Appendix 2. Table of Command Value Ranges
IV - 2
Appendix 2. Table of Command Value Ranges
(1) Linear axis: Input increment [mm] (M system) Least command
increment 0.001 0.0001 0.00001 0.000001
Maximum stroke (value for machine coordinate system)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Maximum programmable dimension
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Rapid traverse rate (including dry run)
1 to 1000000 mm/min 1 to 1000000 mm/min 1 to 1000000 mm/min 1 to 1000000 mm/min
Cutting feed rate (including dry run) Asynchronous feed (feed per minute)
0.001 to 1000000.000 mm/min
0.0001 to 1000000.0000 mm/min
0.00001 to 1000000.00000 mm/min
0.000001 to 1000000.000000 mm/min
Synchronous feed (feed per revolution)
0.001 to 999.999 mm/rev
0.0001 to 999.9999 mm/rev
0.00001 to 999.99999 mm/rev
0.000001 to 999.999999 mm/rev
2nd to 4th reference position compensation (value for machine coordinate system)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Tool compensation amount (shape)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Tool compensation amount (wear)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Incremental feed amount
0.001 mm/pulse 0.0001 mm/pulse 0.00001 mm/pulse 0.000001 mm/pulse
Handle feed amount 0.001 mm/pulse 0.0001 mm/pulse 0.00001 mm/pulse 0.000001 mm/pulse Soft limit range (value with machine coordinate system)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Dwell time 0 to 99999.999 s 0 to 99999.9999 s 0 to 99999.99999 s 0 to 99999.999999 s Backlash compensation amount
9999999 pulse 9999999 pulse 9999999 pulse 9999999 pulse
Pitch error compensation amount
-32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse
Thread lead (F) 0.001 to 999.999 mm/rev
0.0001 to 999.9999 mm/rev
0.00001 to 999.99999 mm/rev
0.000001 to 999.999999 mm/rev
Thread lead (precision E)
0.00001 to 999.99999 mm/rev
0.000001 to 999.999999 mm/rev
0.0000001 to 999.9999999 mm/rev
0.00000001 to 999.99999999 mm/rev
Thread lead (ridges/inch)
0.03 to 999.99 0.026 to 999.999 0.0255 to 999.9999 0.02541 to 999.99999
Appendix 2. Table of Command Value Ranges
IV - 3
(2) Linear axis: Input increment [inch] (M system)
Least command increment 0.0001 0.00001 0.000001 0.0000001
Maximum stroke (value for machine coordinate system)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Maximum programmable dimension
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Rapid traverse rate (including dry run)
1 to 100000 inch/min 1 to 100000 inch/min 1 to 100000 inch/min 1 to 100000 inch/min
Cutting feed rate (including dry run) Asynchronous feed (feed per minute)
0.0001 to 100000.0000 inch/min
0.00001 to 100000.00000 inch/min
0.000001 to 100000.000000 inch/min
0.0000001 to 100000.0000000 inch/min
Synchronous feed (feed per revolution)
0.0001 to 999.9999 inch/rev
0.00001 to 999.99999 inch/rev
0.000001 to 999.999999 inch/rev
0.0000001 to 999.9999999 inch/rev
2nd to 4th reference position compensation (value for machine coordinate system)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Tool compensation amount (shape)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Tool compensation amount (wear)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Incremental feed amount
0.0001 inch/pulse 0.00001 inch/pulse 0.000001 inch/pulse 0.0000001 inch/pulse
Handle feed amount 0.0001 inch/pulse 0.00001 inch/pulse 0.000001 inch/pulse 0.0000001 inch/pulse Soft limit range (value with machine coordinate system)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Dwell time 0 to 99999.999 s 0 to 99999.9999 s 0 to 99999.99999 s 0 to 99999.999999 s Backlash compensation amount
9999999 pulse 9999999 pulse 9999999 pulse 9999999 pulse
Pitch error compensation amount
-32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse
Thread lead (F) 0.0001 to 99.9999 inch/rev
0.00001 to 99.99999 inch/rev
0.000001 to 99.999999 inch/rev
0.0000001 to 99.9999999 inch/rev
Thread lead (precision E)
0.000001 to 39.370078 inch/rev
0.0000001 to 39.3700787 inch/rev
0.00000001 to 39.37007874 inch/rev
0.000000001 to 39.370078740 inch/rev
Thread lead (ridges/inch)
0.0101 to 9999.9999 0.01001 to 9999.99999
0.010001 to 9999.999999
0.0100001 to 9999.9999999
Appendix 2. Table of Command Value Ranges
IV - 4
(3) Rotation axis: degree [] (M system)
Least command increment 0.001 0.0001 0.00001 0.000001
Maximum stroke (value for machine coordinate system)
99999.999 99999.9999 99999.99999 99999.999999
Maximum programmable dimension
99999.999 99999.9999 99999.99999 99999.999999
Rapid traverse rate (including dry run)
1 to 1000000 /min 1 to 1000000 /min 1 to 1000000 /min 1 to 1000000 /min
Cutting feed rate (including dry run) Asynchronous feed (feed per minute)
0.001 to 1000000.000 /min
0.0001 to 1000000.0000 /min
0.00001 to 1000000.00000 /min
0.000001 to 1000000.000000 /min
Synchronous feed (feed per revolution)
0.001 to 999.999 /rev 0.0001 to 999.9999 /rev
0.00001 to 999.99999 /rev
0.000001 to 999.999999 /rev
2nd to 4th reference position compensation (value with machine coordinate system)
99999.999 99999.9999 99999.99999 99999.999999
Incremental feed amount
0.001 /pulse 0.0001 /pulse 0.00001 /pulse 0.000001 /pulse
Handle feed amount 0.001 /pulse 0.0001 /pulse 0.00001 /pulse 0.000001 /pulse Soft limit range (value with machine coordinate system)
99999.999 99999.9999 99999.99999 99999.999999
Backlash compensation amount
9999999 pulse 9999999 pulse 9999999 pulse 9999999 pulse
Pitch error compensation amount
-32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse
Appendix 2. Table of Command Value Ranges
IV - 5
(1) Linear axis: Input increment [mm] (L system)
Least command increment 0.001 0.0001 0.00001 0.000001
Maximum stroke (value for machine coordinate system)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Maximum programmable dimension
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Rapid traverse rate (including dry run)
1 to 1000000 mm/min 1 to 1000000 mm/min 1 to 1000000 mm/min 1 to 1000000 mm/min
Cutting feed rate (including dry run) Asynchronous feed (feed per minute)
0.001 to 1000000.000 mm/min
0.0001 to 1000000.0000 mm/min
0.00001 to 1000000.00000 mm/min
0.000001 to 1000000.000000 mm/min
Synchronous feed (feed per revolution)
0.0001 to 999.9999 mm/rev
0.00001 to 999.99999 mm/rev
0.000001 to 999.999999 mm/rev
0.0000001 to 999.9999999 mm/rev
2nd to 4th reference position compensation (value for machine coordinate system)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Tool compensation amount (shape)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Tool compensation amount (wear)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Incremental feed amount
0.001 mm/pulse 0.0001 mm/pulse 0.00001 mm/pulse 0.000001 mm/pulse
Handle feed amount 0.001 mm/pulse 0.0001 mm/pulse 0.00001 mm/pulse 0.000001 mm/pulse Soft limit range (value with machine coordinate system)
99999.999 mm 99999.9999 mm 99999.99999 mm 99999.999999 mm
Dwell time 0 to 99999.999 s 0 to 99999.9999 s 0 to 99999.99999 s 0 to 99999.999999 s Backlash compensation amount
9999999 pulse 9999999 pulse 9999999 pulse 9999999 pulse
Pitch error compensation amount
-32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse
Thread lead (F) 0.001 to 999.999 mm/rev
0.0001 to 999.9999 mm/rev
0.00001 to 999.99999 mm/rev
0.000001 to 999.999999 mm/rev
Thread lead (precision E)
0.00001 to 999.99999 mm/rev
0.000001 to 999.999999 mm/rev
0.0000001 to 999.9999999 mm/rev
0.00000001 to 999.99999999 mm/rev
Thread lead (ridges/inch)
0.03 to 9999.99 0.026 to 9999.999 0.0255 to 9999.9999 0.02541 to 9999.99999
Appendix 2. Table of Command Value Ranges
IV - 6
(2) Linear axis: Input increment [inch] (L system)
Least command increment 0.0001 0.00001 0.000001 0.0000001
Maximum stroke (value for machine coordinate system)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Maximum programmable dimension
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Rapid traverse rate (including dry run)
1 to 100000 inch/min 1 to 100000 inch/min 1 to 100000 inch/min 1 to 100000 inch/min
Cutting feed rate (including dry run) Asynchronous feed (feed per minute)
0.0001 to 100000.0000 inch/min
0.00001 to 100000.00000 inch/min
0.000001 to 100000.000000 inch/min
0.0000001 to 100000.0000000 inch/min
Synchronous feed (feed per revolution)
0.000001 to 99.999999 inch/rev
0.0000001 to 99.9999999 inch/rev
0.00000001 to 99.99999999 inch/rev
0.000000001 to 99.999999999 inch/rev
2nd to 4th reference position compensation (value for machine coordinate system)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Tool compensation amount (shape)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Tool compensation amount (wear)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Incremental feed amount
0.0001 inch/pulse 0.00001 inch/pulse 0.000001 inch/pulse 0.0000001 inch/pulse
Handle feed amount 0.0001 inch/pulse 0.00001 inch/pulse 0.000001 inch/pulse 0.0000001 inch/pulse Soft limit range (value with machine coordinate system)
9999.9999 inch 9999.99999 inch 9999.999999 inch 9999.9999999 inch
Dwell time 0 to 99999.999 s 0 to 99999.9999 s 0 to 99999.99999 s 0 to 99999.999999 s Backlash compensation amount
9999999 pulse 9999999 pulse 9999999 pulse 9999999 pulse
Pitch error compensation amount
-32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse
Thread lead (F) 0.0001 to 99.9999 inch/rev
0.00001 to 99.99999 inch/rev
0.000001 to 99.999999 inch/rev
0.0000001 to 99.9999999 inch/rev
Thread lead (precision E)
0.000001 to 39.370078 inch/rev
0.0000001 to 39.3700787 inch/rev
0.00000001 to 39.37007874 inch/rev
0.000000001 to 39.370078740 inch/rev
Thread lead (ridges/inch)
0.0101 to 9999.9999 0.01001 to 9999.99999
0.010001 to 9999.999999
0.0100001 to 9999.9999999
Appendix 2. Table of Command Value Ranges
IV - 7
(3) Rotation axis: degree [] (L system)
Least command increment 0.001 0.0001 0.00001 0.000001
Maximum stroke (value for machine coordinate system)
99999.999 99999.9999 99999.99999 99999.999999
Maximum programmable dimension
99999.999 99999.9999 99999.99999 99999.999999
Rapid traverse rate (including dry run)
1 to 1000000 /min 1 to 1000000 /min 1 to 1000000 /min 1 to 1000000 /min
Cutting feed rate (including dry run) Asynchronous feed (feed per minute)
0.001 to 1000000.000 /min
0.0001 to 1000000.0000 /min
0.00001 to 1000000.00000 /min
0.000001 to 1000000.000000 /min
Synchronous feed (feed per revolution)
0.0001 to 999.9999 /rev
0.00001 to 999.99999 /rev
0.000001 to 999.999999 /rev
0.0000001 to 999.9999999 /rev
2nd to 4th reference position compensation (value with machine coordinate system)
99999.999 99999.9999 99999.99999 99999.999999
Incremental feed amount
0.001 /pulse 0.0001 /pulse 0.00001 /pulse 0.000001 /pulse
Handle feed amount 0.001 /pulse 0.0001 /pulse 0.00001 /pulse 0.000001 /pulse Soft limit range (value with machine coordinate system)
99999.999 99999.9999 99999.99999 99999.999999
Backlash compensation amount
9999999 pulse 9999999 pulse 9999999 pulse 9999999 pulse
Pitch error compensation amount
-32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse -32768 to 32767 pulse
Appendix 3. Circular Cutting Radius Error
IV - 8
Appendix 3. Circular Cutting Radius Error When circular cutting is performed, an error is caused between the command coordinate and the tracking coordinate due to the tracking delay in the smoothing circuit and servo system, and the workpiece ends up with a radius smaller than the commanded value. The method for obtaining this error (radius error) is shown below.
A : Command coordinate B : Tracking coordinate R : Command radius (mm) R : Radius error (mm) : Angle error (rad) F : Cutting feed rate (m/min)
A
F
B
R
R
F
The radius error R and angle error are calculated from the following formula.
Exponential acceleration/ deceleration R = ( Ts2 + Tp2) ( )2 (mm) Linear acceleration/ deceleration R = ( Ts2 + Tp2) ( )2 (mm)
= tan-1 (Ts ) + tan-1 (Tp ) (rad) Ts: Time constant (s) of specified smoothing circuit Tp: Position loop time constant
(Note 1) When the R radius error applying with circular cutting does not come within the allowable value, proceed to reduce the cutting feed rate F, set Ts to a lower value or review the program.
(Note 2) In the steady state, R is constant. However, it is not constant with command start and stop transitions. Under command start and stop conditions, therefore, the tracking coordinate should be as shown in the figure below.
Start/stop
Command Tracking
R R
F R
F R
1 2
1 2
1 R
F 103
60 1
24 1 2
1 R
F 103
60
Appendix 4. Registering/Editing the Fixed Cycle Program 4.1 Fixed Cycle Operation Parameters
IV - 9
Appendix 4. Registering/Editing the Fixed Cycle Program The subprogram for the fixed cycle can be input, output and edited.
! CAUTION
Do not change the fixed cycle program without prior approval from the machine maker. 4.1 Fixed Cycle Operation Parameters
To input/output or edit the data of each fixed cycle subprogram, use the Data I/O and Edit screens in the same way as when creating usual user-created work programs. In this case, the parameters must have been set. Set "1" in parameter "#1166 fixpro". If this parameter is valid, the IN/OUT and Edit screens are usable only for operating a fixed cycle control subprogram. During this period, program file displays only fixed cycle programs. Thus, after fixed cycle program operation, return parameter to "0". (Note) Parameter "#1166 fixpro" will be set to 0 when the power is turned OFF.
4.2 Transmitting/Erasing the Fixed Cycle Program
Transmit/erase the fixed cycle program from the Data I/O screen. Check that fixed cycle operation parameter "#1166 fixpro" is valid. The operating procedure is the same as a user machining program.
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 10
4.3 Standard Fixed Cycle Subprogram (For L system)
G37 (O370) Automatic tool length measurement
G31 Z #5 F #3 ; 1F [ROUND [ ABS [#2 - [ ##10 #11 #12 ] ] ] GT #8 ] GOTO 1 ; 1F [ROUND [ ##10 #11 - #12 ] EQ #4 ] GOTO 1 ; ##9 = #10 - #12/#11 - #2/#11 + ##9 ; #3003 = #1 ; N2 ; M99 ; N1 # 3901 = 126 ;
G74 (O740) End face cutoff cycle
G. 1 ; 1F [ ABS [ #2 ] GT 0 ] GOTO 10 ; #14 = 1 ; N10 #13 = #3 ; IF [ #15 NE 0 ] GOTO 11 ; #13 = #3 - #5 ; N11 #16 = 0 ; D0 1 ; #10 = 0 ; #11 = #4 ; D0 2 ; #10 = #10 + #4 ; IF [ ABS [ #10 ] GE [ABS [ #1 ] ] ] GOTO 1 ; G01 X #11 ; G00 X #6 ; #11 = #4 - #6 ; END 2 ; N1 G01 X#1 #10 + #11 ; IF [ #15 EQ 0 ] GOTO 20 ; IF [ #16 EQ 0 ] GOTO 21 ; N20 G00 Y#5 ; N21 #16 = 1 ; G00X - #1 ; IF [ #14 ] GOTO 3 ; #12 = #12 + #3 ; IF [ ABS [ #12 ] LT [ABS [ #2 ] ] ] GOTO 2 ; #14 = 1 ; #13 = #2 - #12 + #13 ; N2 G00 Y #13 ; #13 = #3 - #5 ; END 1 ; N3 G00 Y - #2 - #5 ; M99 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 11
G75 (O750) Longitudinal cutting cycle
G. 1 ; 1F [ ABS [ #1 ] GT 0 ] GOTO 10 ; #14 = 1 ; N10 #13 = #4 ; IF [ #15 NE 0 ] GOTO 11 ; #13 = #4 - #5 ; N11 #16 = 0 ; D0 1 ; #10 = 0 ; #11 = #3 ; D0 2 ; #10 = #10 + #3 ; IF [ ABS [ #10 ] GE [ABS [ #2 ] ] ] GOTO 1 ; G01 Y #11 ; G00 Y #6 ; #11 = #3 - #6 ; END 2 ; N1 G01 Y#2 - #10 + #11 ; IF [ #15 EQ 0 ] GOTO 20 ; IF [ #16 EQ 0 ] GOTO 21 ; N20 G00 X#5 ; N21 #16 = 1 ; G00Y - #2 ; IF [ #14 ] GOTO 3 ; #12 = #12 + #4 ; IF [ ABS [ #12 ] LT [ABS [ #1 ] ] ] GOTO 2 ; #14 = 1 ; #13 = #1 - #12 + #13 ; N2 G00 X #13 ; #13 = #4 - #5 ; END 1 ; N3 G00 X - #1 - #5 ; M99 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 12
G75.1 (O751) Groove cutting cycle
G. 1 ; #3003 = #8 OR 1 ; G0 X #1 ; G1 Y #2 ; G0 Y #2 ; X #5 ; 1F [ #3 EQ 0 ] GOTO 1 ; G1 X - #3 Y #4 ; N1 G1 Y#6 ; X - #7 ; G0Y - #2 ; X - #5 ; 1F [ #3 EQ 0 ] GOTO 2 ; G1 X #3 Y #4 ; N2 G1 Y#6 ; X #7 ; #3003 = #8 ; G0Y - #2 ; M99 ;
G76 (O760) Compound thread cutting cycle
G. 1 ; #12 = 1 ; #13 = #9 ; 1F [ ABS [ #13 ] GE [ ABS [ #8 ] ] ] GOTO 1 ; #16 = 1 ; #13 = #8 ; N1 #11 = #13 ; 1F [ ABS [ #11 ] LT [ ABS [ #4 #5 ] ] ] GOTO 2 ; #11 = #4 - #5 ; #14 = 1 ; N2 #17 = #11 ; #18 = ROUND [ [ #4 - #11 - #5 ] #7 ] ; IF [ [ #18 XOR #1 ] GE 0 ] GOTO 10 ; #18 = - #18 ; N10 #19 = #18 ; #10 = ROUND [ [ #11 + #5 ] #7 ] ; IF [ [ #10 XOR #1 ] GE 0 ] GOTO 20 ; #10 = - #10 ; N20 G00 X#10 ; #20 = #10 D0 1 ; #15 = ROUND [ #10 #3/#1 ] ; G00 Y #2 + #3 - #4 - #15 + #11 ; G33 X#1 - #10 - #18 Y -#3 + #15 ; G00 Y - #2 + #4 #11 ; IF [ #14 GT 0 ] GOTO 3 ; IF [ #16 GT 0 ] GOTO 7 ; #12 = #12 + 1 ; #13 = ROUND [ #9 SQRT [ #12 ] ] ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 13
IF [ ABS [ #13 #11 ] GE [ ABS [ #8 ] ] ] GOTO 8 ; #16 = 1 ; N7 #13 = #11 + #8 ; N8 #11 = #13 ; IF [ ABS [ #11 ] LT [ ABS [ #4 #5 ] ] ] GOTO 9 ; #11 = #4 - #5 ; #14 = 1 ; N9 #10 = ROUND [ [ #17 - #11 ] #7 ] ; IF [ [ #10XOR#1] GE 0 ] GOTO 6 ; #10 = -#10 ; N6 #10 = #10 + #20 ; G00 X - #1 + #10 + #18 ; IF [ #14 LT 0 ] GOTO 11 ; #18 = 0 ; GOTO 12 ; N11 #18 = #19 - #10 + #20 ; N12 END 1 ; N3 IF [ ABS [ #6 ] LT 1 ] GOTO 5 ; #14 = 0 ; #13 = 0 ; D0 2 ; IF [ #14 GT 0 ] GOTO 5 ; #13 = #13 + #6 ; IF [ ABS [ #13 ] LT [ ABS [ #5 ] ] ] GOTO 4 ; #13 = #5 ; #14 = 1 ; N4 G00 X #10 #1 ; G00 Y #2 + #3 - #4 + #13 #15 + #11 ; G33 X #1 - #10 Y - #3 + #15 ; G00 Y - #2 + #4 - #13 - #11 ; END 2 ; N5 G00 X - #1 ; M99 ;
G76.1 (O761) 2-part system simultaneous compound thread cutting cycle
G. 1 ; N761 !L10 #12 = 1 ; #13 = #9 ; 1F [ ABS [ #13 ] GE [ ABS [ #8 ] ] ] GOTO 1 ; #16 = 1 ; #13 = #8 ; N1 #11 = #13 ; 1F [ ABS [ #11 ] LT [ ABS [ #4 #5 ] ] ] GOTO 2 ; #11 = #4 - #5 ; #14 = 1 ; N2 #17 = #11 ; #18 = ROUND [ [ #4 - #11 - #5 ] #7 ] ; IF [ [ #18 XOR #1 ] GE 0 ] GOTO 10 ; #18 = - #18 ; N10 #19 = #18 ; #10 = ROUND [ [ #11 + #5 ] #7 ] ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 14
IF [ [ #10 XOR #1 ] GE 0 ] GOTO 20 ; #10 = - #10 ; N20 G00 X#10 ; #20 = #10 D0 1 ; #15 = ROUND [ #10 #3/#1 ] ; G00 Y #2 + #3 - #4 - #15 + #11 ; !L11 ; G33 X#1 - #10 - #18 Y -#3 + #15 ; G00 Y - #2 + #4 - #11 ; !L12 ; IF [ #14 GT 0 ] GOTO 3 ; IF [ #16 GT 0 ] GOTO 7 ; #12 = #12 + 1 ; #13 = ROUND [ #9 SQRT [ #12 ] ] ; IF [ ABS [ #13 - #11 ] GE [ ABS [ #8 ] ] ] GOTO 8 ; #16 = 1 ; N7 #13 = #11 + #8 ; N8 #11 = #13 ; IF [ ABS [ #11 ] LT [ ABS [ #4 #5 ] ] ] GOTO 9 ; #11 = #4 - #5 ; #14 = 1 ; N9 #10 = ROUND [ [ #17 - #11 ] #7 ] ; IF [ [ #10XOR#1] GE 0 ] GOTO 6 ; #10 = -#10 ; N6 #10 = #10 + #20 ; G00 X - #1 + #10 + #18 ; IF [ #14 LT 0 ] GOTO 11 ; #18 = 0 ; GOTO 12 ; N11 #18 = #19 - #10 + #20 ; N12 END 1 ; N3 IF [ ABS [ #6 ] LT 1 ] GOTO 5 ; #14 = 0 ; #13 = 0 ; D0 2 ; IF [ #14 GOTO ] GOTO 5 ; #13 = #13 + #6 ; IF [ ABS [ #13 ] LT [ ABS [ #5 ] ] ] GOTO 4 ; #13 = #5 ; #14 = 1 ; N4 G00 X #10 - #1 ; G00 Y #2 + #3 #4 + #13 - #15 + #11 ; !L11 ; G33 X #1 - #10 Y - #3 + #15 ; G00 Y - #2 + #4 - #13 - #11 ; !L12 ; END 2 ; N5 G00 X - #1 ; M99 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 15
G76.2 (O762) 2-system simultaneous compound thread cutting cycle
G. 1 ; N762 !L10 ; #12 = 1 ; #13 = #9 ; 1F [ ABS [ #13 ] GE [ ABS [ #8 ] ] ] GOTO 1 ; #16 = 1 ; #13 = #8 ; N1 #11 = #13 ; 1F [ ABS [ #11 ] LT [ ABS [ #4 - #5 ] ] ] GOTO 2 ; #11 = #4 - #5 ; #14 = 1 ; N2 #17 = #11 ; #18 = ROUND [ [ #4 - #11 - #5 ] #7 ] ; IF [ [ #18 XOR #1 ] GE 0 ] GOTO 10 ; #18 = - #18 ; N10 #19 = #18 ; #10 = ROUND [ [ #11 + #5 ] #7 ] ; IF [ [ #10 XOR #1 ] GE 0 ] GOTO 20 ; #10 = - #10 ; N20 IF [# 27 NE 1 ] GOTO 21 ; G00 X#10 ; N21 #20 = #10 ; #28 = 1 ; D01 ; #15 = ROUND [ #10 #3/#1 ] ; #29 = #28 MOD 2 ; IF [ [ #27 EQ 1 ] AND [#29 EQ 0 ] GOTO 22 ; IF [ [ #27 EQ 2 ] AND [#29 EQ 1 ] GOTO 22 ; G00 Y #2 + #3 - #4 - #15 + #11 ; !L11 ; G33 X#1 - #10 - #18 Y -#3 + #15 ; G00 Y - #2 + #4 - #11 ; #21 = #18 ; !L12 ; N22 IF [ #14 GT 0 ] GOTO 3 ; IF [ #16 GT 0 ] GOTO 7 ; #12 = #12 + 1 ; #13 = ROUND [ #9 SQRT [ #12 ] ] ; IF [ ABS [ #13 - #11 ] GE [ ABS [ #8 ] ] ] GOTO 8 ; #16 = 1 ; N7 #13 = #11 + #8 ; N8 #11 = #13 ; IF [ ABS [ #11 ] LT [ ABS [ #4 - #5 ] ] ] GOTO 9 ; #11 = #4 - #5 ; #14 = 1 ; N9 #10 = ROUND [ [ #17 - #11 ] #7 ] ; IF [ [ #10XOR#1] GE 0 ] GOTO 6 ; #10 = -#10 ; N6 #10 = #10 + #20 ; IF [ [ #27 EQ 1 ] AND [#29 EQ 1 ] GOTO 24 ; IF [ [ #27 EQ 2 ] AND [#29 EQ 0 ] GOTO 24 ; IF [ [ #27 EQ 2 ] AND [#28 EQ 1 ] GOTO 23 ; G00 X #1 + #10 + #21 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 16
GOTO 24 ; N23 G00 X#10 ; N24 IF [ #14 LT 0 ] GOTO 11 ; #18 = 0 ; GOTO 12 ; N11 #18 = #19 - #10 + #20 ; N12 #28 = #28 + 1 ; END 1 ; N3 IF [ ABS [ #6 ] LT 1 ] GOTO 5 ; #14 = 0 ; #13 = 0 ; D0 2 ; IF [ #14 GT 0 ] GOTO 5 ; #13 = #13 + #6 ; IF [ ABS [ #13 ] LT [ ABS [ #5 ] ] ] GOTO 4 ; #13 = #5 ; #14 = 1 ; N4 #29 = #28 MOD 2 ; IF [ [ #27 EQ 1 ] AND [#29 EQ 1 ] GOTO 25 ; IF [ [ #27 EQ 2 ] AND [#29 EQ 0 ] GOTO 25 ; G00 X #10 - #1 + #21 ; #21 = 0 ; G00 Y #2 + #3 #4 + #13 - #15 + #11 ; !L11 ; G33 X #1 - #10 Y #3 + #15 ; G00 Y - #2 + #4 - #13 - #11 ; !L12 ; N25 #28 = #28 + 1 ; END 2 ; N5 G00 X - #1 ; M99 ; %
G77 (O770) Longitudinal cutting cycle
G. 1 ; 1F [ [ #1 EQ 0 ] OR [ #2 EQ 0 ] ] GOTO 1 ; Y #2 + #7 ; G1 X #1 Y - #7 ; Y - #2 ; G0 X - #1 ; N1 M99 ;
G78 (O780) Thread cutting cycle
G. 1 ; 1F [ [ #1 EQ 0 ] OR [ #2 EQ 0 ] ] GOTO 1 ; Y #2 + #7 ; G33 X #1 Y - #7 F #9 E #10 ; G0 Y - #2 ; X - #1 ; N1 M99 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 17
G79 (O790) End face cutoff cycle
G. 1 ; 1F [ [ #1 EQ 0 ] OR [ #2 EQ 0 ] ] GOTO 1 ; X #1 + #7 ; G1 X - #7 Y #2 ; X - #1 ; G0 Y - #2 ; N1 M99 ;
G83 G87 (O830) Deep hole drilling cycle B
G. 1 ; 1F [ #30 ] GOTO 2 ; M #24 ; #29 = #11 #28 = 0 ; Z #2 ; #2 = ##5 #3003 = #8 OR 1 ; D0 1 ; #28 = #28 #11 #26 = - #28 - #29 ; Z #26 ; IF [ ABS [ #28 ] GE [ ABS [ #3 ] ] ] GOTO 1 ; G1 Z #29 ; G0 Z #28 ; G29 = #11 + #14 ; END 1 ; N1 G1 Z #3 - #26 ; G4 P #4 ; #3003 = #8 ; G0Z - #3 - #2 ; IF [#24 EQ #0 ] GOTO 2 ; M #24 + 1 ; G4 P #21 ; N2 M99 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 18
G83 G87 (O831) Deep hole drilling cycle A
G. 1 ; 1F [ #30 ] GOTO 2 ; M #24 ; #29 = #0 #28 = #11 ; Z #2 ; #2 = ##5 #3003 = #8 OR 1 ; D0 1 ; #29 = #29 + #11 ; IF [ ABS [ #29 ] GE [ ABS [ #3 ] ] ] GOTO 1 ; G1 Z #28 ; G0 Z - #14 ; #28 = #11 + #14 ; END 1 ; N1 G1 Z #3 - #29 + #28 ; G4 P #4 ; #3003 = #8 ; G0Z - #3 - #2 ; IF [#24 EQ #0 ] GOTO 2 ; M #24 + 1 ; G4 P #21 ; N2 M99 ;
G83.2 (O832) Deep hole drilling cycle 2
G. 1 ; 1F [ #30 ] GOTO 3 ; #3003 = #8 OR 1 ; #29 = #12 #28 = 0 ; G0 Z #2 ; IF [ #12 NE #0 ] GOTO 1 ; IF [ #11 EQ #0 ] GOTO 2 ; N1 #28 = #28 - #12 #26 = - #28 - #29 ; IF [ ABS [ #28 ] GE [ ABS [ #3 ] ] ] GOTO 2 ; G1 Z #12 ; G4 P #4 ; G0 Z #28 - #2 ; G4P # 13 ; G29 = #11 + #15 ; D0 1 ; #28 = #28 - #11 #26 = - #28 - #29 ; G0 Z #26 + #2 ; IF [ ABS [ #28 ] GE [ ABS [ #3 ] ] ] GOTO 2 ; G1 Z #29 ; G4 P #4 ; G0 Z #28 - #2 ; G4 P # 13 ; END 1 ; N2 G1 Z #3 - #26 ; G4 P #4 ; #3003 = #8 ; G0Z - #3 - #2 ; N3 M99 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.3 Standard Fixed Cycle Subprogram (For L system)
IV - 19
G84 G88 (O840) Tap cycle
G. 1 ; 1F [ #30 ] GOTO 2 ; M #24 ; Z #2 ; #2 = ##5 #3003 = #8 OR 1 #3004 = #9 OR 3 ; G1 Z #3 ; G4 P #4 ; M4 ; #3900 = 1 ; G1 Z - #3 ; #3004 = #9 ; M3 ; #3003 = #8 ; IF [#24 EQ #0 ] GOTO 1 ; M #24 + 1 ; G4 P #21 ; N1 G0 Z #2 ; N2 M99 ;
G85 G89 (O850) Boring cycle
G. 1 ; 1F [ #30 ] GOTO 2 ; M #24 ; Z #2 ; #2 = ##5 #3003 = #8 OR 1 ; G1 Z #3 ; G4 P #4 ; #3003 = #8 ; Z - #3 F #23 ; F #22 ; IF [#24 EQ #0 ] GOTO 1 ; M #24 + 1 ; G4 P #21 ; N1 G0 Z #2 ; N2 M99 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.4 Standard Fixed Cycle Subprogram (For M system)
IV - 20
4.4 Standard Fixed Cycle Subprogram (For M system)
G81 (O810) Drill, spot drill
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Return.
G82 (O820) Drill, counter boring
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Dwell. Return.
G83 (O830) Deep hole drill cycle
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Define the cutting amount. Initialize the return amount (total cutting amount). Inhibit single block stop. Define the return amount of the next block. Calculate the feed amount. Feed. Does the total cutting amount (return amount) exceed the cut amount? Cutting feed
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; G1 Z#3 ; #3003 = #8 ; G0 Z - #3 - #2 ; N1 M99%
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; G1 Z#3 ; G4 P#4 ; #3003 = #8 ; G0 Z - #3 - #2 ; N1 M99%
G. 1 ; 1F [#30] GOTO2 ; #29 = #11 #28 = 0 Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; DO 1 ; #28 = #28 - #11 #26 = - #28 - #29 Z#26 ; IF [ABS [#28] GE [ABS [#3] ] ] GOTO 1 ; G1 Z#29 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.4 Standard Fixed Cycle Subprogram (For M system)
IV - 21
Return. Define the cutting amount for block 2 and after. Cutting feed Return.
G84 (O840) Tap cycle
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Invalidate feed hold/override. Dwell. Rotate the spindle reversely. Dwell. Rotate the spindle forward. Return.
G85 (O850) Boring 1
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Return.
G0 Z#28 ; #29 = #11 + #14 ; END1 ; N1 G1 Z#3 - #26 ; #3003 = #8 ; G0 Z - #3 - #2 ; N2 M99%
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; #3004 = #9 OR 3 ; G1 Z#3 ; G4 P#4 ; M4 ; #3900 = 1 ; G1 Z - #3 ; #3004 = #9 ; G4 P#4 ; M3 ; #3003 = #8 ; G0 Z = #2 ; N1 M99%
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; G1 Z#3 ; #3003 = #8 ; Z - #3 ; G0 Z - #2 ; N1 M99%
Appendix 4. Registering/Editing the Fixed Cycle Program 4.4 Standard Fixed Cycle Subprogram (For M system)
IV - 22
G86 (O860) Boring 2
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Dwell. Stop the spindle. Return. Rotate the spindle forward.
G87 (O870) Back boring
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Orient the spindle. Cancel single block stop inhibition. Inhibit single block stop. Cancel single block stop inhibition. Rotate the spindle forward. Inhibit single block stop. Orient the spindle. Shift. G87 is not affected by the G98 or G99 modal. Cancel single block stop inhibition. Shift. Rotate the spindle forward.
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; G1 Z#3 ; G4 P#4 ; M5 ; G0 Z - #3 - #2 ; #3003 = #8 ; M3 ; N1 M99%
G. 1 ; 1F [#30] GOTO1 ; #3003 = #8 OR 1 ; M19 ; X#12 Y#13 ; #3003 = #8 ; Z#2 G#6 H#7 ; #3003 = #8 OR 1 ; G1 X - #12 Y - #13 ; #3003 = #8 ; M3 ; #3003 = #8 OR 1 ; Z#3 ; M19 ; G0 X#12 Y#13 ; Z - #2 - #3 ; #3003 = #8 ; X - #12 Y - #13 ; M3 ; N1 M99%
Appendix 4. Registering/Editing the Fixed Cycle Program 4.4 Standard Fixed Cycle Subprogram (For M system)
IV - 23
G88 (O880) Boring 3
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Dwell. Cancel single block stop inhibition. Rotate the spindle forward Inhibit single block stop. Return. Cancel single block stop inhibition. Rotate the spindle forward.
G89 (O890) Boring 4
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Dwell. Return.
G73 (O831) Step cycle
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Initialize the total cutting amount. Define the cutting amount. Single block stop command Increment the total cutting amount counter. Does the total cutting amount exceed the cut amount Z?
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; G1 Z#3 ; G4 P#4 ; #3003 = #8 ; M5 ; #3003 = #8 OR 1 ; G0 Z - #3 - #2 ; #3003 = #8 ; M3 ; N1 M99 ;
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; G1 Z#3 ; G4 P#4 ; #3003 = #8 Z - #3 ; G0 Z - #2 ; N1 M99%
G. 1 ; 1F [#30] GOTO2 ; #29 = 0 #28 = #11 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; DO 1 ; #29 = #29 + #11 ; IF [ABS [#29] GE [ABS [#3] ] ] GOTO 1 ;
Appendix 4. Registering/Editing the Fixed Cycle Program 4.4 Standard Fixed Cycle Subprogram (For M system)
IV - 24
Cutting feed Dwell. Return. Define the cutting amount for block 2 and after. Cutting feed Dwell. Return.
G74 (O841) Reverse tap cycle
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Inhibit single block stop. Invalidate feed hold/override. Dwell. Rotate the spindle forward. Dwell. Rotate the spindle reversely. Return.
G1 Z#28 ; G4 P#4 ; G0 Z #14 ; #28 = #11 + #14 ; END1 ; N1 G1 Z#3 #29 + #28 ; G4 P#4 ; #3003 = #8 ; G0Z - #3 - #2 ; N2 M99%
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; #3004 = #9 OR 3 ; G1 Z#3 ; G4 P#4 ; M3 ; #3900 = 1 ; Z - #3 ; #3004 = #9 ; G4 P#4 ; M4 ; #3003 = #8 ; G0 Z - #2 ; N1 M99%
Appendix 4. Registering/Editing the Fixed Cycle Program 4.4 Standard Fixed Cycle Subprogram (For M system)
IV - 25
G75 (O750) Circle cutting cycle
Fixed cycle block 1 movement command. Check for fixed cycle invalidity. Decide the circular direction. G03 circular G02 circular Check compensation amount Inner circumference half lap Outer circumference one lap Inner circumference half lap Return.
G76 (O861) Fine boring
Fixed cycle block 1 movement command Check for fixed cycle invalidity. Single block stop command Orient the spindle. Shift. Return. Shift. Rotate the spindle forward.
G. 1 ; 1F [#30] GOTO1 ; Z#2 G#6 H#7 ; #2 = ##5 #3003 = #8 OR 1 ; G1 Z#3 ; M19 ; X#12 Y#13 ; G0 Z - #3 - #2 ; #3003 = #8 ; X - #12 Y - #13 ; M3 ; N1 M99%
G. 1 ; IF [#30] GOTO 1 ; #28=#18; #2 = ##5 IF[#28GE0]GOTO2; #27=3#28=-#28; GOTO3; N2 #27=2; N3 #26=[#[16000+#4]+#[17000+#4]]*#99; IF[#26GE#28]GOTO1; Z#2G#6H#7; #2=##5#3003=#8OR1; G1Z#3; #28=#28-#26#29=#28/2; G#27X-#28I-#29; I#28P1; X#28I#29; #3003=#8; G0Z-#3-#2; N1 M99%
Appendix 5. RS-232C I/O Device Parameter Setting Examples
IV - 26
Appendix 5. RS-232C I/O Device Parameter Setting Examples
Cable connection Parameter setting examples
NC I/O 1 1 2 2 3 3 4 4 5 5 6 6 20 20 7 7
NC I/O 1 1 2 2 3 3 14 14 5 5 6 6 20 20 7 7
NC I/O 1 1 2 2 3 3 4 4 5 8 6 20 8 7 7
NC I/O 1 1 2 2 3 3 4 4 5 5 6 6 20 20 8 8 7 7
NC I/O 1 1 2 2 3 3 4 4 5 5 6 6 20 20 8 8 7 7
Follows communication protocol. (NC side) 2 : SD 3 : RD 4 : RS 5 : CS 6 : DR 20 : ER 7 : GND
DEVICE NAME BAUD RATE 2 2 2 2 2 STOP BIT 3 3 3 3 3 PARITY EFFECTIVE 0 0 0 0 0 EVEN PARITY 0 0 0 0 0 CHR. LENGTH 3 3 3 3 3 HAND SHAKE 3 2 3 3 3 DC CODE PARITY 1 0 1 1 1 DC2/DC4 OUTPUT 0 0 1 0 1 CR OUTPUT 0 0/1 0 0 0 FEED CHR. 0 0 0 0 0 PARITY V 0 0 0 0/1 0/1 TIME-OUT SET 100 100 100 100 100
Follows communication software.
Appendix 6. Alarms 6.1 List of Alarms
IV - 27
Appendix 6. Alarms 6.1 List of Alarms 6.1.1 Operation Alarms
(The bold characters are the messages displayed on the screen.) M Message
Error No. Message Class
(1) Class: M01 Operation error
Alarms occurring due to incorrect operation by the operator during NC operation and those by machine trouble are displayed.
Error No. Details Remedy 0001 Dog overrun
When returning to the reference position the near-point detection limit switch did not stop over the dog but overran the dog.
Increase the length of the near-point dog. Reduce the reference position return speed.
0002 Some ax does not pass Z phase One of the axes did not pass the Z-phase during the initial reference position return after the power was turned ON.
Move the detector one rotation or more in the opposite direction of the reference position and repeat reference position return.
0003 R-pnt direction illegal When manually returning to the reference position the return direction differs from the axis movement direction selected with the AXIS SELECTION key.
The selection of the AXIS SELECTION key's +/- direction is incorrect. The error is canceled by feeding the axis in the correct direction.
0004 External interlock axis exists The external interlock function has activated (the input signal is "OFF") and one of the axes has entered the interlock state.
As the interlock function has activated release it before resuming operation.
Check the sequence on the machine side. Check for broken wires in the interlock signal
line. 0005 Internal interlock axis exists
The internal interlock state has been entered. The absolute position detector axis has been removed. A command for the manual/automatic simultaneous valid axis was issued from the automatic mode. The manual speed command was issued while the tool length measurement 1 signal is ON.
The servo OFF function is valid so release it first.
An axis that can be removed has been issued so perform the correct operations.
The command is issued in the same direction as the direction where manual skip turned ON so perform the correct operations.
During the manual/automatic simultaneous mode the axis commanded in the automatic mode became the manual operation axis. Turn OFF the manual/automatic valid signal for the commanded axis.
Turn ON the power again and perform absolute position initialization.
Turn OFF the tool length measurement 1 signal to start the program by the manual speed command.
0006 H/W stroke end axis exists The stroke end function has activated (the input signal is "OFF") and one of the axes is in the stroke end status.
Move the machine manually. Check for broken wires in the stroke end signal
wire. Check for trouble in the limit switch.
Appendix 6. Alarms 6.1 List of Alarms
IV - 28
Error No. Details Remedy
0007 S/W stroke end axis exists The stored stroke limit I II IIB or IB function has activated.
Move it manually. If the stored stroke limit in the parameter is
incorrectly set correct it. 0008 Chuck/tailstock stroke end ax
The chuck/tail-stock barrier function turned ON and an axis entered the stroke end state.
Reset the alarm with reset and move the machine in the reverse direction.
0009 Ref point return No. invalid Return to the No. 2 reference position was performed before return to the No. 1 reference position was completed.
Execute No. 1 reference position return.
0019 Sensor signal illegal ON The sensor signal was already ON when the tool measurement mode (TLM) signal was validated. The sensor signal turned ON when there was no axis movement after the tool measurement mode (TLM) signal was validated. The sensor signal turned ON at a position within 100m from the final entry start position.
Turn the tool measurement mode signal input OFF, and move the axis in a safe direction.
The operation alarm will turn OFF even when the sensor signal is turned OFF.
(Note) When the tool measurement mode signal input is turned OFF, the axis can be moved in either direction. Pay attention to the movement direction.
0020 Ref point retract invalid Return to the reference position was performed before the coordinates had not been established.
Execute reference position return
0021 Tool ofs invld after R-pnt Reference position return was performed during tool retract return, and therefore the tool compensation amount became invalid after reference position return was completed.
The error is cleared if the operation mode is changed to other than reference position return before the axis performs reference position return.
The error is cleared when reference position return is completed.
The error is cleared if reset 1 is input or the emergency stop button is pushed.
0024 R-pnt ret invld at abs pos alm A zero point return signal was input during an absolute position detection alarm.
Reset the absolute position detection alarm and then perform zero point return.
0025 R-pnt ret invld at zero pt ini A zero point return signal was input during zero point initialization of the absolute position detection system.
Complete zero point initialization and then perform zero point return.
0030 Now skip on The skip signal remains input when the skip return operation changed to the measurement operation.
Increase the skip return amount.
0031 No skip Even though 1st skip was to the correct position, the 2nd skip could not be found.
Check whether the measurement target has moved.
0050 Chopping axis R-pnt incomplete The chopping axis has not completed zero point return before entering the chopping mode. All axes interlock will be applied.
