|
|
NC alarms
14040
[Channel %1: ] Block %2 error in end point of circle
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
In circular interpolation, either the circle radii for the initial point and the end point are further apart or the circle center
points are further apart than specified in the machine data.
1. In circle radius programming the starting and end points are identical, thus the circle position is not determined by
starting and end points.
2. Radii: The NCK calculates from the present starting point and the other programmed circle parameters the radii for the
starting and the end point.
An alarm message is issued if the difference between the circle radii is either
- greater than the value in the MD21000 $MC_CIRCLE_ERROR_CONST (for small radii, if the programmed radius is smaller
than the quotient of the machine data MD21000 $MC_CIRCLE_ERROR_CONST divided by MD21010
$MC_CIRCLE_ERROR_FACTOR), or
- greater than the programmed radius multiplied by the MD21000 $MC_CIRCLE_ERROR_FACTOR (for large radii, if the
programmed radius is greater than the quotient of the machine data MD21010 $MC_CIRCLE_ERROR_CONST divided by
MD21010 $MC_CIRCLE_ERROR_FACTOR).
3. Center points: A new circle center is calculated using the circle radius at the starting position. It lies on the mid-
perpendicular positioned on the connecting straight line from the starting point to the end point of the circle. The angle in
the radian measure between both straight lines from the starting point to the center calculated/programmed as such must
be lower than the root of 0.001 (corresponding to approx. 1.8 degrees).
4. Full circle with INTERSEC: Full circle is not allowed for the INTERSEC function.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Please inform the authorized personnel/service department.
Check MD21000 $MC_CIRCLE_ERROR_CONST and MD21010 $MC_CIRCLE_ERROR_FACTOR. If the values are within
reasonable limits, the circle end point or the circle mid-point of the part program block must be programmed with greater
accuracy.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14045
[Channel %1: ] Block %2 error in tangential circle programming
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The alarm can be caused by the following:
The tangent direction is not defined in the tangent circle programming, e.g. because no other traversing block has been
programmed before the current block. No circle can be formed from start and end point as well as tangent direction because
- seen from the start point - the end point is located in the opposite direction to that indicated by the tangent.
It is not possible to form a tangent circle since the tangent is located perpendicular to the active plane.
In the particular case in which the tangent circle changes to a straight line, several complete circular revolutions were
programmed with TURN.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14048
[Channel %1: ] Block %2 wrong number of revolutions in circle programming
Parameters:
%1 = Channel number
%2 = Block number, label
Alarms
216
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
In the circle programming, an inadmissible number of full revolutions has been specified.
The number of revolutions must not be negative and must not be greater than 1000000.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14050
[Channel %1: ] Block %2 nesting depth for arithmetic operations exceeded
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
For calculating arithmetic expressions in NC blocks, an operand stack with a fixed set size is used. With very complex
expressions, this stack can overflow. This may also occur with extensive expressions in synchronized actions.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Divide up complex arithmetic expressions into several simpler arithmetic blocks.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14051
[Channel %1: ] Block %2 arithmetic error in part program
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
- In calculating an arithmetic expression, an overflow has occurred (e.g. division by zero)
- In a data type, the representable value range has been exceeded
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Analyze the program and correct the defective point in the program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14055
[Channel %1: ] Block %2 impermissible NC language substitution, error code %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
This alarm occurs in conjunction with an NC language substitution configured in MD30465 $MA_AXIS_LANG_SUB_MASK.
Error code %3 gives more detailed information about the cause of the problem:
Error code:
1: Several events had been programmed, causing the replacement cycle to be called. Only one substitution is allowed per
part program line.
2: A block-by-block synchronized action had also been programmed for the part program line with the NC language
substitution.
3: The system variables $P_SUB_SPOSIT and $P_SUB_SPOSMODE were called outside a replacement cycle.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Modify the NC program
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
217
NC alarms
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14060
[Channel %1: ] Block %2 invalid skip level with differential block skip
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
With "Differential block skip", a skip level greater than 7 has been specified. (In packet 1 specification of a value for the skip
level is rejected by the converter as a syntax error, i.e. the only possibility is a "Suppress block" ON/OFF on one level).
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Enter a skip level (number behind the slash) less than 8.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14065
[channel %1: ] block %2 error in SPRINT/ISOPRINT command: error code %4 information %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Additional information
%4 = Error code
Explanation:
When interpreting the SPRINT or ISOPRINT command, an error was detected which was described in more detail by
parameter %4. Parameter %3 may supply additional information on the incurring problem.
List of error codes (parameter %4):
1: invalid format description %3 recognized
2: Format %.nP: overrange when converting into 32 bit number
3: Format %P: Character %3 cannot be converted with the code selected by MD 10750 / $MN_SPRINT_FORMAT_P_CODE.
4: Maximum string length of 400 bytes exceeded
5: SPRINT/ISOPRINT command programmed with an invalid number of parameters
6: SPRINT/ISOPRINT parameters programmed with impermissible data type
7: Format %m.nP: overrange due to parameter n with MD 10751 / $MN_SPRINT_FORMAT_P_DECIMAL = 0
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct SPRINT and/or ISOPRINT command(s).
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14066
[channel %1: ] block %2 error when outputting to external device on command %3, error code:
%4
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Part program command
%4 = Error code
Alarms
218
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
When processing the commands ISOOPEN, ISOPRINT, ISOCLOSE or EXTOPEN, WRITE, EXTCLOSE, an error was detected
which is described in detail by the error code.
List of error codes:
1: external device cannot be opened
2: external device is not configured
3: external device configured with invalid path
4: no access rights for external device
5: external device already exclusively assigned
6: external device already assigned in shared mode
7: file length greater than LOCAL_DRIVE_MAX_FILESIZE
8: maximum number of external devices exceeded
9: option not set for LOCAL_DRIVE
11: V24 already occupied by Easy-Message function
12: Append/Overwrite specification is inconsistent with extdev.ini
14: external device not assigned or opened
15: error when writing to external device
16: invalid external path programmed
21: error when closing external device
22: external device not installed (mounted)
90: Timeout
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Correcting the parameterization of the ISOOPEN, ISOPRINT or ISOCLOSE command. See also MD 10830
$MN_EXTERN_PRINT_DEVICE and MD 10831 $MN_EXTERN_PRINT_MODE.
Check the configuration of the external device on the memory card in /user/sinumerik/nck/extdev.ini and /oem/
sinumerik/nck/extdev.ini.
Check the connection and functioning of the external device.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14070
[Channel %1: ] Block %2 memory for variables not sufficient for subroutine call
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A called subroutine cannot be processed (opened), either because the internal data memory to be created for general
purposes is not large enough, or because the available memory for the local program variables is too small. The alarm can
only occur in MDI mode.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Analyze the part program section:
1. Has the most useful data type always been selected in the variable definitions? (For example REAL for data bits is poor;
BOOL would be better)
2. Can local variables be replaced by global variables?
Programm
Clear alarm with the RESET key. Restart part program
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
219
NC alarms
14080
[Channel %1: ] Block %2 jump destination %3 not found
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Jump destination
Explanation:
In conditional and unconditional jumps, the jump destination within the program must be a block with a label (symbolic
name instead of block number). If no jump destination has been found with the given label when searching in the
programmed direction, an alarm is output.
For parameterizable returns with RET to block number or label, the jump destination within the program must be a block
with the block number or label (symbolic name instead of block number).
For returns over several levels (parameter 2), the jump destination must be a block within the program level you jumped to.
For returns with a string as return destination, the search string must be a name known in the control and the search string
must be preceded in the block by a block number and/or a label only.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Check NC part program for the following possible errors:
1. Check whether the target designation is identical with the label.
2. Is the jump direction correct?
3. Has the label been terminated with a colon?
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14082
[Channel %1: ] Block %2 label %3 program section not found
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Start or end label
Explanation:
The start point for repetition of the program part with CALL <program name> BLOCK <start label> TO <end label> has not
been found or the same program part repetition has been called recursively.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Check the start and end labels for programming repetition in the user program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14085
[Channel %1: ] Block %2 instruction not allowed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The instruction 'TML()' may only be used in the subprogram, which replaces the T command.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
220
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14088
[Channel %1: ] Block %2 axis %3 doubtful position
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis name, spindle number
Explanation:
An axis position larger than 3.40e+38 increments has been programmed. This alarm can be suppressed with bit11 in
MD11410 $MN_SUPPRESS_ALARM_MASK.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14089
[Channel %1: ] Block %2 Function %3 is no longer supported.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = String: function
Explanation:
An obsolete function was programmed or triggered, which is no longer supported in the current software version. The
function in question is named in parameter 3.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
COMPON: Replace "COMPON" with "COMPCAD" and check machine data: MD28070
$MC_MM_NUM_BLOCKS_IN_PREP>=80, MD28520 $MC_MM_MAX_AXISPOLY_PER_BLOCK>=3, MD28530
$MC_MM_PATH_VELO_SEGMENTS>=5, MD28540 $MC_MM_ARCLENGTH_SEGMENTS>=10.
COMPCURV: Replace "COMPCURV" with "COMPCAD" and check machine data: MD28070
$MC_MM_NUM_BLOCKS_IN_PREP>=80, MD28520 $MC_MM_MAX_AXISPOLY_PER_BLOCK>=3, MD28530
$MC_MM_PATH_VELO_SEGMENTS>=5, MD28540 $MC_MM_ARCLENGTH_SEGMENTS>=10.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14091
[Channel %1: ] Block %2 illegal function, index %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Index
Explanation:
A function has been programmed or triggered which is not permitted in the current program context. The function in
question is encoded in the "index" parameter:
Index == 1: "RET" command was programmed in the main program level
Index == 2: Conflict between "Cancel level"/"Clear number of passes" and "Implicit GET"
Index == 3: Conflict ASUB start immediately after selection of overstore (up to P3)
Index == 4: MD10760 $MN_G53_TOOLCORR = 1 : SUPA/G153/G53 programmed in G75
Index == 5: POSRANGE command not programmed in synchronized action
Index == 6: SIRELAY command not programmed in synchronized action
Index == 7: GOTOF/GOTOB/GOTO command programmed with string variable in synchronized action.
