Alarm

Message

Description

0001

TH ERROR

A TH error was detected during reading from an input device.  The read code that caused the TH error and how many  statements it is from the block can be verified in the diagnostics  screen.

0002

TV ERROR

An error was detected during the single–block TV error.  The TV check can be suppressed by setting TVC parameter No.  0000#0 to “0”.

0003

TOO MANY DIGIT

Data entered with more digits than permitted in the NC  instruction word.  

The number of permissible digits varies according to the  function and the word.

0004

INVALID BREAK POINT OF WORDS

NC word(s) address + numerical value not in word format. This  alarm is also generated when a custom macro does not contain  a reserved word, or does not conform to the syntax.

0005

NO DATA AFTER ADDRESS

NC word(s) address + numerical value not in word format. This  alarm is also generated when a custom macro does not contain  a reserved word, or does not conform to the syntax.

0006

ILLEGAL USE OF MINUS SIGN

A minus sign (–) was specified at an NC instruction word or  system variable where no minus signal may be specified.

0007

ILLEGAL USE OF DECIMAL POINT

A decimal point (.) was specified at an address where no  decimal point may be specified, or two decimal points were  specified.

0009

IMPROPER NC-ADDRESS

An illegal address was specified, or parameter 1020 is not set.

0010

IMPROPER G-CODE

An unusable G code is specified.

0011

FEED ZERO ( COMMAND )

The cutting feedrate instructed by an F code has been set to 0.  This alarm is also generated if the F code instructed for the S  code is set extremely small in a rigid tapping instruction as the  tool cannot cut at the programmed lead.

0014

CAN NOT COMMAND G95

A synchronous feed is specified without the option for threading  / synchronous feed. Modify the program.

0015

TOO MANY SIMULTANEOUS AXES

A move command was specified for more axes than can be  controlled by simultaneous axis control.  

Either add on the simultaneous axis control extension option, or  divide the number of programmed move axes into two blocks.

Alarm 

Message

Description

0020

OVER TOLERANCE OF RADIUS

An arc was specified for which the difference in the radius at the  start and end points exceeds the value set in parameter No.  3410. Check arc center codes I, J and K in the program.  The tool path when parameter No. 3410 is set to a large value is  spiral.

0021

ILLEGAL PLANE SELECT

The plane selection instructions G17 to G19 are in error.  Reprogram so that same 3 basic parallel axes are not specified  simultaneously.  

This alarm is also generated when an axis that should not be  specified for plane machining is specified, for example, for  circular interpolation or involute interpolation.  

To enable programming of 3 or more axes, the helical  interpolation option must be added to each of the relevant axes.

0022

R OR I,J,K COMMAND NOT FOUND

The command for circular interpolation lacks arc radius R or  coordinate I, J, or K of the distance between the start point to  the center of the arc.

0025

CIRCLE CUT IN RAPID (F0)

F0 (rapid traverse in inverse feed or feed specified by an F code  with 1–digit number) was specified during circular interpolation  (G02, G03) or involute interpolation (G02.2, G03.2).

0027

NO AXES COMMANDED IN G43/G44

 No axis is specified in G43 and G44 blocks for the tool length  offset type C.  

Offset is not canceled but another axis is offset for the tool  length offset type C.  

Multiple axes were specified for the same block when the tool  length compensation type is C.

0028

ILLEGAL PLANE SELECT

The plane selection instructions G17 to G19 are in error.  Reprogram so that same 3 basic parallel axes are not specified  simultaneously.  

This alarm is also generated when an axis that should not be  specified for plane machining is specified, for example, for  circular interpolation or involute interpolation.  

To enable programming of 3 or more axes, the helical  interpolation option must be added to each of the relevant axes.

0029

ILLEGAL OFFSET VALUE

Illegal offset No.

0030

ILLEGAL OFFSET NUMBER

An illegal offset No. was specified.  

This alarm is also generated when the tool shape offset No.  exceeds the maximum number of tool offset sets in the case of  tool offset memory B.

0031

ILLEGAL P COMMAND IN G10

The relevant data input or option could not be found for the L  No. of G10.  

No data setting address such as P or R was specified.  An address command not concerned with data setting was  specified. An address varies with the L No.  

The sign or decimal point of the specified address is in error, or  the specified address is out of range.

0032

ILLEGAL OFFSET VALUE IN G10

In setting an offset amount by G10 or in writing an offset amount  by system variables, the offset amount was excessive.

0033

NO INTERSECTION AT CUTTER  COMPENSATION

The intersection cannot be obtained by the intersection  calculation in tool radius/tool nose radius compensation. Modify  the program.

0034

NO CIRC ALLOWED IN STUP/EXT  BLK

In tool radius/tool nose radius compensation, a startup or  cancellation is performed in the G02 or G03 mode. Modify the  program.

Alarm 

Message

Description

0035

CAN NOT COMMANDED G31

- G31 cannot be specified. This alarm is generated when a G  code (such as for tool radius/tool nose radius compensation)  of group 07 is not canceled.  

- A torque limit skip was not specified in a torque limit skip  command (G31P98 or P99). Specify the torque limit skip in the  PMC window or the like. Or, specify the torque limit override  by address Q.

0037

CAN NOT CHANGE PLANE IN  G41/G42

The compensation plane G17/G18/G19 was changed during  cutter or tool-nose radius compensation. Modify the program.

0038

INTERFERENCE IN CIRCULAR  BLOCK

Overcutting will occur in tool radius/tool nose radius  compensation because the arc start point or end point coincides  with the arc center. Modify the program.

0039

CHF/CNR NOT ALLOWED IN  

G41,G42

Chamfering or corner R was specified with a start-up, a cancel,  or switching between G41 and G42 in G41 and G42 commands  (tool radius/tool nose radius compensation). The program may  cause overcutting to occur in chamfering or corner R. Modify the  program.

0041

INTERFERENCE IN CUTTER  

COMPENSATION

In tool radius/tool nose radius compensation, excessive cutting  may occur. Modify the program.

0042

G45/G48 NOT ALLOWED IN CRC

Tool offset (G45 to G48) is commanded in tool radius  compensation or three-dimensional cutter compensation. Modify  the program.

0043

ILLEGAL T-CODE COMMAND

On a system with a DRILL-MATE ATC installed, M06 is not specified in a block that specifies a T code. Alternatively, a T  code beyond the allowable range is specified.

0044

G27-G30 NOT ALLOWED IN FIXED  CYC

One of G27 to G30 is commanded in canned cycle mode.  Modify the program.

0045

ADDRESS Q NOT FOUND (G73/G83)

 In a high-speed peck drilling cycle (G73) or peck drilling cycle  (G83), the amount of each-time cutting is not specified by  address Q, or Q0 is specified. Modify the program.

0046

ILLEGAL REFERENCE RETURN  COMMAND

A command for a return to the second, third or fourth reference  position is error. (The address P command is in error.)  Although an option for a return to the third or fourth reference  position was not set, 3 or 4 was specified in address P.

0047

ILLEGAL AXIS SELECT

Two or more parallel axes (in parallel with a basic axis) have  been specified upon start-up of 3-dimensional tool  compensation or three-dimensional coordinate conversion.

0048

BASIC 3 AXIS NOT FOUND

Start-up of 3-dimensional tool compensation or  

three-dimensional coordinate conversion has been attempted,  but the three basic axes used when Xp, Yp, or Zp is omitted are  not set in parameter No. 1022.

0049

ILLEGAL COMMAND(G68,G69)

When three-dimensional coordinate conversion (G68 or G69)  was specified, the tool compensation was not canceled. Or,  programs of three-dimensional coordinate conversion (G68,  G69) and tool compensation (G43, G44 or G49) were not  nested. Or, the three-dimensional coordinate conversion was  specified during the tool length compensation and another tool  length compensation was specified.

0050

CHF/CNR NOT ALLOWED IN THRD  BLK

Chamfering or corner R is commanded in the thread cutting  block. Modify the program.

0051

MISSING MOVE AFTER CNR/CHF

Improper movement or the move distance was specified in the  block next to the chamfering or corner R block. Modify the  program.

Alarm

Message

Description

0052

CODE IS NOT G01 AFTER CHF/CNR

 The block next to the chamfering or corner R block is not G01  (or vertical line). Modify the program.

0053

TOO MANY ADDRESS COMMANDS

In the chamfering and corner R commands, two or more of I, J,  K and R are specified.

0054

NO TAPER ALLOWED AFTER  CHF/CNR

A block in which chamfering in the specified angle or the corner  R was specified includes a taper command. Modify the program.

0055

MISSING MOVE VALUE IN CHF/CNR

 In chamfering or corner R block, the move distance is less than  chamfer or corner R amount. Modify the program.

0056

NO END POINT & ANGLE IN  

CHF/CNR

In direct dimension drawing programming, both an end point  and an angle were specified in the block next to the block in  which only an angle was specified (Aa). Modify the program.

0057

NO SOLUTION OF BLOCK END

Block end point is not calculated correctly in direct dimension  drawing programming. Modify the program.

0058

END POINT NOT FOUND

Block end point is not found in direct dimension drawing  programming. Modify the program.

0060

SEQUENCE NUMBER NOT FOUND

[External data input/output]  

The specified number could not be found for program number  and sequence number searches.  

Although input/output of a pot number of tool data or offset  input was requested, no tool number was input after power on.  The tool data corresponding to the entered tool number could  not be found.  

[External workpiece number search]  

The program corresponding to the specified workpiece  number could not be found.  

[Program restart]  

In the program restart sequence number specification, the  specified sequence number could not be found.

0061

P OR Q COMMAND IS NOT IN THE  MULTIPLE REPETITIVE CYCLES  BLOCK

Address P or Q is not specified in multiple repetitive cycle (G70,  G71, G72, or G73) command.

0062

THE CUTTING AMOUNT IS ILLEGAL  IN THE ROUGH CUTTING CYCLE

A zero or a negative value was specified in a multiple repetitive  canned rough-cutting cycle (G71 or G72) as the depth of cut.

0063

THE BLOCK OF A SPECIFIED  SEQUENCE NUMBER IS NOT  FOUND

The sequence number specified by addresses P and Q in  multiple repetitive cycle (G70, G71, G72, or G73) command  cannot be searched.

0064

THE FINISHING SHAPE IS NOT A  MONOTONOUS CHANGE(FIRST  AXES)

In a shape program for the multiple repetitive canned  rough-cutting cycle (G71 or G72), the command for the first  plane axis was not a monotonous increase or decrease.

0065

G00/G01 IS NOT IN THE FIRST  BLOCK OF SHAPE PROGRAM

In the first block of the shape program specified by P of the  multiple repetitive canned cycle (G70, G71, G72, or G73), G00  or G01 was not specified.

0066

UNAVAILABLE COMMAND IS IN THE  MULTIPLE REPETIVE CYCLES  BLOCK

An unavailable command was found in a multiple repetitive  canned cycle (G70, G71, G72, or G73) command block.

0067

THE MULTIPLE REPETIVE CYCLES  IS NOT IN THE PART PROGRAM  STORAGE

A multiple repetitive canned cycle (G70, G71, G72, or G73)  command is not registered in a tape memory area.

0069

LAST BLOCK OF SHAPE PROGRAM  IS AN ILLEGAL COMMAND

In a shape program in the multiple repetitive canned cycle (G70,  G71, G72, or G73), a command for the chamfering or corner R  in the last block is terminated in the middle.

0070

NO PROGRAM SPACE IN MEMORY

The memory area is insufficient.  

Delete any unnecessary programs, then retry.

Alarm 

Message

Description

0071

DATA NOT FOUND

- The address to be searched was not found.  

- The program with specified program number was not found  in program number search.  

- In the program restart block number specification, the  specified block number could not be found.  

Check the data.

0072

DATA NOT FOUND

The number of programs to be stored exceeded 63 (basic), 125  (option), 200 (option), 400 (option) or 1000 (option). Delete  unnecessary programs and execute program registration again.

0073

PROGRAM NUMBER ALREADY IN  USE

The commanded program number has already been used.  Change the program number or delete unnecessary programs  and execute program registration again.

0074

PROGRAM NUMBER ALREADY IN  USE

The program number is other than 1 to 9999. Modify the  program number.

0075

PROTECT

An attempt was made to register a program whose number was  protected.  

In program matching, the password for the encoded program  was not correct.  

An attempt was made to select a program being edited in the  background as the main program.  

An attempt was made to call a program being edited in the  background as a subprogram.

0076

PROGRAM NOT FOUND

The specified program is not found in the subprogram call,  macro call or graphic copy.  

The M, G, T or S codes are called by a P instruction other than  that in an M98, G65, G66, G66.1 or interrupt type custom  macro, and a program is called by a No. 2 auxiliary function  code.  

This alarm is also generated when a program is not found by  these calls.

0077

TOO MANY SUB,MACRO NESTING

The total number of subprogram and macro calls exceeds the  permissible range.  

Another subprogram call was executed during an external  memory subprogram call.

0078

SEQUENCE NUMBER NOT FOUND

The specified sequence No. was not found during sequence  number search.  

The sequence No. specified as the jump destination in GOTO––  and M99P–– was not found.

0079

PROGRAM NOT MATCH

The program in memory does not match the program stored on  tape.  

Multiple programs cannot be matched continuously when  parameter No. 2200#3 is set to “1”.  

Set parameter No. 2200#3 to “0” before executing a match.

0080

G37 MEASURING POSITION  

REACHED SIGNAL IS NOT  

PROPERLY INPUT

- For machining center series  

When the tool length measurement function (G37) is  performed, a measuring position reached signal goes 1 in front  of the area determined by the ε value specified in parameter  No.6254. Alternatively, the signal does not go 1.  

- For lathe  

When the automatic tool compensation function (G36, G37) is  used, a measuring position reached signals (XAE1, XAE2)  does not go 1 within the range determined by the ε value  specified in parameters No.6254 and No.6255.

Alarm 

Message

Description

0081

G37 OFFSET NO. UNASSIGNED

- For machining center series  

The tool length measurement function (G37) is specified  without specifying an H code.  

Correct the program.  

- For lathe  

The automatic tool compensation function (G36, G37) is  specified without specifying an T code.  

Correct the program.

0082

G37 SPECIFIED WITH H CODE

- For machining center series  

The tool length measurement function (G37) is specified  together with an H code in the same block.  

Correct the program.  

- For lathe  

The automatic tool compensation function (G36, G37) is  specified together with an T code in the same block.  Correct the program.

0083

G37 IMPROPER AXIS COMMAND

- For machining center series  

An error has been found in axis specification of the tool length  measurement function (G37). Alternatively, a move command  is specified as an incremental command.  

Correct the program.  

- For lathe  

An error has been found in axis specification of the automatic  tool compensation function (G36, G37).  

Alternatively, a command is specified as an incremental  command.  

Correct the program.

0085

OVERRUN ERROR

The next character was received from the I/O device connected  to reader/punch interface 1 before it could read a previously  received character.

0086

DR OFF

During I/O process by reader/punch interface 1, the data set ready input signal of the I/O device (DR) was OFF. Possible  causes are an I/O device not turn on, a broken cable, and a  defective printed circuit board.

0087

BUFFER OVERFLOW

During a read by reader/punch interface 1, although a read stop command was issued, more than 10 characters were input. The  I/O device or printed circuit board was defective.

0090

REFERENCE RETURN  

INCOMPLETE

1. The reference position return cannot be performed normally  because the reference position return start point is too close  to the reference position or the speed is too slow. Separate  the start point far enough from the reference position, or  specify a sufficiently fast speed for reference position return.

2. An attempt was made to set the zero position for the  absolute position detector by return to the reference position  when it was impossible to set the zero point.  

 Rotate the motor manually at least one turn, and set the  zero position of the absolute position detector after turning  the CNC and servo amplifier off and then on again.

0091

MANUAL REFERENCE POSITION  RETURN IS NOT PERFORMED IN  FEED HOLD

Manual return to the reference position cannot be performed  when automatic operation is halted. Perform the manual return  to the reference position when automatic operation is stopped or  reset.

