OSP-U10L Chapter 5 Alarm B-2

SECTION 5 ALARM B

2213 Program parameter excess
Eeoelale4059
The buffer register for storing program parameters is full.
Too many commands are designated in one block.
Or, an error occurred during GET and PUT command processing. For program parameters, refer to the parameter classification code table.
[Object]
System
[Code]
1-> More than 127 factor classification codes or factor parameters are designated.
2-> More than 64 factor numerical values are designated.
3-> Factor classification code or/and factor parameter stack shift range error. (This alarm does not normally occur)
4-> Factor numerical value stack shift range error. (This alarm does not normally occur)
[Probable Fault Cause]
[Code] 1, 2-> Warning sequence occurred
[Code] 3, 4-> Control software error
Program example:
N010 ABC=1 BCD=2 …
BCD=1
The expression has three factor classification codes and factor parameters.
In this manner, if the total number of factor classification codes and factor parameters exceeds 127, code 1 alarm occurs.
In this manner, if the total number of factor numerical values exceeds 64, code 2 alarm occurs.
[Measures to Take]
If code 1 or code 2 alarm occurs, too many commands are designated in one block; designate commands in two or more blocks. If code 3 or code 4 occurs, contact an
OKUMA software center.
2214 Suffix command
Eeoelale4060
The suffix expression is incorrect.
The data value of the system variable suffix expression is too large or too small.
Tool length and tool nose radius compensation
1 to 32 (1 to 64 for 64-pair specifications)
Tool interference
1 to 12
Two suffixes are designated in the system variable or I/O variable.
Suffix expression: [*] in V***[*] as a variable
[Object]
System
[Code]
2-> Two suffix expressions are used in an I/O variable
None-> Two suffix expressions are used in a system variable
Others-> Hexadecimal value of the programmed suffix expression
[Probable Fault Cause]
Suffix expression
Program example:
VTOFX[34]=10 ->[Code] 22 (hexadecimal number of 34)
^^ Designate 1 to 32.
VNSRZ[-1]=5 ->[Code] FFFFFFFF (hexadecimal number of -1)
^^ Designate 1 to 32
V1=VDIN[1, 2] ->[Code] 2
^^^ Two suffixes cannot be designated
VDOUT[1, 2]=20 -> No code
^^^ Two suffixes cannot be designated
2215 Local variable excess
Eeoelale4061
The number of local variables exceeds 127.
Local variable: User-specified variable name that can be used only within a task program
[Object]
System
LC37-003 P-182
SECTION 5 ALARM B
[Code]
1
[Measures to Take]
Reduce the number of local variables used.
2216 System variable setting value error
Eeoelale4062
The setting value for the system variable is outside the permissible range.
Permissible setting range (example)
Chamfering amount
0 to 1.000
Tool nose radius compensation
-999.999 to 999.999
Tool length compensation
-99999.999 to 99999.999
Positive variable limit ≤ Positive stroke end limit
Negative variable limit ≥ Negative stroke end limit
Positive (negative) stroke end limit is set in the system parameters.
[Object]
System
[Code]
Hexadecimal number of the set value
[Probable Fault Cause]
System variable
Operation example:
In parameter setting mode, in-position zone was set to 2 in user parameters.
[Measures to Take]
Set the system variable within the permissible range.
2217 Output variable setting value error
Eeoelale4063 The output variable setting is incorrect.
[Object]
System
[Code]
Hexadecimal number of the erroneous value
2-FF-> Not specified in 1 bit
100-> Not specified in 1 byte
[Probable Fault Cause]
Program error
Program example:
:
VDOUT[1]=2
VDOUT[9]=256
:
[Measures to Take]
 Check the VDOUT command.
 The output variable setting must be within the range specified for each variable.
 Because VDOUT[1] is a 1-bit value, set the data to 0 or 1.
 Because VDOUT[9] is a byte value, set the data to 0 to 255.
[Related Specifications]
User task 2
2218 G-code not available
Eeoelale4064 A G-code not available in the selected specification is designated.
[Object]
System
LC37-003 P-183
SECTION 5 ALARM B
[Code]
Hexadecimal number of designated G-code
[Probable Fault Cause]
G-code
If code 8C (hexadecimal for 140) occurs, G140 was designated.
If code A (hexadecimal for 10) occurs, G10 was designated.
[Measures to Take]
Designate a G-code available in the specification.
2219 M-code not available
Eeoelale4065 An M-code not available in the selected specification is designated.
[Object]
System
[Code]
Hexadecimal number of designated M-code
[Probable Fault Cause]
 M-code
 If code A (hexadecimal for 10) occurs, M10 was designated.
 If code 3C (hexadecimal for 60) occurs, M60 was designated.
[Measures to Take]
Designate an M-code available in the specification.
2220 Left side command not available
Eeoelale4066
Illegal command on the left side of the expression
Schedule program-> In the VSET block, the command designated on the left side is neither a common variable nor an output variable.
Main program, subprogram-> The command designated on the left side is not G or M address character, extended address character, local variable, common variable, system variable, or output variable.
Address character: One-character variable expression defined by NC, such as G, M, N, O, and V
Extended address character: Two-character variable expression defined by NC
Local variable: Variable named and used by user
<2 alphabetic characters><2 numeric characters>
Common variable: Variable used commonly in main programs and subprograms
System variable: System-defined variable that cannot be renamed by the user
Output variable: Variable valid for signal output to external devices <VDOUT>[variable number]
[Object]
System (None for schedule program)
[Code]
XXYY: Factor classification code or parameter designated on the left side
XX: Factor classification code
YY: Factor parameter
[Probable Fault Cause]
Command designated on the left side
Program example:
VDIN[35]=5 Input variable and data value are designated on the left side
20=VTOFX[1]
[Measures to Take]
Do not designate commands that are not permitted.
2221 Output variable number not available
Eeoelale4067 An output variable not available in the selected specification is designated.
[Object]
System
[Code]
Hexadecimal number of output variable number
LC37-003 P-184
SECTION 5 ALARM B
Program example:
VDOUT[****]=10
**** <- Output variable number
[Measures to Take]
Designate an available output variable.
2222 Input variable number not available
Eeoelale4068 An input variable not available in the selected specification is designated.
[Object]
System
[Code]
Hexadecimal number of input variable number
[Probable Fault Cause]
Input variable number
Program example:
VDIN[**]=10
** <- Input variable number
[Measures to Take]
Designate an available input variable.
2223 Turret command code not available
Eeoelale4069 G13 and G14 commands are designated on a machine with only 1 turret.
[Object]
System
[Code]
Hexadecimal number of designated G-code
[Probable Fault Cause]
G13, G14
Program example:
N010 G13
N020 G00 X50
N030 G01 Z40
[Measures to Take]
Do not designate the G13 or G14 command on a machine without the turret selection function.
2224 Generating cutting command code not available
Eeoelale4070 G101, G102, or G103 generating cutting command is designated when the B-turret is used.
[Object]
System
[Code]
Hexadecimal number of designated G-code or none
[Probable Fault Cause]
Program error
Program example:
G14
G101 X176.00 C294.62 F100
:
[Measures to Take]
Check G101, G102, G103, G132, G133, and G14 commands.
:
G13
G101 X176.00 C294.62 F100
:
[Related Specifications]
Generating cutting
LC37-003 P-185
SECTION 5 ALARM B
2225 Y-Z circular interpolation command not available
Eeoelale4071 Circular interpolation command is designated in Y-axis mode where Y-Z circular interpolation is not provided.
[Object]
System
[Code]
Hexadecimal number of designated G-code
[Probable Fault Cause]
Program error
2226 Constant speed thread cutting command not available
Eeoelale4072
G31, G32, G33, G34, or G35 thread cutting command is designated while constant cutting speed control is ON.
(Thread cutting cannot be executed correctly when spindle speed varies with the X-axis command.)
[Object]
System
[Probable Fault Cause]
Program error
Program example:
N010 G96
N020 G31
:
[Measures to Take]
Modify the program (designate the thread cutting command after canceling the constant cutting speed command).
2227 Mnemonic or local variable
Eeoelale4073 Local variable name has more than 4 characters or a mnemonic is misspelled. A mnemonic is a character string registered in the control software and used to execute a fixed processing (such as CALL, GOTO, MODIN,
MODOUT). A misspelled mnemonic (if not exceeding 4 characters) will be treated as a local variable.
[Object]
System
[Cause]
Program command
Program example:
N100 MODNN — Spelling error
N200 ABCDE=1
^^^^^ Local variable contains 5 or more characters
[Remedy]
Check whether the program that caused the alarm contains a misspelled keyword or a local variable with more than 4 characters. If a keyword is misspelled, correct the spelling. If it is a local variable
problem, change its name to not more than 4 characters.