Index == 8: COA application "Cutting generator" not active
Index == 9: Tool radius compensation active in G75
Index == 10: Number of return levels too big, with RET (...xy) across several program levels
Index == 11: The function is not implemented for this variable
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
221
NC alarms
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Index == 1: Substitute "RET" command with M17/M30
Index == 2: Insert an auxiliary block (e.g. M99) after the subroutine call to which the "Cancel level"/"Clear number of passes"
refers
Index == 3: Overstore an auxiliary block (e.g. M99), then start ASUB (up to P3)
Index == 4: With MD10760 $MN_G53_TOOLCORR = 1: Do not activate SUPA/G53/G153 in the G75 block
Index == 5: Program POSRANGE command in synchronized action
Index == 6: Program SIRELAY command in synchronized action
Index == 7: Program GOTOF/GOTOB/GOTO command with block number or label
Index == 8: Load COA application "Cutting generator"
Index == 9: Tool radius compensation active in G75
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14092
[Channel %1: ] Block %2 axis %3 is wrong axis type
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis name, spindle number
Explanation:
One of the following programming errors has occurred:
1. The keyword WAITP(x) "Wait with the block change until the specified positioning axes has reached its end point", was
used for an axis that is not a positioning axis.
2. G74 "Reference point approach from the program" was programmed for a spindle. (Only axis addresses are permissible.)
3. The keyword POS/POSA was used for a spindle. (For spindle positioning, keywords SPOS and SPOSA should be
programmed.)
4. If the alarm occurs for the function "Thread tapping without compensating chuck " (G331) the following reasons are
conceivable:
- The master spindle is not in position-controlled operation.
- Incorrect master spindle
- Master spindle without encoder
5. An axis name that is no longer available has been programmed, e.g. when using axial variables as index. Or it was
programmed as index NO_AXIS.
6. If 14092 is output as note for alarm 20140 motion synchronized action: traverse the command axis, then the the
following causes are possible:
- The axis is presently being traversed by the NC program.
- An overlaid movement is active for the axis.
- The axis is active as slave axis of a coupling.
- An interpolation compensation such as a temperature compensation is active for the axis.
7. PRESETON/ PRESETONS were programmed for an unknown channel axis.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
- Correct the part program according to which of the above errors is involved.
- Program SPOS.
- Set the correct master spindle with SETMS.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
222
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14093
[Channel %1: ] Block %2 path interval <= 0 with polynomial interpolation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
In the polynomial interpolation POLY, a negative value or 0 has been programmed under the keyword for the polynomial
length PL=...
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Press the NC Stop key and select the function "Correction block" with the softkey PROGRAM CORRECT. The correction pointer
positions on the incorrect block.
Correct the value given in PL = ...
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14094
[Channel %1: ] Block %2 polynomial degree greater than 3 programmed for polynomial
interpolation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The polynomial degree in the polynomial interpolation is based on the number of programmed coefficients for an axis. The
maximum possible polynomial degree is 3, i.e. the axes are according to the function:
f(p) = a0 + a1 p + a2 p2 + a3 p3
The coefficient a0 is the actual position at the start of interpolation and is not programmed!
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Reduce the number of coefficients. The polynomial block may have a form no greater than the following:
N1 POLY PO[X]=(1.11, 2.22, 3.33) PO[Y]=(1.11, 2.22, 3.33)
N1 PO[n]=... PL=44
n ... n ... axis identifier, max. 8 path axes per block
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14095
[Channel %1: ] Block %2 radius for circle programming too small
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The radius entered for radius programming is too small, i.e. the programmed radius is smaller than half of the distance
between start and end point.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14096
[Channel %1: ] Block %2 illegal type conversion
Parameters:
%1 = Channel number
%2 = Block number, label
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
223
NC alarms
Explanation:
During the program run, a variable value assignment or an arithmetic operation has caused data to be processed in such a
way that they have to be converted to another type. This would lead to the value range being exceeded.
Value ranges of the various variable types:
- REAL: Property: Fractional number with dec. pt., value range: +/-(2.2*10e-308 ... 1.8*10e308)
- INT: Property: Integers with signs, value range: -2147483648 ... +2147483647
- BOOL: Property: Truth value FALSE, TRUE, value range: 0 or 1
- CHAR: Property: 1 ASCII character, value range: 0-255
- STRING: Property: Character string (max. length depends on the variable), value range: 0 ... 255
- AXIS: Property: Axis addresses, value range: Channel identifier
- FRAME: Property: Geometric information, value range: ---
Overview of type conversions:
- from REAL to: REAL: yes, INT: yes*, BOOL: yes1), CHAR: yes*, STRING: -, AXIS: -, FRAME: -
- from INT to: REAL: yes, INT: yes, BOOL: yes1), CHAR: if value 0 ...255, STRING: -, AXIS: -, FRAME: -
- from BOOL to: REAL: yes, INT: yes, BOOL: yes, CHAR: yes, STRING: -, AXIS: -, FRAME: -
- from CHAR to: REAL: yes, INT: yes, BOOL: yes1), CHAR: yes, STRING: yes, AXIS: -, FRAME: -
- from STRING to: REAL: -, INT: -, BOOL: yes2), CHAR: only if 1 character, STRING: yes, AXIS: -, FRAME: -
- from AXIS to: REAL: -, INT: -, BOOL: -, CHAR: -, STRING: -, AXIS: yes, FRAME: -
- from FRAME to: REAL: -, INT: -, BOOL: -, CHAR: -, STRING: -, AXIS: -, FRAME: yes
1) Value <> 0 corresponds to TRUE, value ==0 corresponds to FALSE.
2) String length 0 => FALSE, otherwise TRUE.
3) If only 1 character.
It is not possible to convert from type AXIS and FRAME nor into type AXIS and FRAME.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the program section such that the value range is not exceeded, e.g. by a modified variable definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14097
[Channel %1: ] Block %2 string cannot be converted to AXIS type
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The called function AXNAME - conversion of the transferred parameters of the STRING type to an axis name (return value)
of the AXIS type - has not found this axis identifier in the machine data.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Please inform the authorized personnel/service department. Check the transferred parameter (axis name) of the function
AXNAME to determine whether a geometry, channel or machine axis of this name has been configured by means of the
machine data:
MD10000 $MN_AXCONF_MACHAX_NAME_TAB
MD20060 $MC_AXCONF_GEOAX_NAME_TAB
MD20080 $MC_AXCONF_CHANAX_NAME_TAB
Select the transfer string in accordance with the axis name, and change the axis name in the machine data if necessary. (If
a change of name is to take place via the NC part program, this change must first be validated by means of a "POWER-ON").
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14098
[Channel %1: ] Block %2 conversion error: no valid number found
Parameters:
%1 = Channel number
%2 = Block number, label
Alarms
224
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
The string is not a valid INT or REAL number.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program. If it is an entry, you can check whether the string is a number with the predefined ISNUMBER
function with the same parameter.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14099
[Channel %1: ] Block %2 result in string concatenation too long
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The result of the string chaining returns a string which exceeds the maximum string length specified by the system.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Adapt the part program. With the STRLEN function, you can query the size of the sum string before executing the chaining
operation.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14101
[Channel %1: ] Block %2 orientation transformation not active
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Euler angles or a vector have been used in programming an orientation and no orientation transformation is active, i.e. the
keyword TRAORI(n) (n ... number of transformation grouping) is missing.
Example of correct transformation programming:
N100 ... TRAORI(1)
N110 G01 X... Y... ORIWKS
N120 A3... B3... C3...
N130 A3... B3... C3...
:
N200 TAFOOF
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Before the transformation is applied, the number of the transformation grouping must be specified with the keyword
TRAORI(n) (n is between 1 and 4).
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14102
[Channel %1: ] Block %2 polynomial degree greater than 5 programmed for orientation vector
angle
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
During polynomial interpolation for the orientation vector, a polynomial degree larger than 5 has been programmed.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
225
NC alarms
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14103
[Channel %1: ] Block %2 error %3 when calling function CORRTRAFO.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
An error occurred when the CORRTRAFO function was called. The error number specifies the cause of the error.
Error numbers:
1: No transformation active.
2: The current active transformation is not an orientation transformation.
3: The active orientation transformation was not defined with kinematic chains.
10: The call parameter _CORR_INDEX is negative.
11: The call parameter _CORR_MODE is negative.
12: Invalid reference to the section of a partial chain (1st position of _CORR_INDEX). The value must not be greater than the
number of orientation axes in the partial chain.
13: Invalid reference to the orientation axis of a partial chain (1st position of _CORR_INDEX). The value must be less than
the number of orientiation axes in the partial chain.
14: Invalid reference to a partial chain (10th position of _CORR_INDEX). Only the values 0 and 1 are permissible (reference
to part or tool chain). This error number also occurs if the partial chain to which _CORR_INDEX refers, does not exist.
15: In the section referred to with the parameter _CORR_INDEX, no correction element is defined($NT_CORR_ELEM_P or
$NT_CORR_ELEM_T).
20: Invalid correction mode (1st position of _CORR_MODE). Only the values 0, 1, 8, and 9 are permissible.
21: Invalid correction mode (10th and / or 100th position of _CORR_MODE). When reading a system variable, the 100th
position must always be zero. When reading or writing an axis direction, only the one's position is permitted to be not equal
to zero.
30: The 100th position of _CORR_MODE is invalid. Only the values 0 and 1 are permissible.
31: The 1000th position of _CORR_MODE is invalid. Only the values 0 and 1 are permissible.
40: The direction vector to be taken over as the axis direction is the zero vector.
41: In the correction of an offset vector, the deviation from the current value is greater than the maximum value set in setting
data 41610 $SN_CORR_TRAFO_LIN_MAX in at least one coordinate.
42: In the correction of a direction vector, the angle deviation from the current direction is greater than the maximum value
set in setting data 41611 $SN_CORR_TRAFO_DIR_MAX.
43: The attempt to write a system variable was rejected due to missing write authorization.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change function call.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14104
[Channel %1: ] Block %2 Active transformation allows neither vector programming nor
interpolation
Parameters:
%1 = Channel number
%2 = Block number, label
Alarms
226
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
The active orientation transformation does not allow either the programming of vectors for the tool orientation or the vector
interpolation (ORIVECT, ORICONxx, etc.) of the orientation. This is because the set kinematics of the transformation do not
have enough degrees of freedom to represent a general orientation of the tool, although the number of orientation axes
(rotary axes) would be sufficient for this purpose.
This occurs with the following kinematics:
The directions of rotation of 2 successive orientation axes are parallel (see MD24570 $MC_TRAFO5_AXIS1_x[0..2],
MD24572 $MC_TRAFO5_AXIS2_x[0..2] and MD24573 $MC_TRAFO5_AXIS3_x[0..2] (with 6-axis kinematics)).
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Change the NC program and/or the settings of the machine data
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14106
[Channel %1: ] Block %2 Error when calling the ORISOLH function. Error code %3.
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
An error occurred while processing the ORISOLH function call.
An error code defines the cause of the error in more detail:
-2: A valid transformation (6-axis orientation transformation) is not active.
-3: The first parameter of the function ORISOLH (_CNTRL) is negative.
-4: The units digit of the first parameter of the function ORISOLH (_CNTRL) is invalid.
