The P/S (Program / Syntax) alarms that appear on FANUC control screens are most often caused by a typo in the program, a missing address, or a command sequence the control did not expect. This page collects the P/S alarm codes that are not yet covered on Mentor CNC’s other pages (the FANUC 0/00/0-Mate guide, the G71/G72/G74/G75 cycle pages, and CNC Milling Lesson 9).
General Programming and Syntax Errors
P/S 001 — ADDRESS NOT FOUND
Machine type: Lathe and machining center (general programming error)
Meaning: No numeric value was entered after an address (e.g. X, Y, Z); another address or end of block followed instead.
Example of incorrect use: `X Y100` (no value after X)
Solution: Always write a valid number after every address. Example: `X100 Y100`
P/S 003 — TH PARITY ALARM (Tezgâh Tipi: Özellikle veri aktarımı yapılan tüm tezgâhlar)
Machine type: Lathe and machining center — usually occurs when reading a program via RS232 or a memory card.
Meaning: A bit with incorrect parity was detected during reading. There may be noise or a cable problem on the data communication line.
Solution:
- Check the data transfer cables and connections.
- Verify the I/O parameters (stop bit, baud rate) against the machine manual.
- Reload the program. If the problem persists, the computer or the card interface may be faulty.
P/S 004 — TV PARITY ALARM
Machine type: Lathe and machining center (when TV control is active)
Meaning: The number of characters in a block was odd, triggering a TV (vertical) parity check error. This alarm only occurs when TV parity check is enabled.
Solution:
- You can disable TV control via a parameter.
- Or add a space to the block to make the character count even.
P/S 005 — TOO MANY DIGITS
Machine type: Lathe and machining center
Meaning: More digits were entered for an address than the maximum allowed. (e.g. X1234567890)
Solution: Make sure the value is within the valid range (generally no more than 8 digits).
P/S 006 — ILLEGAL USE OF NEGATIVE SIGN
Machine type: Lathe and machining center
Meaning: The "-" sign was used incorrectly — a second "-" after an address, or a "-" without an address.
Example of incorrect use: `X- -100`
Solution: Use only one "-" sign per address, and make sure it comes before the number.
P/S 007 — ILLEGAL USE OF DECIMAL POINT
Machine type: Lathe and machining center
Meaning: A decimal point (".") was used where it should not be (e.g. immediately after an address).
Solution: Use the decimal point only within a numeric value, not right after the address.
P/S 008 — PROGRAM HAS AN ERROR AT THE END
Machine type: Lathe and machining center
Meaning: The program was not terminated with `M02`, `M30` or `M99`; only a `%` was used to end it.
Solution: Add the correct end code to the end of the program: `M30` for the main program, `M99` for a subprogram.
P/S 009 — ILLEGAL ADRESS INPUT
Machine type: Lathe and machining center
Meaning: An invalid character (address) was used — for example `@` or `#`.
Solution: Use only valid addresses (X, Y, Z, G, M, F, S, T, etc.).
P/S 011 — NO FEEDRATE COMMANDED
Machine type: Lathe and machining center
Meaning: No F (feedrate) value was entered in a cutting move block.
Solution: Always define an F value in every `G01`, `G02`, `G03`, etc. block.
P/S 014 — ILLEGAL LEAD COMMAND
Machine type: Lathe (variable-lead threading)
Meaning: In a variable-lead thread (G34) command, the lead increase/decrease given by the K address exceeded the maximum value or was negative.
Solution: Check the K value; make sure it is positive and within the allowed limits.
P/S 015 — TOO MANY AXES COMMANDED
Machine type: Machining center (multi-axis)
Meaning: More axes were commanded than can be controlled simultaneously.
Solution: Do not specify more axes than necessary in the same block; check the machine's axis capacity.
Circular Interpolation and Plane Selection Errors
P/S 020 — OVER TOLERANCE OF RADIUS
Machine type: Lathe and machining center (circular interpolation)
Meaning: While drawing an arc with `G02/G03`, the difference between the distance from the start point to the arc center and the distance to the end point exceeded the tolerance set in parameter 0876.
Solution: Check the start, end and center coordinates in the program, or increase the 0876 tolerance (with caution).
P/S 021 — ILLEGAL PLANE AXIS COMMANDED
Machine type: Lathe and machining center
Meaning: During circular interpolation, an axis not belonging to the selected plane (G17/G18/G19) was commanded.
Solution: Make sure the correct plane is selected before a circular move.