2228 VSET statement Left-side command
Eeoelale4074 In the schedule program, commands other than common variables and I/O variables cannot be used.
[Code]
Hexadecimal number of designated factor code
[Cause]
Program error
Program example:
VSET RR=RR+1
:
[Remedy]
Check the VSET command.
:
VSET V1=V1+1
:
LC37-003 P-186
SECTION 5 ALARM B
2229 Expression right side
Eeoelale4075
An unusable command is designated on the right side of the expression; only numbers, input variables, system variables, common variables, local variables, or extended address characters can be used.
Input variable: Effective variable in external device signal input <VDIN>[variable number]
System variable: System-defined variable that cannot be renamed by the user
Common variable: Variable shared between main program and subprograms <V><2-digit number>
Local variable: Variable named and used by the user
<2 alphabetic characters><2 numeric characters>
Extended address character: Two-character variable expression defined by NC
[Object]
System
[Code]
Designated factor classification code
[Cause]
Right side of expression
Program example:
VDOUT[31]=VDOUT[31]+1
^^^^ Output variable cannot be designated on the right side of an expression.
[Remedy]
Correct the right-side expression.
Example: VDOUT[31]=1
2230 Expression operation
Eeoelale4076 Expression operation error
[Object]
System
[Code]
XXYY
XX:
Bit 0-> Addition overflow
Bit 1-> Absolute value to integer conversion overflow
Bit 2-> BCD-to-BIN conversion error
Bit 3-> BIN-to-BCD conversion error
Bit 4-> DROUND, DFIX, or DFUP command is designated in a non-metric (inch) unit system.
YY: Floating-point calculation error
Bit 0-> Conversion to integer overflow
Bit 1-> Exponential underflow
Bit 2-> Exponential overflow
Bit 3-> Square root of negative number
Bit 4-> Division by zero
Bit 5-> Angle overflow
2231 Expression syntax
Eeoelale4077 Expression syntax error
[Object]
System
[Code]
1-> Subscript expression is nested in a subscript expression.
2-> Subscript expression lacks "[".
3-> 3 or more subscript expressions (4 or more subscript expressions in graphic system variables)
4-> "[" and "]" do not match.
5-> Operators and their elements do not match.
6-> Program terminated in the middle of expression.
7-> Answer is not unique.
Subscript: [*] used as a variable in V***[*]
[Cause]
Program number where the alarm occurred
LC37-003 P-187
SECTION 5 ALARM B
Program error
Program example:
[Code] 1->VTOFX[VMDT[1]]=4.5
[Code] 2->VTOFX[5]=4.5
[Code] 3->VTOFX[1, 2, 3]=4.5
In this case, alarm code 5 appears due to the relationship between the level and operator number.
[Code] 4->VTOFX[2]=4.5
[Code] 5->VTOFX[4]=4.5 (Code 5 is mainly displayed when an alarm occurs.)
[Code] 6-> Since an end code is always designated at the end of a command, this alarm code does not occur.
[Code] 7 VTOFX[1, 2]=4.5
[Remedy]
Correct the program according to the code at the time of the alarm.
2232 Expression subscript
Eeoelale4078
Right-side subscript expression error.
Note: When an error occurs in the right-side subscript expression, "ALARM B 2214 Subscript command" is displayed.
Subscript: [*] used as a variable in V***[*]
[Object]
System
[Code]
None-> More than one subscript expression.
Others-> Result of subscript expression exceeds the subscript range.
[Cause]
Subscript expression causing the alarm
Program example: V1=VTOFX[0] VTOFX subscript range is 1 to 32 (1 to 64 for 64-set tool offset specification).
V1=VTOFX[1, 2] Two subscripts are used.
[Remedy]
Correct the subscript expression so that the calculation result falls within the subscript expression range.
2233 Expression buffer overflow
Eeoelale4079 Too many expression terms to calculate.
[Object]
System
[Code]
1-> Operand stack overflow occurred when calculating subscript expressions and operation expressions (more than 16).
2-> Operator stack overflow occurred when calculating operation expressions (more than 8).
Program example:
V1=1+[1+[1+[1+[1+[1+[1+[1+[1+1]]]]]]]] ->[Code] 1
The number of operands to the left of the first right bracket is 18.
V1=1+[1+[1+[1+[1+[1+[1+[1+1]]]]]]]]] ->[Code] 2
Calculation is still impossible when reading the 9th number; data stack overflow.
Same as above
V1=1+2+3+4+5+6+7+8+9 ->[Code] 2
Although there are 9 numbers in total, sequential calculation cannot be performed from the leftmost side. Therefore, operand stack overflow does not occur.
[Remedy]
The NC stores operation data (up to 16) and operators (up to 8) starting from the left according to the priority level of operators.
Change the expression by moving higher-priority operations to the left of lower-priority operations.
2234 Expression local variable
Eeoelale4080 Designated local variable is not registered.
[Object]
System
[Character-string] Designated local variable name
Program example:
VTOFX[2] =BDIK
LC37-003 P-188
SECTION 5 ALARM B
^^^^ Unregistered local variable
[Remedy]
Do not use unregistered local variables.
If the designated local variable has not been assigned a value, assign a value to the local variable before the relevant block.
2235 No equal sign
Eeoelale4081 A character other than "=" was designated where "=" should be used.
[Object]
System
[Code]
XXYY: Factor classification code and factor parameter designated where "=" should be used.
XX: Factor classification code
YY: Factor parameter
Program example: VTOFX[8]36 VTOFX[8]=36
V13V5V13=V5
VZOFX*20VZOFX=20
[Remedy]
Correct the expression.
2236 No program end code
Eeoelale4082 No end code at the end of the block. There is only "(" without ")". No LAP end code G80.
[Object]
System
[Code]
1-> No program end code
2-> There is only "(" without ")".
2237 Conditional branch (IF, GOTO) sequence name
Eeoelale4083 In the IF or GOTO statement, there is no jump sequence number or the sequence number is incorrect.
[Object]
System (None for schedule program)
[Code]
1-> No sequence name designated at conditional branch
2-> Designated sequence name not found
[Cause]
IF and GOTO branch statements
Program example:
N005 IF [VDIN[34]EQ1]
— Branch destination not designated
[Remedy]
Designate the branch destination sequence name.
Do not use a sequence name that is not used in the program as the branch destination sequence name.
Example:
N010 IF [VDIN[34]
EQ1]
N050
:
N050 CALL OTFRD
:
[Related Specifications]
User task
2238 Conditional branch (IF, GOTO) condition
Eeoelale4084 IF statement or conditional judgment expression is incorrect.
LC37-003 P-189
SECTION 5 ALARM B
[Object]
System (None for schedule program)
[Code]
1-> No "[" after IF
2-> Comparison expression after IF is not enclosed in [ ].
Program example:
[Code] 1
N10 IF [V1 ＋ V2 EQ 3] N100
N20 G00 X500 Z500
N100 G00 X0 Z0
[Code] 2
N10 IF [VTOFX[1]] N100
N20 G00 X500 Z500
N100 M03 S500
[Related Specifications]
User task
2239 Data word 'F’
Eeoelale4085
In G04 mode, the value following the F command is negative or zero.
When the value following the F command is converted into "0.01sec" units in G04 mode, the condition: 0<F≤99999999 is not satisfied.
[Object]
System
[Code]
1->F value does not satisfy: -99999999≤F≤99999999
2->F value is negative or zero.
[Probable Cause]
F command
Program example:
G01 X50 Z50 F-0.2 — [Code] 2
G04 F1000000 — [Code] 1
^^^^^^ The unit is 100000000 when converted to a value of 0.01 sec.
[Measures to Take]
Designate a value that satisfies the range.
2240 DATA WORD 'F' or 'E'
Eeoelale4086
Illegal F or E command
When an F or E command is converted into "microns/rev" or "0.1mm/min" units, the converted result does not satisfy the condition:
-99999≤F (or E) ≤99999.999
In G34 or G35 mode, an overflow occurred when calculating the feed pulses.
[Object]
SYSTEM
[Code]
1->F or E value does not satisfy: -99999≤F (or E) ≤99999.999
3->Overflow occurred when calculating feed pulses
[Probable Cause]
Program error
F or E command value in the program caused the alarm.
In G34 or G35 mode, the pulse count is calculated up to the distance where the F and E command functions end. However, because the F and E commands are incorrect, an overflow occurs during calculation and the pulse count cannot be calculated.
Program example:
G01 X100 F100000.000 — [Code] 1
G34 Z100 F1 E-0.2 — [Code] 3
[Measures to Take]
[Code] 1->Change the F or E command value so that it satisfies the range.