-5: The tens digit of the first parameter of the function ORISOLH (_CNTRL) is invalid.
-6: The hundreds digit of the first parameter of the function ORISOLH (_CNTRL) is invalid.
-7: The thousands digit of the first parameter of the function ORISOLH (_CNTRL) is invalid.
-10: No tool was active when calling the function ORISOLH.
-11: An error occurred when calling the ORISOLH function (extended orientation cannot be set).
-12: The adjustment of the free axis angle for the Hirth tooth system is not possible for the first or only solution.
-13: The adjustment of the free axis angle for the Hirth tooth system is not possible for the second solution.
-14: The adjustment of the free axis angle for the Hirth tooth system is not possible for either of the two solutions.
-15: The first orientation axis is parameterized as a Hirth axis.
-16: Both the second and the third rotary axis are parameterized as Hirth axes. Only one of the two axes can be a Hirth axis.
-17: With the "Swivel direct" function, at least one of the specified axis positions is not compatible with the associated Hirth
tooth system.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Change the NC program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14107
[Channel %1: ] Block %2 illegal position in $NT_ROT_AX_POS[%3,%4].
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Trafo index
%4 = Axis index
Explanation:
The position of the specified manual rotary axis is illegal; in other words, it violates the axis limits defined in
$NT_ROT_AX_MIN / $NT_ROT_AX_MAX.
This alarm may occur if a transformation is selected which uses this axis.
In the case of manual axes with Hirth tooth systems, the transformation may involve a position which, due to the rounding
of the value contained in $NT_ROT_AX_POS, actually relates to the adjacent grid position. The alarm may, therefore, also
occur if the content of $NT_ROT_AX_POS is within permissible limits but the modified position used internally violates these
limits.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
227
NC alarms
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Change the NC program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14109
[Channel %1: ] Block %2 simultaneous linear and rotary axis movement with static
orientation transformation.
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The interpolation type CP (G group code 49) is not permitted with an active static orientation transformation if linear and
rotary axes have to interpolate simultaneously.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Change the NC program:
Activate dynamic orientation transformation.
Change the G code for group 49.
Execute linear and rotary axis movement successively rather than simultaneously.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14110
[Channel %1: ] Block %2 Euler angles and orientation vector components programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
An orientation were programmed with Euler angles and the component of an orientation vector at the same time.
Example:
N50 TRAORI (1)
N55 A2=10 B2=20 C3=50 ; alarm, because Euler angle and orientation vector
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Program only one type, in other words when transformation is switched on program either Euler angles only or orientation
vectors (direction vectors) only.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14111
[Channel %1: ] Block %2 Euler angles, orientation vector and transformation axes
programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
An orientation has been programmed at the same time as Euler angles or components of an orientation vector and the
machine axis influenced by the orientation.
Example:
N50 TRAORI (1)
N55 A2=70 B2=10 C2=0 X50 ; alarm, because Euler angle and axes were programmed
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Alarms
228
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Remedy:
Program only one type, in other words with transformation switched on program either Euler angles only or orientation
vectors (direction vectors) only or deselect transformation (TRAFOOF) and set tool orientation by programming the auxiliary
axes.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14112
[Channel %1: ] Block %2 programmed orientation path not possible, error no. %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
In a 5-axis transformation, the two orientation axes place a coordinate system, comprising lengths and circles of latitude,
on a spherical surface. However, in some cases, the complete orientation sphere cannot be reached by the tool orientation.
This could be the case, for example, if the directions of rotation of the two orientation axes are not perpendicular to one
another. Then, there are usually are up to 2 pole caps on the orientation sphere, the orientation of which cannot be set with
the existing kinematics of the machine. This alarm is output if an orientation is programmed that lies outside the possible
range on the orientation sphere.
A non-settable orientation can only be specified by vector programming (direct programming of the vector components,
Euler or RPY angle, programming with virtual orientation axes), whereas a non-settable orientation cannot arise when the
rotary axis positions are programmed. Non-settable intermediate orientations can also only occur if vector interpolation is
active, whereas it can never occur with rotary axis interpolation. This alarm can therefore never occur if rotary axes are
programmed and the orientation is traversed by means of rotary axis interpolation.
The error number that is also output differentiates between specific situations:
1: The range of settable orientation is limited, but it is not restricted to one plane. This is, for example, the case with "normal"
nutator kinematics CA' with a rotary axis inclined at 45 degrees. The possible orientation range is then restricted to one
hemisphere.
2: The maximum settable orientation range is reduced to one plane. This means that the orientation can only be swiveled
in one plane. This situation is often caused by an incorrect, unwanted configuration of the orientation axes. This is, for
example, the case if the orientation axes are entered in the incorrect order. For example, if the axis sequence AC is specified
for tool kinematics instead of CA. If the initial setting of the tool is in the Z direction, the orientation can only be swiveled
in the YZ plane. This also occurs if the initial setting of the tool points in the X direction for CA tool kinematics.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Change the part program and program an orientation that can be set with the kinematics of the machine. The alarm can also
be caused by an error in the configuration of the orientation axes of the transformation. In this case change the
configuration.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14113
[Channel %1: ] Block %2 programmed lead angle too large
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
No further explanation.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14114
[Channel %1: ] Block %2 programmed tilt angle too large
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
No further explanation.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
229
NC alarms
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14115
[Channel %1: ] Block %2 illegal definition of workpiece surface
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The surface normal vectors programmed at the beginning of block and at the end of block point in opposite directions.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14116
[Channel %1: ] Block %2 absolute orientation programmed while ORIPATH/ORIPATHS is active
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The orientation has been entered as an absolute value (e.g. by a direction vector or a rotation vector), although ORIPATH or
ORIPATHS are active. When ORIPATH/ORIPATHS is active, the orientation is determined from the lead angle, tilt angle and
angle of rotation relative to the path tangent and surface normal vector.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14117
[Channel %1: ] Block %2 no angle or direction of the cone programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
With taper circumference interpolation of orientation (ORICONCW and ORICONCC), either the opening angle or the
direction vector of the taper must be programmed. Otherwise, the change of orientation is not clearly defined.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14118
[Channel %1: ] Block %2 no end orientation programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
With taper circumference interpolation of orientation, no end orientation has been programmed. The change of orientation
is therefore not clearly defined.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Alarms
230
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14119
[Channel %1: ] Block %2 no intermediate orientation programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
With taper circumference interpolation of orientation with ORICONIO, an intermediate orientation must also be
programmed in addition to the end orientation.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14120
[Channel %1: ] Block %2 plane determination for programmed orientation not possible
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The programmed orientation vectors (direction vectors) in the beginning of block and end of block point include an angle
of 180 degrees. Therefore the interpolation plane cannot be determined.
Example:
N50 TRAORI (1)
N55 A3=0 B3=0 C3=1
N60 A3=0 B3=0 C3=-1 ; the vector of this block is precisely opposite to that in the preceding block.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program so that the orientation vectors of a block are not directly opposed to each other, for instance by
dividing the block up into 2 subblocks.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14121
[Channel %1: ] Block %2 no orientation defined (distance equals zero).
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The programmed coordinates for the 2nd space curve with XH, YH, ZH
do not define any tool orientation, as the distance of the curve to the TCP is becoming zero.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Change the part program so that the distance between the two curves is not becoming zero and
that a tool orientation is defined.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14122
[Channel %1: ] Block %2 angle and direction of the cone programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
With taper circumference interpolation of orientation with ORICONCW and ORICONCC, only the opening angle or the
direction of the taper may be programmed. Programming of both in one single block is not allowed.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
231
NC alarms
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14123
[Channel %1: ] Block %2 nutation angle of the cone too small
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
With taper circumference interpolation, the programmed opening angle of the taper must be greater than the half of the
angle between the start and end orientation. Otherwise, a taper cannot be defined.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14124
[Channel %1: ] Block %2 start tangent for orientation is zero
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
With taper circumference interpolation with tangential continuation (ORICONTO), the start tangent of orientation must not
be zero.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14125
[Channel %1: ] Block %2 programmed rotation is not possible
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The programmed rotation of tool orientation cannot be traversed.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14126
[Channel %1: ] Block %2 ORIPATH lift factor impermissible.
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The value programmed with ORIPLF = r is not within the permissible range. The relative retraction factor must lie within
interval 0 <= r < 1.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Alarms
232
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14127
[Channel %1: ] Block %2 rotation programmed several times
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The rotation (3rd degree of freedom of orientation at 6-axis transformations) has been programmed several times.
The rotation is clearly defined by one of the following specifications:
- Specification of the rotary axis positions included in the transformation
- Specification of Euler or RPY angles (A2, B2, C2)
- Specification of the normal orientation vector (AN3, BN3, CN3)
- Specification of the THETA angle of rotation
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14128
[Channel %1: ] Block %2 absolute programming of the orienting rotation with active ORIROTC.
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The rotation of orientation (3rd degree of freedom of orientation for 6-axis transformations) has been programmed with
G code ORIROTC active. This is not possible, as the rotation of orientation is oriented relatively to the path tangent when
ORIROTC is active.
With ORIROTC, it is only possible to program the angle of rotation THETA that indicates the angle
of the rotation vector to the path tangent.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14130
[Channel %1: ] Block %2 too many initialization values given
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
On assigning an array by means of SET, more initialization values than existing array elements have been specified in the
program run.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Reduce the number of initialization values.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
233
NC alarms
14132
[Channel %1: ] Block %2 orientation axes incorrectly configured
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The following error causes can exist:
- The configuration of the orientation axes does not match the machine kinematics. For example if the position measuring
system has not been set for the rotary axes.
- An axis that is required as an orientation axis is currently not available as a path axis.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Adapt the machine data.
Provide the required orientation axes using GET(..) or GETD(..).
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14133
[Channel %1: ] Block %2 G code for orientation definition not allowed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
It is only possible to program a G code of the 50th G code group if MD21102 $MC_ORI_DEF_WITH_G_CODE is set to TRUE.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Adapt machine data.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14134
[Channel %1: ] Block %2 G code for orientation interpolation not allowed: error no. %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
The causes of the errors are specified in more detail by the following error numbers:
1: A G code of the 51st G code group may only be programmed if MD21104 $MC_ORI_IPO_WITH_G_CODE has been set to
TRUE.
2: Also, if the G code ORIANGLE of the 51st group is programmed, MD21102 $MC_ORI_DEF_WITH_G_CODE must be set to
TRUE.
3. The combination of the G code ORIANGLE of the 51st group and ORIAXPOS of the 50th group is not allowed.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Adapt machine data.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14135
[Channel %1: ] Block %2 Programmed offset of the orientation not possible: Error code %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Alarms
234
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
The programmed override of the orientation leads to an invalid tool orientation in the specified block or is not defined. The
programmed offset vector leads to the end orientation of this block becoming a zero vector (vector with the length 0), or
the direction vector of the rotation is not defined.
