This is Part 6, the final part of the English reference for FANUC P/S (Program / Setting) alarm numbers, covering 5130–5559. This range is dominated by PMC axis and flexible synchronization control, tool management and tool interference, tilted surface machining (G68.2), tool center point control, and option authentication.
- 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
The exact text on your screen is authoritative — messages, descriptions, and parameter numbers vary by FANUC series, options, and software version. Many codes here require specific options (flexible synchronization, tilted surface machining, tool management) and will not appear without them.
5130–5220: PMC Axis Overlap, Tool Measurement, Reference Position Adjustment
| Code | Message | Meaning / action |
|---|---|---|
| 5130 | NC axis and PMC axis command conflict (superimposed) | When superimposing PMC axis control, the NC command and the PMC axis control command conflict. Correct the program or the ladder. |
| 5131 | NC command that cannot be issued simultaneously with PMC axis control | PMC axis control and a 3D coordinate conversion or polar coordinate interpolation command were issued at the same time. Correct the program or the ladder. |
| 5132 | PMC axis cannot be superimposed | A superimposition axis was selected for an axis to be superimposed with PMC axis control. |
| 5195 | Direction cannot be determined | In the tool compensation measured value direct input B function, the measurement operation is invalid. For single-contact input: (1) the direction of the stored pulse is inconsistent — stop in offset write mode, servo off, direction change; (2) the tool moved along two axes (X and Z) simultaneously. For movement direction discrimination specification: the same two causes, plus (3) the direction indicated by the tool compensation amount write signal does not match the axis movement direction. |
| 5211 | Invalid axis movement command | In servo spindle synchronous mode, the NC issued a servo axis command. Correct the program. |
| 5219 | Cannot recover | In a 3D coordinate conversion or tilted surface machining command, manual intervention and return cannot be performed. |
| 5220 | Reference position adjustment mode | Parameter DATx (No. 1819 #2), which automatically sets the reference position, is set to 1. For manual operation, position the machine to the reference point and perform a manual reference position return. |
5242–5257: Flexible Synchronous Control
| Code | Message | Meaning / action |
|---|---|---|
| 5242 | Invalid axis number | During automatic operation, when the flexible synchronous control mode was switched from off to on, the master axis number / slave axis number was not set correctly. This error occurs in flexible synchronous control between paths when either: (1) the axis number of the master or slave axis is wrong; (2) there is a loop relationship between the master and slave axes. This error occurs when inter-path flexible synchronous control starts. |
| 5243 | Data out of range | If the flexible synchronous control mode is changed from off to on during automatic operation, the gear ratio setting is incorrect. |
| 5244 | Signal status error | During automatic operation, when the flexible synchronous control state changed, the selection signal did not turn on or off after the M code was executed. Flexible synchronous control was turned on/off while an axis was not stopped (except when using flexible synchronous control automatic phase adjustment). Flexible synchronous control was turned off in tilted surface machining command mode. |
| 5245 | Other control axis controlled simultaneously | Occurs when: in a mode other than automatic operation, synchronous mode was enabled while a flexible synchronous control group whose master axis is a PMC axis or servo motor spindle control axis was already in synchronous mode; an attempt was made to enable a synchronous group whose master axis is a PMC axis or servo motor spindle control axis while the master axis of another flexible synchronous control group is a normal axis; the master or slave axis of a synchronous axis overlaps with an EGB virtual axis, an oscillation axis, a tilting axis control related axis, a mixed control related axis, or a superimposed control related axis; the slave axis of a synchronous axis overlaps with a synchronous control related axis; the system entered or is entering zero return mode; a servo alarm occurred in a system performing inter-path flexible synchronous control; an emergency stop occurred in another system during inter-path flexible synchronous control; or inter-path flexible synchronous mode is not enabled when inter-path flexible synchronous control is executed in automatic operation mode. |
| 5253 | Command mode cannot be switched | A mode switching M code command was issued but the mode cannot be switched: the G code mode was not canceled when the mode switching M code was issued; the values of parameters No. 13020 and No. 13021 are the same; the high-speed program check function is currently checking; the program recovery function is currently searching; or an interrupt occurred in an interrupt-type custom macro. |
| 5257 | G41/G42 cannot be commanded in MDI mode | Tool diameter and cutting edge R compensation was performed in MDI mode (depending on the setting of parameter MCR, No. 5008 #4). |
5303–5339: Touch Panel, Spindle Selection, Tool Management
| Code | Message | Meaning / action |
