Who is this list for?
FANUC alarm lists run to thousands of lines and most of them are the service engineer’s problem: a board fault, an FSSB communication error, a PMC system alarm. There is nothing the operator can do about those.
This page is built differently. It covers the alarms the person standing at the machine actually meets — when a cycle parameter is entered wrongly, when an axis runs past its limit, when the tool hits the part, or when the spindle cannot reach speed. Every row says what the alarm means and what the operator can do about it.
Five groups, ~150 alarms1) Cycles, compensation and programming · 2) Overtravel · 3) Servo, overload and crash · 4) Spindle · 5) Encoder, battery and lost reference. Source: FANUC Series 0i-MODEL F Maintenance Manual, Appendix A alarm list.
What does the letter in front of the alarm number mean?
| Prefix | Group | Whose problem? |
|---|---|---|
| PS | Program and operation alarms | Operator / programmer |
| OT | Overtravel | Operator |
| SV | Servo alarms | Operator checks first, then service |
| SP | Spindle alarms | Operator checks first, then service |
| DS | Other alarms (battery, reference, fan) | Operator / maintenance |
| OH | Overheat | Operator / maintenance |
| SR | Communication alarms | Operator (transfer settings) |
| BG | Background edit alarms | Operator |
| PW | Alarms requiring power to be turned off | Service |
| IO | Memory file alarms | Operator / service |
Numbering differences between 0i-F and older seriesSeries 0i-MODEL F displays alarms as a letter prefix plus four digits:
PS0061, SV0410, OT0506. Older series (0, 0-MC, 16/18/21i) show the same alarms as three digits with no prefix: 061, 410, 506. Same alarm, different display.1. Cycle, compensation and programming alarms
This is the group operators meet most often. Enter a cycle parameter wrongly and the machine does not move — it alarms.
Multiple repetitive turning cycles (G70–G76)
| Alarm | Message | What happened | What the operator should do |
|---|---|---|---|
| PS0061 | P OR Q COMMAND IS NOT IN THE MULTIPLE REPETITIVE CYCLES | Address P or Q is missing from the cycle block. | Check the G71/G72/G73 line; both the contour start (P) and end (Q) sequence numbers must be there. |
| PS0062 | THE CUTTING AMOUNT IS ILLEGAL IN THE ROUGH CUTTING CYCLE | Zero or a negative depth of cut in the roughing cycle. | Check U (depth of cut) and R (retract) in G71. Neither can be zero or negative. |
| PS0063 | THE BLOCK OF A SPECIFIED SEQUENCE NUMBER IS NOT FOUND | The sequence numbers given in P and Q do not exist in the program. | Check that the N numbers written in P and Q really exist. A typo here is very common. |
| PS0064 | THE FINISHING SHAPE IS NOT A MONOTONOUS CHANGE (FIRST AXIS) | The finish contour does not change monotonically on the first axis. | The contour must increase or decrease continuously in X. If the profile doubles back, use G71 Type II or G73. |
| PS0065 | G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM | The first contour block does not contain G00 or G01. | Start the block pointed to by P with G00 or G01. |
| PS0066 | UNAVAILABLE COMMAND IS IN THE MULTIPLE REPETITIVE CYCLES | A command the cycle does not accept appears inside the contour. | Between P and Q there must be no subprogram call, macro or another cycle. |
| PS0067 | THE MULTIPLE REPETITIVE CYCLES IS NOT IN THE PART PROGRAM | G70/G71/G72/G73 was commanded from MDI. | These cycles cannot run from MDI. Save as a program and run it in AUTO. |
