This is Part 3 of the English reference for FANUC P/S (Program / Setting) alarm numbers, covering 0492–1308.
- Part 1 — P/S alarms 0001–0224
- Part 2 — P/S alarms 0230–0461
- Part 3 — P/S alarms 0492–1308
- Part 4 — P/S alarms 1332–1973
- Part 5 — P/S alarms 2032–5110
- Part 6 — P/S alarms 5130–5559
Each entry gives the alarm message and the practical meaning or first action on the floor. The exact text on your screen is authoritative — messages, descriptions, and parameter numbers vary by FANUC series, options, and software version. Confirm any parameter number on your machine before changing it.
0492–0497: Built-in 3D Interference Check
| Code | Message | Meaning / action |
|---|---|---|
| 0492 | Interference check invalid shape: [object name] | The shape data of the [object name] specified in the CNC built-in 3D interference check is invalid. |
| 0493 | Interference check movement axis invalid: [object name] | The movement axis data of the [object name] specified in the CNC built-in 3D interference check is invalid. |
| 0494 | 3D interference check function disabled | The CNC built-in 3D interference check function has been disabled by parameter ICE (No. 10930 #0). |
| 0495 | Too many shapes for interference check | The total number of cuboids contained in all objects to be checked for collision, excluding tools, exceeds 23. |
| 0496 | Error in P and Q commands in G22.2 | In the G22.2 command, the P and Q commands are out of range or not specified. Correct the program. |
| 0497 | Interference check tool shape cannot be created with the tool management function | Although parameter ICT (No. 10930 #2) is set to automatically create the tool shape using the tool management function, the tool management function option is not present. |
0501–0509: M Code, Superimposition, Tool Position Offset
| Code | Message | Meaning / action |
|---|---|---|
| 0501 | Specified M code cannot be executed | The command method of the M code set in parameters No. 11631 to 11646 is not macro execution, macro interrupt, macro call using G/M code, or subprogram call using T/S/second auxiliary function code. |
| 0502 | G code that cannot be commanded | (1) A G code that cannot be used in flexible synchronization mode between paths was specified. (2) A G code that cannot be used in the superimposition priority state was specified. |
| 0503 | Modal state that cannot be superimposed | This is a modal state of a G code that cannot be superimposed. |
| 0509 | Tool position compensation cannot be specified | Tool position compensation (lathe system) was commanded in the same block as thread cutting. Or tool position compensation (lathe system) was commanded in scaling, coordinate rotation, or programmable mirror mode. |
0511–0514: Cs Contour Control and Arbitrary Axis Exchange
| Code | Message | Meaning / action |
|---|---|---|
| 0511 | Cs contour control high-speed switching format error | The format of Cs contour control high-speed switching is incorrect. |
| 0512 | Cs contour control high-speed switching command not possible | The following commands cannot be used together with Cs contour control high-speed switching: movement commands, synchronous control, mixed control, superimposed control, simple spindle synchronous control, simple spindle electronic gear box, manual reference position return. |
| 0513 | Cs contour control high-speed switching setting error | The setting for Cs contour control high-speed switching is incorrect. Possible causes: the Cs contour control high-speed switching M code values duplicate across multiple Cs contour control axes; or the Cs contour control high-speed switching completion signal CSMCx did not become 1, so the M code returned FIN. |
| 0514 | Invalid arbitrary axis exchange command | (1) During arbitrary axis exchange, an acquisition command was issued to an axis that has not been released. (2) The values of P, Q, R, I, J, K and L specified with G52.1, G52.2 and G52.3 are invalid. (3) The value of parameter No. 11560 is duplicated. (4) A release command (G52.1) was issued to an already released axis. (5) Axes with different values of parameter FAN (No. 11562 #1) were exchanged. (6) An offset was not canceled when arbitrary axis exchange was performed. |
0527–0539: Pitch Error Compensation and Thread Cutting
| Code | Message | Meaning / action |
|---|---|---|
| 0527 | Pitch error compensation data input error | Due to the parameter setting, there is data where the difference between a pitch error compensation point judged to require checking and the adjacent compensation point exceeds the range of −128 to +127. Correct the pitch error compensation data or change the parameter. |
| 0528 | Thread format error | The format of arbitrary speed thread cutting is incorrect. |
