FANUC Alarm Code List: P/S Alarms 0230–0461 Explained (Part 2)-CNCShare

This is Part 2 of the English reference for FANUC P/S (Program / Setting) alarm numbers, covering 0230–0461. Part 1 covers 0001–0224.

Each entry gives the alarm message and the practical meaning or first action on the floor. As with Part 1: the exact text on your screen is authoritative — messages, descriptions, and parameter numbers vary by FANUC series and software version. Confirm any parameter number on your machine before changing it.

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

0230–0233: Programmable Parameter Input and Helical Axis

Code	Message	Meaning / action
0230	Cutting depth R not specified	Cutting depth R was not specified in the G161 block, or the specified value of R is negative. Correct the program.
0231	G10 L52 format error	The command format is wrong when entering programmable parameters.
0232	Too many helical axes	Three or more axes were specified as helical axes using helical interpolation.
0233	Device is in use	When attempting to use a device such as RS-232-C, that device is being used by another user.

0245–0251: T Code and Tool Change

Code	Message	Meaning / action
0245	T code cannot be specified	A G code that cannot be specified in the same block as a T code was used (G50, G10, G04, G28, G28.2, G29, G30, G30.2, G53).
0247	Illegal data output code	The output code for an encrypted program defaults to EIA. Specify ISO as the output code.
0250	Invalid Z axis command for tool change	A Z axis movement command was issued in the same block as the M06 command.
0251	Illegal T code for tool change	A T code that cannot be used together with M06 T□□ was specified.

0300–0309: Scaling, Reference Position Return, Chamfering

Code	Message	Meaning / action
0300	Illegal command during scaling	A G code that cannot be executed during scaling was executed. Correct the program. On T-series machines this alarm is triggered if any of these are executed during scaling: finishing cycle (G70, G72), outer diameter roughing cycle (G71, G73), end face roughing cycle (G72, G74), closed loop cutting cycle (G73, G75), end face cutoff cycle (G74, G76), outer/inner diameter cutoff cycle (G75, G77), compound thread cutting cycle (G76, G78), end face drilling cycle (G83), end face tapping cycle (G84), end face boring cycle (G85), side drilling cycle (G87), side tapping cycle (G88), side boring cycle (G89), outer/inner diameter turning cycle (G77, G20), thread cutting cycle (G78, G21), face turning cycle (G79, G24). G codes are listed in B-system then C-system order.
0301	This setting prohibits resetting the reference position	A manual reference position return without a dog was attempted while parameter IDGx (No. 1012 #0), which prohibits resetting the reference position, is set to 1.
0302	Reference position return without a dog is not possible	The reference point cannot be set during reference position return because there is no dog. Possible causes: the axis was not moved in the reference position return direction by jog feed; the axis is moving in the direction opposite to the manual reference position return direction; or the position detector did not capture the one-turn signal, so the grid for manual reference position return was not established (diagnosis data No. 0201 #6 must be 1).
0303	Cannot return to the reference position	After enabling reference position setting at an arbitrary position for Cs contour control (parameter CRF, No. 3700 #0 = 1), a G00 command was issued to the Cs contour control axis after switching the serial spindle to Cs contour control mode, without first performing reference position return. Issue G28 to perform reference position return before issuing G00.
0304	G28 issued while the reference position is not established	An automatic reference position return (G28) command was issued while the reference position had not yet been established.
0305	Intermediate point of the reference position not specified	G29 (return from reference position) was executed directly after power-on without executing G28 (automatic reference position return) or G30 (2nd, 3rd, 4th reference position return).
0306	Illegal chamfering / corner R command	In the block specifying chamfering, the correspondence between the movement axis and the I, J and K commands is incorrect.
0307	Reference position setting cannot be started	You are attempting to execute a dog-type reference position setting on an axis that uses the dogless reference position setting function.
0308	G72.1 nesting error	A G72.1 command was issued again during G72.1 rotational copy.
0309	G72.2 nesting error	A G72.2 command was issued again during G72.2 parallel copy.