Reset or turn the chopping signal OFF, and then carry out zero point return.
Appendix 6. Alarms 6.1 List of Alarms
IV - 29
Error No. Details Remedy
0051 Synchronous error excessive The synchronization error of the master and slave axes exceeded the allowable value under synchronous control. A deviation exceeding the synchronization error limit value was found with the synchronization deviation detection.
Select the correction mode and move one of the axes in the direction in which the errors are reduced.
Increase the allowable value or reset it to 0 (check disabled).
When using simple C-axis synchronous control, set the contents of the R435 register to 0.
Check the parameter (#2024 synerr). 0053 No spindle select signal
Synchronous tapping command was issued when the spindle select signals (SWS) for all spindles were OFF in the multiple-spindle control II.
Turn ON the spindle select signal (SWS) responding to the tapping spindle before performing the synchronous tapping command.
0054 No spindle serial connection Synchronous tapping command was issued when the spindle that the spindle select signal (SWS) was ON was not serially connected in the multiple-spindle control II.
Make sure the spindle select signal (SWS) for the responding spindle is ON.
When issuing a command, consider the machine construction.
0055 Spindle fwd/rvs run para err Asynchronous tapping command was issued when M code of the spindle frd/rvs run command set by the parameter "#3028 sprcmm" was one of the followings in the multiple-spindle control II. One of M0, M1, M2, M30, M98, M99, M198 M code No. that commands macro interrupt
signal valid/invalid
Change the value of the parameter #3028 sprcmm.
0056 Tap pitch/thread number error The command of the pitch/thread number is not correct in the synchronous tapping command of the multiple-spindle control II. The pitch is too small for the spindle rotation speed. Thread number is too large for the spindle rotation speed.
Check the pitch/thread number and rotation speed of the tapping spindle.
0060 Handle ratio too large Handle ratio is too large for the rapid traverse rate (or external deceleration speed when external deceleration is valid).
Set a smaller ratio.
0065 R-pos offset value illegal At the start of reference position initial setting, setting of reference position offset value (#2034 rfpofs) is other than 0.
Set the reference position offset value (#2034 rfpofs) to 0, then turn the power ON again to perform reference position initial setting.
0066 R-pos scan distance exceeded Reference position could not be established within the maximum scan distance.
Check the scale to see if it has dirt or damage. Check if the servo drive unit supports this
function.
Appendix 6. Alarms 6.1 List of Alarms
IV - 30
Error No. Details Remedy
0101 No operation mode Check for a broken wire in the input mode signal wire.
Check for trouble in the mode selector switch. Check the sequence program.
0102 Cutting override zero The "cutting feed override" switch on the machine operation panel is set to zero. The override was set to "0" during a single block stop.
Set the "cutting feed override" switch to a value other than zero to clear the error.
When the "cutting feed override" switch is set to a value other than zero check for a short circuit in the signal wire.
Check the sequence program. 0103 External feed rate zero
"The manual feed speed" switch on the machine operation panel is set to zero when the machine is in the jog mode or automatic dry run mode. The "Manual feedrate B speed" is set to zero during the jog mode when manual feedrate B is valid. The "each axis manual feedrate B speed" is set to zero during the jog mode when each axis manual feedrate B is valid.
Set "the manual feed speed" switch to a value other than zero to release the error.
If "the manual feed speed" switch is set to a value other than zero check for a short circuit in the signal wire.
Check the sequence program.
0104 F 1-digit feed rate zero The F1-digit feedrate is set to zero when the F1-digit feed command is being executed.
Set the F1-digit feedrate on the setup parameter screen.
0105 Spindle stop The spindle stopped during the synchronous feed command.
Rotate the spindle. If the workpiece is not being cut start dry run. Check for a broken wire in the spindle encoder
cable. Check the connections for the spindle encoder
connectors. Check the spindle encoder pulse. Reconsider the program. (Command, address)
0106 Handle feed ax No. illegal An axis not found in the specifications was designated for handle feed or the handle feed axis was not selected.
Check for broken wires in the handle feed axis selection signal wire.
Check the sequence program. Check the No. of axes listed in the
specifications. 0107 Spindle rotation speed over
The spindle rotation speed exceeded the axis clamp speed during the thread cutting command.
Lower the commanded spindle rotation speed.
0108 Fixed pnt mode feed ax illegal An axis not found in the specifications was designated for the fixed point mode feed or the fixed point mode feedrate is illegal.
Check for broken wires in the fixed mode feed axis selection signal wire and fixed point mode feedrate wire.
Check the fixed point mode feed specifications. 0109 Block start interlock
An interlock signal that locks the start of the block has been input.
Check the sequence program.
0110 Cutting block start interlock An interlock signal that locks the start of the cutting block has been input.
Check the sequence program.
Appendix 6. Alarms 6.1 List of Alarms
IV - 31
Error No. Details Remedy
0111 Restart switch ON The restart switch was turned ON before the restart search was completed, and the manual mode was selected.
Search the block to be restarted. Turn OFF the restart switch.
0112 Program check mode The automatic start button was pressed during program check or in program check mode.
Press the reset button to cancel the program check mode.
0113 Auto start in buffer correct The automatic start button was pressed during buffer correction.
Press the automatic start button after buffer correction is completed.
0115 In reset process The automatic start button was pressed during resetting or tape rewinding.
When rewinding the tape wait for the winding to end or press the reset button to stop the winding and then press the automatic start button.
During resetting wait for resetting to end and then press the automatic start button.
0117 Playback not possible The playback switch was turned ON during editing.
During editing cancel the function by pressing the input or previous screen key and then turn ON the playback switch.
0118 Turn stop in normal line cntrl The turning angle at the block joint exceeded the limit during normal line control.
Normal line control type I The normal line control axis turning speed (#1523 C_feed) has not been set.
Normal line control type II When turning in the inside of the arc, the parameter "#8041 C-rot. R" setting value is larger than the arc radius.
Check the program. Set the normal line control axis turning speed.
(Parameter "#1523 C_feed") Set the C axis turning diameter smaller than the
arc radius, or check the setting value of the C axis turning diameter. (Parameter "#8041 C rot. R")
0119 Reverse run impossible Any of the following conditions are occurring. a) There is no block to run backward b) Eight blocks without a travel command continued
a) Release with forward run. b) Release with reset.
0120 In synchronous correction mode The synchronous correction mode switch was pressed in a non-handle mode.
Select the handle or manual feed mode. Turn OFF the correction mode switch.
0121 No synchronous control option The synchronous control system (register R2589) was set with no synchronous control option.
Set 0 in register R2589.
0123 Computer link B not possible The cycle start was attempted before resetting was completed. An attempt was made to perform computer link B operation at the second part system and following in a multi-part system.
Perform the cycle start after resetting is completed.
Set 0 in "#8109 HOST LINK", and then set 1 again before performing the cycle start.
The computer link B operation cannot be performed at the second part system and following in a multi-part system.
0124 X/Z axes simultaneous prohibit The basic axis corresponding to the inclined axis was started simultaneously in the manual mode while the inclined axis control was valid.
Turn the inclined axis and basic axis start OFF for both axes. (This also applied for manual/automatic simultaneous start.)
Invalidate the basic axis compensation, or command one axis at a time.
Appendix 6. Alarms 6.1 List of Alarms
IV - 32
Error No. Details Remedy
0125 Rapid override zero The "rapid traverse override" switch on the machine operation panel is set to zero.
Set the "rapid traverse override" switch to a value other than zero to clear the error.
When the "rapid traverse override" switch is set to a value other than zero, check for a short circuit in the signal wire.
Check the sequence program. 0126 Program restart machine lock
Machine lock was applied on the return axis while manually returning to the restart position.
Release the machine lock before resuming operations.
0127 Rot axis parameter error The orthogonal coordinate axis name does not exist. The rotary axis name does not exist. The orthogonal coordinate axis name is duplicated. The number of axes that were selected to change tool length compensation along the tool axis amount exceeds the maximum number of axes. The orthogonal coordinate axis name is that of the rotary axis name.
Review the rotational axis configuration parameters.
0128 Restart pos return incomplete Automatic return was performed with an axis whose return to the restart position was not complete.
Perform restart position return manually. Validate the parameter "automatic return by
program restart" (#1302 AutoRP), then execute automatic start.
0150 Chopping override zero The override became "0" while performing the chopping operation.
Check the chopping override (R2530). Check the rapid traverse override (R2502).
0151 Command axis chopping axis A chopping axis movement command was issued from the program during the chopping mode. (This alarm will not occur when the movement amount is commanded as 0.) (All axes interlock state will be applied.)
Reset, or turn OFF the chopping signal. When the chopping signal is turned OFF, the axis will return to the reference position, and then the program movement command will be executed.
0153 Bottom dead center pos. zero The bottom dead center position is set to the same position as the upper dead center position.
Correctly set the bottom dead center position.
0154 Chopping disable for handle ax Chopping was started when the chopping axis was selected as the handle axis.
Select an axis other than the chopping axis as the handle axis, or start chopping after changing the mode to another mode.
0160 No speed set out of soft limit Returned from the outside of the soft limit range for the axis with no maximum speed set for the outside of the soft limit range.
Set the maximum speed for the outside of the soft limit range. (Parameter "#2021 out_f")
Change the soft limit range. (Parameter "#2013 OT-" "#2014 OT+")
Appendix 6. Alarms 6.1 List of Alarms
IV - 33
Error No. Details Remedy
0166 Aux axis changeover error One of the following attempts was made on an axis that is switchable between NC axis and auxiliary axis.
A command was issued to an auxiliary axis from machining program.
When there were more than one NC axis having a same name, a command was issued to those axes from machining program.
NC axis control select signal was turned OFF while the NC axis was in motion.
NC axis control select signal was turned ON while the auxiliary axis was in motion.
If you wish to issue a command to the axis from machining program, turn ON the NC axis control select signal so as to set the axis as an NC axis.
When more than one axis have a same name, let only one of the axes work as an NC axis.
Do not change NC axis control select signal while the axis is in motion.
0170 Ill. op during T tip control An attempt was made to perform an incorrect operation during tool tip center control.
Change to the previous operation mode and reboot.
1005 G114.n command illegal An attempt was made to execute G114.n during execution of G114.n. G51.2 was commanded when the G51.2 spindle-spindle polygon machining mode was already entered with a separate part system.
Cancel with G113. Issue the spindle synchronous cancel signal
(Y18B8: SPSYC). Cancel with G50.2. Cancel with the spindle-spindle polygon cancel
signal (YCD1). 1007 Spindle in-use by synchro tap
The spindle is being used in synchronized tapping.
Cancel synchronized tapping.
1026 SP-C ax ctrl runs independntly C axis mode command was issued for polygon machining spindle. C axis mode command was issued for synchronized tapping spindle. Polygon command was issued for synchronized tapping spindle. Spindle is being used as spindle/C axis.
Cancel the C axis command. Cancel the polygon machining command. Cancel the C axis with servo OFF.
1030 Synchronization mismatch Different M codes were commanded in the two part systems as the synchronization M codes. Synchronization with the "!" code was commanded in another part system during M code synchronization. Synchronization with the M code was commanded in another part system during synchronization with the "!" code.
Correct the program so that the M codes match.
Correct the program so that the same synchronization codes are commanded.
1031 Multiple C axes select invalid The C axis selection signal was changed when multiple C axes could not be selected. An axis that cannot be controlled as the multiple C axes selection was selected.
Check and correct the parameters and program.
Appendix 6. Alarms 6.1 List of Alarms
IV - 34
Error No. Details Remedy
1032 Tap retract Sp select illegal Tap return was executed when a different spindle was selected. Cutting feed will wait until synchronization is completed.
Select the spindle for which tap cycle was halted before the tap return signal was turned ON.
1033 Sp-Sp polygon cut interlock Cutting feed will wait until synchronization is completed.
Wait for synchronization to end.
1034 Mixed sync ctrl prmtr illegal Mixed synchronization control exceeding the number of control axes was attempted. Mixed synchronization control with duplicated axis addresses was attempted.
Check the parameter settings for mixed synchronization control.
1035 Mixed sync ctrl disable modal Mixed synchronization was commanded for a part system in which mixed synchronization control is disabled as shown below.
During nose R compensation mode During pole coordinate interpolation mode During cylindrical interpolation mode During balance cut mode During fixed cycle machining mode During facing turret mirror image
Check the program.
1036 Synchro ctrl setting disable The synchronous control operation method selection (R2589 register) was set when the mode was not the C axis mode. The synchronous control operation method selection (R2589 register) was set in the zero point not set state.
Mirror image disable state The external mirror image or parameter mirror image was commanded during facing turret mirror image.
Set the R2589 register to 0. Check the program and parameters.
1037 Synchro start/cancel disable Synchronous control was started or canceled when synchronous control could not be started or canceled.
Check the program and parameters.
1038 Move cmnd invld to synchro ax A movement command was issued to a synchronous axis in synchronous control.
Check the program.
1106 Sp synchro phase calc illegal The spindle synchronization phase alignment command was issued while the spindle synchronization phase calculation request signal was ON.
Check the program. Check the sequence program.
Appendix 6. Alarms 6.1 List of Alarms
IV - 35
(2) Class: M90 Message: Parameter set mode
M90 Messages output when the setup parameter lock function is enabled are displayed.
Error No. Details Remedy -Setup parameter lock released
The setup parameter lock is released. Automatic start is disabled when setup parameters can be set.
Refer to the manual issued by the machine tool builder.
Appendix 6. Alarms 6.1 List of Alarms
IV - 36
6.1.2 Stop Codes These codes indicate a status that caused the controller to stop for some reason. (The bold characters are the messages displayed on the screen.)
T Message
Error No. Message Class
(1) Class: T01 Cycle start prohibit
This indicates the state where automatic operation cannot be started when attempting to start it from the stop state.
Error No. Details Remedy 0101 Axis in motion
Automatic start is not possible as one of the axes is moving.
Try automatic start again after all axes have stopped.
0102 NC not ready Automatic start is not possible as the NC is not ready.
Another alarm has occurred. Check the details and remedy.
0103 Reset signal ON Automatic start is not possible as the reset signal has been input.
Turn OFF the reset input signal. Check that the reset switch is not ON
constantly due to trouble. Check the sequence program.
0104 Auto operation pause signal ON The FEED HOLD switch on the machine operation panel is ON (valid).
Check the FEED HOLD switch. The feed hold switch is the B contact. Check for broken wires in the feed hold signal
wire. Check the sequence program.
0105 H/W stroke end axis exists Automatic start is not possible as one of the axes is at the stroke end.
If one of the axis' ends is at the stroke end move the axis manually.
Check for broken wire in the stroke end signal wire.
Check for trouble in the stroke end limit switch. 0106 S/W stroke end axis exists
Automatic start is not possible as one of the axes is at the stored stroke limit.
Move the axis manually. If an axis is not at the end check the parameter
details. 0107 No operation mode
The operation mode has not been selected. Select the automatic operation mode. Check for broken wires in the automatic
operation mode (memory tape MDl) signal wire.
0108 Operation mode duplicated Two or more automatic operation modes are selected.
Check for a short circuit in the mode selection signal wire (memory tape MDl).
Check for trouble in the switch. Check the sequence program.
0109 Operation mode changed The automatic operation mode changed to another automatic operation mode.
Return to the original automatic operation mode and start automatic start.
Appendix 6. Alarms 6.1 List of Alarms
IV - 37
Error No. Details Remedy
0110 Tape search execution Automatic start is not possible as tape search is being executed.
Begin automatic start after the tape search is completed.
0112 Restart pos. return incomplete Automatic start is not possible as the axis has not been returned to the restart position.
Manually return to the restart position. Turn the automatic restart valid parameter ON,
and then execute automatic start. 0113 CNC overheat
Automatic start is not possible because a thermal alarm (Z53 CNC overheat) has occurred.
The NC controller temperature has exceeded the specified temperature.
Take appropriate measures to cool the unit.
0115 Cycle st. prohibit(Host comm.) Automatic start cannot be executed as the NC is communicating with the host computer.
Execute automatic start after the communication with the host computer is completed.
0116 Cycle st prohibit(Battery alm) Automatic start cannot be executed because the voltage of the battery inserted in the NC control unit has dropped.
Replace the battery of the NC control unit. Contact the service center.
0117 R-pnt offset value not set As the reference position offset value has not been set, automatic operation cannot be used.
Perform the initial reference position setting, then set the reference position offset value (#2034 rfpofs).
0138 In absolute position alarm A start signal was input during an absolute position detection alarm.
Reset the absolute position detection alarm and then input the start signal.
0139 In abs posn initial setting A start signal was input while initializing the absolute position detector's zero point.
Complete zero point initialization before inputting the start signal.
0180 Cycle start prohibit Automatic start is disabled in servo auto turning valid.
Set "0" to "#1164 ATS" when the servo auto turning is not executed.
0190 Cycle start prohibit Automatic start is disabled because setup parameters can be set.
Refer to the manual issued by the machine tool builder.
0191 Cycle start prohibit Automatic start was caused during file deletion or writing.
Cause automatic start after file deletion or writing is completed.
0193 Cycle st. prohibit (Term exp'd) Automatic start is disabled because the valid term has been expired.
Enter the decryption code and turn the power ON again.
Appendix 6. Alarms 6.1 List of Alarms
IV - 38
(2) Class: T02 Feed hold
The feed hold state been entered due to a condition in the automatic operation.
Error No. Details Remedy 0201 H/W stroke end axis exists
An axis is at the stroke end. Manually move the axis away from the stroke
end limit switch. The machining program must be corrected.
0202 S/W stroke end axis exists An axis is at the stored stroke limit.
Manually move the axis. The machining program must be corrected.
0203 Reset signal ON The reset signal has been input.
The program execution position has returned to the start of the program. Execute automatic operation from the start of the machining program.
0204 Auto operation pause signal ON The FEED HOLD switch is ON.
Resume automatic operation by pressing the "CYCLE START" switch.
0205 Operation mode changed The operation mode changed to another mode during automatic operation.
Return to the original automatic operation mode and resume automatic operation by pressing the "CYCLE START" switch.
0206 Acc/dec time cnst too large The acceleration and deceleration time constants are too large. (This problem occurs at the same time as system alarm Z59.)
Increase the set value of the parameter "#1206 G1bF".
Decrease the set value of the parameter "#1207 G1btL".
Lower the cutting speed. 0215 Abs posn detect alarm occurred
An absolute position detection alarm occurred. Reset the absolute position detection alarm.
0220 Aux axis changeover error A movement command was issued to an auxiliary axis.
When NC axis control selection signal is ON, automatic operation can be resumed by pressing the "CYCLE START" switch.
Appendix 6. Alarms 6.1 List of Alarms
IV - 39
(3) Class: T03 Block stop
This indicates that automatic operation stopped after executing one block of the program.
Error No. Details Remedy 0301 Single block stop signal ON
The SINGLE BLOCK switch on the machine operation panel is ON. The single block or machine lock switch changed.
Automatic operation can be resumed by turning the CYCLE START switch ON.
0302 Block stop cmnd in user macro The block stop command was issued in the user macro program.
Automatic operation can be resumed by turning the CYCLE START switch ON.
0303 Operation mode changed The automatic mode changed to another automatic mode.
Return to the original automatic operation mode and resume automatic operation by turning the CYCLE START switch ON.
0304 MDI completed The last block of MDI was completed.
Set MDI again and turn the CYCLE START switch ON to resume MDl operation.
0305 Block start interlock The interlock signal that locks the block start is entered.
Check the sequence program.
0306 Cutting blck start interlock The interlock signal that locks the block cutting start is entered.
Check the sequence program.
0310 Inclined Z offset change Whether to validate the offset of the inclined Z-axis switched during program operation.
Automatic operation can be restarted by turning ON the CYCLE START switch.
0330 Aux axis changeover error NC axis control selection signal was OFF while traveling NC axis.
When NC axis control selection signal is ON, automatic operation can be resumed by pressing the "CYCLE START" switch.
(4) Class: T04 Collation stop
This indicates that collation stop was applied during automatic operation.
Error No. Details Remedy 0401 Collation stop
Collation stop occurred. Automatic operation can be restarted with
automatic start.
Appendix 6. Alarms 6.1 List of Alarms
IV - 40
(5) Class: T10 Fin wait
This indicates the operation state when an alarm did not occur during automatic operation and nothing seems to have happened.
Error No. Details 0 The error number is displayed while each of the completion wait modes listed in the table below is
ON. It disappears when the mode is canceled.
0
Alarm No.
Unclamp signal wait (Note 2)
In dwell execu- tion
Alarm No.
Door open (Note 1)
Waiting for spindle position to be looped
Alarm No.
Waiting for spindle orienta- tion to complete
Waiting for cutting speed decelera- tion
Waiting for rapid traverse decelera- tion
Waiting for MSTB comp- letion
0 0 0
1 1 1
8 8 2
9 9 3
4
5
6
7
8
9
A
B
C
D
E
F
(Note 1) This mode is enabled by the door interlock function. (Note 2) The system is waiting for the index table indexing unclamp signal to turn ON or OFF
Appendix 6. Alarms 6.1 List of Alarms
IV - 41
6.1.3 Servo/Spindle Alarms This section describes alarms occurred by the errors in the servo system such as the drive unit motor and encoder, etc. The alarm message alarm No. and axis name will display on the alarm message screen. The axis where the alarm occurred and the alarm No. will also display on the servo monitor screen and the spindle monitor screen respectively. If several alarms have occurred up to two errors per axis will display on the servo monitor screen and the spindle monitor screen respectively.
(Note 1) The alarm class and alarm reset method combinations are preset. Alarm class Reset method Resetting methods S01 PR After removing the cause of the alarm, reset the
alarm by turning the NC power ON again.
S02 PR After correcting the parameter, reset the alarm by turning ON the NC power again.
S03 NR After removing the cause of the alarm, reset the alarm by inputting the NC RESET key.
S04 AR After removing the cause of the alarm, reset the alarm by turning the drive unit power ON again.
S51 - This is cleared if a correct value is set. S52 - -
(Note 2) The resetting method may change according to the alarm class. For example, even if "S03 SERVO ALARM: NR" is displayed, it may be necessary to turn the NC
power ON again.
S Message : xx
Axis name
Alarm No. (Parameter No.)
Reset method
Message
Alarm class
Servo : Axis name
Spindle : "S1","S2","S3","S4"
Appendix 6. Alarms 6.1 List of Alarms
IV - 42
(1) Class: S01/S03/S04 Servo alarm (a) Servo drive unit alarm
No. Message Details Reset method Stop method
0010 Insufficient voltage A drop of bus voltage was detected in main circuit. PR Dynamic stop 0011 Axis selection error The axis selection rotary switch has been incorrectly set. AR Initial error 0012 Memory error 1 A hardware error was detected during the power ON
self-check. AR Initial error
0013 Software processing error 1 An error was detected for the software execution state. PR Dynamic stop 0016 Init mag pole pos detect err The initial magnetic pole position, detected in the initial
magnetic pole position detection control, is not reliable. In the DC excitation function, this error will be detected when the servo ON has been set before the magnetic pole shift amount is set while the absolute position detector is used.
PR Dynamic stop
0017 A/D converter error A current feedback error was detected. PR Dynamic stop 0018 Motor side dtc: Init commu err An error was detected in the initial communication with
the motor side detector. PR Initial error
001A Machine side dtc: Init comu er An error was detected in the initial communication with the machine side detector.
PR Initial error
001B Machine side dtc: Error 1 001C Machine side dtc: Error 2 001D Machine side dtc: Error 3 001E Machine side dtc: Error 4
An error was detected by the detector connected to the machine side. The error details are different according to the connected detector. Refer to "Detector alarm".
Dynamic stop
001F Machine side dtc: Commu error An error was detected in the communication with the machine side detector.
PR Dynamic stop
0021 Machine side dtc: No signal An error was detected in the ABZ-phase in the full closed loop control system.
PR Dynamic stop
0024 Grounding The motor power cable is in contact with FG (Frame Ground).
PR Dynamic stop
0025 Absolute position data lost The absolute position was lost in the detector. AR Initial error 0026 Unused axis error A power module error was detected on the axis set to
Free. PR Dynamic stop
0027 Machine side dtc: Error 5 0028 Machine side dtc: Error 6 0029 Machine side dtc: Error 7 002A Machine side dtc: Error 8
An error was detected by the detector connected to the machine side. The error details are different according to the connected detector. Refer to "Detector alarm".
Dynamic stop
002B Motor side dtc: Error 1 002C Motor side dtc: Error 2 002D Motor side dtc: Error 3 002E Motor side dtc: Error 4
An error was detected by the detector connected to the motor side. The error details are different according to the connected detector. Refer to "Detector alarm".
Dynamic stop
002F Motor side dtc: Commu error An error was detected in the communication with the motor side detector.
PR Dynamic stop
0030 Over regeneration Over-regeneration level exceeded 100%. The regenerative resistor is overloaded.
PR Dynamic stop
0031 Overspeed The motor speed exceeded the allowable speed. PR Deceleration stop enabled
0032 Power module overcurrent The power module detected the overcurrent. PR Dynamic stop 0033 Overvoltage The bus voltage in main circuit exceeded the allowable
value. PR Dynamic stop
0034 NC-DRV commu: CRC error An error was detected in the data received from the NC. PR Deceleration stop enabled
Appendix 6. Alarms 6.1 List of Alarms
IV - 43
No. Message Details Reset
method Stop method
0035 NC command error The travel command data received from the NC was excessive.
PR Deceleration stop enabled
0036 NC-DRV commu: Commu error The communication with the NC was interrupted. PR Deceleration stop enabled
0037 Initial parameter error An incorrect set value was detected among the parameters send from the NC at the power ON.
PR Initial error
0038 NC-DRV commu: Protocol error 1 An error was detected in the communication frames received from the NC.
PR Deceleration stop enabled
0039 NC-DRV commu: Protocol error 2 An error was detected in the axis data received from the NC.
PR Deceleration stop enabled
003A Overcurrent Excessive motor drive current was detected. PR Dynamic stop 003B Power module overheat The power module detected an overheat. PR Dynamic stop 003C Regeneration circuit error An error was detected in the regenerative transistor or in
the regenerative resistor. PR Dynamic stop
003D Pw sply volt err acc/dec A motor control error, due to an input voltage failure, was detected.
PR Dynamic stop
003E Magnet pole pos detect err The magnetic pole position, detected in the magnetic pole position detection control, is not reliable.
AR Dynamic stop
0041 Feedback error 3 Either a missed feedback pulse in the motor side detector or an error in the Z-phase was detected in the full closed loop system.
PR Dynamic stop
0042 Feedback error 1 Either a missed feedback pulse in the detector used for the position detection or an error in the Z-phase was detected.
PR Dynamic stop
0043 Feedback error 2 An excessive difference in feedback was detected between the machine side detector and the motor side detector.
PR Dynamic stop
0045 Fan stop An overheat of the power module was detected during the cooling fan stopping.
PR Dynamic stop
0046 Motor overheat Either the motor or the motor side detector detected an overheat.
NR Deceleration stop enabled
0048 Motor side dtc: Error 5 0049 Motor side dtc: Error 6 004A Motor side dtc: Error 7 004B Motor side dtc: Error 8
An error was detected by the detector connected to the motor side. The error details are different according to the connected detector. Refer to "Detector alarm".
Dynamic stop
004F Instantaneous power interrupt The control power supply has been shut down for 50ms or more.
NR Deceleration stop enabled
0050 Overload 1 Excessive load current was detected. NR Deceleration stop enabled
0051 Overload 2 Excessive load current was detected. NR Deceleration stop enabled
0052 Excessive error 1 A position tracking error was detected. (during servo ON) NR Deceleration stop enabled
0053 Excessive error 2 A position tracking error was detected. (during servo OFF) NR Dynamic stop
0054 Excessive error 3 The anomalous motor current was detected at the detection of Excessive error 1. NR Dynamic stop
0058 Collision detection 1: G0 A disturbance torque exceeded the tolerable disturbance torque in rapid traverse modal (G0). The tolerable disturbance torque is decided by SV060:TLMT.
NR Maximum capacity deceleration stop
0059 Collision detection 1: G1 A disturbance torque exceeded the tolerable disturbance torque in the cutting feed modal (G1). The tolerable disturbance torque is decided by SV060:TLMT and SV035:SSF4/clG1(bitC, bitD and bitE).
NR Maximum capacity deceleration stop
005A Collision detection 2 A current command with the maximum capacity current value was detected.
NR Maximum capacity deceleration stop
005B Sfty obsrvation: Cmd spd err A commanded speed exceeding the safe speed was detected in speed monitoring mode.
PR Deceleration stop enabled
Appendix 6. Alarms 6.1 List of Alarms
IV - 44
No. Message Details Reset
method Stop method
005D Sfty obsrvation: Door stat err
The door state signal input in the NC does not coincide with the door state signal input in the drive unit. Otherwise, door open state was detected in normal mode.
PR Deceleration stop enabled
005E Sfty obsrvation: FB speed err A motor speed exceeding the safe speed was detected in the speed monitoring mode.
PR Deceleration stop enabled
005F External contactor error A contact of the external contactor is welding. NR Deceleration stop enabled
0060
0077
Power supply alarm The power supply unit detected an error. The error details are different according to the connected power supply unit. Refer to "Power supply alarm".
Dynamic stop
0080 Motor side dtc: cable err A difference of type was detected between the motor side detector and the cable connected to the detector. Otherwise, the cable type for the motor side detector was not successfully achieved.
AR Initial error
0081 Machine side dtc: cable err A difference of type was detected between the machine side detector and the cable connected to the detector. Otherwise, the cable type for the machine side detector was not successfully achieved.
AR Initial error
0087 Drive unit communication error The communication frame between drivers was aborted. PR Dynamic stop 0088 Watchdog The drive unit does not operate correctly. AR Dynamic stop 008A Drivers commu data error 1 The communication data 1 between drivers exceeded the
tolerable value in the communication between drivers. PR Dynamic stop
008B Drivers commu data error 2 The communication data 2 between drivers exceeded the tolerable value in the communication between drivers.
PR Dynamic stop
(Note1) Definitions of terms in the table are as follows. Motor side detector: Detector connected to CN2 Machine side detector: Detector connected to CN3
(Note2) Resetting methods NR: Reset with the NC RESET button. This alarm can also be reset with the PR and AR resetting conditions. PR: Reset by turning the NC power ON again. This alarm can also be reset with the AR resetting conditions.
When the control axis is removed, this alarm can be reset with the NC RESET button. (Excluding alarms 32 and 37.) AR: Reset by turning the servo drive unit power ON again.
Separate table : Detector alarm (Servo drive unit)
Alarm number when the detector is connected to the motor side 2B 2C 2D 2E 48 49 4A 4B
Alarm number when the detector is connected to the machine side 1B 1C 1D 1E 27 28 29 2A
OSA17 OSE104, OSE105 OSA104, OSA105 OSA405, OSA166
Memory alarm LED alarm Data alarm - - - - -
OSA18 CPU alarm - Data alarm - - - - -
MDS-B-HR
MITSUBISHI
Memory error - Data error - Scale not connected - - -
AT343, AT543 Mitutoyo Initialization error
EEPROM error
Photoelectric type, static
capacity type data
mismatch
ROM/RAM error CPU error
Photoelectric type
overspeed
Static capacity type
error
Photoelectric type error
LC191M, LC491M RCN723, RCN223
APE391M HEIDENHAIN Initialization
error EEPROM
error
Relative/ absolute
position data mismatch
ROM/RAM error CPU error Overspeed
Absolute position data
error
Relative position data
error
Futaba absolute position scale Futaba - - - - - - Waveform
error
Overspeed Absolute position is
lost
MP scale, MPI scale
Mitsubishi Heavy
Industries
Installation accuracy
fault -
Detection position deviance
Scale breaking
Absolute value
detection fault
- Gain fault Phase fault
MJ831 SONY - - - - - - - Detector alarm
(Note1) Definitions of terms in the table are as follows. Motor side detector: Detector connected to CN2 Machine side detector: Detector connected to CN3
(Note2) A driver processes all reset types of alarms as "PR". However, "AR" will be applied according to the detector.
Appendix 6. Alarms 6.1 List of Alarms
IV - 45
(b) Spindle drive unit alarm
No. Message Details Reset method Stop method
0010 Insufficient voltage A drop of bus voltage was detected in main circuit. PR Coast to a stop 0011 Axis selection error The axis selection rotary switch has been incorrectly set. AR Initial error 0012 Memory error 1 A hardware error was detected during the power ON
self-check. AR Initial error
0013 Software processing error 1 An error was detected for the software execution state. PR Coast to a stop 0016 Init mag pole pos detect err The magnetic pole position, detected in the initial
magnetic pole position detection control, is not reliable. PR Coast to a stop
0017 A/D converter error A current feedback error was detected. PR Coast to a stop 0018 Motor side dtc: Init commu err An error was detected in the initial communication with
the motor side detector. PR Initial error
0019 Detector commu err in syn cont An error was detected in the communication with the extended connection detector.
PR Coast to a stop
001A Machine side dtc: Init comu er An error was detected in the initial communication with the machine side detector.
PR Initial error
001B Machine side dtc: Error 1 001C Machine side dtc: Error 2 001D Machine side dtc: Error 3 001E Machine side dtc: Error 4
An error was detected by the detector connected to the machine side. The error details are different according to the connected detector. Refer to "Detector alarm".
Coast to a stop
001F Machine side dtc: Commu error An error was detected in the communication with the machine side detector.
PR Coast to a stop
0020 Motor side dtc: No signal The cable type of the motor side detector does not coincide with the detector type set with the parameter.
PR Initial error
The cable type of the machine side detector does not coincide with the detector type set with the parameter.
PR Initial error 0021 Machine side dtc: No signal Excessive speed error
An error was detected in the ABZ-phase in the full closed loop control system.
PR Coast to a stop
0023 Grounding An excessive speed tracking error was detected (during servo ON).
NR Coast to a stop
0024 Machine side dtc: No signal A grounding of the motor power cable or motor was detected.
AR Coast to a stop
0026 Unused axis error A power module error was detected on the axis set to Free.
PR Coast to a stop
0027 Machine side dtc: Error 5 0028 Machine side dtc: Error 6 0029 Machine side dtc: Error 7 002A Machine side dtc: Error 8
An error was detected by the detector connected to the machine side. The error details are different according to the connected detector. Refer to "Detector alarm".
Coast to a stop
002B Motor side dtc: Error 1 002C Motor side dtc: Error 2 002D Motor side dtc: Error 3 002E Motor side dtc: Error 4
An error was detected by the detector connected to the motor side. The error details are different according to the connected detector. Refer to "Detector alarm".
Coast to a stop
002F Motor side dtc: Commu error An error was detected in the communication with the motor side detector.
PR Coast to a stop
0030 Over regeneration Over-regeneration level exceeded 100%. The regenerative resistor is overloaded.
PR Coast to a stop
0031 Overspeed The motor speed exceeded the allowable speed. PR Deceleration stop enabled
0032 Power module overcurrent The power module detected the overcurrent. PR Coast to a stop 0033 Overvoltage The bus voltage in main circuit exceeded the allowable
value. PR Coast to a stop
0034 NC-DRV commu: CRC error An error was detected in the data received from the NC. PR Deceleration stop enabled
0035 NC command error An error was detected in the travel command data received from the NC.
PR Deceleration stop enabled
0036 NC-DRV commu: Commu error The communication with the NC was interrupted. PR Deceleration stop enabled
0037 Initial parameter error An incorrect set value was detected among the parameters send from the NC at the power ON.
PR Initial error
Appendix 6. Alarms 6.1 List of Alarms
IV - 46
No. Message Details Reset
method Stop method
0038 NC-DRV commu: Protocol error 1 An error was detected in the communication frames received from the NC.
PR Deceleration stop enabled
0039 NC-DRV commu: Protocol error 2 An error was detected in the axis data received from the NC.
PR Deceleration stop enabled
003A Overcurrent Excessive motor drive current was detected. PR Coast to a stop 003B Power module overheat The power module detected an overheat. PR Coast to a stop 003C Regeneration circuit error An error was detected in the regenerative transistor or in
the regenerative resistor. PR Coast to a stop
003E Magnet pole pos detect err The magnetic pole position, detected in the magnetic pole position detection control, is not reliable.
AR Coast to a stop
0041 Feedback error 3 An error was detected in the feedback of the motor side detector.
PR Coast to a stop
0042 Feedback error 1 An error was detected in the feedback of the machine side detector.
PR Coast to a stop
0043 Feedback error 2 An excessive difference in feedback was detected between the motor side detector and the machine side detector.
PR Coast to a stop
0045 Fan stop A cooling fan in the drive unit stopped. PR Coast to a stop 0046 Motor overheat Either the motor or the motor side detector detected an
overheat. NR Deceleration stop
enabled 0048 Motor side dtc: Error 5 0049 Motor side dtc: Error 6 004A Motor side dtc: Error 7 004B Motor side dtc: Error 8
An error was detected by the detector connected to the motor side. The error details are different according to the connected detector. Refer to "Detector alarm".
Coast to a stop
004C Current err mag pole estim Current detection failed at the pulse-applied magnetic pole estimation by IPM spindle motor.
NR Coast to a stop
004E NC command mode error An error was detected in the spindle control mode send from the NC.
NR Deceleration stop enabled
004F Instantaneous power interrupt The control power supply has been shut down for 50ms or more.
NR Deceleration stop enabled
0050 Overload 1 Excessive load current was detected. NR Deceleration stop enabled
0051 Overload 2 Excessive load current was detected. NR Deceleration stop enabled
0052 Excessive error 1 A position tracking error was detected. (during servo ON) NR Deceleration stop enabled
0054 Excessive error 3 The anomalous motor current was detected at the detection of Excessive error 1.
NR Coast to a stop
005B Sfty obsrvation: Cmd spd err A commanded speed exceeding the safe speed was detected in speed monitoring mode.
PR Deceleration stop enabled
005D Sfty obsrvation: Door stat err
The door state signal input in the NC does not coincide with the door state signal input in the drive unit. Otherwise, door open state was detected in normal mode.
PR Deceleration stop enabled
005E Sfty obsrvation: FB speed err A motor speed exceeding the safe speed was detected in the speed monitoring mode.
PR Deceleration stop enabled
005F External contactor error A contact of the external contactor is welding. NR Deceleration stop enabled
0060
0077
Power supply alarm The power supply unit detected an error. The error details are different according to the connected power supply unit. Refer to "Power supply alarm".
Coast to a stop
0080 Motor side dtc: cable err The connected cable type does not coincide with the motor side detector type. PR Initial error
0081 Machine side dtc: cable err The connected cable type does not coincide with the machine side detector type. PR Initial error
0087 Drive unit communication error The communication frame between drivers was aborted. PR Coast to a stop 0088 Watchdog The drive unit does not operate correctly. AR Coast to a stop 008A Drivers commu data error 1 The communication data 1 between drivers exceeded the
tolerable value in the communication between drivers. PR Coast to a stop
008B Drivers commu data error 2 The communication data 2 between drivers exceeded the tolerable value in the communication between drivers. PR Coast to a stop
(Note) Resetting methods NR: Reset with the NC RESET button. This alarm can also be reset with the PR and AR resetting conditions. PR: Reset by turning the NC power ON again. This alarm can also be reset with the AR resetting conditions.
When the control axis is removed, this alarm can be reset with the NC RESET button. (Excluding alarms 32 and 37.) AR: Reset by turning the servo drive unit power ON again.
Appendix 6. Alarms 6.1 List of Alarms
IV - 47
Separate table : Detector alarm (Spindle drive unit)
Alarm number when the detector is connected to the motor side 2B 2C 2D 2E 48 49 4A 4B
Alarm number when the detector is connected to the machine side 1B 1C 1D 1E 27 28 29 2A
TS5690 TS5691 Memory error Waveform
error - - - Overspeed - Relative
position data error
MDS-B-HR Initialization error - Data error - Connection
error - - -
OSA18
MITSUBISHI
CPU error - Data error - - - - -
ERM280 +
APE391M HEIDENHAIN Initialization
error EEPROM
error - - CPU error Overspeed - Relative
position data error
MPCI scale Mitsubishi
Heavy Industries
Installation accuracy
fault -
Detection position deviance
Scale breaking - - Gain fault Phase fault
(Note) A driver processes all reset types of alarms as "PR". However, "AR" will be applied according to the detector.
(c) Power supply alarm
No. LED display Message Details Reset
method 0061
Pw sply: Pwr module overcurnt Overcurrent protection function in the power module has started its
operation. PR
0062
Pw sply: Frequency error The input power supply frequency increased above the
specification range. PR
0067
Pw sply: Phase interruption An open-phase condition was detected in input power supply circuit. PR
0068
Pw sply: Watchdog The system does not operate correctly. AR
0069
Pw sply: Grounding The motor power cable is in contact with FG (Frame Ground). PR
006A
Pw sply: Ext contactor weld A contact of the external contactor is welding. PR
006B
Pw sply: Rush relay welding A resistor relay for rush short circuit fails to be OFF. PR
006C
Pw sply: Main circuit error An error was detected in charging operation of the main circuit
capacitor. PR
006E
Pw sply: Memory error/AD error An error was detected in the internal memory or A/D converter. AR
006F
Power supply error No power supply is connected to the drive unit, or a communication
error was detected. AR
0070
Pw sply: Ext emergency stp err A mismatch of the external emergency stop input and NC
emergency stop input continued for 30 seconds. PR
0071
Pw sply: Instant pwr interrupt The power was momentarily interrupted. NR
0072
Pw sply: Fan stop A cooling fan built in the power supply unit stopped, and overheat
occurred in the power module. PR
0073
Pw sply: Over regeneration Over-regeneration detection level became over 100%. The
regenerative resistor is overloaded. This alarm cannot be reset for 15 min from the occurrence to protect the regeneration resistor. Leave the drive system energized for more than 15 min, then turn the power ON to reset the alarm.
NR
0075
Pw sply: Overvoltage L+ and L- bus voltage in main circuit exceeded the allowable value.
As the voltage between L+ and L- is high immediately after this alarm, another alarm may occur if this alarm is reset in a short time. Wait more than 5 min before resetting so that the voltage drops.
NR
0076
Pw sply: Ext EMG stop set err The rotary switch setting of external emergency stop is not correct,
or a wrong external emergency stop signal is input. AR
0077
Pw sply: Power module overheat Thermal protection function in the power module has started its
operation. PR
(Note 1) If a power supply alarm (60 to 77) occurs, all servos will stop with the dynamic brakes, and all spindles will coast to a stop. (Note 2) "b", "C" and "d" displayed on the power supply unit's LED as a solid light (not flickering) do not indicate an alarm.
Appendix 6. Alarms 6.1 List of Alarms
IV - 48
(2) Class: S02 Message: Initial parameter error
An error was found in the parameters transmitted from the controller to the drive unit when the power was turned ON. Remove the cause of the alarm, and then reset the alarm by turning the controller power OFF once.
Alarm No. Details Remedy
2201 to
2264
The servo parameter setting data is illegal. The alarm No. is the No. of the servo parameter where the error occurred.
Check the descriptions for the appropriate servo parameters and correct them.
2301 The number of constants to be used in the following functions is too large: Electronic gears Position loop gain Speed feedback conversion
Check that all the related parameters are specified correctly.
sv001:PC1, sv002:PC2, sv003:PGN1 sv018:PIT, sv019:RNG1, sv020:RNG2
2302 When high-speed serial incremental detector (OSE104, OSE105) is connected, parameters for absolute position are set to ON. Set the parameters for absolute position detection to OFF. To detect an absolute position, replace the incremental specification detector with an absolute position detector.
Check that all the related parameters are specified correctly.
sv017:SPEC, sv025:MTYP
2303 No servo option is found. The closed loop (including the ball screw- end detector) or dual feedback control is an optional function.
Check that all the related parameters are specified correctly.
sv025:MTYP/pen sv017:SPEC/dfbx
2304 No servo option is found. The SHG control is an optional function.
Check that all the related parameters are specified correctly.
sv057:SHGC sv058:SHGCsp
2305 No servo option is found. The adaptive filtering is an optional function.
Check that all the related parameters are specified correctly.
sv027:SSF1/aflt 13001
to 13256
Parameter error The spindle parameter setting data is illegal. The alarm No. is the No. of the spindle parameter where the error occurred.
Check the descriptions for the appropriate spindle parameters and correct them. Refer to Alarm No.37 in Spindle Drive Maintenance Manual.
(3) Class: S51 Message: Parameter error This warning is displayed if a parameter outside the tolerance range is set. Illegal settings will be ignored. This alarm will be reset when a correct value is set.
Alarm No. Details Remedy
2201 to
2264
Servo parameter setting data is illegal. The alarm No. is the No. of the servo parameter where the warning occurred.