|---|---|---|
| 5303 | Touch panel error | The touch panel is not connected correctly, or it could not be initialized after power-on. Eliminate the cause, then power off and on again. |
| 5305 | Illegal spindle selection P command | When selecting a spindle with address P under multi-spindle control, one of these errors occurred: (1) address P was not specified; (2) parameter No. 3781 was not set to the spindle to be selected; (3) a G code that cannot be specified together with the S_P_; command was specified; (4) multi-spindle is invalid because parameter EMS (No. 3702 #1) is 1; (5) the spindle amplifier number for each spindle is not specified in parameter No. 3717; (6) a command was issued to a spindle whose selection is prohibited (parameter No. 11090); (7) an invalid value is specified in parameter No. 11090. |
| 5312 | Error in G10 L75/L76/L77 command | The command format from G10 L75/L76/L77 to G11 is incorrect, or a command value is outside the data range. Correct the program. |
| 5316 | Tool type number not found | There is no tool of the specified tool model. Correct the program or register the tool. |
| 5317 | All tools have reached the end of their life | All tools of the specified model have expired. Replace those tools. |
| 5320 | Diameter/radius mode cannot be switched | Diameter/radius specification was switched while: (1) a buffered program is being executed; (2) an axis is moving; (3) a diameter/radius dynamic switching function command was issued to an axis with parameter TMDx (No. 10730 #0) = 1. |
| 5324 | Cannot return to the reference position | In a 3D coordinate conversion or tilted surface machining command, manual reference position return cannot be performed. |
| 5329 | M98 and NC command issued together during a fixed cycle | In preset cycle mode, a subprogram call that is not a single block was specified. Correct the program. |
| 5330 | G50.9 format error | A coordinate value was not specified in the G50.9 command block; an M code or B code was not specified in the G50.9 command block; G50.9 was specified in fixed cycle mode; or three consecutive G50.9 command blocks were specified. |
| 5331 | Illegal command coordinate | The specified absolute coordinate value was not reached. The coordinate value specified in the G50.9 command block or movement command is incorrect. |
| 5339 | Format error in a synchronous/mixed/superimposed control command issued by program | (1) The P, Q and L values specified in G51.4/G50.4/G51.5/G50.5/G51.6/G50.6 are invalid. (2) The value of parameter No. 12600 is duplicated. |
5346–5391: Cs Contour Control, Constant Surface Speed, Virtual Axis
| Code | Message | Meaning / action |
|---|---|---|
| 5346 | Return to the reference position | Coordinate establishment of the Cs contour control axis has not been performed. Perform a manual reference position return. Occurs when: (1) Cs axis coordinate establishment is executed while the Cs axis origin position established status signal CSPENx = 0; (2) the spindle amplifier is not transmitting position information; (3) the servo motor is off when Cs axis coordinate establishment starts; (4) the Cs axis is in synchronous or superimposed control state; (5) an emergency stop occurs during coordinate establishment; (6) an attempt is made to cancel mixed control of the Cs axis during coordinate establishment; (7) an attempt is made to start synchronous, mixed, or superimposed control of the Cs axis during coordinate establishment. |
| 5355 | S not specified in the G96 command | Surface speed S was not specified in the constant surface speed control command G96. Specify S in the G96 command block. |
| 5356 | A G code that cannot be commanded | A G code that cannot be specified in virtual axis command mode or real axis command mode was specified. |
| 5357 | Illegal axis specification | A real axis in the virtual plane was commanded in virtual command mode, or a virtual axis was commanded in real axis command mode. |
| 5359 | Mode switching error | Occurs when: (1) during automatic operation a mode change was attempted without using a non-buffered M code; (2) the mode was changed to virtual command mode while the reference point of at least one axis in the virtual plane was not established; (3) in virtual command mode the reference point of an axis in the virtual plane is no longer established; (4) the mode was changed during non-linear interpolation positioning (parameter LRP, No. 1401 #1 = 0); (5) the mode was changed in one of these modes — tool diameter compensation, tool length compensation, tool position offset, scaling, programmable mirror, coordinate rotation, fixed cycle; (6) the mode was changed while a real axis in the virtual plane was moving. |
| 5360 | Tool interference check error | This error occurs when changing G10 data input or file input data would cause interference with another tool, or when attempting to change the tool shape data of a tool already registered in the magazine. |
| 5361 | Magazine data inconsistency | Tools stored in the magazine interfere with each other. Re-register the tools in the magazine, or change the tool management data and tool shape data. When this alarm occurs, tool interference checking is not performed when registering tools in the magazine management table, and the empty magazine search function does not work correctly. When this alarm occurs, the power must be cycled once. |