[Code] 2->Check the F or E command value and change it so that it does not cause an alarm.
LC37-003 P-190
SECTION 5 ALARM B
2241 DATA WORD 'I'
Eeoelale4087
Illegal I command
I command value is not: -99999.999≤I≤99999.999
[Object]
SYSTEM
[Code]
1->I command in circular command
Others->Hexadecimal number of I command in threading fixed cycle
Hexadecimal number of I command in non-circular command and non-threading
[Probable Cause]
I command
Program example:
G02 X50 Z70 I100000 K10 — [Code] 1
[Measures to Take]
Change the I command value so that it satisfies the range.
Example: G02 X50 Z70 I10 K10
2242 DATA WORD 'J'
Eeoelale4088
Illegal J command
J command value is not: 0<J≤99999.999.
Or J command is not used in G36 or G37 mode.
[Object]
SYSTEM
[Code]
1->J value is negative
2->J value does not satisfy: 0<J≤99999.999
[Probable Cause]
J command
Program example: G33 X50 Z20 F0.2 J-5 [Code] 1
[Measures to Take]
Change the J command value so that it satisfies the range.
Example: G33 X50 Z20 F0.2 J5
2243 DATA WORD 'K'
Eeoelale4089
Illegal K command
K command value is not: -99999.999≤K≤99999.999
[Object]
SYSTEM
[Code]
1->K command in circular command
Others->Hexadecimal number of K command in threading fixed cycle
Hexadecimal number of K command in non-circular command and non-threading
[Probable Cause]
K command
Program example:
G02 X30 Z30 I20 K100000 — [Code] 1
[Measures to Take]
Change the K command value so that it satisfies the range.
Example: G02 X30 Z30 I20 K-10
2244 DATA WORD 'L'
Eeoelale4090
Illegal L command
L command value in circular interpolation is not: 0<L≤99999.999
In threading, chamfering amount following L and K (and I) commands is not: 0 to 99999.999.
In gauging cycle, L value is not: 0 to 99999.999.
In other modes, L command value is not: -99999.999≤L≤99999.999
LC37-003 P-191
SECTION 5 ALARM B
Or, for machines with cam turning specification, when setting D (major axis of ellipse) and L (cam lift) values in the shape definition file (LSF), the D value is incorrect.
[Code]
None->D value is incorrect
1->In circular interpolation, L command value does not satisfy: -99999.999≤L≤99999.999
2->In circular interpolation, L command value is negative.
Others->Hexadecimal number of L command in non-circular interpolation mode
[Probable Cause]
L command value (used for cam turning specification models)
Program example: G33 Z100 F1 L5 K-6
[Measures to Take]
Change the L command value so that it satisfies the range.
Correct the D value.
2245 DATA WORD 'P'
Eeoelale4091
Illegal P command
P command value is not: -9999≤P≤9999
[Object]
SYSTEM
[Code]
Hexadecimal number of P command
[Probable Cause]
P command
Program example:
N010 G13
N020 G00 X500 Z500 P10000
[Measures to Take]
Change the P command value so that it satisfies the range.
Example:
N010 G13
N020 G00 X500 Z500 M03 S1000 P10
:
N010 G14
N020 G00 X500 Z500 M03 S1000 P10
2246 DATA WORD 'S'
Eeoelale4092
Illegal S command
S command value is not: 0≤S≤9999
Or in synchronized tapping there is no S=0 or another S command is present
[Object]
SYSTEM
[Code]
Hexadecimal number of S command or $FFFFFFFF
Hexadecimal number of S command: S command is not 0≤S≤9999
$FFFFFFFF: In synchronized tapping there is no S=0 or another S command is present
[Probable Cause]
S command
Program example: N010 G00 X500 Z500 M42 S10000 T0101
[Measures to Take]
Change the S command value so that it satisfies the range.
Example: N010 G00 X500 Z500 M42 S3000 T0101
2247 DATA WORD NO 'S'
Eeoelale4093
G96 or G97 without S code.
G96: Constant cutting speed control ON
G97: Cancel G96
LC37-003 P-192
SECTION 5 ALARM B
[Object]
SYSTEM
Character-string: G140, G141, G142 coordinate system
[Code]
1
[Probable Cause]
G96, G97
Program example: N010 G96
[Measures to Take]
Designate an S command.
Example:
N010 G96 S100
:
N200 G97 S500
2248 DATA WORD 'T'
Eeoelale4094
Illegal T command
In T******, two digits are used to represent the tool number, tool length offset number, and tool radius compensation number, respectively, and the number is greater than 32 (96 for 96-tool specification).
[Object]
SYSTEM
[Code]
When T command is not 0<T≤9999999, its hexadecimal number
When tool number, tool length offset number, or tool radius compensation number is greater than 32, the rightmost 4 digits are the hexadecimal number of that number.
[Probable Cause]
T command
Program example:
T011156->[Code]B0038
T243512->[Code]C0023
T112 0101->[Code]650070
T-1->[Code] FFFFFFFF
T100000000->[Code]5F5E100
[Measures to Take]
Designate T command with 4 or 6 digits; each 2 digits must not exceed 32 (96 for 96-tool specification).
2249 DATA WORD 'X'
Eeoelale4095
Illegal X command
X command value is not: -99999.999≤X≤99999.999
Or, the X command value designated by incremental word is not -99999.999≤X≤99999.999 when converted into an absolute value.
[Object]
SYSTEM
[Code]
Hexadecimal number of X command value
[Probable Cause]
X command
Program example: N010 G00 X100000 Z200
[Measures to Take]
Change the X command value so that it satisfies the range.
2250 DATA WORD 'X', 'Z'
Eeoelale4096
In G31, G32, G33 mode (threading fixed cycle), only X or Z command is present, or neither is present.
In G30 gauging mode, X and Z are designated at the same time.
[Object]
LC37-003 P-193
SECTION 5 ALARM B
SYSTEM
[Code]
1->In G31, G32, G33 mode, only X or Z command is present, or neither is present.
2->In G30 gauging mode, X and Z are designated at the same time.
3->In G101 mode, X start point and end point are 0 (in X-C coordinate system) or both X and Y are 0 (in X-Y coordinate system).
4->In LAP block, only X or Z command is present.
Program example:
[Code] 1
G00 X100 Z100 S100 M03
G33 X80 F3
^^^^ Both X and Z must be designated simultaneously. [Code] 2
[Code] 2
G30 X30 Z50 D10 L10
^^^^^^ Delete X or Z.
[Remedy]
 In a threading fixed cycle called by G31, G32, or G33, both X and Z must be specified.
 In a gauging cycle called by G30, either X or Z must be specified.
2251 Data word 'Z'
Eeoelale4097
Illegal Z command
The commanded Z value in circular interpolation is not: -99999.999<=Z<=99999.999
Or, the commanded Z value specified with an incremental word is not -99999.999<=Z<=99999.999 when converted to an absolute value.
[Object]
SYSTEM
[Code]
Hexadecimal number of commanded Z value
[Probable Fault Cause]
Commanded Z value
Program example: N010 G00 X500 Z100000
[Remedy]
Change the commanded Z value so that it falls within the range.
2252 Data word arc calculation
Eeoelale4098
In a circular interpolation command, the arc center coordinates cannot be calculated from the L, X, and Z commands.
In circular interpolation, the command error between I, K and X, Z exceeds the permissible value (standard: 20 um).
[Object]
SYSTEM
[Code]
1-> The L value is less than half the distance to the target point.
2-> Overflow or error occurred during arc center calculation.
3-> The radius calculated from the I, K command is in error, or the distance between the end point and the arc center exceeds the permissible value.
4-> I, K command is commanded as zero.
10-> The circular interpolation end point, tool radius compensation, or tool length compensation calculated by LAP exceeds the specified value.
[Probable Fault Cause]
I, K, L commands and X, Z commands in the G02/G03 block.
Program example:
[Code] 1
G00 X50 Z50
G02 X50 Z0 L20 F0.1
M02
[Code] 2
G00 X0 Z100
G02 X105 Z20 K-100 F0.1
M02
LC37-003 P-194
SECTION 5 ALARM-B
[Code] 3
G00 X0 Z50
G03 X95 I-1 K-20 F0.1
M02
[Remedy]
Change the command values so that an arc can be generated.
2253 Data word angle
Eeoelale4099
In a G00, G01, G02, G03, G34, or G35 block, the A command is specified at the same time with X and Z commands.
The target point calculated from the angle command is not within the range of -99999.999 to 99999.999.
In a G31 or G33 block, the A command and I command are specified at the same time.