0092

ZERO RETURN CHECK (G27)  ERROR

The axis specified in G27 has not returned to zero.  Reprogram so that the axis returns to zero.

Alarm 

Message

Description

0094

P TYPE NOT ALLOWED (COORD  CHG)

P type cannot be specified when the program is restarted. (After  the automatic operation was interrupted, the coordinate system  setting operation was performed.) Perform the correct operation  according to the User's manual.

0095

P TYPE NOT ALLOWED (EXT OFS  CHG)

P type cannot be specified when the program is restarted. (After  the automatic operation was interrupted, the external workpiece  offset amount changed.) Perform the correct operation  according to the User's manual.

0096

P TYPE NOT ALLOWED (WRK OFS  CHG)

P type cannot be specified when the program is restarted. (After  the automatic operation was interrupted, the workpiece offset  amount changed.) Perform the correct operation according to  the User's manual.

0097

P TYPE NOT ALLOWED (AUTO  EXEC)

P type cannot be directed when the program is restarted. (After  power ON, after emergency stop or alarms 0094 to 0097 reset,  no automatic operation is performed.) Perform automatic  operation.

0098

G28 FOUND IN SEQUENCE RETURN

 A command of the program restart was specified without the  reference position return operation after power ON or  emergency stop, and G28 was found during search. Perform the  reference position return.

0099

MDI EXEC NOT ALLOWED AFT.  SEARCH

After completion of search in program restart, a move command  is given with MDI.

0109

FORMAT ERROR IN G08

A value other than 0 or 1 was specified after P in the G08 code,  or no value was specified.

0110

OVERFLOW :INTEGER

An integer went out of range during arithmetic calculations.

0111

OVERFLOW :FLOATING

A decimal point (floating point number format data) went out of  range during arithmetic calculations.

0112

ZERO DIVIDE

An attempt was made to divide by zero in a custom macro.

0113

IMPROPER COMMAND

A function which cannot be used in custom macro is  commanded. Modify the program.

0114

ILLEGAL EXPRESSION FORMAT

The format used in an expression in a custom macro statement  is in error. The parameter tape format is in error.

0115

VARIABLE NO. OUT OF RANGE

A number that cannot be used for a local variable, common  variable, or system variable in a custom macro is specified.  In the EGB axis skip function (G31.8), a non-existent custom  macro variable number is specified. Or, the number of custom  macro variables used to store skip positions is not sufficient.  Alternatively, the header data in high-speed cycle machining is  improper. This alarm is issued in the following cases.  1) The header corresponding to the specified call machining  cycle number is absent.  

2) The value of cycle connection information falls outside the  allowable range (0 to 999).  

3) The number of data items in the header falls outside the  allowable range (1 to 65535).  

4) The storage start data variable number of executable data  falls outside the allowable ranges (#20000 to  

#85535/#200000 to #986431/#2000000 to #3999999).  5) The storage end data variable number of executable data  falls outside the allowable ranges  

(#85535/#986431/#3999999).  

6) The storage start data variable number of executable data  is the same as the variable number used by the header.

0116

WRITE PROTECTED VARIABLE

An attempt was made in a custom macro to use on the left side  of an expression a variable that can only be used on the right  side of an expression.

Alarm

Message

Description

0118

TOO MANY BRACKET NESTING

Too many brackets “[ ]” were nested in a custom macro.  The nesting level including function brackets is 5.

0119

ARGUMENT VALUE OUT OF RANGE

 The value of an argument in a custom macro function is out of  range.

0122

TOO MANY MACRO NESTING

Too many macro calls were nested in a custom macro.

0123

ILLEGAL MODE FOR  

GOTO/WHILE/DO

A GOTO statement or WHILE–DO statement was found in the  main program in the MDI or DNC mode.

0124

MISSING END STATEMENT

The END instruction corresponding to the DO instruction was  missing in a custom macro.

0125

MACRO STATEMENT FORMAT  ERROR

The format used in a macro statement in a custom macro is in  error.

0126

ILLEGAL LOOP NUMBER

DO and END Nos. in a custom macro are in error, or exceed the  permissible range (valid range: 1 to 3).

0127

DUPLICATE NC,MACRO  

STATEMENT

An NC statement and macro statement were specified in the  same block.

0128

ILLEGAL MACRO SEQUENCE  NUMBER

The specified sequence No. could not be found for sequence  number search.  

The sequence No. specified as the jump destination in GOTO--  and M99P-- could not be found.

0129

USE 'G' AS ARGUMENT

G is used as an argument in a custom macro call. G can be  specified as an argument only in an every-block call (G66.1).

0130

NC AND PMC AXIS ARE  

CONFLICTED

The NC command and the PMC axis control command were  conflicted. Modify the program or ladder.

0136

SPOS AXIS - OTHER AXIS SAME  TIME

The spindle positioning axis and another axis are specified in  the same block.

0137

M-CODE & MOVE CMD IN SAME  BLK.

The spindle positioning axis and another axis are specified in  the same block.

0138

SUPERIMPOSED DATA OVERFLOW

 The total distribution amount of the CNC and PMC is too large  during superimposed control for PMC axis control.

0139

CANNOT CHANGE PMC CONTROL  AXIS

The PMC axis was selected for the axis for which the PMC axis  is being controlled.

0140

PROGRAM NUMBER ALREADY IN  USE

In the background, an attempt was made to select or delete the  program being selected in the foreground. Perform the correct  operation for the background edition.

0141

CAN NOT COMMAND G51 IN 3-D  OFFSET

G51 (Scaling ON) is commanded in the 3-dimensional tool  compensation mode. Modify the program.

0142

ILLEGAL SCALE RATE

The scaling rate is 0 times or 10000 times or more.  Modify the setting of the scaling rate. (G51P_ … or G51I_J_K_  … or parameter (No. 5411 or 5421))

0143

COMMAND DATA OVERFLOW

An overflow occurred in the storage length of the CNC internal  data. This alarm is also generated when the result of internal  calculation of scaling, coordinate rotation and cylindrical  interpolation overflows the data storage. It also is generated  during input of the manual intervention amount.

0144

ILLEGAL PLANE SELECTED

The coordinate rotation plane and arc or tool radius⋅tool nose  radius compensation plane must be the same. Modify the  program.

0145

ILLEGAL USE OF G12.1/G13.1

The axis No. of plane selection parameter No. 5460 (linear axis)  and No. 5461(axis of rotation) in the polar coordinate  interpolation mode is out of range (1 to number of controlled  axes).

Alarm 

Message

Description

0146

ILLEGAL USE OF G-CODE

The modal G code group contains an illegal G code in the polar  coordinate interpolation mode or when a mode was canceled.  Only the following G codes are allowed: G40, G50, G69.1  An illegal G code was specified while in the polar coordinate  interpolation mode.  

The following C codes are not allowed: G27, G28, G30, G30.1,  G31 to G31.4, G37 to G387.3, G52, G92, G53, G17 to G19,  G81 to G89, G68  

In the 01 group, G codes other than G01, G02, G03, G02.2 and  G03.2 cannot be specified.

0148

SETTING ERROR

Automatic corner override deceleration rate is out of the settable  range of judgement angle. Modify the parameters (No.1710 to  No.1714).

0149

FORMAT ERROR IN G10L3

In registration (G10L3 to G11) of tool life management data, an address other than Q1, Q2, P1, and P2 or an unusable address  was specified.

0150

ILLEGAL LIFE GROUP NUMBER

The tool group number exceeded the maximum allowable value. The tool group number (P after specification of G10 L3;) or the  group number given by the tool life management T code in a  machining program.

0151

GROUP NOT FOUND AT LIFE DATA

The tool group specified in a machining program is not set in tool life management data.

0152

OVER MAXIMUM TOOL NUMBER

The number of tools registered in one group exceeded the maximum allowable registration tool number.

0153

T-CODE NOT FOUND

In registration of tool life data, a block in which the T code needs to be specified does not include the T code. Alternatively, in  tool exchange method D, M06 is specified solely. Modify the  program.

0154

NOT USING TOOL IN LIFE GROUP

- For the tool management command

H99 or D99 was specified when no tool management data  number is assigned to the spindle position. Modify the  program.  

- For the tool life management command  

The H99 command, D99 command, or the H/D code set by  parameters No. 13265 and No. 13266 was specified when no  tool belonging to a group is used.

0155

ILLEGAL T-CODE COMMAND

In the machining program, the T code that is present in the block containing M06 does not correspond to the group currently  being used. Modify the program.

0156

P/L COMMAND NOT FOUND

The P and L commands are not specified in the beginning of a program for setting a tool group. Modify the program.

0157

TOO MANY TOOL GROUPS

In registration of tool life management data, the group setting command block counts of P (group number) and L (tool life)  exceeded the maximum group count.

0158

TOOL LIFE VALUE OUT OF RANGE

The life value that is being set is too large. Change the setting.

0159

ILLEGAL TOOL LIFE DATA

Tool life management data is corrupted for some reason. Register the tool data in the tool group or the tool data in the  group again by G10L3; or MDI input.

Alarm 

Message

Description

0160

MISMATCH WAITING M-CODE

A waiting M-code is in error.  

<1> When different M codes are specified for path 1 and path 2  as waiting M codes without a P command.  

<2> When the waiting M codes are not identical even though  the P commands are identical  

<3> When the waiting M codes are identical and the P  commands are not identical (This occurs when a P  command is specified with binary value.)  

<4> When the number lists in the P commands contain a  different number even though the waiting M codes are  identical (This occurs when a P command is specified by  combining path numbers.)  

<5> When a waiting M code without a P command (2-path  waiting) and a waiting M code with a P command  

(3-or-more-path waiting) were specified at the same time  <6> When a waiting M code without a P command was  specified for 3 or more paths.

0161

ILLEGAL P OF WAITING M-CODE

P in a waiting M-code is incorrect.  

<1> When address P is negative  

<2> When a P value inappropriate for the system configuration  was specified  

<3> When a waiting M code without a P command (2-path  waiting) was specified in the system having 3 or more  paths.

0163

ILLEGAL COMMAND IN G68/G69

G68 and G69 are not independently commanded in balance cut. An illegal value is commanded in a balance cut combination  (address P).

0169

ILLEGAL TOOL GEOMETRY DATA

Incorrect tool figure data in interference check. Set correct data,  or select correct tool figure data.

0175

ILLEGAL G07.1 AXIS

An axis which cannot perform cylindrical interpolation was  specified. More than one axis was specified in a G07.1 block.  An attempt was made to cancel cylindrical interpolation for an  axis that was not in the cylindrical interpolation mode.  For the cylindrical interpolation axis, set not “0” but one of 5, 6 or  7 (parallel axis specification) to parameter No. 1022 to instruct  the arc with axis of rotation (ROT parameter No. 1006#1 is set  to “1” and parameter No. 1260 is set) ON.

0176

ILLEGAL G-CODE USE(G07.1 MODE)

 A G code was specified that cannot be specified in the  cylindrical interpolation mode. This alarm also is generated  when an 01 group G code was in the G00 mode or code G00  was instructed.  

Cancel the cylindrical interpolation mode before instructing code  G00.

Alarm 

Message

Description

0178

ILLEGAL COMMAND G05

The settings of bits 4 to 6 of parameter No.7501 are invalid or  G05 was specified in any of the following mode.  

- Hypothetical axis interpolation (G07)  

- Cylindrical interpolation (G07.1)  

- Polar coordinate interpolation (G12.1)  

- Polar coordinates command (G16)  

- Spindle speed fluctuation detection (G26)  

- Tool radius ⋅ tool nose radius compensation (G41/G42)  - Normal direction control (G41.1/G42.1)  

- Scaling (G51)  

- Programmable mirror image (G51.1)  

- Coordinate system rotation (G68)  

- Canned cycle (G81 to G89)  

- Constant surface speed control (G96)  

- Macro interruption(M96)

0179

PARAM. (NO.7510) SETTING ERROR

 The number of controlled axes set by the parameter No. 7510  exceeds the maximum number. Modify the parameter setting  value.  

The distribution of high-speed cycle machining stopped.

0190

ILLEGAL AXIS SELECTED (G96)

An illegal value was specified in P in a G96 block or parameter  No. 5844.

0194

SPINDLE COMMAND IN  

SYNCHRO-MODE

A Cs contour control mode, spindle positioning command, or  rigid tapping mode was specified during the spindle  synchronous control mode or simple spindle synchronous  control mode.

0197

C-AXIS COMMANDED IN SPINDLE  MODE

The program specified a movement along the Cs-axis when the  Cs contour control switching signal was off.

0199

MACRO WORD UNDEFINED

Undefined macro word was used. Modify the custom macro.

0200

ILLEGAL S CODE COMMAND

In the rigid tap, an S value was out of range or was not  specified. The parameter (Nos. 5241 to 5243) setting is an S  value which can be specified for the rigid tap.  

Correct the parameters or modify the program.

0201

FEEDRATE NOT FOUND IN RIGID  TAP

The command F code for a cutting feedrate is a zero.  If the value of F command is much smaller than that of the S  command, when a rigid tap command is specified, this alarm is  generated. This is because cutting is not possible by the lead  specified by the program.

0202

POSITION LSI OVERFLOW

In the rigid tap, spindle distribution value is too large. (System  error)

0203

PROGRAM MISS AT RIGID TAPPING

 In the rigid tap, position for a rigid M code (M29) or an S  command is incorrect. Modify the program.

0204

ILLEGAL AXIS OPERATION

In the rigid tap, an axis movement is specified between the rigid  M code (M29) block and G84 (or G74) block. Modify the  program.

0205

RIGID MODE DI SIGNAL OFF

Although a rigid M code (M29) is specified in rigid tapping, the  rigid mode DI signal (DGN G061.0) is not ON during execution  of the G84 (or G74) block. Check the PMC ladder diagram to  find the reason why the DI signal is not turned on.

0206

CAN NOT CHANGE PLANE (RIGID  TAP)

Plane changeover was instructed in the rigid mode. Modify the  program.

0207

RIGID DATA MISMATCH

The specified distance was too short or too long in rigid tapping.

Alarm 

Message

Description

0210

CAN NOT COMMAND M198/M99

1 The execution of an M198 or M99 command was attempted  during scheduled operation. Alternatively, the execution of an  M198 command was attempted during DNC operation. Modify  the program.  

2 The execution of an M99 command was attempted by an  interrupt macro during pocket machining in a multiple  repetitive canned cycle.

0212

ILLEGAL PLANE SELECT

The direct drawing dimensions programming is commanded for  the plane other than the Z-X plane. Correct the program.

0213

ILLEGAL COMMAND IN  

SYNCHRO-MODE

In feed axis synchronization control, the following errors  occurred during the synchronous operation.  

1) The program issued the move command to the slave axis.  2) The program issued the manual operation to the slave axis. 3) The program issued the automatic reference position return  

command without specifying the manual reference position  return after the power was turned on.

0214

ILLEGAL COMMAND IN  

SYNCHRO-MODE

Coordinate system is set or tool compensation of the shift type  is executed in the synchronous control. Correct the program.

0217

DUPLICATE G51.2(COMMANDS)

G51.2 is further commanded in the G51.2 mode. Modify the  program.

0218

NOT FOUND P/Q COMMAND

P or Q is not commanded in the G51.2 block, or the command  value is out of the range. Modify the program. For a polygon  turning between spindles, more information as to why this alarm  occurred is indicated in DGN No. 471.

0219

COMMAND G51.2/G50.2  

INDEPENDENTLY

G51.2 and 50.2 were specified in the same block for other  commands. Modify the program in another block.

0220

ILLEGAL COMMAND IN  

SYNCHR-MODE

In the synchronous operation, movement is commanded by the  NC program or PMC axis control interface for the synchronous  axis. Modify the program or check the PMC ladder.

0221

ILLEGAL COMMAND IN  

SYNCHR-MODE

Polygon machining synchronous operation and axis control or  balance cutting are executed at a time. Modify the program.

0222

DNC OP. NOT ALLOWED IN BG-EDIT

 Input and output are executed at a time in the background  edition. Execute a correct operation.

