
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
487
This function specifies Sequence No. of a block to be restarted when a tool
is broken down or when it is desired to restart machining operation after
a day off, and restarts the machining operation from that block. It can also
be used as a high–speed program check function.
There are two restart methods: the P–type method and Q–type method.
P TYPE Operation can be restarted anywhere. This restart method is used when operation is stopped because of a broken tool.
Program start point (machining start point)
Restart position
Return operation
ÇÇ ÇÇ
Q TYPE Before operation can be restarted, the machine must be moved to the programmed start point (machining start point)
ÇÇ ÇÇ ÇÇ
Program start point (machining start point)
Return operation
Restart position
4.4 PROGRAM RESTART
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
488
Procedure for Program Restart by Specifying a Sequence Number
1 Retract the tool and replace it with a new one. When necessary, change the offset. (Go to step 2.)
1 When power is turned ON or emergency stop is released, perform all necessary operations at that time, including the reference position return.
2 Move the machine manually to the program starting point (machining start point), and keep the modal data and coordinate system in the same conditions as at the machining start.
3 If necessary, modify the offset amount.
1 Turn the program restart switch on the machine operator’s panel ON.
2 Press PROG key to display the desired program.
3 Find the program head.
4 Enter the sequence number of the block to be restarted, then press th [P TYPE] or [Q TYPE] soft key.
If the same sequence number appears more than once, the location of the target block must be specified. Specify a frequency and a sequence number.
Procedure 1
[ P TYPE ]
[ Q TYPE ]
Procedure 2
[COMMON TO P TYPE / Q TYPE]
� �����
Sequence number
���
[Q TYPE]
or
[P TYPE] Frequency
� �����
Sequence number
[P TYPE]
or
[Q TYPE]
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
489
5 The sequence number is searched for, and the program restart screen appears on the CRT display.
PROGRAM RESTART
DESTINATION X 57. 096 Y 56. 877 Z 56. 943
M 1 2 1 2 1 2 1 2 1 2 1 * * * * * * * *
* * * * * * * ** * * * * * * *
T * * * * * * * ** * * * * * * *
S * * * * *
O0002 N01000
S 0 T0000
MEM * * * * * * * * * * 10 : 10 : 40
(OPRT)RSTR
DISTANCE TO GO 1 X 1. 459 2 Y 10. 309 3 Z 7. 320
DIR
DESTINATION shows the position at which machining is to restart. DISTANCE TO GO shows the distance from the current tool position to the position where machining is to restart. A number to the left of each axis name indicates the order of axes (determined by parameter setting) along which the tool moves to the restart position. The coordinates and amount of travel for restarting the program can be displayed for up to five axes. If your system supports six or more axes, pressing the [RSTR] soft key again displays the data for the sixth and subsequent axes. (The program restart screen displays only the data for CNC–controlled axes.) M: Fourteen most recently specified M codes T: Two most recently specified T codes S: Most recently specified S code B: Most recently specified B code Codes are displayed in the order in which they are specified. All codes are cleared by a program restart command or cycle start in the reset state.
6 Turn the program re–start switch OFF. At this time, the figure at the left side of axis name DISTANCE TO GO blinks.
7 Check the screen for the M, S, T, and B codes to be executed. If they are found, enter the MDI mode, then execute the M, S, T, and B functions. After execution, restore the previous mode. These codes are not displayed on the program restart screen.
8 Check that the distance indicated under DISTANCE TO GO is correct. Also check whether there is the possibility that the tool might hit a workpiece or other objects when it moves to the machining restart position. If such a possibility exists, move the tool manually to a position from which the tool can move to the machining restart position without encountering any obstacles.
9 Press the cycle start button. The tool moves to the machining restart position at the dry run feedrate sequentially along axes in the order specified by parameter settings (No. 7310). Machining is then restarted.
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
490
Procedure for Program Restart by Specifying a Block Number
1 Retract the tool and replace it with a new one. When necessary, change the offset. (Go to step 2.)
1 When power is turned ON or emergency stop is released, perform all necessary operations at that time, including the reference position return.
2 Move the machine manually to the program starting point (machining start point), and keep the modal data and coordinate system in the same conditions as at the machining start.
3 If necessary, modify the offset amount.
1 Turn the program restart switch on the machine operator’s panel ON.
2 Press PROG key to display the desired program.
3 Find the program head. Press function RESET key.
4 Enter the number of the block to be restarted then press the [P TYPE] or [Q TYPE] soft key. The block number cannot exceed eight digits.
5 The block number is searched for, and the program restart screen appears on the display.
PROGRAM RESTART
DESTINATION X 57. 096 Y 56. 877 Z 56. 943
DISTANCE TO GO X 1. 459 Y 10. 309 Z 7. 320
M 1 2 1 2 1 2 1 2 1 2 1 * * * * * * * *
* * * * * * * ** * * * * * * *
T * * * * * * * ** * * * * * * *
S * * * * *
O0002 N01000
S 0 T0000
MEM * * * * * * * * * * 10 : 10 : 40
FL.SDL (OPRT)RSTR DIR
DESTINATION shows the position at which machining is to restart. DISTANCE TO GO shows the distance from the current tool position to the position where machining is to restart. A number to the left of each axis name indicates the order of axes (determined by parameter setting) along which the tool moves to the restart position.