0310–0319: File Call, Direct Drawing Dimension Input, Threading and Cutoff Cycles

Code	Message	Meaning / action
0310	Specified file not found	In a subprogram/macro call, the specified file was not found.
0311	Invalid file name call format	The format for calling a subprogram/macro by file name is invalid.
0312	Error in direct drawing dimension input	The direct drawing dimension input command format is wrong. A G code that cannot be used for direct drawing dimension input was specified. There are two or more blocks without movement in consecutive direct drawing dimension input commands. A comma was specified in direct drawing dimension input when comma specification is not enabled (parameter CCR, No. 3405 #4 = 1).
0313	Out of range	In variable-lead thread cutting, the lead increase/decrease value specified at address K exceeds the maximum command value, or the command makes the lead negative.
0314	Polygon machining setting error	The axis setting for polygon machining is invalid. Polygon machining: the tool rotation axis is not specified (parameter No. 7610). Inter-spindle polygon machining: no valid spindle is set (parameters No. 7640 to 7643); a non-serial spindle was specified; or the spindle is not connected. When polygon machining and inter-spindle polygon machining are used together: parameter 7605 selecting the polygon machining type was changed while in polygon machining mode; or the spindle used for polygon machining overlaps with the one used for inter-spindle polygon machining.
0315	Invalid cutting edge angle in thread cutting cycle	The cutting edge angle is a value that cannot be used in the compound canned cycle thread cutting cycle (G76).
0316	Invalid minimum cutting depth in thread cutting cycle	The minimum cutting depth in the compound canned cycle thread cutting cycle (G76) is greater than the thread height.
0317	Invalid thread command in thread cutting cycle	In the compound canned cycle thread cutting cycle (G76), the thread height or cutting depth is 0 or negative.
0318	Invalid clearance amount in cutoff cycle	Although the escape direction in the compound canned cycle cutoff cycle (G74, G75) is fixed, delta d is negative.
0319	Invalid end point command in cutoff cycle	In the compound canned cycle cutoff cycle (G74, G75), the movement amount of delta i or delta k is 0 but U or W is not 0.

0320–0329: Compound Canned Cycles (G70–G76)

Code	Message	Meaning / action
0320	Invalid movement/cutting depth amount in cutoff cycle	In the compound canned cycle cutoff cycle (G74, G75), delta i or delta k (travel amount / cutting depth) is negative.
0321	Invalid number of repetitions in closed loop cycle	The number of repetitions in the compound canned cycle closed loop cycle (G73) is 0 or negative.
0322	End point shape beyond the start point	In the shape program of the compound canned cycle roughing cycle (G71, G72), a shape beyond the cycle start point was specified.
0323	First block of the geometry program is a type II command	In the compound fixed cycle roughing cycle (G71, G72), a type II instruction was specified in the first block of the shape program. For G71 it is a Z (W) instruction; for G72 it is an X (U) instruction.
0324	Interrupt macro executed during a compound cycle	An interrupt macro was executed during a compound fixed cycle (G70, G71, G72, G73).
0325	This command cannot be used in a geometry program	(1) An invalid instruction was specified in the shape program of a compound fixed cycle (G70, G71, G72, G73). (2) When cutting edge R compensation can be specified in the shape program of the turning compound fixed cycle finishing cycle (G70) (parameter NT2, No. 5106 #3 = 1), G41 or G42 was specified in a block other than the start block of the shape program.
0326	Last block of the shape program is a direct drawing dimension input command	The command in the last block of the compound canned cycle shape program (G70, G71, G72, G73) is in the middle of a direct drawing dimension input command.
0327	Modal of the compound cycle cannot be controlled	A compound canned cycle (G70, G71, G72, G73) was issued in a modal state where commands cannot be issued.
0328	Illegal material side specification for cutting edge R compensation	The material side specification of cutting edge R compensation (G41, G42) does not apply to the material side of the compound canned cycle (G71, G72).
0329	Final shape is not monotonic (plane second axis)	In the shape program of the compound canned cycle roughing cycle (G71, G72), the command for the plane second axis is not monotonically increasing or decreasing.