P/S 023 — ILLEGAL RADIUS COMMAND
Machine type: Lathe and machining center
Meaning: A negative radius value was entered while drawing an arc with R.
Solution: The R value must be positive.
P/S 028 — ILLEGAL PLANE SELECT
Machine type: Lathe and machining center
Meaning: Two or more axes were incorrectly specified at the same time during plane selection (G17/G18/G19).
Solution: Check the correct plane selection.
Tool Offset and Tool Radius Compensation (CRC) Errors
P/S 029 — ILLEGAL OFFSET VALUE
Machine type: Lathe and machining center (tool offset)
Meaning: The offset value specified with a T code is too large.
Solution: Check the offset values and make sure they are within the valid range.
P/S 030 — ILLEGAL OFFSET NUMBER
Machine type: Lathe and machining center
Meaning: The offset number specified in the T function is outside the valid range.
Solution: Check the T number (e.g. T0101, offset 01).
P/S 031 — ILLEGAL P COMMAND IN G10
Machine type: Lathe and machining center
Meaning: While setting an offset with `G10`, the offset number following the P address is invalid or too large.
Solution: Check the P value.
P/S 032 — ILLEGAL OFFSET VALUE IN G10
Machine type: Lathe and machining center
Meaning: While writing an offset with `G10` or system variables, the amount is too large.
Solution: Enter the offset amount within the limits.
P/S 033 — NO SOLUTION AT CRC
Machine type: Lathe and machining center (tool nose radius compensation)
Meaning: During tool nose radius compensation (G41/G42), the intersection point could not be calculated.
Solution: Review the move geometry in the program; there may be insufficient clearance or corners that are too tight.
P/S 034 — NO CIRC ALLOWED IN ST-UP/EXT BLK
Machine type: Lathe and machining center
Meaning: In tool radius compensation mode, a `G02/G03` circular move cannot be used in the start-up or cancel block.
Solution: Use a linear (G01) move before or after G41/G42.
P/S 035 — CAN NOT COMMANDED G31
Machine type: Lathe and machining center
Meaning: G31 (skip cutting) was commanded while in tool radius compensation mode.
Solution: Do not use G31 while G41/G42 is active.
P/S 036 — INTERFERENCE IN CIRCULAR BLOCK
Machine type: Lathe and machining center
Meaning: During tool radius compensation, an arc block would cause excessive cutting — there is interference with the arc center.
Solution: Recalculate the arc coordinates in the program.
P/S 037 — CAN NOT CHANGE PLANE IN CRC
Machine type: Lathe and machining center
Meaning: The plane cannot be changed while tool radius compensation is active.
Solution: Cancel compensation with G40 before changing the plane.
P/S 039 — CHC/CNR NOT ALLOWED IN CRC
Machine type: Lathe and machining center
Meaning: Chamfering or corner-R (C/R) cannot be used in the compensation start-up/cancel block. It can cause excessive cutting.
Solution: Perform the chamfer before or after the compensation mode, not inside it.
P/S 040 — INTERFERENCE IN G90/G94 BLOCK
Machine type: Lathe (canned cycles)
Meaning: In G90/G94 canned cycles, tool radius compensation would cause excessive cutting.
Solution: Turn off compensation with G40 before the cycle, or adjust the program coordinates.
P/S 041 — INTERFERENCE IN CRC
Machine type: Lathe and machining center
Meaning: A general excessive-cutting condition in tool radius compensation.
Solution: Check the program geometry and the tool offset.
Reference Point Return Errors
P/S 046 — ILLEGAL REFERENCE RETURN COMMAND
Machine type: Lathe and machining center
Meaning: With `G28`, a P value other than P2, P3 or P4 was entered for returning to the 2nd, 3rd or 4th reference point.
Solution: Use only P2/P3/P4, or write G28 without a P.
P/S 090 — REFERENCE RETURN INCOMPLETE
Machine type: Lathe and machining center
Meaning: The return to reference point could not be completed — the starting point is too close to the reference, or the speed is too low.
Solution: Move the axis away from the reference point and perform the return at an adequate (rapid) speed.
P/S 091 — MANUAL RETURN TO REFERENCE POSITION IS IMPOSSIBLE
Machine type: Lathe and machining center
Meaning: Manual return to reference cannot be performed because the system is temporarily in a stop state.
Solution: Press RESET, then manually go to the reference point.