Procedure 1
[ P TYPE ]
[ Q TYPE ]
Procedure 2
[COMMON TO P TYPE / Q TYPE]
� � � � � � � � �
Block number
[P TYPE]
or
[Q TYPE]
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
491
The coordinates and amount of travel for restarting the program can be displayed for up to five axes. If your system supports six or more axes, pressing the [RSTR] soft key again displays the data for the sixth and subsequent axes. (The program restart screen displays only the data for CNC–controlled axes.) M: Fourteen most recently specified M codes T: Two most recently specified T codes S: Most recently specified S code B: Most recently specified B code Codes are displayed in the order in which they are specified. All codes are cleared by a program restart command or cycle start in the reset state.
6 Turn the program re–start switch OFF. At this time, the figure at the left side of axis name DISTANCE TO GO blinks.
7 Check the screen for the M, S, T, and B codes to be executed. If they are found, enter the MDI mode, then execute the M, S, T, and B functions. After execution, restore the previous mode. These codes are not displayed on the program restart screen.
8 Check that the distance indicated under DISTANCE TO GO is correct. Also check whether there is the possibility that the tool might hit a workpiece or other objects when it moves to the machining restart position. If such a possibility exists, move the tool manually to a position from which the tool can move to the machining restart position without encountering any obstacles.
9 Press the cycle start button. The tool moves to the machining restart position at the dry run feedrate sequentially along axes in the order specified by parameter settings (No. 7310). Machining is then restarted.
When the CNC is stopped, the number of executed blocks is displayed on the program screen or program restart screen. The operator can specify the number of the block from which the program is to be restarted, by referencing the number displayed on the CRT. The displayed number indicates the number of the block that was executed most recently. For example, to restart the program from the block at which execution stopped, specify the displayed number, plus one.
The number of blocks is counted from the start of machining, assuming one NC line of a CNC program to be one block.
< Example 1 >
CNC Program Number of blocks
O 0001 ; G90 G92 X0 Y0 Z0 ; G01 X100. F100 ; G03 X01 –50. F50 ; M30 ;
1 2 3 4 5
Explanations
� Block number
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
492
< Example 2 >
CNC Program Number of blocks
O 0001 ; G90 G92 X0 Y0 Z0 ; G90 G00 Z100. ; G81 X100. Y0. Z–120. R–80. F50. ; #1 = #1 + 1 ; #2 = #2 + 1 ; #3 = #3 + 1 ; G00 X0 Z0 ; M30 ;
1 2 3 4 4 4 4 5 6
Macro statements are not counted as blocks.
The block number is held in memory while no power is supplied. The number can be cleared by cycle start in the reset state.
The program screen usually displays the number of the block currently being executed. When the execution of a block is completed, the CNC is reset, or the program is executed in single–block stop mode, the program screen displays the number of the program that was executed most recently. When a CNC program is halted or stopped by feed hold, reset, or single–block stop, the following block numbers are displayed:
Feed hold : Block being executed Reset : Block executed most recently Single–block stop : Block executed most recently
For example, when the CNC is reset during the execution of block 10, the displayed block number changes from 10 to 9.
When MDI intervention is performed while the program is stopped by single–block stop, the CNC commands used for intervention are not counted as a block.
When the block number displayed on the program screen exceeds eight digits, the block number is reset to 0 and counting continues.
Under any of the following conditions, P–type restart cannot be performed:
⋅ When automatic operation has not been performed since the power was turned on
⋅ When automatic operation has not been performed since an emergency stop was released
⋅ When automatic operation has not been performed since the coordinate system was changed or shifted (change in an external offset from the workpiece reference point)
The block to be restarted need not be the block which was interrupted; operation can restart with any block. When P–type restart is performed, the restart block must use the same coordinate system as when operation was interrupted.
� Storing / clearing the block number
� Block number when a program is halted or stopped
� MDI intervention
� Block number exceeding eight digits
Limitations
� P–type restart
� ���� �� ����%
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
493
When single block operation is ON during movement to the restart position, operation stops every time the tool completes movement along an axis. When operation is stopped in the single block mode, MDI intervention cannot be performed.
During movement to the restart position, manual intervention can be used to perform a return operation for an axis if it has not yet been performed for the axis. A return operation cannot be done further on axes for which a return has already been completed.
Never reset during the time from the start of a search at restart until machining is restarted. Otherwise, restart must be performed again from the first step.
Regardless of whether machining has started or not, manual operation must be performed when the manual absolute mode is on.