Check the descriptions for the appropriate servo parameters and correct them.
13001 to
13256
Spindle parameter setting data is illegal. The alarm No. is the No. of the spindle parameter where the warning occurred.
Check the descriptions for the appropriate spindle parameters and correct them. Refer to Spindle Drive Maintenance Manual.
Appendix 6. Alarms 6.1 List of Alarms
IV - 49
(4) Class: S52 Servo warning
When a warning occurs, a warning No. will appear on the NC monitor screen and with the LEDs on the front of the drive unit. Check the warning No., and remove the cause of the warning by following this list.
(a) Servo drive unit warning
No. Message Details Reset method Stop method
0096 Scale feedback error An excessive difference in feedback amount was detected between the motor side detector and the MPI scale in MPI scale absolute position detection system.
* -
0097 Scale offset error An error was detected in the offset data that is read at the NC power-ON in MPI scale absolute position detection system.
PR -
009E Absolute position detector: Revolution counter error
An error was detected in the revolution counter data of the absolute position detector. The accuracy of absolute position is not guaranteed.
* -
009F Battery voltage drop The battery voltage to be supplied to the absolute position detector is dropping.
* -
00A6 Fan stop warning A cooling fan in the drive unit stopped. * - 00E0 Overregeneration warning Over-regeneration detection level exceeded 80%. * - 00E1 Overload warning A level of 80% of the Overload 1 alarm state was
detected. * -
00E4 Set parameter warning An incorrect set value was detected among the parameters send from the NC in the normal operation.
* -
00E6 Control axis detachment warning A control axis is being detached. (State display) * - 00E7 In NC emergency stop state In NC emergency stop. (State display) * Deceleration stop
enabled 00E8
00EF
Power supply warning The power supply unit detected a warning. The error details are different according to the connected power supply unit. Refer to "Power supply warning".
* - *EA
Deceleration stop enabled
(Note1) Definitions of terms in the table are as follows. Motor side detector: Detector connected to CN2 Machine side detector: Detector connected to CN3
(Note 2) Resetting methods *: Automatically reset once the cause of the warning is removed. NR: Reset with the NC RESET button. This warning can also be reset with the PR and AR resetting conditions. PR: Reset by turning the NC power ON again. This warning can also be reset with the AR resetting conditions.
When the control axis is removed, this warning can be reset with the NC RESET button. (Excluding warning 93.) AR: Reset by turning the servo drive unit power ON again.
(Note 3) Servo and spindle motor do not stop when the warning occurs. (Note 4) When an emergency stop is input, servo and spindle motor decelerate to a stop.
(When SV048, SV055 or SV056 is set for servo and when SP055 or SP056 is set for spindle.)
(b) Spindle drive unit warning
No. Message Details Reset method Stop method
00A6 Fan stop warning A cooling fan in the drive unit stopped. * - 00E0 Overregeneration warning Over-regeneration detection level exceeded 80%. * - 00E1 Overload warning A level of 80% of the Overload 1 alarm state was
detected. * -
00E4 Set parameter warning A parameter was set to the value over the setting range. * - 00E6 Control axis detachment warning A control axis is being detached. (State display) * - 00E7 In NC emergency stop state In NC emergency stop. (State display) * Deceleration stop
enabled 00E8
00EF
Power supply warning The power supply unit detected a warning. The error details are different according to the connected power supply unit. Refer to "Power supply warning".
* -
(Note 1) Resetting methods *: Automatically reset once the cause of the warning is removed. NR: Reset with the NC RESET button. This warning can also be reset with the PR and AR resetting conditions. PR: Reset by turning the NC power ON again. This warning can also be reset with the AR resetting conditions.
When the control axis is removed, this warning can be reset with the NC RESET button. (Excluding warning 93.) AR: Reset by turning the servo drive unit power ON again.
(Note 2) Servo and spindle motor do not stop when the warning occurs. (Note 3) When an emergency stop is input, servo and spindle motor decelerate to a stop.
(When SV048, SV055 or SV056 is set for servo and when SP055 or SP056 is set for spindle.)
Appendix 6. Alarms 6.1 List of Alarms
IV - 50
(c) Power supply warning
No. LED display Message Details Reset
method 00E9
Instantaneous power interruption warning
The power was momentarily interrupted. NR
00EA
In external emergency stop state External emergency stop signal was input. *
00EB
Power supply: Over regeneration warning
Over-regeneration detection level exceeded 80%. *
00EE
Pw sply: Fan stop warning A cooling fan built in the power supply unit stopped. *
(Note 1) Resetting methods *: Automatically reset once the cause of the warning is removed. NR: Reset with the NC RESET button. This warning can also be reset with the PR and AR resetting conditions. PR: Reset by turning the NC power ON again. This warning can also be reset with the AR resetting conditions.
When the control axis is removed, this warning can be reset with the NC RESET button. (Excluding warning 93.) AR: Reset by turning the servo drive unit power ON again.
(Note 2) Servo and spindle motor do not stop when the warning occurs.
Appendix 6. Alarms 6.1 List of Alarms
IV - 51
6.1.4 MCP Alarm An error has occurred in the drive unit and other interfaces. (The bold characters are the messages displayed on the screen.)
Y Message
Alarm No. Error No. Message Class
Appendix 6. Alarms 6.1 List of Alarms
IV - 52
(1) Class: Y02 System alarm
An error occurred in the data transmitted between the MCP and drive unit after the power was turned ON.
Error No. Details Remedy 0050 System alm: Process time over The software or hardware may be damaged.
Contact the service center. Alarm No.
0000 SV commu er: CRC error 1 (10 times/910.2 ms)
0001 SV commu er: CRC error 2 (2 continuous times)
0002 SV commu er: Recv timing err (2 continuous times)
0051
xy03 SV commu er: Data ID error (2 continuous times) x: Channel No. (0 to) y: Drive unit rotary switch No.
(0 to) xy04 SV commu er: Recv frame No.
(2 continuous times) x: Channel No. (0 to) y: Number of reception frame -1
(0 to) x005 SV commu er: Commu error
(No error classification) x: Channel No. (0 to)
x006 SV commu er: Connect error x: Channel No. (0 to)
xy20 SV commu er: Init commu error The drive unit could not shift to the initial communication run time and stopped. x: Channel No. (0 to) y: Drive unit rotary switch No.
(0 to) xy30 SV commu er: Node detect error
No response from drive unit to the request from NC when setting network configuration. x: Channel No. (0 to) y: Station No. (0 to)
xy31 SV commu er: Commu not support
Drive unit's software version doesn't support the communication mode that the controller requires. x: Channel No. (0 to) y: Station No. (0 to)
A communication error has occurred between the controller and drive unit. Take measures against noise. Check that the communication cable connector
between the controller and drive unit and one between the drive units are tight.
Check whether the communication cable between the controller and drive unit and one between the drive units are disconnected.
A drive unit may be faulty. Take a note of the 7-segment LED contents of each drive unit and report to the Service Center.
Update the drive unit software version.
(Note) When two or more "Y02 System alarms" occur at the same time, only the alarm which occurs first is
displayed.
Appendix 6. Alarms 6.1 List of Alarms
IV - 53
(2) Class: Y03 Message: Drive unit unequipped
The drive unit is not correctly connected.
Error No. Details Remedy Alphabet
(axis name)
Servo axis drive unit not mounted
1 to 4 PLC axis drive unit not mounted
S No.1 spindle axis drive unit not mounted
T No.2 spindle axis drive unit not mounted M No.3 spindle axis drive unit not mounted N No.4 spindle axis drive unit not mounted
Check the drive unit mounting state. Check the end of the cable wiring. Check the cable for broken wires. Check the connector insertion. The drive unit input power is not being input. The drive unit axis No. switch is illegal.
(3) Class : Y05 Message: Initial parameter error
Details Remedy There is a problem in the value set for the number of axes or the number of part systems.
Check the value set for the corresponding parameters. #1001 SYS_ON #1002 axisno #1039 spinno, etc.
(4) Class: Y06 Message: mcp_no setting error
There are differences in the MCP and axis parameters when the NC power is turned ON.
Error No. Details Remedy 0001 There is a skipped number in the channels.
0002 The random layout setting is duplicated.
0003 The drive unit fixed setting "0000" and random layout setting "" are both set.
0004 The spindle/C axis "#1021 mcp_no" and "#3031 smcp_no" are not set to the same values.
0005 A random layout is set for the "#1154 pdoor" =1 two-part system.
0006 The channel No. parameter is not within the setting range.
Check the values set for the following parameters. #1021 mcp_no #3031 smcp_no
Appendix 6. Alarms 6.1 List of Alarms
IV - 54
(5) Class: Y07 Message: Too many axes connected
The number of connected axes exceeds the number allowed in the system.
(Alarm No.)
0 0
Exceeded number of axes at drive unit interface channel 1
Exceeded number of axes at drive unit interface channel 2
Alarm No. Details Remedy
0000 to
00FF
The number of axes connected to each channel exceeds the maximum number of connectable axes. The exceeded number of axes per channel is displayed as alarm No. This alarm occurs when the drive unit is connected only with the 2nd channel without connecting with the 1st channel.
Remove connected axes from the channel whose alarm No. is other than 0 for the number displayed as the alarm No. Keep the number of connected axes to or less than the maximum that can be connected.
(Note 1) The number of axes is limited per each drive unit interface channel.
(Note 2) Maximum number of axes that can be connected differs depending on whether or not an expansion unit is available or the setting of "#11012 16 axes for 1ch". The maximum number of connectable axes is as shown below.
Extension unit #11012 16 axes for 1ch Maximum number of axes to be connected
(Per 1 channel) Yes 0/1
0 8 axes
No 1 16 axes
(Note 3) If this alarm occurs, the alarm "Y03 Message: Drive unit unequipped" will not occur.
(Note 4) This alarm is displayed taking precedence over the alarm "Y08 Too many drive units connected" and "Y09 Too many axisno connected".
Appendix 6. Alarms 6.1 List of Alarms
IV - 55
(6) Class: Y08 Message: Too many drive units connected
The number of connected drive units exceeds the number allowed in the system.
(Alarm No.)
0 0
Exceeded number of drive units at drive unit interface channel 1
Exceeded number of drive units at drive unit interface channel 2
Alarm No. Details Remedy 0000
to 00FF
The number of drive units connected to each channel exceeds 8. The exceeded number of drive units per channel is displayed as alarm No.
Remove drive units from the channel whose alarm No. is other than 0 for the number displayed as the alarm No. Keep the number of connected drive units to 8 or less.
(Note 1) The drive unit is not counted when all the axes connected to it are invalid.
(Note 2) If this alarm occurs, the alarm "Y03 Message: Drive unit unequipped" will not occur.
(Note 3) The alarm "Y07 Too many axes connected" and "Y09 Too many axisno connected" are displayed taking precedence over this alarm.
Appendix 6. Alarms 6.1 List of Alarms
IV - 56
(7) Class: Y09 Message: Too many axisno connected
The connected axes No. (drive unit's rotary switch No.) is bigger than the No. allowed in the system.
(Alarm No.)
0 0
"1" when the axis No. at drive unit interface channel 1 is too big
"1" when the axis No. at drive unit interface channel 2 is too big
Alarm No. Details Remedy 0000
to 0011
The No. of the axis (drive unit's rotary switch No.) connected to each channel is bigger than the No. allowed.
For the channel whose alarm No. is 1, keep the axis No. (drive unit's rotary switch No.) not bigger than the No. allowed.
(Note 1) The axis No. is limited per each drive unit interface channel.
(Note 2) The biggest allowed connected axis No. differs depending on whether or not an expansion unit is available or the setting of "#11012 16 axes for 1ch". The biggest connectable axis No. is as shown below.
Extension unit #11012 16 axes for 1ch Highest allowed connected axis No.
(Per 1 channel) Yes 0/1
0 0 to 7
No 1 0 to F
(Note 3) If this alarm occurs, the alarm "Y03 Message: Drive unit unequipped" will not occur.
(Note 4) This alarm is displayed taking precedence over the alarm "Y08 Too many drive units connected".
(Note 5) The alarm "Y07 Too many axes connected" is displayed taking precedence over this alarm.
(8) Class: Y12 Message: No commu. with axis drv unit
Details Remedy Even though the high-speed synchronous tapping option is valid, drive unit that doesn't support the option is connected.
Replace it with a drive unit that supports the option.
(9) Class: Y13 Message: No commu. with sp drv unit
Details Remedy Even though the high-speed synchronous tapping option is valid, drive unit that doesn't support the option is connected.
Replace it with a drive unit that supports the option.
(10) Class: Y14 Message: Comm btwn drives not ready
Details Remedy Communication of drive units failed to be ready within a specified time.
Connection of drive units may be wrong. Check if any of drive units is broken.
Appendix 6. Alarms 6.1 List of Alarms
IV - 57
(11) Class: Y20 Safety observation alarm
When this alarm is output, emergency stop mode is applied. Refer to "remedy" of each alarm as to how to cancel the alarm.
Error No. Alarm No. Details Remedy 0001 Axis name Parameter compare error
The speed monitoring parameter in the NC and the parameter transmitted to the drive unit are not matched. The name of the axis with an error is displayed.
The NC or the servo drive unit may be damaged. Contact the service center.
0002 Axis name Sfty obsrvation: Cmd spd err The speed exceeding the speed set with the parameter was commanded during the speed monitoring mode. The name of the axis with an error is displayed.
Check the speed monitoring parameter and the user PLC. Restart the NC.
0003 Axis name Sfty obsrvation: FB pos err The commanded position transmitted to the servo drive unit from NC and the feedback position to be received from the servo drive unit are totally different during the speed monitoring mode. The name of the axis with an error is displayed.
The NC or the servo drive unit may be damaged. Contact the service center.
0004 Axis name Sfty obsrvation: FB speed err Actual rotation speed of the motor is exceeding the speed set with speed monitoring parameter during the speed monitoring mode. The name of the axis with an error is displayed.
Check the speed observation parameter and the user PLC. Restart the NC.
0005 Door No. Door signal: Input mismatch Door state signals on the NC side and the drive side do not match. It may be caused by the followings: Cable disconnection Damaged door switch Damaged NC or servo drive unit
Check the cable. Check the door switch. Restart the NC.
0006 Door No. No spd obsv mode in door open The door open state was detected when the speed monitoring mode was invalid. The causes may be same as the ones for 0005 (Door signal: Input mismatch). Also the user PLC may not be correct.
Check the user PLC. Restart the NC.
Appendix 6. Alarms 6.1 List of Alarms
IV - 58
Error No. Alarm No. Details Remedy
0007 Axis name Speed obsv: Para incompatible Two speed monitoring parameters are not matched at the rising edge of the speed monitoring mode signal. The name of the axis with an error is displayed.
Change the relevant parameters so that the two speed monitoring parameters match. Restart the NC.
0008 Contactor No.
Contactor welding detected Contactor welding was detected.
Make sure that contactor's auxiliary b contact signal is output correctly to the device set on "#1380 MC_dp1" and "#1381 MC_dp2". If welding, replace the contactor. Restart the NC.
0009 - No spec: Safety observation The servo parameter and the spindle parameter of the speed monitor are set for a system with no safety observation option.
Turn OFF the servo parameter SV113/bitF, the spindle parameter SP229/bitF and the spindle type servo parameter SV113/bitF. Then, restart the NC.
0010 - SDIO connector input volt err 24VDC power is not supplied to SDIO connector correctly. (SDIO 4A pin supply voltage was dropped to 16V or less, or 1ms or more instant power interrupt was detected.) In this case, "Pw sply:Inst pw interpt(DC24V)" alarm occurs because the contactor control output signal cannot be controlled. This state remains until restarting the NC even if the cause of the alarm has been removed.
Check the wiring. Supply 24VDC power to the SDIO connector. Restart the NC.
(12) Class: y21 Safety observation warning The warning will be cancelled when the cause of the warning is removed.
Error No. Alarm No. Details Remedy 0001 Axis name Speed obsv signal: Speed over
The speed exceeds the safety speed limit when the speed monitoring mode signal is ON. The name of the axis with an error is displayed.
When decelerated, the warning will be removed, and the speed monitor will be started.
Appendix 6. Alarms 6.1 List of Alarms
IV - 59
(13) Class: Y51 Parameter error
An error occurred in a parameter that causes an alarm while the control axis was operating.
Error No. Details Remedy 0001 Parameter G0tL illegal
The time constant has not been set or the setting exceeded the setting range.
Check #2004 G0tL.
0002 Parameter G1tL illegal The time constant has not been set or the setting exceeded the setting range.
Check #2007 G1tL.
0003 Parameter G0t1 illegal The time constant has not been set or the setting exceeded the setting range.
Check #2005 G0t1.
0004 Parameter G1t1 illegal The time constant has not been set or the setting exceeded the setting range.
Check #2008 G1t1.
0009 Parameter grid space illegal Check #2029 grspc.
0012 Parameter stapt1-4 illegal The time constant has not been set or the setting exceeded the setting range.
Check spindle parameters #3017 stapt1 to #3020 stapt4.
0015 Parameter skip_tL illegal The time constant has not been set or the setting exceeded the setting range.
Check #2102 skip_tL.
0016 Parameter skip_t1 illegal The time constant has not been set or the setting exceeded the setting range.
Check #2103 skip_t1.
0017 Parameter G0bdcc illegal #1205 G0bdcc for the 2nd part system is set to acceleration/deceleration before G0 interpolation.
Check #1205 G0bdcc.
0018 OMR-II parameter error The OMR-II related parameter settings are incorrect. In this case, the OMR-II is disabled.
Check the related parameter settings.
0019 PLC indexing stroke length err When the linear axis equal indexing is validated for the PLC indexing axis, "#12804 aux_tleng" has not been set. Otherwise, it is out of the setting range.
Check "#12804 aux_tleng".
0020 No hi-accu acc/dec t-const ext Option to extend the high-accuracy acceleration/deceleration time constant is unavailable.
Set "#1207 G1btL" to the value with which high-accuracy time constant extension specification is unavailable.
0101 Values of PC1/PC2 too large The PC1 and PC2 settings used for the rotary axis are too large.
Check "#2201 PC1" and "#2202 PC2".
Appendix 6. Alarms 6.1 List of Alarms
IV - 60
(14) Class: Y90 Message: No spindle signal
Alarm No. Z open phase
B open phase
A open phase
1 2 3 4 5 6 7
0 0
(Alarm No.)
No.2 spindle
No.1 spindle
No.3 spindle No.4 spindle
Alarm No. Details Remedy
0001 to
0007
There is an error in the spindle encoder signal. The data transmission to the drive unit is stopped when this error occurs.
Check the spindle encoder's feedback cable and the encoder.
Appendix 6. Alarms 6.1 List of Alarms
IV - 61
6.1.5 System Alarms
(The bold characters are the messages displayed on the screen.)
Z31 DataServer error
Warning No. Message
Warning No. Explanation 0001 Socket open error(socket) 0002 Socket bind error(bind) 0003 Connection wait queue error(listen) 0004 Connection request error(accept) 0005 Data recv error(socket error) 0006 Data recv error(data error) 0007 Data send error(socket error) 0008 Data send error(data error) 000A Socket close error(close)
(Note) If warning No. 0001, 0002, 0003, or 000A is displayed, set the parameters, then turn power OFF and
turn it ON again.
Appendix 6. Alarms 6.1 List of Alarms
IV - 62
(The bold characters are the messages displayed on the screen.)
Message Details Remedy Z40
Format mismatch
This appears when the parameter MemVal is formatted at 0, and MemVal is set to 1.
Either return the MemVal setting, or format and restart.
Z51 E2PROM error 00xx
Z51 E2PROM error 0011: Read error Z51 E2PROM error 0012: Write error
If the same alarm is output by the same operation, the cause is an H/W fault. Contact the Service Center.
Z52 Battery fault 000x
The voltage of the battery inserted in the NC control unit has dropped. (The battery used to save the internal data.)
0001: Battery warning 0002: Battery detecting circuit error 0003: Battery alarm
(Note 1)
Replace the battery of the NC control unit. Check for disconnection of the battery
cable. After treating the battery check the
machining program.
Z53 CNC overheat
The controller or operation board temperature has risen above the designated value. (Note 2)
Cooling measures are required. Turn OFF the controller power or lower
the temperature with a cooler etc. Z55
RIO communication stop
This occurs when an error occurs in the communication between the controller and remote l/O unit. Cable breakage Remote l/O unit fault Power supply to remote l/O unit fault (Note 3)
Check and replace the cables. Replace the remote I/O unit. Check the power supply. (existence of
supply voltage)
Z57 System warning
The program memory capacity setting value cannot be formatted. The expansion cassette (HR437) is not mounted after formatting. An expansion cassette different from the expansion cassette (HR437) mounted during formatting is mounted.
Check the state of the following items. Program memory capacity Status of expansion cassette (HR437)
mounting APLC open option
Z58 ROM write not completed
The machine tool builder macro program was not written to the FROM after being registered, edited, copied, condensed, merged, the number changed, or deleted.
Write the machine tool builder macro program to the FROM.
If the operations, such as editing, done while the NC power was OFF can be invalidated, the program does not need to be written to the FROM.
Z59 Acc/dec time cnst too large
Acceleration and deceleration time constants are too large. (This alarm is output at the same time as "T02 Acc/dec time cnst too large 0206.")
Increase the value specified as the "#1206 G1bF" parameter.
Decrease the value specified as the "#1207 G1btL" parameter.
Lower the feedrate. Z60
Fieldbus communi- cation error
Communication error has occurred on the Fieldbus communication using HN571/HN573/HN575.
Refer to (Note 4) for details.
Z64 Valid term soon to be expired xx
The valid term will be expired in less than a week. Remaining valid term is xx more days.
Obtain a decryption code by making a payment. Enter the decryption code.
Z65 Valid term has been expired
No decryption code was input before the valid term was expired.
Obtain a decryption code by making a payment. Enter the decryption code.
Appendix 6. Alarms 6.1 List of Alarms
IV - 63
Message Details Remedy
Z67 CC-Link communication error
A communication error occurred during CC-Link communication using CC-Link unit.
Refer to "List of Messages" in CC-Link (Master/Slave) Specification manual (BNP-C3039-214).
Z68 CC-Link unconnected
The cable connected between CC-Link unit and each device is disconnected or broken.
Connect the cable. Check whether or not the cable is broken.
! CAUTION
If the battery low warning is issued, save the machining programs, tool data and parameters in an input/output device, and then replace the battery. When the battery alarm is issued, the machining programs, tool data and parameters may be destroyed. Reload the data after replacing the battery.
Do not replace the battery while the power is ON.
Do not short circuit, charge, heat, incinerate or disassemble the battery.
Dispose of the spent battery following local laws.
(Note 1) The display of Z52 battery fault 0001 can be removed by resetting. However, the warning state will not be cancelled until the battery is replaced.
(Note 2) Temperature warning If the alarm is displayed when an overheat alarm is detected the overheat signal will be output simultaneously. If the machine is in automatic operation the operation will be continued but restarting will not be possible after resetting or stopping with M02/M30. (Starting will be possible after block stop or feed hold.) The alarm will be reset and the overheat signal will turn OFF when the temperature drops below the specified temperature.
Z53 CNC overheat 000x 0001 : The temperature in the controller is high. 0002 : The temperature around the communication terminal (setting and display unit) is high. 0003 : The temperature in the controller and around the communication terminal (setting and display unit) is high.
The ambient temperature must be lowered immediately when a "Z53 CNC overheat" alarm occurs but if machining must be continued the alarm can be invalidated by turning the following parameter OFF.
7 6 5 4 3 2 1 0 PLC parameter bit selection #6449
Communication terminal (setting and display unit) 0: Detection invalid Controller 1: Detection valid
Appendix 6. Alarms 6.1 List of Alarms
IV - 64
(Note 3) RIO communication interrupt
If communication between the control unit and remote I/O unit fails, the alarm and remote I/O unit number are displayed.
Z55 RIO communication stop
(a) and (b) above indicate the following matters.
Alarm number
RIO (seventh station)
RIO (sixth station)
RIO (fifth station)
RIO (fourth station)
Alarm number
RIO (third station)
RIO (second station)
RIO (first station)
RIO (0th station)
0 0
1 1
2 2
3 3
4 4
5 5
6 6
7 7
8 8
9 9
A A
B B
C C
D D
E E
F F
(a)(b)
Board connection remote I/O communication interrupted station Remote I/O 3rd part system communication interrupted station Remote I/O 1st part system communication interrupted station Remote I/O 2nd part system communication interrupted station
This also applies for the remote I/O 1st part system communication interrupted station, remote I/O 3rd part system communication interrupted station and board connection remote I/O communication interrupted station.
Appendix 6. Alarms 6.1 List of Alarms
IV - 65
(Note 4)
Z60 Fieldbus communication error n1 n2 n3 n4 Classification No.
Message
Class. No.
Details
Shows state of the master channel (shown in hexadecimal number) 00: Offline In initializing 40: Stop Cutting I/O communication 80: Clear Resetting output data of each slave by sending 0 data.
n1
C0: In operation In I/O communication n2 Shows error state (shown in hexadecimal number)
7 6 5 4 3 2 1 0Bit
BIT Details 0 Control error: Parameter error 1 Auto clear error: Communication with all the slave channels was cut because
a communication with one slave channel had an error. 2 Non exchange error: Slave channel with communication error is found 3 Fatal error: The communication cannot be continued because sever network
failure exists. 4 Event error: Short-circuit was found on the network. 5 Not ready: CNC communication is not ready. 6 Time out error: Time out was detected in communication with each channel. 7 Not used
n3 Shows error No. (shown in hexadecimal number)
Refer to "(a) Error in master channel" and "(b) Error in slave channel" for details. n4 Shows slave No. where communication error has occurred. (shown in hexadecimal
number) "FF" means an error in master channel.
Appendix 6. Alarms 6.1 List of Alarms
IV - 66
(a) Error in master channel (when remote address with an error is FF (hexadecimal number))
Value in n3
Details Remedy
0 No error Operating normally 32 No USR_INTF-task Damage in HN571. Replace HN571. 33 No global data field 34 No FDL-task 35 No PLC-task 37 Master parameter incorrect 39 Slave parameter incorrect 3C Data offset exceeding allowable set
value received Check the configuration setting.
3D Slave data send range overlap 3E Slave data receive range overlap 3F Not set data hand shake Damage in HN571. Replace HN571. 40 RAM range exceeded 41 Slave parameter data set illegal CA No segment D4 Data base read illegal Download the configuration data again. D5 Operating system illegal Damage in HN571. Replace HN571. DC Watch dog error DD Hand shake mode
No data communication by 0
DE Master auto clear mode When setting auto clear mode, the auto clear mode was performed because one slave was not able to connect in run time.
(b) Error in slave channel (when remote address with an error is other than FF (hexadecimal number))
Value in n4
Details Remedy
2 Station overflow reported 3 Station stopped responding to
master command 9 No slave required responding data 11 No station respond 12 No master to logical token ring 15 Illegal parameter requested
Check the configuration of slave channel in which error has occurred. Check if there is any short-circuit in wire to bus.
Appendix 6. Alarms 6.1 List of Alarms
IV - 67
6.1.6 Absolute Position Detection System Alarms
(The bold characters are the messages displayed on the screen.) Z Message
Axis name Error No. Message Class
(1) Class: Z70 Abs data error
This error is displayed if the absolute position data is lost in the absolute position detection system.
Error No. Details Remedy Zero point
initialization Alarm reset when power
is turned OFF
Servo alarm No.
0001 Abs posn base set incomplete
Zero point initialization is incomplete. Otherwise, the spindle was removed.
Complete zero point initialization.
Required - -
0002 Absolute position lost The absolute position reference point data saved in the NC has been destroyed.
Input the parameters. If the reference point data cannot be restored perform zero point initialization.
(Required) - -
0003 Abs posn param changed The parameters used to detect the absolute position have been changed. #1003 iunit #2201 PC1 #1016 iout #2202 PC2 #1017 rot #2218 PIT #1018 ccw #2219 RNG1 #1040 M_inch #2220 RNG2 #2049 type #2225 MTYP
Correctly set the parameters. Turn the power on again and perform zero point initialization.
Required - -
0004 Abs posn initial set illegal The zero point initialization point is not at the grid position.
Reperform zero point initialization.
Required - -
0005 Abs posn param restored Restoration was possible with parameter input in the above No.0002 state.
Turn the power on again and operation will be possible.
Not required - -
0080 Abs posn data lost The absolute value data was lost, because the multi-rotation counter data in the detector was incorrect, etc.
Replace the detector and complete zero point initialization.
Required - (9E) etc.
Appendix 6. Alarms 6.1 List of Alarms
IV - 68
Error No. Details Remedy Zero point
initialization Alarm reset when power
is turned OFF
Servo alarm No.
0101 Abs posn error(servo alm 25) The power was turned ON again after the servo alarm No. 25 displayed.
Reperform zero point initialization.
Required - (25)
0106 Abs posn error(servo alm E3)
The power was turned ON again after the servo alarm No. E3 displayed.
Reperform zero point initialization.
Required - (E3)
(Note) To release alarm "Z70 Abs data error", enter the parameter data output when establishing the
absolute position and turn ON the power again. For the rotary axis, however, the alarm cannot be released by entering the parameter data.
(2) Class: Z71 Abs encoder failure
This alarm is displayed if an error is found in the detector for the absolute position detection system.
Error No. Details Remedy Zero point
initialization Alarm reset when power
is turned OFF
Servo alarm No.
0001 AbsEncoder:Backup voltage drop
The backup voltage in the absolute position detector dropped.
Replace the battery check the cable connections and check the detector. Turn the power ON again and perform zero point initialization.
Required - (Z70-0101
displays after power is
turned ON again.)
25
0003 AbsEncoder: Commu error Communication with the absolute position detector was not possible.
Check and replace the cables card or detector. Turn the power ON again and perform zero point initialization.
(Required) Only when detector is replaced.
Reset 91
0004 AbsEncoder: Abs data changed
The absolute position data fluctuated when establishing the absolute position.
Check and replace the cables card or detector. Turn the power ON again and perform zero point initialization.
(Required) Only when detector is replaced.
Reset 93
0005 AbsEncoder: Serial data error
An error was found in the serial data from the absolute position detector.
Check and replace the cables card or detector. Turn the power ON again and perform zero point initialization.
(Required) Only when detector is replaced.
Reset 92
0006 AbsEncoder: Abs/inc posn diffr
Servo alarm E3 Absolute position counter warning
Operation is possible until the power is turned off.
(Required) When power is turned ON
again.
Reset (Z70-0106
displays after power is
turned ON again.)
E3
0007 AbsEncoder: Initial commu err
Initial communication with the absolute position detector was not possible.
Check and replace the cables card or detector. Turn the power ON again and perform zero point initialization.
(Required) Only when detector is replaced.
Reset 18
Appendix 6. Alarms 6.1 List of Alarms
IV - 69
(3) Class: Z72 Message: Position check error
This alarm is displayed if an error is detected when comparing the detector's absolute position and controller coordinate values in the absolute position system.
(4) Class: Z73 Message: Absolute position data warning
This warning is displayed for the absolute position detection system.
Alarm No. Details Remedy
0001 Battery for abs data fault Servo alarm 9F Low battery voltage
If the battery voltage is low or the cable is damaged, there is no need to initialize the absolute position.
(Note) When this alarm occurs, do not turn OFF the drive unit power to protect the absolute position data.
Replace the battery while the drive unit power is ON.
Appendix 6. Alarms 6.1 List of Alarms
IV - 70
6.1.7 Distance-coded Reference Scale Errors
(The bold characters are the messages displayed on the screen.)
Z Message
Axis name
Error No.
Message
Alarm class
(1) Class: Z80 Distance-coded ref scale err
Error No. Details Remedy
0001 Basic position lost The basic point data memorized by the NC is broken.
Input the parameter. If the basic point data cannot be recovered, perform the initial reference position setting.
0002 Basic position restore The basic point data is recovered by parameter input.
Operation can be started after turning the power ON.
0003 No spec: Distance-coded scale Even if the distance-coded reference scale is not included in the specification, it is set to be available.
Check the specification. If you do not use this function, set the detector
type in servo parameters correctly.
(2) Class: Z81 Synchronous control
Error No. Details Remedy
0001 R-pos adjustment data lost Reference position adjustment value data in the NC is damaged.
Input the parameter. If the data cannot be recovered by the parameter, establish the reference position again.
0002 R-pos adjustment data restored After the error 0001, by inputting the parameter, the data was recovered.
After the reference position establishment, you can continue the operation.
Appendix 6. Alarms 6.1 List of Alarms
IV - 71
6.1.8 Messages during Emergency Stop (The bold characters are the messages displayed on the screen.)
EMG Emergency stop Error items
Error Item Details Remedy
PLC The user PLC has entered the emergency stop state during the sequence process.
Investigate and remove the cause of the user PLC emergency stop.
EXIN The emergency stop input signal for machine operation board or handy terminal is significant (open).
Cancel the emergency stop input signal. Check the wiring to see if any wiring is broken.
SRV An alarm occurred in the servo system causing an emergency stop.
Investigate and remove the cause of the servo alarm.
STOP The user PLC (ladder sequence) is not running. Check if the rotary switch CS2 on the top of the controller front panel is set to 1.
Check if the PLC edit file save screen (onboard function) [4RUN/SP] (run/stop) switch is turned ON.
SPIN Spindle drive unit not mounted The spindle drive unit is not mounted.
Cancel the causes of the other emergency stop.
Check emergency stop signal input in the spindle drive unit.
PC_H High-speed PC processing abnormal Check the sequence program. (To stop monitoring the high-speed PC processing temporarily, set 1 in "#1219 aux03/bit1". Disable the monitoring function only as a temporary measure.)
PARA Setting of the door open II fixed device is illegal. The dog signal random assignment parameter setting is illegal.
Specify the "#1155 DOOR_m" and "#1156 DOOR_s" parameters correctly. (When the door open II fixed device is not used, set "#1155 DOOR_m" and "#1156 DOOR_s" to "100".)
Correctly set the "#2073 zrn_dog", "#2074 H/W_OT+", "#2075 H/W_OT-" and "#1226 aux10/bit5" parameters.
Appendix 6. Alarms 6.1 List of Alarms
IV - 72
Error No. Details Remedy
LINK If the FROM/TO instruction is not executed within 500 ms, an emergency stop occurs.
Try to execute the FROM or TO instruction one or more times every 500 ms.
* Measure the time in which no interrupt request is issued from MELSEC and store the result in the R register. R10190: Current time-out counter R10191: Counter for maximum time-out after
power-on R10192: Counter for maximum time-out after
system start-up (backed up) MELSEC is held in error and reset states. Check the MELSEC states.
The contents of MELSEC-specific code area in buffer memory have been destroyed.
Check the MELSEC states.
PLC serial link communication has stopped.
(Note) When "WAIT" is entered for the PLC serial link, only the preparation sequence has been established before the communication stops. Therefore, it is supposed that the basic specification parameters related to serial link parameters #1902 and #1903 are incorrect or the #1909 set-time is too short.
Check that HR571 card wiring and external sequencer transmission are normal.
Check the diagnostic screen for link communication errors.
Check whether the basic specification parameters related to serial link parameters are specified correctly.
WAIT The preparation sequence is not sent from the master station. Otherwise, the contents of the received preparation sequence are inconsistent with those of the parameters, so that the usual sequence cannot be started.
(Note) When "LINK" is also entered for the PLC serial link, refer to "Note" in the section, "LINK".
Check that the HR571 card rotary switch and wiring and the external sequencer transmission are normal.
Check the diagnostic screen for link communication errors.
XTEN The HR571 card operates abnormally or the rotary switch is set incorrectly.
Check the HR571 card rotary switch and replace the HR571 card if required.
LAD The user PLC (ladder sequence) has an illegal code.
Check the user PLC (ladder sequence) to see if it uses illegal device numbers or constants.
CVIN The external emergency stop function for power supply is valid. So, the emergency stop input signal for power supply is significant (open).
Cancel the emergency stop input signal. Check the wiring to see if any wiring is broken.
MCT An emergency stop occurs because the contactor shutoff test is executing.
Automatically cancel the emergency stop after the contactor shutoff is confirmed.
When the contactor shutoff cannot be confirmed within 5 seconds after contactor shutoff test signal (Y742) is input, "Y20 Contactor welding detected" alarm will occur, and the emergency stop status remains.
Turn the power ON again after confirming "contactor's auxiliary b contact" signal is correctly output to the device that is set with "#1330 MC_dp1" and "#1331 MC_dp2".
Appendix 6. Alarms 6.1 List of Alarms
IV - 73
6.1.9 Auxiliary Axis Alarms Refer to "1.3 Servo/spindle alarms" for details of the alarm class and alarm clear class combination. (The bold characters are the messages displayed on the screen.)
S Message Axis No. 1 to 4 Alarm information (Follows MR-J2-CT alarm information) Message Alarm class
(1) Class: S01 Aux ax servo alarm
Alarm information Details Remedy
0011 Aux ax PCB err (Drive circuit) An error occurred in the drive unit's internal PCB.
Replace servo drive unit.
0013 Aux ax S/W processing error An error occurred in the drive unit's internal reference clock.
Replace servo drive unit.
Aux ax motor/detector type err 0016 Motor type error. Use a correct drive unit and motor
combination. Detector initial communication error. Connect correctly.
Replace the motor. Replace or repair cable.
Detector CPU error. Replace the motor (detector). 0017 Aux ax PCB error(A/D err)
An error occurred in the drive unit's internal A/D converter. Replace servo drive unit.
0025 Aux ax absolute posn lost An error occurred in the detector's internal absolute position data.
Turn the power ON for 2 to 3 minutes while the alarm is occurring, and then turn the power ON again.
Replace the battery, and initialize the absolute position again.
0034 Aux ax CRC error An error occurred in the communication with the NC.
Take countermeasures against noise.
0036 Aux ax communication timeout Communication with the NC was cut off.
Connect correctly. Turn the NC power ON. Replace the drive unit or NC.
0037 Aux ax parameter error The parameter setting value is incorrect.
Set the parameter correctly.
0038 Aux ax frame error An error occurred in the communication with the NC.
Take countermeasures against noise.
0039 Aux ax commu INFO error Undefined data was transferred from the NC.
Change the NC software version to a compatible version.
Appendix 6. Alarms 6.1 List of Alarms
IV - 74
(2) Class: S02 Aux ax servo alarm
Alarm information Details Remedy
0011 Aux ax PCB err (Drive circuit) An error occurred in the drive unit's internal PCB.
Replace servo drive unit.
0013 Aux ax S/W processing error An error occurred in the drive unit's internal reference clock.
Replace servo drive unit.
0015 Aux ax EEROM error A write error occurred to the EEROM in the drive unit.
Replace servo drive unit.
0017 Aux ax PCB error(A/D err) An error occurred in the drive unit's internal A/D converter.
Replace servo drive unit.
0018 Aux ax PCB error(LSI err) An error occurred in the drive unit's internal LSI.
Replace servo drive unit.
0020 Aux ax detector error An error occurred in the communication between the servo drive unit and detector.
Connect correctly. Replace or repair cable.
0024 Aux ax ground fault detection A ground fault of the output was detected when the power was turned ON.
Repair the ground fault section. Replace the cable or motor.
(3) Class: S03 Aux ax servo alarm
Alarm information Details Remedy
0010 Aux ax under voltage The power voltage is 160V or less.
Review the power supply. Replace the servo drive unit.
0030 Aux ax regeneration error
The tolerable regeneration power of the internal regenerative resistor or external regenerative option was exceeded.
Set the parameter #50002 correctly. Connect correctly. Lower the positioning frequency. Change the regenerative option to
a larger capacity. Lower the load. Review the power supply.
Regenerative transistor error Replace the servo drive unit.
0031 Aux ax overspeed The motor's rotation speed exceeded the tolerable momentary speed.
Increase the acceleration/ deceleration time constant.
Review the gear ratio. Replace the detector.
0032 Aux ax overcurrent A current exceeding the servo drive unit's tolerable current flowed.
Repair the wiring. Replace the servo drive unit. Take countermeasures against
noise.
Appendix 6. Alarms 6.1 List of Alarms
IV - 75
Alarm
information Details Remedy
0033 Aux ax overvoltage The voltage of the converter in the servo drive unit was 400V or more.
Wire correctly. Replace the servo drive unit. For the internal regenerative
resistor, replace the drive unit. For the external regenerative option,
replace the regenerative option. 0046 Aux ax motor overheating
An operation state causing the motor to overheat continued.
Reduce the motor load. Review the operation pattern.
0050 Aux ax overload 1 The servo drive unit or servomotor overload protection function activated.
Reduce the motor load. Review the operation pattern. Change to a motor or drive unit
with large output. Change the setting of the
automatic tuning response characteristics.
Correct the connection. Replace the servomotor.
0051 Aux ax overload 2 The max. output current flowed for several seconds due to a machine collision or overload.
Review the operation pattern. Change the setting of the
automatic tuning response characteristics.
Correct the connection. Replace the servomotor.
0052 Aux ax excessive error A position deflection exceeding the excessive error detection setting value occurred.
Increase the acceleration/ deceleration time constant.
Increase the torque limit value. Review the power facility capacity. Review the operation pattern. Replace the servomotor. Connect correctly. Repair or replace the cable.
Appendix 6. Alarms 6.1 List of Alarms
IV - 76
(4) Class: S52 Message: Aux ax servo warning
Alarm information Details Remedy
0092 Aux ax battery voltage drop The absolute position detection battery voltage dropped.
Mount a battery. Replace the battery and initialize
the absolute position.
00E0 Aux ax overregeneration warning The regeneration power may have exceeded the tolerable range of the built-in regenerative resistor or external regenerative option.
Lower the positioning frequency. Change the regenerative option to
a larger one. Lower the load.
00E1 Aux ax overload warning The overload alarm 1 could occur.
Refer to the items for S03 0050.
00E3 Aux ax abs position counter warning There is an error in the absolute position detector internal data.
Take countermeasures against noise.
Replace the servomotor.
00E9 Aux ax main circuit OFF warning The servo ON signal was input while the main circuit power was OFF. The contactor operation is faulty.
Turn ON the main circuit power.
(5) Class: Z70 Message: Aux ax abs position error
Alarm information Details Remedy
0001 Aux ax abs posn base set incomplete The zero point (reference point) has not been initialized in the absolute position system.
Initialize the zero point (reference point).
0002 Aux ax absolute position lost The absolute position coordinate data in the drive unit has been lost.
Initialize the zero point (reference point).
0003 Aux ax abs posn param changed The absolute position system related parameters have been changed or lost.
Correctly set the parameters and then initialize the zero point (reference point).
(6) Class: Z71 Message: Aux ax drop voltage
Alarm information Details Remedy
0001 Aux ax abs encoder: back up voltage drop The data in the detector has been lost. Battery voltage drop. Detector cable wire breakage or looseness.
Check the battery and detector cable and then initialize the zero point (reference point).
Appendix 6. Alarms 6.1 List of Alarms
IV - 77
(7) Class: Z73 Message: Aux ax system warning
Alarm information Details Remedy
0001 Aux ax battery for abs data fault Battery voltage drop. Detector cable wire breakage or looseness.
Check the battery and detector cable. The zero point does not need to be initialized.
0003 Aux ax absolute position counter warning An error occurred in the detector's absolute position counter.
Replace the detector.
(8) Class: M00 Aux ax operation error
Alarm information Details Remedy
0001 Aux ax dog overrun When executing dog-type reference position, the zero point return speed is too fast or the dog length is too short.
Lower the zero point return speed or increase the dog length.
0003 Aux ax R-pnt direction illegal When executing reference position return, the axis was moved in the opposite of the designated direction.
Move the axis in the correct direction.
0004 Aux ax external interlock The axis interlock function is valid.
Cancel the interlock signal
0005 Aux ax internal interlock An interlock was established by the servo OFF function.
Cancel the servo OFF.
0007 Aux ax soft limit The soft limit was reached.
Check the soft limit setting and machine position
0024 Aux ax R ret invld at abs alm Reference position return was executed during an absolute position alarm.
Initialize the absolute position reference point and then fix the absolute position coordinates.
0025 Aux ax R ret invld at ini Reference position return was executed while initializing the absolute position.
Initialize the absolute position reference point and then fix the absolute position coordinates.
Appendix 6. Alarms 6.1 List of Alarms
IV - 78
(9) Class: M01 Aux ax operation error
Alarm information Details Remedy
0101 Aux ax no operation mode The operation mode is not designated, or the operation mode was changed during axis movement.
Correctly designate the operation mode.