| 5362 | Switch inch and mm at the origin | You attempted inch/metric unit switching at a position other than the reference point. Move to the reference point, then perform the inch/metric switch. |
| 5364 | Illegal command during program check | (1) A G code that cannot be executed in high-speed program check mode was specified. (2) Tilting axis control is enabled. (3) One of these was performed: high-precision oscillation operation in high-speed program check mode; starting high-speed program check mode during high-precision oscillation operation; reference position return of an axis whose reference point is not yet established in high-speed program check mode. (4) The PMC axis selection signal EAX* <G0136> was switched in high-speed program check mode. (5) G10 was specified for parameter PGR (No. 3454 #3) in high-speed program check mode. (6) G10 was specified for parameter PGS (No. 3001 #6) in high-speed program check mode. |
| 5365 | Program check mode cannot be switched | The high-speed program check input signal PGCK <Gn290.5> was switched while the program was running. |
| 5372 | Modal G code that cannot be executed (G53.2) | A G code other than G00 or G01 in group 01 was specified in a block specifying G53.2, or G53.2 was specified while a modal G code other than G00 or G01 in group 01 was in effect. |
| 5373 | Macro call argument conversion error | When resuming MDI program operation, the macro call argument in the program output could not be converted to 9 digits. |
| 5374 | Flexible synchronous mode mismatch | The current flexible synchronous mode does not match the flexible synchronous mode programmed in the program restart block. |
| 5375 | Flexible synchronous mode cannot be changed | The flexible synchronous mode changed while program operation was being resumed. |
| 5376 | Slave axis cannot be controlled | During flexible synchronization, a command was issued to the slave axis. |
| 5377 | Invalid command after flexible synchronous cancel | After flexible synchronous release, an incremental command was issued for the slave axis before an absolute command was issued. |
| 5378 | Invalid restart block specification | When specifying the block after flexible synchronous release as the restart block, the block after the absolute command for the slave axis was not specified. |
| 5379 | Writing to the slave axis is disabled | The slave axis parameter of feed axis synchronous control cannot be set directly. |
| 5381 | Command cannot be issued during flexible synchronous control | Occurs when: a G28 command was issued to the master axis while the reference point of the flexible synchronous control master axis was not yet established; or a G27/G28/G29/G30/G53 command was issued for the slave axis. |
| 5384 | Rigid retraction not possible | When returning from rigid tapping with a G30 command, the coordinate system mode at the time of the rigid tapping interruption differs from that at the time of the rigid tapping return. |
| 5391 | G92 command not possible | The workpiece coordinate system setting G92 (G50 for the lathe G code system A) cannot be commanded. Occurs when: (1) G92 was issued without an absolute value command after changing tool length compensation using the tool length compensation offset type; (2) G92 and G49 are in the same block. |
5406–5559: Tool Radius Compensation, Tilted Surface Machining, Option Authentication
| Code | Message | Meaning / action |
|---|---|---|
| 5406 | G41.3 / G40 format error | (1) A movement command is included in the G41.3 or G40 block. (2) A G code or M code that suppresses buffering is included in the G41.3 block. |
| 5435 | Parameter (TLAC) out of range | The parameter setting is incorrect (outside the setting value range). Check parameters No. 19655, 19656, 19657 and 1022. |
| 5436 | Rotary axis parameter setting error | The parameter setting is incorrect (rotary axis setting). |
| 5437 | Main rotary axis parameter setting error | The parameter setting is incorrect (main rotary axis setting). |
| 5445 | G39 cannot be used for movement control | The circular interpolation command for tool radius and cutting edge R compensation (G39) was specified together with a movement command rather than as an independent command. Correct the program. |
| 5446 | G41/G42 interference avoidance not possible | In the interference check avoidance function of tool diameter and cutting edge R compensation, interference cannot be avoided because there is no interference avoidance vector. |
| 5447 | G41/G42 interference avoidance is dangerous | The interference check avoidance function of tool diameter and cutting edge R compensation determined that performing the avoidance operation is dangerous. |
| 5448 | G41/G42 interference avoidance action | In the interference check avoidance function of tool diameter and cutting edge R compensation, further interference occurred with an already created interference avoidance vector. |
| 5456 | G68.2 issued again in G68.2 mode | The tilted surface machining command G68.2 was issued more than once. To perform a new coordinate conversion, cancel the current command first and then issue it again. |
| 5457 | G68.2 format error | G68.2 format error. |
| 5458 | Illegal use of G53.1/G53.6 | A G53.1/G53.6 command was issued before the G68.2 command; a G53.1/G53.6 command was not issued alone; the rotary axis controlling the tool axis direction in the +Z axis direction of the feature coordinate system has no angle solution; or no tool was specified in the G53.6 command. |
