This is Part 5 of the English reference for FANUC P/S (Program / Setting) alarm numbers, covering 2032–5074. This part includes communication and network errors, P-CODE macro variables, peripheral axis control, and the sheet-metal / punch-press and laser cycle command range (4500–4751).
- 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 in the 4500–4751 range relate to punch press, nibbling, and laser options and will never appear on a machining center or lathe.
2032–2095: Ethernet, Data Server, P-CODE Macros
| Code | Message | Meaning / action |
|---|---|---|
| 2032 | Embedded Ethernet / data server error | The embedded Ethernet / data server function returned an error. Check the embedded Ethernet or data server error message screen for details. |
| 2038 | Communication function combination error | The combination of hardware or software options used for the communication function is invalid. Details of the invalid combination are shown in diagnosis numbers 4400 and 4401. |
| 2052 | #500–#549 P-CODE macro common selection (SETVN not available) | The variable name cannot be entered. The SETVN command cannot be used for P-CODE macro common variables #500 to #549. |
| 2053 | #30000 number does not match | An attempt was made to enter a P-CODE specific variable that does not exist in the system. |
| 2054 | #40000 number does not match | An attempt was made to enter an extended P-CODE specific variable that does not exist in the system. |
| 2070 | G02.1 / G03.1 format error | The format is wrong. The specified arc length exceeds the interpolable range. |
| 2090 | Suspended block not found | The final coordinates of the interrupted machining block calculated by temporary execution differ from those of the stored interrupted machining block. Possible causes: the number of executed blocks counted during normal operation does not match the number during temporary execution; after the program was interrupted the program was modified, changing the number of blocks or movement amount before the interrupted block and thus its final coordinates; the offset amount changed; or the coordinate system changed. |
| 2095 | Peripheral axis control program registration error | The peripheral axis control program cannot be registered because: the end of the program was detected without a G100 command being executed after G101 (or G102, G103); or the Q command is missing from the same block as the peripheral axis control program registration start command (G101, G102, G103) — this occurs only when an axis of a system is specified as a peripheral axis for multiple peripheral axis controls. |
4010–4511: Output Buffer, Repositioning, Sheet-Metal Cycles
| Code | Message | Meaning / action |
|---|---|---|
| 4010 | Invalid real value in the output buffer | The actual value of the output buffer is incorrect. |
| 4500 | Illegal repositioning command | (1) An automatic repositioning command (G75) was issued without the workpiece clamp M code or workpiece unclamp M code being set. (2) An automatic repositioning command (G75) and an M code or T code were issued at the same time. (3) A workpiece clamp M code was issued at the same time as a circular interpolation command (G02/G03), or a circular interpolation command was issued after the workpiece clamp M code. (4) A workpiece clamp M code was issued in coordinate system rotation mode (G84), or a coordinate system rotation command was issued after the workpiece clamp M code. (5) A workpiece clamp M code was issued in tool radius compensation mode (G41/G42), or a tool radius compensation command was issued after the workpiece clamp M code. |
| 4502 | Illegal bolt hole circle command | A bolt hole circle (G26) command was executed under these conditions: I, J or K not specified; I command value (r) less than or equal to 0; K command value (n) = 0. |
| 4503 | Line angle command error | A line at angle (G76) command was executed under these conditions: I, J or K not specified; K command value (n) is 0 or less. |
| 4504 | Arc command error | An arc (G77) command was executed under these conditions: I, J, P or K not specified; I command value (r) less than or equal to 0; K command value (n) less than or equal to 0. |
| 4505 | Grid command error | A grid command (G78, G79) was executed under these conditions: one of I, J, P or K not specified; P command value (nx) less than or equal to 0; K command value (ny) less than or equal to 0. |
| 4506 | Shear command error | A shear (G86) command was executed under these conditions: I, J or P not specified; when parameter AIP (No. 16202 #0) = 0, the absolute I command value (l) is less than 1.5 times the absolute P command value (w1); when parameter AIP (No. 16202 #0) = 1, the absolute I command value (l) is less than the absolute P command value (w1); P command value (w1) = 0. |