| PS0069 | LAST BLOCK OF SHAPE PROGRAM IS AN ILLEGAL COMMAND | The last contour block ends with an invalid command. | Check the block pointed to by Q; it must not end with a chamfer or corner R (CHF/CNR). |
| PS0060 | SEQUENCE NUMBER NOT FOUND | The program or sequence number searched for was not found. | If you ran a block search, check the N number you entered. |
Drilling cycles and tapping
| Alarm | Message | What happened | What the operator should do |
|---|---|---|---|
| PS0044 | G27-G30 NOT ALLOWED IN FIXED CYC | A reference return was commanded while a canned cycle was active. | Cancel the cycle with G80 before G28. |
| PS0045 | ADDRESS Q NOT FOUND (G73/G83) | The peck depth Q is missing or zero in the peck drilling cycle. | Add a Q value to the G73/G83 line. It cannot be zero. |
| PS0203 | PROGRAM MISS AT RIGID TAPPING | The position of the M29 or S command is wrong in rigid tapping. | Put M29 S... immediately before the G84 block, with nothing in between. |
| PS0204 | ILLEGAL AXIS OPERATION | There is an axis move between M29 and G84. | Do not place any motion block between M29 and G84. |
| PS0205 | RIGID MODE DI SIGNAL OFF | M29 was commanded but the machine did not return the rigid mode signal. | Check that the machine has the rigid tapping option. If the signal never arrives, call service. |
| PS0207 | RIGID DATA MISMATCH | The distance specified in rigid tapping is too short or too long. | Check the Z depth and R level on the G84 line, and confirm the pitch (F). |
| PS0080 | G37 MEASURING POSITION REACHED SIGNAL IS NOT PROPER | No measurement signal during automatic tool length measurement. | Check that the probe/switch works and that the tool approaches from the correct direction. |
| PS0081 | G37 OFFSET NO. UNASSIGNED | No H number was selected before G37. | Select the relevant H offset number before the G37 block. |
| PS0082 | G37 SPECIFIED WITH H CODE | G37 and an H code were written in the same block. | Move H to the preceding block. |
Cutter radius compensation (G41/G42), chamfer and corner R
| Alarm | Message | What happened | What the operator should do |
|---|---|---|---|
| PS0033 | NO INTERSECTION AT CUTTER COMPENSATION | The intersection cannot be calculated under compensation. | The tool radius may be larger than the pocket or corner radius. Use a smaller tool or check the offset value. |
| PS0034 | NO CIRC ALLOWED IN ST-UP/EXT BLK | A circular move was commanded on the compensation start-up or cancel block. | Use a straight G01 move on the G41/G42 and G40 lines. |
| PS0035 | CAN NOT COMMANDED G31 | G31 skip was commanded while compensation was active. | Cancel compensation with G40 before G31. |
| PS0037 | CAN NOT CHANGE PLANE IN CRC | The plane (G17/G18/G19) was changed under compensation. | Command G40 before changing the plane. |
| PS0041 | INTERFERENCE IN CUTTER COMPENSATION | Compensation detected that excessive cutting would occur. | There is a feature narrower than the tool radius on the contour. Use a smaller tool or fix the contour. |
| PS0042 | G45/G48 NOT ALLOWED IN CRC | Tool offset G45–G48 was commanded under compensation. | Do not mix the two compensation types. |
| PS0050 | CHF/CNR NOT ALLOWED IN THRD BLK | A chamfer or corner R was commanded in a thread cutting block. | Remove the C or R chamfer command from the threading line. |
| PS0051 | MISSING MOVE AFTER CNR/CHF | The move after the chamfer/corner R block is wrong. | The block after the chamfer needs enough travel. |