If no absolute–position detector (absolute pulse coder) is provided, be sure to perform reference position return after turning on the power and before performing restart.
Alarm No. Contents
071 The specified block number for restarting the program is not found.
094 After interruption, a coordinate system was set, then P–type restart was specified.
095 After interruption, the coordinate system shift was changed, then P–type restart was specified.
096 After interruption, the coordinate system was changed, then P–type restart was specified.
097
When automatic operation has not been performed since the power was turned on, emergency stop was released, or P/S alarm 094 to 097 was reset, P–type restart was speci- fied.
098 After the power was turned on, restart operation was per- formed without reference position return, but a G28 com- mand was found in the program.
099 A move command was specified from the MDI panel during a restart operation.
5020 An erroneous parameter was specififed for restarting a pro- gram.
WARNING As a rule, the tool cannot be returned to a correct position under the following conditions. Special care must be taken in the following cases since none of them cause an alarm: Manual operation is performed when the manual absolute mode is OFF. Manual operation is performed when the machine is locked. When the mirror image is used. When manual operation is performed in the course of axis movement for returning operation. When the program restart is commanded for a block between the block for skip cutting and
subsequent absolute command block.
� -��"�� ����%
� . �� � ������������
� �����
� . �� � �������
� ��������� �������� ������
Alarm
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
494
The schedule function allows the operator to select files (programs)
registered on a floppy–disk in an external input/output device (such as
Handy File) and specify the execution order and number of repetitions
(scheduling) for performing automatic operation.
It is also possible to select only one file from the files in the external
input/output device and execute it during automatic operation.
FILE DIRECTORY
FILE NO. FILE NAME
0001 O0010 0002 O0020 0003 O0030 0004 O0040
Set file number and number of repetitions.
ORDER FILE NO REPETITION
01 0002 2 02 0003 1 03 0004 3 04 0001 2
Scheduling screen
Executing automatic operation
List of files in an external input/output device
4.5 SCHEDULING FUNCTION
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
495
Procedure for Scheduling Function
1 Press the MEMORY switch on the machine operator’s panel, then
press the PROG function key on the MDI panel.
2 Press the rightmost soft key (continuous menu key), then press the [FL. SDL] soft key. A list of files registered in the Floppy Cassette is displayed on screen No. 1. To display more files that are not displayed on this screen, press the page key on the MDI panel. Files registered in the Floppy Cassette can also be displayed successively.
FILE DIRECTORY O0001 N00000
MEM * * * * * * * * * * 19 : 14 : 47
PRGRM (OPRT)
CURRENT SELECTED : SCHEDULE NO. FILE NAME (METER) VOL 0000 SCHEDULE 0001 PARAMETER 58.5 0002 ALL PROGRAM 11.0 0003 O0001 1.9 0004 O0002 1.9 0005 O0010 1.9 0006 O0020 1.9 0007 O0040 1.9 0008 O0050 1.9
SCHDUL
Screen No.1
DIR
3 Press the [(OPRT)] and [SELECT] soft keys to display “SELECT FILE NO.” (on screen No. 2). Enter a file number, then press the [F SET] and [EXEC] soft keys. The file for the entered file number is selected, and the file name is indicated after “CURRENT SELECTED:”.
O0001 N00000
MEM * * * * * * * * * * 19 : 17 : 10
FILE DIRECTORY
CURRENT SELECTED:O0040 NO.  AUTOMATIC OPERATION B–64124EN/01
496
4 Press the REMOTE switch on the machine operator’s panel to enter the RMT mode, then press the cycle start switch. The selected file is executed. For details on the REMOTE switch, refer to the manual supplied by the machine tool builder. The selected file number is indicated at the upper right corner of the screen as an F number (instead of an O number).
F0007 N00000
RMT * * * * * * * * * * 13 : 27 : 54
FILE DIRECTORY
CURRENT SELECTED:O0040
PRGRM (OPRT)SCHDUL
Screen No.3
DIR
1 Display the list of files registered in the Floppy Cassette. The display procedure is the same as in steps 1 and 2 for executing one file.
2 On screen No. 2, press the [(OPRT)] and [SELECT] soft keys to display “SELECT FILE NO.”
3 Enter file number 0, and press the [F SET], and [EXEC] soft keys. “SCHEDULE” is indicated after “CURRENT SELECTED:”.
4 Press the leftmost soft key (return menu key) and the [SCHDUL] soft key. Screen No. 4 appears.
F0000 N02000
MEM * * * * * * * * * * 22 : 07 : 00
FILE DIRECTORY
ORDER FILE NO. REQ.REP CUR.REP 01 02 03 04 05 06 07 08 09 10
>_
PRGRM DIR
Screen No.4
SCHDUL (OPRT)
� Procedure for executing the scheduling function
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
497
Move the cursor and enter the file numbers and number of repetitions in the order in which to execute the files. At this time, the current number of repetitions “CUR.REP” is 0.