P/S 092 — AXES NOT ON THE REFERENCE
Machine type: Lathe and machining center
Meaning: The axis specified by a G28 (automatic reference return) or G27 (reference check) command did not reach the reference position.
Solution: Manually move the axis to the reference position and try again.
Chamfer, Corner-R and Direct Dimension Programming Errors
P/S 050 — CHF/CNR NOT ALLOWED IN THRD BLK
Machine type: Lathe (threading)
Meaning: A chamfer (C) or corner-R command was entered in a threading block.
Solution: Do not add these commands to a threading block.
P/S 051 — MISSING MOVE AFTER CHF/CNR
Machine type: Lathe and machining center
Meaning: The block following a chamfer or corner-R block has insufficient or unsuitable movement.
Solution: Add at least one linear move block after the chamfer.
P/S 052 — CODE IS NOT G01 AFTER CHF/CNR
Machine type: Lathe and machining center
Meaning: The block immediately following a chamfer or corner-R block is not linear (G01).
Solution: The move after a chamfer must be G01.
P/S 053 — TOO MANY ADDRESS COMMAND
Machine type: Lathe and machining center
Meaning: Two or more of I, K, R were specified in a chamfer block, or in direct dimension programming a character other than C/R follows the comma.
Solution: Use only the required address.
P/S 054 — NO TAPER ALLOWED AFTER CHF/CNR
Machine type: Lathe
Meaning: A chamfer or corner-R block contains a taper command.
Solution: Do not use a taper in a chamfer block.
P/S 055 — MISSING MOVE VALUE IN CHF/CNR
Machine type: Lathe and machining center
Meaning: The chamfer or corner-R amount is larger than the move distance in the block.
Solution: Increase the move distance or reduce the chamfer amount.
P/S 056 — NO END POINT & ANGLE IN CHF/CNR
Machine type: Lathe and machining center
Meaning: Only an angle (A) was specified in a chamfer block; the end point is missing.
Solution: Also enter an X or Z value.
P/S 057 — NO SOLUTION OF BLOCK END
Machine type: Lathe (direct drawing dimension programming)
Meaning: The block end could not be calculated in direct drawing programming.
Solution: Check the given angle and distance combination.
P/S 058 — END POINT NOT FOUND
Machine type: Lathe (direct drawing dimension programming)
Meaning: The block end point could not be found.
Solution: Review the coordinate and angle values again.
Program Number, Sequence Number and Memory Management Errors
P/S 059 — PROGRAM NUMBER NOT FOUND
Machine type: Lathe and machining center
Meaning: While searching for an external program number, the specified program could not be found in memory.
Solution: Verify the program number and make sure the program is loaded.
P/S 060 — SEQUENCE NUMBER NOT FOUND
Machine type: Lathe and machining center
Meaning: The N number specified in a sequence number search could not be found.
Solution: Check the N number.
P/S 063 — SEQUENCE NUMBER NOT FOUND
Machine type: Lathe (G70-G73)
Meaning: The sequence number specified in the P address could not be found.
Solution: Make sure the N number given with P exists in the program.
P/S 070 — NO PROGRAM SPACE IN MEMORY
Machine type: Lathe and machining center
Meaning: There is not enough space in memory.
Solution: Delete unneeded programs or work via DNC.
P/S 071 — DATA NOT FOUND
Machine type: Lathe and machining center
Meaning: The searched-for address or program number could not be found.
Solution: Check the value you entered.
P/S 072 — TOO MANY PROGRAMS
Machine type: Lathe and machining center
Meaning: The number of programs in memory exceeded the maximum limit (standard 63, option 125/200).
Solution: Delete unneeded programs.
P/S 073 — PROGRAM NUMBER ALREADY IN USE
Machine type: Lathe and machining center
Meaning: The program number you entered already belongs to another program.
Solution: Use a different number, or delete the old program.
P/S 074 — PROGRAM NUMBER
Machine type: Lathe and machining center
Meaning: The program number is outside the 1-9999 range.
Solution: Enter a valid number.
P/S 076 — ADDRESS P NOT DEFINED
Machine type: Lathe and machining center
Meaning: The P address is missing in a subprogram call with M98, G65 or G66.
Solution: Specify the program number to be called with P.
P/S 077 — SUB PROGRAM NESTING ERROR
Machine type: Lathe and machining center
Meaning: The subprogram nesting limit was exceeded (usually 8 levels).
Solution: Reduce the number of nested subprograms.