0330–0337: Single Canned Cycles, Offsets, Misoperation Prevention

Code	Message	Meaning / action
0330	Invalid axis command in a single cycle	In a single type canned cycle (G90, G92, G94), an axis other than the plane was specified.
0331	Illegal axis number in AX[]	An invalid value was specified for the axis number in AX[ ].
0332	Illegal axis address in AXNUM[]	An invalid axis address was specified in AXNUM[ ].
0334	Outside the valid setting range	Offset data outside the valid setting range was specified (misoperation prevention function).
0335	Multiple M codes specified	In the M code queueing function with peripheral equipment, a command for another M code is issued at the same time in the queued M code block.
0336	Tool length compensation specified for two or more axes	An attempt was made to apply an offset to another axis without canceling that offset with tool length compensation C. Or multiple axes were specified in a G43/G44 block while tool length compensation C was in use.
0337	Maximum increment exceeded	The command value exceeds the maximum increment. (Misoperation prevention function)

0340–0349: Nano Smoothing and Tool Exchange

Code	Message	Meaning / action
0340	Nano smoothing operation restart error	An attempt was made to resume operation with nano smoothing after manual intervention with manual absolute mode enabled.
0341	Block count limit for continuous commands exceeded (nano smoothing)	The number of blocks that can be controlled continuously in nano smoothing mode has exceeded the limit.
0342	Custom macro interrupt and nano smoothing enabled	A custom macro interrupt was enabled in nano smoothing mode, or nano smoothing mode was commanded while a custom macro interrupt was enabled.
0343	Invalid nano smoothing command	G43, G44 and G49 commands were used during nano smoothing.
0344	Nano smoothing cannot continue	An instruction or operation was executed that makes nano smoothing unable to continue.
0345	Z axis position incorrect at tool exchange	The Z axis position is incorrect at tool exchange.
0346	Invalid tool number at tool exchange	The tool exchange tool position has not been established.
0347	Illegal simultaneous tool exchange command	Illegal simultaneous tool exchange command.
0348	Tool exchange Z axis position not established	The tool exchange Z axis position has not been established.
0349	Tool exchange spindle stop not completed	Tool exchange spindle stop has not been completed.

0350–0359: Synchronous Control and Mixed Control

Code	Message	Meaning / action
0350	Synchronous control axis number parameter setting error	The synchronous control axis number (parameter No. 8180) setting is invalid.
0351	Control cannot be started/canceled because the controlled axis is moving	An attempt was made to start or cancel synchronous control using the synchronous control axis selection signal while the synchronous control target axis was moving.
0352	Synchronous control axis configuration error	Occurs when: (1) attempting synchronous control on an axis that is already synchronized, mixed, or superimposed; (2) attempting to synchronize a descendant in a parent-child relationship; (3) using a setting where no parent-child relationship is established.
0353	Movement command issued to an axis that cannot execute it	Synchronous case: a movement command was issued to an axis with parameter NUMx (No. 8163 #7) = 1, or to a slave axis. Mixed case: a movement command was issued to an axis with parameter NUMx (No. 8163 #7) = 1, or with parameter MUMx (No. 8162 #7) = 1.
0354	Automatic reference position return issued while reference position not established during synchronous control	Occurs when G28 is issued to the master axis at its parked position during synchronous control while the slave axis reference position has not been established.
0355	Mixed control axis number parameter setting error	The mixed control axis number (parameter No. 8183) setting is invalid.
0356	Control cannot be started/canceled because the mixed control target axis is moving	An attempt was made to start or cancel mixed control using the mixed control axis selection signal while the mixed control target axis was moving.
0357	Mixed control axis configuration error	Occurs when attempting mixed control on an axis that is already in a synchronous, mixed, or superimposed state.
0359	Automatic reference position return issued while reference position not established during mixed control	Occurs when G28 is issued to the mixed axis during mixed control while the reference position of the mixed partner has not been established.