0103 Aux ax feedrate 0 The operation parameter's feedrate setting is zero. The operation parameter feedrate setting is zero. Or, the override is valid, and the override value is zero.
Set a value other than zero in the feedrate setting or override value.
0160 Aux ax sta No. illegal A station No. exceeding the No. of indexed divisions was designated.
Correctly designate the station No.
0161 Aux ax R-pnt ret incomplete Automatic/manual operation was started before reference position return was executed with the incremental system.
Execute the reference position return.
0162 Aux abs position initializing The start signal was input while initializing the absolute position reference point.
Complete the absolute position reference point initialization.
0163 Aux ax abs position error The start signal was input during an absolute position alarm.
Initialize the absolute position reference point and then fix the absolute position coordinates.
0164 Aux ax arbitrary positioning The manual operation mode was started during the random positioning mode.
Turn the random positioning mode OFF before switching to the manual operation mode.
0165 Aux uneven index sta No. ilgl The commanded station No. was higher than 9 or the number of indexing stations during uneven indexing.
Check the commanded station No. and the parameter "#50100 station" setting.
Appendix 6. Alarms 6.1 List of Alarms
IV - 79
(10) Class: Y02 Auxiliary axis MCP alarms An error occurred during data transfer between the MCP and auxiliary axis drive unit after turning on the power.
Error No. Details Remedy 0050 Aux ax sys alm: Proc time over The software or hardware may be damaged.
Contact the service center. 0000 Aux ax commu er:CRC error 1
(10 times/910.2ms) 0001 Aux ax commu er:CRC error 2
(2 continuous times) 0002 Aux ax commu er:Recv timing
(2 continuous times) xx03 Aux ax commu er:Data ID
(2 continuous times) xx: Axis No.
0051
xx04 Aux ax commu er:Recv frame no. (2 continuous times) xx: Axis No.
A communication error has occurred between the controller and drive unit. Take measures against noise. Check that the communication cable connector
between the controller and drive unit and one between the drive unit are tight.
Check whether the communication cable between the controller and drive unit and one between the drive units are disconnected.
A driving drive unit may be faulty. Take a note of the 7-segment LED contents of each driving drive unit and report to the Service Center.
(11) Class: Y03 Message: Aux ax drive unit unequipped The drive unit is not properly connected.
Error No. Details Remedy Axis No.
1 to 4 bit correspondence (bit 0: 1st axis, bit 1: 2nd axis, bit 2: 3rd axis, bit 3: 4th axis)
Check the auxiliary axis drive unit mounting state. Check the end of the cable wiring. Check the cable for broken wires. Check the connector insertion. The auxiliary axis drive unit input power is not being input. The auxiliary axis drive unit axis No. switch is illegal.
Appendix 6. Alarms 6.1 List of Alarms
IV - 80
6.1.10 Computer Link Errors
(The bold characters are the messages displayed on the screen.)
L Message
Error No.
Message
Alarm class
(1) Class: L01 Computer link error
Error No. Details Remedy
-2 Serial port being used Serial port has already being opened or cannot be used.
Check whether the same port being used by Anshin-net, etc.
Recheck the parameters for tape operation port. -4 Timeout error
Communication ends with timeout CNC has a 248-byte receive buffer. The time during which CNC receives 248 bytes exceeds the "TIME-OUT" value set in the I/O device parameter.
Set a greater timeout value in the input/output device parameter.
Recheck the HOST software as to whether or not the HOST transmits data in response to DC1 from CNC (data request).
Check whether or not start code of computer link parameter is set to 0.
-10 Host ER signal OFF HOST ER (CNC DR) signal is not turned ON.
Check whether or not the cable is disconnected from the connector.
Check whether or not the cable is broken. Check whether or not the HOST power is turned
ON. -15 Parity H error
Communication ends with parity H. Recheck the HOST software as to whether or not
the data to be transmitted to CNC is ISO code. -16 Parity V error
Communication ends with parity V. Recheck the data to be transmitted to CNC.
-17 Overrun error Although CNC transmits DC3 (request to stop data transfer) to the HOST, it receives data of 10 bytes or more from the HOST, thus terminates communication. When CNC is transmitting data to the HOST, it receives data of 10 bytes or more from the HOST.
Recheck the software as to whether or not the HOST stops transmitting data within 10 bytes after receiving DC3.
Recheck the HOST software as to whether or not the HOST transmits data such as a command or header to CNC during receiving a work program.
Appendix 6. Alarms 6.1 List of Alarms
IV - 81
6.1.11 User PLC Alarms
(The bold characters are the messages displayed on the screen.) U Message
Sub-status 2 Sub-status 1 Message Alarm class
Sub-status Message 1 2
Details Remedy
U01 No user PLC
- - PLC program is not input. (Note) Emergency stop (EMG) will
be applied.
Download the PLC program of the format selected with the PLC environment selection parameters (bit selection #51/bit 4).
0x0010 - PLC scan time error The scan time is 1 second or longer.
Edit the PLC program size to a smaller size.
0x0040 - PLC program operation mode illegal
PLC program different from the designated mode was downloaded.
(Note) Emergency stop (EMG) will be applied.
Download the PLC program having the same format as when the power was reset or turned ON.
0x0080 - GPPW ladder code error (Note) Emergency stop (EMG) will
be applied.
Download the correct GPPW format PLC program.
0x008x - PLC4B ladder code error An illegal circuit was found in the PLC4B ladder. bit1: PC medium-speed circuit
illegal bit2: PC high-speed circuit illegal
(Note) Emergency stop (EMG) will be applied.
Download the correct PLC4B format PLC program.
U10 Illegal PLC
0x0400 Number of ladder steps
Software illegal interrupt The PLC program process stopped abnormally due to an illegal software command code.
(Note) Emergency stop (EMG) will be applied.
Turn the power ON again. If the error is not reset, download the correct PLC program.
Appendix 6. Alarms 6.1 List of Alarms
IV - 82
Sub-status Message
1 2 Details Remedy
Software exception The PLC program process stopped abnormally due to a bus error, etc.
bit 0: BIN command operation error bit 1: BCD command operation
error
Refer to the methods for using the BCD and BIN function commands.
U10 Illegal PLC
0x800x Number of PLC program steps
bit6: CALL/CALLS/RET command error
bit7: IRET command execution error
(Note) Emergency stop (EMG) is applied for bit 6/7.
Turn the power ON again. If the error is not reset, download the correct PLC program.
U50 PLC stopped
The PLC program is stopped. Start the PLC program.
U55 PLC stopped / is not saved
The PLC program is stopped and not written into ROM.
Write the PLC program into ROM.
U60 Ladder is not saved
The PLC program is not written into ROM.
Write the PLC program into ROM.
(Note) The number of PLC program steps displayed on the screen may not match the actual number of error
occurrence steps because of the PLC program timing. Use this as a guideline of the occurrence place.
Appendix 6. Alarms 6.1 List of Alarms
IV - 83
6.1.12 Network Service Errors
Message Details Remedy N001
Modem initial error
There is an error in the modem connection when the power is turned ON.
Check the connection between the NC and modem, connection port and modem power.
N002 Redial over
The dial transmission failed more than the designated No. of redial times.
Wait a while, and then transmit again.
N003 TEL unconnect
The phone line is not connected. Check the modems phone line connection.
N004 Net communication error
An error other than the above errors occurred during communication.
Note down the circumstances under which this error occurred, and contact the Service Center.
N005 Invalid net communication
The modem connection port is being used for another function such as input/output.
The modem connection port settings are incorrect.
Quit using the modem connection port with the other function, and then turn the power ON again.
Check the modem connection port settings.
N006 Received result of diagnosis
The diagnosis data file has been received
Erase the message.
N007 Send data size over
A file larger than Anshin-net server capacity (64Kbyte) has been transmitted during machining data sharing.
Reduce the size of machining program file so that it won't exceed the capacity of Anshin-net server.
N008 No file on server
When machining data sharing function is being executed, file reception fails, as the file does not exist on Anshin-net server.
Before receiving file, confirm that a machining program file exists on Anshin-net server.
N009 Password error
File reception fails due to wrong password when machining data sharing is being executed.
Input the password again.
N010 Customer number error
Data reception fails due to wrong customer number when machining data sharing is being executed.
Input the customer number again.
N011 Storage capacity over
As the size of file to be received is bigger than free space on the NC side, file reception fails during machining data sharing.
Ensure sufficient free space on the NC side.
N012 File deletion error
A file on Anshin-net server cannot be deleted when machining data sharing is being executed.
Check if the file exists on Anshin-net server. Note down the circumstances under which
this error occurred, and contact the Service Center.
Appendix 6. Alarms 6.2 Operation Messages
IV - 84
6.2 Operation Messages The following messages display on each screen.
6.2.1 Search-related Operation Messages Message Details
Searching The operation search is being executed. Search completed The operation search was completed correctly. Verifying The program is being verified. Verifying stopped The program verification stopped. Search error Could not find the designated ONB number.
Review the ONB number or machining program settings. The operation search could not be completed correctly. When the parameter (#9005) of the tape mode port was set out of the
range or when the port was not connected, an operation search of NC serial was performed.
The T code list search failed. Review the program name. Could not find the machining program in HD or IC card. Check the parameters for HD operation or IC card operation. Tape search was executed during the HOST LINK communication.
Setting error The directory name exceeded the display range. A directory path for which the entire directory cannot be displayed cannot be designated in the directory name area.
The search is not possible because ONB number is not designated. Restart search is completed The restart search was completed. Executing restart search The restart search is being executed. Execute operation search The program is not searched.
Execute the operation search. Can't cancel verify stop The compare stop cannot be canceled because the operation is not
in a compare stop. Executing top search The top search is being executed correctly. Top search completed The top search was completed correctly. Top search not completed The restart search (type 2) was executed without the top search. Can't input data Data input was attempted during M, S, T, B history display. Input some of ONB Awaiting ONB number input Verifying stop posn already registered
The verify stop position has already been registered.
No searched program The program has not been searched. Program restarting The program is being restarted. Program error The restart search was executed in the program with an error. N/B block not found The restart search was executed, designating N or B No. not exist. Restart search interrupted by reset
Reset was executed during the restart search.
No. of repetitions exceeded The restart search was executed, designating the number of repetitions exceeding the number set in the program.
Program not found The restart search was executed, designating a program No. not exist.
Appendix 6. Alarms 6.2 Operation Messages
IV - 85
6.2.2 Graphic Display-related Operation Messages
Message Details Searching The check search is being executed.
Search error Could not find the designated ONB number. Review the ONB number or machining program settings.
The check search could not be completed correctly. When the parameter (#9005) of the tape mode port was set out of the
range or when the port was not connected, an operation search of NC serial was performed.
Executing automatic operation An attempt was made to perform operations such as parameter, tool compensation amount data and coordinate system offset settings during auto operation. (Input/output also possible during auto operation)
The machining program and MDI data that the operator is attempting to edit cannot be edited during auto operation.
It is not possible to be executed a check search or check start-up during auto operation.
An attempt was made to set the verify stop position during auto operation.
Setting error The directory name exceeded the display range. A directory path for which the entire directory cannot be displayed cannot be designated in the directory name area.
The check search is not possible because ONB number is not designated.
A non-existent axis name or setting that does not exist in the format was made when making the display mode settings. Set using an existing axis name.
Incorrect tool No. was specified at the execution of tool clear. Execute operation search The program is not searched.
Execute the operation search. Checking The program check is being executed. Check stopped The program check is being stopped. Work form is illegal A workpiece is not drawn correctly because the two or more
workpiece widths are set to "0". Push [Check reset] menu An error occurred in the graphic check.
Press the [Check reset] menu key to reset the error. Executing trace The trace mode is valid. Program check completed The trace in the program check completed with an M02/M30 code. Reset complete The program check was reset. Tool interfere with work The tool contacted the workpiece when performing rapid traverse
(G0) movement with the interference check enabled. Program checking The program check is being executed. Executing reset operation The program check is being reset. Executing trace(tip posn) The tip position trace mode is valid. Executing BG simulation The back ground simulation is being executed. Draw library inside error (n) Contact the service center.
Appendix 6. Alarms 6.2 Operation Messages
IV - 86
Message Details
Program check not possible Graphic check was attempted during the Computer link B operation. Execute check search The program check is disabled. Execute the check search. Solid check disabled (memory shortage)
The 3D program check is disabled due to the memory shortage. Separate the programs and execute the check drawing again. Press the menu [Work init] once before performing the check drawing again.
6.2.3 Variable (Common variables, local variables) - related Operation Messages Message Details
Erase? (Y/N) Message to confirm the line erase. [Y] or [INPUT] : Variables are deleted. [N] : Variables are not deleted.
6.2.4 PLC Switch-related Operation Messages
Message Details Set up parameter ?(Y/N) Message to confirm the parameter setup.
[Y] or [INPUT] : It will be possible to make settings. [N] : It will not be possible to make settings.
6.2.5 Compensation-related (Tool compensation, coordinate system offset) Operation Messages
Message Details Erase? (Y/N) Message to confirm the erasing.
[Y] or [INPUT] : Erase the data. [N] : Do not erase the data.
Clear all axes? (Y/N) Message to confirm the all axes clear. [Y] or [INPUT] : Clear the data for all axes. [N] : Do not clear the data.
Cannot return to origin Operations other than line paste, paste and data input cannot be undone.
It is the initial state. Cannot undo. The last operation was performed in another part system. Cannot
undo the operation. Clear all? (Y/N) Message to confirm the clearing the all data.
[Y] or [INPUT] : Clear all data. [N] : Do not clear the data.
Input P number The coordinate system [Coord G54.1 P] menu was pressed. The expansion workpiece coordinate system P No. was input.
Data clear complete Clearing of the collection data is complete. Execute the collection data clear?
Determines whether to clear the collection data. Press [Y] or [INPUT] to clear the data.
Appendix 6. Alarms 6.2 Operation Messages
IV - 87
6.2.6 Data Input/Output-related Operation Messages Message Details
Overwrite this file?(Y/N) Message to confirm the overwriting. [Y] or [INPUT] : Overwrite the file. [N] : Do not overwrite the file.
Over run error The buffer overran or overflowed. Memory over The program cannot be written, because the memory capacity will be
exceeded. Edit lock B It is not possible to change machining program B (8000 to 8999: user
standard subprogram) or machining program C (9000 to 9999: machine tool builder custom program) as edit lock B is enabled.
Edit lock C It is not possible to change machining program C (9000 to 9999: machine tool builder custom program) as edit lock C is enabled.
Can't make directory on this device
Creation of a directory was attempted for a device that cannot have a directory.
Designated file does not exist The file specified in device A, and B does not exist. The applicable file does not exist in the specified directory.
The file name is a directory A directory was designated for the file transfer. A directory cannot be transferred.
Change complete The data conversion completed correctly. Changing The data is being converted. Erase complete The file has been erased. Erase ended. Some file not erased
The file erasing completed, but there are some files that could not be erased.
Verify error An error occurred when performing a file verification.
Compare error. Compare next file?(Y/N)
Message to confirm the comparison [Y] or [INPUT] : Compare the next file. [N] : Do not compare the next file.
Compare complete The data comparison completed. Verifying The data is being compared. The file already exists The input file name already exists.
The file name after renaming already exists. Can't erase designated file Erasing was attempted of a file that cannot be erased. Can't rename designated file An attempt was made to change the name of a file that cannot be
renamed.
Can't condense designated file Condensing of a file that cannot be condensed was attempted.
Designated file is locked Changing was attempted of a locked file. Can't open file for dev A Could not find the file for device A.
Or, the file is in a state in which it cannot be accessed. Can't open file for dev B Could not find the file for device B.
Or, the file is in a state in which it cannot be accessed. Can't read file for dev A Could not read in the file for device A.
Recheck the connection status for device A or the input/output parameter setting.
Can't read file for dev B Could not read in the file for device B. Recheck the connection status for device B or the input/output parameter setting.
Appendix 6. Alarms 6.2 Operation Messages
IV - 88
Message Details
Can't close file for dev A Contact the service center
Can't close file for dev B Contact the service center.
Can't write file for dev A Could not write in the file for device B. Recheck the connection status for device A or the input/output parameter setting.
Can't write file for dev B Could not write in the file for device B. Recheck the connection status for device B or the input/output parameter setting.
Can't seek file for dev A Contact the service center. Can't seek file for dev B Contact the service center.
File name not designated for dev A
A file name was not designated for device A.
File name not designated for dev B
A file name was not designated for device B.
Can't open directory for dev A Could not find a directory corresponding to device A.
Can't open directory for dev B Could not find a directory corresponding to device B.
Different devices designated in A and B
The same device must be designated for devices A and B, but differing devices were designated.
Timeout error A timeout error occurred when communicating with the external device.
Checking Cannot be executed during a check
Make directory complete Creation of the directory has been completed.
Dir create Complete Creation of the directory has been completed.
Can't make directory An error occurred while creating the directory. The directory is not empty A file was found in the directory.
Erase the file in the directory. Directory pass is illegal The designated directory path name is illegal.
Input a correct directory path name. Data protect Setting, erasing, parameter setting, etc., of the various data is
prohibited, because the data protect key is validated. Transfer complete The data transfer completed correctly. Transferring The data is being transferred. Parity H error A parity H error was detected. Parity V error A parity V error was detected. File entry over The No. of registration files designated in the specifications was
exceeded, so the file could not be registered. Program No. not found in the file There is no program number in the selected file. Executing format The formatting is being executed. Format complete The formatting completed. Format error The formatting failed. Framing error An error occurred between the NC and the external device. Variable conversion error An error occurred during the M2 macro conversion, and the
conversion failed.
Appendix 6. Alarms 6.2 Operation Messages
IV - 89
Message Details
Merge complete The data merge completed. Merge execution The data merge is being executed. Memory alloc error Securing of the communication data range failed. Rename complete The rename has been completed.
OK? (Y/N) Message to confirm the operation. [Y] or [INPUT] : Execute the operation
[N] : Cancel the operation.
I/O not ready An error occurred between the NC and the external device. I/O parameter error The external device settings and input/output parameters do not
match. I/O port busy Input/output was not possible as the I/O port is busy. FD write protect The FD is write-protected.
Release the write protection. PLC running An attempt was made to input a user PLC during PLC RUN.
Stop the PLC on the maintenance screen. FD not ready An attempt was made to perform an FD operation search with no FD.
An attempt was made to display the FD list with no FD. MemoryCard not ready An attempt was made to perform operations with no memory card.
DS not ready An attempt was made to perform operations with no data server.
Can't write in READ-ONLY file Contact the service center.
Condense complete Condensing has been completed.
A directory does not exist The specified directory does not exist.
Setting complete normally Decryption code setting file of the credit system was set normally.
Appendix 6. Alarms 6.2 Operation Messages
IV - 90
6.2.7 Parameter-related Operation Messages Message Details
Designate copy end posn The copy start position was specified using the cursor. Continue and specify the copy end position using the cursor.
Copy start posn and end posn reversed
When the copy range was designated, a position before the start position was designated as the end position.
Columns of copy start and end different
A different column (axis or part system) was specified for the copy start/end position at the screen with the arrangement configuration for each axis and part system.
Copy range is inadequate Could not find the parameter No. for the copy start position. A value larger than the last parameter No. was designated as the
copy end position parameter No. Check the designated copy range.
Setting error The port is already being used. The parameter HOST LINK was turned ON during the Anshin-net
communication. Setting error: column n The nth column setting data is inappropriate when multiple axes were
set at the same time (/ division). (Settings have been made up to the (n-1)th column.)
Password is illegal The password designated for displaying the Machine Parameter screen is illegal.
Input the password The menu key for first displaying the Machine Parameter screen was pressed after the power was turned ON.
Paste error An attempt was made to paste in a different parameter from the copy parameter.
Paste? (Y/N) Message to confirm the operation when pasting. [Y] or [INPUT] : Paste the data at the current cursor position. [N] : Do not paste the data.
Data protect Setting, erasing, parameter settings, etc., of the various data is prohibit, because the data protect key is validated.
Executing automatic operation An attempt was made to make parameter settings during auto operation.
Can't select The password designated for displaying the machine parameters has not been input.
Display of the machine parameters was attempted on the [Param No.] menu, but the password has not been input. Press the [Machine param] menu, and input the password for displaying the machine parameters.
No odd number for R register start No.
An odd number cannot be used for R register start No. Use an even number.
Appendix 6. Alarms 6.2 Operation Messages
IV - 91
6.2.8 Measurement-related (Workpiece, rotation) Operation Messages Message Details
TLM switch OFF Measurement, retrieving of the skip position, writing the coordinates data etc. was attempted when the TLM switch was OFF.
Can't take-in skip posn Could not retrieve the skip position. Check the following:
< When measuring the workpiece > 1. Is the name of the axis to be measured designated in the basic axis
(I, J, K)? 2. Is the axis that executed the axis movement a measurement axis? < When measuring the rotation > 1. Is the name of the axis to be measured designated in the coordinate
rotation plane (horizontal axis, vertical axis)? 2. Is the axis that executed the axis movement a measurement axis?
Can't write coordinates data Could not obtain the measured axis No. The measured angle was illegal. Could not write into the coordinate system offset.
Measure again. The work coordinate offset data was attempted to set when the
measurement counter does not have the necessary values. The work coordinate offset date was attempted to set in the slave
axis. Sensor take in not possible Could not retrieve the position measured with the touch sensor.
Measure again. Can't measure Measurement failed. Sensor signal was illegally turned on
The sensor signal was already ON when the tool measurement mode (TLM) signal was validated.
The sensor signal turned ON when there was no axis movement after the tool measurement mode (TLM) signal was validated.
The sensor signal turned ON at a position within 100m from the final entry start position.
Move the axis in a safe direction after turning the sensor signal OFF or turning the tool measurement mode signal OFF.
Can't write compensation data The cursor position and the cell for writing the compensation amount (length dimension, radius dimension) do not match. Match the cursor position with the cell for writing the compensation amount.
Offset No. not found During manual tool length measurement, the sensor was turned ON designating tool compensation No. not exist.
During manual tool length measurement, the measurement method was switched to manual tool length measurement 2 designating tool compensation No. not exist.
Correctly set the R register of compensation No. TLM axis is illegal During 2 or more axes movement, the tool length measurement was
executed by turning the sensor ON. Keep the tool away from the sensor and execute the measurement by one axis.
TLM axis not returned to ref. position
The tool length measurement was executed by tuning the sensor ON for the axis in which dog-type reference point return has not been executed. Carry out reference point return for the measurement axis.
Can't write rotation parameter The measured result cannot be set in the process parameter.
Appendix 6. Alarms 6.2 Operation Messages
IV - 92
Message Details
Can't calculate center & angle for rot
Three points necessary for calculation are not retrieved.
Center shift amount or censor radius was failed to retrieve.
Calculation of the center and the angle was failed.
Input 0 to coord center & angle for rot
The center and the angle are not "0".
Set "0" in the parameter "#8623 Coord rot centr (H)", "#8624 Coord rot centr (V)" and "#8627 Coord rot angle".
Can't calculate Hole center cannot be determined.
Meas axis not returned to ref. position
The workpiece measurement was executed when dog-type reference point return has not been executed. Carry out reference point return for the measurement axis.
Appendix 6. Alarms 6.2 Operation Messages
IV - 93
6.2.9 Tool (Tool registration, tool life) -related Operation Messages Message Details
Designated group already exists An already existing group No. was designated when changing the group No. (Tool life screen (grp))
An already existing group No. was designated when newly creating the group. (Tool life screen (grp list)) Designate a group No. that does not already exist.
Designated group does not exist Erasing was attempted on the Tool life screen (grp list) of a group that does not exist.
Can't register group The group registration process on the Tool life screen (grp list) failed. Can't delete group The group deletion process on the Tool life screen (grp list) failed. Erase? (Y/N) Message to confirm the erasing.
[Y] or [INPUT] : Erase the data [N] : Do not erase the data.
Delete all groups? (Y/N) Message to confirm the erasing of all groups. [Y] or [INPUT] : Erase all groups [N] : Do not erase all groups.
Can't delete all groups All groups' deletion cannot be executed because data protection key (KEY 1) is validated or automatic operation mode is validated, etc. during all groups' deletion. All groups' deletion cannot be executed because nothing has been registered to group, also.
Pot number not exist The set pot number does not exist. Check the pot number.
Create new file? (Y/N) Message to confirm the operation when newly creating data, files, etc. [Y] or [INPUT] : Newly create. [N] : Cancel the operation.
Input the tool number Waiting tool number input. Clear not possible The clear range is incorrect. Spindle/stndby tool display not possible
The spindle standby cannot be displayed due to the user PLC setting. Contact the machine tool builder.
Format tool life data? (Y/N) Determines whether to format the tool life management data. When [Y] is input, the formatting is executed.
Tool life format complete The tool life management data formatting completed. Exists in spindle/standby. Set? (Y/N)
An attempt was made to set the same No. as the tool No. for spindle/standby.
Exists in magazine 1. Set? (Y/N) An attempt was made to set the same No. as the tool No. that has been registered to the valid magazine.
Exists in magazine 2. Set? (Y/N) An attempt was made to set the same No. as the tool No. that has been registered to the valid magazine.
Exists in magazine 3. Set? (Y/N) An attempt was made to set the same No. as the tool No. that has been registered to the valid magazine.
Exists in magazine 4. Set? (Y/N) An attempt was made to set the same No. as the tool No. that has been registered to the valid magazine.
Exists in magazine 5. Set? (Y/N) An attempt was made to set the same No. as the tool No. that has been registered to the valid magazine.
Appendix 6. Alarms 6.2 Operation Messages
IV - 94
6.2.10 Editing-related Operation Messages Message Details
Buffer correct not possible Buffer correction cannot be performed for this program. Buffer correction was attempted during the BTR operation.
Can't write into file Could not write the data to the memory with the buffer correction. Contact the service center.
Overwrite this file?(Y/N) Message to confirm when registering MDI [Y] or [INPUT] : Overwrite the file. [N] : Do not overwrite the file.
Memory over The program cannot be written, because the memory capacity will be exceeded.
Designated character string not found
Could not find the search results and character string in the program.
Save current file ?(Y/N) Message to confirm the saving. [Y] : Save the changes to the current file. [N] : Do not save the changes to the current file.
A file does not exist An attempt was made to select and edit a non-existent file.
Executing Following menu's process is executing now: "Line paste", "Line clear", "Undo", "String search", "String replace", "Miss warning", or "Next miss".
Designated file does not exist An attempt was made to select and erase a non-existent file. Erase complete The data erasing completed. Can't erase designated file The selected file cannot currently be erased. Designated file does not exist A file that does not exist was designated when file editing. Designated file already exists When creating a new file, a file name was designated that already
exists. Replace? (Y/N) Message to confirm the character string replacement.
[Y] or [INPUT] : Replace the character string. [N] : Do not replace the character string.
File access error Contact the Service Center. File open error The designated file is already open. Editing A program is being edited on the screen.
Save the program to write it into the memory. Program entry over The program could not be registered in the memory when attempted,
because the No. of registrations designated in the specifications would be exceeded.
Block char nos over The character number limitation in one block was exceeded.
Paste error Pasting was attempted within the copy range of the same file.
Copy range is inadequate The copy range designation is inadequate. Check whether the designated range exists.
The range was designated exceeding 100 lines during mass editing. Area designation is inadequate
The area designation is inadequate. Check whether the designated area exists.
Designated line is out of program range
Designation was attempted of a line No. larger than the No. of lines in the entire program.
Appendix 6. Alarms 6.2 Operation Messages
IV - 95
Message Details
MDI no setting Editing of the MDI was started, but the MDI setting was incomplete. Abs/Inc mode is illegal During playback editing:
G90 was set when control parameter "Playback G90" was OFF. G91 was set when control parameter "Playback G90" was ON.
MDI search complete The MDI search completed. Can't search in MDI mode The restart search was attempted during MDI mode.
Execute the restart search after switching other than MDI mode. MDI Set ended MDI setting cannot be executed. MDI Setting error MDI setting was completed. MDI search error Could not execute the MDI search. MDI entry complete MDI entry has been completed. Can't edit except in MDI mode "#1144 mdlkof" (MDI setting lock) is "0" and therefore it is not possible
to edit the MDI program in a mode other than MDI mode. Input miss was detected An input miss was detected. Input miss was not detected A search was performed for an input miss, however, none was found. Can't edit a file except in NC memory
Editing cannot be performed at the edit window for programs other than those in the NC memory.
Save it The cursor was tried to move beyond the editable range during mass-editing. Save, then operate again.
Save not possible A special file (history file etc.) that cannot be saved was edited and an attempt was made to save it. Perform an operation to quit editing.
Failed saving due to file size over, etc. during mass-editing. Setting of "#1166 fixpro" was illegal. Use the settings for a regular
program. MDI cannot be entered due to MDI editing mode. Press INPUT key
and finish editing. Save left side file? (Y/N)
Message to confirm whether saving the left side file of the multi-program display type [Y]: Save the change [N]: Do not save the change
Save right side file? (Y/N)
Message to confirm whether saving the right side file of the multi-program display type [Y]: Save the change [N]: Do not save the change
Can't edit because of size over The program cannot be written, because the memory capacity will be exceeded.
If the memory capacity of the transfer designation device is exceeded during the automatic backup, increase the available memory of the device.
Can't edit the searched file The serial file cannot be edited.
DS not ready
Operation was attempted when a DS was not inserted. Creating or opening a program was attempted when a DS was not
inserted. FD not ready
The FD operation search was attempted when an FD was not inserted.
The FD list display was attempted when an FD was not inserted. Creating or opening a program was attempted when an FD was not
inserted.
Appendix 6. Alarms 6.2 Operation Messages
IV - 96
Message Details
MemoryCard not ready Operation was attempted when a memory card was not inserted.
This cannot be specified Invalid special characters (/E, etc.) were set.
Loading Loading file.
Saving Saving file.
Can't execute playback edit The playback editing cannot be executed because the right side area is mass-editing mode.
Playback editing was attempted while program file to be edited is not designated. Display a program file in the right side area.
Program display lock C The program display or search cannot be executed. Review the parameter "#1121 pglk_c" (program display lock).
6.2.11 Diagnosis-related Operation Messages Message Details
Erase? (Y/N) Message to confirm alarm history clear operation [Y] or [INPUT] : Erase the data [N] : Do not erase the data.
Can't write data The data cannot be written. Device is illegal The designated device is inadequate. Modal output not possible The modal output process failed. Modal clear not possible The modal cancel process failed. Continue display not possible Continuous display is not possible because data is not set at the
cursor position. One-shot output not possible The one-shot output process failed. Setting data not found The data has not been set. Select a menu A device No. was set without selecting a menu operation.
Press any operation menu and input the device No. with a menu highlighted.
Appendix 6. Alarms 6.2 Operation Messages
IV - 97
6.2.12 Maintenance-related Operation Messages Message Details
Password is illegal The input password is incorrect. Input password The [Password] menu key was pressed, and the password input
mode was entered. Input a password.
Now making back-up Currently backing up system data and the user PLC program to a specified device.
Backupping The SRAM data is being backed up on the HD. Backup complete Backup of the SRAM data on the HD has been completed.
Back up of system data and user PLC program to a specified device has been completed.
Backup error An error occurred while backing up the SRAM data on the HD. Select directory to backup
Select area by moving cursor, using and keys.
Press the "INPUT" key to confirm.
Select directory to restore Select file by moving cursor, using and keys. Press the "INPUT" key to confirm.
Executing format The formatting is being executed correctly. Format complete The formatting completed correctly. Format error The NC memory formatting failed.
Contact the nearest service center. Quit HMI ?(Y/N) Message to confirm the HMI quitting
[Y] or [INPUT] : Quit the HMI. [N] : Do not quit the HMI.
Format NC memory?(Y/N) Message to confirm the NC memory formatting [Y] or [INPUT] : Start formatting the NC memory. [N] : Do not format the NC memory.
Execute SRAM backup ?(Y/N) Message to confirm the SRAM back up [Y] or [INPUT] : The SRAM data is backed up to the HD. [N] : The SRAM data is not backed up to the HD.
PLC running. Does it stop? (Y/N) Message to confirm the PLC STOP [Y] or [INPUT] : Backup the SRAM data on the HD. [N] : Do not backup the SRAM data on the HD.
Restoring The system data and user PLC program are now being restored to the NC from a specified device.
Restore complete Restoration of system data and user PLC program to the NC from a specified device has been completed.
Auto adjust error The H/W status cannot be read properly, and therefore it is not possible to perform auto adjustments. Check the remote I/O unit. Perform manual adjustments.
The unit is defective. Replace the unit. Change Ope. test mode Operation of the Operation test screen was attempted when the
operation adjustment mode was not selected. Test mode sig valid signal is now OFF
The operation adjustment mode cannot be selected because the operation adjustment mode valid signal (R9998/bit0) is 0.
Appendix 6. Alarms 6.2 Operation Messages
IV - 98
Message Details
Auto adjust complete Analog output adjustment completed normally. Auto adjust execution Performing analog output adjustment normally. Execute? (Y/N) Message to confirm the operation
[Y] or [INPUT] : The currently selected operation is performed. [N] : The currently selected operation is not performed.
Unit not equipped The machine is not equipped with an analog output unit. A serial number is inaccurate The system data to be restored and the serial number in the NC do
not match, and therefore it is not possible to restore. Check to ensure that the serial number in the NC has been set and
that the system data to be restored matches. Operating aux axis It is not possible to set parameter and input/output data during
auxiliary axis operation. It is not possible to change the display axis during auxiliary axis
operation.
Appendix 6. Alarms 6.2 Operation Messages
IV - 99
6.2.13 Data Sampling-related Operation Messages Message Details
Executing sampling The waveform data is being sampled.
Input the axis name This appears when the data type is selected in the Ch1 or Ch2 data setting area. Input the name of the axis to be sampled.
Input axis name/signal No./bit This appears when the data type is selected in the Ch1 or Ch2 data setting area. Set the sampling conditions common for Ch1 and Ch2.
Input device name/device No. Input device name/device No. Input file/sub-ID/item/data This appears when an NC file is selected in the Ch1 or Ch2 data
setting area. Change the area Change the area.
Sampling conditions are illegal The data cannot be sampled as the setting conditions are illegal. Review the data, vertical scale, sampling rate and horizontal scale on the Condition setting screen.
Can't start sampling "#1224 aux08/bit0" is "0" and sampling start-up cannot be performed. The collection invalid The parameters are set to prevent data being collected. Check the
parameters. The collection begin? Determines whether to start data collection. Press [Y] or [INPUT] to
start data collection. The collection stop? Determines whether to stop data collection. Press [Y] or [INPUT] to
stop data collection. The collection is being executed An attempt was made to start data collection while data collection
was being performed. The collection is stopping An attempt was made to stop data collection while data collection was
stopped. The collection invalid The data collection is set invalid in the parameter. Check the
parameter. Scroll execution The waveform display is being scrolled.
Refresh execution The waveform is being refreshed.
Appendix 6. Alarms 6.2 Operation Messages
IV - 100
6.2.14 Absolute Position Detection-related Operation Messages Message Details
Setting absolute position set Setting from the screen was attempted of absolute position detection data when the "Absolute Position Set" was not ON. Press the menu key [Absolute Position Set] to turn it ON.
Not the abs position detection system
An absolute position detection system has not been selected for the currently selected axis. The machine parameter (Axis specification parameter "#2049 type") must be set.
Axis name inappropriate The set axis name is inappropriate. Check the axis name. Not passed on grid The absolute position basic point was set without passing the grid
after the power ON in the dogless-type absolute position detection. Return one grid back and repeat the procedure.
Can't start Settings of "#0 absolute posn set", "#2 Z-point" and "#2055 pushf" are not adequate.
"AbsEncoder: Serial data error" alarm (Z71 0005) has occurred. Check the parameter and the alarm.
Illegal direction JOG starting direction is illegal in the machine end stopper method of the dogless-type absolute position detection.
6.2.15 System Setup-related Operation Messages Message Details
Initial parameter creating The initial parameter is being created.
Initial parameter transferring The initial parameter is being transferred.
Spindle initial parameter transferring
The spindle initial parameter is being transferred.
Can't write data The data cannot be written. Setting of the initial parameter failed. Contact the service center.
Param set ended. Format NC memory? (Y/N)
After completing the parameter setting, it determines whether executing the file format or not. Enter [Y] or [INPUT] to execute the file format.
Write sample ladder? (Y/N) It determines whether executing writing the sample PLC program or not. Enter [Y] or [INPUT] to start writing the sample PLC program.
Sample ladder not found The file to set the sample PLC program is lost. Contact the service center.
Appendix 6. Alarms 6.2 Operation Messages
IV - 101
6.2.16 Automatic Backup-related Operation Messages Message Details
Auto backup disabled (Device illegal)
Set a correct value in the device No. of the automatic backup device.
Auto backup disabled (No DS) When turning ON the power next time, insert DS.
Auto backup disabled (No memory card)
When turning ON the power next time, insert the memory card.
Auto backup proceeding Wait for the automatic backup to complete.
Auto backup completed The automatic back up is completed.
Memory over The memory capacity of the transfer designation device was exceeded during the automatic backup. Increase the available memory of the transfer designation device.
File access error A file access error occurred during the automatic backup. Contact the service center.
Can't make directory The storage destination directory of the automatic backup data described in the custom definition file does not exist. Create the directory of the storage destination.
Write protect The memory card is write-protected. Release the write protection.
6.2.17 Alarm History-related Operation Messages Message Details
The collection begin? (Y/N) Determines whether to start alarm history. Press [Y] or [INPUT] to start alarm history.
The collection stop? (Y/N) Determines whether to stop alarm history. Press [Y] or [INPUT] to stop alarm history.
The collection is being executed An attempt was made to start alarm history while alarm history was being performed.
The collection is stopping An attempt was made to stop alarm history while alarm history was being stopped.
Execute the collection data clear?(Y/N)
Determines whether to clear alarm history. Press [Y] or [INPUT] to clear alarm history.
Data clear complete The alarm history cleared was completed. The collection begin The alarm history was started. The collection stop The alarm history was stopped.
Appendix 6. Alarms 6.2 Operation Messages
IV - 102
6.2.18 Anshin-net-related Operation Messages (1) Messages related to all Anshin-net screens
Message Details (None) Press one-touch call to
call the NC service. Do not turn the power OFF during the one-touch call.
Communication has not been started. A call is being placed with automatic alarm notification or one-touch call, and a call is being received from the NC service.
(2) Messages related to automatic alarm notification
Message Details dialing Do not turn the power OFF
until the automatic alarm notification ends.
A call is being placed with automatic alarm notification.
Communication starts when an alarm occurs, but the line is not connected yet in this state.
This state is also entered when standing by for transmission.
Communication has been started with emergency stop by the servo, spindle or PLC alarm, or by the establishment of the conditions set in the parameters.
Waiting for dialing Do not turn the power OFF until the automatic alarm notification ends.
Redialing since the NC service is using the line for other communication.
Verifying the user registration
Do not turn the power OFF until the automatic alarm notification ends.
User authentication is being executed by the NC service side.
Connecting Do not turn the power OFF until the automatic alarm notification ends.
The line is connected with automatic alarm notification.
Receiving Do not turn the power OFF until the automatic alarm notification ends.
The diagnosis data is being received with automatic alarm notification.
Sending Do not turn the power OFF until the automatic alarm notification ends.
The diagnosis data is being sent with automatic alarm notification.
Transmission completed
Press one-touch call to call the NC service. Do not turn the power OFF during the one-touch call.
Automatic alarm notification has ended, and the line has been disconnected.
Reception completed Press one-touch call to call the NC service. Do not turn the power OFF during the one-touch call.
Automatic alarm notification has ended, and the line has been disconnected.
This is displayed when at least one file has been received.
(Status of communication with NC service)
Connecting with NC service. Wait for communication to end.
In connection standby state since line is being used by Anshin-net.
Appendix 6. Alarms 6.2 Operation Messages
IV - 103
(3) Messages related to automatic alarm notification
Message Details Operator notice effective
If automatic operation stops while operator notification is valid, the designated telephone number will be contacted.
Operator notification is valid. If machining ends normally or abnormally in this
state, communication with operator notification will start.
Dialing Do not turn the power OFF until the operator notification ends.
Data is being transmitted with operator notification.
Communication will start when machining ends normally or abnormally, but the line is not connected yet in this state.
This state is also entered when standing by for transmission.
Waiting for dialing Do not turn the power OFF until the operator notification ends.
Redialing since the NC service is using the line for other communication.
Verifying the user registration
Do not turn the power OFF until the operator notification ends.
User authentication is being executed by the NC service side.
Connecting Do not turn the power OFF until the operator notification ends.
The line is connected with operator notification.
Receiving Do not turn the power OFF until the operator notification ends.
The diagnosis data is being received with operator notification.
Sending Do not turn the power OFF until the operator notification ends.
The diagnosis data is being sent with operator notification.
Transmission completed
Press one-touch call to call the NC service. Do not turn the power OFF during the one-touch call.
Operator notification has ended, and the line has been disconnected.
Reception completed Press one-touch call to call the NC service. Do not turn the power OFF during the one-touch call.
Operator notification has ended, and the line has been disconnected.
This is displayed when at least one file has been received.
(Status of communication with NC service)
Connecting with NC service. Wait for communication to end.
In connection standby state since line is being used by Anshin-net.
Appendix 6. Alarms 6.2 Operation Messages
IV - 104
(4) Messages related to automatic alarm notification
Message Details Carry out one-touch call? (Y/N)
Press "Y" to make a one-touch call and "N" to cancel. If the line is being in use, a connection with NC service will be established as soon as the line becomes idle.
A connection with NC service has not been established.
The system is confirming whether to actually make a one-touch call.
This is displayed when the Call menu is pressed. Press Y or INPUT to execute one-touch call.
Message Details
Dialing Do not turn the power OFF until the one-touch call ends.
Data is being transmitted with one-touch call. Communication will start when one-touch call is
executed, but the line is not connected yet in this state.
This state is also entered when standing by for transmission.
Waiting for dialing Do not turn the power OFF until the one-touch call ends.
Redialing since the NC service is using the line for other communication.
Verifying the user registration
Do not turn the power OFF until the one-touch call ends.
User authentication is being executed by the NC service side.
Connecting Do not turn the power OFF until the one-touch call ends.
The line is connected with one-touch call.
Receiving Do not turn the power OFF until the one-touch call ends.
The diagnosis data is being received with one-touch call.
Sending Do not turn the power OFF until the one-touch call ends.
The diagnosis data is being sent with one-touch call.
Transmission completed
Press one-touch call to call the NC service. Do not turn the power OFF during the one-touch call.
Communication with one-touch call has ended, and the line has been disconnected.
Reception completed Press one-touch call to call the NC service. Do not turn the power OFF during the one-touch call.
Communication with one-touch call has ended, and the line has been disconnected.
This is displayed when at least one file has been received.
(Status of communication with NC service)
Connecting with NC service. Wait for communication to end.
In connection standby state since line is being used by Anshin-net.
Appendix 6. Alarms 6.2 Operation Messages
IV - 105
(5) Messages related to transmission request from NC service
Message Details Verifying the distination
Connecting with NC service. Wait for communication to end.
User authentication is being executed by the NC system side.
Connecting Connecting with NC service. Wait for communication to end.
The line is connected upon transmission request from NC service.
Receiving Connecting with NC service. Wait for communication to end.
Data is being received upon transmission request from NC service.
Sending Connecting with NC service. Wait for communication to end.
Data is being sent upon transmission request from NC service.
Transmission completed
Press one-touch call to call the NC service. Do not turn the power OFF during the one-touch call.
Transmission request from NC service has been completed, and the line has been disconnected.
Reception completed Press one-touch call to call the NC service. Do not turn the power OFF during the one-touch call.
Transmission request from NC service has been completed, and the line has been disconnected.
This is displayed when at least one file or message has been received.
(6) Messages related to number 1 to 3 menu operations
Message Details (None) Press one-touch call to
call the NC service. Do not turn the power OFF during the one-touch call.
The selected telephone No. will be set as the telephone No. to be notified to the NC service.
Hereafter, the telephone No. set with one-touch call or operator notification will be notified to the NC service.
(7) Messages related to arbitrary number setting
Message Details (None) Input the telephone No. to
be notified. The input telephone No. will be set as the
telephone No. to be notified to the NC service. Hereafter, the telephone No. set with one-touch
call or operator notification will be notified to the NC service.
Appendix 6. Alarms 6.2 Operation Messages
IV - 106
(8) Messages related to sharing of machining data
Message Details Transmit by the set password?(Y/N)
The line is not connected with NC service. The system is confirming whether to transfer machining data. Press
"Y" or "INPUT" to transfer machining data, "N" to cancel. OK? (Y/N) The line is not connected with NC service.