5 Press the REMOTE switch on the machine operator’s panel to enter the RMT mode, then press the start switch. The files are executed in the specified order. When a file is being executed, the cursor is positioned at the number of that file. The current number of repetitions CUR.REP is increased when M02 or M30 is executed in the program being run.
O0000 N02000
RMT * * * * * * * * * * 10 : 10 : 40
FILE DIRECTORY
ORDER FILE NO. REQ.REP CUR.REP 01 5 5 02 0003 23 23 03 0004 9999 156 04 0005 LOOP 0 05 06 07 08 09 10
PRGRM (OPRT)DIR
Screen No.5
SCHDUL
0007
If no file number is specified on screen No. 4 (the file number field is left blank), program execution is stopped at that point. To leave the file
number field blank, press numeric key 0 then INPUT .
If a negative value is set as the number of repetitions, <LOOP> is displayed, and the file is repeated indefinitely.
When the [(OPRT)], [CLEAR], and [EXEC] soft keys are pressed on screen No. 4, all data is cleared. However, these keys do not function while a file is being executed.
When the soft key [PRGRM] is pressed on screen No. 1, 2, 3, 4, or 5, the program screen is displayed.
Up to 9999 can be specified as the number of repetitions. If 0 is set for a file, the file becomes invalid and is not executed.
By pressing the page key on screen No. 4, up to 20 files can be registered.
When M codes other than M02 and M30 are executed in a program, the current number of repetitions is not increased.
Explanations
� Specifying no file number
� Endless repetition
� Clear
� Return to the program screen
Restrictions
� Number of repetitions
� Number of files registered
� M code
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
498
During the execution of file, the floppy directory display of background editing cannot be referenced.
To resume automatic operation after it is suspended for scheduled operation, press the reset button.
Alarm No. Description
086 An attempt was made to execute a file that was not regis- tered in the floppy disk.
210 M198 and M099 were executed during scheduled opera- tion, or M198 was executed during DNC operation.
� Displaying the floppy disk directory during file execution
� ���� ����" ��� ���
���� ����
�� �
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
499
The subprogram call function is provided to call and execute subprogram
files stored in an external input/output device(Handy File, FLOPPY
CASSETTE, FA Card)during memory operation.
When the following block in a program in CNC memory is executed, a
subprogram file in the external input/output device is called:
1. FS10/11 tape format
M198 P���� L∆∆∆∆ ;
Number of repetitions
File number for a file in the I/O device
I/O devices call instruction
2. Other than FS10/11 tape format
M198 P���� ∆∆∆∆ ;
Number of repetitions
I/O devices call instruction
File number for a file in the I/O device
The subprogram call function is enabled when parameter No.0102 for the input/output device is set to 3. Either format 1 or 2 can be used. A different M code can be used for a subprogram call depending on the setting of parameter No.6030. In this case, M198 is executed as a normal M code. The file number is specified at address P. If the SBP bit (bit 2) of parameter No.3404 is set to 1, a program number can be specified. When a file number is specified at address P, Fxxxx is indicated instead of Oxxxx.
Programs in memory execution mode
�� �
�� � ���� ���� -'�� (+���
�� ��=@ 8���� ���� �
�> �
�5 �
: First call/return
: Second call/return
: Third call/return
Program in the external input/output device
Fig. 4.6 Program flow when m198 is specified
4.6 SUBPROGRAM CALL FUNCTION (M198)
Format
Explanation
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
500
NOTE 1 When M198 in the program of the file saved in a floppy
cassette is executed, a P/S alarm (No.210) is given. When a program in the memory of CNC is called and M198 is executed during execution of a program of the file saved in a floppy cassette, M198 is changed to an ordinary M–code.
� When MDI is intervened and M198 is executed after M198 is commanded in the memory mode, M198 is changed to an ordinary M–code. When the reset operation is done in the MDI mode after M198 is commanded in the MEMORY mode, it does not influence on the memory operation and the operation is continued by restarting it in the MEMORY mode.
Restrictions
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
501
The movement by manual handle operation can be done by overlapping it with the movement by automatic operation in the automatic operation mode.
�
Programmed depth of cut
Depth of cut by handle interruption
Tool position after handle interruption
Tool position during automatic operation
Fig. 4.7 Manual handle interruption
� Handle interruption axis selection signals For the handle interruption axis selection signals, refer to the manual supplied by the machine tool builder.
During automatic operation, handle interruption is enabled for an axis if the handle interruption axis selection signal for that axis is on. Handle interruption is performed by turning the handle of the manual pulse generator.
WARNING The travel distance by handle interruption is determined according to the amount by which the manual pulse generator is turned and the handle feed magnification (x1, x10, xM, xN). Since this movement is not accelerated or decelerated, it is very dangerous to use a large magnification value for handle interruption. The move amount per scale at x1 magnification is 0.001 mm (metric output) or 0.0001 inch (inch output).
NOTE Handle interruption is disabled when the machine is locked during automatic operation.