| PS0052 | CODE IS NOT G01 AFTER CHF/CNR | The block after a chamfer/corner R is not G01. | Continue with G01 after a chamfer or corner R. |
| PS0053 | TOO MANY ADDRESS COMMANDS | Two or more of I, J, K and R were specified in a chamfer/corner R command. | Leave only one chamfer/corner address on the line. |
| PS0055 | MISSING MOVE VALUE IN CHF/CNR | The move distance is less than the chamfer or corner amount. | Reduce the chamfer value or lengthen the move. |
General programming and custom macro
| Alarm | Message | What happened | What the operator should do |
|---|---|---|---|
| PS0010 | IMPROPER G-CODE | A G code the machine does not have was used. | It may be an option, or the G code system (A/B/C) may differ. Check the machine’s G code list. |
| PS0011 | FEED ZERO (COMMAND) | The cutting feedrate was set to F0, or not given at all. | Add an F value to the G01/G02/G03 line. |
| PS0020 | OVER TOLERANCE OF RADIUS | The radius difference between arc start and end exceeds the tolerance. | Check the arc’s I, J, K or R values; CAM rounding is a common cause. |
| PS0021 | ILLEGAL PLANE SELECT | The plane selection is in error. | Check the G17/G18/G19 line and which plane the circular move belongs in. |
| PS0027 | NO AXES COMMANDED IN G43/G44 | No axis in the tool length compensation block. | Add the Z move to the G43 line. |
| PS0029 | ILLEGAL OFFSET VALUE | Invalid offset value. | Check the value entered in the offset table. |
| PS0030 | ILLEGAL OFFSET NUMBER | A non-existent offset number was called. | Make sure the H or D number is within the machine’s offset count. |
| PS0076 | PROGRAM NOT FOUND | The subprogram or macro called was not found. | Check that the O number called with M98 P… exists in memory. |
| PS0077 | TOO MANY SUB, MACRO NESTING | The subprogram/macro nesting limit was exceeded. | Shorten the subprogram chain; you may have left out an M99 return. |
| PS0310 | FILE NOT FOUND | The file was not found on a subprogram or macro call. | If running from external memory, check the path and file name. |
| PS0112 | ZERO DIVIDE | A division by zero in a custom macro. | Make sure the divisor variable is not zero. |
| PS0114 | ILLEGAL EXPRESSION FORMAT | A macro expression is badly formed. | Check the brackets and operators. |
| PS0115 | VARIABLE NO. OUT OF RANGE | An unusable variable number. | Check how far the #500 series common variables go on your machine. |
| PS0116 | WRITE PROTECTED VARIABLE | An attempt to write to a read-only variable. | Some system variables are read-only. |
| PS0122 | TOO MANY MACRO NESTING | The macro nesting limit was exceeded. | Shorten the macro call chain. |
| PS0124 | MISSING END STATEMENT | No END matching the DO. | Write an END for every DO. |
| PS0126 | ILLEGAL LOOP NUMBER | The DO/END number is invalid (must be 1–3). | Use matching numbers such as DO1/END1. |
| PS0127 | DUPLICATE NC, MACRO STATEMENT | An NC statement and a macro statement in the same block. | Put the macro expression on its own line. |
| PS5010 | END OF RECORD | An EOR (%) code appears in the middle of a block. | The program may have been corrupted during transfer. Transfer it again. |
2. Overtravel (OT) alarms
These come up when an axis leaves the permitted area. There are two kinds: a software limit (SOFT) is a virtual boundary set by parameter, while a hardware limit (HARD) means a physical limit switch has been tripped.