The system is confirming whether to erase machining data. Press "Y" or "INPUT" to erase machining data, "N" to cancel.
dialing A call is being placed. "Transmit by the set password?(Y/N)" or "OK? (Y/N)" is shown.
Pressing "Y" or "INPUT" starts the communication. The line is not connected yet in this state.
Connecting The line is connected for sharing of machining data. Transmitting The machining data is being transmitted. Transmission completed Machining data transmission has ended, and the line has been
disconnected. Receiving The machining data is being received. Reception completed Machining data reception has ended, and the line has been
disconnected. Erase complete Machining data erasing has ended, and the line has been
disconnected. Waiting for dialing In dialing standby state since the line is being used. Input the password The password, which is required for the transmission/reception of
machining data, has not been set. Input the password set on the Anshin-net parameter 1 screen.
Input the user number The user number, which is required for the transmission/reception of machining data, has not been set. Input the user number set on the Anshin-net parameter 1 screen.
Appendix 6. Alarms 6.2 Operation Messages
IV - 107
6.2.19 Messages Related to Machine Tool Builder Network System (1) Messages related to all Machine Tool Builder Network System (MTB net) Screens.
Message Details (None) Press the [Send] menu
when you transmit the diagnosis data to MTB. Don't turn OFF the power supply while transmitting.
Communication has not been started.
Message Details Network service is connected The settings of the MTB net parameter 1,2 cannot be changed
since the system is communicating with Call Center or machine tool builder. Set again after the communication has ended.
(2) Messages related to transmission of diagnosis data
Message Details Transmit diagnosis data? (Y/N)
Press Y (transmit the diagnosis data) or N (cancel). You'll connect with MTB when it gets available if line used.
The system is confirming the transmission of diagnosis data.
dialing Don't turn OFF a power supply until diagnosis data transmission ends.
The diagnosis data is being transmitted. The line is not connected yet in this state.
Verifying the user registration
Don't turn OFF a power supply until diagnosis data transmission ends.
The system is waiting for an authentication response from remote diagnosis tool kit.
Waiting for the reply Don't turn OFF a power supply until diagnosis data transmission ends.
The line has been disconnected once, and the system is waiting for a connection with the machine tool builder.
Verifying the destination
Don't turn OFF a power supply until diagnosis data transmission ends.
The line has been connected corresponding to the received call from the machine tool builder. The system is confirming the destination of connection.
Connecting Don't turn OFF a power supply until diagnosis data transmission ends.
The system is connected or connecting with machine tool builder.
Transmitting Don't turn OFF a power supply until diagnosis data transmission ends.
The diagnosis data is actually being transmitted.
Transmission completed
Press Y (transmit the diagnosis data) or N (cancel). You'll connect with MTB when it gets available if line used.
The transmission of diagnosis data has ended, and the line has been disconnected.
Appendix 6. Alarms 6.2 Operation Messages
IV - 108
Message Details
Waiting for dialing Don't turn OFF a power supply until diagnosis data transmission ends.
The machine tool builder is using the line for other communication.
(Status of communication with NC service)
Connecting with NC service. Please wait until the communication ends.
In connection standby state since line is being used by Anshin-net.
(Status of communication with machine manufacturer)
Connecting with MTB. Please wait until the communication ends.
In connection standby state since line is being used by the machine tool builder.
(3) Messages related to reception of the diagnosis results
Message Details Verifying the destination
Connecting with MTB. Please wait until the communication ends.
The line has been connected corresponding to the received call from the machine tool builder. The system is confirming the destination of connection.
Connecting Connecting with MTB. Please wait until the communication ends.
The system is connected or connecting with machine tool builder.
Receiving Connecting with MTB. Please wait until the communication ends.
The diagnosis results are actually being received.
Reception completed Press the [Send] menu when you transmit the diagnosis data to MTB. Don't turn OFF the power supply while transmitting.
Reception of the diagnosis results has ended, and the line has been disconnected.
(4) Messages related to reception of messages
Message Details Verifying the destination
Connecting with MTB. Please wait until the communication ends.
The line has been connected corresponding to the received call from the machine tool builder. The system is confirming the destination of connection.
Connecting Connecting with MTB. Please wait until the communication ends.
The system is connected or connecting with machine tool builder.
Reception completed Press the [Send] menu when you transmit the diagnosis data to MTB. Don't turn OFF the power supply while transmitting.
Reception of the message has ended, and the line has been disconnected.
Appendix 6. Alarms 6.2 Operation Messages
IV - 109
6.2.20 Other Operation Messages Message Details
Executing automatic operation Cannot be performed during automatic operation. Perform the operation again after automatic operation has been completed.
Setting error The setting data is inadequate. (Alphabetic characters were set where only numeric characters can be set, etc.)
The data has not been set. There is no specification.
Data range error The input data exceeded the range. Set the value again within the range.
Data protect Setting, erasing, parameter setting, etc., of the various data is prohibited, because the data protect key is validated. Reconsider the data protect key setting.
Write protect Attempted to create a new program file in the write-protected device
Opened the program file of the write-protected device
Attempted to save the program file of the write-protected device
Attempted to correct the buffer for the write-protected file.
Attempted to edit or correct the buffer for the read-only program file.
Edit lock B It is not possible to change machining program B (8000 to 8999: user standard subprogram) or machining program C (9000 to 9999: machine tool builder custom program) as edit lock B is enabled.
Edit lock C It is not possible to change machining program C (9000 to 9999: machine tool builder custom program) as edit lock C is enabled.
Origin set not possible The operation is in a state in which origin set is not possible. Check the parameter "#1123 origin (Origin set prohibited)" setting.
Check that the axis has stopped. Check that idling (post-reset status) is currently being performed.
Can't command manual value The manual numerical value protect is valid and therefore it is not possible to perform a manual numerical value command.
Getting T code list T code list is being retrieved.
T code list complete Retrieving T code list is completed.
Load meter display not possible The load meter cannot be displayed. Contact the machine tool builder.
Pallet running Each setting was executed during pallet running.
APC executing Each setting was executed during automatic pallet changer executing.
Appendix 6. Alarms 6.3 Program Error
IV - 110
6.3 Program Error (The bold characters are the message displayed in the screen.) These alarms occur during automatic operation and the causes of these alarms are mainly program errors which occur for instance when mistakes have been made in the preparation of the machining programs or when programs which conform to the specification have not been prepared.
Error No. Details Remedy
P 10 No. of simultaneous axes over The number of axis addresses commanded in the same block exceeds the specifications.
Divide the alarm block command into two. Check the specifications.
P 11 Illegal axis address The axis address commanded by the program and the axis address set by the parameter do not match.
Revise the axis names in the program.
P 20 Division error An axis command which cannot be divided by the command unit has been issued.
Check the program.
P 29 Not accept command The normal line control command (G40.1, G41.1, G42.1) has been issued during the modal in which the normal line control is not acceptable.
Check the program.
P 30 Parity H error The number of holes per character on the paper tape is even for EIA code and odd for ISO code.
Check the paper tape. Check the tape puncher and tape reader.
P 31 Parity V error The number of characters per block on the paper tape is odd.
Make the number of characters per block on the paper tape even.
Set the parameter parity V selection OFF. P 32 Illegal address
An address not listed in the specifications has been used.
Check and revise the program address. Check and correct the parameters values. Check the specifications.
P 33 Format error The command format in the program is not correct.
Check the program.
Illegal G code A G code not listed in the specifications has been used. An illegal G code was commanded during the coordinate rotation command (G68).
Check and correct the G code address in the program.
P 34
G51.2 or G50.2 was commanded when the rotary tool axis No. (#1501 polyax) was set to "0". G51.2 or G50.2 was commanded when the tool axis was set to the linear axis (#1017 rot "0").
Check the parameter setting values.
P 35 Setting value range over The setting range for the addresses has been exceeded.
Check the program.
P 36 Program end error "EOR" has been read during tape and memory mode.
Enter the M02 and M30 command at the end of the program.
Enter the M99 command at the end of the subprogram.
Appendix 6. Alarms 6.3 Program Error
IV - 111
Error No. Details Remedy
P 37 O, N number zero A zero has been specified for program and sequence Nos.
The program Nos. are designated across a range from 1 to 99999999.
The sequence Nos. are designated across a range from 1 to 99999.
P 38 No spec: Add. Op block skip "/n" has been issued even though there are no optional block skip addition specifications.
Check the specifications.
P 39 No specifications A non-specified G code was specified. The selected operation mode is not used.
Check the specifications.
P 40 Pre-read block error When tool radius compensation is executed there is an error in the pre-read block and so the interference check is disabled.
Reconsider the program.
P 48 Restart pos return incomplete Movement command was executed before executing the block that is restart-searched.
Carry out program restart again. Movement command cannot be executed before executing the block that is restart-searched.
P 49 Invalid restart search Restart search was attempted for the
3-dimensional circular interpolation. Restart search was attempted during the
cylindrical interpolation, polar coordinate interpolation, and tool tip center control.
Reconsider the program. Reconsider the restart search position.
P 50 No spec: Inch/Metric change Inch/Metric changeover (G20/G21) command was issued even though there is no inch/metric conversion specification.
Check the specifications.
P 60 Compensation length over The commanded movement distance is excessive. (Over 231)
Reconsider the axis address command.
P 61 No spec: Unidirectional posit. Unidirectional positioning (G60) was commanded even though there is no unidirectional positioning specification.
Check the specifications.
P 62 No F command No feed rate command has been issued. There is no F command in the cylindrical
interpolation or polar coordinate interpolation immediately after the G95 mode is commanded.
The default movement modal command at power ON is G01. This causes the machine to move without a G01 command if a movement command is issued in the program, and an alarm results. Use an F command to specify the feed rate.
Specify F with a thread lead command. P 63 No spec: High-speed machining
High-speed machining cancel (G5P0) was commanded even though there is no high-speed machining mode specification.
Check the specifications.
P 65 No spec: High speed mode 3 Check the high-speed mode III specifications.
Appendix 6. Alarms 6.3 Program Error
IV - 112
Error No. Details Remedy
P 70 Arc end point deviation large There is an error in the arc start and end
points as well as in the arc center. The difference of the involute curve through
the start point and the end point is large. When arc was commanded, one of the two
axes configuring the arc plane was a scaling valid axis.
Check the numerical values of the addresses that specify the start and end points, arc center as well as the radius in the program.
Check the "+" and "-" directions of the address numerical values.
Check the scaling valid axis.
P 71 Arc center error The arc center is not sought during
R-specified circular interpolation. The curvature center of the involute curve
cannot be obtained.
Check the numerical values of the addresses in the program.
Check whether the start point or end point is on the inner side of the base circle for involute interpolation. When carrying out tool radius compensation, check that the start point and end point after compensation are not on the inner side of the base circle for involute interpolation.
Check whether the start point and end point are at an even distance from the center of the base circle for involute interpolation.
P 72 No spec: Herical cutting A helical command has been issued though it is not included in the specifications.
Check the helical specifications. An Axis 3 command was issued by the
circular interpolation command. If there is no helical specification, the linear axis is moved to the next block.
P 73 No spec: Spiral cutting A spiral command was issued despite the fact that such a command does not exist in the specifications.
The G02.1 and G03.1 commands are issued for circular interpolation.
Check the spiral specifications.
P 74 Can't calculate 3DIM arc The end block was not specified during 3-dimension circular interpolation supplementary modal, and therefore it is not possible to calculate the 3-dimension circular interpolation. Furthermore, it not possible to calculate the 3-dimension circular interpolation due to an interruption during 3-dimension circular interpolation supplementary modal.
Reconsider the program.
P 75 3DIM arc illegal An unusable G code was issued during 3-dimension circular interpolation modal. Or, a 3-dimension circular interpolation command was issued during a modal for which a 3-dimension circular interpolation command cannot be issued.
Reconsider the program.
P 76 No spec: 3DIM arc interpolat G02.4/G03.4 was commanded even though there is no 3-dimension circular interpolation specification.
Check the specifications.
P80 No spec: Hypoth ax interpolat Hypothetical axis interpolation (G07) was commanded even though there is no hypothetical axis interpolation specification.
Check the specifications.
Appendix 6. Alarms 6.3 Program Error
IV - 113
Error No. Details Remedy
P 90 No spec: Thread cutting A thread cutting command was issued even though there is no thread cutting command specification.
Check the specifications.
P 91 No spec: Var lead threading Variable lead thread cutting (G34) was commanded even though there is no variable lead thread cutting specification.
Check the specifications.
P 93 Illegal pitch vaule The thread lead (thread pitch) when performing the thread cutting command is incorrect.
Set the correct thread lead command for the thread cutting command.
P100 No spec: Cylindric interpolat A cylindrical interpolation command was issued even though there is no cylindrical interpolation specification.
Check the specifications.
P110 Plane select during figure rot Plane selection (G17/G18/G19) was commanded during figure rotation.
Check the machining program.
P111 Plane selected while coord rot Plane selection commands (G17, G18, G19) were issued during a coordinate rotation command (G68).
After command G68, always issue a plane selection command following a G69 (coordinate rotation cancel) command.
P112 Plane selected while R compen Plane selection commands (G17, G18,
G19) were issued while tool radius compensation (G41, G42) and nose R compensation (G41, G42, G46) commands were being issued.
Plane selection commands were issued after completing nose R compensation commands when there are no further axis movement commands after G40, and compensation has not been cancelled.
Issue plane selection commands after completing (axis movement commands issued after G40 cancel command) tool radius compensation and nose R compensation commands.
P113 Illegal plane select The circular command axis differs from the selected plane.
Issue a circular command after correct plane selection.
P120 No spec: Feed per rotation Feed per rotation (G95) was commanded even though there is no feed per rotation specification.
Check the specifications.
P121 F0 command during arc modal F0 (F 1-digit feed) was commanded during the arc modal (G02/G03).
Check the machining program.
P122 No spec: Auto corner override An auto corner override command (G62) was issued even though there is no auto corner override specification.
Check the specifications. Delete the G62 command from the program.
P123 No spec: High-accuracy control High-accuracy control command was issued even though there is no high-accuracy control specification
Check the specifications.
Appendix 6. Alarms 6.3 Program Error
IV - 114
Error No. Details Remedy
P124 No spec: Inverse time feed There is no inverse time option.
Check the specifications.
P125 G93 mode error A G code command that cannot be issued
was issued during G93 mode. G93 command was issued during a modal
for which inverse time feed cannot be performed.
Reconsider the program.
P126 Invalid cmnd in high-accuracy An illegal command was issued during the high-accuracy control mode. A G code group 13 command was issued
during the high-accuracy control mode. Milling, cylindrical interpolation or pole
coordinate interpolation was commanded during the high-accuracy control mode.
Reconsider the program.
P127 No spec: SSS Control The SSS control valid parameter was set to ON although there is no SSS control specification.
Check the specifications. If there is no SSS control specification, set the parameter #8090 SSS ON to 0.
P130 2nd M function code illegal The 2nd miscellaneous function address commanded in the program differs from the address set in the parameters. miscellaneous function.
Check and correct the 2nd miscellaneous function address in the program.
P131 No spec: Cnst surface ctrl G96 A constant surface speed control command (G96) was issued even though there is no specification.
Check the specifications. Change the constant surface speed control
command (G96) to a rotation speed command (G97).
P132 Spindle rotation speed S=0 No spindle rotation speed command has been issued.
Reconsider the program.
P133 Illegal P-No. G96 An invalid constant surface speed control axis has been specified.
Reconsider the parameter specified for the constant surface speed control axis.
P140 No spec: Pos compen cmd The position compensation command (G45 to G48) specifications are not available.
Check the specifications.
P141 Pos compen during rotation Position compensation was commanded during the figure rotation or coordinate rotation command.
Reconsider the program.
P142 Pos compen invalid arc A position compensation invalid arc command was commanded.
Reconsider the program.
Appendix 6. Alarms 6.3 Program Error
IV - 115
Error No. Details Remedy
P150 No spec: Nose R compensation Even though there were no tool radius
compensation specifications, tool radius compensation commands (G41 and G42) were issued.
Even though there were no nose R compensation specifications, nose R compensation commands (G41, G42, and G46) were issued.
Check the specifications.
P151 Radius compen during arc mode A compensation command (G40 G41 G42 G43 G44 G46) has been issued in the arc modal (G02 G03).
Issue the linear command (G01) or rapid traverse command (G00) in the compensation command block or cancel block. (Set the modal to linear interpolation.)
P152 No intersection In interference block processing during execution of a tool radius compensation (G41 or G42) or nose R compensation (G41 G42 or G46) command the intersection point after one block is skipped cannot be determined.
Reconsider the program.
P153 Compensation interference An interference error has arisen while the tool radius compensation command (G41 G42) or nose R compensation command (G41 G42 G46) was being executed.
Reconsider the program.
P154 No spec: 3D compensation A three-dimensional compensation command was issued even though there are no three-dimensional compensation specifications.
Check the specifications.
P155 Fixed cyc exec during compen A fixed cycle command has been issued in the radius compensation mode.
The radius compensation mode is established when a fixed cycle command is executed and so the radius compensation cancel command (G40) should be issued.
P156 R compen direction not defined At the start of G46 nose R compensation the compensation direction is undefined if this shift vector is used.
Change the vector to that with which the compensation direction is defined.
Exchange with a tool having a different tip point No.
P157 R compen direction changed During G46 nose R compensation the compensation direction is inverted.
Change the G command to that which allows inversion of the compensation direction (G00 G28 G30 G33 or G53).
Exchange with a tool having a different tip point No.
Turn ON the "#8106 G46 NO REV-ERR" parameter.
P158 Illegal tip point During G46 nose R compensation the tip point is illegal (other than 1 to 8).
Change the tip point No. to a legal one.
Appendix 6. Alarms 6.3 Program Error
IV - 116
Error No. Details Remedy
P170 No offset number The compensation No. (DOO TOO HOO) command was not given when the radius compensation (G41 G42 G43 G46) command was issued. Alternatively the compensation No. is larger than the number of sets in the specifications.
Add the compensation No. command to the compensation command block.
Check the number of compensation No. sets a correct it to a compensation No. command within the permitted number of tool compensation sets.
P171 No spec:Comp input by prog G10 Compensation data input by program (G10) was commanded even though there is no specification of compensation data input by program.
Check the specifications.
P172 G10 L number error (G10 L-No. error) The L address command is not correct when the G10 command is issued.
Check the address L-No. of the G10 command and correct the No.
P173 G10 P number error (G10 compensation error) When the G10 command is issued a compensation No. outside the permitted number of sets in the specifications has been commanded for the compensation No. command.
First check the number of compensation sets and then set the address P designation to within the permitted number of sets.
P174 No spec:Comp input by prog G11 Compensation data input by program cancel (G11) was commanded even though there is no specification of compensation data input by program.
Check the specifications.
P177 Tool life count active Registration of tool life management data with G10 was attempted when the used data count valid signal was ON.
The tool life management data cannot be registered when counting the used data. Turn the used data count valid signal OFF.
P178 Tool life data entry over The number of registration groups total number of registered tools or the number of registrations per group exceeded the specifications range.
Review the number of registrations.
P179 Illegal group No. When registering the tool life management
data with G10 the group No. was commanded in duplicate.
A group No. that was not registered was designated during the T 99 command.
An M code command must be issued as a single command but coexists in the same block as that of another M code command.
The M code commands set in the same group exist in the same block.
The group No. cannot be commanded in duplicate. When registering the group data register it in group units.
Correct to the correct group No.
P180 No spec: Drilling cycle A fixed cycle command was issued though there are not fixed cycle (G72 - G89) specifications.
Check the specifications. Correct the program.
Appendix 6. Alarms 6.3 Program Error
IV - 117
Error No. Details Remedy
P181 No spindle command (Tap cycle) The spindle rotation speed command has not been issued when the fixed cycle for drilling command is given. "S*****" type S command does not exist in the same block with the synchronous tapping cycle.
Issue the spindle rotation speed command (S) when the fixed cycle for drilling command G84 G74 (G84 G88) is given.
Enter "S*****" type S command.
P182 Synchronous tap error Connection to the main spindle unit was not
established. The synchronous tapping was attempted
with the spindle not serially connected under the multiple-spindle control I.
Check connection to the main spindle. Check that the main spindle encoder exists. Set 1 to the parameter #3024 (sout).
P183 No pitch/thread number The pitch or thread number command has not been issued in the tap cycle of a fixed cycle for drilling command.
Specify the pitch data and the number of threads by F or E command.
P184 Pitch/thread number error The pitch or the number of threads per inch
is illegal in the tap cycle of the fixed cycle for drilling command.
The pitch is too small for the spindle rotation speed.
The thread number is too large for the spindle rotation speed.
Check the pitch or the number of threads per inch.
P185 No spec: Sync tapping cycle Synchronous tapping cycle (G84/G74) was commanded even though there is no synchronous tapping cycle specification.
Check the specifications.
P186 Illegal S cmnd in synchro tap S command was issued during synchronous tapping modal.
Cancel the synchronous tapping before issuing the S command.
P190 No spec: Turning cycle A lathe cutting cycle command was input although the lathe cutting cycle was undefined in the specification.
Check the specification. Delete the lathe cutting cycle command.
P191 Taper length error In the lathe cutting cycle the specified length of taper section is illegal.
The radius set value in the lathe cycle command must be smaller than the axis shift amount.
P192 Chamfering error Chamfering in the thread cutting cycle is illegal.
Set a chamfering amount not exceeding the cycle.
P200 No spec: MRC cycle The compound type fixed cycle for turning machining I (G70 to G73) was commanded when the compound type fixed cycle for turning machining I specifications were not provided.
Check the specification.
Appendix 6. Alarms 6.3 Program Error
IV - 118
Error No. Details Remedy
P201 Program error (MRC) When called with a compound type fixed
cycle for turning machining I command, the subprogram contained at least one of the following commands:
Reference position return command (G27, G28, G29, G30)
Thread cutting (G33, G34) Fixed cycle skip-function (G31, G31.n)
The first move block of the finish shape program in compound type fixed cycle for turning machining I contains an arc command.
Delete the following G codes from this subprogram that is called with the compound type fixed cycle for turning machining I commands (G70 to G73): G27 G28 G29, G30 G31 G33 G34, and fixed cycle G codes.
Remove G2 and G3 from the first move block of the finish shape program in compound type fixed cycle for turning machining I.
P202 Block over (MRC) The number of blocks in the shape program of the compound type fixed cycle for turning machining I is over 50 or 200 (this differs according to the model).
Specify 50 or a less value. The number of blocks in the shape program called by the compound type fixed cycle for turning machining I commands (G70 to G73) must be decreased below 50 or 200 (this differs according to the model).
P203 D cmnd figure error (MRC) The compound type fixed cycle for turning machining I (G70 to G73) shape program could not cut the work normally because it defined an abnormal shape.
Check the compound type fixed cycle for turning machining I (G70 to G73) shape program.
P204 E cmnd fixed cycle error A command value of the compound type fixed cycle for turning machining (G70 to G76) is illegal.
Check the compound type fixed cycle for turning machining (G70 to G76) command value.
P210 No spec: Pattern cycle A compound type fixed cycle for turning machining II (G74 to G76) command was input although it was undefined in the specification.
Check the specification.
P220 No spec: Special fixed cycle No special fixed cycle specifications are available.
Check the specifications.
P221 No. of special fixed holes = 0 A 0 has been specified for the number of holes in special fixed cycle mode.
Reconsider the program.
P222 G36 angle error A G36 command specifies 0 for angle intervals.
Reconsider the program.
P223 G12/G13 radius error The radius value specified with a G12 or G13 command is below the compensation amount.
Reconsider the program.
P224 No spec: Circular (G12/G13) There are no circular cutting specifications.
Check the specifications.
Appendix 6. Alarms 6.3 Program Error
IV - 119
Error No. Details Remedy
P230 Subprogram nesting over A subprogram has been called 8 or more
times in succession from the subprogram. The program in the data server contains the
M198 command. The program in the IC card has been called
more than once (the program in the IC card can be called only once at a time).
Check the number of subprogram calls and correct the program so that it does not exceed 8 times.
P231 No sequence No. At subprogram call time the sequence No. set at return from the subprogram or specified by GOTO was not set.
Specify the sequence Nos. in the call block of the subprogram.
P232 No program No. The machining program has not been found
when the machining program is called. The file name of the program registered in
IC card is not corresponding to O No.
Enter the machining program. Check the subprogram storage destination
parameters. Ensure that the external device (including IC
card) that contains the file is mounted. P235 Program editing
Operation was attempted for the file under program editing.
Execute the program again after completion of program editing.
P240 Program editing Operation was attempted for the file under program editing.
Check the specifications.
P241 No variable No. The variable No. commanded is out of the range specified in the specifications.
Check the specifications. Check the program variable No.
P242 = not defined at vrble set The "=" sign has not been commanded when a variable is defined.
Designate the "=" sign in the variable definition of the program.
P243 Can't use variables An invalid variable has been specified in the left or right side of an operation expression.
Correct the program.
P244 Invalid set date or time Date or time was set earlier than current date or time in the system variables (#3011, #3012) when the credit system was valid.
Date or time cannot be changed. Reconsider the program.
P250 No spec: Figure rotation Figure rotation (M98 I_J_P_H_L_) was commanded even though there is no figure rotation specification.
Check the specifications.
P251 Figure rotation overlapped Figure rotation command was issued during figure rotation.
Check the machining program.
P252 Coord rotate in fig. rotation A coordinate rotation related command (G68, G69) was issued during figure rotation.
Reconsider the program.
P260 No spec: Coordinates rotation Even though there were no coordinate rotation specifications, a coordinate rotation command was issued.
Check the specifications.
Appendix 6. Alarms 6.3 Program Error
IV - 120
Error No. Details Remedy
P270 No spec: User macro A macro specification was commanded though there are no such command specifications.
Check the specifications.
P271 No spec: Macro interrupt A macro interruption command has been issued though it is not included in the specifications.
Check the specifications.
P272 NC and macro texts in a block A statement and a macro statement exist together in the same block.
Reconsider the program and place the executable statement and macro statement in separate blocks.
P273 Macro call nesting over The number of macro call nests exceeded the specifications.
Reconsider the program and correct it so that the macro calls do not exceed the limit imposed by the specification.
P275 Macro argument over The number of macro call argument type II sets has exceeded the limit.
Reconsider the program.
P276 Illegal G67 command A G67 command was issued though it was not during the G66 command modal.
Reconsider the program. The G67 command is the call cancel
command and so the G66 command must be designated first before it is issued.
P277 Macro alarm message An alarm command has been issued in #3000.
Refer to the operator messages on the DIAG screen.
Refer to the instruction manual issued by the machine tool builder.
P280 Brackets [ ] nesting over The number of parentheses "[" or "]" which can be commanded in a single block has exceeded five.
Reconsider the program and correct it so the number of "[" or "]" is five or less.
P281 Brackets [ ] not paired The number of "[" and "]" parentheses commanded in a single block does not match.
Reconsider the program and correct it so that "[" and "]" parentheses are paired up properly.
P282 Calculation impossible The arithmetic formula is incorrect.
Reconsider the program and correct the formula.
P283 Divided by zero The denominator of the division is zero.
Reconsider the program and correct it so that the denominator for division in the formula is not zero.
P290 IF sentence error There is an error in the IF conditional GOTO statement.
Reconsider the program.
P291 WHILE sentence error There is an error in the WHILE conditional DO -END statement.
Reconsider the program.
P292 SETVN sentence error There is an error in the SETVN statement when the variable name setting was made.
Reconsider the program. The number of characters in the variable
name of the SETVN statement must be 7 or less.
P293 DO-END nesting over The number of DO-END nesting levels in WHILE conditional DO -END statement has exceeded 27.
Reconsider the program and correct it so that the nesting levels of the DO - END statement does not exceed 27.
Appendix 6. Alarms 6.3 Program Error
IV - 121
Error No. Details Remedy
P294 DO and END not paired The DO's and END's are not paired off properly.
Reconsider the program and correct it so that the DO's and END's are paired off properly.
P295 WHILE/GOTO in tape There is a WHILE or GOTO statement on the tape during tape operation.
During tape operation a program which includes a WHILE or GOTO statement cannot be executed and so the memory operation mode is established instead.
P296 No address (macro) A required address has not been specified in the user macro.
Review the program.
P297 Address-A error The user macro does not use address A as a variable.
Review the program.
P298 G200-G202 cmnd in tape User macro G200 G201 or G202 was specified during tape or MDI mode.
Review the program.
P300 Variable name illegal The variable names have not been commanded properly.
Reconsider the variable names in the program and correct them.
P301 Variable name duplicated The name of the variable has been duplicated.
Correct the program so that the name is not duplicated.
P310 Not use GMSTB macro code G, M, S, T, or B macro code was called during fixed cycle.
Review the program. Review the parameter.
P350 No spec: Scaling command The scaling command (G50, G51) was issued when the scaling specifications were not available.
Check the specifications.
P360 No spec: Program mirror A mirror image (G50.1 or G51.1) command has been issued though the programmable mirror image specifications are not provided.
Check the specifications.
P370 No spec: Facing t-post MR The facing turret mirror image specifications are not provided.
Check the specifications.
P371 Facing t-post MR illegal Mirror image for facing tool posts was commanded to an axis for which external mirror image or parameter mirror image is valid. Mirror image for facing tool posts validating mirror image for a rotary axis was commanded.
Check the program. Check the parameters.
P380 No spec: Corner R/C The corner R/C was issued when the corner R/C specifications were not available.
Check the specifications. Remove the corner chamfering/corner
rounding command from the program.
Appendix 6. Alarms 6.3 Program Error
IV - 122
Error No. Details Remedy
P381 No spec: Arc R/C Corner chamfering II /corner rounding II was specified in the arc interpolation block although corner chamfering/corner rounding II is unsupported.
Check the specifications.
P382 No corner movement The block next to corner chamfering/ corner rounding is not a movement command.
Replace the block succeeding the corner chamfering/corner rounding command by G01 command.
P383 Corner movement short In the corner chamfering/corner rounding command the movement distance was shorter than the value in the corner chamfering/corner rounding command.
Make the corner chamfering/corner rounding less than the movement distance since this distance is shorter than the corner chamfering/ corner rounding.
P384 Corner next movement short When the corner chamfering/corner rounding command was input the movement distance in the following block was shorter than the length of the corner chamfering/corner rounding.
Make the corner chamfering/corner rounding less than the movement distance since this distance in the following block is shorter than the corner chamfering/corner rounding.
P385 Corner during G00/G33 A block with corner chamfering/corner rounding was given during G00 or G33 modal.
Recheck the program.
P390 No spec: Geometric A geometric command was issued though there are no geometric specifications.
Check the specifications.
P391 No spec: Geometric arc There are no geometric IB specifications.
Check the specifications.
P392 Angle < 1 degree (GEOMT) The angular difference between the geometric line and line is 1 or less.
Correct the geometric angle.
P393 Inc value in 2nd block (GEOMT) The second geometric block was specified by an incremental value.
Specify this block by an absolute value.
P394 No linear move command (GEOMT) The second geometric block contains no linear command.
Specify the G01 command.
P395 Illegal address (GEOMT) The geometric format is invalid.
Recheck the program.
P396 Plane selected in GEOMT ctrl A plane switching command was executed during geometric command processing.
Execute the plane switching command before geometric command processing.
P397 Arc error (GEOMT) In geometric IB the circular arc end point does not contact or cross the next block start point.
Recheck the geometric circular arc command and the preceding and following commands.
P398 No spec: Geometric1B Although the geometric IB specifications are not included a geometric command is given.
Check the specifications.
Appendix 6. Alarms 6.3 Program Error
IV - 123
Error No. Details Remedy
P411 Illegal modal G111 G111 was issued during milling mode. G111 was issued during nose R
compensation mode. G111 was issued during constant surface
speed. G111 was issued during mixed
synchronization control. G111 was issued during fixed cycle. G111 was issued during polar coordinate
interpolation. G111 was issued during cylindrical
interpolation mode.
Before commanding G111, cancel the following commands. Milling mode Nose R compensation Constant surface speed Mixed synchronization control Fixed cycle Polar coordinate interpolation Cylindrical interpolation
P412 P412 No spec: Axis name switch Axis name switch (G111) was issued even though there is no axis name switch (G111) specification.
Check the specifications.
P420 No spec: Para input by program Parameter input by program (G10) was commanded even though there is no specification of parameter input by program.
Check the specifications.
P421 Parameter input error The specified parameter No. or set data is
illegal. An illegal G command address was input in
parameter input mode. A parameter input command was input
during fixed cycle modal or nose R compensation.
G10L50, G10L70, G11 were not commanded in independent blocks.
Check the program.
P430 R-pnt return incomplete A command was issued to move an axis
which has not returned to the reference position away from that reference position.
A command was issued to an axis removal axis.
Execute reference position return manually. The command was issued to an axis for
which axis removal is validated so invalidate axis removal.
P431 No spec: 2,3,4th R-point ret A command for second third or fourth reference position return was issued though there are no such command specifications.
Check the specifications.
P432 No spec: Start position return Start position return (G29) was commanded even though there is no start position return specification.
Check the specifications.
P433 No spec: R-position check Reference position check (G27) was commanded even though there is no reference position check specification.
Check the specifications.
Appendix 6. Alarms 6.3 Program Error
IV - 124
Error No. Details Remedy
P434 Compare error One of the axes did not return to the reference position when the reference position check command (G27) was executed.
Check the program.
P435 G27 and M commands in a block An M command was issued simultaneously in the G27 command block.
An M code command cannot be issued in a G27 command block and so the G27 command and M code command must be placed in separate blocks.
P436 G29 and M commands in a block An M command was issued simultaneously in the G29 command block.
An M code command cannot be issued in a G29 command block and so the G29 command and M code command must be placed in separate blocks.
P438
G52 invalid during G54.1 A local coordinate system command was issued during execution of the G54.1 command.
Review the program.
P450 No spec: Chuck barrier The chuck barrier on command (G22) was specified although the chuck barrier was undefined in the specification.
Check the specification.
P451 No spec: Stroke chk bef travel Stroke check before travel (G22/G23) was commanded even though there is no stroke check before travel specification.
Check the specification.
P452 Limit before travel exists An illegal command such as the start or end point of the traveling axis is inside the prohibited area or the axis passes through the prohibited area, was detected when Stroke check before travel (G22) was ON.
Review the coordinate values of the axis address commanded in the program.
P460 Tape I/O error An error has arisen in the tape reader or alternatively in the printer during macro printing.
Check the power and cable of the connected devices.
Check the I/O device parameters.
P461 File I/O error A file of the machining program cannot be read. IC card has not been inserted.
In memory mode, the programs stored in memory may have been destroyed. Output all of the programs and tool data once and format them.
Ensure that the external device (including an IC card, etc) that contains the file is mounted.
Check the parameters for HD operation or IC card operation.
P462 Computer link commu error A communication error occurred during the BTR operation.
"L01 Computer link error" is displayed simultaneously, so remedy the problem according to the error No.
P480 No spec: Milling Milling was commanded when the milling
specifications were not provided. Polar coordinate interpolation was
commanded when the polar coordinate interpolation specifications were not provided.
Check the specification.
Appendix 6. Alarms 6.3 Program Error
IV - 125
Error No. Details Remedy
P481 Illegal G code (mill) An illegal G code was used during the
milling mode. An illegal G code was used during
cylindrical interpolation or polar coordinate interpolation.
The G07.1 command was issued during the tool radius compensation.
Check the program.
P482 Illegal axis (mill) A rotary axis was commanded during the
milling mode. Milling was executed even though an illegal
value was set for the milling axis No. Cylindrical interpolation or polar coordinate
interpolation was commanded during mirror image.
Cylindrical interpolation or polar coordinate interpolation was commanded before the tool compensation was completed after the T command.
G07.1 was commanded when cylindrical interpolation was not possible (there is no rotary axis, or external mirror image is ON).
An axis other than a cylindrical coordinate system axis was commanded during cylindrical interpolation.
Check the machining program, parameters and PLC I/F signal.
P484 R-pnt ret incomplete (mill) Movement was commanded to an axis that
had not completed reference position return during the milling mode.
Movement was commanded to an axis that had not completed reference position return during cylindrical interpolation or polar coordinate interpolation.
Carry out manual reference position return.
Appendix 6. Alarms 6.3 Program Error
IV - 126
Error No. Details Remedy
P485 Illegal modal (mill) The milling mode was turned ON during
nose R compensation or constant surface speed control.
A T command was issued during the milling mode.
The mode was switched from milling to cutting during tool compensation.
Cylindrical interpolation or polar coordinate interpolation was commanded during the constant surface speed control mode (G96).
The command unacceptable in the cylindrical interpolation was issued.
A T command was issued during the cylindrical interpolation or polar coordinate interpolation mode.
A movement command was issued when the plane was not selected just before or after the G07.1 command.
A plane selection command was issued during the polar coordinate interpolation mode.
Cylindrical interpolation or polar coordinate interpolation was commanded during tool radius compensation.
The G16 plane in which the radius value of a cylinder is 0 was specified.
A cylindrical interpolation or polar coordinate interpolation command was issued during coordinate rotation by program (G68).
Check the program. Before issuing G12.1, issue G40 or G97. Before issuing G12.1, issue a T command. Before issuing G13.1, issue G40. Specify the radius value of a cylinder other
than 0, or specify the X axis's current value other than 0 before issuing G12.1/G16.
P486 Milling error The milling command was issued during the
mirror image (when parameter or external input is turned ON).
Polar coordinate interpolation, cylindrical interpolation or milling interpolation was commanded during mirror image for facing tool posts.
The start command of the cylindrical interpolation or polar coordinate interpolation was issued during the normal line control.
Check the program.
P511 Synchronization M code error Two or more synchronization M codes were
commanded in the same block. The synchronization M code and "!" code
were commanded in the same block. Synchronization with the M code was
commanded in 3rd part system or more. (Synchronization with the M code is valid only in 1st part system or 2nd part system.)
Check the program.
P550 No spec: G06.2(NURBS) There is no NURBS interpolation option.
Check the specifications.
Appendix 6. Alarms 6.3 Program Error
IV - 127
Error No. Details Remedy
P551 G06.2 knot error The knot (k) command value is smaller than the value for the previous block.
Reconsider the program. Specify the knot by monotone increment.
P552 Start point of 1st G06.2 err The block end point immediately before the G06.2 command and the G06.2 first block command value do not match.
Match the G06.2 first block coordinate command value with the previous block end point.
P554 Invld manual interrupt in G6.2 Manual interruption using a block was performed while in G06.2 mode.
Perform for blocks other than G06.2 mode when manually interrupting.
P555 Invalid restart during G06.2 Restart was attempted from the block in G06.2 mode.
Restart from the block other than in G06.2 mode.
P600 No spec: Auto TLM An automatic tool length measurement command (G37) was execute though there are no such command specifications.
Check the specifications.
P601 No spec: Skip A skip command (G31) was issued though there are no such command specifications.
Check the specifications.
P602 No spec: Multi skip A multiple skip command (G31.1 G31.2 or G31.3) was issued though there are no such command specifications.
Check the specifications.
P603 Skip speed 0 The skip speed is 0.
Specify the skip speed.
P604 TLM illegal axis No axis or more than one axis was specified in the automatic tool length measurement block.
Specify only one axis.
P605 T & TLM command in a block The T code is in the same block as the automatic tool length measurement block.
Specify this T code before the block.
P606 T cmnd not found before TLM The T code was not yet specified in automatic tool length measurement.
Specify this T code before the block.
P607 TLM illegal signal Before the area specified by the D command or decelerating area parameter d the measurement position arrival signal went ON. The signal remains OFF to the end.
Check the program.
P608 Skip during radius compen A skip command was specified during radius compensation processing.
Specify a radius compensation cancel (G40) command or remove the skip command.
P610 Illegal parameter The parameter setting is not correct. G114.1 was commanded when the spindle
synchronization with PLC I/F command was selected.
G113 was commanded when the spindle-spindle polygon machining option was OFF and the spindle synchronization with PLC I/F command was selected.
Check whether "#1549 Iv0vR1" to "#1553 Iv0vR5" are set in descending order (in order of large values).
Check whether "#1554 Iv0rd2" to "#1557 Iv0rd5" are set in descending order.
Check and correct "#1514 expLinax" and "#1515 expRotax".
Check the program. Check the parameter.
Appendix 6. Alarms 6.3 Program Error
IV - 128
Error No. Details Remedy
P611 No spec: Exponential function Specification for exponential interpolation is not available.
Check the specification.
P612 Exponential function error A movement command for exponential interpolation was issued during mirror image for facing tool posts.
Check the program.
P700 Illegal command value Spindle synchronization was commanded to a spindle that is not connected serially.
Check the program. Check the parameter.
P900 No spec: Normal line control A normal line control command (G40.1, G41.1, G42.1) was issued when the normal line control specifications were not provided.
Check the specifications.
P901 Normal line control axis G92 A coordinate system preset command (G92) was issued to a normal line control axis during normal line control.
Check the program.
P902 Normal line control axis error The normal line control axis was set to a
linear axis. The normal line control axis was set to the
linear type rotary axis II axis. The normal line control axis has not been
set. The normal line control axis was the same
as the plane selection axis.
Correct the normal line control axis.
P903 Plane chg in Normal line ctrl The plane selection command (G17, G18, G19) was issued during normal line control.
Delete the plane selection command (G17, G18, G19) from the program for normal line control.
P920 No spec: 3D coord conv There is no specification for 3-dimensional coordinate conversion.
Check the specifications.
P921 Illegal G code at 3D coord A G code command that cannot be performed was made during 3-dimensional coordinate conversion modal.
Refer to "Mitsubishi CNC 700/70 Series Programming Instruction Manual (Machining Center Series)" for further details of usable G commands.
When the basic specification parameter "#1229 set01/bit3" is ON, turn the parameter OFF or specify the constant surface speed control cancel (G97).
P922 Illegal mode at 3D coord A 3-dimensional coordinate conversion command was issued during a modal for which 3-dimensional coordinate conversion cannot be performed.
Refer to "Mitsubishi CNC 700/70 Series Programming Instruction Manual (Machining Center Series)" for further details of usable G commands.
P923 Illegal addr in 3D coord blk A G code for which G68 to combination could not be performed was specified for the same block.
Refer to "Mitsubishi CNC 700/70 Series Programming Instruction Manual (Machining Center Series)" for further details of usable G commands.
Appendix 6. Alarms 6.3 Program Error
IV - 129
Error No. Details Remedy
P930 No spec: Tool axis compen A tool length compensation along the tool axis command was issued even though there is no tool length compensation along the tool axis specification.
Check the specifications.
P931 Executing tool axis compen A G code that cannot be commanded exists during tool length compensation along the tool axis.
Reconsider the program.
P932 Rot axis parameter error There is a mistake in the linear axis name and rotary axis name in the rotary axis configuration parameters.
Set the correct value and reboot.
P940 No spec: Tool tip control There is no tool tip center control specification.
Check the specifications.
P941 Invalid T tip control command A tool tip center control command was issued during a modal for which a tool tip center control command cannot be issued.
Reconsider the program.
P942 Invalid cmnd during T tip ctrl A G code that cannot be commanded was issued during tool tip center control.
Reconsider the program.
P943 Tool posture command illegal In the case of tool tip center control type 1, if the signs at the tool-side rotary axis or table base-side rotary axis start and finish points differ, a tool base-side rotary axis or table workpiece-side rotary axis rotation exists for the same block, and does not pass a singular point. In the case of tool tip center control type 2, the posture vector command is incorrect.
Reconsider the program.
P990 PREPRO error Combining commands that required pre-reading (nose R offset corner chamfering/corner rounding geometric I geometric IB and compound type fixed cycle for turning machining) resulted in eight or more pre-read blocks.
Reduce the number of commands that require pre-reading or delete such commands.