0224

ZERO RETURN NOT FINISHED

A reference return has not been performed before the start of  automatic operation.  

(Only when bit 0 (ZRNx) of parameter No. 1005 is 0)  Perform a reference position return.

0230

R CODE NOT FOUND

Cut depth R is not specified in the block including G161. Alternatively, the value specified for R is negative.  Modify the program.

0231

ILLEGAL FORMAT IN G10 L52

Errors occurred in the specified format at the  

programmable-parameter input.

0232

TOO MANY HELICAL AXIS  

COMMAND

Three or more axes were specified as helical axes in the helical  interpolation mode. Five or more axes were specified as helical  axes in the helical interpolation B mode.

0233

DEVICE BUSY

When an attempt was made to use a unit such as that  connected via the RS-232-C interface, other users were using it.

0241

ILLEGAL FORMAT IN G02.2/G03.2

The end point of an involute curve on the currently selected  plane, or the center coordinate instruction I, J or K of the  corresponding basic circle, or basic circle radius R was not  specified.

Alarm 

Message

Description

0242

ILLEGAL COMMAND IN G02.2/G03.2

An illegal value was specified in the involute curve.  The coordinate instruction I, J or K of the basic circle on the  currently selected plane or the basic circle radius R is “0”, or the  start and end points are not inside the basic circle.

0243

OVER TOLERANCE OF END POINT

The end point is not positioned on the involute curve that  passes through the start point, and this error exceeds the  permissible error limit (parameter No. 2510).

0245

T-CODE NOT ALLOWED IN THIS  BLOCK

One of the G codes, G50, G10, and G04, which cannot be  specified in the same block as a T code, was specified with a T  code.

0247

THE MISTAKE IS FOUND IN THE  OUTPUT CODE OF DATA.

When an encrypted program is output, EIA is set for the output  code. Specify ISO.

0250

TOOL CHANGE ILLEGAL Z AXIS  COMMAND

A Z-axis move command was performed in the same block for  M06 command.

0251

TOOL CHANGE ILLEGAL T  

COMMAND

An unusable T code was specified in M06Txx.

0253

G05 CAN NOT BE COMMANDED

A binary operation was specified during advanced preview  control mode.

0300

ILLEGAL COMMAND IN SCALING

An illegal G code was specified during scaling. Modify the  program. For the T system, one of the following functions is  specified during scaling, this alarm is generated.  

- finishing cycle (G70 or G72)  

- outer surface rough-cutting cycle (G71 or G73)  

- end side rough-cutting cycle (G72 or G74)  

- closed loop cutting cycle (G73 or G75)  

- end side cutting-off cycle (G74 or G76)  

- outer surface or inner surface cutting-off cycle (G75 or G77)  - multiple repetitive threading cycle (G76 or G78)  

- face drill cycle (G83 or G83)  

- face tap cycle (G84 or G84)  

- face boring cycle (G85 or G85)  

- side drill cycle (G87 or G87)  

- side tap cycle (G88 or G88)  

- side boring cycle (G89 or G89)  

- outer surface turning cycle or inner surface boring cycle (G77  or G20)  

- threading cycle (G78 or G21)  

- end side turning cycle (G79 or G24)  

(Specify G codes for systems B and C in that order.)

0301

RESETTING OF REFERENCE  RETURN IS INHIBITED

Although parameter No. 1012#0 (IDGx) was set to 1 to inhibit  the reference position from being set again for a return to the  reference position without a dog, an attempt was made to  perform a manual return to the reference position.

0302

SETTING THE REFERENCE  

POSITION WITHOUT DOG IS NOT  PERFORMED

The reference position could not be set for a return to the  reference position without a dog. Possible causes are:  - The axis was not moved in the direction of a return to the  reference position for jog feeding.  

- The axis was moved in the direction opposite to the direction  of a manual return to the reference position.

Alarm 

Message

Description

0303

REFERENCE POSITION RETURN IS  NOT PERFORMED

When the setting of a reference position at any position was  possible in Cs contour control (parameter CRF (No. 3700#0) =  1), a G00 command was issued for the Cs contour axis without  a return to the reference position after the serial spindle was  switched to Cs contour control mode.  

Perform a reference position return with a G28 command before  issuing a G00 command.

0304

G28 IS COMMANDED WITHOUT  ZERO RETURN

Although a reference position was not set, an automatic return  to the reference position (G28) was commanded.

0305

INTERMEDIATE POSITION IS NOT  ASSIGNED

Although a G28 (automatic return to the reference position),  G30 (return to the second, third, or fourth reference position), or  G30/1 (return to the floating reference position) command was  not issued after power-up, G29 (return from the reference  position) was commanded.

0306

MISMATCH AXIS WITH CNR/CHF

The correspondence between the moving axis and the I, J, or K  command is incorrect in a block in which chamfering is  specified.

0307

CAN NOT START REFERENCE  RETURN WITH MECHANICAL  STOPPER SETTING

An attempt was made to set a butt-type reference position for an  axis for which to use the function to set a reference position  without a dog.

0308

G72.1 NESTING ERROR

G72.1 was specified again during G72.1 rotation copying.

0309

G72.2 NESTING ERROR

G72.2 was specified again during G72.2 parallel copying.

0310

FILE NOT FOUND

The specified file could not be found during a subprogram or  macro call.

0311

CALLED BY FILE NAME FORMAT  ERROR

An invalid format was specified to call a subprogram or macro  using a file name.

0312

ILLEGAL COMMAND IN DIRECT  DRAWING DIMENSIONS  

PROGRAMMING

Direct input of drawing dimensions was commanded in an  invalid format.  

An attempt was made to specify an invalid G code during direct  input of drawing dimensions.  

Two or more blocks not to be moved exist in consecutive  commands that specify direct input of drawing dimensions.  Although non-use of commas (,) (parameter No. 3405#4 = 1)  was specified for direct input of drawing dimensions, a comma  was specified.

0313

ILLEGAL LEAD COMMAND

The variable-lead threading increment specified in address K  exceeds the specified maximum value in variable-lead  threading. Or, a negative lead value was specified.

0314

ILLEGAL SETTING OF POLYGONAL  AXIS

An axis was specified invalidly in polygon turning.  

For polygon turning:  

A tool rotation axis is not specified.  

(Parameter No. 7610)  

For polygon turning between spindles:  

Valid spindles are not specified.  

(Parameter Nos. 7640 to 7643)  

- A spindle other than the serial spindle.  

- A spindle is not connected.

0315

ILLEGAL NOSE ANGLE COMMAND  IS IN THE THREAD CUTTING CYCLE

An invalid tool tip angle is specified in a multiple repetitive  canned threading cycle (G76).

0316

ILLEGAL CUTTING AMOUNT IS IN  THE THREAD CUTTING CYCLE

An minimum depth of cut higher than the thread height is  specified in a multiple repetitive canned threading cycle (G76).

0317

ILLEGAL THREAD COMMAND IS IN  THE THREAD CUTTING CYCLE

A zero or a negative value is specified in a multiple repetitive  canned threading cycle (G76) as the thread height or the depth  of cut.

Alarm 

Message

Description

0318

ILLEGAL RELIEF AMOUNT IS IN THE  DRILLING CYCLE

Although an escape direction is set in a multiple repetitive  canned cutting-off cycle (G74 or G75), a negative value is  specified for ∆d.

0319

THE END POINT COMMAND IS  ILLEGAL IN THE DRILLING CYCLE

Although the ∆i or ∆k travel distance is set to 0 in a multiple  repetitive canned cutting-off cycle (G74 or G75), a value other  than 0 is specified for a U or W.

0320

ILLEGAL MOVEMENT  

AMOUNT/CUTTING AMOUNT IS IN  THE DRILLING CYCLE

A negative value is specified in a multiple repetitive canned  cutting-off cycle (G74 or G75) as ∆i or ∆k (travel distance/the  depth of cut).

0321

ILLEGAL REPEATED TIME IS IN THE  PATTERN REPEATING CYCLE

A zero or a negative value is specified in a multiple repetitive  canned closed loop cycle (G73) as a repeated time.

0322

FINISHING SHAPE WHICH OVER OF  STARTING POINT

An invalid shape which is over the cycle starting point is  specified in a shape program for a multiple repetitive canned  rough-cutting cycle (G71 or G72).

0323

THE FIRST BLOCK OF SHAPE  PROGRAM IS A COMMAND OF  TYPE II

Type II is specified in the first block of the shape program  specified by P in a multiple repetitive canned rough-cutting cycle  (G71 or G72). Z (W) command is for G71.  

X (U) command is for G72.

0324

THE INTERRUPTION TYPE MACRO  WAS DONE IN THE MULTIPLE  REPETIVE CYCLES

An interruption type macro was issued during the multiple  repetitive canned cycle (G70, G71, G72, or G73).

0325

UNAVAILABLE COMMAND IS IN  SHAPE PROGRAM

An usable command was issued in a shape program for a  multiple repetitive canned cycle (G70, G71, G72, or G73).

0326

LAST BLOCK OF SHAPE PROGRAM  IS A DIRECT DRAWING  

DIMENSIONS

In a shape program in the multiple repetitive canned cycle (G70,  G71, G72, or G73), a command for direct input of drawing  dimensions in the last block is terminated in the middle.

0327

MODAL THAT MULTIPLE REPETIVE  CYCLES CANNOT BE DONE

A multiple repetitive canned cycle (G70, G71, G72, or G73) was  commanded in a modal state in which a multiple repetitive  canned cycle could not be commanded.

0328

ILLEGAL WORK POSITION IS IN THE  TOOL NOSE RADIUS  

COMPENSATION

The specification for the blank side for a tool nose radius  compensation (G41 or G42) is incorrect in a multiple repetitive  canned cycle (G71 or G72).

0329

THE FINISHING SHAPE IS NOT A  MONOTONOUS CHANGE(SECOND  AXES)

In a shape program for the multiple repetitive canned  rough-cutting cycle (G71 or G72), the command of the second  plane axis was not a monotonous increase or decrease.

0330

ILLEGAL AXIS COMMAND IS IN THE  TURNING CANNED CYCLE

An axis other than the plane is specified n a canned cycle(G90,  G92, or G94).

0331

ILLEGAL AXIS NUMBER IN AX[]

An illegal value is specified for an AX[] axis number.

0332

ILLEGAL AXIS ADDRESS IN  

AXNUM[]

An illegal value is specified for an AXNUM[] axis address.

0333

TOO MANY SPINDLE COMMANDS

Multiple spindle commands could be found in the same block in  using an expansion spindle name.  

Only one spindle could be commanded in the same block.

0334

OFFSET IS OUT OF EFFECTIVE  RANGE

An offset data which was out of the effective range was  specified. (malfunction prevention function)

0335

PLURAL M CODE

Multiple M codes are commanded simultaneously in a block for  a wait function with peripheral devices by an M code.

0336

TOOL COMPENSATION  

COMMANDED MORE TWO AXES

For a tool length compensation C, an attempt was made to  command the offset to other axes without canceling the offset.  Or, for a tool length compensation C, multiple axes are specified  in G43 or G44 block.

0337

EXCESS MAXIMUM INCREMENTAL  VALUE

The command value exceeded the maximum amount of  incremental. (malfunction prevention function)

Alarm 

Message

Description

0338

CHECKSUM ERROR

An incorrect value was detected in a checksum.  

(malfunction prevention function)

0340

ILLEGAL RESTART(NANO  

SMOOTHING)

With manual absolute turned on, an attempt was made to restart  the operation in nano smoothing mode after performing the  manual interaction.

0341

TOO MANY COMMAND BLOCK  (NANO SMOOTHING)

There are more blocks than can be commanded consecutively  in nano smoothing mode.

0342

CUSTOM MACRO INTERRUPT  ENABLE IN NANO SMOOTHING

A custom macro interrupt was enabled in nano smoothing  mode. Or, nano smoothing mode was commanded with a  custom macro interrupt enabled.

0343

ILLEGAL COMMAND IN NANO  SMOOTHING

G43, G44, or G49 was commanded during a nano smoothing.

0344

CANNOT CONTINUE NANO  

SMOOTHING

An illegal command or operation by which a nano smoothing  could not be continued was performed.

0345

TOOL CHANGE ILLEGAL Z AXIS  POS

A tool change position on the Z-axis is incorrect.

0346

TOOL CHANGE ILLEGAL TOOL NUM

 A tool change position is not set.

0347

TOOL CHANGE ILLEGAL COMMAND  IN SAME BLK.

Tool changing is commanded twice or more in the same block.

0348

TOOL CHANGE Z AXIS POS NOT  ESTABLISHED

A tool change spindle on the Z-axis is not set.

0349

TOOL CHANGE SPINDLE NOT STOP

 A tool change spindle stop is not stopped.

0350

PARAMETER OF THE INDEX OF  THE SYNCHRONOUS CONTROL  AXIS SET ERROR.

An illegal synchronization control axis number (parameter No.  8180) is set.

0351

BECAUSE THE AXIS IS MOVING,  THE SYNC CONTROL IS CAN'T BE  USED.

While the axis being subject to synchronization control was  moving, an attempt was made to start or cancel the  synchronization control by a synchronization control axis  selection signal.

0352

SYNCHRONOUS CONTROL AXIS  COMPOSITION ERROR.

This error occurred when:  

1) An attempt was made to perform synchronization control for  the axis during a synchronization, composition, or  

superposition.  

2) An attempt was made to synchronize a further  

great-grandchild for a parent-child-grandchild relation.  3) An attempt was made to operate synchronization control  although a parent-child-grandchild relation was not set.

0353

THE INSTRUCTION WAS DONE FOR  THE AXIS WHICH WAS NOT ABLE  TO MOVE.

This error occurred when:  

- For synchronization  

1) A move command was issued to the axis for which  parameter No. 8163#7NUMx is set to 1.  

2) A move command was issued to the slave axis.  - For composition  

1) A move command was issued to the axis for which  parameter No. 8163#7NUMx is set to 1.  

2) A move command was issued to the axis for which  parameter No. 8162#7MUMx is set to 1.

0354

THE G28 WAS INSTRUCTED IN  WITH THE REF POS NOT FIXED IN  SYNC MODE

This error occurred when G28 was specified to the master axis  being parking during synchronization control, but an axis  reference position is not set for the slave axis.

0355

PARAMETER OF THE INDEX OF  THE COMPOSITE CONTROL AXIS  SET ERROR.

An illegal composite control axis number (parameter No. 8183)  is specified.

Alarm 

Message

Description

0356

BECAUSE THE AXIS IS MOVING,  THE COMP CONTROL IS CAN'T BE  USED.

While the axis being subject to composite control was moving,  an attempt was made to start or cancel the composite control by  a composite control axis selection signal.

0357

COMPOSITE CONTROL AXIS  COMPOSITION ERROR.

This error occurred when an attempt was made to perform  composite control for the axis during a synchronization,  composition, or superposition.

0359

THE G28 WAS INSTRUCTED IN  WITH THE REF POS NOT FIXED IN  COMP MODE

This error occurred when G28 was specified to the composite  axis during composite control, but a reference position is not set  to the other part of the composition.

0360

PARAMETER OF THE INDEX OF  THE SUPERPOS CONTROL AXIS  SET ERROR.

An illegal superposition control axis number (parameter No.  8186) is specified.

0361

BECAUSE THE AXIS IS MOVING,  THE SUPERPOS CONTROL IS  CAN'T BE USED.

While the axis being subject to superposition control was  moving, an attempt was made to start or cancel the  superposition control by a superposition control axis selection  signal.

0362

SUPERPOSITION CONTROL AXIS  COMPOSITION ERROR.

This error occurred when:  

1) An attempt was made to perform superposition control for  the axis during a synchronization, composition, or  

superposition.  

2) An attempt was made to synchronize a further  

great-grandchild for a parent-child-grandchild relation.

0363

THE G28 WAS INSTRUCTED IN TO  THE SUPERPOS CONTROL SLAVE  AXIS.

This error occurred when G28 was specified to the  superposition control slave axis during superposition control.