0360–0369: Superimposed Control and Tool Compensation

Code	Message	Meaning / action
0360	Superimposed control axis number parameter setting error	The superimposed control axis number (parameter No. 8186) setting is invalid.
0361	Control cannot be started/canceled because the superimposed axis is moving	An attempt was made to start or cancel superimposed control using the superimposed control axis selection signal while the superimposed control target axis was moving.
0362	Superimposed control axis configuration error	Occurs when: (1) attempting superimposed control on an axis that is already synchronized, mixed, or superimposed; (2) attempting to synchronize a great-grandchild in a parent-child relationship.
0363	Automatic reference position return (G28, G30) issued to a superimposed control slave axis	Occurs when G28 is issued to a superimposed control slave axis during superimposed control.
0364	Machine coordinate system selection (G53) issued to a superimposed control slave axis	Occurs when G53 is issued to the slave axis while the master axis is moving during superimposed control.
0365	Maximum number of SV/SP axes in the system exceeded	The number of controlled axes or controlled spindles usable in a single system has exceeded the maximum. (For a loader system, this alarm occurs if the number of axes per system is set to 5 or more.)
0366	A G code that cannot be used with the turret system was specified	G43 and G43.7 were issued while the turret tool change method is selected (parameter TCT, No. 5040 #3 = 0).
0367	3D coordinate conversion issued during synchronous control with parameter PKUx (No. 8162 #2) = 0	A 3D coordinate conversion command was issued during synchronous control while parameter PKUx (No. 8162 #2) is set to 0.
0368	Tool compensation not canceled	With the automatic tool change method selected (parameter TCT, No. 5040 #3 = 1), G43.7 was issued in G43 mode, or G43 was issued in G43.7 mode. Or a tool compensation command was issued after changing parameter TCT (No. 5040 #3) while tool compensation still remained.
0369	G31 format error	In a torque limit skip command (G31 P98/P99), no axis was specified or two or more axes were specified. In the torque limit skip command, the command value at address Q is out of range; the command range for address Q is 1 to 254. Or the continuous high-speed skip option is not present.

0370–0376: Skip Functions, Tilting Axis Control

Code	Message	Meaning / action
0370	Illegal G31 P / G04 Q	(1) The command value at address P in G31 is out of range; with the multi-step skip function enabled, the range for address P is 1 to 4. (2) The command value at address Q in G04 is out of range; with the multi-step skip function enabled, the range for address Q is 1 to 4. (3) Commands were sent to P1–4 with G31 and Q1–4 with G04 even though the multi-step skip function is not enabled. (4) T system: the command value at address P in G72 or G74 is out of range; with the multi-step skip function enabled, the range for address P is 1 to 4, or commands were sent to P1–4 with G72 or G74 even though the function is not enabled.
0371	G10 L50 format error	In the programmable parameter input command format, an attempt was made to change the encryption parameter (No. 3220), key parameter (No. 3221), or protection range parameters (No. 3222, 3223) of the “key and program encryption function.” Correct the program.
0372	Cannot return to the reference position	During manual reference position return with tilting axis control, or during automatic reference position return when no reference position return has been performed since power-on, the system attempted orthogonal axis reference position return before tilting axis reference position return completed. Perform tilting axis reference position return first, then orthogonal axis reference position return.
0373	High-speed skip signal selection error	For each skip command (G31, G31 P1 to G31 P4) and dwell command (G04, G04 Q1 to G04 Q4), different systems selected the same high-speed skip signal.
0374	Tool management data registration error (G10)	G10 L75/L76 data registration was executed while one of these was in progress: data registration from the PMC window, data registration from FOCAS2, or data registration by G10 L75/L76 in another system. After finishing the above, command G10 L75/L76 again.
0375	Tilting axis control not possible (synchronous / mixed / superimposed)	This axis configuration does not permit tilting axis control. Occurs when: (1) not all axes related to tilting axis control are in synchronous control mode, or the tilting axis is not synchronized with the tilting axis and the orthogonal axis is not synchronized with the orthogonal axis; (2) not all axes related to tilting axis control are in mixed control mode, or the tilting axis is not mixed with the tilting axis and the orthogonal axis is not mixed with the orthogonal axis; (3) an axis related to tilting axis control is in superimposed control mode.
0376	Scale with reference origin: invalid parameter	(1) Parameter 2002 #3 is disabled while parameter 1815 #1 (OPTx) for the independent pulse coder is enabled. (2) Parameter 1815 #5 (APCx) for the absolute position detector is enabled.