4.7 MANUAL HANDLE INTERRUPTION
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
502
The following table indicates the relation between other functions and the movement by handle interrupt.
Display Relation
Machine lock Machine lock is effective. The tool does not move even when this signal turns on.
Interlock Interlock is effective. The tool does not move even when this signal turns on.
Mirror image Mirror image is not effective. Interrupt functions on the plus direction by plus direction command, even if this signal turns on.
The following table shows the relation between various position display data and the movement by handle interrupt.
Display Relation
Absolute coordinate value
Handle interruption does not change absolute coordinates.
Relative coordinate value
Handle interruption does not change relative coordinates.
Machine coordinate value
Machine coordinates are changed by the travel distance specified by handle interruption.
Press the function key POS , then press the chapter selection soft key
[HNDL]. The move amount by the handle interrupt is displayed. The following 4 kinds of data are displayed concurrently.
O0000 N02000
MDI * * * * * * * * * * 10 : 29 : 51
HANDLE INTERRUPTION
(INPUT UNIT) (OUTPUT UNIT) X 69.594 X 69.594 Y 137.783 Y 137.783 Z –61.439 Z –61.439
(RELATIVE) X 0.000 X 0.000 Y 0.000 Y 0.000 Z 0.000 Z 0.000
(DISTANCE TO GO)
PART COUNT 287 RUN TIME 1H 12M CYCLE TIME 0H 0M 0S
ABS REL ALL (OPRT)HNDL
Explanations
� Relation with other functions
� Position display
� Travel distance display
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
503
(a) INPUT UNIT : Handle interrupt move amount in input unit system Indicates the travel distance specified by handle interruption according to the least input increment.
(b) OUTPUT UNI : Handle interrupt move amount in output unit system
Indicates the travel distance specified by handle interruption according to the least command increment.
(c) RELATIVE : Position in relative coordinate system These values have no effect on the travel distance
specified by handle interruption.
(d) DISTANCE TO GO : The remaining travel distance in the current block has no effect on the travel distance specified by handle interruption.
The handle interrupt move amount is cleared when the manual reference position return ends every axis.
By setting bit 2 (IHD) of parameter No. 7100 and bit 5 (HIE) of parameter No. 7103 to 1, acceleration/deceleration for manual handle interruption can always be of the acceleration/deceleration type for manual feed, without being affected by automatic operation or some other mode. More specifically, the acceleration/deceleration type set with bit 4 (JGLx) of parameter No. 1610 and bit 0 (CTLx) of parameter No. 1610 is applied. Set a time constant with parameter No. 1624, and an FL feedrate with parameter No. 1625.
� Independent acceleration/deceleration
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
504
During automatic operation, the mirror image function can be used for
movement along an axis. To use this function, set the mirror image switch
to ON on the machine operator’s panel, or set the mirror image setting to
ON from the MDI panel.
Y
X
Y–axis mirror image goes on.
Programmed tool path
Tool path after the mirror image function is used
Tool
Fig. 4.8 Mirror image
The following procedure is given as an example. For actual operation, refer to the manual supplied by the machine tool builder.
1 Press the single block switch to stop automatic operation. When the mirror image function is used from the begining of operation, this step is omitted.
2 Press the mirror image switch for the target axis on the machine operator’s panel. Alternatively, turn on the mirror image setting by following the steps below:
2–1 Set the MDI mode.
2–2 Press the OFFSETSETTING function key.
2–3 Press the [SETING] soft key for chapter selection to display the setting screen.
SETTING (MIRROR IMAGE) O0020 N00001
MEM * * * * * * * * * * 14 : 47 : 57
MIRROR IMAGE X = (0 : OFF 1 : ON) MIRROR IMAGE Y = 0 (0 : OFF 1 : ON) MIRROR IMAGE Z = 0 (0 : OFF 1 : ON)
OFFSET WORK (OPRT)
>_
1
SETING
4.8 MIRROR IMAGE
Procedure
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
505
2–4 Move the cursor to the mirror image setting position, then set the target axis to 1.
3 Enter an automatic operation mode (memory mode or MDI mode), then press the cycle start button to start automatic operation.
� The mirror image function can also be turned on and off by setting bit 0 of parameter 0012 (MIRx) to 1 or 0.
� For the mirror image switches, refer to the manual supplied by the machine tool builder.
The direction of movement during manual operation, the direction of movement from an intemidiate point to the reference position during automatic reference position return (G28), the direction of approach during unidirectional positioning (G60), and the shift direction in a boring cycle (G76, G87) cannot be reserved.
Explanations
Limitations
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
506
In cases such as when tool movement along an axis is stopped by feed hold during automatic operation so that manual intervention can be used to replace the tool: When automatic operation is restarted, this function returns the tool to the position where manual intervention was started. To use the conventional program restart function and tool withdrawal and return function, the switches on the operator’s panel must be used in conjunction with the MDI keys. This function does not require such operations.