Appendix 7. G Code Guidance Display List
IV - 130
Appendix 7. G Code Guidance Display List
O: Modal, : Unmodal G code Group Function Modal
00 01 Positioning O 01 01 Linear interpolation O 02 01 Circular interpolation CW (clockwise) /
Spiral/Conical interpolation CW (type2) O
03 01 Circular interpolation CCW (counterclockwise) / Spiral/Conical interpolation CCW (type2) O
02.1 01 Spiral/Conical interpolation CW (type1) O 03.1 01 Spiral/Conical interpolation CCW (type1) O 02.3 01 Exponential function interpolation positive rotation O 03.3 01 Exponential function interpolation negative rotation O 02.4 01 3-dimensional circular interpolation O 03.4 01 3-dimensional circular interpolation O 04 00 Dwell 05 00 High-speed high-accuracy control II/High-speed machining
mode O
05.1 00 High-speed high-accuracy control I/Spline O 06.2 01 NURBS interpolation O 07 00 Hypothetical axis interpolation O
07.1 107 21 Cylindrical interpolation O
08 00 High-accuracy control 1 O 09 00 Exact stop check 10 00 Program data input (parameter /compensation data/parameter
coordinate rotation data) -
11 00 Program data input cancel - 12 00 Circular cut CW (clockwise) 13 00 Circular cut CCW (counterclockwise)
12.1 112 21 Polar coordinate interpolation ON O
13.1 113 21 Polar coordinate interpolation cancel -
15 18 Polar coordinate command OFF - 16 18 Polar coordinate command ON O 17 02 Plane selection X-Y O 18 02 Plane selection Z-X O 19 02 Plane selection Y-Z O 20 06 Inch command O 21 06 Metric command O 22 04 Stroke check before travel ON - 23 04 Stroke check before travel cancel - 27 00 Reference position check 28 00 Reference position return 29 00 Start position return 30 00 2nd to 4th reference position return
30.1 00 Tool change position return 1 30.2 00 Tool change position return 2 30.3 00 Tool change position return 3 30.4 00 Tool change position return 4 30.5 00 Tool change position return 5 30.6 00 Tool change position return 6
Appendix 7. G Code Guidance Display List
IV - 131
O: Modal, : Unmodal
G code Group Function Modal 31 00 Skip/Multi-step skip function 2
31.1 00 Multi-step skip function 1-1 31.2 00 Multi-step skip function 1-2 31.3 00 Multi-step skip function 1-3 33 01 Thread cutting O 34 00 Special fixed cycle (bolt hole circle) 35 00 Special fixed cycle (line at angle) 36 00 Special fixed cycle (arc) 37 00 Automatic tool length measurement
37.1 00 Special fixed cycle (grid) 38 00 Tool radius compensation vector designation 39 00 Tool radius compensation corner arc 40 07 Tool radius compensation cancel /
3-dimentional tool radius compensation cancel -
41 07 Tool radius compensation left / 3-dimentional tool radius compensation left O
42 07 Tool radius compensation right / 3-dimentional tool radius compensation right O
40.1 15 Normal line control cancel - 41.1 15 Normal line control left ON O 42.1 15 Normal line control right ON O 43 08 Tool length compensation (+) O 44 08 Tool length compensation (-) O
43.1 08 Tool length compensation along the tool axis O 43.4 08 Tool center point control type 1 O 43.5 08 Tool center point control type 2 O 45 00 Tool position offset (extension) 46 00 Tool position offset (reduction) 47 00 Tool position offset (doubled) 48 00 Tool position offset (halved) 49 08 Tool length compensation cancel/Tool center point control
cancel -
50 11 Scaling cancel - 51 11 Scaling ON O
50.1 19 G command mirror image cancel - 51.1 19 G command mirror image ON O 52 00 Local coordinate system setting O 53 00 Basic machine coordinate system selection 54 12 Workpiece coordinate system 1 selection O 55 12 Workpiece coordinate system 2 selection O 56 12 Workpiece coordinate system 3 selection O 57 12 Workpiece coordinate system 4 selection O 58 12 Workpiece coordinate system 5 selection O 59 12 Workpiece coordinate system 6 selection O
54.1 12 Workpiece coordinate system selection 48 / 96 sets extended O 60 00 Unidirectional positioning 61 13 Exact stop check mode O
61.1 13 High-accuracy control 1 ON O 61.2 13 High-accuracy spline interpolation O 62 13 Automatic corner override O 63 13 Tapping mode O
63.1 13 Synchronous tapping mode (normal tapping) O 63.2 13 Synchronous tapping mode (reverse tapping) O
Appendix 7. G Code Guidance Display List
IV - 132
O: Modal, : Unmodal
G code Group Function Modal 64 13 Cutting mode O 65 00 User macro call 66 14 User macro modal call A O
66.1 14 User macro modal call B O 67 14 User macro modal call cancel - 68 16 Programmable coordinate rotation mode ON/3-dimensional
coordinate conversion mode ON O
69 16 Programmable coordinate rotation mode OFF/3-dimensional coordinate conversion mode OFF
-
73 09 Fixed cycle (step) O 74 09 Fixed cycle (reverse tap) O 75 09 Fixed cycle (circle cutting cycle) O 76 09 Fixed cycle (fine boring) O 80 09 Fixed cycle cancel - 81 09 Fixed cycle (drill/spot drill) O 82 09 Fixed cycle (drill/counter boring) O 83 09 Fixed cycle (deep drilling) O 84 09 Fixed cycle (tapping) O 85 09 Fixed cycle (boring) O 86 09 Fixed cycle (boring) O 87 09 Fixed cycle (back boring) O 88 09 Fixed cycle (boring) O 89 09 Fixed cycle (boring) O 90 03 Absolute value command O 91 03 Incremental command value O 92 00 Coordinate system setting O
92.1 00 Workpiece coordinate system pre-setting 93 05 Inverse time feed O 94 05 Per-minute feed (Asynchronous feed) O 95 05 Per-revolution feed (Synchronous feed) O 96 17 Constant surface speed control ON O 97 17 Constant surface speed control OFF - 98 10 Fixed cycle Initial level return O 99 10 Fixed cycle R point level return O
Appendix 7. G Code Guidance Display List
IV - 133
O: Modal, : Unmodal G code list
2 3 4 5 6 7 Group Function Modal
G00 G00 G00 G00 G00 G00 01 Positioning O G01 G01 G01 G01 G01 G01 01 Linear interpolation O
G02 G02 G02 G02 G02 G02 01 Circular interpolation CW / Helical interpolation CW O
G03 G03 G03 G03 G03 G03 01 Circular interpolation CCW / Helical interpolation CCW O
G02.3 G02.3 G02.3 G02.3 G02.3 G02.3 01 Exponential interpolation CW O G03.3 G03.3 G03.3 G03.3 G03.3 G03.3 01 Exponential interpolation CCW O G04 G04 G04 G04 G04 G04 00 Dwell
G07.1 G107
G07.1 G107 19 Cylindrical interpolation O
G09 G09 G09 G09 G09 G09 00 Exact stop check
G10 G10 G10 G10 G10 G10 00 Parameter/Compensation data input by program/ Tool life management data registration
-
G11 G11 G11 G11 G11 G11 00 Program parameter input / Tool life management data registration mode cancel
-
G12.1 G112
G12.1 G112 19 Polar coordinate interpolation ON O
G13.1 G113
G13.1 G113 19 Polar coordinate interpolation cancel -
G12.1 G12.1 G12.1 G12.1 19 Milling interpolation ON O G13.1 G13.1 G13.1 G13.1 19 Milling interpolation cancel - G14 G14 G14 G14 18 Balance cut OFF - G15 G15 G15 G15 18 Balance cut ON O
G16 G16 G16 G16 02 Milling interpolation plane selection Y-Z cylindrical plane O
G17 G17 G17 G17 G17 G17 02 Plane selection X-Y O G18 G18 G18 G18 G18 G18 02 Plane selection Z-X O G19 G19 G19 G19 G19 G19 02 Plane selection Y-Z O G20 G20 G20 G20 G20 G20 06 Inch command O G21 G21 G21 G21 G21 G21 06 Metric command O G22 G22 G22 G22 04 Barrier check ON O G23 G23 G23 G23 04 Barrier check OFF -
G22 G22 00 Soft limit ON G23 G23 00 Soft limit OFF -
G27 G27 G27 G27 G27 G27 00 Reference position return check G28 G28 G28 G28 G28 G28 00 Automatic reference position return G29 G29 G29 G29 G29 G29 00 Return from reference position G30 G30 G30 G30 G30 G30 00 2nd, 3rd and 4th reference position return
G30.1 G30.1 G30.1 G30.1 G30.1 G30.1 00 Tool change position return 1 G30.2 G30.2 G30.2 G30.2 00 Tool change position return 2 G30.3 G30.3 G30.3 G30.3 00 Tool change position return 3 G30.4 G30.4 G30.4 G30.4 00 Tool change position return 4 G30.5 G30.5 G30.5 G30.5 00 Tool change position return 5 G31 G31 G31 G31 G31 G31 00 Skip function/Multiple-step skip function 2
Appendix 7. G Code Guidance Display List
IV - 134
O: Modal, : Unmodal
G code list 2 3 4 5 6 7
Group Function Modal
G31.1 G31.1 G31.1 G31.1 G31.1 G31.1 00 Multiple-step skip function 1-1 G31.2 G31.2 G31.2 G31.2 G31.2 G31.2 00 Multiple-step skip function 1-2 G31.3 G31.3 G31.3 G31.3 G31.3 G31.3 00 Multiple-step skip function 1-3 G32 G33 G32 G33 G32 G33 01 Thread cutting O G34 G34 G34 G34 G34 G34 01 Variable lead thread cutting O G35 G35 G35 G35 G35 G35 01 Circular thread cutting CW O G36 G36 G36 G36 G36 G36 01 Circular thread cutting CCW O
G37 G37 G36/G3 7
G36/G3 7
G36/G3 7
G37.1 G37.2
G36/G3 7
G37.1 G37.2
00 Automatic tool length measurement
G40 G40 G40 G40 G40 G40 07 Tool nose R compensation cancel - G41 G41 G41 G41 G41 G41 07 Tool nose R compensation left O G42 G42 G42 G42 G42 G42 07 Tool nose R compensation right O
G46 G46 G46 G46 G46 G46 07 Tool nose R compensation (direction automatically selected) ON O
G43.1 G43.1 G43.1 G43.1 G43.1 G43.1 20 1st spindle control mode O G44.1 G44.1 G44.1 G44.1 G44.1 G44.1 20 Selected spindle control mode O G47.1 G47.1 G47.1 G47.1 G47.1 G47.1 20 All spindles simultaneous control mode O
G50 G92 G50 G92 G50 G92 00 Coordinate system setting/Spindle clamp speed setting O
G50.2 G50.2 G50.2 G50.2 11 Scaling cancel - G51.2 G51.2 G51.2 G51.2 11 Scaling ON O
G50.2 G250
G50.2 G250 00 Polygon machining mode cancel
(spindle-tool axis synchronization) -
G51.2 G251
G51.2 G251 00 Polygon machining mode ON
(spindle-tool axis synchronization)
G52 G52 G52 G52 G52 G52 00 Local coordinate system setting O
G53 G53 G53 G53 G53 G53 00 Basic machine coordinate system selection
G54 G54 G54 G54 G54 G54 12 Workpiece coordinate system selection 1 O G55 G55 G55 G55 G55 G55 12 Workpiece coordinate system selection 2 O G56 G56 G56 G56 G56 G56 12 Workpiece coordinate system selection 3 O G57 G57 G57 G57 G57 G57 12 Workpiece coordinate system selection 4 O G58 G58 G58 G58 G58 G58 12 Workpiece coordinate system selection 5 O G59 G59 G59 G59 G59 G59 12 Workpiece coordinate system selection 6 O
G54.1 G54.1 G54.1 G54.1 G54.1 G54.1 12 Workpiece coordinate system 48 sets expanded O
G61 G61 G61 G61 G61 G61 13 Exact stop check mode O G62 G62 G62 G62 G62 G62 13 Automatic corner override O
G63 G63 G63 G63 G63 G63 13/1 9 Tapping mode O
G64 G64 G64 G64 G64 G64 13/1 9 Cutting mode O
G65 G65 G65 G65 G65 G65 00 User macro call G66 G66 G66 G66 G66 G66 14 User macro modal call A O
G66.1 G66.1 G66.1 G66.1 G66.1 G66.1 14 User macro modal call B O G67 G67 G67 G67 G67 G67 14 User macro modal call cancel -
Appendix 7. G Code Guidance Display List
IV - 135
O: Modal, : Unmodal
G code list 2 3 4 5 6 7
Group Function Modal
G68 G68 G68 G68 15 Mirror image for facing tool posts ON O G69 G69 G69 G69 15 Mirror image for facing tool posts OFF -
G68 G68 15 Mirror image for facing tool posts ON or balance cut mode ON O
G69 G69 15 Mirror image for facing tool posts OFF or balance cut mode cancel -
G70 G70 G70 G70 G70 G70 09 Finishing cycle O G71 G71 G71 G71 G71 G71 09 Longitudinal rough cutting cycle O G72 G72 G72 G72 G72 G72 09 Face rough cutting cycle O G73 G73 G73 G73 G73 G73 09 Formed material rough cutting cycle O G74 G74 G74 G74 G74 G74 09 Face cut-off cycle O G75 G75 G75 G75 G75 G75 09 Longitudinal cut-off cycle O G76 G76 G76 G76 G76 G76 09 Compound thread cutting cycle O
G76.1 G76.1 G76.1 G76.1 G76.1 G76.1 09 2-part system synchronous thread-cutting cycle (1) O
G76.2 G76.2 G76.2 G76.2 G76.2 G76.2 09 2-part system synchronous thread-cutting cycle (2) O
G90 G77 G90 G77 G90 G77 09 Longitudinal cutting fixed cycle O G92 G78 G92 G78 G92 G78 09 Thread cutting fixed cycle O G94 G79 G94 G79 G94 G79 09 Face cutting fixed cycle O G80 G80 G80 G80 G80 G80 09 Fixed cycle for drilling cancel - G81 G81 G81 G81 G81 G81 09 Fixed cycle (drill/spot drilling) O G82 G82 G82 G82 G82 G82 09 Fixed cycle (drill/counter boring) O G79 G83.2 G79 G83.2 G79 G83.2 09 Deep hole drilling cycle 2 O
G83 G83 G83 G83 G83 G83 09 Deep hole drilling cycle (Z axis)/ Small-diameter deep-hole drilling cycle O
G83.1 G83.1 G83.1 G83.1 G83.1 G83.1 09 Stepping cycle O G84 G84 G84 G84 G84 G84 09 Tap cycle (Z axis) O G85 G85 G85 G85 G85 G85 09 Boring cycle (Z axis) O G87 G87 G87 G87 G87 G87 09 Deep hole drilling cycle (X axis) O G88 G88 G88 G88 G88 G88 09 Tap cycle (X axis) O G89 G89 G89 G89 G89 G89 09 Boring cycle (X axis) O
G84.1 G84.1 G84.1 G84.1 G84.1 G84.1 09 Reverse tap cycle (Z axis) O G84.2 G84.2 G84.2 G84.2 G84.2 G84.2 09 Synchronous tapping cycle O G88.1 G88.1 G88.1 G88.1 G88.1 G88.1 09 Reverse tap cycle (X axis) O G50.3 G92.1 G50.3 G92.1 G50.3 G92.1 00 Workpiece coordinate preset G96 G96 G96 G96 G96 G96 17 Constant surface speed control ON O G97 G97 G97 G97 G97 G97 17 Constant surface speed control OFF - G98 G94 G98 G94 G98 G94 05 Feed per minute (Asynchronous feed) O G99 G95 G99 G95 G99 G95 05 Feed per revolution (Synchronous feed) O G90 G90 G90 03 Absolute value command O G91 G91 G91 03 Incremental value command O G98 G98 G98 10 Fixed cycle initial return O G99 G99 G99 10 Fixed cycle R point return O
Appendix 7. G Code Guidance Display List
IV - 136
O: Modal, : Unmodal
G code list 2 3 4 5 6 7
Group Function Modal
G113 G113 G113 G113 00 Spindle synchronization polygon machining cancel (spindle-spindle synchronization) mode cancel
-
G114.1 G114.1 G114.1 G114.1 00 Spindle synchronization
G114.2 G114.2 G114.2 G114.2 00 Polygon machining (spindle-spindle synchronization) mode ON
G114.3 G114.3 G114.3 G114.3 00 Tool spindle synchronization II (Hobbing)
G115 G115 G115 G115 G115 G115 00 Start point designation synchronization Type 1
G116 G116 G116 G116 G116 G116 00 Start point designation synchronization Type 2
G117 G117 G117 G117 G117 G117 00 Miscellaneous function output during axis movement
Appendix 8. IP Address Resetting Procedure at Disabled Network Communication 8.1 Connectable Control Unit IP Address List Screen
IV - 137
Appendix 8. IP Address Resetting Procedure at Disabled Network Communication [700 Series Only]
8.1 Connectable Control Unit IP Address List Screen
After NC starts, when the communication between the control unit and the display unit cannot be established even after the time-out time passes, the connectable control unit IP address list screen appears. The contents of IP address list screen is displayed in English. If no IP address is displayed, check if there are any loose or disconnected cable, hardware breakdown, etc.
(2)
(3)
(4)
(5)
(1)
Display items
Display item Details (1) Connect NC address This displays IP address of the connection destination control unit. (2) PC IP address
PC Subnet PC Gateway
This displays IP address, subnet mask, gateway settings.
(3) IP address This displays IP address of the connectable control unit. (4) System Version This displays system version of the connectable control unit. (5) Serial No. This displays serial No. of the connectable control unit.
(Note 1) For (3), (4) and (5), up to ten lines are displayed at a time. When the display item exceeds ten lines,
the following lines can be displayed with the Page down key.
Appendix 8. IP Address Resetting Procedure at Disabled Network Communication 8.2 Resetting Procedure
IV - 138
8.2 Resetting Procedure
Operation method
(1) Select IP address of the connection destination control unit by , , Page up , Page down keys from IP address list, and press the INPUT key.
The dialog which notifies the change of the network setting is displayed as follows.
To establish the communication between the selected control unit and the display unit, the Ethernet parameter is temporarily changed.
(2) Press the INPUT key.
After a while, the NC screen is displayed. (If the NC screen is not displayed, remove the control unit from external network, and carry out the procedure (1) again.) (Note) In the step, the communication between the
control unit and the display unit is temporarily established. Therefore, unless the parameter is reset (in the procedure (3)), the system will be returned to the state of procedure (1) at the next NC startup.
(3) Set the Ethernet parameter by referring to the
following example of the network connection, and restart NC.
LAN
Operation panel I/O unit #1934 Local IP address (=Connect NC address (Note 1))
Control unit #1926 Global IP address
Display unit #11005 PC IP address
Host PC
The NC screen is normally displayed.
(Note 1) "Connect NC address" is the same as the setting of "[HOSTS] TCP1" in setting file "melcfg.ini". The setting file "melcfg.ini" is in the following directory. C:WINDOWSmelcfg.ini ncsysmelcfg.ini
(Note 2) When the control unit is added in user's network environment, match and change the parameters "#1926(PR) Global IP address", "#1927(PR) Global Subnet mask" and "#1928(PR) Global Gateway" to the user environment. Normally, the parameters "#1934 Local IP address", "#1935 Local Subnet mask" and "Connect NC address" need not be changed from the default setting value.
Appendix 8. IP Address Resetting Procedure at Disabled Network Communication 8.3 Message
IV - 139
8.3 Message The following messages display when IP address is reset.
Message Details Searching The system is searching the connectable NC control unit to establish
the communication between the control unit and the display unit. Please wait until the search is completed.
Socket error The system could not find the connectable control unit because of the network interference. Turn OFF the NC power supply, and review the wiring for the network connection.
Setting error - Connect NC address
The automatic connection with the control unit failed because the setting file to set and save the unit's IP address was not found/is read-only/has illegal format. Review "[HOSTS] TCP1" setting in the setting file "melcfg.ini".
Searching IP address The system is automatically searching the appropriate IP address because IP address of the display unit is inapposite. Please wait until the search is completed.
Review the setting of the Ethernet parameter after the screen starts.
The IP address setting of connected control unit and display unit was completed. Please review the setting of the Ethernet parameter after the screen starts.
Searching PC IP address failed. No empty IP address was found by the automatic search for the IP address of the display unit. Please remove the control unit from the network, and turn ON the NC power supply again.
Appendix 9. User Parameter List 9.1 Process Parameters
IV - 140
Appendix 9. User Parameter List 9.1 Process Parameters
#1026 base_l Base axis I Set the names of the basic axes that compose the plane. Set the axis name set in "#1013 axname". If all three items ("base_I", "base_J" and "base_K") do not need to be set, such as for 2-axis specifications, input "0", and the parameter will be blank. Normally when X Y and Z are specified respectively for base_l_J_K the following relation will be established: G17: X-Y G18: Z-X G19: Y-Z Specify the desired axis name to set an axis address other than above.
---Setting range--- Axis names such as X, Y or Z
#1027 base_J Base axis J Set the names of the basic axes that compose the plane. Set the axis name set in "#1013 axname". If all three items ("base_I", "base_J" and "base_K") do not need to be set, such as for 2-axis specifications, input "0", and the parameter will be blank. Normally when X Y and Z are specified respectively for base_l_J_K the following relation will be established: G17: X-Y G18: Z-X G19: Y-Z Specify the desired axis name to set an axis address other than above.
---Setting range--- Axis names such as X, Y or Z
#1028 base_K Base axis K Set the names of the basic axes that compose the plane. Set the axis name set in "#1013 axname". If all three items ("base_I", "base_J" and "base_K") do not need to be set, such as for 2-axis specifications, input "0", and the parameter will be blank. Normally when X Y and Z are specified respectively for base_l_J_K the following relation will be established: G17: X-Y G18: Z-X G19: Y-Z Specify the desired axis name to set an axis address other than above.
---Setting range--- Axis names such as X, Y or Z
#1029 aux_I Flat axis I Set the axis name when there is an axis parallel to "#1026 base_I".
---Setting range--- Axis names such as X, Y or Z
#1030 aux_J Flat axis J Set the axis name when there is an axis parallel to "#1027 base_J".
---Setting range--- Axis names such as X, Y or Z
#1031 aux_K Flat axis K Set the axis name when there is an axis parallel to "#1028 base_K".
---Setting range--- Axis names such as X, Y or Z
Appendix 9. User Parameter List 9.1 Process Parameters
IV - 141
#1084 RadErr Arc error Set the tolerable error range when the end point deviates from the center coordinate in the circular command.
---Setting range--- 0 to 1.000 (mm)
#1171 taprov Tap return ovr Set the tap return override value for the synchronous tapping. When "0" is set, it will be regarded as 100%.
---Setting range--- 1 to 100 (%)
#1185 spd_F1 Feedrate F1 Set the feedrate for the F command in the F 1-digit command ("#1079 F1digit" is set to "1"). Feedrate when F1 is issued (mm/min)
---Setting range--- 1 to 60000 (mm/min)
#1186 spd_F2 Feedrate F2 Set the feedrate for the F command in the F 1-digit command ("#1079 F1digit" is set to "1"). Feedrate when F2 is issued (mm/min)
---Setting range--- 1 to 60000 (mm/min)
#1187 spd_F3 Feedrate F3 Set the feedrate for the F command in the F 1-digit command ("#1079 F1digit" is set to "1"). Feedrate when F3 is issued (mm/min)
---Setting range--- 1 to 60000 (mm/min)
#1188 spd_F4 Feedrate F4 Set the feedrate for the F command in the F 1-digit command ("#1079 F1digit" is set to "1"). Feedrate when F4 is issued (mm/min)
---Setting range--- 1 to 60000 (mm/min)
#1189 spd_F5 Feedrate F5 Set the feedrate for the F command in the F 1-digit command ("#1079 F1digit" is set to "1"). Feedrate when F5 is issued (mm/min)
---Setting range--- 1 to 60000 (mm/min)
#1506 F1_FM F1 upper limit Set the maximum value up to which the F 1-digit feedrate can be changed.
---Setting range--- 0 to 60000 (mm/min)
#1507 F1_K F1 change constant Set the constant that determines the speed change rate per manual handle graduation in F 1-digit feedrate change mode.
---Setting range--- 0 to 32767
Appendix 9. User Parameter List 9.1 Process Parameters
IV - 142
(No. of workpieces machined)
#8001 WRK COUNT M Set the M code for counting the number of the workpiece repeated machining. The number of the M-codes set by this parameter is counted. The No. will not be counted when set to "0".
---Setting range--- 0 to 99
#8002 WRK COUNT Set the initial value of the number of workpiece machining. The number of current workpiece machining is displayed.
---Setting range--- 0 to 999999
#8003 WRK COUNT LIMIT Set the maximum number of workpiece machining. A signal will be output to PLC when the number of machining times is counted to this limit.
---Setting range--- 0 to 999999
(Automatic tool length measurement)
#8004 SPEED Set the feedrate during automatic tool length measurement.
---Setting range--- 1 to 1000000 (mm/min)
#8005 ZONE r Set the distance between the measurement point and deceleration start point.
---Setting range--- 0 to 99999.999 (mm)
#8006 ZONE d Set the tolerable range of the measurement point. An alarm will occur when the sensor signal turns ON before the range, set by this parameter, has not been reached from the measurement point, or when the signal does not turn ON after the range is passed.
---Setting range--- 0 to 99999.999 (mm)
(Automatic corner override)
#8007 OVERRIDE Set the override value for automatic corner override.
---Setting range--- 0 to 100 (%)
#8008 MAX ANGLE Set the maximum corner opening angle where deceleration should start automatically. When the angle is larger than this value deceleration will not start.
---Setting range--- 0 to 180 ()
#8009 DSC. ZONE Set the position where deceleration starts at the corner. Designate at which length point before the corner deceleration should start.
---Setting range--- 0 to 99999.999 (mm)
Appendix 9. User Parameter List 9.1 Process Parameters
IV - 143
(Wear data input)
#8010 ABS. MAX for L system only Set the maximum value when inputting the tool wear compensation amount. A value exceeding this setting value cannot be set. Absolute value of the input value is set. (If a negative value is input, it is treated and set as a positive value.) If "0" is input, this parameter will be disabled.
---Setting range--- 0 to 99.999 (mm) (Input setting increment applies)
#8011 INC. MAX for L system only Set the maximum value for when inputting the tool wear compensation amount in the incremental mode. A value exceeding this setting value cannot be set. Absolute value of the input value is set. (If a negative value is input, it is treated and set as a positive value.) If "0" is input, this parameter will be disabled.
---Setting range--- 0 to 99.999 (mm) (Input setting increment applies)
(C axis normal line)
#8041 C-rot.R Set the length from the center of the normal line control axis to the tool tip. This is used to calculate the turning speed at the block joint. This is enabled during the normal line control type II.
---Setting range--- 0.000 to 99999.999 (mm)
#8042 C-ins.R Set the radius of the arc to be automatically inserted into the corner during normal line control. This is enabled during the normal line control type I.
---Setting range--- 0.000 to 99999.999 (mm)
#8043 Tool HDL FD OFS Set the length from the tool holder to the tool tip.
---Setting range--- 0.000 to 99999.999 (mm)
#8044 UNIT*10 Set the command increment scale. The scale will be "1" when "0" is set.
---Setting range--- 0 to 10000 (fold) 0: One fold
Appendix 9. User Parameter List 9.1 Process Parameters
IV - 144
<3-dimensional tool radius compensation>
#8071 3-D CMP for M system only Set the value of the denominator constants for 3-dimensional tool radius compensation. Set the value of "p" in the following formula. Vx = i x r/p, Vy = j x r/p, Vz = k x r/p Vx, Vy, Vz : X, Y, and Z axes or vectors of horizontal axes i, j, k : Program command value r : Offset p =(i2 + j2 + k2) when the set value is "0".
---Setting range--- 0 to 99999.999
#8072 SCALING P for M system only Set the scale factor for reduction or magnification in the machining program specified by G50 or G51 command. This parameter will be valid when the program specifies no scale factor.
---Setting range--- -99.999999 to 99.999999
#8075 SpiralEndErr for M system only Set the tolerable error range (absolute value) when the end point position, commanded by the spiral or conical interpolation command with the command format type 2, differs from the end point position obtained from the speed and increment/decrement amount.
---Setting range--- 0 to 99999.999 (mm)
#8078 Screen Saver Timer Set the period of time before turn-OFF of the display unit backlight. When "0" is set, the backlight is not turned OFF.
---Setting range--- 0 to 60 (min) 0: The backlight is not turned OFF
#8621 Coord rot plane (H) Set the plane (horizontal axis) for coordinate rotation control. Usually, set the name of the 1st axis. When not set, "X" axis will be set.
---Setting range--- Axis name
#8622 Coord rot plane (V) Set the plane (vertical axis) for coordinate rotation control. Usually, set the name of the 2nd axis. When not set, "Y" axis will be set.
---Setting range--- Axis name
#8623 Coord rot centr (H) Set the center coordinates (horizontal axis) for coordinate rotation control.
---Setting range--- -999999.999 to 999999.999 (mm)
Appendix 9. User Parameter List 9.1 Process Parameters
IV - 145
#8624 Coord rot centr (V) Set the center coordinates (vertical axis) for coordinate rotation control.
---Setting range--- -999999.999 to 999999.999 (mm)
#8625 Coord rot vctr (H) Set the vector components (horizontal axis) for coordinate rotation control. When this parameter is set, the coordinate rotation control angle (#8627) will be automatically calculated.
---Setting range--- -999999.999 to 999999.999 (mm)
#8626 Coord rot vctr (V) Set the vector components (vertical axis) for coordinate rotation control. When this parameter is set, the coordinate rotation control angle (#8627) will be automatically calculated.
---Setting range--- -999999.999 to 999999.999 (mm)
#8627 Coord rot angle Set the rotation angle for coordinate rotation control. When this parameter is set, the coordinate rotation vector (#8625, #8626) will be "0".
---Setting range--- -360.000 to 360.000 ()
#8701 Tool length Set the length to the touch tool tip.
---Setting range--- 99999.999 (mm)
#8702 Tool Dia Set the diameter of the sphere at the touch tool tip.
---Setting range--- 99999.999 (mm)
#8703 OFFSET X This sets the deviation amount (X direction) from the touch tool center to the spindle center.
---Setting range--- 99999.999 (mm)
#8704 OFFSET Y Set the deviation amount (Y direction) from the touch tool center to the spindle center.
---Setting range--- 99999.999 (mm)
#8705 RETURN Set the one-time return distance for contacting again.
---Setting range--- 0 to 99999.999 (mm)
#8706 FEED Set the feedrate when contacting again.
---Setting range--- 1 to 60000 (mm/min)
Appendix 9. User Parameter List 9.1 Process Parameters
IV - 146
#8707 Skip past amout (H) Set the difference (horizontal axis direction) between the skip read value and actual skip position.
---Setting range--- 99999.999 (mm)
#8708 Skip past amout (V) Set the difference (vertical axis direction) between the skip read value and actual skip position.
---Setting range--- 99999.999 (mm)
#8709 EXT work sign rvs Select when using the external workpiece coordinate system with Z shift. Select whether to reverse the sign. 0: External workpiece offset (Z shift) without sign reversal 1: External workpiece offset (Z shift) with sign reversal
#8710 EXT work ofs invld Set whether to enable external workpiece offset subtraction when setting the workpiece coordinate offset. 0: Not subtract the external workpiece offset. (Conventional specification) 1: Subtract the external workpiece offset.
#8711 TLM L meas axis Set the tool length measurement axis. Set the "#1022 axname2" axis name.
---Setting range--- Axis name (Note) If the axis name is illegal or not set, the 3rd axis name will be set as default.
#8712 TLM D meas axis Set the tool diameter measurement axis. Set the "#1022 axname2" axis name.
---Setting range--- Axis name (Note) If the axis name is illegal or not set, the 1st axis name will be set as default.
#19001 Syn.tap(,S)cancel 0: Retain the spindle speed (,S) in synchronous tap return 1: Cancel the spindle speed (,S) in synchronous tap return with G80
#19002 Zero-point mark Select the position for displaying the zero point mark in the graphic trace and 2D check. 0: Machine coordinates zero point (same as conventional method) 1: Workpiece coordinate zero point
#19003 PRG coord rot type Select the start point of the initial travel command after G68 command. 0: Calculate the end position using the current position on the local coordinate system before rotating, without rotating the start point in accordance with the coordinates rotation. 1: Calculate the end position, assuming that the start point rotates in accordance with the coordinates rotation.
Appendix 9. User Parameter List 9.1 Process Parameters
IV - 147
#19425 ManualB Std R1 Set a radius used as standard for the rotary axis speed. When the setting value of #19425 is larger than that of "#19427 ManualB Std R2", #19425 setting will be used as surface speed control standard radius 2: #19427 setting will be used as surface speed control standard radius 1.
---Setting range--- 0 to 99999.999 (mm)
#19426 ManualB Std F1 This sets the rotary axis speed for surface speed control standard radius 1 (ManualB Std R1). When the setting value of #19426 is larger than that of "#19428 ManualB Std F2", #19426 setting will be used as surface speed control standard speed 2: #19427 setting will be used as surface speed control standard speed 1.
---Setting range--- 1 to 1000000 (/min)
#19427 ManualB Std R2 Set a radius used as standard for the rotary axis speed. When the same value is set as "#19425 ManualB Std R1", the surface speed control standard speed 1 (ManualB Std F1) will be selected as the rotary axis speed if the radius is less than that value. The surface speed control standard speed 2 (ManualB Std F2) is selected if larger than the set value.
---Setting range--- 0 to 99999.999 (mm)
#19428 ManualB Std F2 Set the rotary axis speed for surface speed control standard radius 2 (ManualB Std R2).
---Setting range--- 1 to 1000000 (/min)
Appendix 9. User Parameter List 9.2 Fixed Cycle
IV - 148
9.2 Fixed Cycle
(Fixed cycle)
#8012 G73 n for M system only Set the return amount for G73 (step cycle).
---Setting range--- 0 to 99999.999 (mm)
#8013 G83 n Set the return amount for G83 (deep hole drilling cycle).
---Setting range--- 0 to 99999.999 (mm)
#8014 CDZ-VALE for L system only Set the screw cut up amount for G76 and G78 (thread cutting cycle).
---Setting range--- 0 to 127 (0.1 lead)
#8015 CDZ-ANGLE for L system only Set the screw cut up angle for G76 and G78 (thread cutting cycle).
---Setting range--- 0 to 89 ()
#8016 G71 MINIMUM for L system only Set the minimum value of the last cutting amount by the rough cutting cycle (G71, G72). The cutting amount of the last cutting will be the remainder. When the remainder is smaller than this parameter setting, the last cycle will not be executed.
---Setting range--- 0 to 999.999 (mm)
#8017 G71 DELTA-D for L system only Set the change amount of the rough cutting cycle. The rough cutting cycle (G71, G72) cutting amount repeats d+d, d, d-d using the value (d) commanded with D as a reference. Set the change amount d.
---Setting range--- 0 to 999.999 (mm)
#8018 G84/G74 n for M system only Not used. Set to "0".
(Fixed cycle)
#8051 G71 THICK Set the amount of cut-in by the rough cutting cycle (G71, G72)
---Setting range--- 0 to 99999.999 (mm)
#8052 G71 PULL UP Set the amount of pull-up when returning to the cutting start point for the rough cutting cycle (G71. G72).
---Setting range--- 0 to 99999.999 (mm)
Appendix 9. User Parameter List 9.2 Fixed Cycle
IV - 149
#8053 G73 U Set the X-axis cutting margin of the forming rough cutting cycle (G73).
---Setting range--- -99999.999 to 99999.999 (mm)
#8054 G73 W Set the Z-axis cutting margin of the forming rough cutting cycle (G73).
---Setting range--- -99999.999 to 99999.999 (mm)
#8055 G73 R Set how many times cutting will be performed in the forming rough cutting cycle (G73).
---Setting range--- 0 to 99999 (times)
#8056 G74 RETRACT Set the amount of retract (amount of cut-up) of the cutting-off cycle (G74, G75).
---Setting range--- 0 to 999.999 (mm)
#8057 G76 LAST-D Set the amount of final cut-in by the compound type thread cutting (G76).
---Setting range--- 0 to 999.999 (mm)
#8058 G76 TIMES Set how many times the amount of final cut-in cycle (G76 finish margin) will be divided in the compound type thread cutting (G76).
---Setting range--- 0 to 99 (times)
#8059 G76 ANGLE Set the angle (thread angle) of the tool nose in the compound type thread cutting (G76).
---Setting range--- 0 to 99 ()
#8083 G83S modeM for M system only Set the M command code for changing to the small diameter deep hole drilling cycle mode.
---Setting range--- 1 to 99999999
#8084 G83S Clearance for M system only Set the clearance amount for the small diameter deep hole drilling cycle (G83).
---Setting range--- 0 to 999.999 (mm)
Appendix 9. User Parameter List 9.2 Fixed Cycle
IV - 150
#8085 G83S Forward F for M system only Set the feedrate from the R point to the cutting start position in the small diameter deep hole drilling cycle (G83).
---Setting range--- 0 to 99999 (mm/min)
#8086 G83S Back F for M system only Set the speed for returning from the hole bottom during the small diameter deep hole drilling cycle (G83).
---Setting range--- 0 to 99999 (mm/min)
Appendix 9. User Parameter List 9.3 Control Parameters 1
IV - 151
9.3 Control Parameters 1
#1041(PR) l_inch Initial inch Select the unit system for the program travel amount when the power is turned ON or reset and for position display.
0: Metric system 1: Inch system
(Note) Selection of inch and metric unit When the setting value of "#1041 I_inch" is changed, the unit of length is changed after reset. The following parameters concerning length, however, are not changed automatically. Change the setting values of following parameters according to the new unit system.
#8004 SPEED #8027 Toler-1 #8056 G74 RETRACT #8005 ZONE r #8028 Toler-2 #8057 G76 LAST-D #8006 ZONE d #8029 FairingL #8075 SpiralEndErr
#8009 DSC. ZONE #8030 MINUTE LENGS #8010 ABS. MAX. #8037 CorJudgeL #8011 INC. MAX. #8041 C-rot. R #8085 G83S Forward F #8012 G73n #8042 C-ins. R #8086 G83S Back F #8013 G83n #8051 G71 THICK #8016 G71 MINIMUM #8052 G71 PULL UP
#8017 G71 DELTA-D #8053 G73 U #8018 G84/G74n #8054 G73 W
Barrier data Base specifications parameter "#8004 SPEED" is 10 inches/min. unit for the inch system.
Workpiece coordinate offset
Tool compensation amount (Tool length compensation amount, tool wear compensation amount and tool tip compensation amount)
#8084 G83S Clearance
Machining parameter
Axis parameter
#1084 RadErr
#8300-#8306, #8311-#8314
#8204 OT-CHECK-N #8205 OT-CHECK-P #8206 TOOL CHG.P #8209 G60 Shift
#1078 Decpt2 Decimal pnt type 2 Select the increment of position commands that do not have a decimal point.
0: Minimum input command unit (follows "#1015 cunit") 1: 1mm (or 1inch) unit (For the dwell time, 1s unit is used.)
#1080 Dril_Z (For M system only) Drilling Z fixed Select a fixed cycle hole drilling axis.
0: Use an axis vertical to the selected plane as hole drilling axis. 1: Use the Z axis as the hole drilling axis regardless of the selected plane.
#1091 Mpoint Ignore middle pnt Select how to handle the middle point during G28 and G30 reference position return.
0: Pass the middle point designated in the program and move to the reference position. 1: Ignore the middle point designated in the program and move straight to the reference position.
#1103 T_life T-life mgmt valid Select whether to use the tool life management.
0: Not use 1: Use
Appendix 9. User Parameter List 9.3 Control Parameters 1
IV - 152
#1104 T_Com2 Tool cmd mthd 2 Select how to handle the tool command in the program when "#1103 T_Life" is set to "1".
0: Handle the command as group No. 1: Handle the command as tool No.
#1105 T_Sel2 Tool selection method 2 Select the tool selection method when "#1103 T_Life" is set to "1".
0: Select in order of registered No. from the tools used in the same group. 1: Select the tool with the longest remaining life from the tools used or unused in the same group.
#1106 Tcount Tool mgmt count for L system only Select the input method when address N is omitted in inputting the data (G10 L3 command) for tool life management function II.
0: Time specified input 1: Number of times specified input
#1126 PB_G90 Playback G90 Select the method to command the playback travel amount in the playback editing. 0: Incremental value 1: Absolute value
#1128 RstVCI Com-var RET clear Select how to handle the common variables when resetting. 0: Common variables won't change after resetting. 1: The following common variables will be cleared by resetting: #100 to #149 when 100 sets of variables are provided. #100 to #199 when 200 sets or more of variables are provided.
#1129 PwrVCl Clear variables by power-ON Select how to handle the common variables when the power is turned ON. 0: The common variables are in the same state as before turning the power OFF. 1: The following common variables will be cleared when the power is turned ON: #100 to #149 when 100 sets of variables are provided. #100 to #199 when 200 sets or more of variables are provided.
#1148 I_G611 Initial hi-precis Set the high accuracy control mode for the modal state when the power is turned ON.
0: G64 (cutting mode) at power ON 1: G61.1 (high-accuracy control mode) at power ON
#1302 AutoRP Auto restart valid Select the method to move to the restart position when restarting the program.
0: Move the system manually to the restart position and then restart the program. 1: The system automatically moves to the restart position at the first activation after the program restarts.
#8101 MACRO SINGLE Select how to control the blocks where the user macro command continues. 0: Do not stop while macro blocks continue. 1: Stop every block during signal block operation.
#8102 COLL. ALM OFF Select the interference (bite) control to the workpiece from the tool diameter during tool radius compensation and nose R compensation. 0: An alarm will be output and operation stops when an interference is judged. 1: Changes the path to avoid interference.
Appendix 9. User Parameter List 9.3 Control Parameters 1
IV - 153
#8103 COLL. CHK OFF Select the interference (bite) control to the workpiece from the tool diameter during tool radius compensation and nose R compensation. 0: Performs interference check. 1: Does not perform interference check.
#8105 EDIT LOCK B Select the edit lock for program Nos. 8000 to 9999 in the memory. 0: Enable the editing. 1: Prohibit the editing of above programs. When "1" is set, the file cannot be opened.
#8106 G46 NO REV-ERR for L system only Select the control for the compensation direction reversal in G46 (nose R compensation). 0: An alarm will be output and operation will stop when the compensation direction is reversed (G41 -> G42 G42 -> G41). 1: An alarm won't occur when the compensation direction is reversed, and the current compensation direction will be maintained.
#8107 R COMPENSATION Select whether to move to the inside because of a delay in servo response to a command during arc cutting mode. 0: Move to the inside, making the arc smaller than the command value. 1: Compensate the movement to the inside.
#8108 R COMP Select Select the arc radius error compensation target. 0: Perform compensation over all axes. 1: Perform compensation axis by axis. (Note) This parameter is effective only when "#8107 R COMPENSATION" is "1".
#8109 HOST LINK Select whether to enable computer link B instead of the RS-232C port. 0: Disable (Enable normal RS-232C communication.) 1: Enable (Disable normal RS-232C communication.)
#8110 G71/G72 POCKET Select whether to enable the pocket machining when there is a dimple (pocket) in the rough cutting cycle (G71, G72) finishing program. 0: OFF 1: ON
#8111 Milling Radius Select the diameter and radius of the linear axis for milling (cylindrical/pole coordinate) interpolation. 0: All axes radius command 1: Each axis setting (follows "#1019 dia") (Note) This parameter is valid only in the milling (cylindrical/polar coordinate) interpolation mode.
#8112 DECIMAL PNT-P Select whether to enable the decimal point command for G04 address P. 0: Disable 1: Enable
Appendix 9. User Parameter List 9.3 Control Parameters 1
IV - 154
#8113 Milling Init G16 Set which plane to execute for milling machining after the power is turned ON or reset.
#8113 #8114 Plane 0 0 G17 plane 0 1 G19 plane 1 0 1 1
G16 plane
0: Not G16 plane 1: G16 plane (Note) This parameter is valid for the G code system 2 or 3 ("#1037 cmdtyp"="3" or "4").
#8114 Milling Init G19 Set which plane to execute for milling machining after the power is turned ON or reset.
#8113 #8114 Plane 0 0 G17 plane 0 1 G19 plane 1 0 1 1
G16 plane
0: Not G19 plane 1: G19 plane (Note) This parameter is valid for the G code system 2 or 3 ("#1037 cmdtyp"="3" or "4").
#8116 Coord rot para invd Select whether to enable the coordinate rotation by the parameters. 0: Enable 1: Disable
#8117 OFS Diam DESIGN Select tool radius or tool diameter compensation amount to be specified. 0: Tool radius compensation amount 1: Tool diameter compensation amount
#8119 Comp. unit switch Select the setting unit of compensation amount that has no decimal point. 0: 1mm (or 1inch) unit 1: The minimum command unit (follows "#1003 iunit")
#8121 Screen Capture Select whether to enable the screen capture function. 0: Disable 1: Enable (Note1) By setting this parameter to "1", and by keeping pushing the [SHIFT] key, screen capture will be executed. (Note2) This parameter is valid only with M70 Series.