0364

THE G53 WAS INSTRUCTED IN TO  THE SUPERPOS CONTROL SLAVE  AXIS.

This error occurred when G53 was specified to the slave axis  being moved during superposition control.

0365

TOO MANY MAXIMUM SV/SP AXIS  NUMBER  

PER PATH

The maximum control axis number or maximum control spindle  number which could be used within a path was exceeded.  (For a loader path, this alarm is generated if the number of axis  per path is set to 5 or greater.)

0366

IMPROPER G-CODE IN TURRET  METHOD

When the turret change tools method was selected (parameter  No. 5040#3 (TCT) = 0), G43, G43.1, G43.4, G43.5, or G43.7  was commanded.

0367

3-D CONV. WAS COMMANDED IN  SYNC MODE AS THE PARAMETER  PKUx(NO.8162#2) IS 0.

A three-dimensional coordinate conversion was commanded  during synchronization control when the parameter PKUx  (No.8162#2) was 0.

0368

OFFSET REMAIN AT OFFSET  COMMAND

When the ATC change tools method was selected (parameter  No. 5040#3 (TCT) = 1) during G43, G43.1, G43.4, or G43.5  mode, G43.7 was commanded. Or, G43, G43.1, G43.4, or  G43.5 was commanded during G43.7 mode.

0369

G31 FORMAT ERROR

- No axis is specified or tow or more axes are specified in the  torque limit switch instruction (G31P98/P99).  

- The specified torque Q value in the torque limit switch  instruction is out of range. The torque Q range is 1 to 254.  - The high-speed continuous skip option is not present.

Alarm 

Message

Description

0370

G31P/G04Q ERROR

1) The specified address P value for G31 is out of range. The  address P range is 1 to 4 in a multistage skip function.  2) The specified address Q value for G04 is out of range. The  address Q range is 1 to 4 in a multistage skip function.  3) P1-4 for G31, or Q1-4 for G04 was commanded without a  multistage skip function option.  

4) <T series > The specified value of address P of G72 or G74  falls outside the range. Address P ranges from 1 to 4 in the  multistage skip function. P1-4 was specified in G72 or G74  even though the multistage skip function option is not  present.

0371

ILLEGAL FORMAT IN G10 OR L50

In a command format for a programmable parameter input, an  attempt was made to change the parameter for an encryption  (No. 3220), key (No. 3221), or protection range (No.3222 or  No.3223) as a "the encryption function for the key and program."  Modify the program.

0372

REFERENCE RETURN  

INCOMPLETE

An attempt was made to perform an automatic return to the  reference position on the orthogonal axis before the completion  of a return to the reference position on the angular axis.  However, this attempt failed because a manual return to the  reference position during angular axis control or an automatic  return to the reference position after power-up was not  commanded. First, return to the reference position on the  angular axis, then return to the reference position on the  orthogonal axis.

0373

ILLEGAL HIGH-SPEED SKIP SIGNAL

 In the skip commands (G31, G31P1 to G31P4) and dwell  commands (G04, G04Q1 to G04Q4), the same high-speed  signal is selected in different paths.

0374

ILLEGAL REGISTRATION OF TOOL  MANAGER(G10)

G10L75 or G10L76 data was registered during the following  data registration:  

- From the PMC window.  

- From the FOCAS2.  

- By G10L75 or G10L76 in another system.  

Command G10L75 or G10L76 again after the above operation  is completed.

0375

CAN NOT ANGULAR  

CONTROL(SYNC:MIX:OVL)

Angular axis control is disabled for this axis configuration.  1) When some related axes under angular axis control are not  in synchronous control mode or when one angular axis is not  paired with the other angular axis or one Cartesian axis is  not paired with the other Cartesian axis in synchronous  control  

2) When some related axes under composite control are not in  composite control mode or when one angular axis is not  paired with the other angular axis or one Cartesian axis is  not paired with the other Cartesian axis in composite control  

3) When related axes under angular axis control is switched to  superposition control mode1)

0376

SERIAL DCL: ILLEGAL PARAMETER

 1. When Parameter No.1815#1 is set to “1”, parameter  No.2002#3 is set to “0”  

2. The absolute-position detection function is enabled.  (Parameter No.1815#5 is set to “1”. )

0387

ILLEGAL RTM DI/DO VAR

There is no DI/DO variable that has a specified signal address  (alphabet, number).

Alarm 

Message

Description

0389

ILLEGAL RTM SIGNAL BIT

Bits other than bits 0 to 7 cannot be specified with a DI/DO  signal.

0391

RTM BRANCH OVER

The number of branches supported with real time custom  macros was exceeded.

0392

TOO MANY SENTENCE CONTROL

Many reserved words (ZONCE, ZEDGE, ZWHILE, ZDO, ZEND,  G65, M99) for RTM control were used in a real time macro  command.

0393

NO SENTENCE CONTROL

In a real time macro command, there is no data to be assigned.

0394

ILLEGAL SENTENCE CONTROL

The matching of reserved words (ZONCE, ZEDGE, ZWHILE,  ZDO, ZEND, G65, M99) for RTM control is incorrect.

0395

ILLEGAL NC WORD CONTROL

Control code G65 or M99 for calling a subprogram or returning  from a subprogram is not coded correctly.

0396

ILLEGAL RTM SENTENCE  

CONTROL

In other than a real time macro command, a reserved word  (ZONCE, ZEDGE, ZWHILE, ZDO, or ZEND) for RTM control is  used.

0397

RTM BUFFER OVER

There is no buffer available for real time macro commands.  Too many blocks read in advance are buffered as triggers used  by real time macro commands.

0398

'ID OVER IN BUFFER

In blocks read in advance, there are too many real time macro  commands with the same ID.

0399

'ID EXECUTION IN SAME TIME

An attempt was made to execute real time macro commands  with the same ID by using the same NC statement as a trigger.

0400

ONESHOT CMDOVER

Too many one-shot real time macro commands are specified.

0401

EXEC CMD NUM OVER IN SAME  TIME

The number of real time macro commands that can be executed  simultaneously was exceeded

0402

ILLEGAL TOKEN FOR RTM

A token, variable, or function that is not supported by the real  time custom macro function was detected.

0403

ACCESS TO RTM PROTECT VAR

An attempt was made to access a protected variable.

0404

RTM ERROR

An error related to a real time macro command occurred.

0406

CODE AREA SHORTAGE

The storage size of the real time macro area is insufficient.

0407

DOUBLE SLASH IN RTM MODE

In the compile mode, an attempt was made to set the compile  mode again.

0408

G90 IS NOT PERMITTED

The absolute command cannot be specified.

0409

ILLEGAL AXIS NO

An invalid axis number is specified.

0410

MIDDLE POINT IS NOT ZERO

An intermediate point other than 0 is specified with G28.

0411

SIMULTANEOUSLY AXES OVER

The maximum number of axes that can be controlled  simultaneously was exceeded.

0412

ILLEGAL G CODE

An unusable G code was used.

0413

ILLEGAL ADDRESS

An unusable address was used.

0414

ILLEGAL PMC AXIS NO.

An invalid PMC axis number is specified.

0415

GROUP IS IN USE

The group to which the specified axis belongs is already in  used.

0416

UNABLE TO USE THE AXIS

The specified axis cannot be used.

0417

AXIS IS UNABLE TO MOVE

The specified axis is placed in the inoperative state.

0418

ILLEGAL FEED SETTING

An incorrect feedrate is set.

0419

ILLEGAL DISTANCE SETTING

A travel distance beyond the specifiable range is specified.

0420

CONSTANT NUMBER P

A subprogram is specified not by using a constant.

0421

ILLEGAL ARGUMENT G54

With G65, an invalid argument, L, is used.

0422

ILLEGAL ARGUMENT G54

With G65, an invalid argument is used.

0423

NO PMC AXIS CONTROL OPTION

The option for PMC axis control is missing.

0424

MULTIPLE AXES IN ONE GROUP

Multiple axes are using one group.

0425

ONE AXIS USE MULTIPLE GROU

One axis is using multiple groups.

Alarm 

Message

Description

0429

ILLEGAL COMMAND IN G10.6

When retract was started in a threading block, a retract  command had been issued for the long axis direction of  threading.

0430

TOOL LIFE PAIRS ZERO

Tool life management group number parameter No.6813 is 0.

0431

ILLEGAL T/R DATA OF TOOL LIFE

The arbitrary group number (T) or remaining amount setting (R)  is invalid.

0432

UNAVAILABLE POSTURE IN TPC

A command specifying an impossible tool posture was issued in  tool posture control. Review the machine configuration and  command.

0436

ILLEGAL PARAMETER IN WSC

An incorrect parameter was specified in compensation of  workpiece placement error.  

- The basic three axes are not specified in parameter No.1022.

0437

ILLEGAL COMMAND IN WSC

An invalid command related to compensation of workpiece  placement error was specified.  

- An illegal G code was specified in the workpiece placement  error compensation mode.  

- There is an error in the modal setting used when the  compensation of workpiece placement error is started.  - G54.4 was not specified solely.  

- There is not the P command in the block including the G54.4  command. Alternatively, the value following P is out of the  range.  

- Compensation of workpiece placement error was specified  redundantly.

0438

ILLEGAL PARAMETER IN TOOL  DIRC CMP

When compensation of workpiece placement error is performed  in a 5-axis cutting machine (compensation in the tool direction  (bit 0 (RCM) of parameter No. 11200 is 0)), an illegal parameter  is set.  

- Acc./Dec. before interpolation is disabled. Set parameter No.  1660.  

- Acc./Dec. before rapid traverse interpolation is disabled. Set  bit 1 of parameter No. 1401, bit 5 of parameter No. 1950, and  parameter No. 1671.  

- The parameters (No.19680 to No.19714) for configuring the  machine are incorrect.  

- The axis set by parameters No. 19681 and No. 19686 is not a  rotation axis.  

- The basic three axes are not set in parameter No. 1022.  - Bit 6 (TOS) of parameter No. 5006 is set to 0 when tool length  compensation is performed during compensation of workpiece  placement error. Set this parameter to 1.

0439

ILLEGAL COMMAND IN TOOL DIRC  CMP

When compensation of workpiece placement error was  performed in a 5-axis cutting machine (compensation in the tool  direction (bit 0 (RCM) of parameter No. 11200 is 0)), an illegal  command was issued.  

- An unspecifiable G code was specified.  

- There is an error in the modal setting used during startup.  - An axis not related to 5-axis machining was specified.  - The absolute coordinates of a rotation axis could not be  

obtained in the startup block of compensation of workpiece  placement error or tool center point control.

0445

ILLEGAL AXIS OPERATION

The positioning command was issued in the speed control  mode. Check the SV speed control mode in-progress signal.

Alarm 

Message

Description

0446

ILLEGAL COMMAND IN  

 G96.1/G96.2/G96.3/G96.4

G96.1, G96.2, G96.3, and G96.4 are specified in the block that  includes other commands. Modify the program.

0447

ILLEGAL SETTING DATA

The live tool axis is incorrectly set. Check the parameter for  spindle control with servo motor.

0455

ILLEGAL COMMAND IN GRINDING

In grinding canned cycles:  

1) <M series> The signs of the I, J, and K commands do not  match.  

2) <M series/T series > The amount of travel of the grinding  axis is not specified.

0456

ILLEGAL PARAMETER IN GRINDING

 Parameters related to grinding canned cycles are incorrectly set.  Probable causes are given below.  

1) <M series/T series> The axis number of the grinding axis is  incorrectly set (parameters No. 5176 to No. 5179).  2) <M series> The axis number of the dressing axis is  incorrectly set (parameters No. 5180 to No. 5183).  3) <M series/T series> The axis numbers of the cut axis,  grinding axis, and dressing axis (only for the M series)  overlap.

0460

ILLEGAL TORCH AXIS NUMBER

The axis number set in parameter No. 5490 (torch control axis) exceeds the number of control axes.

0461

ILLEGAL SETTING OF ROTATE AXIS FOR TORCH

The parameter setting (bit 0 of parameter No. 1006 = 1) of the rotation axis is not applied to the torch turning axis.

1014

ILLEGAL FORMAT OF PROGRAM  NO.

Address O or N is not followed by a number.

1016

EOB NOT FOUND

EOB (End of Block) code is missing at the end of a program  input in the MDI mode.

1018

M99 IN MAIN PROGRAM

A M99 was commanded during main program when the  parameter AMM (No. 7712#4) = 1 was set.

1059

COMMAND IN BUFFERING MODE

The manual intervention compensation request signal MIGET  became “1” when a advanced block was found during automatic  operation.  

To input the manual intervention compensation during automatic  operation, a sequence for manipulating the manual intervention  compensation request signal MIGET is required in an M code  instruction without buffering.

1077

PROGRAM IN USE

An attempt was made in the foreground to execute a program  being edited in the background.  

The currently edited program cannot be executed, so end  editing and restart program execution.

1079

PROGRAM FILE NOT FOUND

The program of the specified file No. is not registered in an  external device. (external device subprogram call)

1080

DUPLICATE DEVICE SUB  

PROGRAM CALL

Another external device subprogram call was made from a  subprogram after the subprogram called by the external device  subprogram call.

1081

EXT DEVICE SUB PROGRAM CALL  MODE ERROR

The external device subprogram call is not possible in this  mode.

1091

DUPLICATE SUB-CALL WORD

More than one subprogram call instruction was specified in the  same block.

1092

DUPLICATE MACRO-CALL WORD

More than one macro call instruction was specified in the same  block.

1093

DUPLICATE NC-WORD & M99

An address other than O, N, P or L was specified in the same  block as M99 during the macro modal call state.

Alarm

Message

Description

1095

TOO MANY TYPE-2 ARGUMENT

More than ten sets of I, J and K arguments were specified in the  type–II arguments (A, B, C, I, J, K, I, J, K, ...) for custom  macros.

1096

ILLEGAL VARIABLE NAME

An illegal variable name was specified. A code that cannot be  specified as a variable name was specified. [#_OFSxx] does not  match the tool offset memory option configuration.

1097

TOO LONG VARIABLE NAME

The specified variable name is too long.

1098

NO VARIABLE NAME

The specified variable name cannot be used as it is not  registered.

1099

ILLLEGAL SUFFIX [ ]

A suffix was not specified to a variable name that required a  suffix enclosed by [ ].  

A suffix was specified to a variable name that did not require a  suffix enclosed by [ ].  

The value enclosed by the specified [ ] was out of range.

1100

CANCEL WITHOUT MODAL CALL

Call mode cancel (G67) was specified even though macro  continuous–state call mode (G66) was not in effect.

1101

ILLEGAL CNC STATEMENT IRT.

An interrupt was made in a state where a custom macro  interrupt containing a move instruction could not be executed.

1115

READ PROTECTED VARIABLE

An attempt was made in a custom macro to use on the right  side of an expression a variable that can only be used on the left  side of an expression.

1120

ILLEGAL ARGUMENT FORMAT

The specified argument in the argument function (ATAN, POW)  is in error.

1124

MISSING DO STATEMENT

The DO instruction corresponding to the END instruction was  missing in a custom macro.

1125

ILLEGAL EXPRESSION FORMAT

The description of the expression in a custom macro statement  contains an error.  

A parameter program format error.  

The screen displayed to enter periodic maintenance data or item  selection menu (machine) data does not match the data type.

1128

SEQUENCE NUMBER OUT OF  RANGE

The jump destination sequence No. in a custom macro  statement GOTO instruction was out of range (valid range: 1 to  99999999).

1131

MISSING OPEN BRACKET

The number of left brackets ([) is less than the number of right  brackets (]) in a custom macro statement.

1132

MISSING CLOSE BRACKET

The number of right brackets (]) is less than the number of left  brackets ([) in a custom macro statement.

1133

MISSING '='

An equal sign (=) is missing in the arithmetic calculation  instruction in a custom macro statement.

1134

MISSING ','

A delimiter (,) is missing in a custom macro statement.

1137

IF STATEMENT FORMAT ERROR

The format used in the IF statement in a custom macro is in  error.