Before this function can be used, MIN (bit 0 of parameter No. 7001) must be set to 1.
In manual absolute off mode, the tool does not return to the stop position, but instead operates according to the manual absolute on/off function.
For the return operation, the dry run feedrate is used, and the jog feedrate override function is enabled.
Return operation is performed according to positioning based on nonlinear interpolation.
If the single block stop switch is on during return operation, the tool stops at the stop position and restarts movement when the cycle start switch is pressed.
If a reset occurs or an alarm is issued during manual intervention or the return operation, this function is cancelled.
This function can be used in the MDI mode as well.
This function is enabled only when the automatic operation hold LED is on. When there is no travel distance remaining, this function has no effect even if a feed hold stop is performed with the automatic operation hold signal *SP (bit 5 of G008).
When the tool is replaced using manual intervention for a reason such as damage, the tool movement cannot be restarted by a changed offset in the middle of the interrupted block.
When performing manual intervention, never use the machine lock, mirror image, or scaling functions.
4.9 MANUAL INTERVENTION AND RETURN
Explanations
� Manual absolute on/off
� Override
� Return operation
� Single block
� Cancellation
� MDI mode
Limitations
� Enabling and disabling manual intervention and return
� Offset
� Machine lock, mirror image, and scaling
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
507
N1
N2
N1 Point A
N2
N1 Point A
N2
Point B
N1 Point A
N2
B
1. The N1 block cuts a workpiece
Tool
Block start point
2. The tool is stopped by pressing the feed hold switch in the middle of the N1 block (point A).
3. After retracting the tool manually to point B, tool movement is restarted.
4. After automatic return to point A at the dry run feedrate, the remaining move command of the N1 block is executed.
Manual intervention
WARNING When performing manual intervention, pay particular attention of machining and the shape of the workpiece so that the machine and tool are not damaged.
Example
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
508
“DNC operation with Memory Card” is a function that it is possible to perform machining with executing the program in the memory card, which is assembled to the memory card interface, where is the left side of the screen.
There are two methods to use this function as follows.
(a) By starting automatic operation (cycle start) during the DNC operation mode (RMT), it is possible to perform machining (DNC operation) while a program is being read from a memory card, as by using the external input/output unit such as a floppy cassette and so on. (Fig. 4.10.1 (a))
(b) It is possible to read sub–programs written in the memory card and execute them by the command Subprogram call (M198). (Fig. 4.10.1 (b))
It is possible to do the DNC operation with Memory card instead of the normal memory operation by memory in the CNC.
Memory in CNC (Program)
Memory Card (Program)
Execution of programs
Normal Memory operation by memory in the CNC
DNC operation with Memory card
Fig. 4.10.1 (a)
It is possible to execute the subprogram in the memory card during memory operation.
Memory in CNC (Program)
Memory Card (Sub Program)
Execution of programs
Normal Memory operation by memory in the CNC
Subprogram Call (M198)
Fig. 4.10.1 (b)
4.10 DNC OPERATION WITH MEMORY CARD
4.10.1 Specification
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
509
NOTE To use this function, it is necessary to set the parameter of No.20 to 4 by setting screen. No.20 [I/O CHANEL: Setting to select an input/output unit] Setting value is 4.: It means using the memory card interface.
Please set the parameter of No.0020 to 4 in the setting screen in advance.
(1)Change to RMT mode.
(2)Push [PROG] function key.
(3)Push [ > ] soft key (continuance menu).
(4)When [DNC–CD] soft key is pushed, the following screen is displayed.
(5)The screen can be scrolled by page key. An arbitrary file number is input, and [F SRH] soft key is pushed. Then the arbitrary file name is displayed at the top of DNC operation (memory card) screen.
(6)When the file number that is executed is input and the [DNC–ST] soft key is pushed, the file name that is selected is set to DNC FILE.
(7)When the cycle start is done, the program that is selected is executed.
4.10.2 Operations
<IP_ADDRESS> DNC Operation
Procedure
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
510
When the following block in a program in CNC memory is executed, a subprogram file in memory card is called.
1. Normal format
M198 P���� ∆∆∆∆ ;
File number for a file in the memory card
Number of repetition Memory card call instruction
2. FS15 tape format
M198 P���� L∆∆∆∆ ;
File number for a file in the memory card
Memory card call instruction
File number of repetition
Both format 1 and 2 can be used. A different M code can be used for a subprogram call depending on the setting of parameter No. 6030. In this case, M198 is executed as a normal M code. The file number is specified at address P. If the SBP (bit 2) of parameter No. 3404 is set to 1, a program number can be specified. When a file number is specified at address P, Fxxxx is indicated instead of Oxxxx.
NOTE Please set the parameter of No. 0020 to 4 in the setting screen in advance.
<IP_ADDRESS> Subprogram Call (M198)
Format
Explanation
OPERATIONB–64124EN/01 4. AUTOMATIC OPERATION
511
(1)The memory card can not be accessed, such as display of memory card list and so on, during the DNC operation with memory card.