#8122 Keep G43 MDL M-REF Select whether to keep the tool length offset by high speed manual reference position return during tool length offset. 0: Will not be kept (Cancel) 1: Kept
Appendix 9. User Parameter List 9.3 Control Parameters 1
IV - 155
#8124 Mirr img at reset Select the operation type of the mirror image by parameter setting and the mirror image by external input.
0: The current mirror image is canceled, and new mirror image will start with the machine position at reset as the mirror center. 1: The mirror center is kept to continue the mirror image.
#8145 Validate F1 digit Select whether to execute the F command with a 1-digit code command or with a direct numerical command. 0: Direct numerical command (command feedrate during feed per minute or rotation) 1: 1-digit code command (with the feedrate specified by the parameters "#1185 spd_F1" to "#1189 F5")
#8154(PR) Not used. Set to "0".
#8155 Sub-pro interrupt Select the method for the user macro interrupt. 0: The user macro interrupt of macro type 1: The user macro interrupt of sub-program type
#8156 Fine thread cut E Select the address E type when cutting an inch screw. 0: Specify the number of threads per inch for inch screw cutting. 1: Specify the precision lead for inch screw cutting.
#8157 Radius comp type B (M system) / Nose R comp type B (L system) For M system Select the method of the arithmetic processing for the intersection point when the start-up or cancel commands are operated during radius compensation. 0: The processing does not handle the start-up or cancel command block: handle the offset vector in the direction vertical to that of the command instead. 1: The processing is executed for the intersection point between the command block and the next block. For L system Select the method of the arithmetic processing for the intersection point when the start-up or cancel commands are operated during nose R or radius compensation. 0: The processing does not handle the start-up or cancel command block: handle the offset vector in the direction vertical to that of the command instead. 1: The processing is executed for the intersection point between the command block and the next block.
#8158 Init const sur spd Select the initial state after power-ON. 0: Constant surface speed control cancel mode. 1: Constant surface speed control mode.
#8159 Synchronous tap Select whether to use the floating tap chuck in G74 and G84 tap cycles. 0: With a floating tapping chuck 1: Without a floating tapping chuck
Appendix 9. User Parameter List 9.3 Control Parameters 1
IV - 156
#8160 Start point alarm Select an operation when the operation start point cannot be found while moving to the next block of G117. 0: The auxiliary function is enabled after the block for the movement has finished. 1: The program error (P33) occurs.
Appendix 9. User Parameter List 9.4 Control Parameters 2
IV - 157
9.4 Control Parameters 2
#1025 l_plane Initial plane Select the plane to be selected when the power is turned ON or reset.
0: X-Y plane (G17 command state) 1: X-Y plane (G17 command state) 2: Z-X plane (G18 command state) 3: Y-Z plane (G19 command state)
#1037(PR) cmdtyp Command type Set the G code list and compensation type for programs.
cmdtyp G code list Compensation type 1 List 1 (for M) Type A
(one compensation amount for one compensation No.) 2 List 1 (for M) Type B
(shape and wear compensation amounts for one compensation No.)
3 List 2 (for L) Type C (shape and wear compensation amounts for one compensation No.)
4 List 3 (for L) Ditto
5 List 4 (for special L) Ditto
6 List 5 (for special L) Ditto
7 List 6 (for special L) Ditto
8 List 7 (for special L) Ditto
9 List 8 (for M) M2 format type A
Type A (one compensation amount for one compensation No.)
10 List 8 (for M) M2 format type B
Type B (shape and wear amounts for one compensation No.)
There are some items in the specifications that can be used or cannot be used according to the value set in this parameter. The file structure may also change depending on the compensation data type.
#1073 I_Absm Initial absolute Select the mode (absolute or incremental) at turning ON the power or reset.
0: Incremental setting 1: Absolute setting
#1074 l_Sync Initial sync feed Select the feedrate mode at turning ON the power or reset.
0: Asynchronous feed (feed per minute) 1: Synchronous feed (feed per revolution)
#1075 I_G00 Initial G00 Select the linear command mode at turning ON the power or reset.
0: Linear interpolation (G01 command state) 1: Positioning (G00 command state)
#1076 Abslnc ABS/INC address for L system only Select the command method for the absolute and incremental commands.
0: Use G command for the absolute and incremental commands. 1: Use axis name for the absolute and incremental commands.
(The axis name in "#1013 axname" will be the absolute command, "#1014 incax" will be the incremental command.) When "1" is selected, using two axis names, one each for the absolute and incremental commands, allows to issue the absolute and incremental commands appropriately to an axis.
Appendix 9. User Parameter List 9.4 Control Parameters 2
IV - 158
#1085 G00Drn G00 dry run Select whether to apply dry run (feed at manual setting speed instead of command feedrate) to the G00 command. 0: Not apply to G00. (move at rapid traverse rate) 1: Apply to G00. (move at manual setting speed)
#1086 G0lntp G00 interp OFF Select the G00 travel path type. 0: Move linearly toward the end point. (interpolation type) 1: Move to the end point of each axis at the rapid traverse feedrate for each axis. (non-interpolation) (Note) If this parameter is set to "1", neither of the following functions will be available: rapid traverse constant inclination acceleration/deceleration and rapid traverse constant inclination multi-step acceleration/deceleration.
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 159
9.5 I/O Parameters
There are basically two types of input/output parameters which must be set when inputting outputting or referring to data or when performing tape operation.
9001 to 9018, 9051, 9052 parameters:
Set which channel to connect which device to for each I/O application.
901 to 9528 parameters: Set the transmission speed, etc., for each input/output device. Up to five types of input/output device parameters can be set in device 0 to 4.
#9001 DATA IN PORT Select the port for inputting the data such as machine program and parameters. 1: ch1 2: ch2
#9002 DATA IN DEV. Select the device No. for inputting the data. (The device Nos. correspond to the input/output device parameters.)
---Setting range--- 0 to 4
#9003 DATA OUT PORT Select the port for outputting the data such as machine program and parameters. 1: ch1 2: ch2
#9004 DATA OUT DEV. Select the device No. for outputting the data. (The device Nos. correspond to the input/output device parameters.)
---Setting range--- 0 to 4
#9005 TAPE MODE PORT Select the input port for running with the tape mode. 1: ch1 2: ch2
#9006 TAPE MODE DEV. Select the device No. to be run with the tape mode. (The device Nos. correspond to the input/output device parameters.)
---Setting range--- 0 to 4
#9007 MACRO PRINT PORT Select the output port used for the user macro DPRINT command. 1: ch1 2: ch2
#9008 MACRO PRINT DEV. Select the device No. used for the DPRINT command. (The device Nos. correspond to the input/output device parameters.)
---Setting range--- 0 to 4
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 160
#9009 PLC IN/OUT PORT Select the port for inputting/outputting various data with PLC. 1: ch1 2: ch2
#9010 PLC IN/OUT DEV. Select the device No. used for the PLC input/output. (The device Nos. correspond to the input/output device parameters.)
---Setting range--- 0 to 4
#9011 REMOTE PRG IN PORT Select the port for inputting remote programs. 1: ch1 2: ch2
#9012 REMOTE PRG IN DEV. Select the device No. used to input remote programs. The device Nos. correspond to the input/output device parameters.
---Setting range--- 0 to 4
#9013 EXT UNIT PORT Select the port for communication with an external unit. 1: ch1 2: ch2
#9014 EXT UNIT DEV. Select the unit No. used for communication with an external unit (The unit Nos. correspond to the input/output device parameters.)
---Setting range--- 0 to 4
#9017 HANDY TERMINAL PORT Select the port for communication with a handy terminal. 1: ch1 2: ch2
#9018 HANDY TERMINAL DEV. Select the device No. used for communication with a handy terminal. (The device Nos. correspond to the input/output device parameters.)
---Setting range--- 0 to 4
#9051 Data I/O port Select whether to use display side serial port or NC side serial port for data input/output function. 0: Display side serial port 1: Display side serial port 2: NC side serial port (Note) The setting range differs according to the model.
#9052 Tape mode port Select whether to use display side serial port or NC side serial port for tape mode. 0: NC side serial port 1: Display side serial port 2: NC side serial port (Note) The setting range differs according to the model.
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 161
#9101 DEV0 DEVICE NAME Set the device name corresponding to the device No. Set a simple name for quick identification.
---Setting range--- Use alphabet characters numerals and symbols to set a name within 3 characters.
#9102 DEV0 BAUD RATE Select the serial communication speed. 0: 19200 (bps) 1: 9600 2: 4800 3: 2400 4: 1200 5: 600 6: 300 7: 110
#9103 DEV0 STOP BIT Select the stop bit length used in the start-stop system. Refer to "#9104 DEV0 PARITY CHECK". At the output of data, the number of characters is always adjusted for the parity check. 1: 1 (bit) 2: 1.5 3: 2
#9104 DEV0 PARITY CHECK Select whether to add the parity check bit to the data.
ON OFF
Start bit Data bit Parity bit Stop bit
1 character
b1 b2 b3 b4 b5 b6 bn
Set this parameter in accordance with the I/O device specifications. 0: Not add a parity bit in I/O mode 1: Add a parity bit in I/O mode
#9105 DEV0 EVEN PARITY Select odd or even when parity is added to the data. This parameter is ignored when no parity is added. 0: Odd parity 1: Even parity
#9106 DEV0 CHR. LENGTH Set the length of the data bit. Refer to "#9104 DEV0 PARITY CHECK". 0: 5 (bit) 1: 6 2: 7 (NC connection not supported) 3: 8
#9107 DEV0 TERMINATR TYP Select the code to terminate data reading. 0, 3: EOR 1, 2: EOB or EOR
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 162
#9108 DEV0 HAND SHAKE Select the transmission control method. No handshaking will be used when a value except 1 to 3 is set. 1: RTS/CTS method 2: No handshaking 3: DC code method
#9109 DEV0 DC CODE PRTY Select the DC code type when the DC code method is selected. 0: Not add parity to DC code (DC3 = 13H) 1: Add parity to DC code (DC3 = 93H)
#9111 DEV0 DC2/4 OUTPUT Select the DC code handling when outputting data to the output device.
---Setting range--- DC2 / DC4 0: None / None 1: Yes / None 2: None / Yes 3: Yes / Yes
#9112 DEV0 CR OUTPUT Select whether to add the (CR) code just before the EOB (L/F) code during output. 0: Not add 1: Add
#9113 DEV0 EIA OUTPUT Select ISO or EIA code for data output. In data input mode, the ISO and EIA codes are identified automatically. 0: ISO code output 1: EIA code output
#9114 DEV0 FEED CHR. Set the length of the tape feed to be output at the start and end of the data during tape output.
---Setting range--- 0 to 999 (characters)
#9115 DEV0 PARITY V Select whether to perform the parity check for the number of characters in a block at the input of data. At the output of data, the number of characters is always adjusted to for the parity check. 0: Not perform parity V check 1: Perform parity V check
#9116 DEV0 TIME-OUT (sec) Set the time out time to detect an interruption in communication. Time out check will not be executed when set to "0".
---Setting range--- 0 to 30 (s)
#9117 DEV0 DR OFF Select whether to enable the DR data check in data I/O mode. 0: Enable 1: Disable
#9118 DEV0 DATA ASCII Select the code of the output data. 0: ISO/EIA code (Depends on whether #9113, #9213, #9313, #9413 or #9513 EIA output parameter is set up.) 1: ASCII code
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 163
#9119 DEV0 INPUT TYPE Select the mode for input (verification). 0: Standard input (Data from the very first EOB is handled as significant information.) 1: EOBs following the first EOB of the input data are skipped until data other than EOB is input
#9121 DEV0 EIA CODE [ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " [ ". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified.
---Setting range--- 0 to FF (hexadecimal)
#9122 DEV0 EIA CODE ] Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " ] ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified.
---Setting range--- 0 to FF (hexadecimal)
#9123 DEV0 EIA CODE # Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "#". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified.
---Setting range--- 0 to FF (hexadecimal)
#9124 DEV0 EIA CODE * Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified.
---Setting range--- 0 to FF (hexadecimal)
#9125 DEV0 EIA CODE = Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "=". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified.
---Setting range--- 0 to FF (hexadecimal)
#9126 DEV0 EIA CODE : Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " : ". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified.
---Setting range--- 0 to FF (hexadecimal)
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 164
#9127 DEV0 EIA CODE $ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "$". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified.
---Setting range--- 0 to FF (hexadecimal)
#9128 DEV0 EIA CODE ! Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "!". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified.
---Setting range--- 0 to FF (hexadecimal)
#9201 DEV1 DEVICE NAME Set the device name corresponding to the device No. Set a simple name for quick identification. Use alphabet characters numerals and symbols to set a name within 3 characters.
#9202 DEV1 BAUD RATE Select the serial communication speed. 0: 19200 (bps) 1: 9600 2: 4800 3: 2400 4: 1200 5: 600 6: 300 7: 110
#9203 DEV1 STOP BIT Select the stop bit length used in the start-stop system. Refer to "#9204 DEV1 PARITY CHECK". At the output of data, the number of characters is always adjusted to for the parity check. 1: 1 (bit) 2: 1.5 3: 2
#9204 DEV1 PARITY CHECK Select whether to add a parity check bit to the data.
ON OFF
Start bit Data bit Parity bit Stop bit
1 character
b1 b2 b3 b4 b5 b6 bn
Set this parameter in accordance with the I/O device specifications. 0: Not add a parity bit in I/O mode 1: Add a parity bit in I/O mode
#9205 DEV1 EVEN PARITY Select whether even or odd parity will be used when parity is used. This parameter is ignored when no parity is added. 0: Odd parity 1: Even parity
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 165
#9206 DEV1 CHR. LENGTH Select the length of the data bit. Refer to "#9204 DEV1 PARITY CHECK". 0: 5 (bit) 1: 6 2: 7 (NC connection not supported) 3: 8
#9207 DEV1 TERMINATR TYP Select the code to terminate data reading. 0,3: EOR 1,2: EOB or EOR
#9208 DEV1 HAND SHAKE Select the transmission control method. No handshaking will be used when a value except 1 to 3 is set. 1: RTS/CTS method 2: No handshaking 3: DC code method
#9209 DEV1 DC CODE PRTY Select the DC code type when the DC code method is selected. 0: Not add parity to DC code (DC3 = 13H) 1: Add parity to DC code (DC3 = 93H)
#9211 DEV1 DC2/4 OUTPUT Select the DC code handling when outputting data to the output device. DC2 / DC4 0: None / None 1: Yes / None 2: None / Yes 3: Yes / Yes
#9212 DEV1 CR OUTPUT Select whether to add the (CR) code just before the EOB (L/F) code during output. 0: Not add 1: Add
#9213 DEV1 EIA OUTPUT Select ISO or EIA code for data output. In data input mode, the ISO and EIA codes are identified automatically. 0: ISO code output 1: EIA code output
#9214 DEV1 FEED CHR. Set the length of the tape feed to be output at the start and end of the data during tape output. 0 to 999 (characters)
#9215 DEV1 PARITY V Select whether to perform the parity check for the number of characters in a block at the input of data. At the output of data, the number of characters is always adjusted to for the parity check. 0: Not perform parity V check 1: Perform parity V check
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 166
#9216 DEV1 TIME-OUT (sec) Set the time out time to detect an interruption in communication. Time out check will not be executed when set to "0". 0 to 30 (s)
#9217 DEV1 DR OFF Select whether to enable the DR data check in data I/O mode. 0: Enable 1: Disable
#9218 DEV1 DATA ASCII Select the code of the output data. 0: ISO/EIA code (Depends on whether #9113, #9213, #9313, #9413 or #9513 EIA output parameter is set up.) 1: ASCII code
#9219 DEV1 INPUT TYPE Select the mode for input (verification). 0: Standard input (Data from the very first EOB is handled as significant information.) 1: EOBs following the first EOB of the input data are skipped until data other than EOB is input
#9221 DEV1 EIA CODE [ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " [ ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9222 DEV1 EIA CODE ] Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " ] ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9223 DEV1 EIA CODE # Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "#". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. . 0 to FF (hexadecimal)
#9224 DEV1 EIA CODE Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 167
#9225 DEV1 EIA CODE = Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "=". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9226 DEV1 EIA CODE : Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " : ". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9227 DEV1 EIA CODE $ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "$". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9228 DEV1 EIA CODE ! Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "!". When output with EIA code data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9301 DEV2 DEVICE NAME Set the device name corresponding to the device No. Set a simple name for quick identification. Use alphabet characters numerals and symbols to set a name within 3 characters.
#9302 DEV2 BAUD RATE Select the serial communication speed. 0: 19200 (bps) 1: 9600 2: 4800 3: 2400 4: 1200 5: 600 6: 300 7: 110
#9303 DEV2 STOP BIT Select the stop bit length used in the start-stop system. Refer to "#9304 DEV2 PARITY CHECK". At the output of data, the number of characters is always adjusted to for the parity check. 1: 1 (bit) 2: 1.5 3: 2
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 168
#9304 DEV2 PARITY CHECK Select whether to add a parity check bit to the data.
ON OFF
Start bit Data bit Parity bit Stop bit
1 character
b1 b2 b3 b4 b5 b6 bn
Set this parameter in accordance with the I/O device specifications. 0: Not add a parity bit in I/O mode 1: Add a parity bit in I/O mode
#9305 DEV2 EVEN PARITY Select whether even or odd parity will be used when parity is used. This parameter is ignored when no parity is added. 0: Odd parity 1: Even parity
#9306 DEV2 CHR. LENGTH Select the length of the data bit. Refer to "#9304 DEV2 PARITY CHECK". 0: 5 (bit) 1: 6 2: 7 (NC connection not supported) 3: 8
#9307 DEV2 TERMINATR TYP Select the code to terminate data reading. 0, 3: EOR 1, 2: EOB or EOR
#9308 DEV2 HAND SHAKE Select the transmission control method. No handshaking will be used when a value except 1 to 3 is set. 1: RTS/CTS method 2: No handshaking 3: DC code method
#9309 DEV2 DC CODE PRTY Select the DC code type when the DC code method is selected. 0: Not add parity to DC code (DC3 = 13H) 1: Add parity to DC code (DC3 = 93H)
#9311 DEV2 DC2/4 OUTPUT Select the DC code handling when outputting data to the output device. DC2 / DC4 0: None / None 1: Yes / None 2: None / Yes 3: Yes / Yes
#9312 DEV2 CR OUTPUT Select whether to add the (CR) code just before the EOB (L/F) code during output. 0: Not add 1: Add
#9313 DEV2 EIA OUTPUT Select ISO or EIA code for data output. In data input mode, the ISO and EIA codes are identified automatically. 0: ISO code output 1: EIA code output
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 169
#9314 DEV2 FEED CHR. Set the length of the tape feed to be output at the start and end of the data during tape output. 0 to 999 (characters)
#9315 DEV2 PARITY V Select whether to perform the parity check for the number of characters in a block at the input of data. At the output of data, the number of characters is always adjusted to for the parity check. 0: Not perform parity V check 1: Perform parity V check
#9316 DEV2 TIME-OUT (sec) Set the time out time to detect an interruption in communication. Time out check will not be executed when set to "0". 0 to 30 (s)
#9317 DEV2 DR OFF Select whether to enable the DR data check in data I/O mode. 0: Enable 1: Disable
#9318 DEV2 DATA ASCII Select the code of the output data. 0: ISO/EIA code (Depends on whether #9113, #9213, #9313, #9413 or #9513 EIA output parameter is set up.) 1: ASCII code
#9319 DEV2 INPUT TYPE Select the mode for input (verification). 0: Standard input (Data from the very first EOB is handled as significant information.) 1: EOBs following the first EOB of the input data are skipped until data other than EOB is input
#9321 DEV2 EIA CODE [ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " [ ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9322 DEV2 EIA CODE ] Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " ] ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9323 DEV2 EIA CODE # Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "#". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 170
#9324 DEV2 EIA CODE Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9325 DEV2 EIA CODE = Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "=". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9326 DEV2 EIA CODE : Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " : ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9327 DEV2 EIA CODE $ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "$". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9328 DEV2 EIA CODE ! Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "!". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9401 DEV3 DEVICE NAME Set the device name corresponding to the device No. Set a simple name for quick identification. Use alphabet characters numerals and symbols to set a name within 3 characters.
#9402 DEV3 BAUD RATE Select the serial communication speed. 0: 19200 (bps) 1: 9600 2: 4800 3: 2400 4: 1200 5: 600 6: 300 7: 110
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 171
#9403 DEV3 STOP BIT Select the stop bit length used in the start-stop system. Refer to "#9404 DEV3 PARITY CHECK". At the output of data, the number of characters is always adjusted to for the parity check. 1: 1 (bit) 2: 1.5 3: 2
#9404 DEV3 PARITY CHECK Select whether to add a parity check bit to the data.
ON OFF
Start bit Data bit Parity bit Stop bit
1 character
b1 b2 b3 b4 b5 b6 bn
Set this parameter in accordance with the I/O device specifications. 0: Not add a parity bit in I/O mode 1: Add a parity bit in I/O mode
#9405 DEV3 EVEN PARITY Select whether even or odd parity will be used when parity is used. This parameter is ignored when no parity is added. 0: Odd parity 1: Even parity
#9406 DEV3 CHR. LENGTH Select the length of the data bit. Refer to "#9404 DEV3 PARITY CHECK". 0: 5 (bit) 1: 6 2: 7 (NC connection not supported) 3: 8
#9407 DEV3 TERMINATR TYP Select the code to terminate data reading. 0, 3: EOR 1, 2: EOB or EOR
#9408 DEV3 HAND SHAKE Select the transmission control method. No handshaking will be used when a value except 1 to 3 is set. 1: RTS/CTS method 2: No handshaking 3: DC code method
#9409 DEV3 DC CODE PRTY Select the DC code type when the DC code method is selected. 0: Not add parity to DC code (DC3 = 13H) 1: Add parity to DC code (DC3 = 93H)
#9411 DEV3 DC2/4 OUTPUT Select the DC code handling when outputting data to the output device. DC2 / DC4 0: None / None 1: Yes / None 2: None / Yes 3: Yes / Yes
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 172
#9412 DEV3 CR OUTPUT Select whether to add the (CR) code just before the EOB (L/F) code during output. 0: Not add 1: Add
#9413 DEV3 EIA OUTPUT Select ISO or EIA code for data output. In data input mode, the ISO and EIA codes are identified automatically. 0: ISO code output 1: EIA code output
#9414 DEV3 FEED CHR. Set the length of the tape feed to be output at the start and end of the data during tape output. 0 to 999 (characters)
#9415 DEV3 PARITY V Select whether to perform the parity check for the number of characters in a block at the input of data. At the output of data, the number of characters is always adjusted to for the parity check. 0: Not perform parity V check 1: Perform parity V check
#9416 DEV3 TIME-OUT (sec) Set the time out time to detect an interruption in communication. Time out check will not be executed when set to "0". 0 to 30 (s)
#9417 DEV3 DR OFF Select whether to enable the DR data check in data I/O mode. 0: Enable 1: Disable
#9418 DEV3 DATA ASCII Select the code of the output data. 0: ISO/EIA code (Depends on whether #9113, #9213, #9313, #9413 or #9513 EIA output parameter is set up.) 1: ASCII code
#9419 DEV3 INPUT TYPE Select the mode for input (verification). 0: Standard input (Data from the very first EOB is handled as significant information.) 1: EOBs following the first EOB of the input data are skipped until data other than EOB is input.
#9421 DEV3 EIA CODE [ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " [ ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 173
#9422 DEV3 EIA CODE ] Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " ] ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9423 DEV3 EIA CODE # Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "#". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9424 DEV3 EIA CODE Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9425 DEV3 EIA CODE = Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "=". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9426 DEV3 EIA CODE : Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " : ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9427 DEV3 EIA CODE $ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "$". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9428 DEV3 EIA CODE ! Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "!". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 174
#9501 DEV4 DEVICE NAME Set the device name corresponding to the device No. Set a simple name for quick identification. Use alphabet characters numerals and symbols to set a name within 3 characters.
#9502 DEV4 BAUD RATE Select the serial communication speed. 0: 19200 (bps) 1: 9600 2: 4800 3: 2400 4: 1200 5: 600 6: 300 7: 110
#9503 DEV4 STOP BIT Select the stop bit length used in the start-stop system. Refer to "#9504 DEV4 PARITY CHECK". At the output of data, the number of characters is always adjusted to for the parity check. 1: 1 (bit) 2: 1.5 3: 2
#9504 DEV4 PARITY CHECK Select whether to add a parity check bit to the data.
ON OFF
Start bit Data bit Parity bit Stop bit
1 character
b1 b2 b3 b4 b5 b6 bn
Set this parameter in accordance with the I/O device specifications. 0: Not add a parity bit in I/O mode 1: Add a parity bit in I/O mode
#9505 DEV4 EVEN PARITY Select whether even or odd parity will be used when parity is used. This parameter is ignored when no parity is added. 0: Odd parity 1: Even parity
#9506 DEV4 CHR. LENGTH Select the length of the data bit. Refer to "#9504 DEV4 PARITY CHECK". 0: 5 (bit) 1: 6 2: 7 (NC connection not supported) 3: 8
#9507 DEV4 TERMINATR TYP Select the code to terminate data reading. 0. 3: EOR 1, 2: EOB or EOR
#9508 DEV4 HAND SHAKE Select the transmission control method. No handshaking will be used when a value except 1 to 3 is set. 1: RTS/CTS method 2: No handshaking 3: DC code method
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 175
#9509 DEV4 DC CODE PRTY Select the DC code type when the DC code method is selected. 0: Not add parity to DC code (DC3 = 13H) 1: Add parity to DC code (DC3 = 93H)
#9511 DEV4 DC2/4 OUTPUT Select the DC code handling when outputting data to the output device. DC2 / DC4 0: None / None 1: Yes / None 2: None / Yes 3: Yes / Yes
#9512 DEV4 CR OUTPUT Select whether to add the (CR) code just before the EOB (L/F) code during output. 0: Not add 1: Add
#9513 DEV4 EIA OUTPUT Select ISO or EIA code for data output. In data input mode, the ISO and EIA codes are identified automatically. 0: ISO code output 1: EIA code output
#9514 DEV4 FEED CHR. Set the length of the tape feed to be output at the start and end of the data during tape output. 0 to 999 (characters)
#9515 DEV4 PARITY V Select whether to perform the parity check for the number of characters in a block at the input of data. At the output of data, the number of characters is always adjusted to for the parity check. 0: Not perform parity V check 1: Perform parity V check
#9516 DEV4 TIME-OUT (sec) Set the time out time to detect an interruption in communication. Time out check will not be executed when set to "0". 0 to 30 (s)
#9517 DEV4 DR OFF Select whether to enable the DR data check in data I/O mode. 0: Enable 1: Disable
#9518 DEV4 DATA ASCII Select the code of the output data. 0: ISO/EIA code (Depends on whether #9113, #9213, #9313, #9413 or #9513 EIA output parameter is set up.) 1: ASCII code
#9519 DEV4 INPUT TYPE Select the mode for input (verification). 0: Standard input (Data from the very first EOB is handled as significant information.) 1: EOBs following the first EOB of the input data are skipped until data other than EOB is input.
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 176
#9521 DEV4 EIA CODE [ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " [ ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9522 DEV4 EIA CODE ] Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " ] ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9523 DEV4 EIA CODE # Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "#". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9524 DEV4 EIA CODE Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9525 DEV4 EIA CODE = Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "=". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9526 DEV4 EIA CODE : Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code " : ". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
#9527 DEV4 EIA CODE $ Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "$". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
Appendix 9. User Parameter List 9.5 I/O Parameters
IV - 177
#9528 DEV4 EIA CODE ! Set the code in hexadecimal, which does not duplicate the existing EIA codes, for the special code "!". When output with EIA code, data can be output using the alternate code in which the special ISO code, not included in EIA, is specified. 0 to FF (hexadecimal)
Appendix 9. User Parameter List 9.6 Ethernet Parameters
IV - 178
9.6 Ethernet Parameters Set the parameters related to Ethernet input/output. After setting up the parameter (PR) listed in the table, turn OFF the NC power. To validate the parameter, turn ON the power again. When the Ethernet parameter setting is mistaken, NC screen might not be able to be displayed because the communication between the display unit and the control unit is disabled. When the communication between the display unit and the control unit has been disabled, the connectable control unit IP address list screen is displayed at NC startup. Reset the Ethernet parameter according to the "Appendix 8. IP Address Resetting Procedure at Disabled Network Communication [700 Series Only]".
11005,9701,9706 parameters:
When several TCP/IP drivers are installed and the IP address is set manually ("#9701 IP address automatic setting" is set to 0), the same setting will be made for all parameters.
9711 to 9781 parameters:
Set the server information required for using the Ethernet function. Server information for up to four units can be set.
#1926(PR) Grobal IP address IP address Set the main CPU's IP address. Set the NC IP address seen from an external source.
#1927(PR) Global Subnet mask Subnet mask Set the subnet mask for the IP address.
#1928(PR) Global Gateway Gateway Set the IP address for the gateway.
#1934(PR) Local IP address Set the HMI side CPU's IP address.
#1935(PR) Local Subnet mask Set the HMI side CPU's subnet mask.
#11005(PR) PC IP address IP address setting Set the IP address for the display unit or PC in which machining programs are stored. Set the IP address for the display unit on which the automatic power OFF will be executed. (Note) When "0.0.0.0" is input, "192.168.100.2" is automatically set. *This parameter is used only for 700 Series. PC subnet Set the subnet mask for the display unit or PC in which machining programs are stored. PC Gateway Set the gateway for the display unit or PC in which machining programs are stored.
#9701(PR) IP addr auto set The IP address is automatically assigned from the server. 0: Manual setting 1: Automatic setting (Note) When the automatic setting is selected, "#11005 PC IP address, PC Subnet, PC Gateway" will be invalid.
Appendix 9. User Parameter List 9.6 Ethernet Parameters
IV - 179
#9706 Host No. Select the No. of the host to be used from host 1 to host 4.
---Setting range--- 1 to 4 : Host No.
#9711 Host1 host name Set the host computer name. This parameter allows the NC to easily recognize the host computer on the network. Set the host computer's name (name registered in C:windowshosts) or the IP address. ---Setting example--- For host name: mspc160 For IP address: 150.40.0.111 (Note) Set the host computer's TCP/IP address if communication is not carried out correctly.
---Setting range--- 15 characters (alphanumeric) or less
#9712 Host1 user name Set the user name when logging into the host computer.
---Setting range--- 15 characters (alphanumeric) or less
#9713 Host1 password Set the password when logging into the host computer.
---Setting range--- 15 characters (alphanumeric) or less
#9714 Host1 directory Set the directory name of the host computer. The directory released to the client (NC unit) with the host computer's server is handled as root directory by the NC unit.
---Setting range--- 31 characters (alphanumeric) or less
#9715 Host1 host type Select the type of the host computer. 0: UNIX/PC automatic judgment 1: UNIX 2: PC (DOS) (Note) When "0" is set, the settings for the following parameters will be invalid. #9716 Wrd pos: name #9717 Wrd pos: size #9718 Wrd pos: Dir #9719 Wrd pos: cmnt #9720 Wrd num: cmnt
#9716 Host 1 Wrd pos: name Set the file name display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
Appendix 9. User Parameter List 9.6 Ethernet Parameters
IV - 180
#9717 Host 1 Wrd pos: size Set the size display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9718 Host 1 Wrd pos: Dir Set the
display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces. ---Setting range--- 0 to 100 0: Default value
#9719 Host 1 Wrd pos: cmnt Set the comment (date, time, etc.) display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9720 Host 1 Wrd num: cmnt Set the number of words to be displayed as a comment. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9721 Host 1 no total siz Set whether to display the total number of characters registered in the machining programs of host1 when displaying the file list. If there are many files in the directory to be referred to, the list can be updated quickly by setting "1". 0: Display 1: Not display
#9731 Host2 host name Set the host computer name. This parameter allows the NC to easily recognize the host computer on the network. Set the host computer's name (name registered in C:windowshosts) or the IP address. ---Setting example--- For host name: mspc160 For IP address: 150.40.0.111 (Note) Set the host computer's TCP/IP address if communication is not carried out correctly.
---Setting range--- 15 characters (alphanumeric) or less
#9732 Host2 user name Set the user name when logging into the host computer.
---Setting range--- 15 characters (alphanumeric) or less
#9733 Host2 password Set the password when logging into the host computer.
---Setting range--- 15 characters (alphanumeric) or less
Appendix 9. User Parameter List 9.6 Ethernet Parameters
IV - 181
#9734 Host2 directory Set the directory name of the host computer. The directory released to the client (NC unit) with the host computer's server is handled as the root directory by the NC unit.
---Setting range--- 31 characters (alphanumeric) or less
#9735 Host2 host type Select the type of the host computer. 0: UNIX/PC automatic judgment 1: UNIX 2: PC (DOS) (Note) When "0" is set, the settings for the following parameters will be invalid. #9736 Wrd pos: name #9737 Wrd pos: size #9738 Wrd pos: Dir #9739 Wrd pos: cmnt #9740 Wrd num: cmnt
#9736 Host 2 Wrd pos: name Set the file name display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9737 Host 2 Wrd pos: size Set the size display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9738 Host 2 Wrd pos: Dir Set the
display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces. ---Setting range--- 0 to 100 0: Default value
#9739 Host 2 Wrd pos: cmnt Set the comment (date, time, etc.) display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9740 Host 2 Wrd num: cmnt Set the number of words to be displayed as a comment. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
Appendix 9. User Parameter List 9.6 Ethernet Parameters
IV - 182
#9741 Host 2 no total siz Set whether to display the total number of characters registered in the machining programs of host1 when displaying the file list. If there are many files in the directory to be referred to, the list can be updated quickly by setting "1".
---Setting range--- 0: Display 1: Not display
#9751 Host3 host name Set the host computer name. This parameter allows the NC to easily recognize the host computer on the network. Set the host computer's name (name registered in C:windowshosts) or the IP address. ---Setting example--- For host name: mspc160 For IP address: 150.40.0.111 (Note) Set the host computer's TCP/IP address if communication is not carried out correctly.
---Setting range--- 15 characters (alphanumeric) or less
#9752 Host3 user name Set the user name when logging into the host computer.
---Setting range--- 15 characters (alphanumeric) or less
#9753 Host3 password Set the password when logging into the host computer.
---Setting range--- 15 characters (alphanumeric) or less
#9754 Host3 directory Set the directory name of the host computer. The directory released to the client (NC unit) with the host computer's server is handled as the root directory by the NC unit.
---Setting range--- 31 characters (alphanumeric) or less
#9755 Host3 host type Select the type of the host computer. 0: UNIX/PC automatic judgment 1: UNIX 2: PC (DOS) (Note) When "0" is set, the settings for the following parameters will be invalid. #9756 Wrd pos: name #9757 Wrd pos: size #9758 Wrd pos: Dir #9759 Wrd pos: cmnt #9760 Wrd num: cmnt
#9756 Host 3 Wrd pos: name Set the file name display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
Appendix 9. User Parameter List 9.6 Ethernet Parameters
IV - 183
#9757 Host 3 Wrd pos: size Set the size display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9758 Host 3 Wrd pos: Dir Set the
display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces. ---Setting range--- 0 to 100 0: Default value
#9759 Host 3 Wrd pos: cmnt Set the comment (date, time, etc.) display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9760 Host 3 Wrd num: cmnt Set the number of words to be displayed as a comment. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9761 Host 3 no total siz Set whether to display the total number of characters registered in the machining programs of host1 when displaying the file list. If there are many files in the directory to be referred to, the list can be updated quickly by setting "1".
---Setting range--- 0: Display 1: Not display
#9771 Host4 host name Set the host computer name. This parameter allows the NC to easily recognize the host computer on the network. Set the host computer's name (name registered in C:windowshosts) or the IP address. ---Setting example--- For host name: mspc160 For IP address: 150.40.0.111 (Note) Set the host computer's TCP/IP address if communication is not carried out correctly.
---Setting range--- 15 characters (alphanumeric) or less
#9772 Host4 user name Set the user name when logging into the host computer.
---Setting range--- 15 characters (alphanumeric) or less
Appendix 9. User Parameter List 9.6 Ethernet Parameters
IV - 184
#9773 Host4 password Set the password when logging into the host computer.
---Setting range--- 15 characters (alphanumeric) or less
#9774 Host4 directory Set the directory name of the host computer. The directory released to the client (NC unit) with the host computer's server is handled as the root directory by the NC unit.
---Setting range--- 31 characters (alphanumeric) or less
#9775 Host4 host type Select the type of the host computer. 0: UNIX/PC automatic judgment 1: UNIX 2: PC (DOS) (Note) When "0" is set, the settings for the following parameters will be invalid. #9776 Wrd pos: name #9777 Wrd pos: size #9778 Wrd pos: Dir #9779 Wrd pos: cmnt #9780 Wrd num: cmnt
#9776 Host 4 Wrd pos: name Set the file name display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9777 Host 4 Wrd pos: size Set the size display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9778 Host 4 Wrd pos: Dir Set the
display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces. ---Setting range--- 0 to 100 0: Default value
#9779 Host 4 Wrd pos: cmnt Set the comment (date, time, etc.) display position (nth word from left) of the list displayed when the ftp command "dir" is executed. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
Appendix 9. User Parameter List 9.6 Ethernet Parameters
IV - 185
#9780 Host 4 Wrd num: cmnt Set the number of words to be displayed as a comment. (Note) One word designates a character string divided by one or more spaces.
---Setting range--- 0 to 100 0: Default value
#9781 Host 4 no total siz Set whether to display the total number of characters registered in the machining programs of host1 when displaying the file list. If there are many files in the directory to be referred to, the list can be updated quickly by setting "1".
---Setting range--- 0: Display 1: Not display
(Note 1) The user name and password are required when logging in. (Note 2) It is necessary to enable reading/writing when exchanging files. (Note 3) With the Personal WEB Server and Windows NT 4.0 fpt Server, the file list format can be selected
from DOS or UNIX. (Note 4) The directory released to the client (NC unit) with the host computer's server is handled as the root
directory by the NC unit.
Appendix 9. User Parameter List 9.7 Computer Link Parameters
IV - 186
9.7 Computer Link Parameters
#9601 BAUD RATE Select the rate at which data is transferred.
---Setting range--- 0: 19200 (bps) 1: 9600 2: 4800 3: 2400 4: 1200 5: 600 6: 300 7: 110 8: 38400
#9602 STOP BIT Select the stop bit length used in the start-stop system. Refer to "#9603 PARITY EFFECTIVE". At the output of data, the number of characters is always adjusted to for the parity check. 1: 1 (bit) 2: 1.5 3: 2
#9603 PARITY EFFECTIVE Select whether to add the parity bit to the data. The parameter is set when using a parity bit separately from the data bit.
ON OFF
Start bit Data bit Parity bit Stop bit
1 character
b1 b2 b3 b4 b5 b6 bn
Set this parameter according to the specifications of input/output device. 0: Not add a parity bit at the input/output 1: Add a parity bit at the input/output
#9604 EVEN PARITY Select odd or even when parity is added to the data. This parameter is ignored when no parity is added. 0: Odd parity 1: Even parity
#9605 CHR. LENGTH Select the length of the data bit. Refer to "#9603 PARITY EFFECTIVE". 0: 5 (bit) 1: 6 2: 7 (NC connection not supported) 3: 8
#9606 HAND SHAKE Select the transmission control method. "3" (DC code method) should be set for computer link B. 0: No control 1: RTS/CTS method 2: No handshaking 3: DC code method
Appendix 9. User Parameter List 9.7 Computer Link Parameters
IV - 187
#9607 TIME-OUT SET Set the time-out time at which an interruption of data transfer during data input/output should be detected. "0" means infinite time-out.
---Setting range--- 0 to 999 (1/10s)
#9608 DATA CODE Set the code to be used for the data description. Refer to "#9603 PARITY EFFECTIVE". 0: ASCII code 1: ISO code
#9609 LINK PARAM. 1
bit1: DC1 output after NAK or SYN Select whether to output the DC1 code after the NAK or SYN code is output. 0: Not output the DC1 code. 1: Output the DC1 code.
bit7: Enable/disable resetting Select whether to enable the resetting in the computer link. 0: Enable 1: Disable
#9610 LINK PARAM. 2
Bit 2: Specify the control code parity (even parity for the control code). Select whether to add an even parity to the control code, in accordance with the I/O device specifications. 0: Not add a parity bit to the control code 1: Add a parity bit to the control code
Bit 3: Parity V Select whether to enable checking of parity V in one block at the input of the data. 0: Disable 1: Enable
#9611 Link PARAM. 3 Not used. Set to "0".
#9612 Link PARAM. 4 Not used. Set to 0.
#9613 Link PARAM. 5 Not used. Set to 0.
#9614 START CODE Select the code used to command the first transfer of file data. This parameter is used for a specific user. Normally set "0". 0: DC1 (11H) 1: BEL (07H)
Appendix 9. User Parameter List 9.7 Computer Link Parameters
IV - 188
#9615 CTRL. CODE OUT
bit 0: NAK output Select whether to send the NAK code to the host if a communication error occurs in computer link B. 0: Not output the NAK code 1: Output the NAK code.
bit 1: SYN output Select whether to send the SYN code to the host if NC resetting or an emergency stop occurs in computer link B. 0: Not output the SYN code. 1: Output the SYN code.
bit 3: DC3 output Select whether to send the DC3 code to the host when the communication ends in computer link B. 0: Not output the DC3 code. 1: Output the DC3 code.
#9616 CTRL. INTERVAL Not used. Set to 0.
#9617 WAIT TIME Not used. Set to 0.
#9618 PACKET LENGTH Not used. Set to 0.
#9619 BUFFER SIZE Not used. Set to 0.
#9620 START SIZE Not used. Set to 0.
#9621 DC1 OUT SIZE Not used. Set to 0.
#9622 POLLING TIMER Not used. Set to 0.
#9623 TRANS. WAIT TMR Not used. Set to 0.
#9624 RETRY COUNTER Not used. Set to 0.
Appendix 9. User Parameter List 9.8 Subprogram Storage Destination Parameters
IV - 189
9.8 Subprogram Storage Destination Parameters
#8880 Subpro stor D0: dev Select the storage destination (device) for the subprogram. When D0 is designated at a subprogram call, the subprogram to be called will be searched from the device selected with this parameter. (Example) The following will be searched: M98 P (program No.), D0 Device: "#8880 Subpro stor D0: dev" device Directory: "#8881 Subpro stor D0: dir" directory (Note 1) When the called subprogram is not found in the selected storage destination, a program error will occur. (Note 2) When D0 to D4 is not designated at a subprogram call, the subprogram will be searched from the memory.
---Setting range--- Device name
Setting value Display name M Memory G HD F FD R Memory card D Data server E Ethernet
#8881 Subpro stor D0: dir Select the storage destination (directory) for the subprogram. When D0 is designated at a subprogram call, the subprogram to be called will be searched from the directory selected with this parameter. Refer to "#8880 Subpro stor D0: dev".
---Setting range--- Directory 48 characters
#8882 Subpro stor D1: dev Select the storage destination (device) for the subprogram. When D1 is designated at a subprogram call, the subprogram to be called will be searched from the device selected with this parameter. (Example) The following will be searched: M98 P (program No.), D1 Device: "#8882 Subpro stor D1: dev" device Directory: "#8883 Subpro stor D1: dir" directory (Note 1) When the called subprogram is not found in the selected storage destination, a program error will occur. (Note 2) When D0 to D4 is not designated at a subprogram call, the subprogram will be searched from the memory.
---Setting range--- Setting value Display name
M Memory G HD F FD R Memory card D Data server E Ethernet
Appendix 9. User Parameter List 9.8 Subprogram Storage Destination Parameters
IV - 190
#8883 Subpro stor D1: dir Select the storage destination (directory) for the subprogram. When D1 is designated at a subprogram call, the subprogram to be called will be searched from the directory selected with this parameter. Refer to "#8882 Subpro stor D1: dev".
---Setting range--- Directory 48 characters
#8884 Subpro stor D2: dev Select the storage destination (device) for the subprogram. When D2 is designated at a subprogram call, the subprogram to be called will be searched from the device selected with this parameter. (Example) The following will be searched: M98 P (program No.), D2 Device: "#8884 Subpro stor D2: dev" device Directory: "#8885 Subpro stor D2: dir" directory (Note 1) When the called subprogram is not found in the selected storage destination, a program error will occur. (Note 2) When D0 to D4 is not designated at a subprogram call, the subprogram will be searched from the memory.
---Setting range--- Setting value Display name
M Memory G HD F FD R Memory card D Data server E Ethernet
#8885 Subpro stor D2: dir Select the storage destination (directory) for the subprogram. When D2 is designated at a subprogram call, the subprogram to be called will be searched from the directory selected with this parameter. Refer to "#8884 Subpro stor D2: dev".