0387–0399: DI/DO Variables and Real-Time Custom Macros

Code	Message	Meaning / action
0387	Illegal DI/DO variable specification	A DI/DO variable with the specified signal address (letter, number) does not exist.
0389	Illegal bit specification for a DI/DO variable	A DI/DO signal cannot specify a bit other than 0 to 7.
0390	Unsupported macro variable	An unsupported macro variable was used in a real-time custom macro.
0391	Number of branches in the control range exceeded	The number of branches supported by the real-time custom macro has been exceeded.
0392	Multiple control methods used	Many reserved words that control the RTM (ZONCE, ZEDGE, ZWHILE, ZDO, ZEND, G65, M99) were used in a real-time macro command.
0393	No data to assign	There is no data to be replaced in the real-time macro command.
0394	Relationship between controllers is incorrect	The reserved words that control the RTM (ZONCE, ZEDGE, ZWHILE, ZDO, ZEND, G65, M99) are not correctly supported.
0395	G65 or M99 written incorrectly	The command for subprogram call or return control, G65 or M99, is written incorrectly.
0396	RTM control written outside the RTM	You are using a reserved word that controls the RTM (ZONCE, ZEDGE, ZWHILE, ZDO, ZEND) outside a real-time macro instruction.
0397	RTM usable buffer full	There is not enough space in the buffer for the real-time macro instruction. There are too many look-ahead blocks triggered by buffered real-time macro instructions.
0398	ID exceeded	There are too many real-time macro commands with the same ID in the look-ahead blocks.
0399	The same ID is started simultaneously	An attempt was made to execute real-time macro commands with the same ID using the same NC statement as a trigger.

0400–0409: Real-Time Macro Execution

Code	Message	Meaning / action
0400	Number of single instructions exceeded the limit	There are too many one-shot real-time macro commands.
0401	Number of simultaneously executed programs exceeded	The number of real-time macro commands executed simultaneously has exceeded the limit.
0402	An unsupported token was used	An unsupported token, variable, or function was detected in a real-time custom macro.
0403	Access to a protected variable	An attempt was made to access a protected variable.
0404	Real-time macro command error	An error occurred in a real-time macro command.
0406	Code space exceeded	The memory capacity of the real-time macro area is insufficient.
0407	Do not use // during an RTM command	An attempt was made to enter compile mode again while already in compile mode.
0408	Absolute command not possible	The absolute command is not available.
0409	Invalid axis number	The axis number is invalid.

0410–0429: G28, Axis Groups, G10.6 Retraction

Code	Message	Meaning / action
0410	Midpoint of G28 is not 0	The center point specified by G28 is not 0.
0411	Number of simultaneously controlled axes exceeded maximum	The number of simultaneously controlled axes has exceeded the maximum.
0412	An invalid G code was used	An invalid G code was used.
0413	Invalid address used	An invalid address was used.
0415	Group of the specified axis is in use	The group to which the specified axis belongs is in use.
0416	Specified axis cannot be used	The specified axis cannot be used.
0417	Specified axis is in an inoperable state	The specified axis is in an inoperable state.
0418	Feedrate setting is incorrect	The feedrate setting is incorrect.
0419	Movement data out of range	The movement data is out of range.
0420	Subprogram not specified with a constant	The subprogram was not specified with a constant.
0421	Invalid argument used in G65	An invalid argument L was used in G65.
0422	Invalid argument used in G65	An invalid argument was used in G65.
0424	A group is used on multiple axes	It uses one group on multiple axes.
0429	G10.6 command error	When starting retraction in a thread cutting block, the retraction command was issued along the thread cutting long axis direction.