P/S 078 — NUMBER NOT FOUND
Machine type: Lathe and machining center
Meaning: The program/sequence number specified with M98/M99/G65/G66 or GOTO could not be found.
Solution: Check the target number and make sure the program has not been edited.
P/S 079 — PROGRAM VERIFY ERROR
Machine type: Lathe and machining center
Meaning: The program in memory does not match the program read from the external device.
Solution: Check both the program in memory and the source program, then reload.
Automatic Tool Offset Measurement (G37) Errors
P/S 080 — G37 ARRIVAL SIGNAL NOT ASSERTED
Machine type: Lathe and machining center (automatic tool measurement)
Meaning: During G37 (automatic tool compensation), no signal arrived within the specified area.
Solution: Check the tool measurement probe and the parameter settings.
P/S 081 — OFFSET NUMBER NOT FOUND IN G37
Machine type: Lathe and machining center
Meaning: No T code was specified while performing automatic compensation with G36/G37.
Solution: Give the T code in the same block or before it.
P/S 082 — T-CODE NOT ALLOWED IN G37
Machine type: Lathe and machining center
Meaning: A T code cannot be used in the same block as G36/G37.
Solution: Write the T code in a separate block.
P/S 083 — AXIS COMMAND IN G37
Machine type: Lathe and machining center
Meaning: The G36/G37 block contains an invalid axis command, or an incremental command was used.
Solution: Use absolute (G90) coordinates and specify valid axes.
Data Communication and DNC Errors
P/S 085 — COMMUNICATION ERROR
Machine type: Lathe and machining center (RS232 transfer)
Meaning: An overrun, parity or framing error occurred during data input via the reader/punch interface.
Solution: Check the cable, baud rate and stop bit settings.
P/S 086 — DR SIGNAL OFF
Machine type: Lathe and machining center
Meaning: The I/O device's ready (DR) signal turned off during data transfer.
Solution: Check the device's power, the cable and the PCB.
P/S 087 — BUFFER OVERFLOW
Machine type: Lathe and machining center
Meaning: A buffer overflow occurred during data transfer — 10 characters were read despite the end-of-read command.
Solution: The I/O device or PCB may be faulty; call for service.
P/S 180 — COMMUNICATION ERROR (REMOTE BUF)
Machine type: Lathe and machining center
Meaning: A remote buffer connection error.
Solution: Check the cable, parameters and I/O unit.
Coordinate System and P-Type Command Errors
P/S 094 — P TYPE NOT ALLOWED (COORD CHG)
Machine type: Lathe and machining center (program restart)
Meaning: A P type cannot be specified during program restart after a coordinate system change.
Solution: Follow the correct restart procedure.
P/S 095 — P TYPE NOT ALLOWED (EXT OFS CHG)
Machine type: Lathe and machining center
Meaning: A P type cannot be used during program restart if the external workpiece offset was changed.
Solution: Perform the restart procedure according to the operator's manual.
P/S 097 — P TYPE NOT ALLOWED (AUTO EXEC)
Machine type: Lathe and machining center
Meaning: A P type is invalid on restart after power-on or an emergency stop.
Solution: Start automatic operation and perform the restart procedure in the correct order.
P/S 098 — G28 FOUND IN SEQUENCE RETURN
Machine type: Lathe and machining center
Meaning: A G28 was found during the search on a restart command after power-on/emergency stop.
Solution: Perform a reference return before the restart procedure.
P/S 099 — MDI EXEC NOT ALLOWED AFTER SEARCH
Machine type: Lathe and machining center
Meaning: An MDI move command cannot be given after a program restart search has completed.
Solution: Run the program in automatic mode instead of using MDI.
Parameter Write Enable and Memory Clear
P/S 100 — PARAMETER WRITE ENABLE
Machine type: Lathe and machining center
Meaning: PWE (Parameter Write Enable) was turned on (PWE=1).
Solution: After finishing the parameter changes, set PWE back to 0 and reset the system. The alarm is persistent and will not clear until PWE is set to 0.
P/S 101 — PLEASE CLEAR MEMORY
Machine type: Lathe and machining center
Meaning: Power was cut while a program was being edited.
Solution: Set PWE=1, hold down DELETE while powering on, and clear memory (all programs will be deleted — restore from backup if you have one).
Macro Programming and Variable Errors
P/S 109 — P/S ALARM (G08 P değeri hatalı)
Machine type: Lathe and machining center
Meaning: In G08, a value other than 0 or 1 was written after P, or nothing was written at all.