1138

WHILE STATEMENT FORMAT  ERROR

The format used in the WHILE statement in a custom macro is  in error.

1139

SETVN STATEMENT FORMAT  ERROR

The format used in the SETVN statement in a custom macro is  in error.

1141

ILLEGAL CHARACTER IN VAR.  NAME

The SETVN statement in a custom macro contacts a character  that cannot be used in a variable name.

1142

TOO LONG V-NAME (SETVN)

The variable name used in a SETVN statement in a custom  macro exceeds 8 characters.

1143

BPRNT/DPRNT STATEMENT  

FORMAT ERROR

The format used in the BPRINT statement or DPRINT  statement is in error.

Alarm

Message

Description

1144

G10 FORMAT ERROR

The G10 L No. contains no relevant data input or corresponding  option.  

Data setting address P or R is not specified.  

An address not relating to the data setting is specified. Which  address to specify varies according to the L No.  

The sign, decimal point or range of the specified address are in  error.

1145

G10.1 TIME OUT

The response to a G10.1 instruction was not received from the  PMC within the specified time limit.

1146

G10.1 FORMAT ERROR

The G10.1 instruction format is in error.

1152

G31.9/G31.8 FORMAT ERROR

The format of the G31.9 or G31.8 block is erroneous in the  following cases:  

- The axis was not specified in the G31.9 or G31.8 block.  - Multiple axes were specified in the G31.9 or G31.8 block.  - The P code was specified in the G31.9 or G31.8 block.

1153

CANNOT USE G31.9

G31.9 cannot be specified in this modal state. This alarm is also  generated when G31.9 is specified when a group 07 G code  (e.g. tool radius compensation) is not canceled.

1160

COMMAND DATA OVERFLOW

An overflow occurred in the position data within the CNC. This alarm is also generated if the target position of a command  exceeds the maximum stroke as a result of calculation such as  coordinate conversion, offset, or introduction of a manual  intervention amount.

1180

ALL PARALLEL AXES IN PARKING

All of the axis specified for automatic operation are parked.

1196

ILLEGAL DRILLING AXIS SELECTED

 An illegal axis was specified for drilling in a canned cycle for  drilling.  

If the zero point of the drilling axis is not specified or parallel  axes are specified in a block containing a G code in a canned  cycle, simultaneously specify the parallel axes for the drilling  axis.

1200

PULSCODER INVALID ZERO  

RETURN

The grid position could not be calculated during grid reference  position return using the grid system as the one–revolution  signal was not received before leaving the deceleration dog.  This alarm is also generated when the tool does not reach a  feedrate that exceeds the servo error amount preset to  parameter No. 1841 before the deceleration limit switch is left  (deceleration signal *DEC returns to “1”).

1202

NO F COMMAND AT G93

F codes in the inverse time specification mode (G93) are not  handled as modal, and must be specified in individual blocks.

1223

ILLEGAL SPINDLE SELECT

1) An attempt was made to execute an instruction that uses the  spindle although the spindle to be controlled has not been  set correctly.  

2) Interpolation type rigid tapping was specified in a path in  which the Cs contour control function is not enabled.

1282

ILLEGAL COMMAND IN 3-D OFFSET

 An illegal G code was specified in the 3-dimensional tool  compensation mode.

1283

ILLEGAL IJK IN 3-D OFFSET

When bit 0 (ONI) of parameter No. 6029 is set to 1, I, J, and K  commands are specified without the decimal point in  3-dimensional tool compensation mode.

1298

ILLEGAL INCH/METRIC  

CONVERSION

An error occurred during inch/metric switching.

Alarm 

Message

Description

1300

ILLEGAL ADDRESS

The axis No. address was specified even though the parameter  is not an axis–type while loading parameters or pitch error  compensation data from a tape or by entry of the G10  parameter.  

Axis No. cannot be specified in pitch error compensation data.

1301

MISSING ADDRESS

The axis No. was not specified even though the parameter is an  axis–type while loading parameters or pitch error compensation  data from a tape or by entry of the G10 parameter.  Or, data No. address N, or setting data address P or R are not  specified.

1302

ILLEGAL DATA NUMBER

A non–existent data No. was found while loading parameters or  pitch error compensation data from a tape or by entry of the G10  parameter.  

An invalid address R value is specified in a pattern program for  each machining purpose on the high–speed high–precision  setting screen.  

This alarm is also generated when illegal word values are found.

1303

ILLEGAL AXIS NUMBER

An axis No. address exceeding the maximum number of  controlled axes was found while loading parameters from a tape  or by entry of the G10 parameter.

1304

TOO MANY DIGIT

Data with too many digits was found while loading parameters or  pitch error compensation data from a tape.

1305

DATA OUT OF RANGE

Out–of–range data was found while loading parameters or pitch  error compensation data from a tape.  

The values of the data setting addresses corresponding to L  Nos. during data input by G10 was out of range.  

This alarm is also generated when NC programming words  contain out–of–range values.

1306

MISSING AXIS NUMBER

A parameter which requires an axis to be specified was found  without an axis No. (address A) while loading parameters from a  tape.

1307

ILLEGAL USE OF MINUS SIGN

Data with an illegal sign was found while loading parameters or  pitch error compensation data from a tape, or by entry of the  G10 parameter. A sign was specified to an address that does  not support the use of signs.

1308

MISSING DATA

An address not followed by a numeric value was found while  loading parameters or pitch error compensation data from a  tape.

1329

ILLEGAL MACHINE GROUP  

NUMBER

An machine group No. address exceeding the maximum  number of controlled machine groups was found while loading  parameters from a tape or by entry of the G10 parameter.

1330

ILLEGAL SPINDLE NUMBER

An spindle No. address exceeding the maximum number of  controlled spindles was found while loading parameters from a  tape or by entry of the G10 parameter.

1331

ILLEGAL PATH NUMBER

An path No. address exceeding the maximum number of  controlled path was found while loading parameters from a tape  or by entry of the G10 parameter.

1332

DATA WRITE LOCK ERROR

Could not load data while loading parameters, pitch error  compensation data and work coordinate data from tape.

1333

DATA WRITE ERROR

Could not write data while loading data from tape.

1360

PARAMETER OUT OF RANGE  (TLAC)

Illegal parameter setting. (Set value is out of range.)

1361

PARAMTER SETTING ERROR 1  (TLAC)

Illegal parameter setting. (axis of rotation setting)

Alarm 

Message

Description

1362

PARAMETER SETTING ERROR 2  (TLAC)

Illegal parameter setting (tool axis setting)

1370

PARAMETER SETTING ERROR  (DM3H-1)

Out–of–range data was set during setting of the  

three–dimensional handle feed parameter.

1371

PARAMETER SETTING ERROR  (DM3H-2)

An illegal axis of rotation was set during setting of the  three–dimensional handle feed parameter.

1372

PARAMETER SETTING ERROR  (DM3H-3)

An illegal master axis was set during setting of the  three–dimensional handle feed parameter.

1373

PARAMETER SETTING ERROR  (DM3H-4)

An illegal parallel axis or twin table was set during setting of the  three–dimensional handle feed parameter.

1470

G40.1 –G42.1 PARAMETER MISS

A parameter setting related to normal direction control is illegal. The axis number of a normal direction controlled axis is set in  parameter No. 5480, but that axis number is in the range of the  number of controlled axes.  

The axis set as a normal direction controlled axis is not set as a  rotation axis (ROTx, bit 0 of parameter No. 1006) = 1 and  No.1022=0).  

Set the feedrate at which to insert rotation about a normal  direction controlled axis in parameter No. 5481, in the range of 1  to 15000 mm/min.

1508

DUPLICATE M-CODE (INDEX TABLE  REVERSING)

A function to which the same code as this M code is set exists.  (index table indexing)

1509

DUPLICATE M-CODE  

(SPOS AXIS ORIENTATION)

A function to which the same code as this M code is set exists.  (spindle positioning, orientation)

1510

DUPLICATE M-CODE (SPOS AXIS  POSITIONING)

A function to which the same code as this M code is set exists.  (spindle positioning, positioning)

1511

DUPLICATE M-CODE (SPOS AXIS  RELEASE)

A function to which the same code as this M code is set exists.  (spindle positioning, mode cancel)

1531

ILLEGAL USE OF DECIMAL POINT  (F-CODE)

When the feedrate instruction contains valid data below the  decimal point, the alarm is set and the F code contains valid  data below the decimal point.

1532

ILLEGAL USE OF DECIMAL POINT  (E-CODE)

When the feedrate instruction contains valid data below the  decimal point, the alarm is set and the E code contains valid  data below the decimal point.

1533

ADDRESS F UNDERFLOW (G95)

The feedrate for the hole drilling axis calculated from the F and  S codes is too slow in the feed per single rotation mode (G95).

1534

ADDRESS F OVERFLOW (G95)

The feedrate for the hole drilling axis calculated from the F and  S codes is too fast in the feed per single rotation mode (G95).

1535

ADDRESS E UNDERFLOW (G95)

The feedrate for the hole drilling axis calculated from the E and  S codes is too slow in the feed per single rotation mode (G95).

1536

ADDRESS E OVERFLOW (G95)

The feedrate for the hole drilling axis calculated from the E and  S codes is too fast in the feed per single rotation mode (G95).

1537

ADDRESS F UNDERFLOW  

(OVERRIDE)

The speed obtained by applying override to the F instruction is  too slow.

1538

ADDRESS F OVERFLOW  

(OVERRIDE)

The speed obtained by applying override to the F instruction is  too fast.

1539

ADDRESS E UNDERFLOW  

(OVERRIDE)

The speed obtained by applying override to the E instruction is  too slow.

1540

ADDRESS E OVERFLOW  

(OVERRIDE)

The speed obtained by applying override to the E instruction is  too fast.

1541

S-CODE ZERO

“0” has been instructed as the S code.

1542

FEED ZERO (E-CODE)

“0” has been instructed as the feedrate (E code).

1543

ILLEGAL GEAR SETTING

The gear ratio between the spindle and position coder, or the  set position coder number of pulses is illegal in the spindle  positioning function.

Alarm 

Message

Description

1544

S-CODE OVER MAX

The S command exceeds the maximum spindle rotation  number.

1548

ILLEGAL AXIS MODE

The spindle positioning axis/Cs contour control axis was  specified during switching of the controlled axis mode.

1561

ILLEGAL INDEXING ANGLE

The specified angle of rotation is not an integer multiple of the  minimum indexing angle.

1564

INDEX TABLE AXIS – OTHER AXIS  SAME TIME

The index table indexing axis and another axis have been  specified in the same block.

1567

INDEX TABLE AXIS DUPLICATE  AXIS COMMAND

Index table indexing was specified during axis movement or on  an axis for which the index table indexing sequence was not  completed.

1580

ENCODE ALARM (PSWD&KEY)

When an attempt was made to read a program, the specified  password did not match the password on the tape and the  password on tape was not equal to 0.  

When an attempt was made to punch an encrypted tape, the  password was not in the range 0 to 99999999.  

The password parameter is No. 2210.

1581

ENCODE ALARM (PARAMETER)

When an attempt was made to punch an encrypted tape, the  punch code parameter was set to EIA. Set parameter ISO (No.  0000#1) to “0”. An incorrect instruction was specified for  program encryption or protection.  

This alarm is generated if an attempt is made to perform  program editing, deletion, or range-specified punch-out in the  protected range in the lock state. Or, a program outside the  protected range is specified in rage specification punch-out in  the unlock state.  

The protected range is defined from the program No. preset by  parameter No. 3222 up to the program No. preset to parameter  No. 3223. When both parameters are set to “0”, the protected  range becomes O9000 to O9999.

1590

TH ERROR

A TH error was detected during reading from an input device.  The read code that caused the TH error and how many  statements it is from the block can be verified in the diagnostics  screen.

1591

TV ERROR

An error was detected during the single–block TV error.  The TV check can be suppressed by setting TVC parameter No.  0000#0 to “0”.

1592

END OF RECORD

The EOR (End of Record) code is specified in the middle of a  block.  

This alarm is also generated when the percentage at the end of  the NC program is read.  

For the program restart function, this alarm is generated if a  specified block is not found.

1593

EGB PARAMETER SETTING ERROR

 Error in setting a parameter related to the EGB  

(1) The setting of SYN, bit 0 of parameter No. 2011, is not  correct.  

(2) The slave axis specified with G81 is not set as a rotation  axis. (ROT, bit 0 of parameter No. 1006)  

(3) Number of pulses per rotation (Parameter (No. 7772 or No.  7773) or (No. 7782 or 7783) is not set.)  

(4) For a hobbing-machine-compatible command, parameter No.  7710 is not specified.

Alarm

Message

Description

1594

EGB FORMAT ERROR

Error in the format of the block of an EGB command  (1) T (number of teeth) is not specified in the G81 block.  (2) In the G81 block, the data specified for one of T, L, P, and Q  is out of its valid range.  

(3) n the G81 block, only one of P and Q is specified.  (4) In the G81.5 block, there is no command for the master or  slave axis.  

(5) In the G81.5 block, data out of the specified range is  specified for the master or slave axis.

1595

ILL-COMMAND IN EGB MODE

During synchronization with the EGB, a command that must not  be issued is issued.  

(1) Slave axis command using G27, G28, G29, G30,G30.1,  G33, G53, etc.  

(2) Inch/metric conversion command using G20, G21, etc.

1596

EGB OVERFLOW

An overflow occurred in the calculation of the synchronization  coefficient.

1597

EGB AUTO PHASE FORMAT ERROR

 Format error in the G80 or G81 block in EGB automatic phase  synchronization  

(1) R is outside the permissible range.

1598

EGB AUTO PHASE PARAMETER  SETTING ERROR

Error in the setting of a parameter related to EGB automatic  phase synchronization  

(1) The acceleration/deceleration parameter is not correct.  (2) The automatic phase synchronization parameter is not  correct.

1618

ILLEGAL P-DATA(WHEEL WEAR  COMPENSATION)

There is an error in P-data in compensation selection of grinding  wheel wear compensation. Alternatively, the P command is not  present.

1619

ILLEGAL AXIS(WHEEL WEAR  COMPENSATION)

The compensation axis was switched in the grinding wheel wear  compensation mode or compensation vector hold mode.  Alternatively, parameters No. 5071 and No. 5072, which  determine the axis to be subjected to grinding wheel wear  compensation, are incorrectly set.

1805

ILLEGAL COMMAND

[I/O Device]  

An attempt was made to specify an illegal command during I/O  processing on an I/O device.  

[G30 Zero Return]  

The P address Nos. for instructing No. 2 to No. 4 zero return  are each out of the range 2 to 4.  

[Single Rotation Dwell]  

The specified spindle rotation is “0” when single rotation dwell  is specified.  

[3-dimensional tool compensation]  

A G code that cannot be specified was specified in the  3-dimensional tool compensation mode.  

Scaling instruction G51, skip cutting G31 and automatic tool  length measurement G37 were specified.

1806

DEVICE TYPE MISS MATCH

An operation not possible on the I/O device that is currently  selected in the setting was specified.  

This alarm is also generated when file rewind is instructed even  though the I/O device is not a FANUC Cassette.

1807

PARAMETER SETTING ERROR

An I/O interface option that has not yet been added on was  specified.  

The external I/O device and baud rate, stop bit and protocol  selection settings are erroneous.

Alarm 

Message

Description

1808

DEVICE DOUBLE OPENED

An attempt was made to open a device that is being accessed.

1809

ILLEGAL COMMAND IN G41/G42

Specified direction tool length compensation parameters are  incorrect.  

A move instruction for a axis of rotation was specified in the  specified direction tool length compensation mode.

1820

ILLEGAL DI SIGNAL STATE

1. An each axis workpiece coordinate system preset signal  was turned “1” in the state in which all axes on the path  including the axis on which to perform preset with the each  axis workpiece coordinate system were not stopped or in  which a command was in execution.  

2. When an M code for performing preset with an each axis  workpiece coordinate system preset signal was specified,  the each axis workpiece coordinate system preset signal  was not turned “1”.  