In a G32 block, the A command and K command are specified at the same time.
In a threading fixed cycle, the target point calculated from the angle command is not within the range of -99999.999 to 99999.999.
[Object]
SYSTEM
[Code]
1-> Both X and Z commands are specified at the same time, or the A command and I, K commands are specified at the same time.
2-> Neither X nor Z command is specified.
3-> The target point calculated from the angle command is not within the range of -99999.999 to 99999.999.
Others-> Hexadecimal number of the target point calculated from the A angle command in a threading fixed cycle.
Program example:
[Code] 1
G00 X100 Z100
X120 Z50 A160
^^^^^^ Delete either X or Z command.
[Code] 1
G00 X100 Z100 M3 S100
G34 X120 Z50 A170 F3 E0.1
^^^^^^ Delete either X or Z command.
[Code] 3
G00 X100 Z100
X120A179.999
Target value of Z is 5729477.95.
Change X or A to a smaller value.
[Code] 2
G00 X100 Z100 M3 S500
G03 A150 L30 F0.2
^^^^^^^^ Specify X or Z command.
[Code] 1
G00 X100 Z100 M3 S100
G33 X80 Z50 I10 A170 F3
Specify only I or K command.
2254 Data word threading cycle
Eeoelale4100 In a threading fixed cycle, the shift amount is so large that the cutting direction is changed, or the taper is so large that the tool retracts beyond the threading start point.
[Object]
SYSTEM
[Code]
1-> The taper is too large, and the taper start point exceeds the end point.
2-> The shift amount specified by I, K command is too large, and the threading cycle start point exceeds the end point.
3-> Overflow occurred during calculation of the number of threading points.
Program example:
[Code] 1
G00 X100 Z100 M03 S100
G33 X80 Z50 I20 F3
M02^^^ I command is too large
[Code] 1
G00 X100 Z100 M03 S100
G33 X80 Z50 A120 F3
LC37-003 P-195
SECTION 5 ALARM-B
M02^^^ Taper is too large (A command is too small)
[Code] 2
G00 X100 Z100 M03 S100
M23
G33 X80 Z50 F3 A170 L55 K-55
M22^^^ Shift amount is too large
M02
2255 Data word radius
Eeoelale4101
1) In a G02 or G03 block, both L and I, K commands are present.
2) In a G02 or G03 block, only L command is present, and no I or K command is present.
3) In a G102 or G103 block, no L command is present.
4) In a G132 or G133 block, no L command is present.
5) In a G132 or G133 block, neither Z nor C command is present.
[Object]
SYSTEM
[Code]
1-> In a G02 or G03 block, both L command and I or K command are specified.
2-> In a G02 or G03 block, only L command is specified.
3-> In a G102 or G103 block, no L command is specified.
4-> In a G132 or G133 block, no L command is specified.
5-> In a G132 or G133 block, neither Z nor C command is specified.
[Probable Fault Cause]
A block containing G02, G03, G102, G103, G132, G133
Program example:
[Code] 1
G00 X00 Z100
G03 X110 Z95 L5 K-5
[Remedy]
For a radius command containing an L command, specify both X and Z commands, and do not specify I and K commands.
2256 Data word 'D'
Eeoelale4102
Illegal D command
In a gauging cycle, the D value is not within the range of 0 to 99999.999.
Or, on a machine with cam turning specifications, when setting the D (major axis of ellipse) and L (cam lift) values in the shape definition file (LSF), the D value is incorrect.
[Object]
SYSTEM
[Code]
Hexadecimal number of commanded D value
[Probable Fault Cause]
D command
Program example: G30 Z50 D-10 L10
[Remedy]
Change the D command; 0<=D<=99999.999.
Example: G30 Z50 D10 L10
Check the commanded D value.
[Related Specifications]
 Gauging processing
 Cam turning specifications
2257 Data word gauging cycle
Eeoelale4103
In a G30 gauging cycle, the commanded D value is larger than the distance between the start point and the gauging point.
Or, the commanded CD value is larger than the relative distance between the cycle start point and the target point.
[Object]
SYSTEM
[Code]
LC37-003 P-196
SECTION 5 ALARM-B
X
X=1-> In a G30 gauging cycle, the commanded D value is larger than the distance between the start point and the gauging point.
X=2-> In C-axis gauging, the distance from the start point to the effective target point is greater than 360 degrees.
X=3-> In C-axis gauging, the commanded CD value is larger than the distance between the start point and the gauging point.
[Probable Fault Cause]
 Program example of G30 gauging cycle D command
G00 X50 Z100 G30 Z90 D20 L20
 Program example of G30 gauging cycle CL command
G00 C0 G30 C270 CD=5 CL=120
 Program example of G30 gauging cycle CD command
G00 C0 G30 C90 CD=95 CL=10
[Remedy]
 Change the commanded D value so that it is smaller than the distance between the start point and the gauging point.
Or move the start point away from the gauging point.
 Reduce the commanded CL value so that its target point is close to the start point.
Normally G00 C0 G30 C270 CD=5 CL=80
 Change the commanded CD value so that it is smaller than the distance between the start point and the gauging point.
Or move the start point away from the gauging point.
Normally G00 C0 G30 C90 CD=80 CL=10
[Related Specifications]
Gauging processing
2258 Data word C command
Eeoelale4104
C command alarm
The commanded C value requesting spindle orientation does not satisfy: 0<C<=360.
The C command is specified on the turret B side. Or a C command is specified during G137 coordinate conversion.
The C command is specified in a mode other than G00, G01, G50, G101, G102, G103, or G181 to G190.
The commanded C value is not: -360<C<360 degrees.
The C command calls zero movement in G101 mode.
[Object]
SYSTEM
[Code]
1-> On a multitasking machine, the C command is specified on the turret B side.
2-> The C command is specified in a mode other than G00, G01, G50, G101, G102, G103, or G181 to G190 (milling tool spindle compound fixed cycle).
3-> The C command calls zero movement in G101 mode.
Others: Hexadecimal number of the specified C command
Program example:
M19 C-50->FFFF3CB0 (Hexadecimal number of -50000)
M19 C370->5A550 (Hexadecimal number of 370000)
[Code] 1
G14 <- Command cannot be specified on the turret B side.
M110
G00 X100 C90 M146 M15
M147
M02
[Code] 2
M110
M03 S500
G94 G02 X100 C90 M146 M15 F130
^^^ C command not permitted
M147
M02
[Code] 3
M110
M146 M16
G00 X100 C30 T0101 SB=250 M241
LC37-003 P-197
SECTION 5 ALARM B
G94 Z120 M13
G101 C30 F30
M02 ^^^ C command travel is zero.
[Code] FFFA5AB0 (Hexadecimal value of -370000)
M110
G00 X100 C-370 M146 M15
M147 ^^^ C command must be -360<C<360 deg
M02
[Related Specifications]
Spindle orientation
Multitasking machine
2259 Data word SB command
Eeoelale4105
Designated SB command is not within: 0≤SB≤9999
SB command was designated in B-turret.
[Object]
SYSTEM
[Code]
1-> Designated SB command is not within: 0≤SB≤9999.
Others-> Hexadecimal value of SB command value
[Probable Fault Cause]
Program error
Program example: N010 M13 SB=10000
[Measures to Take]
Check the SB command; check whether the SB command was designated on the B-turret side.
In the above example, the SB command value is greater than 9999; correct the program.
N010 M13 SB=1000
2260 Data word QA command
Eeoelale4106
QA command was designated on the B-turret side.
QA command was designated in a mode other than G00 and G01.
QA command value is not within: 0≤QA≤1999
[Object]
SYSTEM
[Code]
1-> QA command was designated on the B-turret side.
2-> QA command was designated in a mode other than G00 and G01.
4-> QA command in G121 mode.
Others-> Hexadecimal value of QA command value
[Probable Fault Cause]
Block containing QA command
Program example: G01 X100 QA=2000
[Measures to Take]
Check the QA command.
G01 X100 QA=1900
[Related Specifications]
Multitasking machine
2261 Data word X, Y command
Eeoelale4107 In coordinate conversion, both X and Y are 0 simultaneously.
[Object]
SYSTEM
[Probable Fault Cause]
Program error
Program example:
LC37-003 P-198
SECTION 5 ALARM B
G137 C20
G00 X0 Y0
:
[Measures to Take]
Check X and Y commands.
:
G137 C20
G00 X0 Y50
:
[Related Specifications]
Coordinate conversion
2262 Data word incremental command
Eeoelale4108 In coordinate conversion, G code calling incremental mode (G91) was designated.
[Object]
SYSTEM
[Code]
Hexadecimal value of command code
[Probable Fault Cause]
Program error
Program example:
G91
:
G137 C10
:
[Measures to Take]
Designate G90 command (calling absolute mode) before G137 block.