Possible error codes are:
1: Offset vector $P_OFF_O[i] makes the end orientation a zero vector.
2: Offset vector $P_OFF_R[i] makes the rotation of the orientation a zero vector (occurs only with 6-axis kinematics).
3: An angle of rotation was programmed for the orientation with $P_OFF_O_ANGLE, although the associated rotation vector
$P_OFF_O_DIR[i] is not defined.
4: An angle of rotation was programmed for the rotation of the orientation with $P_OFF_R_ANGLE, although the associated
rotation vector $P_OFF_R_DIR[i] is not defined.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Change the NC program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14136
[Channel %1: ] Block %2 Orientation polynomial is not permitted
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Programming of orientation polynomials both for the angles (PO[PHI], PO[PHI]) and for the coordinates of a reference point
on the tool (PO[XH], PO[YH], PO[ZH]) is not permitted. Orientation polynomials can only be programmed, if an orientation
transformation is active and the orientation is changed by interpolating the vector (ORIVECT, ORICONxxx, ORICURVE/
ORICURINV), i.e. the orientation must not be changed by interpolating the axis (ORIAXES).
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Change the NC program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14137
[Channel %1: ] Block %2 Polynomials PO[PHI] and PO[PSI] are not permitted
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A polynomial for the angles PHI and PSI can only be programmed, if the orientation is interpolated in the plane between start
and end orientation (ORIVECT, ORIPLANE) or on a taper (ORICONxxx). If interpolation type ORICURVE is active, no
polynomials can be programmed for angles PHI and PSI.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Change the NC program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14138
[Channel %1: ] Block %2 Polynomials PO[XH], PO[YH] and PO[ZH] are not permitted
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Polynomials for the coordinates of a reference point on the tool (PO[XH], PO[YH], PO[ZH]) can only be programmed, if
interpolation type ORICURVE/ORICURINV is active. If ORIVECT, ORIPLANE, ORICONxxx is active, no polynomials can be
programmed for coordinates XH, YH and ZH.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
235
NC alarms
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Change the NC program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14139
[Channel %1: ] Block %2 Polynomial for angle of rotation PO[THT] is not permitted
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A polynomial for the angle of rotation of orientation (PO[THT]) can only be programmed, if the active transformation
supports it.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Change the NC program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14140
[Channel %1: ] Block %2 position programming without transformation not allowed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A transformation must be active in order to program position information for an axis position.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Modify the program.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14144
[Channel %1: ] Block %2 PTP movement not allowed, error code %3.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
The desired PTP movement is not possible.
The causes of the errors are described in more detail by the following error codes.
- 1. A PTP interpolation is not possible with the currently active transformation.
- 2. PTP interpolation and tool radius compensation must not be active simultaneously.
- 3. The PTP interpolation types PTPWOC and PTPWOC2 are only permissible with orientation transformations.
- 4. PTP interpolation and COMPSURF must not be active simultaneously.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Modify the program.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
Alarms
236
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14146
[Channel %1: ] Block %2 CP or PTP movement without transformation not allowed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A transformation must be active in order to program a G code, CP or PTP movement.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Modify the program.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14147
[Channel %1: ] Block %2 spline for orientation not possible.
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
If an orientation has been programmed while BSPLINE is active, the interpolation of
tool orientation must be interpolated via a 2nd space curve. This means that G code ORICURVE/ORICURINV
must be active for the interpolation of the orientation.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Change the NC program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14148
[Channel %1: ] Illegal reference system for Cartesian manual traverse
Parameters:
%1 = Channel number
Explanation:
In the SD42650 $SC_CART_JOG_MODE, an illegal value has been entered for the reference system with Cartesian manual
travel.
Reaction:
Alarm display.
Remedy:
Enter a permitted value in the SD42650 $SC_CART_JOG_MODE.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14149
[Channel %1: ] Block %2 Error %3 on selection of the tool carrier with the number %4.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
%4 = Tool carrier number
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
237
NC alarms
Explanation:
An error occurred during the activation of the orientable tool carrier with the stated number, whose geometry data are to
be read from kinematic chains.
The geometry data of a tool carrier are read from kinematic chains if bit0 is set in system data $TC_CARR_KIN_CNTRL[n].
The type of error is indicated more precisely by the number of the error code.
Error code:
1 No kinematic chain elements are available. Remedy: Machine data MD18880 $MN_MM_MAXNUM_KIN_CHAIN_ELEM
must not be equal to zero.
2 An error occurred during the analysis of the kinematic machine model.
3 The tool carrier has an invalid type. Only types "T", "P" and "M" (optionally in upper or lower case) are permissible.
4 No tool chain was specified, this means that system data $TC_CARR_KIN_TOOL_END[n] is empty. For tool carrier types
"T" and "M", this system data must refer to a kinematic chain element.
5 No part chain was specified, this means that system data $TC_CARR_KIN_PART_END[n] is empty. For tool carrier types
"P" and "M", this system data must refer to a kinematic chain element.
6 The kinematic chain element to which the system data $TC_CARR_KIN_TOOL_END[n] refers was not found.
7 The kinematic chain element to which the system data $TC_CARR_KIN_PART_END[n] refers was not found.
8 The kinematic chain element to which the system data $TC_CARR_KIN_TOOL_END[n] refers was found, but it has no
connection to the ROOT element. Kinematic chain elements are only part of the valid machine model if they are connected
to the ROOT element by references.
9 The kinematic chain element to which system data $TC_CARR_KIN_PART_END[n] refers was found, but it has no
connection to the ROOT element. Kinematic chain elements are only part of the valid machine model if they are connected
to the ROOT element by references.
10 The kinematic chain element to which system data $TC_CARR_KIN_TOOL_START[n] refers is not part of the kinematic
chain that forms the connection between the ROOT element and the end point of the tool chain
($TC_CARR_KIN_TOOL_END[n]).
11 The kinematic chain element to which system data $TC_CARR_KIN_PART_START[n] refers is not part of the kinematic
chain that forms the connection between the ROOT element and the end point of the part chain
($TC_CARR_KIN_PART_END[n]).
12 The kinematic chain (tool chain) that forms the connection between the ROOT element and the end point of the tool
chain ($TC_CARR_KIN_TOOL_END[n]) contains too many elements.
13 The kinematic chain (part chain) that forms the connection between the ROOT element and the end point of the part
chain ($TC_CARR_KIN_PART_END[n]) contains too many elements.
14 The kinematic chain (tool chain) that forms the connection between the ROOT element and the end point of the tool
chain ($TC_CARR_KIN_TOOL_END[n]) contains too many rotary axes. With tool carrier type "T", a maximum of 2, with tool
carrier type "M" a maximum of one rotary axis is permissible in this chain.
15 The kinematic chain (part chain) that forms the connection between the ROOT element and the end point of the part
chain ($TC_CARR_KIN_PART_END[n]) contains too many rotary axes. With tool carrier type "P", a maximum of 2, with tool
carrier type "M" a maximum of one rotary axis is permissible in this chain.
16 The kinematic chain (tool chain) that forms the connection between the ROOT element and the end point of the tool
chain ($TC_CARR_KIN_TOOL_END[n]) does not contain any rotary axes. This chain must contain at least one rotary axis.
17 The kinematic chain (part chain) that forms the connection between the ROOT element and the end point of the part
chain ($TC_CARR_KIN_PART_END[n]) does not contain any rotary axes. This chain must contain at least one rotary axis.
18. The kinematic chain (tool chain) for the definition of the tool carrier contains an element of type "AXIS_LIN_VIRT", that
is not permissible for a tool carrier ("virtual" linear axis).
19. The kinematic chain (part chain) for the definition of the tool carrier contains an element of type "AXIS_LIN_VIRT", that
is not permissible for a tool carrier ("virtual" linear axis).
20. The kinematic chain (tool chain) for the definition of the toolcarrier contains an element of type "AXIS_ROT_VIRT", that
is not permissible for a tool carrier ("virtual" rotary axis)).
21. The kinematic chain (part chain) for the definition of the toolcarrier contains an element of type "AXIS_ROT_VIRT", that
is not permissible for a tool carrier ("virtual" rotary axis)
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct the incorrect data in the tool carrier definition or the incorrect definition of the kinematic chains used to parameterise
the tool carrier.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
238
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14150
[Channel %1: ] Block %2 illegal tool carrier number programmed or declared (MD)
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A toolholder number was programmed which is negative or greater than the MD18088 $MN_MM_NUM_TOOL_CARRIER.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Inform the authorized personnel/service department. Program a valid tool carrier number or adapt MD 18088
$MN_MM_NUM_TOOL_CARRIER.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14151
[Channel %1: ] Block %2 illegal tool carrier rotation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A toolholder was activated with an angle of rotation unequal to zero, although the associated axis is not defined. A rotary
axis is not defined when all three direction components are zero.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Set the angle of rotation to zero, or define the associated rotary axis.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14152
[Channel %1: ] Block %2 tool carrier: invalid orientation. Error code: %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
An attempt was made to define a tool orientation by means of the active frame, which cannot be reached with the current
tool carrier kinematics.
This behavior can be caused by the following:
- The two rotary axes of the tool carrier are not perpendicular to one another.
- The tool carrier has less than two rotary axes;
- Rotary axis positions must be set that violate the corresponding axis limitations.
An error code is output with the alarm, which specifies the cause in detail:
1: 1st rotary axis of the first solution violates the lower limit
2: 1st rotary axis of the first solution violates the upper limit
10: 2nd rotary axis of the first solution violates the lower limit
20: 2nd rotary axis of the first solution violates the upper limit
100: 1st rotary axis of the second solution violates the lower limit
200: 1st rotary axis of the second solution violates the upper limit
1000: 2nd rotary axis of the second solution violates the lower limit
2000: 2nd rotary axis of the second solution violates the upper limit
3: The required orientation cannot be set with the given axis configuration
Several of the error codes that indicate a violation of the axis limits can occur simultaneously
As, when an axis limit is violated, an attempt is made to reach a valid position within the permissible axis limits by adding
or subtracting multiples of 360 degrees, it is - if this is not possible - not unequivocally defined whether the lower or upper
axis limit has been violated.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
239
NC alarms
Remedy:
Modify the part program:
- Use TCOABS instead of TCOFR.
- Activate a different frame.
- Change the tool carrier data.
- Change the machining plane G17-G19.