3. The auxiliary function lock is enabled.  

4. When bit 6 (PGS) of parameter No. 3001 was set to 0 (M, S,  T, and B codes are not output in the high speed program  check mode), an M code for turning “1” an each axis  workpiece coordinate system preset signal in the high speed  program check mode was specified.

1823

FRAMING ERROR(1)

The stop bit of the character received from the I/O device  connected to reader/punch interface 1 was not detected.

1830

DR OFF(2)

The data set ready input signal DR of the I/O device connected  to reader/punch interface 2 turned OFF.

1832

OVERRUN ERROR(2)

The next character was received from the I/O device connected  to reader/punch interface 2 before it could read a previously  received character.

1833

FRAMING ERROR(2)

The stop bit of the character received from the I/O device  connected to reader/punch interface 2 was not detected.

1834

BUFFER OVERFLOW(2)

The NC received more than 10 characters of data from the I/O  device connected to reader/punch interface 2 even though the  NC sent a stop code (DC3) during data reception.

1889

ILLEGAL COMMAND IN G54.3

An illegal command was issued in G54.3 block.  

(1) An attempt was made to command G54.3 in a mode in which  it cannot be accepted.  

(2) The command was not issued in a single block.

1898

ILLEGAL PARAMETER IN G54.2

An illegal parameter (Nos. 6068 to 6076) was specified for  fixture offset.

1912

V-DEVICE DRIVER ERROR (OPEN)

An error occurred during device driver control.

1960

ACCESS ERROR (MEMORY CARD)

Illegal memory card accessing  

This alarm is also generated during reading when reading is  executed up to the end of the file without detection of the EOR  code.

1961

NOT READY (MEMORY CARD)

The memory card is not ready.

1962

CARD FULL (MEMORY CARD)

The memory card has run out of space.

1963

CARD PROTECTED (MEMORY  CARD)

The memory card is write–protected.

1964

NOT MOUNTED (MEMORY CARD)

The memory card could not be mounted.

1965

DIRECTORY FULL (MEMORY CARD)

 The file could not be generated in the root directory for the  memory card.

1966

FILE NOT FOUND (MEMORY CARD)

The specified file could not be found on the memory card.

1967

FILE PROTECTED (MEMORY CARD)

 The memory card is write–protected.

Alarm

Message

Description

1968

ILLEGAL FILE NAME (MEMORY  CARD)

Illegal memory card file name

1969

ILLEGAL FORMAT (MEMORY CARD)

 Check the file name.

1970

ILLEGAL CARD (MEMORY CARD)

This memory card cannot be handled.

1971

ERASE ERROR (MEMORY CARD)

An error occurred during memory card erase.

1972

BATTERY LOW (MEMORY CARD)

The memory card battery is low.

1973

FILE ALREADY EXIST

A file having the same name already exists on the memory card.

1990

SPL:ILLEGAL AXIS COMMAND

The axis specified by the smooth interpolation (G5.1Q2) is  illegal.

1993

SPL:CAN'T MAKE VECTOR

The end point and the 2 previous point are the same in  generation of the 3-dimensional tool compensation vector by the  end point for smooth interpolation.

1995

ILLEGAL PARAMETER IN  

G41.2/G42.2

The parameter settings (parameter Nos. 6080 to 6089) for  determining the relationship between the axis of rotation and the  rotation plane are incorrect.

1999

ILLEGAL PARAMETER IN G41.3

The parameter settings (parameter Nos. 6080 to 6089) for  determining the relationship between the axis of rotation and the  rotation plane are incorrect.

2002

NO KNOT COMMAND (NURBS)

Knot has not been specified, or a block not related to NURBS  interpolation was specified in the NURBS interpolation mode.

2003

ILLEGAL AXIS COMMAND (NURBS)

An axis not specified as a control point was specified in the No.  1 block.

2004

ILLEGAL KNOT

There is an insufficient number of knot individual blocks.

2005

ILLEGAL CANCEL (NURBS)

The NURBS interpolation mode was turned OFF even though  NURBS interpolation was not completed.

2006

ILLEGAL MODE (NURBS)

A mode that cannot be paired with the NURBS interpolation  mode was specified.

2007

ILLEGAL MULTI-KNOT

Nested knots for each level can be specified for the start and  end points.

2032

EMBEDDED ETHERNET/DATA SERVER ERROR

An error was returned in the built-in Ethernet/data server function.  

For details, see the error message screen of the built-in  Ethernet or data server.

2051

#200-#499ILLEGAL P-CODE MACRO  COMMON INPUT(NO OPTION)

An attempt was made to enter a custom macro common  variable not existing in the system.

2052

#500-#549P-CODE MACRO  

COMMON SELECT(CANNOT USE  SETVN)

The variable name cannot be entered.  

The SETVN command cannot be used with the P-CODE macro  common variables #500 to #549.

2053

THE NUMBER OF #30000 IS  

UNMATCH

An attempt was made to enter a P-CODE-only variable not  existing in the system.

2054

THE NUMBER OF #40000 IS  

UNMATCH

An attempt was made to enter an extended P-CODE-only  variable not existing in the system.

2060

ILLEGAL PARAMETER IN  

G43.4/G43.5

The parameter for the pivot tool length compensation is  incorrect.

Alarm 

Message

Description

2061

ILLEGAL COMMAND IN G43.4/G43.5

An illegal command was specified in tool center point control.  - A rotation axis command was specified in tool center point  control (type 2) mode.  

- With a table rotary type or mixed-type machine, a I, J, or K  command was specified in the tool center point control (type 2)  command (G43.5) block.  

- A command that does not move the tool center point (only a  rotation axis is moved) was specified for the workpiece in the  G02 mode.  

- G43.4 or G43.5 was specified in the tool center point control  mode.  

- When the workpiece coordinate system is set as the  programming coordinate system (bit 5 (WKP) of parameter No.  19696 is 1), G02 or G03 was specified while the rotation axis  was not perpendicular to the plane.

4010

ILLEGAL REAL VALUE OF OBUF :

The real value for a output buffer is in error.

5006

TOO MANY WORD IN ONE BLOCK

The number of words in a block exceeds the maximum. The  maximum is 26 words. However, this figure varies according to  NC options. Divide the instruction word into two blocks.

5007

TOO LARGE DISTANCE

Due to compensation, point of intersection calculation,  interpolation or similar reasons, a movement distance that  exceeds the maximum permissible distance was specified.  Check the programmed coordinates or compensation amounts.

5009

PARAMETER ZERO (DRY RUN)

The dry run feedrate parameter No. 1410 or maximum cutting  feedrate parameter No. 1422 for each axis has been set to 0.

5010

END OF RECORD

The EOR (End of Record) code is specified in the middle of a  block. This alarm is also generated when the percentage at the  end of the NC program is read.

5011

PARAMETER ZERO (CUT MAX)

The maximum cutting feedrate parameter No. 1430 has been  set to 0.

5014

TRACE DATA NOT FOUND

A transfer could not be made because of no trace data.

5015

NO ROTATION AXIS

No rotation axis was found in a handle feed in the tool axis  direction or in the tool axis right angle direction.

5016

ILLEGAL COMBINATION OF M  CODES

M codes which belonged to the same group were specified in a  block. Alternatively, an M code which must be specified without  other M codes in the block was specified in a block with other M  codes.

5018

POLYGON SPINDLE SPEED ERROR

 In G51.2 mode, the speed of the spindle or polygon  synchronous axis either exceeds the clamp value or is too small.  The specified rotation speed ratio thus cannot be maintained.  For polygon turning between spindles:  

More information as to why this alarm occurred is indicated in  DGN No. 471.

5020

PARAMETER OF RESTART ERROR

An invalid value is set in parameter No. 7310, which specifies the axis order in which the tool is moved along axes to the  machining restart position in dry run. A value ranging from 1 to  the number of controlled axes may be set in this parameter.

5043

TOO MANY G68 NESTING

Three-dimensional coordinate conversion has been specified  three or more times.  

To perform another coordinate conversion, perform cancellation,  then specify the coordinate conversion.

Alarm 

Message

Description

5044

G68 FORMAT ERROR

Errors for three-dimensional coordinate conversion command  are:  

(1) No I, J, or K command was issued in three-dimensional  coordinate conversion command block. (without coordinate  rotation option)  

(2) All of I, J, or K commands were 0 in three-dimensional  coordinate conversion command block.  

(3) No rotation angle R was not commanded in  

three-dimensional coordinate conversion command block.

5046

ILLEGAL PARAMETER (S-COMP)

The setting of a parameter related to straightness compensation  contains an error.  

Possible causes include:  

- A non-existent axis number is set in a moving or compensation  axis parameter.  

- More than 128 pitch error compensation points are set  between the furthest points in the negative and position  regions.  

- The straightness compensation point numbers do not have  correct magnitude relationships.  

- No straightness compensation point is found between the  furthest pitch error compensation point in the negative region  and that in the positive region.  

- The compensation per compensation point is either too large  or too small.

5050

ILL-COMMAND IN G81.1 MODE

During chopping, a move command has been issued for the  chopping axis.

5058

G35/G36 FORMAT ERROR

A command for switching the major axis has been specified for  circular threading. Alternatively, a command for setting the  length of the major axis to 0 has been specified for circular  threading.

5060

ILLEGAL PARAMETER IN  

G02.3/G03.3

The axis parameter setting to perform an exponential  interpolation is in error.  

Parameter No. 5641:  

A liner axis number for performing an exponential interpolation  Parameter No. 5642:  

A rotation axis number for performing an exponential  interpolation  

The settable value is 1 to the number of control axes, but it must  not be duplicated.

5061

ILLEGAL FORMAT IN G02.3/G03.3

The exponential interpolation command (G02.3/G03.3) has a  format error.  

The command range for address I or J is -89.0 to -1.0 or +1.0 to  +89.0. No I or J is specified or out-of -range value is specified.  No address R, or 0 is specified.

5062

ILLEGAL COMMAND IN G02.3/G03.3

The value specified in an exponential interpolation command  (G02.3/03.3) is illegal. A value that does not allow exponential  interpolation is specified. (For example, the value for In is 0 or  negative.)

5064

DIFFERRENT AXIS UNIT

Circular interpolation has been specified on a plane consisting  of axes having different increment systems.

5065

DIFFERRENT AXIS UNIT(PMC AXIS)

 Axes having different increment systems have been specified in  the same DI/DO group for PMC axis control. Modify the setting  of parameter No. 8010.

Alarm

Message

Description

5066

RESTART ILLEGAL SEQUENCE  NUMBER

A sequence number from 7000 to 7999 was read during the  search for the next number in a restart program for the back or  restart function.

5068

FORMAT ERROR IN G31P90

No travel axis was specified. Two or more travel axes were  specified.

5073

NO DECIMAL POINT

No decimal point has been specified for an address requiring a  decimal point.

5074

ADDRESS DUPLICATION ERROR

The same address has been specified two or more times in a  single block. Alternatively, two or more G codes in the same  group have been specified in a single block.

5085

SMOOTH IPL ERROR 1

A block for specifying smooth interpolation contains a syntax  error.

5110

IMPROPER G-CODE (AICC MODE)

An unspecifiable G code was specified in the AI contour control  mode.

5115

ILLEGAL ORDER (NURBS)

There is an error in the specification of the rank.

5116

ILLEGAL KNOT VALUE (NURBS)

Monotone increasing of knots is not observed.

5117

ILLEGAL 1ST CONTROL POINT  (NURBS)

The first control point is incorrect.  

Or, it does not provide a continuity from the previous block.

5118

ILLEGAL RESTART (NURBS)

After manual intervention with manual absolute mode set to on,  NURBS interpolation was restarted.

5122

ILLEGAL COMMAND IN SPIRAL

A spiral interpolation or conical interpolation command has an  error. Specifically, this error is caused by one of the following:  1) L = 0 is specified.  

2) Q = 0 is specified.  

3) R/, R/, C is specified.  

4) Zero is specified as height increment.  

5) Zero is specified as height difference.  

6) Three or more axes are specified as the height axes.  7) A height increment is specified when there are two height  axes.  

8) Q is specified when radius difference = 0.  

9) Q < 0 is specified when radius difference > 0.  10) Q > 0 is specified when radius difference < 0.  11) A height increment is specified when no height axis is  specified.

5123

OVER TOLERANCE OF END POINT  IN SPIRAL

The difference between a specified end point and the calculated  end point exceeds the allowable range (parameter 3471).

5124

CAN NOT COMMAND SPIRAL

A spiral interpolation or conical interpolation was specified in  any of the following modes:  

1) Scaling  

2) Polar coordinate interpolation  

3) In tool radius⋅tool nose radius compensation mode, the  center is set as the end point.

5130

NC AND SUPERIMPOSE AXIS  CONFLICT

In the PMC superposition axis control, the NC command and  The PMC axis control command were conflicted. Modify the  program and the ladder.

5131

NC COMMAND IS NOT COMPATIBLE

 The PMC axis control and three-dimensional coordinate  conversion or a polar coordinate interpolation were specified  simultaneously.

5132

CANNOT CHANGE SUPERIMPOSED  AXIS

The superposition axis was selected for the axis for which the  PMC superposition axis is being controlled.

Alarm 

Message

Description

5195

DIRECTION CAN NOT BE JUDGED

Measurement is invalid in the tool compensation measurement  value direct input B function.  

[For 1-contact input]  

1. The recorded pulse direction is not constant.  

- The machine is at a stop in the offset write mode.  - The servo power is off.  

- Pulse directions are diverse.  

2. The tool is moving along the two axes (X-axis and Y-axis).  [For the movement direction discrimination specification]  1. The recorded pulse direction is not constant.  

- The machine is at a stop in the offset write mode.  - The servo power is off.  

- Pulse directions are diverse.  

2. The tool is moving along the two axes (X-axis and Z-axis).  3. The direction indicated by the tool compensation write  signal does not match the movement direction of the axis.

5196

ILLEGAL AXIS OPERATION

During HPCC or during the execution of a 5-axis-related  function, an unavailable function was used.

5220

REFERENCE POINT ADJUSTMENT  MODE

In case of distance coded linear scale I/F, the reference point  auto setting parameter (No.1819#2) is set to "1". Move the  machine to reference position by manual operation and execute  manual reference return.

5242

ILLEGAL AXIS NUMBER

A master axis number or a slave axis number was not set  correctly when the flexible synchronization control mode was  turned from off to on during automatic operation.

5243

DATA OUTRANGE

A gear ratio was not set correctly when the flexible  synchronization control mode was turned from off to on during  automatic operation.

5244

TOO MANY DI ON

- During automatic operation, the mode signal was not turned on  or off if the flexible synchronization control mode was turned  from off to on or or from on to off, after an M code was  executed.  

- An attempt was made to turn on or off the flexible  synchronization control mode when the axis was not stopped.

Alarm 

Message

Description

5245

OTHER AXIS ARE COMMANDED

- For a flexible synchronization control group for which a PMC  axis was a master axis, an attempt was made to turn on the  synchronous mode during time other than automatic operation.

- An attempt was made to turn on a synchronization group for  which an PMC axis was a master axis when there existed a  flexible synchronization control group for which a non-PMC,  normal axis was a master axis.  

- The master and slave axes as synchronous axes overlap the  EGB axis.  

- The master and slave axes as synchronous axes overlap the  chopping axis.  

- The master and slave axes as synchronous axes overlap the  axis related to angular axis control.  

- The master and slave axes as synchronous axes overlap the  axis related to composite control.  

- The master and slave axes as synchronous axes overlap the  axis related to superposition control.  

- The slave axis as a synchronous axis overlaps the axis related  to synchronization control.  

- The reference position return mode is turned on (was turned  on).

5255

G12.4/G13.4 FORMAT ERROR

The specified P, I, and K are incorrect or I is less than K.

5257

G41/G42 NOT ALLOWED IN MDI  MODE

Tool radius/tool nose radius compensation was specified in MDI  mode. (Depending on the setting of the parameter MCR (No.  5008#4))

5303

TOUCH PANEL ERROR

The touch panel is not connected correctly, or the touch panel  cannot be initialized when the power is turned on. Correct the  cause then turn on the power again.