:
G91
:
G90
G137 C10
:
[Related Specifications]
Coordinate conversion
2263 Data word no command on X, Y two axes
Eeoelale4109 In coordinate conversion, only X or Y was designated.
[Object]
SYSTEM
[Probable Fault Cause]
Program error
Program example:
G137 C10
G00 X10
:
[Measures to Take]
Designate both X and Y simultaneously in coordinate conversion.
:
G137 C10
G00 X10 Y10
:
[Related Specifications]
Coordinate conversion
LC37-003 P-199
SECTION 5 ALARM B
2264 Data word ‘Y’
Eeoelale4110
In coordinate conversion, Y value is not within the range -99999.999≤Y≤99999.999.
If the alarm occurs in other than coordinate conversion, refer to the following codes.
[Code]
Hexadecimal value of Y command value in coordinate conversion
1-> Y command was not designated with G00, G01, G02, G03, G30, G18?, or G50.
3-> Y value does not satisfy: -99999.999≤Y≤99999.999.
7-> Y-axis command was designated in other than Y-axis control mode or coordinate conversion mode.
2265 Data word distance calculation
Eeoelale4111 In coordinate conversion, the converted value is greater than 99999.999.
[Object]
SYSTEM
[Probable Fault Cause]
Program error
Program example:
G137 C20
G00 X99999.999 Y99999.999
:
[Measures to Take]
Check X and Y commands;
(Must satisfy: SQR (X*X+Y*Y) ≤99999.999).
:
G137 C20
G00 X100 Y100
:
[Related Specifications]
Coordinate conversion
2266 Data word ‘R’
Eeoelale4112
In a block containing G181, G184, or G189, R=0 was designated or R command was designated together with X and Z commands. Or X, Z, R values are not within the range -99999.999≤X, (Z or
R) ≤99999.999.
[Object]
SYSTEM
[Code]
1-> R is designated together with X and/or Z
FFFFFFFF-> No X, Z, or R command
Others-> Hexadecimal value of designated X, Z, or R command
[Probable Fault Cause]
Program error
Program example:
G181 X60 R0 C0 K48 F40
:
[Measures to Take]
Check X, Z, and R commands.
[Related Specifications]
Multitasking machine
2267 Data word drilling cycle
Eeoelale4113
In a block containing G181, G184, or G189, the following 3 commands were designated simultaneously:
X, R and I, or Z, R and K
[Object]
SYSTEM
[Code]
1-> X, R and I, or Z, R and K designated simultaneously
LC37-003 P-200
SECTION 5 ALARM B
[Probable Fault Cause]
Program error
Program example: G181 X60 R-27 I48 F40
[Measures to Take]
Check X, Z, R, I, and K commands.
[Related Specifications]
Multitasking machine
2268 Data word arbitrary angle
Eeoelale4114 In the arbitrary angle automatic chamfering block or in the block with only A command axis movement, block command error or next block command error occurred.
[Object]
SYSTEM
[Code]
1-> Because the commanded point is identical to the commanded point in the preceding block, the first line cannot be formed.
2-> A, X, and Z were designated simultaneously.
3-> The next block to be executed is in other than G00, G01, G34, and G35 mode, or contains an incorrect command.
4-> In the block with only A command, there is no A, X, or Z command in the next block to be executed.
5-> In the block with only A command, the next block to be executed is in other than G91 mode.
6-> Because the commanded point in the current block is identical to the commanded point in the next block, the second line cannot be formed.
7-> In the next block to be executed, A, X, and Z were designated simultaneously.
8-> When only A command was designated, there is no intersection between the obtained first line and second line.
[Probable Fault Cause]
Program error
Program example:
G75 G01 X60 Z90 A120 L5 F10
:
[Measures to Take]
Check error details in the program from the alarm code; eliminate the cause that impedes execution of the arbitrary angle chamfering command.
:
G75 G01 X60 L5 F10
[Related Specifications]
Automatic arbitrary angle chamfering
2269 Data word arbitrary angle calculation
Eeoelale4115 Calculation error occurred during processing of arbitrary angle command.
[Object]
SYSTEM
[Code]
XYY
YY:
Bit 0-> Overflow when converted into integer
Bit 1-> Exponent underflow
Bit 2-> Exponent overflow
Bit 3-> Square root of negative number
Bit 5-> SIN, COS, TAN, and COT angle overflow
X:
1-> When calculating the slope of the first line from the commanded point in the preceding block and ”A” degrees
2-> When calculating the slope of the first line from the commanded point in the current block and the commanded point in the preceding block
3-> When calculating the slope of the second line from the commanded point in the current block and the commanded point in the next block
4-> When calculating the slope of the second line from the commanded point in the next block and ”A” degrees.
LC37-003 P-201
SECTION 5 ALARM B
5-> When calculating the slope of the second line from the commanded point in the current block and ”A” degrees.
6-> When calculating the commanded point (intersection of the first and second lines) in a block containing only ”A” command.
[Probable Fault Cause]
Program error
[Measures to Take]
Check error details in the program from the alarm code; eliminate the cause that impedes execution of the arbitrary angle chamfering command.
[Related Specifications]
Automatic arbitrary angle chamfering
2270 Data word CD command
Eeoelale4116 CD value exceeds the relative distance from the cycle start point to the cycle end point.
[Code]
1
[Probable Fault Cause]
0≤CD≤360.000
2271 Data word CL command
Eeoelale4117 The CL value exceeds the relative distance from the cycle start point to the cycle end point.
[Code]
1
[Probable Fault Cause]
0≤CL≤360.000
2272 Data word ‘TM’
Eeoelale4118
Illegal TM command
The “oo” value designated in the “TM=oo**” command is larger than the number of turret tools set in the parameters. Or, the parameter is not set. Or, the designated “**” value is greater than 32.
[Parameter]
Number of turret tools: Optional parameter word No.47/No.48
[Parameter]
MC system parameter (Turret/Door)
Number of tools for turret A side
Number of tools for turret B side
[Object]
SYSTEM
[Code]
If the TM command is not within the range of 0<TM<99999999, the code indicates the hexadecimal value of the TM command value.
If the tool number is greater than the number of turret tools or the tool length offset number is greater than 32, the lower 4 digits of the code indicate the hexadecimal value of the designated value.
[Probable Fault Cause]
TM command value
Program example:
G14
TM=0233
:
[Measures to Take]
Check the TM command value.
G14
TM=0232
:
LC37-003 P-202
SECTION 5 ALARM B
2273 Data word ‘W’
Eeoelale4119
Sub-spindle axis movement command W error.
1) A W-axis movement command was designated on the turret B side.
2) A W-axis movement command was designated in a mode other than G00, G01, or G50.
3) The W-axis movement value does not satisfy: -99999.999≤W≤99999.999
4) A W-axis movement command was designated in G141 sub-spindle mode.
5) A W-axis movement command was designated in G123 mode on the turret A side.
[Object]
SYSTEM
[Code]
1-> A W-axis movement command was designated on the turret B side.
2-> A W-axis movement command was designated in a mode other than G00, G01, or G50.
3-> A W-axis movement command was designated in G141 sub-spindle mode.
4-> A W-axis movement command was designated in G123 mode on the turret A side.
Others-> Hexadecimal value of the W-axis command
[Probable Fault Cause]
W-axis command
Program example:
G14
G01 W100.5 F100 G94
:
[Measures to Take]
Check the W-axis command in the program.
:
G14
G01 W100.5 F100 G94
:
[Related Specifications]
Sub-spindle
2274 Data word ‘CB’
Eeoelale4120 The M-axis orientation angle command value is smaller than 0 or larger than 360.
[Object]
SYSTEM
[Code]
Hexadecimal value of the CB command value
[Probable Fault Cause]
Program error
Program example: M229 CB=360
[Measures to Take]
Correct the CB value in the program.
2275 Data word ‘HP’
Eeoelale4121
In the G20 home position command, the HP command value is not 1 to 8, or there is no HP command in the G20 block. Or, the G20 command was designated when the home position function is not provided.
G21 tool change position offset was designated in an incorrect format. (G21 command is also designated in G171 or ATC macro command M321.)
[Code]
1-> HP command value is not 1 to 8.
2-> No HP command in the G20 block.
3-> G20 command was designated when the home position function is not provided.
4-> No HP command in the G21 block.
5-> G21 command was designated when the home position function is not provided.
6-> G21 command was designated when the ATC function is not provided.
7-> A number other than 1 to 5 was designated for the HP command.
8-> G21 command was designated on the turret B specification side.