| 4507 | Illegal square command | A square (G87) command was executed under these conditions: I, J or P not specified; P command value (w1) less than or equal to 0; Q command value (w2) less than or equal to 0; absolute I command value (lx) less than 3 times the absolute P command value (w1); absolute J command value (ly) less than 3 times the absolute Q command value (w2). |
| 4508 | Radius command error | A radius (G88) command was executed under these conditions: I, J, K, P or Q not specified; I command value (r) less than or equal to 0; Q command value (p) less than or equal to 0; an arc inside diameter was specified (d less than 0) and the tool diameter absolute value is equal to or greater than the specified arc diameter (2r); the specified arc length (2p × r × absolute Dq / 360) is less than the Q command value (p). |
| 4509 | Illegal slant command | A slant (G89) command was executed under these conditions: I, J, P or Q not specified; Q command value (p) less than or equal to 0; I command value (l) less than the Q command value (p). |
| 4510 | Illegal linear punching command | A linear punching (G45) command was executed under these conditions: X, Y or P not specified; punching distance less than 1.5 times the P command value (w1); P command value (w1) less than or equal to 0; Q command value (w2) less than or equal to 0. |
| 4511 | Illegal arc punching command | An arc punching (G46, G47) command was executed under these conditions: R or Q not specified; R command value (r) = 0; Q command value (p) less than or equal to 0; start point equals end point; arc length less than the Q command value (p). |
4520–4544: Nibbling and Multi-Punch Macros
| Code | Message | Meaning / action |
|---|---|---|
| 4520 | Command cannot be issued in nibbling mode | T, M, G04, G05, G05.1, G08, G28, G30.1, G32, G70 or G75 was issued while nibbling with the M function. |
| 4521 | X and Y axis pitch in nibbling mode | While nibbling with the M function, the movement amount of the X and Y axes exceeded the maximum pitch (parameters No. 16188 to 16192). |
| 4522 | C axis pitch during nibbling | During nibbling, the C axis movement amount exceeded the maximum pitch (parameter No. 16194). |
| 4523 | Illegal circular nibbling command | A circular nibbling (G68) command was executed under these conditions: one of I, J, K, P or Q not specified; one of I, J, K, P or Q out of range; the inside of the arc was specified (P less than 0) and the absolute value of P is greater than or equal to 2I·Q, which exceeds the maximum pitch (parameter No. 16186). |
| 4524 | Illegal linear nibbling command | A linear nibbling (G69) command was executed under these conditions: one of I, J, P or Q not specified; one of I, J, P or Q out of range; Q greater than the maximum pitch (parameter No. 16186). |
| 4530 | Illegal A/B macro command | A macro number that cannot be used in an A/B macro command was used (other than 1 to 5); the number of characters to be stored exceeds 200; an A/B macro with an unstored number was called; address B was commanded while storing an A/B macro; or address A was not commanded at the beginning of the data block. |
| 4531 | Illegal U/V macro command | An attempt was made to store another macro while another macro is being stored with a U/V macro command; a V command was executed even though no macro is stored; or the correspondence between U and V macro numbers does not match. |
| 4532 | U and V numbers that cannot be used | An invalid macro number was specified in a U/V macro command. |
| 4533 | U/V macro storage capacity exceeded | A U/V macro command tried to store more macros than the macro storage capacity allows. |
| 4534 | A macro number that has not been stored | In a U/V macro command, an unstored macro number W was specified. |
| 4536 | No W or Q command in a multi-punch command | W or Q was not specified in a multi-punch command (G73, G74). |
| 4537 | W or Q not specified in a multi-punch command | In a multi-punch command (G73, G74), the Q command value is not 1 to 4. |
| 4538 | No stored macro for a multi-punch command | An unstored macro number W was specified in a multi-punch command (G73, G74). |
| 4539 | Multi-punch setting is 0 | A multi-punch command (G73, G74) was issued even though the multi-punch setting (parameter No. 16206 or signals MLP1, MLP2 <Gn231.0, .1>) is 0. |
| 4540 | Multi-punch execution command during macro storage | A multi-punch command (G73, G74) was issued while a U/V macro was being stored. |
| 4542 | Multi-punch command error | G73 was commanded even though G98 P0 was commanded. G74 was commanded even though G98 K0 was commanded. |
| 4543 | Multi-punch Q command error | Even though G98 P0 was commanded, Q in the G74 command is not 1 or 3. Even though G98 K0 was commanded, Q in the G73 command is not 1 or 2. |