| 0529 | Thread cutting command cannot be executed | (1) In arbitrary speed thread cutting mode these cannot be used: thread cutting commands other than thread cutting (G32), thread cutting cycle (G92) and compound thread cutting cycle (G76, G76.7); a taper angle smaller than that of the previous section (continuous thread cutting), or a cutting angle smaller than the taper angle (thread cutting cycle); in continuous thread cutting, commands using automatic acceleration/deceleration calculation down to 0 speed; synchronous control, mixed control, superimposed control, manual reference position return, simple spindle synchronous control, simple spindle electronic gear box. (2) An arbitrary speed thread cutting command was issued during Cs contour control. (3) The spindle software does not support arbitrary speed thread cutting. (4) A reset was performed in arbitrary speed thread cutting mode and the Cs contour control switch signal was not set to 0. |
| 0530 | Thread cutting speed too high | During arbitrary speed thread cutting, the feed axis speed exceeded the maximum cutting speed. |
| 0531 | Illegal thread parameter | The parameter setting for arbitrary speed thread cutting is incorrect. Possible causes: the arbitrary speed thread cutting start M code values duplicate across multiple Cs contour control axes; the cancel M code values duplicate; or the feed axis acceleration (parameter No. 11492) is smaller than the spindle (Cs contour control axis) acceleration (parameters No. 11030 to 11032, No. 25710 to 25712). |
| 0532 | Thread re-machining not possible | Thread cutting re-machining cannot be performed. Possible causes: the thread groove has not been measured; the coordinate value of the thread cutting command does not match the thread groove measurement data; or mirroring is applied to the first and second axes of the plane. |
| 0538 | Nose R compensation not canceled | When nose R compensation can be specified in the shape program of the compound turning fixed cycle (G70) finishing cycle (parameter NT2, No. 5106 #3 = 1), G40 is not specified in the last block of the shape program. |
| 0539 | Invalid spindle maximum speed clamp command | The spindle maximum speed clamp command is invalid. The extended name of a spindle cannot be specified in the spindle maximum speed clamp command. |
0542–0602: Manual Absolute and Servo Motor Spindle
| Code | Message | Meaning / action |
|---|---|---|
| 0542 | Manual absolute path error | Because manual absolute was enabled, the issued command produced an invalid interpolation path. Insert an absolute positioning command before G02/G03. |
| 0601 | Movement command issued to a servo motor spindle | A movement command was issued to a servo axis dedicated to a spindle controlled by a servo motor. Correct the program. |
| 0602 | Spindle command error (servo motor spindle) | The servo motor spindle control axis selection is incorrect. If multi-spindle control is enabled, check whether the selected spindle is a servo motor spindle. If multi-spindle control is disabled, check whether the first spindle in the system that issued the SV rotation control mode command is a servo motor spindle. |
1001–1099: Program Format, Registration, Macro Variables
| Code | Message | Meaning / action |
|---|---|---|
| 1001 | Axis control mode error | The axis control mode is invalid. |
| 1013 | Program number position error | Address O or N was specified in a position where it should not be specified (for example, after a macro statement). |
| 1014 | Program number format error | Address O or N is missing digits. |
| 1016 | No EOB | The end of block (EOB) is missing at the end of the program entered in MDI mode. |
| 1059 | Command is buffered | During automatic operation, while look-ahead blocks exist, the manual intervention amount recovery request signal MIGET became 1. To capture the manual intervention amount during automatic operation, the MIGET signal must be operated with a non-buffered M code command. |
| 1077 | Program in use | A program being edited in the background was called to the foreground for execution. Because a background program cannot be executed, finish editing before continuing. |
| 1079 | Program file not found | The program of the specified file number is not registered in the external device (external device subprogram call). |
| 1080 | Multiple external device subprogram calls | An external device subprogram was called from a subprogram that follows a subprogram called by an external device program. |
| 1081 | External device subprogram call mode error | This mode does not permit calling an external device subprogram. |
| 1090 | Format error in NC program statement | The comment part of an NC program statement, program name, or folder name contains lowercase letters. |
| 1091 | Duplicated subprogram call | More than one subprogram call command appears in the same block. |
| 1092 | Duplicated macro call | More than one macro call command appears in the same block. |
| 1093 | NC address / M99 duplicated | In macro mode call mode, an address other than O, N, P or L can be specified in the same block as M99. |
| 1095 | Number of type II arguments exceeded the limit | In custom macro argument specification II (A,B,C,I,J,K,I,J,K,…), more than 11 sets of I, J and K were specified although the maximum is 10. |
| 1096 | Invalid variable name | An invalid variable name was specified, a code that cannot be used as a variable name was specified, or the [#_OFSxx] command does not match the option configuration of the tool compensation memory. |
| 1097 | Variable name too long | The specified variable name is too long. |