| Alarm | Message | What happened | What the operator should do |
|---|---|---|---|
| OT0500 | + OVERTRAVEL (SOFT 1) | The axis exceeded stored stroke check 1 in the positive direction. | Jog or handwheel the axis back in the negative direction, then RESET. |
| OT0501 | − OVERTRAVEL (SOFT 1) | Stored stroke check 1 exceeded in the negative direction. | Move the axis back in the positive direction, then RESET. |
| OT0502 | + OVERTRAVEL (SOFT 2) | Stored stroke check 2 exceeded. On a lathe, entering the chuck/tailstock barrier also raises this. | On a lathe: the tool may have come too close to the chuck or tailstock. Back off and RESET. |
| OT0503 | − OVERTRAVEL (SOFT 2) | Stored stroke check 2 exceeded in the negative direction, or a barrier was entered. | Same — move out in the opposite direction. |
| OT0504 / OT0505 | + / − OVERTRAVEL (SOFT 3) | Stored stroke check 3 exceeded. | Move in the opposite direction, then RESET. |
| OT0506 | + OVERTRAVEL (HARD) | The physical limit switch in the positive direction was tripped. The machine reached the stroke end. | Hold the overtravel release button on the panel and move the axis in the negative direction, then RESET. If there is no such button, see the builder’s manual. |
| OT0507 | − OVERTRAVEL (HARD) | The negative direction limit switch. | Same method, opposite direction. |
| OT0508 | INTERFERENCE: + | A tool moving in the positive direction fouled another tool post. | Turret clash on a twin-turret machine. Check the program and turret positions. |
| OT0509 | INTERFERENCE: − | Turret interference in the negative direction. | Same check. |
| OT0510 | + OVERTRAVEL (PRE-CHECK) | The stroke check before movement detected that the limit would be exceeded. | The control caught it before the machine moved. Check the target coordinate and the work offset — this is usually a wrong G54 value. |
| OT0511 | − OVERTRAVEL (PRE-CHECK) | Same check, negative direction. | Same check. |
The most common causeA software overtravel usually comes from a work offset taken wrongly. Enter a value with the wrong sign or on the wrong axis in G54 and the control tries to run the program outside the working envelope. Check the offset value before you clear the alarm.
3. Servo, overload and crash alarms
This group appears when the tool hits the part, the vice or the fixture, when the feedrate is too high, or when an axis is mechanically obstructed.
Stop firstAfter a crash, look at the tool and the part before pressing RESET. Once the alarm is cleared and the axis is released, it can move suddenly.
| Alarm | Message | What happened | What the operator should do |
|---|---|---|---|
| SV0409 | DETECT ABNORMAL TORQUE | An abnormal load was detected on the servo motor. This is the typical crash alarm. | Inspect the tool and the part. Is the tool broken, has the part shifted? Do not run again until the cause is found. |
| SV0407 | EXCESS ERROR | The positional deviation difference exceeded the limit. | The axis may be mechanically obstructed. Check the slideways and look for trapped chips. |
| SV0410 | EXCESS ERROR (STOP) | Positional deviation while the axis was stopped became too large. | Something is pushing the axis (a jammed part, a failed brake). One of the most common post-crash alarms. |
| SV0411 | EXCESS ERROR (MOVING) | Positional deviation while the axis was moving became too large. | Feedrate too high or the axis is being obstructed. Lower the override and retry; if it repeats, call service. |
| SV0401 | IMPROPER V_READY OFF | The drive ready signal dropped unexpectedly. | Usually the amplifier side. Power cycle the machine; if it repeats, call service. |
| SV0404 | IMPROPER V_READY ON | The ready signal is present when it should not be. | Service matter. |