Solution: Use G08 P1 (feed-forward mode) or G08 P0.
P/S 110 — DATA OVERFLOW
Machine type: Lathe and machining center
Meaning: A value on the fixed decimal-point display exceeded the allowed limit.
Solution: Reduce the value to within the valid range.
P/S 111 — CALCULATED DATA OVERFLOW
Machine type: Lathe and machining center (macro)
Meaning: The result of a macro calculation is invalid (too large or too small).
Solution: Check the variables used in the calculation.
P/S 112 — DIVIDED BY ZERO
Machine type: Lathe and machining center (macro)
Meaning: A division by zero occurred, or an invalid trigonometric operation such as tan 90°.
Solution: Make sure the denominator is not zero.
P/S 113 — IMPROPER COMMAND
Machine type: Lathe and machining center (macro)
Meaning: A function that cannot be used in a custom macro was commanded.
Solution: Use macro commands correctly.
P/S 114 — FORMAT ERROR IN MACRO
Machine type: Lathe and machining center
Meaning: An undefined H code or a format error in an expression occurred in a G25 block.
Solution: Check the macro format.
P/S 115 — ILLEGAL VARIABLE NUMBER
Machine type: Lathe and machining center
Meaning: An undefined variable number was used, or the canned-cycle header data is invalid.
Solution: Make sure the variable number is valid (#1-#999).
P/S 116 — WRITE PROTECTED VARIABLE
Machine type: Lathe and machining center
Meaning: An attempt was made to write to a write-protected variable (e.g. a system variable).
Solution: Only use variables with read/write permission.
P/S 118 — PARENTHESIS NESTING ERROR
Machine type: Lathe and machining center (macro)
Meaning: The bracket nesting limit (5 levels) was exceeded.
Solution: Arrange the brackets properly.
P/S 119 — ILLEGAL ARGUMENT
Machine type: Lathe and machining center (macro)
Meaning: The SQRT (square root) argument is negative, or a BCD/BIN conversion is invalid.
Solution: Make sure the argument is positive.
P/S 122 — DUPLICATE MACRO MODAL-CALL
Machine type: Lathe and machining center
Meaning: A modal macro call was defined twice.
Solution: Call it only once.
P/S 123 — CAN NOT USE MACRO COMMAND IN DNC
Machine type: Lathe and machining center
Meaning: A macro control command cannot be used during a DNC operation.
Solution: Avoid macro control commands during DNC.
P/S 124 — MISSING END STATEMENT
Machine type: Lathe and machining center (macro)
Meaning: A DO-END mismatch occurred.
Solution: Make sure every DO has a matching END.
P/S 125 — FORMAT ERROR IN MACRO
Machine type: Lathe and machining center
Meaning: An invalid address or expression format error occurred in a G65 call.
Solution: Check the macro call format.
P/S 126 — ILLEGAL LOOP NUMBER
Machine type: Lathe and machining center
Meaning: In a DO n command, n is something other than 1, 2 or 3.
Solution: Only use DO1, DO2 or DO3.
P/S 127 — NC MACRO STATEMENT IN SAME BLOCK
Machine type: Lathe and machining center
Meaning: An NC command and a macro command were combined in the same block.
Solution: Write them in separate blocks.
P/S 128 — ILLEGAL MACRO SEQUENCE NUMBER
Machine type: Lathe and machining center
Meaning: The sequence number specified in a GOTO is not within 0-9999, or cannot be found.
Solution: Use a valid N number.
P/S 129 — ILLEGAL ARGUMENT ADDRESS
Machine type: Lathe and machining center
Meaning: An address not permitted in the argument assignment format was used.
Solution: Use valid addresses (A, B, C, etc.).
P/S 199 — MACRO WORD UNDEFINED
Machine type: Lathe and machining center
Meaning: An undefined macro word was used.
Solution: Define the macro variables correctly.
External Alarm Messages and PMC Axis Control
P/S 130 — İLLEGAL ARGUMENT ADDRESS (CNC/PMC eksen çatışması)
Machine type: Lathe and machining center
Meaning: An axis controlled by the CNC received a command from the PMC, or vice versa.
Solution: Set the axis control authority correctly.
P/S 131 — TOO MANY EXTERNAL ALARM MESSAGES
Machine type: Lathe and machining center
Meaning: Five or more external alarm messages occurred at the same time.