If the alarm cannot be cleared and an additional alarm 14710 is generated at RESET, the machine data 20126
$MC_TOOL_CARRIER_RESET_VALUE must be set to zero.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14153
[Channel %1: ] Block %2 unknown tool carrier type: %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Tool carrier type
Explanation:
An invalid tool carrier type was specified in $TC_CARR23[]. Only the following are allowed: t, T, p, P, m, M.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Change the content of the tool carrier data.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14154
[Channel %1: ] Block %2 The amount of fine correction in parameter %3of the orientable
toolholder %4 is too large
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Invalid parameter of the orientable toolholder
%4 = Number of the orientable toolholder
Explanation:
The maximum permissible value of the fine correction in an orientable toolholder is limited by the MD20188
$MC_TOCARR_FINE_LIM_LIN for linear variables, and by the MD20190 $MC_TOCARR_FINE_LIM_ROT for rotary variables.
The alarm can only occur if the SD42974 $SC_TOCARR_FINE_CORRECTION is not equal to zero.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Enter a valid fine correction value.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14155
[Channel %1: ] Block %2 invalid base frame definition for tool carrier offset
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
If a tool carrier selection causes a change in the table offset, a valid base frame must be defined in order to store this offset.
For more information see machine data MD20184 $MC_TOCARR_BASE_FRAME_NUMBER.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Alarms
240
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Remedy:
You have the following possibilities of eliminating the error:
Change the part program.
Change MD20184 $MC_TOCARR_BASE_FRAME_NUMBER.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14156
[Channel %1: ] Toolholder selection error at reset
Parameters:
%1 = Channel number
Explanation:
The settings in MD20110 $MC_RESET_MODE_MASK require that an active orientable toolholder is maintained after the
reset. This is done by deselecting the old orientable toolholder and then reselecting it with data that may have been
modified. If an error occurs during the reselection, this alarm is issued (as a warning) and then an attempt is made to select
the orientable toolholder in the initial setting. If this second attempt is successful, the reset cycle is continued without any
further alarms.
Typically, the alarm only occurs when the old orientable toolholder has been selected with TCOFR, and its axis directions
have been changed in such a way before the reset that a setting suitable for the associated frame is no longer possible. If
there is another cause for the alarm, this results in an alarm also being issued when attempting to select in the initial setting.
This is then also displayed in plain text.
Reaction:
Alarm display.
Remedy:
Check the program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14157
[Channel %1: ] Block %2 illegal interpolation type with MOVT
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
If MOVT is programmed, linear or spline interpolation (G0, G1, ASPLINE, BSPLINE, CSPLINE). must be active.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Modify the program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14159
[Channel %1: ] Block %2 more than two angles programmed with ROTS or AROTS
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Frame rotations are described using space angles with the language commands ROTS or AROTS. A maximum of two angles
can be programmed.
Reaction:
Correction block is reorganized.
Interpreter stop
Interface signals are set.
Alarm display.
Remedy:
Modify the program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14160
[Channel %1: ] Block %2 tool length selection without geometry axis specification
Parameters:
%1 = Channel number
%2 = Block number, label
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
241
NC alarms
Explanation:
If variant C (tool length acts on the programmed axis) is activated by machine data MD20380
$MC_TOOL_CORR_MODE_G43G44 for tool length compensation with H word and G43/G44 in ISO_2 mode, at least one
geometry axis must be specified.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
You have the following possibilities of eliminating the error:
Change the part program.
Change MD20380 $MC_TOOL_CORR_MODE_G43G44.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14161
[Channel: %1: ] Block%2 Error %3 for call of the function CORRTC.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
An error occurred when the CORRTC function was called. The error number specifies the cause of the error.
Error numbers:
1: No tool carrier active.
2: The active tool carrier was not defined with kinematic chains.
10: The call parameter _CORR_INDEX is negative.
11: The call parameter _CORR_MODE is negative.
12: Invalid reference to the section of a partial chain ( _CORR_INDEX).
13: No correction element is defined in the section to which the _CORR_INDEX parameter refers ($TC_CARR_CORR_ELEM).
20: The 100s digit of _CORR_MODE is invalid. Only the values 0 and 1 are permissible.
21: The 1000s digit of _CORR_MODE is invalid. Only the values 0 and 1 are permissible.
30: In the correction of an offset vector, the deviation from the current value is greater than the maximum value set in setting
data 41612 $SN_CORR_TOCARR_LIN_MAX in at least one coordinate.
31: The attempt to write a system variable was rejected due to missing write authorization.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change function call.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14162
[Channel %1: ] Block %2 error %3 on activation of the CUTMOD or CUTMODK function
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Alarms
242
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
An error occurred during the activation of the CUTMOD or CUTMODK function. The type of error is more closely defined by
the error code number:
For errors with error codes less than 100, MD20125 $MC_CUTMOD_ERR can be used to determine whether the error
condition is to lead to the issue of an alarm, and whether the alarm is only to be displayed or also trigger a program stop.
Errors with error codes greater than or equal to 100 always lead to a program stop.
Error code:
1 No valid cutting direction is defined for the active tool.
2 The cutting edge angles (clearance angle and holder angle) of the active tool are both zero.
3 The clearance angle of the active tool has an impermissible value (less than 0 degrees or greater than 180 degrees).
4 The holder angle of the active tool has an impermissible value (less than 0 degrees or greater than 90 degrees).
5 The tool tip angle of the active tool has an impermissible value (less than 0 degrees or greater than 90 degrees).
6 The cutting edge position - holder angle combination of the active tool is impermissible (with cutting edge positions 1
through 4, the holder angle must be greater than or equal to 90 degrees, with cutting edge positions 5 through 8, it must
be less than or equal to 90 degrees).
7 The tool tip is not located in the machining plane, and the angle GAMMA between the tool tip and machining plane
exceeds the upper limit specified using setting data SD42998 $SC_CUTMOD_PLANE_TOL.
8 The cutting plate is not located in the machining plane. Angle ALPHA is greater than 1 degree. The angle ALPHA is the
angle of rotation around the coordinate axis, which is perpendicular to both the axis of rotation of the angle BETA and the
axis of rotation of the angle GAMMA (with G18 the X axis).
100 The rotation matrix to be used for calculating the modification of the cutting edge position does not describe a pure
rotation, that is it contains mirroring, scaling or shearing.
101 When CUTMODK is activated, there is no valid orientation transformation active. A 5 or 6-axis transformation defined
with kinematic chains must be active.
102 The language command "CUTMODK" was called with an invalid parameter. Only the parameters "NEW", "CLEAR", "ON"
and "OFF" are permitted.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct the tool data of the active tool, or modify the part program.
Alternatively, suppress the alarm for all errors with error numbers less than 100 with the aid of MD20125
$MC_CUTMOD_ERR.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14163
[Channel %1: ] Block %2 Tool carrier: Hirth tooth system is not a divisor of the full circle.
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The value of the Hirth increment (in degrees) in at least one axis is not a divisor of the full angle. This can be a problem for
the display if, for example, a negative solution, which matches the Hirth tooth system, is increased by 360 degrees. The
result is no longer divisible by the Hirth increment.
Reaction:
Alarm display.
Remedy:
Set the angle of rotation to zero, or define the associated rotary axis.
Programm
Clear alarm with the Delete key or NC START.
continuation:
14165
[Channel %1: ] Block %2 selected ISO H/D number %3 does not match tool %4
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = ISO H/D number
%4 = Tool number
Explanation:
When an H or D number is programmed in ISO_2 or ISO_3 mode, it must be available in the active tool. The active tool may
also be the last tool loaded on the master spindle or master toolholder. This alarm is output if there is no H or D number on
this tool.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
243
NC alarms
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Set the ISO H/D number correctly.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14166
[Channel %1: ] Block %2 error %3 when programming a tool length offset with TOFF / TOFFL
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
An error occurred while programming a tool length offset with TOFF or TOFFL. More precise information about the type of
error is given by the error code number:
Error code
1 At least one tool length offset component has been programmed twice in one block (with TOFF).
2 At least one tool length offset component has been programmed twice in one block (with TOFFL).
3 Tool length offset components have been programmed in one block with both TOFF and TOFFL.
4 An index must be declared when a tool length offset is programmed with TOFF, the form TOFF=
is not permissible.
5 An illegal index was declared when programming TOFFL (permissible values 1..3).
6 An illegal axis was declared as the index when programming TOFF. Only geometry axes are permitted. Can also occur
with TRAFOOF if TOFFON is active and no geometry axes are known without transformation.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct errors in program block.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14170
[Channel %1: ] Block %2 illegal interpolation type with tool length compensation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
If tool compensation (G43/G44) is activated in the language mode ISO_M, linear interpolation must be activated as the type
of interpolation.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14180
[Channel %1: ] Block %2 H number %3 is not defined
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = H number of ISO mode
Explanation:
The specified H number is not assigned to a tool (ISO_M).
Alarms
244
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14181
[Channel %1: ] Block %2 ISO tool offset %3 not present
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Offset number
Explanation:
Only relevant in ISO2 and ISO3 modes:
When selecting the tool offset with H or D:
Only tool offsets 1 - 98 are permissible in ISO2 and ISO3 modes.
Exception: The structured cutting edge D1 of the active tool can also be selected with H99 in ISO2 mode or with the offset
component in the tool selection in ISO3 mode.
When writing the tool offset with G10:
Only tool offsets 1 - 98 are permissible in ISO2 and ISO3 modes.
Tool offset H99 can only be written in Siemens programming mode (G290) with $TC_DPx[y,z]=.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Correct NC block and select a permissible tool offset in the range 1 to 98.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14182
[Channel %1: ] Block %2 different values under H and D addresses
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Only relevant in ISO2 mode:
Tool length and tool radius are programmed with H and D. The programming leads to contradictory offset numbers in the
coupled offset memories.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Correct NC block. Only program H or D, or program the same value under H and D addresses.
Set MD10890 $MN_EXTERN_TOOLPROG_MODE, Bit6=1. Different values can then be programmed in the H and D addresses.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14183
[Channel %1: ] Block %2 H and D addresses must be programmed after Siemens offset
Parameters:
%1 = Channel number
%2 = Block number, label
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
245
NC alarms
Explanation:
Only relevant in ISO2 mode:
A tool offset in Siemens mode with D>1 is active and an ISO2 command G43, G44,G49 is applied. Furthermore an ISO
offset with H0 - H99 or D0-D98 must be selected.
The alarm is also output, if MD10890 $MN_EXTERN_TOOLPROG_MODE, bit6=1:
If the Siemens offset memory with H99 or a cutting edge has been selected in Siemens mode, both the tool length and tool
radius offsets will have to be reselected the next time the ISO offset memory is selected.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Correct NC block.
Program H and/or D address in the block.