| SV0413 | LSI OVERFLOW | The positional deviation counter overflowed. | Usually after a heavy crash or jam. Have the mechanics checked. |
| SV0430 | SV MOTOR OVERHEAT | The servo motor overheated. | Let the machine rest. Continuous heavy cuts or a seized slideway can cause it. If it repeats, call service. |
| SV0436 | SOFT THERMAL (OVC) | The software thermal protection tripped — the motor is drawing excessive current continuously. | Ease the cutting conditions (depth, feed). Mechanical binding can also cause it. |
| SV0438 | SV ABNORMAL CURRENT | Motor overcurrent. | Power down and look for mechanical obstruction. If it repeats, call service. |
| SV0010 | SV OVERHEAT | Amplifier internal overheat. | Check cabinet fans and filters; is the cabinet door closed, is the ambient temperature high? |
| SV0024 | PS SOFT THERMAL | A load higher than the rating was applied. | Ease the cutting conditions. |
| SV0431 | PS OVERLOAD | Power supply overheat. | Check cooling and ventilation. |
| SV0432 | PS LOW VOLT. CONTROL | The control power supply voltage dropped. | Have the mains supply checked. There may have been a voltage dip in the plant. |
| SV0433 / SV0435 | LOW VOLT. DC LINK | Low DC link voltage. | Supply problem. Inform electrical maintenance. |
| SV0439 | PS OVER VOLT. DC LINK | DC link voltage too high. | Regenerative resistor or supply problem. Service. |
| SV0437 | PS OVERCURRENT | Overcurrent on the input circuit. | Service matter. |
| SV0443 / SV0444 | INTERNAL FAN FAILURE | Internal cooling fan failure. | Report to maintenance. The machine can overheat until the fan is replaced. |
| SV0445 | SOFT DISCONNECT ALARM | The software detected a disconnected encoder. | The encoder cable may be loose. Service. |
| SV0446 | HARD DISCONNECT ALARM | The hardware detected a disconnected built-in Pulsecoder. | Service. |
| SV0447 | HARD DISCONNECT (EXT) | Separate detector (linear scale) disconnected. | Have the scale cable and connector checked. |
| SV0449 | SV IPM ALARM | Power module alarm. | Service matter. |
| SV0460 | FSSB DISCONNECT | The FSSB fibre connection was lost. | Service matter — the operator should not intervene. |
| SV0466 | MOTOR/AMP. COMBINATION | The motor and amplifier do not match. | Seen after a part replacement. Service. |
| SV0421 | EXCESS ERROR (SEMI-FULL) | A difference between semi-closed and full-closed loop feedback. | Possible scale or coupling problem. Service. |
| SV0417 | SERVO PARAMETER SET | An invalid value in a servo parameter. | If a parameter was changed, revert it. Service. |
| DS0608 / DS0609 | SV COOLING / RADIATOR FAN FAILURE | Servo drive fan failure. | Report to maintenance. |
| DS0612 | PS OVERLOAD | Power supply overheat. | Check ventilation and filters. |
| OH0700 | LOCKER OVERHEAT | The CNC cabinet overheated. | Is the cabinet door open, is the air conditioner or fan running, is the filter blocked? |
| OH0701 | FAN MOTOR STOP | The PCB cooling fan stopped. | Report to maintenance; the fan needs replacing. |
4. Spindle (SP) alarms
If the spindle will not reach speed, orientation will not hold, a tool change fails or rigid tapping goes wrong, the alarm lands in this group.
| Alarm | Message | What happened | What the operator should do |
|---|---|---|---|
| SP0740 | RIGID TAP ALARM: EXCESS ERROR | Positional deviation of the stopped spindle exceeded the limit in rigid tapping. | The tap may be binding. Check the pilot hole diameter, the pitch (F) and the speed. |
| SP0741 | RIGID TAP ALARM: EXCESS ERROR | Deviation of the moving spindle exceeded the limit. | Reduce the speed; the tap may be dull or the pilot hole too small. |
| SP0742 | RIGID TAP ALARM: LSI OVERFLOW | Counter overflow during rigid tapping. | Check the program; are the pitch and depth values sensible? |