---Setting range--- Directory 48 characters
Appendix 9. User Parameter List 9.8 Subprogram Storage Destination Parameters
IV - 191
#8886 Subpro stor D3: dev Select the storage destination (device) for the subprogram. When D3 is designated at a subprogram call, the subprogram to be called will be searched from the device selected with this parameter. (Example) The following will be searched: M98 P (program No.), D3 Device: "#8886 Subpro stor D3: dev" device Directory: "#8887 Subpro stor D3: dir" directory (Note 1) When the called subprogram is not found in the selected storage destination, a program error will occur. (Note 2) When D0 to D4 is not designated at a subprogram call, the subprogram will be searched from the memory.
---Setting range--- Setting value Display name
M Memory G HD F FD R Memory card D Data server E Ethernet
#8887 Subpro stor D3: dir Select the storage destination (directory) for the subprogram. When D3 is designated at a subprogram call, the subprogram to be called will be searched from the directory selected with this parameter. Refer to "#8886 Subpro stor D3: dev".
---Setting range--- Directory 48 characters
#8888 Subpro stor D4: dev Select the storage destination (device) for the subprogram. When D4 is designated at a subprogram call, the subprogram to be called will be searched from the device selected with this parameter. (Example) The following will be searched: M98 P (program No.), D4 Device: "#8888 Subpro stor D4: dev" device Directory: "#8889 Subpro stor D4: dir" directory (Note 1) When the called subprogram is not found in the selected storage destination, a program error will occur. (Note 2) When D0 to D4 is not designated at a subprogram call, the subprogram will be searched from the memory.
---Setting range--- Device name
Setting value Display name M Memory G HD F FD R Memory card D Data server E Ethernet
Appendix 9. User Parameter List 9.8 Subprogram Storage Destination Parameters
IV - 192
#8889 Subpro stor D4: dir Select the storage destination (directory) for the subprogram. When D4 is designated at a subprogram calling, the subprogram to be called will be searched from the directory selected with this parameter. Refer to "#8888 Subpro stor D4: dev".
---Setting range--- Directory 48 characters
Appendix 9. User Parameter List 9.9 Axis Parameters
IV - 193
9.9 Axis Parameters
Set up the parameter required for each axis.
#1063 mandog Manual dog-type Select the manual reference position return method for the second return (after the coordinate system is established) and later. The initial reference position return after the power ON is performed with dog-type return, and the coordinate system will be established. (This setting is not required when the absolute position detection is used.)
0: High speed return 1: Dog-type
#8201 AX. RELEASE Select the function to remove the control axis from the control target. 0: Control as normal. 1: Remove from control target.
#8202 OT-CHECK OFF Select whether to enable the stored stroke limit II function set in #8204 and #8205. 0: Enable 1: Disable
#8203 OT-CHECK-CANCEL When the simple absolute position method ("#2049 type" is "9") is selected, the stored stroke limits I, II (or IIB) and IB can be disabled until the first reference position return is executed after the power is turned ON. 0: Enable (according to #8202) 1: Temporarily cancel (Note) "#8203 OT-CHECK-CANCEL" affects all the stored stroke limits.
#8204 OT-CHECK-N Set the coordinates of the (-) direction in the movable range of the stored stroke limit II or the lower limit coordinates of the prohibited range of stored stroke limit IIB. If the sign and value are the same as #8205, the stored stroke limit II (or IIB) will be invalid. If the stored stroke limit IIB function is selected, the prohibited range will be between two points even when #8204 and #8205 are set in reverse. When II is selected, the entire range will be prohibited if #8204 and #8205 are set in reverse.
---Setting range--- 99999.999 (mm)
#8205 OT-CHECK-P Set the coordinates of the (+) direction in the movable range of the stored stroke limit II or the upper limit coordinates of the prohibited range of stored stroke limit IIB.
---Setting range--- 99999.999 (mm)
#8206 TOOL CHG. P Set the coordinates of the tool change position for G30. n (tool change position return). Set with coordinates in the basic machine coordinate system.
---Setting range--- 99999.999 (mm)
#8207 G76/87 IGNR for M system only Select whether to enable the shift operation at G76 (fine boring) and G87 (back boring). 0: Enable 1: Disable
Appendix 9. User Parameter List 9.9 Axis Parameters
IV - 194
#8208 G76/87 (-) for M system only Select the shift direction at G76 and G87. 0: Shift to (+) direction 1: Shift to (-) direction
#8209 G60 SHIFT for M system only Set the last positioning direction and distance for a G60 (unidirectional positioning) command.
---Setting range--- 99999.999 (mm)
#8210 OT INSIDE Select whether the stored stoke limit function set by #8204 and #8205 prevents the machine from moving to the inside or outside of the specified range. 0: Inhibits outside area (Select stored stroke limit II.) 1: Inhibits inside area (Select stored stroke limit II B.)
#8211 MIRR. IMAGE Select whether to enable the parameter mirror image function. 0: Disable 1: Enable
Appendix 9. User Parameter List 9.9 Axis Parameters
IV - 195
#8213(PR) Rotation axis type Select the rotation type (short-cut valid/invalid) or linear type (workpiece coordinate linear type/all coordinate linear type). This parameter is enabled only when "#1017 rot" is set to "1". (Note) 0: Short-cut invalid 1: Short-cut valid 2: Workpiece coordinate linear type 3: All coordinate linear type (Note) The movement method is as follows by the specified rotation axis type.
Setting value 0 1 2 3 Workpiece
coordinate value
Machine coordinate
value/relative position
Display range: 0 to 99999.999
ABS command The incremental amount from the end point to the current position is divided by 360, and the axis moves by the remainder amount according to the sign.
Moves with a short-cut to the end point.
INC command
Moves and returns in the reference position direction for the difference from the current position to the reference position.
Display range: 0 to 359.999 Display range: 0 to 99999.999
Display range: 0 to 359.999
Reference position return
In the same manner as the normal linear axis, moves according to the sign by the amount obtained by subtracting the current position from the end point.
Moves in the direction of the commanded sign by the commanded incremental amount starting at the current position.
The movement to the middle point applies to the ABS command or the INC command. Returns with movement within 360 degrees from the middle point to reference position.
#8215 TLM std length Set the TLM standard length. TLM standard length is the distance from a tool replacement point (reference position) to the measurement basic point (surface) which is used to measure the tool length.
---Setting range--- -99999.999 to 99999.999 (mm)
#8216 Type in G28 return Select the performance after establishing the reference position in reference position return command. 0: Moves to the reference position. 1: Won't move to the reference position.
#8217 Check start point Set a drawing start position in graphic check of each axis.
---Setting range--- -99999.999 to 99999.999 (mm)
Appendix 9. User Parameter List 9.10 Barrier Data (For L System Only)
IV - 196
9.10 Barrier Data (For L System Only)
#8300 P0 Set the reference X-coordinates of the chuck and the tail stock barrier. Set the center coordinate (radius value) of workpiece by the basic machine coordinate system.
---Setting range--- 99999.999 (mm)
#8301 P1 Set the area of the chuck and tail stock barrier. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
#8302 P2 Set the area of the chuck and tail stock barrier. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
#8303 P3 Set the area of the chuck and tail stock barrier. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
#8304 P4 Set the area of the chuck and tail stock barrier. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
#8305 P5 Set the area of the chuck and tail stock barrier. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
#8306 P6 Set the area of the chuck and tail stock barrier. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
#8311 P7 Set the area of the left spindle section. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
Appendix 9. User Parameter List 9.10 Barrier Data (For L System Only)
IV - 197
#8312 P8 Set the area of the left spindle section. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
#8313 P9 Set the area of the right spindle section. X axis: Set the coordinate from the workpiece center (P0). (radius value) Z axis: Set the coordinates in the basic machine coordinate system.
---Setting range--- 99999.999 (mm)
#8314 P10 Set the area of the right spindle section. Set the coordinate from the center of workpiece (P0) for X-axis. (radius value) Set the coordinate value by basic machine coordinate system for Z-axis.
---Setting range--- 99999.999 (mm)
#8310 Barrier ON Select whether to enable the chuck and tailstock barrier. 0: Disable (Setting from special display unit will be enabled) 1: Enable
#8315 Barrier Type (L) Select the shape of the left chuck and tailstock barrier. 0: No area 1: Chuck 2: Tailstock
#8316 Barrier Type (R) Select the shape of the right chuck and tailstock barrier. 0: No area 1: Chuck 2: Tailstock
#8317 ELIV. AX. Name Set the name of the delivery axis when the right chuck and tailstock barrier is movable. When using the multi-part system method and the delivery axis is an axis in the other part system, designate the axis including the part system as 1A, 1B or 2A, 2B. If the part system is not designated as A and B, the set part system will be used.
---Setting range--- A/B/.. (axis name) 1A/1B/.. 2A/2B/.. (with part system designated) 0: Cancel
#8318 Stock Angle (L) Set the angle for the left tailstock end section. The angle will be interpreted as 90 if there is no setting (when "0" is set).
---Setting range--- 0 to 180 () 0: 90 (default)
Appendix 9. User Parameter List 9.10 Barrier Data (For L System Only)
IV - 198
#8319 Stock Angle (R) Set the angle for the right tailstock end section. The angle will be interpreted as 90 if there is no setting (when "0" is set).
---Setting range--- 0 to 180 () 0: 90 (default)
Appendix 9. User Parameter List 9.11 High Accuracy Parameters
IV - 199
9.11 High Accuracy Parameters
#1149 cireft Arc deceleration speed change Select whether to decelerate at the arc entrance or exit.
0: Not decelerate 1: Decelerate
#1205 G0bdcc Acceleration and deceleration before G0 interpolation 0: Post-interpolation acceleration/deceleration is applied to G00. 1: Pre-interpolation acceleration/deceleration is applied to G00 even in the high accuracy control mode. 2: Rapid traverse constant inclination multi-step acceleration/deceleration is enabled.
(Note) "1" cannot be set for the 2nd part system and the following.
#1206 G1bF Maximum speed Set a cutting feedrate when applying pre-interpolation acceleration/deceleration. When high-accuracy control time constant expansion is valid, set the maximum of cutting feed clamp speed of each axis.
---Setting range--- 1 to 999999 (mm/min)
#1207 G1btL Time constant Set a cutting feed time constant when applying pre-interpolation acceleration/deceleration. When "0" is set, the time constant will be clamped at 1ms.
G1bF
G1btL Time
Speed
---Setting range---
Without high-accuracy control time constant expansion : 0 to 5000 (ms) With high-accuracy control time constant expansion : 0 to 30000 (ms)
#1209 cirdcc Arc deceleration speed Set the deceleration speed at the arc entrance or exit.
---Setting range--- 1 to 999999 (mm/min)
#1568 SfiltG1 G01 soft acceleration/deceleration filter Set the filter time constant for smoothly changing the acceleration rate for the cutting feed acceleration/deceleration in pre-interpolation acceleration/deceleration.
---Setting range--- 0 to 200 (ms)
#1569 SfiltG0 G00 soft acceleration/deceleration filter Set the filter time constant for smoothly changing the acceleration rate for the rapid traverse acceleration/deceleration in pre-interpolation acceleration/deceleration.
---Setting range--- 0 to 200 (ms)
Appendix 9. User Parameter List 9.11 High Accuracy Parameters
IV - 200
#1570 Sfilt2 Soft acceleration/deceleration filter 2 Set the filter time constant for smoothly changing the acceleration rate in pre-interpolation acceleration/deceleration. This will be invalid when "0" or "1" is set.
---Setting range--- 0 to 26 (ms)
#1571 SSSdis SSS control adjustment coefficient fixed value selection Fix the shape recognition range for SSS control.
(High-accuracy control)
#8019 R COMP Set a compensation coefficient for reducing a control error in the reduction of a corner roundness and arch radius. The larger the setup value, the smaller the theoretical error will be. However, since the speed at the corner will go down, the cycle time will be extended. Coefficient = 100 - setting value (Note) This is valid when "#8021 COMP CHANGE" is set to "0".
---Setting range--- 0 to 99 (%)
Theor R decrease The value calculated with the following data is displayed for the theoretical radius reduction error amount R (mm).
+
Command path
Path after servo control
R
F
Theoretical radius reduction amount at arc center
#8020 DCC. angle Set up the minimum value of an angle (external angle) that should be assumed to be a corner. When an inter-block angle (external angle) in high-accuracy mode is larger than the set value, it will be determined as a corner and the speed will go down to sharpen the edge.
If the set value is smaller than , the speed goes down to optimize the corner.
(Note) If "0" is set, it will be handled as 5 degrees.
---Setting range--- 0 to 89 (degrees) 0: The angle will be 5.
Appendix 9. User Parameter List 9.11 High Accuracy Parameters
IV - 201
#8021 COMP_CHANGE Select whether to share or separate the compensation coefficient at the corner/curve during the high-accuracy control mode. 0: Share ("#8019 R COMP" is applied.) 1: Separate Corner : #8022 CORNER COMP Curve : #8023 CURVE COMP (Note) Set "1" when using SSS control.
#8022 CORNER COMP Set the compensation coefficient to further reduce or increase the roundness at the corner during the high-accuracy control mode. Coefficient = 100 - setting value (Note) This is valid when "#8021 COMP CHANGE" is set to "1".
---Setting range--- -1000 to 99 (%)
#8023 CURVE COMP Set the compensation coefficient to further reduce or increase the radius reduction amount at the curve (arc, involute, spline) during the high-accuracy control mode. Coefficient = 100 - setting value (Note) This is valid when "#8021 COMP CHANGE" is set to "1". For theoretical radius reduction error amount, refer to "Theor R decrease" in "#8019 R COMP"
---Setting range--- -1000 to 99 (%)
(High-accuracy spline)
#8025 SPLINE ON for M system only Select whether to enable the spline function. 0: Disable 1: Enable Spline interpolation is valid during G61.2 modal, regardless of this setting.
#8026 CANCEL ANG. for M system only Set the angle where the spline interpolation is temporarily canceled. When the angle made by blocks exceeds this parameter setting value, spline interpolation will be canceled temporarily. In consideration of the pick feed, set a value a little smaller than the pick feed angle.
---Setting range--- 0 to 180 () 0: 180 ()
#8027 Toler-1 for M system only Set the maximum chord error (tolerance) in a block that includes an inflection point. Set the tolerance applicable when the applicable block is developed to fine segments by CAM. (normally about 10 m) When "0.000" is set, the applicable block will be linear.
---Setting range--- 0.000 to 100.000 (mm)
#8028 Toler-2 for M system only Set the maximum chord error (tolerance) in a block that includes no inflection point. Set the tolerance applicable when the applicable block is developed to fine segments by CAM. (normally about 10 m) When "0.000" is set, the applicable block will be linear.
---Setting range--- 0.000 to 100.000 (mm)
Appendix 9. User Parameter List 9.11 High Accuracy Parameters
IV - 202
#8029 FairingL for M system only Set the length of the block subject to fairing. (Enabled when "#8033 Fairing ON" is set to "1".)
---Setting range--- 0 to 100.000 (mm)
#8030 MINUTE LENGS for M system only Set the fine-segment length where the spline interpolation is temporarily canceled. When the length of one block exceeds this parameter setting value, spline interpolation is canceled temporarily and linear interpolation is performed. Set a value a little smaller than one block length of the program. If "-1" is set, spline interpolation will be performed regardless of block length.
---Setting range--- -1 to 127 (mm) 0: 1 (mm)
#8033 Fairing ON for M system only Select whether to use the fairing function. 0: Not use 1: Use Fairing function is enabled during G61.2 modal, regardless of this setting.
#8034 AccClamp ON for M system only Select the method for clamping the cutting speed. 0: Clamp with parameter "#2002 clamp" or the corner deceleration function. 1: Clamp the cutting speed with acceleration judgment. (Enabled when "#8033 Fairing ON" is set to "1".)
#8036 CordecJudge for M system only Select the condition to decide a corner. 0: A corner is decided from the angle of the neighboring block. 1: A corner is decided from the angle of the neighboring block, excluding minute blocks. (Enabled when "#8033 Fairing ON" is set to "1".)
#8037 CorJudgeL for M system only Set the length of the block to be excluded when deciding a corner. (Enabled when "#8036 CordecJudge" is set to "1".)
---Setting range--- 0 to 99999.999 (mm)
#8090 SSS ON for M system only Set whether to enable the SSS control with G05 P10000. 0: Disable 1: Enable
#8091 StdLength for M system only Set the maximum value of the range for recognizing the shape. To eliminate the effect of steps or errors, etc., set a large value. To enable sufficient deceleration, set a small value. If "0.000" is set, the standard value (1.000mm) will be applied.
---Setting range--- 0 to 100.000 (mm)
Appendix 9. User Parameter List 9.11 High Accuracy Parameters
IV - 203
#8092 ClampCoeff for M system only Set the clamp speed at the curved section configured of fine segments. Coefficient = setting value
---Setting range--- 1 to 100
#8093 StepLeng for M system only Set the width of the step at which the speed is not to be decelerated. (Approximately the same as the CAM path difference [Tolerance].) If "0" is set, the standard value (5m) will be applied. If a minus value is set, the speed will decelerate at all minute steps.
---Setting range--- -1.000 to 0.100 (mm)
#8094 DccWaitAdd for M system only Set the time to wait for deceleration when the speed FB does not drop to the clamp speed.
---Setting range--- 0 to 100 (ms)
Appendix 9. User Parameter List 9.12 High-accuracy Axis Parameters
IV - 204
9.12 High-accuracy Axis Parameters
#2001 rapid Rapid traverse rate Set the rapid traverse feedrate for each axis. (Note) The maximum value to be set depends on the machine specifications.
---Setting range--- 1 to 1000000 (mm/min)
#2002 clamp Cutting feedrate for clamp function Set the maximum cutting feedrate for each axis. Even if the feedrate in G01 exceeds this value, the clamp will be applied at this feedrate.
---Setting range--- 1 to 1000000 (mm/min)
#2010 fwd_g Feed forward gain Set a feed forward gain for pre-interpolation acceleration/deceleration. The larger the set value, the smaller the theoretical control error will be. However, if a machine vibration occurs, set the smaller value.
---Setting range--- 0 to 200 (%)
#2068 G0fwdg G00 feed forward gain Set a feed forward gain for G00 pre-interpolation acceleration/deceleration. The larger the setting value, the shorter the positioning time during in-position checking. If a machine vibration occurs, set the smaller value.
---Setting range--- 0 to 200 (%)
#2096 crncsp Minimum corner deceleration speed Set the minimum clamp speed for corner deceleration in the high-accuracy control mode. Normally set "0". (Note) This parameter is invalid during SSS control.
---Setting range--- 0 to 1000000 (mm/min)
#2109 Rapid (H-precision) Rapid traverse rate for high-accuracy control mode Set the rapid traverse rate for each axis in the high-accuracy control mode. "#2001 rapid" will be used when "0" is set.
---Setting range--- 0 to 1000000 (mm/min)
#2110 Clamp (H-precision) Cutting feed clamp speed for high-accuracy control mode Set the cutting feed maximum speed for each axis in the high-accuracy control mode. "#2002 clamp" will be used when "0" is set.
---Setting range--- 0 to 1000000 (mm/min)
Appendix 9. User Parameter List 9.13 Operation Parameters
IV - 205
9.13 Operation Parameters
#8901 Counter type 1 Set the type of counter displayed at the upper left of the AUTO/MDI display on the Monitor screen. 1: Current position 2: Work coordinate position 3: Machine position 4: Program position 8: Remain command 9: Manual interrupt amount 10: Next command 11: Restart position 12: Remain distance 16: Tip work coordinate position 18: Tool axis movement 19: Tip machine position 20: Relative position
---Setting range--- 0 to 255
#8902 Counter type 2 Set the type of counter displayed at the lower left of the AUTO/MDI display on the Monitor screen. 1: Current position 2: Work coordinate position 3: Machine position 4: Program position 8: Remain command 9: Manual interrupt amount 10: Next command 11: Restart position 12: Remain distance 16: Tip work coordinate position 18: Tool axis movement 19: Tip machine position 20: Relative position
---Setting range--- 0 to 255
#8903 Counter type 3 Set the type of counter displayed at the upper right of the AUTO/MDI display on the Monitor screen. 1: Current position 2: Work coordinate position 3: Machine position 4: Program position 8: Remain command 9: Manual interrupt amount 10: Next command 11: Restart position 12: Remain distance 16: Tip work coordinate position 18: Tool axis movement 19: Tip machine position 20: Relative position
---Setting range--- 0 to 255
Appendix 9. User Parameter List 9.13 Operation Parameters
IV - 206
#8904 Counter type 4 Set the type of counter displayed at the lower right of the AUTO/MDI display on the Monitor screen. 1: Current position 2: Work coordinate position 3: Machine position 4: Program position 8: Remain command 9: Manual interrupt amount 10: Next command 11: Restart position 12: Remain distance 16: Tip work coordinate position 18: Tool axis movement 19: Tip machine position 20: Relative position
---Setting range--- 0 to 255
#8905 Counter type 5 Set the type of counter displayed at the left of the Manual display on the Monitor screen. 1: Current position 2: Work coordinate position 3: Machine position 4: Program position 8: Remain command 9: Manual interrupt amount 10: Next command 11: Restart position 12: Remain distance 16: Tip work coordinate position 18: Tool axis movement 19: Tip machine position 20: Relative position
---Setting range--- 0 to 255
#8906 Counter type 6 Set the type of counter displayed at the right of the Manual display on the Monitor screen. 1: Current position 2: Work coordinate position 3: Machine position 4: Program position 8: Remain command 9: Manual interrupt amount 10: Next command 11: Restart position 12: Remain distance 16: Tip work coordinate position 18: Tool axis movement 19: Tip machine position 20: Relative position
---Setting range--- 0 to 255
#8910 Edit undo Set whether to enable the Undo function during program edit on the Monitor screen or Edit screen. 0: Disable 1: Enable
Appendix 9. User Parameter List 9.13 Operation Parameters
IV - 207
#8914 Auto Top search Select the operation method for restart search type 2. 0: It is necessary to set the top search position arbitrarily. 1: The restart search is executed from O No. that is designated as head.
#8915 Auto backup day 1 When the NC power is ON after the designated date was passed over, the automatic backup is executed. When "-1" is set to "Auto backup day 1", the automatic backup is executed every turning NC power ON. When "0" is set to all on "Auto backup day 1" to "4", the automatic backup is not executed. It is possible to specify the designated date up to 4 days for a month.
---Setting range--- -1 to 31 ("-1" can be set for "Auto backup day 1" only.)
#8916 Auto backup day 2 When the NC power is ON after the designated date was passed over, the automatic backup is executed. When "-1" is set to "Auto backup day 1", the automatic backup is executed every turning NC power ON. When "0" is set to all on "Auto backup day 1" to "4", the automatic backup is not executed. It is possible to specify the designated date up to 4 days for a month.
---Setting range--- -1 to 31 ("-1" can be set for "Auto backup day 1" only.)
#8917 Auto backup day 3 When the NC power is ON after the designated date was passed over, the automatic backup is executed. When "-1" is set to "Auto backup day 1", the automatic backup is executed every turning NC power ON. When "0" is set to all on "Auto backup day 1" to "4", the automatic backup is not executed. It is possible to specify the designated date up to 4 days for a month.
---Setting range--- -1 to 31 ("-1" can be set for "Auto backup day 1" only.)
#8918 Auto backup day 4 When the NC power is ON after the designated date was passed over, the automatic backup is executed. When "-1" is set to "Auto backup day 1", the automatic backup is executed every turning NC power ON. When "0" is set to all on "Auto backup day 1" to "4", the automatic backup is not executed. It is possible to specify the designated date up to 4 days for a month.
---Setting range--- -1 to 31 ("-1" can be set for "Auto backup day 1" only.)
#8919 Auto backup device Select the automatic backup target device. *The setting range differs according to the model.
---Setting range--- [M700 Series] 0: DS 1: HD 2: Memory card [M70 Series] 0: Memory card
Appendix 9. User Parameter List 9.13 Operation Parameters
IV - 208
#8920 3D tool ofs select Select the method to calculate the drawing position when drawing a solid. With 3D drawing, the drawing position (tool tip position) is calculated with the method designated with this parameter, and the image is drawn. 0: Machine position tool shape setting window data 1: Machine position tool compensation amount 2: Machine position tool shape setting window data 3: Machine position tool shape setting window data
#8921 Mass Edit select Select the editing mode for the machining programs saved in HD, FD, and memory card. When the program size is 1.0MB (When "#8910 Edit Undo" is invalid, 2.0MB) or more, mass-editing will be applied. 0: Regular editing mode 1: Mass-editing mode
#8922 T-reg-dup check Set whether to enable the duplication check in registering tools to magazine pots, and in setting tool Nos. for spindle/standby. 0: Duplication check valid for all valid magazines 1: Duplication check invalid 2: Duplication check valid only for the selected magazine
#8923(PR) Hide Edit-IO menu Set whether to enable the edit-in/out menu. When disabled, the edit-input/output menu won't appear. However, the maintenance-in/out menu is always enabled regardless of this parameter setting. 0: Enable 1: Disable
#8924 MEAS. CONFIRM MSG Select whether to display a confirming message when attempting to write compensation data for tool measurement, or coordinate system data for workpiece measurement. 0: Not display a confirming message 1: Display a confirming message
#8925 SP on 1st part sys Set a spindle No. to be displayed on the 1st part system window when 2-part system simultaneous display is valid. High-order: Select an upper side spindle No. Low-order: Select a lower side spindle No. (Note 1) When "00" is set, spindles will be displayed in a default order (the 1st spindle on the upper side, the 2nd spindle on the lower side) (Note 2) If you designate a bigger number than the setting of "#1039 spinno", or either the high-order or low-order setting is "0", the 1st spindle will be displayed.
---Setting range--- High-order: 0 to 6 Low-order: 0 to 6
Appendix 9. User Parameter List 9.13 Operation Parameters
IV - 209
#8926 SP on 2nd part sys Set a spindle No. to be displayed on the 2nd part system window when 2-part system simultaneous display is valid. High-order: Select an upper side spindle No. Low-order: Select a lower side spindle No. (Note 1) When "00" is set, spindles will be displayed in a default order (the 1st spindle on the upper side, the 2nd spindle on the lower side) (Note 2) If you designate a bigger number than the setting of "#1039 spinno", or either the high-order or low-order setting is "0", the 1st spindle will be displayed.
---Setting range--- High-order: 0 to 6 Low-order: 0 to 6
#8927 SP on 3rd part sys Set a spindle No. to be displayed on the 3rd part system window when 2-part system simultaneous display is valid. High-order: Select an upper side spindle No. Low-order: Select a lower side spindle No. (Note 1) When "00" is set, spindles will be displayed in a default order (the 1st spindle on the upper side, the 2nd spindle on the lower side) (Note 2) If you designate a bigger number than the setting of "#1039 spinno", or either the high-order or low-order setting is "0", the 1st spindle will be displayed.
---Setting range--- High-order: 0 to 6 Low-order: 0 to 6
#8928 SP on 4th part sys Set a spindle No. to be displayed on the 4th part system window when 2-part system simultaneous display is valid. High-order: Select an upper side spindle No. Low-order: Select a lower side spindle No. (Note 1) When "00" is set, spindles will be displayed in a default order (the 1st spindle on the upper side, the 2nd spindle on the lower side) (Note 2) If you designate a bigger number than the setting of "#1039 spinno", or either the high-order or low-order setting is "0", the 1st spindle will be displayed.
---Setting range--- High-order: 0 to 6 Low-order: 0 to 6
Revision History
Date of revision Manual No. Revision details
Aug. 2004 IB(NA)1500042-A First edition created.
Mar. 2005 IB(NA)1500042-B Contents were revised to correspond to Mitsubishi CNC 700 Series software version B0.
The following sections were added to "I. SCREEN OPERATIONS": 1.1 Setting Display Unit Appearance 1.3 Screen Transition Diagram 1.4 Screen Selection Procedure 1.5 Setting Data 1.8 Guidance Function 2.2.2 Changing Whether to Show or Hide the Comment Field 2.3.5 Operation Sequence for Program Restart 2.5.8 Switching Full-screen Display Mode 2.16.2 Setting the Time Display Selection 2.22 Load Meter Display 2.23 Spindle, Standby Display 3.4.4 Erasing the Tool Registration Data 3.12 T Code List 4.2.17 G Code Guidance 4.3.8 Switching to Full-screen Display Mode 4.4.8 Switching to Full-screen Display Mode 5.7 Self Diagnosis Screen 5.8 Data Sampling Screen 6.3 All Backup Screen 6.4 System Setup Screen 6.5 Adjust S-analog Screen 6.6 Absolute Position Setting Screen 6.7 Auxiliary Axis Test Screen 6.8 Diagnosis Data Collection Setting Screen
The following section names were changed: "2.3.3 Directory change screen" -> "2.3.3 File Setting Screen" "5.1 Hardware and software configuration screen (H/W S/W config screen)" -> "5.1 System Configuration Screen "
The following sections were unified. "4.5.9 Formatting an FLD" and "4.5.10 Formatting a Memory card and DS" -> "4.5.9 Formatting an External Device " "6.2.9 Formatting an FLD" and "6.2.10 Formatting a Memory card and DS" -> "6.2.9 Formatting an External Device "
The configuration of "1. Operating the Setting and Display Unit" in "I. SCREEN OPERATIONS" was changed.
The following sections were added to " II. MACHINE OPERATIONS": 7. Stored Stroke Limit
"III. MAINTENANCE" was added. The following sections were added to " IV. APPENDIXES":
6.2.15 System setup-related operation messages 6.2.16 Automatic backup-related operation messages Appendix 7. G Code Guidance Display List
Mistakes were corrected.
Date of revision Manual No. Revision details
Sept. 2005 IB(NA)1500042-C Contents were revised to correspond to Mitsubishi CNC 700 Series software version B3.
The following sections were added to "I. SCREEN OPERATIONS": 1.8.2 Alarm Guidance 1.9 Touch Panel Functions 1.10 Touch Panel S/W Key 2.2.3 Changing the Sorting Method 3.3.1 Tool Measurement (M system) 3.3.2 Tool Measurement (L system) 3.7.4 Carrying Out Rotation Measurement 3.13 Pallet Program Registration 5.9 Anshin-net Screen
The following section was added to " IV. APPENDIXES": 6.2.17 Messages Related to Anshin-net
The following sections were changed to paragraph header: 3.3.1 Carrying Out Tool Length Measurement 3.3.2 Carrying Out Tool Radius Measurement
The following sections were deleted: 6.1.2 Selecting the Parameter No. 6.1.6 Machine Parameters
Mistakes were corrected.
Mar. 2006 IB(NA)1500042-D Contents were revised to correspond to Mitsubishi CNC 700 Series software version C0.
The following sections were added to "I. SCREEN OPERATIONS": 4.2.17 Adding Sequence No. (N No.) Automatically 4.2.19 Playback Editing 4.5.12 Program Display Lock C 5.6.1 Alarm History
Mistakes were corrected.
Sept. 2006 IB(NA)1500042-E Contents were revised to correspond to Mitsubishi CNC 700 Series software version D0.
The following sections were added to "I. SCREEN OPERATIONS": 1.5.2 Inputting Operations 1.11 Screen Saver (Backlight OFF) Function 2.25 All Spindles' Rotation Speed Display 3.7.2 Workpiece Measurement (L System) 4.5.14 Sharing Machining Data 5.9.4 Sharing Machining Data 5.10 Machine Tool Builder Network System (MTB net) Screen 6.2.13 Sharing Machining Data
The configuration of "3.2 Tool Measurement" was changed. The configuration of "3.7 Workpiece Measurement" was changed because
workpiece measurement (L system) is added. Mistakes were corrected.
Date of revision Manual No. Revision details
Aug. 2007 IB(NA)1500042-F Contents were revised to correspond to Mitsubishi CNC 700/70 Series software version E1.
The following sections were added to "I. SCREEN OPERATIONS": 1.12 Screen Capture [70 Series Only] 1.13 Multi-part System Program Management 4.5.15 The Batch Input/Output the Machining Program of NC Memory 6.2.14 The Batch Input/Output the Machining Program of NC Memory
The following sections were added to "II MACHINE OPERATIONS": 6.17 Tool retract return
The following sections were added to "III. MAINTENANCE": 1.2.4 How to Replace the Protective Sheet on the Touch Panel 1.3.3 How to Replace the Protective Sheet on the Touch Panel
Mistakes were corrected.
Dec. 2007 IB(NA)1500042-G Contents were revised to correspond to Mitsubishi CNC 700/70 Series software version E2.
The following sections were added to "I. SCREEN OPERATIONS": 1.10.2 Automatic Display of S/W Keyboard [70 Series Only] 2.1.3 Operation of 2-part System Simultaneous Display
The following sections were added to "III. MAINTENANCE": 5.3 Spindle Override 6.4 Z Axis Cancel 6.11 Mirror Image 6.15 F 1-digit Feed 6.19 Each Axis Machine Lock 6.22 External Deceleration 6.23 Reference Position Retract 6.24 Spindle Orientation 7.2 Chuck Barrier/Tailstock Barrier (L System) 7.3 Computer Link B 7.4 Manual Synchronous Tapping
The following sections were added to "IV. APPENDIXES": Appendix 8. IP Address Resetting Procedure at Disabled Network Communication [700 Series Only] Appendix 9. User Parameter List (Moved from "I. SCREEN OPERATIONS")
Mistakes were corrected.
Global service network
NORTH AMERICA FA Center EUROPEAN FA Center
ASEAN FA Center
CHINA FA Center
TAIWAN FA Center
HONG KONG FA Center
KOREAN FA Center
North America FA Center (MITSUBISHI ELECTRIC AUTOMATION INC.)
Illinois CNC Service Center 500 CORPORATE WOODS PARKWAY, VERNON HILLS, IL. 60061, U.S.A. TEL: +1-847-478-2500 (Se FAX: +1-847-478-2650 (Se California CNC Service Center 5665 PLAZA DRIVE, CYPRESS, CA. 90630, U.S.A. TEL: +1-714-220-4796 FAX: +1-714-229-3818 Georgia CNC Service Center 2810 PREMIERE PARKWAY SUITE 400, DULUTH, GA., 30097, U.S.A. TEL: +1-678-258-4500 FAX: +1-678-258-4519 New Jersey CNC Service Center 200 COTTONTAIL LANE SOMERSET, NJ. 08873, U.S.A. TEL: +1-732-560-4500 FAX: +1-732-560-4531 Michigan CNC Service Satellite 2545 38TH STREET, ALLEGAN, MI., 49010, U.S.A. TEL: +1-847-478-2500 FAX: +1-269-673-4092 Ohio CNC Service Satellite 62 W. 500 S., ANDERSON, IN., 46013, U.S.A. TEL: +1-847-478-2608 FAX: +1-847-478-2690 Texas CNC Service Satellite 1000, NOLEN DRIVE SUITE 200, GRAPEVINE, TX. 76051, U.S.A. TEL: +1-817-251-7468 FAX: +1-817-416-1439 Canada CNC Service Center 4299 14TH AVENUE MARKHAM, ON. L3R OJ2, CANADA TEL: +1-905-475-7728 FAX: +1-905-475-7935 Mexico CNC Service Center MARIANO ESCOBEDO 69 TLALNEPANTLA, 54030 EDO. DE MEXICO TEL: +52-55-9171-7662 FAX: +52-55-9171-7698 Monterrey CNC Service Satellite ARGENTINA 3900, FRACC. LAS TORRES, MONTERREY, N.L., 64720, MEXICO TEL: +52-81-8365-4171 FAX: +52-81-8365-4171 Brazil MITSUBISHI CNC Agent Service Center (AUTOMOTION IND. COM. IMP. E EXP. LTDA.) ACESSO JOSE SARTORELLI, KM 2.1 18550-000 BOITUVA SP, BRAZIL TEL: +55-15-3363-9900 FAX: +55-15-3363-9911
European FA Center (MITSUBISHI ELECTRIC EUROPE B.V.)
Germany CNC Service Center GOTHAER STRASSE 8, 40880 RATINGEN, GERMANY TEL: +49-2102-486-0 FAX:+49-2102486-591 South Germany CNC Service Center KURZE STRASSE. 40, 70794 FILDERSTADT-BONLANDEN, GERMANY TEL: +49-711-3270-010 FAX: +49-711-3270-0141 France CNC Service Center 25, BOULEVARD DES BOUVETS, 92741 NANTERRE CEDEX FRANCE TEL: +33-1-41-02-83-13 FAX: +33-1-49-01-07-25 Lyon CNC Service Satellite U.K CNC Service Center TRAVELLERS LANE, HATFIELD, HERTFORDSHIRE, AL10 8XB, U.K. TEL: +44-1707-282-846 FAX:-44-1707-278-992 Italy CNC Service Center ZONA INDUSTRIALE VIA ARCHIMEDE 35 20041 AGRATE BRIANZA, MILANO ITALY TEL: +39-039-60531-342 FAX: +39-039-6053-206 Spain CNC Service Satellite CTRA. DE RUBI, 76-80 -APDO.420 08190 SAINT CUGAT DEL VALLES, BARCELONA SPAIN TEL: +34-935-65-2236 FAX: Turkey MITSUBISHI CNC Agent Service Center (GENEL TEKNIK SISTEMLER LTD. STI.) DARULACEZE CAD. FAMAS IS MERKEZI A BLOCK NO.43 KAT2 80270 OKMEYDANI ISTANBUL, TURKEY TEL: +90-212-320-1640 FAX: +90-212-320-1649 Poland MITSUBISHI CNC Agent Service Center (MPL Technology Sp. z. o. o) UL SLICZNA 34, 31-444 KRAKOW, POLAND TEL: +48-12-632-28-85 FAX: Wroclaw MITSUBISHI CNC Agent Service Satellite (MPL Technology Sp. z. o. o) UL KOBIERZYCKA 23, 52-315 WROCLAW, POLAND TEL: +48-71-333-77-53 FAX: +48-71-333-77-53 Czech MITSUBISHI CNC Agent Service Center (AUTOCONT CONTROL SYSTEM S.R.O. ) NEMOCNICNI 12, 702 00 OSTRAVA 2 CZECH REPUBLIC TEL: +420-596-152-426 FAX: +420-596-152-112
ASEAN FA Center (MITSUBISHI ELECTRIC ASIA PTE. LTD.) Singapore CNC Service Center 307 ALEXANDRA ROAD #05-01/02 MITSUBISHI ELECTRIC BUILDING SINGAPORE 159943 TEL: +65-6473-2308 FAX: +65-6476-7439 Thailand MITSUBISHI CNC Agent Service Center (F. A. TECH CO., LTD) 898/19,20,21,22 S.V. CITY BUILDING OFFICE TOWER 1 FLOOR 12,14 RAMA III RD BANGPONGPANG, YANNAWA, BANGKOK 10120. THAILAND TEL: +66-2-682-6522 FAX: +66-2-682-6020 Malaysia MITSUBISHI CNC Agent Service Center (FLEXIBLE AUTOMATION SYSTEM SDN. BHD.) 60, JALAN USJ 10/1B 47620 UEP SUBANG JAYA SELANGOR DARUL EHSAN MALAYSIA TEL: +60-3-5631-7605 FAX: +60-3-5631-7636 JOHOR MITSUBISHI CNC Agent Service Satellite (FLEXIBLE AUTOMATION SYSTEM SDN. BHD.) NO. 16, JALAN SHAHBANDAR 1, TAMAN UNGKU TUN AMINAH, 81300 SKUDAI, JOHOR MALAYSIA TEL: +60-7-557-8218 FAX: +60-7-557-3404 Indonesia MITSUBISHI CNC Agent Service Center (PT. AUTOTEKNINDO SUMBER MAKMUR) WISMA NUSANTARA 14TH FLOOR JL. M.H. THAMRIN 59, JAKARTA 10350 INDONESIA TEL: +62-21-3917-144 FAX: +62-21-3917-164 India MITSUBISHI CNC Agent Service Center (MESSUNG SALES & SERVICES PVT. LTD.) B-36FF, PAVANA INDUSTRIAL PREMISES M.I.D.C., BHOASRI PUNE 411026, INDIA TEL: +91-20-2711-9484 FAX: +91-20-2712-8115 BANGALORE MITSUBISHI CNC Agent Service Satellite (MESSUNG SALES & SERVICES PVT. LTD.) S 615, 6TH FLOOR, MANIPAL CENTER, BANGALORE 560001, INDIA TEL: +91-80-509-2119 FAX: +91-80-532-0480 Delhi MITSUBISHI CNC Agent Parts Center (MESSUNG SALES & SERVICES PVT. LTD.) 1197, SECTOR 15 PART-2, OFF DELHI-JAIPUR HIGHWAY BEHIND 32ND MILESTONE GURGAON 122001, INDIA TEL: +91-98-1024-8895 FAX: Philippines MITSUBISHI CNC Agent Service Center (FLEXIBLE AUTOMATION SYSTEM CORPORATION) UNIT No.411, ALABAMG CORPORATE CENTER KM 25. WEST SERVICE ROAD SOUTH SUPERHIGHWAY, ALABAMG MUNTINLUPA METRO MANILA, PHILIPPINES 1771 TEL: +63-2-807-2416 FAX: +63-2-807-2417 Vietnam MITSUBISHI CNC Agent Service Center (SA GIANG TECHNO CO., LTD) 47-49 HOANG SA ST. DAKAO WARD, DIST.1 HO CHI MINH CITY, VIETNAM TEL: +84-8-910-4763 FAX: +84-8-910-2593
China FA Center (MITSUBISHI ELECTRIC AUTOMATION (SHANGHAI) LTD.)
China CNC Service Center 2/F., BLOCK 5 BLDG.AUTOMATION INSTRUMENTATION PLAZA, 103 CAOBAO RD. SHANGHAI 200233, CHINA TEL: +86-21-6120-0808 FAX: +86-21-6494-0178 Shenyang CNC Service Center TEL: +86-24-2397-0184 FAX: +86-24-2397-0185 Beijing CNC Service Satellite 9/F, OFFICE TOWER1, HENDERSON CENTER, 18 JIANGUOMENNEI DAJIE, DONGCHENG DISTRICT, BEIJING 100005, CHINA TEL: +86-10-6518-8830 FAX: +86-10-6518-8030 China MITSUBISHI CNC Agent Service Center (BEIJING JIAYOU HIGHTECH TECHNOLOGY DEVELOPMENT CO.) RM 709, HIGH TECHNOLOGY BUILDING NO.229 NORTH SI HUAN ZHONG ROAD, HAIDIAN DISTRICT , BEIJING 100083, CHINA TEL: +86-10-8288-3030 FAX: +86-10-6518-8030 Tianjin CNC Service Satellite RM909, TAIHONG TOWER, NO220 SHIZILIN STREET, HEBEI DISTRICT, TIANJIN, CHINA 300143 TEL: -86-22-2653-9090 FAX: +86-22-2635-9050 Shenzhen CNC Service Satellite RM02, UNIT A, 13/F, TIANAN NATIONAL TOWER, RENMING SOUTH ROAD, SHENZHEN, CHINA 518005 TEL: +86-755-2515-6691 FAX: +86-755-8218-4776 Changchun Service Satellite TEL: +86-431-50214546 FAX: +86-431-5021690 Hong Kong CNC Service Center UNIT A, 25/F RYODEN INDUSTRIAL CENTRE, 26-38 TA CHUEN PING STREET, KWAI CHUNG, NEW TERRITORIES, HONG KONG TEL: +852-2619-8588 FAX: +852-2784-1323
Taiwan FA Center (MITSUBISHI ELECTRIC TAIWAN CO., LTD.) Taichung CNC Service Center NO.8-1, GONG YEH 16TH RD., TAICHUNG INDUSTIAL PARK TAICHUNG CITY, TAIWAN R.O.C. TEL: +886-4-2359-0688 FAX: +886-4-2359-0689 Taipei CNC Service Satellite TEL: +886-4-2359-0688 FAX: +886-4-2359-0689 Tainan CNC Service Satellite TEL: +886-4-2359-0688 FAX: +886-4-2359-0689
Korean FA Center (MITSUBISHI ELECTRIC AUTOMATION KOREA CO., LTD.)
Korea CNC Service Center 1480-6, GAYANG-DONG, GANGSEO-GU SEOUL 157-200, KOREA TEL: +82-2-3660-9631 FAX: +82-2-3664-8668
Notice
Every effort has been made to keep up with software and hardware revisions in the contents described in this manual. However, please understand that in some unavoidable cases simultaneous revision is not possible. Please contact your Mitsubishi Electric dealer with any questions or comments regarding the