Solution: Review the PMC ladder diagram and clear the alarm sources one by one.
P/S 132 — ALARM NUMBER NOT FOUND
Machine type: Lathe and machining center
Meaning: The alarm number could not be found when clearing an external alarm message.
Solution: Check the ladder diagram.
P/S 133 — ILLEGAL DATA IN EXC. ALARM MSG
Machine type: Lathe and machining center
Meaning: Invalid data in an external alarm/operator message.
Solution: Check the PMC ladder.
P/S 139 — CAN NOT CHANGE PMC CONTROL AXIS
Machine type: Lathe and machining center
Meaning: The axis selected under PMC axis control cannot be changed.
Solution: Check the PMC ladder.
Spindle and Axis Control Errors
P/S 135 — SPINDLE ORIENTATION PLEASE
Machine type: Lathe and machining center (C axis or indexing)
Meaning: A spindle indexing operation was attempted without spindle orientation.
Solution: Perform orientation with M19 first.
P/S 136 — C/H-CODE AND MOVE CMD IN SAME BLOCK
Machine type: Lathe (C axis)
Meaning: Spindle indexing addresses (C, H) and another axis move were combined in the same block.
Solution: Write them in separate blocks.
P/S 194 — SPINDLE COMMAND IN SYNCRO-MODE
Machine type: Lathe and machining center (dual spindle)
Meaning: An unsuitable command was given while the spindles were in synchronous mode.
Solution: Cancel synchronous mode first.
P/S 195 — MODE CHANGE ERROR
Machine type: Lathe and machining center (serial spindle)
Meaning: The serial spindle control mode could not be changed.
Solution: Check the PMC ladder.
P/S 197 — C-AXIS COMMANDED IN SPINDLE MODE
Machine type: Lathe (C axis)
Meaning: A C-axis move was commanded while the CON signal was off.
Solution: Switch to C-axis mode first (M??), or check the PMC signals.
Tool Geometry (Twin Turret) Errors
P/S 161 — COMMAND G68/G69 INDEPENDENTLY (TT tezgâhlar)
Machine type: TT (turret-turret) type machines
Meaning: G68/G69 was not commanded independently in balance cutting.
Solution: Use G69 after G68 and do not place another G code between them.
P/S 169 — ILLEGAL TOOL GEOMETRY DATA (TT)
Machine type: TT type machines
Meaning: Incorrect tool geometry data in interference checking.
Solution: Check the tool offsets.
High-Speed Machining (G05/G107) Errors
P/S 175 — ILLEGAL G107 COMMAND
Machine type: Machining center (cylindrical interpolation)
Meaning: Start-up or cancel conditions for cylindrical interpolation (G107) are not correct.
Solution: Call G107 in the correct way.
P/S 176 — IMPROPER G-CODE IN G107
Machine type: Machining center
Meaning: An invalid G code (e.g. G28, G76, G50, G53, etc.) was used in cylindrical interpolation mode.
Solution: Do not use these codes in G107 mode.
P/S 177 — CHECK SUM ERROR (G05 MODE)
Machine type: Machining center (high-speed machining)
Meaning: A checksum error occurred in G05 mode.
Solution: Check the program and reload it if necessary.
P/S 178 — G05 COMMANDED IN G41/G42 MODE
Machine type: Lathe and machining center
Meaning: G05 was commanded while tool radius compensation was active.
Solution: Do not use G05 without first canceling compensation.
P/S 179 — PARAM SETTING ERROR
Machine type: Lathe and machining center
Meaning: The number of controlled axes set in parameter 597 exceeded the maximum.
Solution: Set the parameter to the correct value.
General Tips for Troubleshooting Alarms
- Note down the alarm number and the on-screen message exactly as shown; the number alone is not enough — your control's exact message narrows down the cause.
- Record the program line (block number) where the alarm occurred; most P/S alarms highlight the relevant block on screen.
- The same alarm number can behave differently across FANUC series; do not directly apply a fix you found online without knowing your machine's exact model and control software version.
- If a fix requires a parameter change, back up the current parameter set first and have the change made by an authorized person.
- When in doubt, rely on your machine builder's or FANUC dealer's official manual.
Summary
The P/S alarm codes on this page cover what is not already covered in Mentor CNC’s FANUC 0/00/0-Mate parameter guide and the G71/G72/G74/G75 cycle pages. When you hit an alarm, check this page first, or the relevant cycle page (G71, G72, G74, G75) if it’s cycle/parameter related.