| 1098 | Missing variable name | The specified variable name cannot be used because it has not been registered. |
| 1099 | Invalid subscript in [ ] | No subscript was specified for a variable name that requires one (using square brackets). A subscript was specified for a variable name that does not require one. The subscript value specified with square brackets is out of range. |
1100–1160: Custom Macro Interrupt and Syntax
| Code | Message | Meaning / action |
|---|---|---|
| 1100 | No call to cancel | Macro mode call mode (G66) is not active, but a call mode cancel command (G67) was issued. |
| 1101 | CNC statement cannot be interrupted | An interrupt was attempted in a state where a custom macro interrupt containing a movement command is not allowed. |
| 1115 | Non-readable variable | In a custom macro statement, a variable that can only be used on the left side of an expression was used on the right side. |
| 1120 | Invalid argument specification | The argument specification of a two-argument function (ATAN, POW) has an error. |
| 1124 | No DO | The DO instruction corresponding to the END instruction in the custom macro was not found. |
| 1128 | Sequence number out of range | The target sequence number of the GOTO command in a custom macro statement is outside the range 1 to 99999999. |
| 1131 | No [ | In a custom macro statement, the number of [ is less than the number of ]. |
| 1132 | No ] | In a custom macro statement, the number of ] is less than the number of [. |
| 1133 | No = | The assignment command = is missing in a calculation command of a custom macro statement. |
| 1137 | IF statement format error | The IF statement in the custom macro is incorrectly formatted. |
| 1138 | WHILE statement format error | The WHILE statement in the custom macro is incorrectly formatted. |
| 1139 | SETVN statement format error | The SETVN statement in the custom macro is incorrectly formatted. |
| 1141 | Invalid character in variable name | An invalid character was used in the variable name in the SETVN statement of a custom macro. |
| 1142 | Variable name too long (SETVN) | The variable name you tried to register in the SETVN statement of a custom macro contains more than 8 characters. |
| 1143 | Print statement format error | The BPRNT or DPRNT statement is incorrectly formatted. |
| 1144 | G10 format error | The G10 L number has no corresponding data input or option. There is no command for setting data address P, R, etc. There is an address command unrelated to the data setting. The address to be commanded varies with the L number. There is an error in the sign, decimal point, or range of the commanded address value. |
| 1145 | G10.1 timeout | The PMC response to the G10.1 command timed out. |
| 1146 | G10.1 format error | The G10.1 command format is incorrect. |
| 1152 | G31.9 / G31.8 format error | The format of a G31.9 (continuous high-speed skip) or G31.8 (EGB skip / flexible synchronous control skip) command block has one of these errors: no axis address specified in the G31.9 or G31.8 block; multiple axis addresses specified; no P command specified; in flexible synchronous mode the axis specified in the G31.8 block is not a slave axis; or in flexible synchronous mode the Q command in the G31.8 block is out of range. |
| 1153 | G31.9 command not possible | This is a modal state in which a G31.9 command cannot be issued. This alarm is triggered if G31.9 is issued without canceling a group 07 G code, such as tool diameter compensation. |
| 1160 | Command value exceeded maximum | An overflow occurred in the CNC internal position data. This error also appears when the target position exceeds the maximum travel due to calculations such as coordinate conversion, offset, and manual intervention amount. |
1196–1308: Drilling Cycle, Reference Position, Parameter Input (G10)
| Code | Message | Meaning / action |
|---|---|---|
| 1196 | Drilling axis selection error | The drilling axis command in a fixed drilling cycle is incorrect. There is no Z axis point command for the drilling axis in the G code command block of the fixed cycle. |
| 1200 | Grid synchronization error | During grid-based zero return, the grid position could not be determined because the one-turn signal was not received before the deceleration dog was released. This alarm also occurs if, before the deceleration limit switch is released (deceleration signal *DEC returns to 1), the feedrate never reached a level exceeding the servo error value set in parameter 1841. |
| 1202 | No F command in G93 | The F code in inverse time specification mode (G93) is not treated as modal, so it must be specified for each block. |
| 1223 | Spindle selection error | A command using a spindle was executed when the controlled spindle was not set correctly. |
| 1298 | Inch/metric switching command error | An error occurred when switching between inch and metric. |
| 1300 | Illegal address | When registering parameters or pitch error compensation data externally, or when entering G10 parameters, an axis number address was specified even though the parameter is not axis type. Pitch error compensation data does not require an axis number. |