If MD10890 $MN_EXTERN_TOOLPROG_MODE, bit6=0, only H or D address must be programmed.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14184
[Channel %1: ] Block %2 G44 is not possible with tool offset H99
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Only relevant in ISO2 mode:
The structured D number D1 of the active tool has been selected with H99. These offset values cannot be calculated
negatively with G44.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Correct NC block.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14185
[Channel %1: ] Block %2 D number %3 is not defined
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = D number of ISO mode
Explanation:
The specified D number is not assigned to a tool (language mode ISO_M).
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14186
[Channel %1: ] Block %2 ISO2 mode, and toolcarrier or tool adapter are both active (identifier
%3)
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Identifier
Alarms
246
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
Only relevant in ISO2 mode:
An attempt has been made to activate an ISO2 offset and toolcarrier or tool adapter together.
Identifier 1: ISO2 offset is active (activated in ISO2 mode) and an attempt has been made to activate an additional toolcarrier
in Siemens mode.
Identifier 2: A toolcarrier has been activated in Siemens mode, and a tool offset is now activated in ISO2 mode.
Identifier 3: A tool is active in the adapter in Siemens mode, and a tool offset is now activated in ISO2 mode.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Correct NC block.
For identifier 1: Select a Siemens offset before activating the toolcarrier.
For identifier 2: Deactivate the toolcarrier before selecting a TLC in ISO2 mode.
For identifier 3: Load a tool (T=0) or activate a tool without an adapter before selecting a TLC in ISO2 mode.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14196
[Channel %1: ] Block %2 error %3 on interpreting the contents of $SC_CUTDIRMOD
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
An error has occured during the interpretation of the strings contained in SD42984 $SC_CUTDIRMOD. This setting data is
always read when a new edge is selected. The error code indicates the cause of the error:
1: The string only consists of blanks or a sign
2: Unknown frame name after $P_
3: No colon after the first valid frame name
4: Insufficient memory space for creating a frame internally
5: Invalid frame index
6: Further characters found after complete string
7: Second frame name is missing after the colon
8: Impermissible frame rotation (surface normals are rotated against each other by 90 degrees or more)
9: Invalid frame chain (the first frame must come before the second frame in the frame chain)
10: Invalid axis name
11: Axis is not a rotary axis
12: Invalid string that cannot be assigned to any of the error types 1 to 11
20: Invalid angle statement (numerical value)
30: Invalid angle of rotation (not an integer multiple of 90 degrees)
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Enter valid string in SD42984 $SC_CUTDIRMOD.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14197
[Channel %1: ] Block %2 D number and H number programmed simultaneously
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A D word and H word have been programmed simultaneously.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
247
NC alarms
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14199
[Channel %1: ] Block %2 illegal plane change for tool with diameter component
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
If a tool has a wear or length component which is evaluated as a diameter for the facing axis (bit 0 and/or bit 1 in MD20360
$MC_TOOL_PARAMETER_DEF_MASK is set) and bit 2 of this MD is also set, this tool may only be used in the plane active on
tool selection. A plane change results in an alarm.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Modify the part program.
Reset bit 2 in MD20360 $MC_TOOL_PARAMETER_DEF_MASK.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14200
[Channel %1: ] Block %2 negative polar radius
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
In the endpoint specification of a traversing block with G00, G01, G02 or G03 in polar coordinates, the polar radius entered
for the keyword RP=... is negative.
Definition of terms:
- Specification of end of block point with polar angle and polar radius, referring to the current pole (preparatory functions:
G00/G01/G02/G03).
- New definition of the pole with polar angle and pole radius, referring to the reference point selected with the G function.
G110 ... last programmed point in the plane, G111 ... zero point of the current work, G112 ... last pole
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct NC part program - permissible inputs for the pole radius are only positive absolute values that specify the distance
between the current pole and the block end point. (The direction is defined by the polar angle AP=...).
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14210
[Channel %1: ] Block %2 polar angle too large
Parameters:
%1 = Channel number
%2 = Block number, label
Alarms
248
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
In specifying the endpoints in a traversing block with G00, G01, G02 or G03 in polar coordinates, the value range of the polar
angle programmed under the keyword AP=... has been exceeded. It covers the range from -360 to +360 degrees with a
resolution of 0.001 degrees.
Definition of terms:
- Specification of end of block point with polar angle and polar radius, referring to the current pole (preparatory functions:
G00/G01/G02/G03).
- New definition of the pole with polar angle and pole radius, referring to the reference point selected with the G function.
G110 ... referred to the last programmed point in the plane, G111 ... referred to the zero point of the current workpiece
coordinate system (Work), G112 ... referred to the last pole.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct NC part program. The permissible input range for the polar angle is between the values -360 degrees and +360
degrees with a resolution of 0.001 degrees.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14250
[Channel %1: ] Block %2 negative pole radius
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
In redefining the pole with G110, G111 or G112 in polar coordinates, the pole radius specified under keyword RP=... is
negative. Only positive absolute values are permitted.
Definition of terms:
- Specification of end of block point with polar angle and polar radius, referring to the current pole (preparatory functions:
G00/G01/G02/G03).
- New definition of the pole with polar angle and pole radius, referring to the reference point selected with the G function.
G110 ... last programmed point in the plane, G111 ... zero point of the current work, G112 ... last pole
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct the NC part program. Permissible inputs for the pole radius are only positive, absolute values that specify the
distance between the reference point and the new pole. (The direction is defined with the pole angle AP=...).
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14260
[Channel %1: ] Block %2 pole angle too large
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
In redefining the pole with G110, G111 or G112 in polar coordinates, the value range of the pole angle specified under
keyword AP=... has been exceeded. It covers the range from -360 to +360 degrees with a resolution of 0.001 degrees.
Definition of terms:
- Specification of end of block point with polar angle and polar radius, referring to the current pole (preparatory functions:
G00/G01/G02/G03).
- New definition of the pole with polar angle and pole radius, referring to the reference point selected with the G function.
G110 ... last programmed point in the plane, G111 ... zero point of the current work, G112 ... last pole
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct NC part program. The permissible input range for the polar angle is between the values -360 degrees and +360
degrees with a resolution of 0.001 degrees.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
249
NC alarms
14270
[Channel %1: ] Block %2 pole programmed incorrectly
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
When defining the pole, an axis was programmed that does not belong to the selected processing level. Programming in
polar coordinates always refers to the plane activated with G17 to G19. This also applies to the definition of a new pole with
G110, G111 or G112.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct the NC part program. Only the two geometry axes may be programmed that establish the current machining plane.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14280
[Channel %1: ] Block %2 polar coordinates programmed incorrectly
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The end point of the displayed block has been programmed both in the polar coordinate system (with AP=..., RP=...) and in
the Cartesian coordinate system (axis addresses X, Y,...).
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct the NC part program - the axis motion may be specified in one coordinate system only.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14290
[Channel %1: ] Block %2 polynomial degree greater than 5 programmed for polynomial
interpolation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A polynomial degree greater than five was programmed for the polynomial interpolation. You can only program polynomials
up to the 5th degree.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14300
[Channel %1: ] Block %2 overlaid handwheel motion activated incorrectly
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Handwheel override has been called up incorrectly:
- 1st For positioning axes:
- Handwheel override programmed for indexing axes,
- No position programmed,
- FA and FDA programmed for the same axis in the block.
- 2nd For contouring axes:
- No position programmed,
- G60 not active,
- 1st G group incorrect (only G01 to CIP).
Alarms
250
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14320
[Channel %3: ] Axis %4: handwheel %1 used twice (%2)
Parameters:
%1 = Handwheel number
%2 = Use
%3 = Channel
%4 = Axis
Explanation:
Informational alarm indicating that the mentioned handwheel is used twice:
The second parameter provides the explanation:
1: Block with axial handwheel override for this axis cannot be executed as the handwheel
for this axis performs a DRF movement
2: Block with velocity override of the path cannot be executed as the handwheel performs
a DRF movement for this axis of the path
3: Block with contour handwheel cannot be executed as the handwheel performs a DRF movement
for this axis of the path
4: PLC axis with axial handwheel override cannot be started immediately as the handwheel performs
a DRF movement for this axis
5: The axis is a reciprocating axis with axial handwheel override; the reciprocating movement cannot be
started immediately as the handwheel performs a DRF movement for this axis
6: The DRF movement for this axis cannot be executed as an axial handwheel override is active for
this axis with the handwheel
7: The DRF movement for this axis cannot be executed as a velocity override of the path with
the handwheel is active and the axis belongs to the path
8: The DRF movement for this axis cannot be executed as the contour handwheel is active with
this handwheel and the axis belongs to the path
9: The DRF movement for this axis cannot be executed as the axis is a PLC axis with handwheel
override that is active with this handwheel
10: The DRF movement for this axis cannot be executed as the axis is active as reciprocating axis
with handwheel override with this handwheel
Reaction:
Alarm display.
Remedy:
Use the handwheel for one purpose at a time only.
Programm
Alarm display showing cause of alarm disappears. No further operator action necessary.
continuation:
14400
[Channel %1: ] Block %2 tool radius compensation active at transformation switchover
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A change of transformation is not allowed when tool radius compensation is active.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Perform tool radius compensation in the NC part program with G40 (in a block with G00 or G01) before performing a
transformation change.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
251
NC alarms
14401
[Channel %1: ] Block %2 transformation not available. Error code %3.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
The required transformation is not available. The cause of the error is explained more closely by the error code.
1: No transformations are available.
2: No transformations of the type "inclined axis" are available.
3: No orientation transformations are available.
4: No transmit transformations are available.
5: No tracyl transformations are available.
6: No chained transformations are available.
7: No OEM transformations are available.
8: No OEM orientation transformations are available.
22: The required transformation of the type "inclined axis" was not found.
23: The required orientation transformation was not found.
24: The required transmit transformation was not found.
25: The required tracyl transformation was not found.
26: The required chained transformation was not found.
40: An attempt was made to activate a transformation defined by kinematic chains. However, no such transformations have
been enabled (MD18866 $MN_MM_NUM_KIN_TRAFOS is zero).
41: No transformation name (first call parameter) was specified for the transformation call TRAFOON.
42: An attempt was made to activate a transformation defined by kinematic chains. However, no such transformation with
the specified name was found.
43: An attempt was made to activate a transformation defined by kinematic chains whose name had been changed since
the last activation. Changed transformation data does not become active until after a NEWCONF or RESET.
44: An attempt was made to activate a transformation defined by kinematic chains. But the stated name is empty (zero
string).
45: An attempt was made to activate a transformation defined by kinematic chains. However, the system variables
$NT_NAME[..] are all empty.
46: An attempt was made to activate a transformation defined by kinematic chains. The stated transformation name was
found more than once in the array of system variables $NT_NAME.
52: An attempt was made to activate a RESET transformation defined by kinematic chains (MD20142
$MC_TRAFO_RESET_NAME). However, no transformation was found with the stated name.