5305

ILLEGAL SPINDLE NUMBER

In a spindle select function by address P for a multiple spindle  control,  

1) Address P is not specified.  

2) Parameter No.3781 is not specified to the spindle to be  selected.  

3) An illegal G code which cannot be commanded with an  S_P_; command is specified.  

4) A multi spindle cannot be used because the parameter EMS  (No. 3702#1) is 1.  

5) The spindle amplifier number of each spindle is not set in  parameter No. 3717.  

6) A prohibited command for a spindle was issued (parameter  No. 11090).  

7) An invalid value is set in parameter No. 11090.

5312

ILLEGAL COMMAND IN G10  

L75/76/77

One of formats in G10L75, G10L76, or G10L77 to G11  commands is in error, or the command value is out of data  range. Modify the program.

5316

TOOL TYPE NUMBER NOT FOUND

A tool with the specified tool-type number could not be found.  Modify the program or register the tool.

5317

ALL TOOL LIFE IS OVER

The lives of all tools with the specified tool-type number have  expired.  

Replace the tool.

5320

DIA./RAD. MODE CAN’T BE  

SWITCHED .

In any of the following states, diameter/radius specification was  switched:  

1) When a buffered program is being executed  

2) When a movement is being made on the axis

Alarm

Message

Description

5329

M98 AND NC COMMAND IN SAME  BLOCK

A subprogram call which is not a single block was commanded  during canned cycle mode.

5339

ILLEGAL FORMAT COMMAND IS  EXECUTED IN SYNC/MIX/OVL  CONTROL.

1. The value of P, Q, or L specified by  

G51.4/G50.4/G51.5/G50.5/G51.6/G50.6 is invalid.  2. A duplicate value is specified by parameter No. 12600.

5346

RETURN TO REFERENCE POINT

The coordinate establishment of the Cs contour control axis is  not made.  

Perform a manual reference position return.  

1. When Cs coordinate establishment is made for the Cs-axis  for which the Cs-axis reference position status signal  CSPENx is 0  

2. When positional information is not sent from the spindle  amplifier  

3. When the servo off state is entered during the start of  Cs-axis coordinate establishment  

4. When the Cs-axis is subjected to synchronous control or  superposition control  

5. When the emergency stop state is entered during coordinate  establishment  

6. When an attempt is made to release composite control for  the Cs axis being subjected to coordinate establishment  7. When an attempt is made to start synchronous, composite,  or superposition control for the Cs axis being subjected to  coordinate establishment.

5360

TOOL INTERFERENCE CHECK  ERROR

This alarm is issued when interference with another tool is  caused by a data modification based on G10 data input or file  reading or when an attempt is made to modify the tool figure  data of a tool registered in the cartridge.

5361

ILLEGAL MAGAZINE DATA

Tools stored in the cartridge are interfering with each other.  Reregister the tools in the cartridge, or modify the tool  management data or tool figure data. If this alarm is issued, no  tool interference check is made when tools are registered in the  cartridge management table. Moreover, empty pot search  operation does not operate normally. If this alarm is issued, the  power must be turned off before operation is continued.

5362

CONVERT INCH/MM AT REF-POS

An inch/metric conversion was performed at a position other  than the reference position. Perform an inch/metric conversion  after returning to the reference position.

Alarm

Message

Description

5364

ILLEGAL COMMAND IN PROGRAM  CHECK

(1) An unspecifiable G code was specified in the high speed  program check mode.  

(2) The angular axis control option or customer's board option is  enabled.  

(3) One of the following operations was performed.  - Chopping in the high speed program check mode  - Starting the high speed program check mode during  chopping  

- High speed cycle machining in the high speed program  check mode  

- Reference position return of an axis for which the reference  position is not established, in the high speed program  check mode  

(4) Switching of PMC axis selection signal EAX*<G0136> was  performed.  

(5) G10 was specified for bit 3 (PGR) of parameter No. 3454 in  the high speed program check mode.  

(6) G10 was specified for bit 6 (PGS) of parameter No. 3001 in  the high speed program check mode.

5365

NOT CHANGE OF PROGRAM  CHECK MODE

(1) Switching of high speed program check input signal  PGCK<Gn290.5> was performed during execution of the  program.

5381

INVALID COMMAND IN FSC MODE

An attempt was made to issue the following commands:  - When the reference position for the master axis under flexible  synchronization control has not been established, G28  command for the master axis.  

- G27/G28/G29/G30/G30.1/G53 command for a slave axis.

5391

CAN NOT USE G92

Workpiece coordinate system setting G92 (or G50 for the lathe  system G-code system A) cannot be specified.  

(1) After tool length compensation was changed by tool length  compensation shift type, G92 was specified when no  absolute command is present.  

(2) G92 was specified in the block in which G49 is present.

5406

G41.3/G40 FORMAT ERROR

(1) The G41.3 or G40 block contains a move command.  (2) The G41.3 block contains a G or M code that suppresses  buffering.

5407

ILLEGAL COMMAND IN G41.3

(1) In the G41.3 mode, a G code of group 01 other than G00  and G01 is specified.  

(2) In the G41.3 mode, an offset command (a G code of group  07) is specified.  

(3) The block next to G41.3 (startup) specifies no movement.

5408

G41.3 ILLEGAL START_UP

(1) In a mode of group 01 other than G00 and G01, G41.3  (startup) is specified.  

(2) The included angle between the tool vector and move vector  is 0 or 180 degrees at the time of startup.

5420

ILLEGAL PARAMETER IN  

G43.4/G43.5

A parameter related to tool center point control is illegal.  - Acceleration/deceleration before interpolation is disabled. Set  parameter No. 1660.  

- Rapid traverse acceleration/deceleration before interpolation is  disabled. Set bit 1 of parameter No. 1401, bit 5 of parameter  No. 19501, parameter No. 1671, and parameter No. 1672.

Alarm 

Message

Description

5421

ILLEGAL COMMAND IN G43.4/G43.5

An illegal command was specified in tool center point control.  - A rotation axis command was specified in tool center point  control (type 2) mode.  

- With a table rotary type or mixed-type machine, a I,J,K  command was specified in the tool center point control (type 2)  command (G43.5) block.  

- A command that does not move the tool center point (only a  rotation axis is moved) was specified for the workpiece in the  G02 mode.  

- When the workpiece coordinate system is set as the  programming coordinate system (bit 5 (WKP) of parameter No.  19696 is 1), G02 or G03 was specified while the rotation axis  was not perpendicular to the plane.  

- A G code not specifiable during the tool center point control  mode was specified.  

- The modal code used to specify tool center point control is  incorrect.  

- During the tool center point control mode, an axis not related  to tool center point control was specified.  

- When bit 0 (RCM) of parameter No. 11200 is set to 0 to  disable tool direction compensation, tool center point control is  specified during the workpiece setting error  

compensation/tilted working plane command mode.  - When tool posture control is enabled under tool center point  control (type 2), a command is specified to set a tool posture  near a singular point. (This alarm may be suppressed with bit  3 (NPC) of parameter No. 19696.) Check the machine  configuration and specification.  

- When tool posture control is enabled under tool center point  control (type 1), a rotary axis angular displacement that  disables tool posture control is specified. Check the machine  configuration and specification.  

- During tool center point control (type 2) or tool posture control,  NURBS interpolation is specified. Check the specification.

5422

EXCESS VELOCITY IN G43.4/G43.5

An attempt was made to make a movement at an axis feedrate  exceeding the maximum cutting feedrate by tool center point  control.

5424

ILLEGAL TOOL DIRECTION

The rotation axis position for specifying the tool axis direction is  not ±90° × n (n = 0, 1, 2,･･･).

5425

ILLEGAL OFFSET VALUE

The offset number is incorrect.

5430

ILLEGAL COMMAND IN 3-D CIR

In a modal state in which three-dimensional circular interpolation  cannot be specified, a three-dimensional circular interpolation  (G02.4/G03.4) is specified. Alternatively, in three-dimensional  circular interpolation mode, a code that cannot be specified is  specified.

5432

G02.4/G03.4 FORMAT ERROR

A three-dimensional circular interpolation command  (G02.4/G03.4) is incorrect.

5433

MANUAL INTERVENTION IN  

G02.4/G03.4 (ABS ON)

In three-dimensional circular interpolation mode (G02.4/G03.4),  manual intervention was made when the manual absolute switch  was on.

5435

PARAMETER OUT OF RANGE (TLAC)

Illegal parameter setting.  

(Set value is out of range.)  

Check parameters No. 19655, No. 19656, No. 19657, and No.  1022.

Alarm

Message

Description

5436

ILLEGAL PARAMETER SETTING OF  ROTARY AXIS(TLAC)

Illegal parameter setting.  

(axis of rotation setting)

5437

ILLEGAL PARAMETER SETTING OF  MASTER ROTARY AXIS(TLAC)

Illegal parameter setting.  

(master axis of rotation setting)

5445

CAN NOT COMMAND MOTION IN  G39

Corner circular interpolation (G39) of tool radius/tool nose radius  compensation is not specified alone but is specified with a move  command.

5446

NO AVOIDANCE AT G41/G42

Because there is no interference avoidance vector, the  interference check avoidance function of tool radius/tool nose  radius compensation does not work.

5447

DANGEROUS AVOIDANCE AT  G41/G42

The interference check avoidance function of tool radius/tool  nose radius compensation operation will lead to danger.

5448

INTERFERENCE TO AVD. AT  

G41/G42

In the interference check avoidance function of tool radius/tool  nose radius compensation, a further interference occurs for an  already created interference avoidance vector.

5456

TOO MANY G68.2 NESTING

Tilted working plane command G68.2 was specified more than  once.  

To perform another coordinate conversion, perform cancellation,  then specify the coordinate conversion.

5457

G68.2 FORMAT ERROR

A G68.2 format error occurred.

5458

ILLEGAL USE OF G53.1

- G53.1 was specified preceding G68.2.  

- G53.1 needs to be specified solely.  

- There is no angle solution for the rotation axis that controls the  tool direction in the +Z-axis direction of the feature coordinate  system.  

- In the setting by which compensation in the tool direction is not  performed (when bit 0 (RCM) of parameter No. 11200 is 0),  G53.1 was specified in the workpiece placement error  compensation mode.

5459

MACHINE PARAMETER INCORRECT

 - The parameter No. 19665 to No. 19667, No. 19680 to No.  19744 for configuring the machine are incorrect.  

- The axis specified with parameter No. 19681 or No. 19686 is  not a rotary axis.  

- In parameter No. 1022, the basic three axes are not set.  - A rotary axis end point found by the NC with tool center point  control type 2, 3-dimensional cutter compensation type 2, or  the tilted working plane command is not within the range set by  parameter No. 19741 to No. 19744.  

- No rotary axis end point was found with tool center point  control type 2 or 3-dimensional cutter compensation type 2.  Check the machine configuration and specification.  

- On a machine whose rotary axis is a virtual axis, tool center  point control type 2 or 3-dimensional cutter compensation type  2 was specified.  

- When programming is performed in the workpiece coordinate  system, tool center point control type 2 or 3-dimensional cutter  compensation type 2 is specified.

Alarm 

Message

Description

5460

ILLEGAL USE OF 3-DIMENSIONAL  CUTTER COMPENSATION

- In the 3-dimensional cutter compensation mode (except the  tool side offset function for a tool rotation type machine), a  move command other than G00/G01 is specified.  

- With a table rotation type machine, when bit 1 (PTD) of  parameter No. 19746 is set to 1, a plane selection is made  with an axis other than the basic three axes at the start of  3-dimensional cutter compensation.  

- When bit 1 (SPG) of parameter No. 19607 is set to 1, there is  a discrepancy between the machine type set in parameter No.  19680 and a G code specifying 3-dimensional cutter  compensation (G41.2, G42.2, G41.4, G42.4, G41.5, or G42.5).

- With a machine that is not of the tool rotation type, G41.3 is  specified.  

- When bit 5 (WKP) of parameter No. 19696 is set to 0, and bit 4  (TBP) of parameter No. 19746 is set to 0, 3-dimensional cutter  compensation and tool center point control are used at the  same time.  

- A rotation axis command is specified in the 3-dimensional  cutter compensation mode (type 2).  

- With a table rotation type or mixed type machine, IJK is  specified in a block that specifies 3-dimensional cutter  compensation (type 2) (G41.6/G42.6).  

- An illegal G code is specified in the 3-dimensional cutter  compensation mode.  

- When 3-dimensional cutter compensation is specified, the  modal state is illegal.  

- When the table coordinate system is set as the programming  coordinate system, table rotate and 3-dimensional cutter  compensation are specified after the start of tool center point  control.  

- There is a difference in type1/type 2 specification between  3-dimensional cutter compensation and tool center point  control.  

- When 3-dimensional cutter compensation and tool center point  control are used at the same time, one of these functions that  is specified earlier than the other is canceled earlier.

5461

ILLEGAL USE OF  

G41.2/G42.2/G41.5/G42.5

A move command other than G00 or G01 was performed during  3-dimensional cutter compensation in a mixed-type machine.

5462

ILLEGAL COMMAND (G68.2/G69)

(1) The modal setting used when G68.2 or G69 is specified is  incorrect.  

(2) An unspecifiable G code was specified in the G68.2 mode.  (3) The offset vector of tool radius/tool nose radius  compensation is not canceled when G68.2 or G69 is  specified.

5463

ILLEGAL PARAMETER IN  

3-DIMENSIONAL CUTTER  

COMPENSATION

A parameter related to 3-dimensional cutter compensation is  illegal.  

- Acceleration/deceleration before interpolation is disabled. Set  parameter No. 1660.  

- Rapid traverse acceleration/deceleration before interpolation is  disabled. Set bit 1 (LRP) of parameter No. 1401, bit 5 (FRP) of  parameter No. 19501, and parameter Nos. No.1671 and 1672.

Alarm 

Message

Description

SW0100

PARAMETER ENABLE SWITCH ON

The parameter setting is enabled (PWE, one bit of parameter  No. 8000 is set to “1”).  

To set the parameter, turn this parameter ON. Otherwise, set  to OFF.

Alarm 

Message

Description

SV0001

SYNC ALIGNMENT ERROR

In feed axis synchronization control, the amount of  compensation for synchronization exceeded the parameter  (No. 8325) setting value.  

This alarm occurs only for a slave axis.

SV0002

SYNC EXCESS ERROR ALARM 2

In feed axis synchronization control, the amount of  synchronization error exceeded the parameter (No. 8332)  setting value. When the synchronization is not completed  after power-up, the determination is made by the parameter  value (No. 8332) multiplied by the parameter (No. 8330)  multiplier.  

This alarm occurs only for a slave axis only.

SV0003

SYNCHRONOUS/COMPOSITE/SUPERI MPOSED CONTROL MODE CAN'T BE  CONTINUED

Since as axis in synchronization, composition, or  superposition mode caused a servo alarm, the mode could  not be continued, If one of the axes in a mode causes a  servo alarm, all axes relating to the axis enter the servo-off  state. This alarm is generated to enable the cause of the  servo-off state to be checked.

SV0004

EXCESS ERROR (G31)

The amount of positional deviation during torque limit skip  command operation exceeded the limit value of the  parameter No.6287.

SV0005

SYNC EXCESS ERROR (MCN)

In feed axis synchronization control, for synchronization, the  difference value of the machine coordinate between a master  and slave axes exceeded the parameter (No. 8314) setting  value.  

This alarm occurs for a master or slave axis.

SV0006

ILLEGAL TANDEM AXIS

For the slave axis under tandem control, absolute position  detection is set (parameter bit 5 (APC) of parameter No.  1815 = 1).

SV0007

SV ALM ANOTHER PATH(MULTI AMP.)

When a multiaxis amplifier was used in a multipath system  across paths, a servo alarm occurred on an axis belonging to  another path.  