Program example:
G20 HP9
LC37-003 P-203
SECTION 5 ALARM B
:
[Related Specifications]
Home position function
2276 Data word ‘CC’
Eeoelale4122 The sub-spindle angular position designated by the CC command is larger than ”359.999″, or is a negative value.
[Object]
SYSTEM
[Code]
Hexadecimal value of the CC command
[Probable Fault Cause]
Program error
Program example:
M239 CC=365
[Measures to Take]
Correct the angle command.
[Related Specifications]
Sub-spindle
2277 Data word torque limit
Eeoelale4123
In the G29 torque limit command or G22 torque skip command, there is no PX or PZ torque command, or torque commands for both axes were designated simultaneously.
The torque command value exceeds the setting range.
[Object]
None
[Code]
X
1-> In the G29 torque limit command or G22 torque skip command, there is no PX or PZ command, or a torque command was designated in a mode other than G29 or G22.
2-> Torque commands for both axes were designated simultaneously in G29 or G22.
3-> PX, PZ torque command exceeds the setting range:
For G29, 0≤PX, PZ≤ Optional parameter word No.89.
For G22, 0≤PX, PZ≤torque limit value set by G29.
4-> In the G22 command, the torque setting axis does not match the axis command.
5-> An axis movement command was designated in the G22, G28/G29 block.
[Probable Fault Cause]
G22, G28/G29 command format error
2278 Subroutine loop
Eeoelale4124 The designated number of subroutine loops is not 1 to 9999.
[Object]
SYSTEM
[Code]
Hexadecimal value of the designated number of loops
[Probable Fault Cause]
Subroutine call command
Program example:
CALL OAAA Q10000 [Code] 2710 (hexadecimal value of 10000)
[Measures to Take]
Set the Q command value within the range from 1 to 9999.
2279 Subroutine stack
Eeoelale4125
The number of subroutine nestings is greater than 8.
LC37-003 P-204
SECTION 5 ALARM B
Or, the number of subroutine return commands RTS exceeds the number of call commands CALL.
Or, the number of MODOUTs is greater than the number of MODINs.
The number of nestings after an axis movement command is greater than 8.
The number of cancel calls after an axis movement command does not match the number of call levels after an axis movement command.
[Object]
SYSTEM
[Code]
1-> Too many RTS statements.
2-> The number of subroutine nestings is greater than 8.
3-> Too many MODOUTs.
4-> The number of MODIN nestings is greater than 8.
5-> MODIN modal call and cancel do not match.
[Probable Fault Cause]
 Number of times CALL, RTS, MODIN, and MODOUT statements are used in the program
 Program error
Program example:
[Code] 3
N100 MODIN O100
N110 G00 X100 Z100
N120 X50 Z50
N130 MODOUT
N140 MODOUT
[Measures to Take]
Check the number of times and nesting levels of CALL, RTS, MODIN, and MODOUT in the program according to the alarm code.
[Related Specifications]
User task 2
2280 Subroutine program name
Eeoelale4126
No subroutine name is designated in the CALL or MODIN block.
Or, the designated subroutine name is not registered in the program name registration stack.
G171 or M321 ATC macro command was designated without switching to automatic mode after power-on.
[Object]
SYSTEM
[Code]
1-> No subroutine name is designated.
2-> The designated subroutine name is not registered in the program name registration stack.
Or, G171 or M321 ATC macro command was designated without switching to automatic mode after power-on. After program selection in automatic operation mode, the name of the subroutine called by a G-code macro command or M-code macro command was changed.
[Probable Fault Cause]
 CALL, MODIN block
Program example:
CALL ->[Code] 1
CALL O ->[Code] 2
^^^^ Unregistered subroutine
 Unless a macro program is resident in buffer, ATC macro commands G171 and M321 cannot be executed.
When switching to automatic operation mode after power-on, the macro program is registered to buffer.
If the subroutine called by a G-code macro program or M-code macro program designated by the program is renamed after program selection in automatic mode, to call the renamed subroutine, the program must be re-selected in automatic mode.
[Measures to Take]
In the CALL or MODIN block, designate only subroutines registered in the program name registration stack.
[Related Specifications]
User task 2 / ATC
LC37-003 P-205
SECTION 5 ALARM B
2281 Subroutine data print
Eeoelale4127 Printout measurement data command is not correctly designated.
[Code]
1-> Printout measurement data command is incorrect.
2-> FD output file name is incorrect.
[Probable Fault Cause]
Program error
Program example:
Code 1->PRNT @
PRNT *
Code 2->PRNT A12345950
[Measures to Take]
 Change characters contained in the measurement printout command to numeric values.
:
PRNT 10
:
 Change isolated alphabetic characters to consecutive letters or digits, or ”_” as the file name.
:
PRNT A1234
:
[Related Specifications]
Measurement data printout
2282 Schedule program ‘Q’
Eeoelale4128 Schedule program contains an incorrect Q command.
[Code]
1-> A numerical value is designated where address character Q is designated.
4-> Another address character is designated where address character Q is designated.
Others-> Q value is not 0<Q≤9999.
Hexadecimal value of the Q value
[Probable Fault Cause]
Schedule program
Program example
PSELECT A.MIN , , 20 — [Code] 1
PSELECT B.MIN , , P 10 — [Code] 4
PSELECT C.MIN , , Q20000 — [Code] D020 (Hexadecimal number of 20000)
[Measures]
Modify the Q command in the schedule program.
For example: PSELECT A.MIN , , Q20
2283 Schedule program mnemonic code
Eeoelale4129
Illegal schedule program command
A command other than PSELECT, IF, GOTO, VSET, and END was designated.
[Code]
Hexadecimal number of the ASCII code of the first 4 characters in the command
[Probable Fault Cause]
Schedule program
Program example: N100 PSELECT A.MIN , , Q10
N200 G00 X100 Z200
:
[Measures]
Delete the erroneous command from the schedule program.
LC37-003 P-206
SECTION 5 ALARM B
2284 Schedule program end
Eeoelale4130 There is no program end command in the schedule program.
[Code]
1
[Probable Fault Cause]
Schedule program
Program example:
N010 CSET V1=1
N020 PSELECT LOADER.MIN
N030 PSELECT SHAFT.MIN
N040 VSET V1=V1+1
N050 IF [V3 LE 10]
N020
[Measures]
Designate the END command at the end of the schedule program.
For example:
N010 VSET V1=1
:
N050 IF [V3 LE 10]
N020
N060 END
2285 Schedule program main program load
Eeoelale4131
An error occurred when loading the main program in the schedule program.
The main program does not exist, the program end code is wrong, etc.
[Code]
3-> An error occurred when loading the main program.
[Probable Fault Cause]
The main program does not exist
Program end code is wrong, etc.
2286 Variable soft-limit over +
Eeoelale4132 Axis movement command designated a target point exceeding the positive variable soft-limit.
[Object]
Axis
[Code]
1-> In the Z-axis state when the sub-spindle mode is selected.
However, an alarm does not occur even if the sub-spindle mode is selected for the ZA-axis + sub-spindle specification in LT specification and the ZB-axis in LT specification (sub-spindle specification not selected).
2-> Axis feed in non-rapid mode
3-> Tool nose radius compensation mode in G00
4-> LAP mode in G00
5-> X-axis in 2-saddle mode
[Measures]
Change the command value so that it is less than the positive variable soft-limit.
Check the zero offset value.
Check the tool offset value.
2287 Variable soft-limit over -
Eeoelale4133 Axis movement command designated a target point smaller than the negative variable soft-limit.
[Object]
Axis
[Code]
1
[Measures]
LC37-003 P-207
SECTION 5 ALARM B
Change the command value so that it is greater than the negative variable soft-limit.
Check the zero offset value.
Check the tool offset value.
2288 User reserve code
Eeoelale4134
An alarm is designated by output variable #992.
When the G171 or M321 ATC macro command was designated, the interlock function was activated, causing this alarm.
Under the Y-axis control mode, the groove width offset measurement command contains a command related to the tool life management function.
[Code]
Output variable data value
MT-> The MT command was not designated before M321.
M321-> When the M321 command was designated, the turret was not at the X-axis positive limit position.
ATP-> An ATP or AHP command was not designated before G171. A non-machine turret number was designated for ATP. Automatic tool change cannot be performed for the turret number designated by ATP.
AHP … In the G171 command, a number other than 1 to 5 was designated for AHP.
[Probable Fault Cause]
If code MT appears, the MT command is not designated for M321.
Although MT was designated, other operations such as reset, manual operation mode selection, machine lock, etc., were performed before M321.
2289 Backup data file write
Eeoelale4135 An error occurred when writing the backup data file to memory.