| SP0752 | SPINDLE MODE CHANGE ERROR | A spindle mode change did not complete (Cs contour, positioning, rigid tapping). | Check where M29 or the mode change command sits; RESET and try again. |
| SP0754 | ABNORMAL TORQUE | An abnormal load was detected on the spindle motor. | The tool may be dull, the cut too heavy or the tool jammed. Review the cutting conditions. |
| SP1202 | SPINDLE SELECT ERROR | An invalid spindle number in multi-spindle control. | Check the spindle selection command in the program. |
| SP1210 | TOOL CHANGE SP MOTION | Too much distribution to the spindle during a tool change. | Check the tool change position and the Z position. |
| SP1211 | TOOL CHANGE SP ORTN EXCESS | Too large an orientation error during a tool change. | Spindle orientation is not holding. Try M19 manually; if it will not hold, call service. |
| SP1212 | TOOL CHANGE SP MOVE EXCESS | Too large a moving error during a tool change. | Magazine/ATC mechanical check. Service may be needed. |
| SP1213 | TOOL CHANGE SP STOP EXCESS | Too large a stop error during a tool change. | The ATC may be engaging before the spindle has fully stopped. Service. |
| SP1214 | TOOL CHANGE SP ILLEGAL | An abnormal spindle sequence during a tool change. | The ATC may have stopped mid-cycle. Follow the builder’s ATC recovery procedure. |
| SP1220 | NO SPINDLE AMP. | No communication with the serial spindle amplifier. | Power cycle the machine. If it repeats, call service — cable or drive problem. |
| SP1221 | ILLEGAL MOTOR NUMBER | The spindle number and motor number do not match. | Parameter problem. Service. |
| SP1224 | ILLEGAL SPINDLE-POSITION CODER | The spindle position coder gear ratio is incorrect. | Parameter problem. Service. |
| SP1225–SP1229 | CRC / FRAMING / COMMUNICATION ERROR (SERIAL SPINDLE) | A communication error between the CNC and the spindle drive. | Usually cable or electrical noise. Power cycle; if it repeats, call service. |
| SP1231 | SPINDLE EXCESS ERROR (MOVING) | Position deviation during spindle rotation was too high. | Seen in rigid tapping or Cs contour mode. Ease the cutting conditions. |
| SP1232 | SPINDLE EXCESS ERROR (STOP) | Position deviation with the spindle stopped was too high. | The spindle cannot hold position or an external force is acting on it. Service. |
| SP1233 | POSITION CODER OVERFLOW | The position coder counter overflowed. | Service matter. |
| SP1234 | GRID SHIFT OVERFLOW | Grid shift overflowed. | Parameter problem. Service. |
| SP1240 | DISCONNECT POSITION CODER | The analog spindle position coder is broken. | Service matter. |
| SP1241 | D/A CONVERTER ERROR | D/A converter error in analog spindle control. | Service matter. |
| SP1243 / SP1252 | ILLEGAL SPINDLE PARAMETER | An invalid spindle parameter. | If a parameter was changed, revert it. Service. |
| SP1244 | MOTION VALUE OVERFLOW | Too much distribution to the spindle. | Check the program. |
| SP1255 | CAN NOT CHANGE SPINDLE MODE | Rigid tapping or positioning mode cannot be entered in analog spindle control. | Check whether the machine has that option. |
| OH0704 | OVERHEAT (SPINDLE) | The spindle overheated. | Let the spindle rest. Check that cooling and lubrication are working. Continuous heavy cuts can cause it. |
| PS0194 | SPINDLE COMMAND IN SYNCHRO-MODE | An invalid spindle command in synchronous mode. | An S command may have been issued with Cs contour or rigid tapping mode active. Check the program. |
| PS5018 | POLYGON SPINDLE SPEED ERROR | The spindle speed is out of range in polygon turning. | Check the speed ratios in the G51.2 block. |
5. Encoder, battery and lost reference alarms
This group usually greets you when the machine is switched on in the morning. The most common cause is a flat absolute position battery.