When a system with two or more paths and multiple servo  axes between paths are controlled by a multiaxis amplifier, if  a servo alarm occurs on an axis belonging to another path of  the same amplifier, the MCC of the amplifier goes down and  SV0401 V-READY OFF occurs on an axis belonging to the  local path in the same amplifier. Since SV0401 is caused  by a servo alarm occurred on an axis in another path,  SV0007 is caused together to clearly indicate the fact.  The axis belonging to another path in the same amplifier  resolves the cause of the servo alarm.

Alarm 

Message

Description

SV0301

APC ALARM: COMMUNICATION  ERROR

Since the absolute-position detector caused a  

communication error, the correct machine position could not  be obtained. (data transfer error)  

The absolute-position detector, cable, or servo interface  module is thought to be defective.

SV0302

APC ALARM: OVER TIME ERROR

Since the absolute-position detector caused an overtime  error, the correct machine position could not be obtained.  (data transfer error)  

The absolute-position detector, cable, or servo interface  module is thought to be defective.

SV0303

APC ALARM: FRAMING ERROR

Since the absolute-position detector caused a framing error,  the correct machine position could not be obtained. (data  transfer error)  

The absolute-position detector, cable, or servo interface  module is thought to be defective.

SV0304

APC ALARM: PARITY ERROR

Since the absolute-position detector caused a parity error,  the correct machine position could not be obtained. (data  transfer error)  

The absolute-position detector, cable, or servo interface  module is thought to be defective.

SV0305

APC ALARM: PULSE ERROR

Since the absolute-position detector caused a pulse error,  the correct machine position could not be obtained.  The absolute-position detector, or cable is thought to be  defective.

SV0306

APC ALARM: OVER FLOW ERROR

Since the amount of positional deviation overflowed, the  correct machine position could not be obtained.  Check to see the parameter No. 2084 or No. 2085.

SV0307

APC ALARM: MOVEMENT EXCESS  ERROR

Since the machine moved excessively, the correct machine  position could not be obtained.

SV0360

ABNORMAL CHECKSUM(INT)

The checksum alarm occurred on the built–in Pulsecoder.

SV0361

ABNORMAL PHASE DATA(INT)

The phase data abnormal alarm occurred on the built–in  Pulsecoder.

SV0362

ABNORMAL REV. DATA(INT)

The speed count abnormal alarm occurred on the built-in  Pulsecoder.

SV0363

ABNORMAL CLOCK(INT)

The clock alarm occurred on the built–in Pulsecoder.

SV0364

SOFT PHASE ALARM(INT)

A digital servo soft detected an abnormality on the built in  Pulsecoder.

SV0365

BROKEN LED(INT)

The digital servo software detected abnormal data on the  built–in Pulsecoder.

SV0366

PULSE MISS(INT)

A pulse error occurred on the built–in Pulsecoder.

SV0367

COUNT MISS(INT)

A count error occurred on the built–in Pulsecoder.

SV0368

SERIAL DATA ERROR(INT)

The communications data could not be received from the  built–in Pulsecoder.

SV0369

DATA TRANS. ERROR(INT)

A CRC error or stop bit error occurred in the communications  data from the built–in Pulsecoder.

SV0380

BROKEN LED(EXT)

Separate detector error

SV0381

ABNORMAL PHASE (EXT)

An abnormal alarm in the position data occurred on the  separate detector.

SV0382

COUNT MISS(EXT)

A count error occurred on the separate detector.

SV0383

PULSE MISS(EXT)

A pulse error occurred on the separate detector.

SV0384

SOFT PHASE ALARM(EXT)

The digital servo software detected abnormal data on the  separate detector.

Alarm

Message

Description

SV0385

SERIAL DATA ERROR(EXT)

The communications data could not be received from the  separate detector.

SV0386

DATA TRANS. ERROR(EXT)

A CRC error or stop bit error occurred in the communications  data from the standalone detector.

SV0387

ABNORMAL ENCODER(EXT)

An abnormality occurred on a separate detector. For more  information, contact the scale manufacturer.

SV0401

IMPROPER V_READY OFF

Although the ready signal (PRDY) of the position control was  ON, the ready signal (VRDY) of the velocity control was OFF.

SV0403

CARD/SOFT MISMATCH

The combination of the axis control card and the servo  software is incorrect.  

Probable causes are given below.  

- The correct axis control card is not attached.  

- The correct servo software is not installed in flash memory.

SV0404

IMPROPER V_READY ON

Although the ready signal (PRDY) of the position control was  OFF, the ready signal (VRDY) of the velocity control was ON.

SV0407

EXCESS ERROR

The difference value of the amount of positional deviation for  the synchronization axis exceeded the setting value. (during  synchronization control only)

SV0409

DETECT ABNORMAL TORQUE

An abnormal load was detected on the servo motor, or during  Cs axis or spindle positioning.  

The alarm can be canceled by RESET.

SV0410

EXCESS ERROR (STOP)

The amount of positional deviation during stopping exceeded  the parameter (No. 1829) setting value.

SV0411

EXCESS ERROR (MOVING)

The amount of positional deviation during traveling became  excessive than the parameter setting value.

SV0413

LSI OVERFLOW

The counter for the amount of positional deviation overflowed

SV0415

MOTION VALUE OVERFLOW

The velocity exceeding the travel velocity limit was  commanded.

SV0417

ILL DGTL SERVO PARAMETER

A digital serve parameter setting is incorrect.  

When bit 4 of diagnosis information No. 203 is 1, an illegal  parameter was detected by the servo software. Identify the  cause with reference to diagnosis information No. 352.  

When bit 4 of diagnosis information No. 203 is 0, the CNC  software detected an illegal parameter. Probable causes  are given below (see diagnosis information No. 280).  1) The value specified in parameter No. 2020 as the motor  model falls outside the specified range.  

2) The motor rotation direction in parameter No. 2022 is not  set to a correct value (111 or -111).  

3) The speed feedback pulse count per motor rotation in  parameter No. 2023 is set to a negative or other incorrect  value.  

4) The position feedback pulse count per motor rotation in  parameter No. 2024 is set to a negative or other incorrect  value.

SV0420

SYNC TORQUE EXCESS

In feed axis synchronization control, for synchronization, the  difference value of torque between a master and slave axes  exceeded the parameter (No. 2031) setting value.  This alarm occurs for a master axis.

SV0421

EXCESS ERROR(SEMI-FULL)

The difference between the feedback from the semi and full  sides exceeded the setting of parameter No.1729.

Alarm 

Message

Description

SV0422

EXCESS VELOCITY IN TORQUE

In torque control, the commanded permissible velocity was  exceeded.

SV0423

EXCESS ERROR IN TORQUE

In torque control, the total permissible move value specified  as a parameter was exceeded.

SV0430

SV MOTOR OVERHEAT

The servo motor has overheated.

SV0431

CNV. OVERLOAD

PSM : Overheat  

β series SVU : Overheat

SV0432

CNV. LOW VOLT CONTROL

PSM : The control power supply voltage has dropped.  PSMR : The control power supply voltage has dropped.  β series SVU : The control power supply voltage has  dropped.

SV0433

CNV. LOW VOLT DC LINK

PSM : Low DC link voltage  

PSMR : Low DC link voltage  

α series SVU : Low DC link voltage  

β series SVU : Low DC link voltage

SV0434

INV. LOW VOLT CONTROL

SVM : Low control power voltage

SV0435

INV. LOW VOLT DC LINK

SVM : Low DC link voltage

SV0436

SOFTTHERMAL(OVC)

The digital servo software detected a software thermal  (OVC).

SV0437

CNV. OVERCURRENT POWER

PSM : Overcurrent on input circuit section.

SV0438

INV. ABNORMAL CURRENT

SVM : Motor overcurrent  

α series SVU : Motor overcurrent  

β series SVU : Motor overcurrent

SV0439

CNV. OVER VOLT DC LINK

PSM : The DC link voltage is too high.  

PSMR : The DC link voltage is too high.  

β series SVU : The DC link voltage is too high.

SV0440

CNV. EX DECELERATION POW.

PSMR : Excessive generative discharge  

α series SVU : Excessive generative discharge, or abnormal  error in generative power circuit

SV0441

ABNORMAL CURRENT OFFSET

The digital servo software detected an abnormality in the  motor current detection circuit.

SV0442

CNV. CHARGE FAILURE

PSM : The spare charge circuit for the DC link is abnormal.  PSMR : The spare charge circuit for the DC link is abnormal.

SV0443

CNV. COOLING FAN FAILURE

PSM : Internal cooling fan failure.  

PSMR : Internal cooling fan failure.  

β series SVU : Internal cooling fan failure.

SV0444

INV. COOLING FAN FAILURE

SVM : Internal cooling fan failure.

SV0445

SOFT DISCONNECT ALARM

The digital servo software detected a disconnected  Pulsecoder.

SV0446

HARD DISCONNECT ALARM

The hardware detected a disconnected built–in Pulsecoder.

SV0447

HARD DISCONNECT(EXT)

The hardware detected a disconnected separate detector.

SV0448

UNMATCHED FEEDBACK ALARM

The sign of the feedback signal from the standalone detector  is opposite to that from the feedback signal from the built–on  Pulsecoder.

SV0449

INV. IPM ALARM

SVM : The IPM (Intelligent Power Module) detected an alarm. α series SVU : The IPM (Intelligent Power Module) detected  an alarm.

SV0453

SPC SOFT DISCONNECT ALARM

Software disconnection alarm of the α Pulsecoder.  Turn off the power to the CNC, then remove and insert the  Pulsecoder cable. If this alarm is issued again, replace the  Pulsecoder.

Alarm 

Message

Description

SV0454

ILLEGAL ROTOR POS DETECT

The magnetic pole detection function terminated abnormally. The magnetic pole could not be detected because the motor  did not run.

SV0456

ILLEGAL CURRENT LOOP

An attempt was made to set the current loop that could not  be set.  

The amplifier pulse module in use does not comply with  HIGH SPEED HRV. Or, requirements to control are not  satisfied in the system.

SV0458

CURRENT LOOP ERROR

The specified current loop differs from the actual current  loop.

SV0459

HI HRV SETTING ERROR

For two axes whose servo axis numbers (parameter No.  1023) are consecutively even and odd numbers, HIGH  SPEED HRV control is possible for one axis and impossible  for the other.

SV0460

FSSB DISCONNECT

The FSSB connection was discontinued.  

Probable causes are:  

1. The FSSB connection cable was disconnected or broken.  2. The amplifier was turned off .  

3. In the amplifier, the low-voltage alarm occurred.

SV0462

SEND CNC DATA FAILED

The correct data could not be received on a slave side  because of the FSSB communication error.

SV0463

SEND SLAVE DATA FAILED

The correct data could not be received in the servo software  because of the FSSB communication error.

SV0465

READ ID DATA FAILED

A read of the ID information for the amplifier has failed at  power-on.

SV0466

MOTOR/AMP. COMBINATION

The maximum current of an amplifier is different to that of a  motor.  

Probable causes are:  

1. The connection command for an amplifier is incorrect.  2. The parameter (No.2165) setting is incorrect

SV0468

HI HRV SETTING ERROR(AMP)

An attempt was made to set up HIGH SPEED HRV control  for use when the controlled axis of an amplifier for which  HIGH SPEED HRV control could not be used.

SV0474

EXCESS ERROR(STOP:SV )

The servo detected that the positional deviation during a stop  exceeded the setting (parameters No. 1839 and No. 1842) in  the n-axis.

SV0475

EXCESS ERROR(MOVE:SV)

The servo detected that the positional deviation during a  travel exceeded the setting (parameters No. 1838 and No.  1841) in the n-axis.

SV0476

ILLEGAL SPEED CMD.(SV )

The servo detected that the speed command exceeded the  safety speed (parameters No. 13821 to No. 13824 (during  position control) or parameters No. 13826 to No. 13829  (during speed control)) during safety monitoring (when safety  monitoring request signal *VLDVx is 0) in the n-axis. Keep  the safety speed.

SV0477

ILLEGAL MACHINE POS.(SV)

The servo detected that the machine position fell outside the  safety area (setting by parameters No. 13831 to No. 13838)  during safety monitoring (when safety monitoring request  signal *VLDVx is 0) in the n-axis. Keep the safety area.  A machine position check is performed only on the axis for  which the reference position has been established. The  axis for which the reference position is not established is not  subjected to a machine position check.

Alarm

Message

Description

SV0478

ILLEGAL AXIS DATA(SV)

The servo detected that an error occurred during transfer of  axis data in the n-axis.  

When an alarm occurred because the configuration of the  servo amplifier was changed, set the axis number for the  servo amplifier (set bit 4 of parameter No. 2212 of the  corresponding axis to 1 and then 0 and turn off the power of  the entire system). When using a multiaxis amplifier, this  operation may not clear the alarm. In this case, repeat this  operation for the axes on which the alarm persists.  If an alarm occurs due to a cause other than the above,  replace the servo amplifier.

SV0481

SAFETY PARAM ERROR(SV)

The servo detected that a safety parameter error occurred in  the n-axis.

SV0484

SAFETY FUNCTION ERROR(SV)

A safety function error related to the servo was detected in  the n-axis.  

- The servo or CNC detected that the safety function was not  executed in the servo.  

- The result of a servo safety function check did not match  the result of a CNC safety function check.  

- An error occurred during a test of the CPU of the servo.  - An error occurred during a check of RAM of the servo.

SV0488

SELF TEST OVER TIME

An MCC interruption test was not complete within the set  period of time (parameter No. 1946). Check the MCC  contact.

SV0489

SAFETY PARAM ERROR(CNC)

The CNC detected that a safety parameter error occurred in  the n-axis.

SV0490

SAFETY FUNCTION ERROR(CNC)

A CNC safety function error occurred in the n-axis.  - The servo detected that the safety function was not  executed in the CNC.  

- The result of a servo safety function check did not match  the result of a CNC safety function check.

SV0494

ILLEGAL SPEED CMD.(CNC)

The CNC detected that the speed command exceeded the  safety speed (parameters No. 13821 to No. 13824 (during  position control) or parameters No. 13826 to No. 13829  (during speed control)) during safety monitoring (when safety  monitoring request signal *VLDVx is 0) in the n-axis. Keep  the safety speed.

SV0495

ILLEGAL MACHINE POS.(CNC)

The CNC detected that the machine position fell outside the  safety area (set range by parameters No. 13831 to No.  13838) during safety monitoring (when safety monitoring  request signal *VLDVx is 0) in the n-axis. Keep the safety  area.  

A machine position check is performed only on the axis for  which the reference position has been established.

Alarm 

Message

Description

SV0496

ILLEGAL AXIS DATA(CNC)

The CNC detected that an error occurred during transfer to  axis data.  

When an alarm occurred because the configuration of the  servo amplifier was changed, set the axis number for the  servo amplifier (set bit 4 of parameter No. 2212 of the  corresponding axis to 1 and 0 again and turn off the power of  the entire system). When using a multiaxis amplifier, this  operation may not clear the alarm. In this case, repeat this  operation for the axes on which the alarm persists.  If an alarm occurs due to a cause other than the above,  replace the servo amplifier.

SV0498

AXIS NUMBER NOT SET(CNC)

The CNC detected that the axis number of the n-axis was not  set for the servo amplifier. The axis number is set  automatically, so turn off the power of the entire system.

SV0600

INV. DC LINK OVER CURRENT

SVM : DC link overcurrent.  

β SVU : DC link overcurrent.

SV0601

INV. RADIATOR FAN FAILURE

SVM : Radiator cooling fan failure.  

β SVU : Radiator cooling fan failure.

SV0602

INV. OVERHEAT

SVM : The servo motor has overheated.

SV0603

INV. IPM ALARM(OH)

SVM : The IPM (Intelligent Power Module) detected an  overheat alarm.  

β SVU : The IPM (Intelligent Power Module) detected an  overheat alarm.

SV0604

AMP. COMMUNICATION ERROR

The communication between SVM and PSM is in error.

SV0605

CNV. EX. DISCHARGE POW.

PSMR : The motor regenerative power is too much.

SV0606