(2)The selection of DNC operation file that is set at DNC OPERATION screen is cleared by the power supply turn off and on. After the power supply is turned on again, it is necessary to select the DNC operation file again.
(3)Please do not pull out and insert memory card during the DNC operation with memory card.
(4) It is not possible to call a program in the memory card from the DNC operation program.
(5)When this function is used, secure the memory card by following the procedure described later, to prevent the card from becoming disconnected or poorly connected due to vibration during operation or for some other reason.
#7 DNM0138
#6 #5 #4 #3 #2 #1 #0
[Data type] Bit
#7 (DNM) The DNC operation with memory card function is 0 : disable.
1 : enable.
Follow the procedure below to fix the memory card.
1. Inserting the memory card into the fixing bracket
Insert the memory card into the fixing bracket in the direction indicated by the arrow.
Fix the memory card to the fixing bracket.
Fix the card at this point.
4.10.3 Limitation and Notes
4.10.4 Parameter
4.10.5 Procedure for Fixing the Memory Card
OPERATION4. AUTOMATIC OPERATION B–64124EN/01
512
2. Inserting the card into the PCMCIA port.
Loosen the screw of the fixing bracket and insert the memory card into the PCMCIA port with the claw of the fixing bracket raised.
Align the claw of the fixing bracket with the groove of the PCMCIA port and then push the bracket in the direction indicated by the arrow.
Tighten the screw of the bracket to fix the memory card.
Align the claw with the groove.
Push the bracket to the right.
Fix the card by tightening the screw.
OPERATIONB–64124EN/01 5. TEST OPERATION
513
5 # -# 0* ��#608 The following functions are used to check before actual machining whether the machine operates as specified by the created program.
5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK 5.2 FEEDRATE OVERRIDE 5.3 RAPID TRAVERSE OVERRIDE 5.4 DRY RUN 5.5 SINGLE BLOCK
OPERATION5. TEST OPERATION B–64124EN/01
514
To display the change in the position without moving the tool, use machine lock. There are two types of machine lock: all–axis machine lock, which stops the movement along all axes, and specified–axis machine lock, which stops the movement along specified axes only. In addition, auxiliary function lock, which disables M, S, and T commands, is available for checking a program together with machine lock.
MDI
X Y Z
The tool does not move but the position along each axis changes on the display.
Tool
Workpiece
Fig. 5.1 Machine lock
Procedure for Machine Lock and Auxiliary Function Lock
Press the machine lock switch on the operator’s panel. The tool does not move but the position along each axis changes on the display as if the tool were moving. Some machines have a machine lock switch for each axis. On such machines, press the machine lock switches for the axes along which the tool is to be stopped. Refer to the appropriate manual provided by the machine tool builder for machine lock.
WARNING The positional relationship between the workpiece coordinates and machine coordinates may differ before and after automatic operation using machine lock. In such a case, specify the workpiece coordinate system by using a coordinate setting command or by performing manual reference position return.
Press the auxiliary function lock switch on the operator’s panel. M, S, T and B codes are disabled and not executed. Refer to the appropriate manual provided by the machine tool builder for auxiliary function lock.
5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK
� Machine Lock
� Auxiliary Function Lock
OPERATIONB–64124EN/01 5. TEST OPERATION
515
M, S, T and B commands are executed in the machine lock state.
When a G27, G28, or G30 command is issued in the machine lock state, the command is accepted but the tool does not move to the reference position and the reference position return LED does not go on.
M00, M01, M02, M30, M98, M99, and M198 (Subprogram call) commands are executed even in the auxiliary function lock state. M codes for calling a subprogram (parameters No. 6071 to 6079) and those for calling a custom macro (parameter No. 6080 to 6089) are also executed.
Restrictions
� M, S, T, B command by only machine lock
� Reference position return under Machine Lock
� . ����� ��� ���%�� �!
����� �! �������� ���%
OPERATION5. TEST OPERATION B–64124EN/01
516
A programmed feedrate can be reduced or increased by a percentage (%) selected by the override dial.This feature is used to check a program. For example, when a feedrate of 100 mm/min is specified in the program, setting the override dial to 50% moves the tool at 50 mm/min.
Tool Check the machining by altering the feedrate from the value speci- fied in the program.
Feedrate 100 mm/min (Specified by programmed)
Feedrate 50 mm/min after feedrate override
Workpiece
Fig. 5.2 Feedrate override
Procedure for Feedrate Override
Set the feedrate override dial to the desired percentage (%) on the machine operator’s panel, before or during automatic operation. On some machines, the same dial is used for the feedrate override dial and jog feedrate dial. Refer to the appropriate manual provided by the machine tool builder for feedrate override.
The override that can be specified ranges from 0 to 254%. For individual machines, the range depends on the specifications of the machine tool builder.
During threading, the override is ignored and the feedrate remains as specified by program.