55: An attempt was made to activate a RESET transformation defined by kinematic chains (MD20142
$MC_TRAFO_RESET_NAME). However, the system variables $NT_NAME[..] are all empty.
56: An attempt was made to activate a RESET transformation defined by kinematic chains (MD20142
$MC_TRAFO_RESET_NAME). However, the stated transformation name was found more than once in the array of system
variables $NT_NAME.
201: A transformation has been incorrectly parameterized.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Error codes 1 to 6 indicate that the control does not contain the requisite software. The transformation cannot even be
activated by setting machine or option data.
For the remaining error codes:
Modify part program; program defined transformations only.
Check MD24... $MC_TRAFO_TYPE_... (assigns the transformation to the part program operation).
Programm
Clear alarm with the RESET key. Restart part program
continuation:
Alarms
252
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14402
[Channel %1: ] Block %2 spline active at transformation change
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A change of transformation is not allowed in a spline curve section. A series of spline blocks must be concluded.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14404
[Channel %1: ] Block %2 illegal parameterization of transformation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Error has occurred when selecting transformation.
Possible causes of error:
- An axis traversed by the transformation has not been enabled:
- is being used by another channel (-> enable)
- is in spindle mode (-> enable with SPOS)
- is in POSA mode (-> enable with WAITP)
- is concurrent Pos axis (-> enable with WAITP)
- Parameterization via machine data has an error
- Axis or geometry axis assignment to the transformation has an error,
- Machine data has an error (-> modify machine data, restart)
Please note: Any axes not enabled might be signaled via alarm 14092 or alarm 1011 instead of alarm 14404.
Transformation-dependent error causes can be in: TRAORI: -
TRANSMIT:
- The current machine axis position is unsuitable for selection (e.g. selection in the pole) (-> change position slightly).
- Parameterization via machine data has an error.
- Special requirement with respect to the machine axis has not been fulfilled (e.g. rotary axis is not a modulo axis) (-> modify
machine data, restart).
TRACYL:
The programmed parameter is not allowed when transformation is selected.
TRAANG:
- The programmed parameter is not allowed when transformation is selected.
- Parameterization via machine data has an error.
- Parameter is faulty (e.g. TRAANG: unfavorable angle value (-> modify machine data, restart)
Persistent transformation:
- Machine data for persistent transformation are wrong (-> consider dependencies, change machine data, restart)
Only with active "OEM transformation" compile cycle:
The axes included in the transformation must be referenced.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Please inform the authorized personnel/service department. Modify part program or machine data.
Only with active "OEM transformation" compile cycle:
Reference the axes included in the transformation before selecting transformation.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
253
NC alarms
14406
[Channel %1: ] Block %2 Parameter error %3 on calling a transformation.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
An error was detected during the attempt to activate a transformation. The cause of the error is indicated more precisely by
the following error code.
-
80. The geometry axes are (almost) linearly dependent. This means that two geometry axes are almost parallel or three
geometry axes lie almost in one plane.
-
81. An orientation axis is impermissible or not completely parameterized as a spindle (with $NT_CNTRL,
$NT_ROT_AX_CNT).
-
90. More than one inclined axis was parameterized in the definition of a TRANSMIT or TRACYL transformation with
kinematic chains.
-
91. Impermissible direction of an inclined axis in the definition of a TRANSMIT or TRACYL transformation with kinematic
chains. The inclined axis does not lie in a main plane.
-
92. The polar axis and the longitudinal axis are not parallel in a TRANSMIT or TRACYL transformation.
-
93. The radial axis must be perpendicular to the polar axis if no longitudinal axis is present.
-
94. The center offset axis must be perpendicular to the polar axis if no longitudinal axis is present.
- 120. During the redirection of a TRAANG transformation to a transformation defined by kinematic chains, a parameter was
stated as an angle that was not the same as the angle defined by the kinematic chains.
- 121. During the redirection of a TRAANG transformation to a transformation defined by kinematic chains, a parameter was
stated as an angle, although the angle of the inclined axis was not defined. This case occurs if there is more than one inclined
axis or if the inclined axis does not lie in a main plane.
-
150. The call of a TRACYL transformation did not state a value for the reference or work diameter.
-
200. The transformation can only be activated in a transformation chain, and not as a single transformation.
- 250. The spindle rotation vector is not parallel to the Z axis of the WCS (see $NT_P_CHAIN_LAST_ELEM). The element to
be entered here must be the last element in the table chain that is not a rotary axis. (If the part of the table chain before
$NT_P_CHAIN_LAST_ELEM contains rotary axes, WKS jumps will occur, which (as described above) violate the prerequisites
for activation).
***************************************************
The following error codes are only output with OEM transformations if an error is detected during the selection of the
transformation:
- 1000. The basic direction of the tool orientation must be parallel to one of the coordinate axes X, Y or Z.
- 1001. The basic direction of the tool orientation must not point in the X direction.
- 1002. The basic direction of the tool orientation must not point in the Y direction.
- 1003. The basic direction of the tool orientation must not point in the Z direction.
- 1004. The normal vector of the tool in the basic position must be parallel to one of the coordinate axes X, Y or Z.
- 1005. The normal vector of the tool in the basic position must not point in the X direction.
- 1006. The normal vector of the tool in the basic position must not point in the Y direction.
- 1007. The normal vector of the tool in the basic position must not point in the Z direction.
Note: Error codes 1000 to 1007 can only occur if $NC_IGNORE_TOOL_ORIENT = FALSE (default value), and the active tool
contains orientations that are not permissible.
In this case, basic directions defined in the variables $NT_BASE_ORIENT and $NT_BASE_ORIENT_NORMAL do not become
active
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Correct incorrect parameterisation.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
Alarms
254
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14407
[Channel %1: ] Block %2 constant axis %3 has an invalid position
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis name, spindle number
Explanation:
An axis with a position that must not be changed during active transformation, has an impermissible position when the
transformation is activated.
The permissible positions are described in the relevant documentation of the transformation.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
- Before activation of the transformation, traverse the affected axis to a permissible position.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14408
[Channel %1: ] Block %2 Transformation TRAINT and function cannot be active
simultaneously. ( %3 )
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
TRAINT cannot be operated with the following functions.
-
10. CUT3DC, CUT3DF, CUT3DCD, CUT3DFF, CUT3DFS, CUT3DCC, CUT3DCCD, CUT3DFD
-
20. PTP, PTPG0, PTPWOC, PTPWOC2
-
30. G17, G19
-
40. G33, G331, G332, G334, G335, G34, G35
-
50. TOFFON
-
60. TOWMCS, TOWWCS, TOWBCS, TOWTCS, TOWKCS
-
70. DIAMONA, DIACYCOFA, DIAM90A, DIAMOFA
-
80. G63
-
90. G961, G962, G97, G971, G972
-
100. LFON
-
110. DRIVE
-
120. NPV (G54, G55, etc.), TRANS, ROT, MIRROR, SCALE, ATRANS, AROT, AMIRROR, ASCALE
-
130. G53, G153, SUPA, SUPD
-
140. The tool type must lie between 500 and 599.
-
150. SPCOF
-
160. Extended lookahead is active MD20443 $MC_LOOKAH_FFORM[n]=1, n=G-code group 59
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Eliminate the incorrect parameterization.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14409
[Channel %1: ] Block %2: Transformation TRAINT has detected a y-WCS position %3 unequal
to 0.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = y-WCS position
Explanation:
The programmed positions result in a y-WCS position unequal to 0 during active transformation.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
255
NC alarms
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Program the axes or the spindle so that y in the WCS is 0, taking into account the correct tool lengths.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14410
[Channel %1: ] Block %2 spline active at geometry axis changeover
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
It is not allowed to change the assignment of geometry axes to channel axes in a spline curve definition.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14411
[Channel %1: ] Block %2 tool radius compensation active at geometry axis changeover
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
It is not permissible to change the assignment of geometry axes to channel axes when tool radius compensation is active.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14412
[Channel %1: ] Block %2 transformation active at geometry axis changeover
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
It is not permissible to change the assignment of geometry axes to channel axes when transformation is active.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14413
[Channel %1: ] Block %2 fine tool correction: changeover geometry/channel axis not allowed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
It is not permissible to change the assignment of geometry axes to channel axes during active tool fine compensation.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program.
Alarms
256
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14414
[Channel %1: ] Block %2 GEOAX function: incorrect call
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The parameters for calling the GEOAX(...) are incorrect.
Possible causes:
- Uneven number of parameters.
- More than 6 parameters were specified.
- A geometry axis number was programmed which was less than 0 or greater than 3.
- A geometry axis number was programmed more than once.
- An axis identifier was programmed more than once.
- An attempt was made to assign a channel axis to a geometry axis which has the same name as one of the channel axes.
- An attempt was made to assign a channel axis to a geometry axis lacking IPO functionality (see MD30460
$MA_BASE_FUNCTION_MASK, Bit8).
- An attempt was made to remove a geometry axis with the same name as one of the channel axes from the geometry axis
grouping.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify the part program or the correction block.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14415
[Channel %1: ] Block %2 tangent control: changeover geometry/channel axis not allowed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
An assignment change of the geometry axes to channel axes is not permitted with active tangential control.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Change part program and delete active tangential control with TANGDEL.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14420
[Channel %1: ] Block %2 index axis %3 frame not allowed
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis
Explanation:
The axis is to be traversed as an indexing axis, but a frame is active. This is not allowed by MD32074
$MA_FRAME_OR_CORRPOS_NOTALLOWED.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Inform the authorized personnel/service department.
Modify the part program.
Change MD32074 $MA_FRAME_OR_CORRPOS_NOTALLOWED.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
257
NC alarms
14430
[Channel %1: ] Block %2 tangential axis %3 must not be traversed as POS axis
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis name
Explanation:
A tangentially followed-up axis cannot be traversed as positioning axis.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Change part program and delete active tangential control with TANGDEL.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14432
[Channel %1: ] Block %2 Rounding length for tangential axis %3 is too small.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis name
Explanation:
For a tangential axis that is coupled during preparation, a rounding length must be indicated with TANGON() on activating
the tangential control, or possibly occuring discontinuities of the tangential axis cannot be smoothed. This rounding length
must be larger than 1 increment.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14434
[Channel %1: ] Block %2 rel. lift-off path for tangential axis %3 is invalid
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis name
Explanation:
Factor r as programmed on TLIFT for the relative lift-off path must be within range 0 =< r < 1.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14500
[Channel %1: ] Block %2 illegal DEF or PROC instruction in the part program
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
NC part programs with high-level language elements are divided into a preceding definition part followed by a program part.