| 4544 | Multi-punch P/R command error | (1) In a multi-punch restart command, the restart position (P) is not within 1 to the total number of machining operations. (2) In a multi-punch end position command, the end position (R) is not within 1 to the total number of machining operations. (3) In a multi-punch end position command, the end position (R) was set to a value smaller than the restart position (P). |
4600–4872: T/C Axis, Laser, Tool Compensation
| Code | Message | Meaning / action |
|---|---|---|
| 4600 | T, C command issued in interpolation mode | A T axis or C axis command was issued in linear interpolation (G01) or circular interpolation (G02, G03) mode. |
| 4601 | T, M commanded | A T or M command was specified in a G10, G22, G23, G52, G53, G72, G73, G74, G75, G92 or G98 block. |
| 4602 | A T command that cannot be issued | A T command that is not registered on the tool registration screen is being issued. |
| 4604 | Axis control command error | There is a C axis command in the same block as a multi-tool T code command. |
| 4606 | T commanded | During normal direction control, a T axis command was specified in an invalid block. |
| 4630 | Laser mode command error | A pitting or pattern command was issued in laser mode. |
| 4650 | G commands that cannot be used in offset mode | An invalid G code was specified in tool diameter compensation mode. |
| 4751 | C axis command cannot be executed | The C axis was specified in an invalid block. |
| 4872 | Automatic setting command error | An M, S or T command was issued at the same time as the safety zone automatic setting command (G32). An automatic setting command was issued in nibbling mode. An automatic setting command was issued in tool radius compensation, coordinate rotation, or scaling mode. |
5006–5074: Program Limits, Feedrate, Address Format
| Code | Message | Meaning / action |
|---|---|---|
| 5006 | Number of words exceeded the limit | The number of words in a single block exceeds the allowable range. The limit varies by model but is typically a maximum of 35 words. Split the command words into two blocks. |
| 5007 | Movement amount exceeds the maximum command value | The movement amount exceeded the maximum command value due to compensation calculation, interference point calculation, interpolation, etc. Check the coordinates and compensation amount in the program command. |
| 5009 | Feedrate 0 (dry run) | The dry run rate parameter (No. 1410) or the maximum cutting feedrate parameter for each axis (No. 1430) is set to 0. |
| 5010 | End of program | The EOR (end of record) code was specified in the middle of a block. This alarm is also triggered when the percent sign at the end of an NC program is read. |
| 5011 | Feedrate 0 (maximum cutting feedrate) | The setting value of the maximum cutting feedrate parameter (No. 1430) is 0. |
| 5016 | Illegal M code combination | M codes in the same group can be combined and specified in the same block, or a single-command M code can be included and specified. |
| 5018 | Inappropriate speed command for the polygon spindle | In G51.2 mode, the speed of the spindle or polygon synchronous axis exceeds the clamp value, or the speed is too low to maintain the commanded speed ratio. During inter-spindle polygon machining, details of this alarm are shown in diagnosis data No. 0471. |
| 5020 | Invalid restart parameter | The setting value of parameter No. 7310, which specifies the order in which axes move to the machining restart position during dry run, is invalid. The setting range is 1 to the number of controlled axes. |
| 5030 | No registration start command but a registration end command | An end command (G100) was issued without a registration start command (G101, G102, G103) being issued (peripheral axis control). |
| 5031 | Another registration start command during a registration command | A registration start command (G101, G102, G103) was issued again during a registration start command (peripheral axis control). |
| 5032 | New operation command registered during peripheral axis control | An attempt was made to register a new operation command during peripheral axis control. |
| 5033 | Peripheral axis control program cannot be registered due to insufficient memory | The peripheral axis control program cannot be registered because program memory is insufficient. |
| 5034 | Multiple operations performed with a G110 command | Multiple operations were performed with a G110 (peripheral axis control) command. |
| 5038 | Peripheral axis control start command M code: 6 or more | Six or more peripheral axis control start command M codes were issued. |
| 5039 | Unregistered peripheral axis control program executed | An attempt was made to execute an unregistered peripheral axis control program. |