| 1301 | No address | Parameters or pitch error compensation data were registered externally, or the axis type was specified in G10 parameter input but no axis number was specified. Or the command for data number address N, setting data address P or R is missing. |
| 1302 | Invalid data number | Parameters or pitch error compensation data were registered externally, or the data number command in G10 parameter input is a nonexistent number. The value of address R is invalid in a command of the machining condition selection function or machining surface quality level adjustment function. This alarm also appears when the value of another command is invalid. |
| 1303 | Invalid axis number | The parameter was registered externally, or the axis number address command in G10 parameter input is outside the range of the maximum number of controlled axes. |
| 1304 | Number of digits exceeded | The number of digits of the parameter or pitch error compensation data entered externally exceeds the allowable value. |
| 1305 | Data out of range | When parameters or pitch error compensation data are registered externally, the data is out of range. When entering data with G10, the value of each data setting address corresponding to the L number is out of range. Some NC command words also have a command range, and this alarm is triggered if it is exceeded. |
| 1306 | No axis number | When registering parameters externally, the axis number (address A) that must be specified was not specified. |
| 1307 | Illegal use of minus sign | There is an error in external parameter registration or pitch error compensation data, or the sign of data in G10 is used incorrectly. A command is being issued to an address where a sign is not allowed. |
| 1308 | No data | When registering parameters or pitch error compensation data externally, no value is specified after the address. |
How to Work With These Alarms
- The 1000–1300 range is dominated by program registration and macro syntax errors. For these, display the program at the alarmed block rather than suspecting hardware.
- 1095–1099 and 1141–1146 are macro variable / parameter input problems — check variable names, subscripts, and the G10 L number against the correct data address.
- 1300–1308 are G10 parameter input errors. The single most common mistake is mixing up axis-type and non-axis-type parameters (1300 vs 1301) — check whether the parameter requires an axis number.
- 1200 (grid synchronization error) is mechanical/encoder related, not a program error: check the deceleration dog, the one-turn signal, and parameter 1841.
Disclaimer: This article is a personal compilation organized from FANUC alarm documentation and field reference material, then translated and grouped by code range. Alarm messages, descriptions, and related parameter numbers vary by system model, installed options, and software version. Always follow the text displayed on your machine and the corresponding official manual. Back up parameters before making changes.
Frequently Asked Questions (FAQ)
1. Why do I get alarm 1300 or 1301 when using G10 to set parameters?
Both are address errors in G10 parameter input, and they point in opposite directions. Alarm 1300 means you specified an axis number address for a parameter that is not axis type — pitch error compensation data also does not need an axis number. Alarm 1301 means you specified an axis-type parameter but omitted the axis number, or the command for data number address N, or setting data address P or R is missing. Check the parameter type and the required addresses for your G10 L number.
2. What does alarm 1200 (grid synchronization error) mean?
It means the grid position could not be determined during grid-based zero return: the one-turn signal was not received before the deceleration dog was released. It also occurs when the feedrate never reached a level exceeding the servo error value set in parameter 1841 before the deceleration limit switch released (deceleration signal *DEC returns to 1). This is an encoder / mechanical side issue rather than a program error — check the deceleration dog, the one-turn signal, and parameter 1841.
3. I get repeated macro alarms around 1091–1099. Where do I look?
These are custom macro syntax and variable errors, not hardware faults. Check: whether more than one subprogram call (1091) or macro call (1092) appears in the same block; whether the argument specification II sets exceed 10 (1095); whether a variable name is invalid (1096), too long (1097), or unregistered (1098); and whether a subscript is missing, wrongly present, or out of range (1099). Correct the macro statement in the program.
4. Are alarms 0492–0497 relevant if my machine has no 3D interference check?
No. The 0492–0497 range relates specifically to the CNC built-in 3D interference check function, which requires the corresponding option. Alarm 0494 in particular simply tells you the function has been disabled by parameter ICE (No. 10930 #0), and 0497 tells you the tool management function option needed to auto-create tool shapes is not present. If your machine does not have this option, these codes will never appear.
© 版权声明
文章版权归作者所有，未经允许请勿转载,本资源仅供学习交流，请于下载后24小时内删除，严禁商用。
THE END
暂无评论内容