[Code]
Hexadecimal number of the memory sector where the error occurred.
[Probable Fault Cause]
Memory board
Operation example: Backup to memory is performed automatically; occurrence of the alarm is not related to operations.
2290 Program name not selected
Eeoelale4136 Designated program name is incorrect. A program name different from the program name* of the currently executed program was designated.
* O**** command was executed.
[Object]
System
[Code]
Hexadecimal number of the ASCII code of 4 characters in the program name following the address character.
[Probable Fault Cause]
Block that caused the alarm (refer to the program example below).
Program example:
1) The CALL command was not designated when calling a subprogram (similarly for MODIN).
N100 G00 N100 G00
N110 G01 N110 G01
N120 G00 N120 G00
CALL O100 O100
N130 G00 N130 G00
Normal Alarm
If a sequence number N is designated before O100, another alarm will occur. (Alarm B 429 Left direction disabled)
2) For a program with two program names, a jump command to jump to the second program was not designated. No GOTO statement was designated.
O100 O100
G00 G00
G00 G00
GOTO N1 O200<- Alarm occurs when this block is executed.
O200 G00
G00 G00
G00 N1 G01
N1 G01 G01
LC37-003 P-208
SECTION 5 ALARM B
G01 :
[Measures]
Do not execute a sequence containing only a program name.
[Related Specifications]
User Task 2
2291 Main sequence
Eeoelale4137 Main sequence error (TRAP#4). Normally, an error does not occur in the main sequence.
[Object]
System
[Code]
1
2292 Restart
[Probable Fault Cause] Eeoelale4138
Restart command. The cycle start button was pressed before sequence return was completed.
[Code]
1-> 2-saddle lathe: The cycle start button was pressed after designating the restart command for only one turret.
For example, 2-saddle lathe:
Key in [A] RE N100, press the WRITE key, and press the cycle start button.
2-> The cycle start button was pressed after the restart command was executed.
For example, 2-saddle lathe:
Key in [A] RE N100, press the WRITE key.
Key in [B] RE N150, press the WRITE key.
Press the cycle start button.
For example, 1-saddle lathe:
Key in RE N100, press the WRITE key.
3-> During A-turret independent operation, the B-turret restart command was designated.
For example, during A-turret independent operation:
Key in [B] RE N200, press the WRITE key. Press the cycle start button.
During B-turret independent operation, the A-turret restart command was designated.
M02 or M30 was designated before movement was completed.
The restart command was designated when no program was selected.
4-> 2-saddle lathe: A/B turrets cannot return to a fixed position.
Program example:
When the return position is as follows;
Turret A stops at P20, waiting for synchronized operation; when turret B returns to the return position before P30, it waits at P30. Therefore, sequence return of turret A cannot be completed.
Turret A Turret B
G13 G14
G140 G141
G0 X100 G0 X200
… …
… P10
P20 …
… …
G0 Z100 G0 Z200
… …
… P30
P40 …
5-> With Y-axis: Restart to Y-axis was designated in non-Y-axis mode.
6-> With Y-axis: Restart to non-Y-axis was designated in Y-axis mode.
7-> For LAW-F machine, the restart command was designated when the Z-axis was not at the positive variable soft-limit.
8-> The restart command was designated when not in single block mode.
2293 MDI special G-code
Eeoelale4139 The designated G-code cannot be executed in MDI mode.
[Object]
System
LC37-003 P-209
SECTION 5 ALARM B
[Code]
1-> G223 MODIN and/or G224 MODOUT status was designated.
80-> G80, G81, or G82 was designated.
85-> G85 or G86 was designated.
[Measures]
Do not input the above G-codes in MDI mode.
2294 Special G-code table
Eeoelale4140 The internal fixed address table determined by the special G-code is incorrect. (This alarm does not normally occur)
[Object]
System
[Code]
Hexadecimal number of the designated G-code
[Probable Fault Cause]
Special G-code table
2295 STM time over
Eeoelale4141 S, T, or M function execution cycle time exceeded the parameter setting value.
[Parameter]
STM time is set by NC optional parameter (word) No. 26 (unit: 0.1 s).
Optional parameter (Cycle time over check) STM time-over timer (0.1 sec)
[Object]
System
[Code]
Hexadecimal number of the set time
[Probable Fault Cause]
An alarm occurred because there was no answer signal after execution of the S, T, or M code.
Program example:
:
M03 M42 S1000 T0303
:
[Measures]
When the alarm occurs, check whether the input signal is issued after execution of the STM command. If two or more commands were designated, execute them one by one in MDI mode to find the STM command that caused the alarm.
S-> Spindle constant speed rotation signal
T-> Turret clamp signal
M-> Spindle rotation complete signal
2296 UGC No program end code
Eeoelale4142 Program end code was read during conversion of user graphic command characters.
[Code]
1-> During conversion of user graphic command execution statement
2-> While skipping user graphic command comment line
[Probable Fault Cause]
Error in UGC command string in part program
Program example:
DEF WORK （UGC WORK）
PS LL， [0， 0]， [100， 100]， 4
：
END
[Measures to Take]
Check the UGC program.
In the example program, there is an error in the comment line.
LC37-003 P-210
SECTION 5 ALARM B
Modified program:
DEF WORK （UGC WORK）
PS LL， [0， 0]
[100， 100]， 4
：
END
2297 UGC DELETE statement
Eeoelale4143 An illegal delete command was designated.
[Code]
User graphic internal code
[Probable Fault Cause]
Character string: DELETE statement designated in user graphic command.
Program example: DELETE PAINT
[Measures to Take]
Check the character string following the DELETE statement.
[Related Specifications]
Graphics
2298 UGC DEF statement
Eeoelale4144 An illegal definition command was designated.
[Code]
User graphic internal code
[Probable Fault Cause]
Character string: DEF statement designated in user graphic command.
Program example: DEF PAINT
：
[Measures to Take]
Check the character string following the DEF statement.
[Related Specifications]
Graphics
2299 UGC TIP statement
Eeoelale4145
An illegal standard processing statement (TIP statement) was designated.
TIP: Statement for processing tool shape
[Code]
User graphic internal code
[Probable Fault Cause]
The TIP statement registering the tool shape in user graphic command.
Program example:
DEF TOOL [1，L]
TIP [[0， 0]，[1，0]，[1，0]]]
：
END
[Measures to Take]
If there is no TIP statement, add a TIP statement.
If there is a TIP statement, check and correct it.
Modified program
DEF TOOL [1，L]
TIP [[0，0]，[1，0]，[1，0]]
：
END
[Related Specifications]
Graphics
LC37-003 P-211
SECTION 5 ALARM B
2300 UGC TIF statement
Eeoelale4146
An illegal standard processing statement (TIF statement) was designated.
TIF: Automatically generates tool interference check data based on tool shape.
TIF[ Tool interference check mode designation, FZN, FZP, FXN, FXP]
Tool interference check mode designation: I for ID turning, O for OD turning.
FZN, FZP, FXN, FXP: Used to designate interference check range from the cutting edge reference point.
[Code]
User graphic internal code
[Probable Fault Cause]
The TIF statement registering the tool shape in user graphic command.
Program example
DEF TOOL [1，L]
TIP [[0， 0]，[1，0]，[0，1]]
TIF [M，5，5，0，]
：
END
[Measures to Take]
If there is no TIF statement, add a TIF statement.
If there is a TIF statement, check and correct it.
Modified program:
DEF TOOL [1，L]
TIP [[0，0]，[1，0]，[0，1]]
TIF [0，5，5，0，]
：
END
[Related Specifications]
Graphics
2301 UGC Shape not registered
Eeoelale4147 User graphic command is not registered.
[Code]
1-> There is no user graphic command (including standard program statements) between the definition registration statement and definition end statement.
[Probable Fault Cause]
User graphic command character string
Program example
DEF WORK
END
：
[Measures to Take]
Add user graphic commands for shape definition.
：
DEF WORK
PS LL，[0，0] [100，150]，4
END
：
[Related Specifications]
Graphics
2302 UGC Illegal number
Eeoelale4148 An illegal numerical value was entered.
[Code]
Digit overflow
[Probable Fault Cause]
Numerical value in user graphic command
Program example: DEF WORK
PS LL， [0， 0]， [1000000， 100]， 4
END
LC37-003 P-212
SECTION 5 ALARM B
[Measures to Take]
Check the numerical value and correct it.
DEF WORK
PS LL，[0， 0]，[100，100]，4
END
[Related Specifications]
Graphics
2303 UGC Illegal character
Eeoelale4149 An illegal code not applicable to the operation code was designated.