Do not put off a battery alarmWhen
DS0307 (battery low) appears the machine keeps running — but if the battery goes completely flat, DS0306 follows and every axis loses its reference. At that point every axis must be re-referenced and every work offset verified. Change the battery with the machine powered on.| Alarm | Message | What happened | What the operator should do |
|---|---|---|---|
| DS0307 | APC ALARM: BATTERY LOW 1 | The absolute position battery is getting weak. First warning. | Replace the battery soon. The machine keeps running; no panic. |
| DS0308 | APC ALARM: BATTERY LOW 2 | The battery voltage has dropped further. | No more delaying. Replace it now. |
| DS0306 | APC ALARM: BATTERY VOLTAGE 0 | The battery is flat and the absolute position data is lost. | Replace the battery, then re-reference every axis. Verify all work offsets before machining. |
| DS0300 | APC ALARM: NEED REF RETURN | The absolute position detector has not been zeroed. | A reference operation is needed. Normal after first commissioning or a battery change. |
| DS0309 | APC ALARM: REF RETURN | An attempt to set the absolute zero under the wrong conditions. | Follow the procedure; the axis must be moved before zeroing. |
| DS0020 | REFERENCE RETURN INCOMPLETE | An automatic reference return could not complete. | Jog the axis away a little and repeat the reference operation. |
| DS0072 | MANUAL REFERENCE RETURN | Manual reference return cannot be performed in this state. | Automatic operation may be halted. RESET and try again. |
| DS0405 | ZERO RETURN END NOT ON REF | The axis did not end up at the correct point after zero return. | Repeat the reference operation. If it repeats, call service. |
| PS0090 | REFERENCE RETURN INCOMPLETE | The start point may be too close to the reference position. | Move the axis away from the reference position and try again. |
| PS0091 | MANUAL REFERENCE POSITION RETURN IS NOT PERFORMED | Manual reference return is not possible while automatic operation is halted. | RESET, then send the axis to reference. |
| PS0224 | ZERO RETURN NOT FINISHED | No reference return was performed before automatic operation. | Send all axes to reference, then cycle start. The most common morning alarm. |
| SV0301–SV0305 | APC ALARM: COMMUNICATION / OVER TIME / FRAMING / PARITY / PULSE ERROR | A communication error with the absolute position detector. | Cable or encoder problem. Service. |
| SV0306 | APC ALARM: OVER FLOW ERROR | The positional deviation overflowed. | Service. |
| SV0307 | APC ALARM: MOVEMENT EXCESS | The machine moved too much while powered off, so the correct position could not be read. | The axis may have been moved by hand while off. Perform a reference operation. |
| SV0360–SV0369 | ABNORMAL CHECKSUM / PHASE / REV. DATA / CLOCK / BROKEN LED (INT) | Built-in Pulsecoder (motor encoder) faults. | Service matter. The motor encoder may need replacing. |
| SV0380–SV0387 | BROKEN LED / COUNT MISS / PULSE MISS / DATA ERROR (EXT) | Separate detector (linear scale) faults. | The scale may be dirty or the cable damaged. Service. |
| DS1450 | ZERO RETURN NOT FINISHED | The 1st reference position return has not completed. | Complete the reference operation. |
| DS2091 | CAN NOT RETURN TO BREAKPOINT | Could not return to the machine position of the breakpoint. | You may need to restart the program. Use a block search. |
| DS5259 | INTERRUPTED POSITION NOT FOUND | The interruption (restart) point was not found. | The restart information is lost. Continue with a block search. |
| PS0233 | DEVICE BUSY | A unit such as the RS-232-C interface is in use by another process. | Another transfer may be running. Wait, or close the other operation. |
When an alarm comes up: the operator’s six-step check
- Do not hit RESET straight away. Write down the alarm number and the message first. Once it is cleared, finding out which axis and which line it happened on gets much harder.
- Look at which line it stopped on. The active block on the program screen points straight at the cause for cycle and compensation alarms.
- Inspect the tool and the part. With SV0409, SV0410 and SV0411 especially, check first whether there has been a crash.
- Look at the prefix. PS and OT are almost always something you can fix yourself; SV, SP and PW may need service.
- Check the alarm history. A repeating alarm is not a coincidence. The history screen shows how often the problem occurs.
- Make the first move after RESET in single block. Lower the feedrate override and keep a hand on feed hold.
What the operator should not doDo not change parameters to silence an alarm. Servo and spindle parameters, backlash values and limit settings are not operator-level. Trying to solve an overtravel alarm by widening the software limit can drive the machine into its mechanical stroke end.