| 5040 | Peripheral axis control command cannot be issued | A peripheral axis control command cannot be issued because: peripheral axis control cannot be executed due to invalid parameter settings (No. 11884 to 11891); data that needs to be deleted after changing the parameter settings (No. 11884 to 11891) has not been deleted; or when starting peripheral axis control from a system different from the system set in parameters (No. 3040 to 3042), the system starting the peripheral axis control does not match the system set in parameter No. 0983. |
| 5043 | G68 nesting | A 3D coordinate conversion command was issued three or more times. To perform a new coordinate conversion, cancel the current command first and then issue it. |
| 5044 | G68 format error | The 3D coordinate conversion command block has one of these errors: (1) the I, J and K commands in the 3D coordinate conversion command block are all 0; (2) the rotation angle R command is missing from the block. |
| 5050 | Illegal command during oscillation | A movement command was issued to an axis in the oscillating state. |
| 5058 | G35 / G36 format error | A command was issued to switch the spindle during circular thread cutting, or the spindle length was set to 0. |
| 5065 | Setting axes with different setting units in the same group | When using a PMC control axis, axes with different setting units should be set to the same DI/DO group. Change parameter No. 8010. |
| 5068 | G31 P90 format error | The axis to be moved was not specified. Two or more axes to be moved were specified. |
| 5073 | No decimal point | A decimal point should have been entered in the address command but was not. |
| 5074 | Duplicate address command | There are two or more of the same address in the same block, or two or more G codes in the same group were specified. |
| 5110 | G code that cannot be controlled (AICC mode) | A G code that cannot be specified in AI advanced control (M system) / AI contour control mode was specified. |
How to Work With These Alarms
- Know which alarms can even apply to your machine. The 4500–4544 range is sheet-metal / punch-press specific (bolt hole circle, shear, square, nibbling, multi-punch macros) and 4600–4751 covers T/C axis and laser options. On a machining center or lathe these will never appear.
- 5009 and 5011 are parameter problems, not program problems: parameter 1410 (dry run rate) or 1430 (maximum cutting feedrate per axis) is set to 0. Setting a feedrate parameter to 0 to “disable” a limit causes these alarms instead.
- 5073 and 5074 are pure program formatting: a missing decimal point, or a duplicated address / two G codes from the same group in one block.
- 5030–5040 are peripheral axis control errors and require that option; they are configuration and registration sequence problems (G100/G101/G102/G103/G110), not part-program geometry errors.
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. Do the 4500 to 4751 alarms apply to my machining center?
Almost certainly not. The 4500–4544 range covers sheet-metal and punch-press cycles (bolt hole circle G26, shear G86, square G87, radius G88, linear and arc punching G45–G47, nibbling G68/G69, and multi-punch macros G73/G74), and 4600–4751 covers T/C axis control and laser functions. These require the corresponding machine type and options. On a machining center or lathe these codes will never appear, so if you see one it confirms the machine has the punch or laser option.
2. Why does my machine alarm 5009 or 5011 with feedrate 0?
Both mean a feedrate parameter is set to 0. Alarm 5009 means the dry run rate parameter (No. 1410) or the maximum cutting feedrate parameter for each axis (No. 1430) is set to 0. Alarm 5011 means specifically that the maximum cutting feedrate parameter (No. 1430) is set to 0. These are parameter setting problems rather than program errors, and they typically appear when someone sets a feedrate parameter to 0 intending to disable a limit.
3. What are alarms 5073 and 5074?
Both are straightforward program formatting errors. Alarm 5073 means a decimal point should have been entered in the address command but was not — check addresses that require a decimal point. Alarm 5074 means there are two or more of the same address in the same block, or two or more G codes from the same group were specified. Split them into separate blocks.
4. I get peripheral axis control alarms in the 5030 to 5040 range. What is wrong?
These relate to the peripheral axis control option and are mostly registration sequence or configuration problems, not part-program geometry errors. Check that the registration start command (G101, G102 or G103) is issued before the end command G100 (5030), that a start command is not issued twice (5031), that no new operation is registered during peripheral axis control (5032), that program memory is sufficient (5033), and that the parameter settings No. 11884 to 11891 are valid and consistent with the system settings No. 3040 to 3042 and No. 0983 (5040).
© 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