[Code]
1-> Hexadecimal number of ASCII code
[Probable Fault Cause]
User graphic command character string
Program example: DEF WORK
PS LL，[0， 0]，[100&100]，4
：
END
[Measures to Take]
Use only the following characters.
0 – 9， A – Z，]， ，， +， -， *， /， [， =
DEF WORK
PS LL，[0，0]，[100，100]，4
：
END
[Related Specifications]
Graphics
2304 UGC User variable
Eeoelale4150 An illegal user variable was designated.
[Code]
0-> User variable was not input
1-> A number was input after the user variable number
2-> Digit overflow in designated user variable number
[Probable Fault Cause]
Character string starting with ”D” in user graphic command character string.
Program example: DEF WORK
PS LL，[0， 0]，[D100，100]，4
END
[Measures to Take]
Check user time variables (D0 - D99) or character string.
DEF WORK
PS LL，[0，0]，[D10，100]，4
END
[Related Specifications]
Graphics
2305 UGC System variable
Eeoelale4151 An illegal system variable was designated.
[Code]
0-> System variable was not input
1-> A number was input after the system variable number
2-> Digit overflow in designated system variable number
[Probable Fault Cause]
Character string starting with ”S” in user graphic command character string.
Program example:
LC37-003 P-213
SECTION 5 ALARM B
DEF WORK
PS LL，[0， 0]，[S100，100]，4
END
[Measures to Take]
Check system time variables (S0 - S99) or character string.
DEF WORK
PS LL，[0，0]，[S10，100]，4
END
[Related Specifications]
Graphics
2306 UGC Illegal command
Eeoelale4152 An illegal character string was designated.
[Code]
Hexadecimal number of ASCII code or user graphic internal code
[Probable Fault Cause]
User graphic command character string
Program example:
DEF WORK
PS LZ，[0， 0]，[100，100]，4
END
[Measures to Take]
Check and correct the user graphic command character string.
DEF WORK
PS LL，[0， 0]，[100，100]，4
END
[Related Specifications]
Graphics
2307 UGC Too many program elements
Eeoelale4153 Element code stack or element numerical value stack overflow
[Code]
1-> Element code stack overflow during character string conversion
2-> Element numerical value stack overflow during character string conversion
3-> Element code stack overflow during command generation
4-> Element numerical value stack overflow during command generation
[Probable Fault Cause]
User graphic command character string
Program example:
D1=D1+1+1+1 … +1
^^^^^^^^^^^^^^^^^^^^^125 or more
[Measures to Take]
User graphic command character string
Reduce the number of element codes and element numerical values, or divide the expression using an assignment statement.
D1=D1+1+1 … +1
^^^^^^^^^^^^^^^^^^^ Less than 124
[Related Specifications]
Graphics
2308 UGC Coordinate data
Eeoelale4154 Mismatched parentheses, illegal element code, or improper number of coordinate system commands
[Target]
System
[Code]
1-> Mismatched parentheses, illegal element code, or too many parentheses in command
LC37-003 P-214
SECTION 5 ALARM B
2-> Mismatched parentheses, or improper number of coordinate commands
3-> Mismatched parentheses, illegal element code, improper number of coordinate commands, or too many parentheses in command
[Probable Fault Cause]
User graphic command
Program example:
PF 3，[0，0]，[10，0]，[0，10]，[7，8]，4
：
[Measures to Take]
Check and correct the user graphic command format.
：
PF 3，[0，0]，[10，0]，[0，10]，4
：
[Related Specifications]
Graphics
2309 UGC END statement
Eeoelale4155 An illegal end statement was designated.
[Target]
System
[Code]
1-> No CR/LF after END.
[Probable Fault Cause]
END statement in user graphic command string.
Program example:
DEF WORK
:
END X
[Remedy]
Delete extra character string after the END statement.
:
DEF WORK
:
END
[Related Specifications]
Graphic
2310 UGC command overflow
Eeoelale4156 User graphic command stack overflow
[Code]
1-> Overflow occurred in the user graphic command string temporary storage area.
[Probable Cause]
User graphic command string
Program example:
:
*DEF
:
*END
*-* More than 600 bytes
[Remedy]
Reduce the number of commands in the command string to reduce the memory space required for macro programs.
:
*DEF
:
*END
*-* Reduce to less than 600 bytes
LC37-003 P-215
SECTION 5 ALARM-B
[Related Specifications]
Graphic
2311 UGC command format
Eeoelale4157 Symbol error: POINT statement, VIEW statement, WINDOW statement, LINE statement, CIRCLE statement, PAINT statement, PAINTI statement, PAINTS statement, PAINTP statement,
CALL statement, PLAIN statement, and sub-statement
[Code]
User graphic internal code
[Probable Cause]
User graphic command
Program example:
:
PS L, [0, 0], [100, 100], 4
:
[Remedy]
Check and correct the user graphic command statement.
:
PS LL, [0, 0], [100, 100], 4
:
[Related Specifications]
Graphic
2312 UGC additional parameter
Eeoelale4158 Illegal additional parameter specified
[Code]
1-> Illegal arc rotation direction (use only L, R, or omit)
Illegal triangle (use only 0, 1, 2, or omit)
Illegal line type, title format, and color (0 to 7 or omit)
[Probable Cause]
User graphic command additional parameter
Program example:
LI [100, 100], 9
:
[Remedy]
Check and correct the user graphic command additional parameter.
:
LI [100, 100], 6
:
[Related Specifications]
Graphic
2313 UGC expression
Eeoelale4159 Expression syntax error
[Code]
1-> More than one solution
2-> Program end code in expression
3-> Operation stack overflow
4-> Operands do not match
5-> Operation classification code stack overflow: Left and right parentheses do not match.
6-> More than two subscript expressions
[Probable Cause]
Sub-statement or quadratic equation in user graphic command
Program example:
PS LL, [0, 0], [100, 100, 100], 4
:
[Remedy]
LC37-003 P-216
SECTION 5 ALARM-B
Check and correct the sub-statement or equation.
:
PS LL, [0, 0], [100, 100, 100], 4
:
[Related Specifications]
Graphic
2314 UGC shape registration area overflow
Eeoelale4160 The total number of previously registered areas and currently registered areas exceeded the allowable value of the shape registration area.
[Code]
1-> No empty area in shape registration area
[Probable Cause]
User graphic registration area
[Remedy]
Delete the current user graphic command string, or delete unused registered user graphic command strings before registering current data.
[Related Specifications]
Graphic
2315 UGC cannot delete
Eeoelale4161 No user graphic command string to delete.
[Code]
1 User graphic command to be deleted is not registered
[Probable Cause]
DELETE statement in user graphic command.
Program example:
:
DELETE MACRO[8]
:
[Remedy]
Check and correct the command string to be deleted.
[Related Specifications]
Graphic
2316 READ/WRITE no spec.
Eeoelale4162 Attempted to execute READ/WRITE command when READ/WRITE function is not provided.
[Object]
SYSTEM
[Probable Cause]
Program error
[Remedy]
Delete the READ/WRITE statement.
[Related Specifications]
User task 2
2317 READ/WRITE capacity overflow
Eeoelale4163 Data size exceeded 160 bytes when READ/WRITE command was executed.
[Object]
SYSTEM
[Code]
1-> Alarm occurred during READ command execution
2-> Alarm occurred during WRITE command execution
LC37-003 P-217
SECTION 5 ALARM-B
[Probable Cause]
Program error
Program example:
PUT ‘AB’
PUT ‘AB’
: 80 lines
PUT ‘AB’
PUT ‘AB’
:
WRITE 1
One character is expressed in a 7-bit code.
To distinguish Roman characters from Katakana, the SO code is placed before Katakana and the SI code is placed before Roman characters. However, if Roman characters (Katakana) are consecutive,
the SI (or SO) code is not attached before the character. In the above example, the SI code is placed at the head of the data, so the data size exceeds 161 bytes, resulting in an alarm.
[Remedy]
Check the GET/PUT command.
:
PUT ‘AB’
PUT ‘AB’
PUT ‘AB’79 lines
PUT ‘AB’
:
WRITE 1
[Related Specifications]
User task 2
2318 READ/WRITE device No.
Eeoelale4164 Device number error in READ/WRITE command.
[Object]
SYSTEM
[Code]
1-> Device number is not a numeric value.
2-> Device number is not 0 to 4.
[Probable Cause]
Program error
Program example
:
WRITE 5
:
[Remedy]
Check the READ/WRITE command.
:
WRITE 4
:
[Related Specifications]
User task 2
2319 READ/WRITE data
Eeoelale4165 Data error in READ/WRITE command.
[Object]
SYSTEM
[Code]
1-> Parity error during read operation
2-> Transmission end code during write data
[Probable Cause]
Hardware