Frequently asked questions
The alarm will not clear with RESET. What now?
The cause is still present. On an overtravel the axis is still outside the limit — you have to move it back first. Some servo alarms (including everything with the PW prefix) clear only when the power is switched off and on. If it still comes back after a power cycle, there is a hardware problem.
The machine crashed into the part. Which alarm appears?
Typically SV0409 DETECT ABNORMAL TORQUE, SV0410 EXCESS ERROR (STOP) and SV0411 EXCESS ERROR (MOVING). If the crash is on the spindle side you get SP0754 ABNORMAL TORQUE. Before pressing RESET after any of these, inspect the tool, the part and the fixture — the axis can move suddenly once it is released.
I keep getting alarms in the G71 cycle. Where should I look?
In order: PS0061 P/Q missing, PS0063 the N numbers in P/Q do not exist, PS0062 depth of cut zero or negative, PS0065 the first contour block is not G00/G01, PS0064 the contour is not monotonic. These five cover the great majority of G71 errors.
A battery alarm appears when I switch on in the morning. Do I have to stop?
No. DS0307 (BATTERY LOW 1) is a warning and the machine keeps running. But do not delay: once the battery goes flat and DS0306 appears, the absolute position of every axis is lost, every axis must be re-referenced and every work offset verified. Change the battery with the machine powered on.
How do I recover an axis from an overtravel alarm?
On a software limit (SOFT, OT0500–OT0505): jog or handwheel the axis in the opposite direction, then RESET. On a hardware limit (HARD, OT0506/OT0507): hold the overtravel release / limit override button on the panel while moving the axis the other way. That button is not in the same place on every machine — check the builder’s manual.
Does the same alarm number mean the same thing on every FANUC series?
Largely yes, but the numbering format differs. 0i-MODEL F shows a letter prefix plus four digits (PS0061, OT0506); older series show the same alarm as three digits with no prefix (061, 506). Some series also have their own ranges, such as the second servo alarm block (600–699) on the 21i.
I keep getting SP0740/SP0741 in rigid tapping.
Check three things: the pilot hole diameter (too small and the tap binds), the pitch value (F) against the tap’s actual pitch, and the speed. Also make sure the M29 S... line sits immediately before G84 with no motion in between.
Which alarms mean I should call service?
As a rule: PS and OT alarms come from the program or the operation and the operator can resolve them. With SV and SP alarms, check the mechanics and cutting conditions first; if they repeat, call service. Alarms with the PW prefix (power must be turned off), FSSB alarms and PMC system alarms are service matters directly.
Safety warningAxes and the spindle can move unexpectedly while an alarm is being dealt with. Stop the spindle and isolate power where necessary before entering the working area. After a crash, do not return to production until the tool, holder, spindle and fixture have been inspected. Parameter changes must be made by authorised personnel with a backup taken first.
Mentor CNC note: The alarm numbers, messages and descriptions on this page are based on Appendix A of FANUC’s official Series 0i-MODEL F Maintenance Manual (B-64605EN/01). The “What the operator should do” column reflects shop-floor practice and is not part of the official manual. What an alarm means on your machine may vary with the control version, the options purchased and the machine tool builder’s configuration; machine alarms defined by the builder (PMC messages) are not included in this list. The machine tool builder’s documentation always takes precedence. This page is for training purposes and does not replace the official manual.
Sources
- FANUC — Series 0i-MODEL F MAINTENANCE MANUAL, document no. B-64605EN/01, Appendix A ALARM LIST: A.1 (1) Alarms on program and operation (PS), (5) Servo alarms (SV), (6) Overtravel alarms (OT), (9) Spindle alarms (SP), (10) Overheat alarms (OH), (11) Other alarms (DS)
- FANUC — Series 0i-MODEL F Common to Lathe System / Machining Center System OPERATOR’S MANUAL, B-64604EN/01 (for the definitions of the cycle and compensation commands)