0430–0461: Tool Life Management, Tool Axis Direction, Spindle Control, Torch

Code	Message	Meaning / action
0430	Tool life management: zero setting	The tool life management number parameter (No. 6813) is set to 0.
0431	Invalid tool life T/R data	The optional group number (T) or the remaining amount setting value (R) is invalid.
0438	Parameter error when correcting tool direction	The parameters are incorrect. When executing tool center point holding type tool axis direction control (G53.6), the acceleration/deceleration function before interpolation is disabled: set parameter No. 1660. The acceleration/deceleration function before interpolation for rapid traverse is disabled: set parameters No. 1401 #1, No. 19501 #5, No. 1671. The parameters configuring the machine (No. 19680 to 19714) are incorrect. The axis set in parameters No. 19681, No. 19686 is not a rotary axis. Three basic axes are not set in parameter No. 1022.
0445	Invalid axis movement command	A positioning command was issued in rotation control mode. Check the SV rotation control mode signal.
0446	Not an independent block	G96.1, G96.2, G96.3 and G96.4 are in the same block as other commands. Correct the program.
0447	Configuration error	The rotary tool axis setting is incorrect. Check the parameters of the servo motor spindle control function.
0451	Invalid auxiliary function table command	When attempting to output an M code in the auxiliary function table, the PMC ladder sequence does not execute the completion process for the previous M code.
0455	Error in canned grinding cycle command	In the preset grinding cycle: (1) M system: the signs of the I, J and K commands do not match. (2) M system / T system: the movement amount of the grinding axis is not specified.
0456	Incorrect parameter setting for canned grinding cycle	There is an error in the parameter settings related to the grinding cycle. Possible causes: (1) the axis number setting for the grinding axis (parameters No. 5176 to 5179) is wrong on the M/T system; (2) the axis number setting for the dressing axis (parameters No. 5180 to 5183) is wrong on the M/T system; (3) the axis numbers of the cutting axis, grinding axis and dressing axis overlap (M system only).
0459	All axes parked	All axes currently controlled by automatic operation are in parked mode.
0460	Invalid torch control axis number	The axis value set in parameter 5490 (torch control axis) exceeds the number of controlled axes.
0461	Rotary axis setting of the torch rotation axis is incorrect	The torch rotation axis is not set as a rotary axis (parameter No. 1006 #0 = 1).

How to Work With These Alarms

Confirm the exact message on your screen. Many of these codes are option-dependent — a code such as 0350 or 0460 only appears when the corresponding control option is installed.
Separate program errors from configuration errors. Codes in the 0310–0329 and 0410–0429 ranges are usually program or modal-state problems; codes in the 0350–0376 range usually point to axis configuration (synchronous / mixed / superimposed) or parameter settings.
Do not cancel a synchronous/mixed control alarm by changing parameters blindly. For 0352, 0357 and 0362 the root cause is almost always an axis already being in another control mode — check the control state before editing axis number parameters.
Back up parameters first. Several of these alarms (0376, 0438, 0456) are resolved by correcting parameter settings, and a wrong parameter can affect machine motion.

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 some FANUC alarm numbers appear on my machine but not in this list, or vice versa?

Because P/S alarm coverage depends on the FANUC series, software version, and which options are installed. For example, alarms in the 0350–0376 range relate to synchronous, mixed and superimposed axis control, and the 0460–0461 range relates to torch control — these only exist when the corresponding option is present. The alarm text on your screen is always authoritative over any published list.

2. What causes alarm 0301 and 0302 on reference position return?

Both relate to how the machine establishes its reference position. Alarm 0301 means a manual reference position return without a dog was attempted while parameter IDGx (No. 1012 #0), which prohibits resetting the reference position, is set to 1. Alarm 0302 means the return without a dog could not complete: the axis was not moved in the return direction by jog feed, the axis is moving opposite to the manual return direction, or the position detector did not capture the one-turn signal so the grid was not established — diagnosis data No. 0201 #6 must be 1.

3. Alarm 0352 / 0357 / 0362 — what is an axis configuration error?

These mean the axis you are trying to place into synchronous, mixed, or superimposed control is already in one of those control modes, or the parent-child axis relationship is not valid. The fix is to check the current control state of the axis and release the existing control first, rather than changing the axis number parameters (No. 8180, 8183, 8186). Only if the parameter value itself is out of range do alarms 0350, 0355 and 0360 apply.

4. I get alarms in the 0320–0329 range on canned cycles. Where do I start?

These almost always point at the shape program of a compound canned cycle (G70–G76), not at the parameters. Check whether the shape program’s first block is a type II command (0323), whether the end point shape goes beyond the cycle start point (0322), whether the plane second axis shape is monotonic (0329), and whether the cutoff cycle travel or depth values are negative where they should not be (0318–0320). Correcting the shape program resolves most of them.