5.2 FEEDRATE OVERRIDE
0 200
JOG FEED RATE OVERRIDE
������������
� Override Range
� Override during thread
OPERATIONB–64124EN/01 5. TEST OPERATION
517
An override of four steps (F0, 25%, 50%, and 100%) can be applied to the rapid traverse rate. F0 is set by a parameter (No. 1421).
ÇÇ ÇÇ ÇÇ
ÇÇ ÇÇ ÇÇ
Rapid traverse rate10m/min
Override 50%
5m/min
Fig. 5.3 Rapid traverse override
Rapid Traverse Override
Select one of the four feedrates with the rapid traverse override switch during rapid traverse. Refer to the appropriate manual provided by the machine tool builder for rapid traverse override.
The following types of rapid traverse are available. Rapid traverse override can be applied for each of them. 1) Rapid traverse by G00 2) Rapid traverse during a canned cycle 3) Rapid traverse in G27, G28, G29, G30, G53 4) Manual rapid traverse 5) Rapid traverse of manual reference position return
5.3 RAPID TRAVERSE OVERRIDE
Procedure
100 25 50
LOW
Rapid traverse override
��� � ����
OPERATION5. TEST OPERATION B–64124EN/01
518
The tool is moved at the feedrate specified by a parameter regardless of the feedrate specified in the program. This function is used for checking the movement of the tool under the state taht the workpiece is removed from the table.
Tool
Table
Fig. 5.4 Dry run
Procedure for Dry Run
Press the dry run switch on the machine operator’s panel during automatic operation. The tool moves at the feedrate specified in a parameter. The rapid traverse switch can also be used for changing the feedrate. Refer to the appropriate manual provided by the machine tool builder for dry run.
The dry run feedrate changes as shown in the table below according to the rapid traverse switch and parameters.

Rapid traverse rate Setting by parameter No.1420. . . . . . .

JV: Jog feedrate override
*1) Dry run feedrate x JV when parameter RDR (bit 6 of No. 1401) is
1. Rapid traverse rate when parameter RDR is 0.
*2) Clamped to the maximum cutting feedrate
JVmax: Maximum value of jog feedrate override
5.4 DRY RUN
*��������
��� � ����
� ��! ��� ����� ��
DRY RUN
MC LOCK
SINGLE BLOCK
OPT STOP
MST LOCK
BLOCK SKIP
WORK LIGHT
OPERATIONB–64124EN/01 5. TEST OPERATION
519
Pressing the single block switch starts the single block mode. When the cycle start button is pressed in the single block mode, the tool stops after a single block in the program is executed. Check the program in the single block mode by executing the program block by block.
Cycle start
Stop
Workpiece
Cycle start
Cycle start
Stop
Stop
Tool
Fig. 5.5 (a) Single block
Procedure for Single block
1 Press the single block switch on the machine operator’s panel. The execution of the program is stopped after the current block is executed.
2 Press the cycle start button to execute the next block. The tool stops after the block is executed.
Refer to the appropriate manual provided by the machine tool builder for single block execution.
5.5 SINGLE BLOCK
*��������
OPERATION5. TEST OPERATION B–64124EN/01
520
If G28 to G30 are issued, the single block function is effective at the intermediate point.
In a canned cycle, the single block stop points are the end of �, , and � shown below. When the single block stop is made after the point � or , the feed hold LED lights.
�
�
�
�&'% ��3����
-��%
�
Fig. 5.5 (b) Single block during canned cycle
Single block stop is not performed in a block containing M98P_;. M99; or G65. However, single block stop is even performed in a block with M98P_ or M99 command, if the block contains an address other than O, N, P, L.
Explanation
� Reference position return and single block
� Single block during a canned cycle
� Subprogram call and single block
OPERATIONB–64124EN/01 6. SAFETY FUNCTIONS
521
6 SAFETY FUNCTIONS To immediately stop the machine for safety, press the Emergency stop button. To prevent the tool from exceeding the stroke ends, Overtravel check and Stroke check are available. This chapter describes emergency stop., overtravel check, and stroke check.
OPERATION6. SAFETY FUNCTIONS B–64124EN/01
522
If you press Emergency Stop button on the machine operator’s panel, the machine movement stops in a moment.
EMERGENCY STOP
Red
Fig. 6.1 Emergency stop
This button is locked when it is pressed. Although it varies with the
machine tool builder, the button can usually be unlocked by twisting it.
EMERGENCY STOP interrupts the current to the motor. Causes of trouble must be removed before the button is released.
6.1 EMERGENCY STOP
��� � ����
OPERATIONB–64124EN/01 6. SAFETY FUNCTIONS
523
When the tool tries to move beyond the stroke end set by the machine tool limit switch, the tool decelerates and stops because of working the limit switch and an OVER TRAVEL is displayed.
Y
Deceleration and stop
Stroke end Limit switch
Fig. 6.2 Overtravel