| 5459 | Machine configuration parameter incorrect | The machine configuration parameters (No. 19665 to 19667, No. 19680 to 19714 and No. 12321) are incorrect; the axis set in parameters No. 19681 and No. 19686 is not a rotary axis; three basic axes are not set in parameter No. 1022; or when the CNC searched for the rotary axis end point in a tilted surface machining command, that end point was outside the range specified in parameters No. 19741 to 19744. |
| 5462 | Illegal command (G68.2/G69) | (1) An error occurred when specifying G68.2/G69 mode. (2) A G code that cannot be specified in G68.2 mode was specified. (3) When specifying G68.2/G69, the offset vector of tool diameter and cutting edge R compensation was not canceled. |
| 5523 | Waiting for option authentication | The option setting status is “waiting for option authentication.” This alarm can be cleared by performing a reset operation as long as it is within the valid period (30 days after the alarm occurs). Contact the service center for authentication before the valid period expires. If authentication is not performed within the valid period, alarm PS5524 is triggered and this alarm can no longer be cleared by a reset. |
| 5524 | Waiting for option authentication (expired) | The authentication waiting period has expired. This alarm cannot be cleared by a reset operation. To cancel this alarm, contact the service center to request authentication. |
| 5557 | No maximum spindle speed clamp command | Before issuing the constant surface speed control command (G96 S_), the maximum spindle speed clamp command (M series: G92 S_; T series: G50 S_) was not issued. Issue the maximum spindle speed clamp command. |
| 5559 | Invalid axis movement command (coordinate system) | An axis movement command was issued when the workpiece coordinate system deviates from the machine coordinate system due to a movement command while machine lock is on. Perform an operation such as reference position return or workpiece coordinate system preset. This alarm is valid when parameter MSC (No. 11501, bit 2) = 1. |
How to Work With These Alarms
- Most codes in this range require an option. Flexible synchronous control (5242–5381), tilted surface machining G68.2 (5456–5462), tool center point control (5435–5459), and tool management (5312–5361) will not appear without the corresponding option installed.
- 5523 vs 5524 is a time-sensitive pair. 5523 can be cleared by a reset within 30 days; once expired it becomes 5524, which can only be cleared by contacting the service center for authentication. If you see 5523 on a newly enabled option, do not ignore it.
- 5361 (magazine data inconsistency) requires a power cycle. The alarm also disables tool interference checking and empty magazine search until the magazine tools are re-registered — do not keep running with it active.
- 5557 is a simple missing-command issue: G96 constant surface speed control requires a maximum spindle speed clamp (G92 S_ on M series, G50 S_ on T series) issued first. This is a genuine safety requirement, not a nuisance — without the clamp the spindle could overspeed.
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. What is the difference between FANUC alarm 5523 and 5524?
Both concern option authentication. Alarm 5523 means the option setting status is “waiting for option authentication” and it can still be cleared by performing a reset, as long as you are within the valid period of 30 days after the alarm first occurred. You should contact the service center for authentication before that period expires. If authentication is not completed in time, the alarm becomes PS5524, which cannot be cleared by a reset and requires contacting the service center to request authentication.
2. Why do I get alarm 5557 when using G96 constant surface speed control?
Because the maximum spindle speed clamp command was not issued first. Before issuing G96 S_, you must issue a maximum spindle speed clamp: G92 S_ on the M series, or G50 S_ on the T series. This is a genuine safety requirement rather than a formality — without the clamp, the spindle could run above its safe maximum as the workpiece diameter changes.
3. My machine shows alarm 5361, magazine data inconsistency. Can I keep running?
No, you should address it. When 5361 is active, tool interference checking is not performed when registering tools in the magazine management table, and the empty magazine search function does not work correctly, so the magazine data can no longer be trusted. Re-register the tools in the magazine or change the tool management data and tool shape data, and note that the power must be cycled once when this alarm occurs.
4. Which of these alarms apply without special options?
Relatively few. Codes that can appear on a standard machine include 5220 (reference position adjustment mode, parameter DATx No. 1819 #2 = 1), 5303 (touch panel not connected or failed to initialize), 5362 (inch/metric switching attempted away from the reference point), 5391 (G92/G50 issued without a preceding absolute command or together with G49), and 5557 (G96 without a spindle speed clamp). Most others — flexible synchronous control 5242–5381, tilted surface machining 5456–5462, tool center point control 5435–5459, and tool management 5312–5361 — require the corresponding option and will never appear without it.
© 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