The transition is not marked specifically; a definition statement is not allowed to follow the 1st program command.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Put definition and PROFC statements at the beginning of the program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
258
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14510
[Channel %1: ] Block %2 PROC instruction missing on subroutine call
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
In subroutine calls with parameter transfer ("call-by-value" or "call-by-reference") the called subroutine must begin with a
PROC statement.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Define the subroutine in accordance with the type used.
1. Conventional subroutine structure (without parameter transfer):
% SPF 123456
:
M17
2. Subroutine structure with keyword and subroutine name (without parameter transfer):
PROC UPNAME
:
M17
ENDPROC
3. Subroutine structure with keyword and subroutine name (with parameter transfer "call-by-value"):
PROC UPNAME (VARNAME1, VARNAME2, ...)
:
M17
ENDPROC
4. Subroutine structure with keyword and subroutine name (with parameter transfer "call-by-reference"):
PROC UPNAME (Typ1 VARNAME1, Typ2 VARNAME2, ...)
:
M17
ENDPROC
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14520
[Channel %1: ] Block %2 illegal PROC instruction in data definition section
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The PROC statement may only be programmed at the beginning of the subroutine.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify NC part program appropriately.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14530
[Channel %1: ] Block %2 EXTERN and PROC instruction do not correspond
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Subroutines with parameter transfer must be known before they are called in the program. If the subroutines are always
available (fixed cycles) the control establishes the call interfaces at the time of system power-up. Otherwise an EXTERN
statement must be programmed in the calling program.
Example:
N123 EXTERN UPNAME (TYP1, TYP2, TYP3, ...)
The type of the variable must match the type given in the definition (PROC statements) or it must be compatible with it. The
name can be different.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
259
NC alarms
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Check the variable types in the EXTERN and the PROC statements for correspondence and correctness.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14540
[Channel %1: ] Block %2 contour tool: the min. limit angle has been programmed more than
once (edge D%3)
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Edge number, label
Explanation:
The limit angle of a contour tool must be unequal zero in an involved edge only.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change tool definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14541
[Channel %1: ] Block %2 contour tool: the max. limit angle has been programmed more than
once (edge D%3)
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Edge number, label
Explanation:
The limit angle of a contour tool must be unequal zero in an involved edge only.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change tool definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14542
[Channel %1: ] Block %2 contour tool: the min. limit angle has not been programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
On defining a contour tool, either no limit angle must be indicated, or both the minimum and the maximum limit angle must
be programmed once for each.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change tool definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
260
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14543
[Channel %1: ] Block %2 contour tool: the max. limit angle has not been programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
On defining a contour tool, either no limit angle must be indicated, or both the minimum and the maximum limit angle must
be programmed once for each.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change tool definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14544
[Channel %1: ] Block %2 contour tool: edge D%3 is not positioned between the two border
edges
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Edge number, label
Explanation:
On defining a form tool with limit, all edges must be positioned between the edge with the minimum limit angle and the
edge with the maximum limit angle when rotating counter-clockwise.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change tool definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14545
[Channel %1: ] Block %2 contour tool: edge D%3 completely encircles edge D%4
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Edge number, label
%4 = Edge number, label
Explanation:
On defining a contour tool, tangents are placed on the adjacent circular edges. It will not be possible, if one edge is
completely encircled by another one.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change tool definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14546
[Channel %1: ] Block %2 contour tool: edge D%3 defines a concave corner
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Edge number, label
Explanation:
The contour of a contour tool must be convex throughout, i.e. there must not be any concave corners.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
261
NC alarms
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change tool definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14547
[Channel %1: ] Block %2 contour tool: checksum erroneous or not available
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
When MD20372 $MC_SHAPED_TOOL_CHECKSUM was set, no edge was found for which the tool length components and
the tool radius equal the negative sum of the previous edges.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Check tool definition. An edge must exist, the tool length components and tool radius of which equal the negative sum of
the previous edges. This will not take the tool length components of the first edge into consideration. On comparing the
components, the relevant sums of basic value and wear value are compared with each other, not the part components
themselves.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14548
[Channel %1: ] Block %2 contour tool: negative radius in edge D%3 is not allowed
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Edge number, label
Explanation:
No negative radii are permitted for contour tools, i.e. the sum of basic radius and wear value must be at least 0.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Check tool definition. Change edge radius.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14549
[Channel %1: ] Block %2 contour tool: impermissible programming. Code no. %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Alarms
262
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
Impermissible programming has been found for contour tools on active tool radius compensation. The error cause is
explained in detail by the error code.
1: In G code group 17, KONT is active during activation
2: In G code group 17, KONT is active during deactivation
9: In G code group 40, CUTCONOF is not active
10: Reprogramming of G41 / G42 in already active tool radius compensation not permissible
20: Circle with more than one rotation not permissible
21: Ellipse (circle not in compensation level)
23: Involute not permissible
24: Several polynomials not permitted in one block only. These blocks could be created by e.g. COMPCAD or G643.
30: Preprocessing stop not permitted
41: Starting point of first compensation block cannot be reached by anyone of the defined cutting edges
42: End point of last compensation block cannot be reached by anyone of the defined cutting edges
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change the NC program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14550
[Channel %1: ] Block %2 contour tool: impermissible tool contour change. Code no. %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error code
Explanation:
A new tool with deviating tool contour was activated for contour tools on active tool radius compensation
The error cause is explained further by an error code.
If the error code is an integer, the lower-value three decimal places specify the number of the edge, in which the error was
detected, while the thousandth digit explains the reason in more detail.
-1: The tool was deleted.
-2: The number of contour elements (edges) explaining the tool, has changed.
1000: The edge center has changed
2000: The edge radius has changed.
3000: The initial angle has changed.
4000: The final angle has changed.
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Change the NC program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14551
[Channel %1: ] Block %2 contour tool: angle area of edge D%3 larger than 359 degrees
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Edge number, label
Explanation:
A single edge must cover a max. angle area of 359 degrees.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
263
NC alarms
Reaction:
Correction block is reorganized.
Local alarm reaction.
Interface signals are set.
Alarm display.
NC Stop on alarm at block end.
Remedy:
Check tool definition.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14600
[Channel %1: ] Block %2 reload buffer %3 cannot be established
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = File name
Explanation:
The download buffer for "execute from external" could not be created. Possible causes:
- Not enough memory available (for minimum see MD18360 $MN_MM_EXT_PROG_BUFFER_SIZE)
- No resources available for HMI NCK communication (see MD18362 $MN_MM_EXT_PROG_NUM)
- The file already exists
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
- Release memory, e.g. by deleting part programs
- Modify MD18360 $MN_MM_EXT_PROG_BUFFER_SIZE and/or MD18362 $MN_MM_EXT_PROG_NUM.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14601
[Channel %1: ] Block %2 reload buffer could not be deleted
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The reload buffer for "Execute from external" could not be deleted because, for example, communication with HMI/PLC had
not been terminated.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
To clear all reload buffers, perform a power on.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14602
[Channel %1: ] Block %2 timeout while reloading from external.
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
No connection could be made to the HMI while reloading EXTCALL external subprograms or executing from external drives
within the monitoring time set in MD10132 $MN_MMC_CMD_TIMEOUT.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
- Check the connection to the HMI
- Increase the monitoring time in MD10132 $MN_MMC_CMD_TIMEOUT.
Alarms
264
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14603
[Channel %1: ] Block %2 timeout during execution from external source.
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
If a program is selected for execution from an external source, it is assumed that the first part program line can be read from
the reload buffer within 60s after the part program has started.
Otherwise, part program processing will be canceled with alarm 14603 based on the assumption that the connection to the
HMI or the external device is faulted.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Check the connection to the HMI and repeat selection of the program that is to be executed from external source.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
- Acknowledge the alarm by pressing the RESET key
- Repeat program selection
- Start the part program
14615
[Channel %1: ] An error occurred while handling the function 'syntax check': identifier %3
Parameters:
%1 = Channel number
%2 = Is not used
%3 = Error code
Explanation:
An error occurred while handling the function syntax check via the PI services _N_CHKSEL, _N_CHKRUN, _N_CHKABO and
_N_SEL_BL. Parameter %3 describes the error situation more closely:
Value
1: An invalid line number was transferred with the PI service _N_SEL_BL
2: An invalid line number for the range end was transferred with the PI service _N_CHKRUN
3: PI service _N_CHKSEL was activated although a block selection (PI service _N_SEL_BL) was active for the selected program.
Reaction:
Alarm display.
Remedy:
Value
1: Supply PI service _N_SEL_BL with the correct line number
2: Supply PI service _N_CHKRUN with the correct line number for the range end
3: Ensure that the channel is in reset status before activating the PI service _N_CHKSEL.
Programm
Clear alarm with the Delete key or NC START.
continuation:
14620
[Channel %1: ] Block %2 Error on opening program %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Program name
Explanation:
Program %3 cannot be executed because it has been locked by another application, e.g. HMI Editor.
Background: Program %3 is stored on an external data medium (CF Card, network drive, USB device), and should be
executed from there in EES mode (execution from external storage). However, program %3 cannot be edited because it is
locked by another application, e.g. HMI Editor, is open for writing and WRITE lock is set for this file.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
- Cancel program with Reset
- Close the application that set the WRITE lock, for example the HMI Editor, and continue program editing with NC Start.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
265
NC alarms
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14621
[Channel %1: ] Block %2 Timeout on access to external program %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Program name
Explanation:
Program %3 is stored on an external data medium (CF card, network drive, USB device). A timeout occurred when the
program was accessed.
Possible cause of error: network disturbance.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
- Rectify network disturbances if applicable
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14622
[Channel %1: ] Access to file %2 disrupted by %3 %4
Parameters:
%1 = Channel number
%2 = File which could not be accessed
%3 = Function with which it is accessed
%4 = Error message
Explanation:
The program is stored on an external data medium (CF card, network drive, USB device). An error occurred when the
program was accessed.
Possible cause of error: network disturbance.
Reaction:
Alarm display.
Remedy:
- Rectify network disturbances if applicable
Programm
Clear alarm with the Delete key or NC START.
continuation:
14623
The EES library does not exist
Explanation:
The EES library does not exist; no part programs can be executed with EES.
Reaction:
Channel not ready.
Alarm display.
Remedy:
Load EES library
Programm
Switch control OFF - ON.
continuation:
14624
The EES library is incompatible.
Explanation:
The EES library is incompatible; no part programs can be executed with EES.
Reaction:
Channel not ready.
Alarm display.
Remedy:
Replace EES library
Programm
Switch control OFF - ON.
continuation:
14625
[Channel %1: ] Block %2 Problems in EES mode accessing file %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = File which could not be accessed
Alarms
266
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
The program is located on an external data medium (network drive, USB device). Problems occurred when accessing the
program.
Possible cause or error: network fault.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
- if necessary, remedy network faults und resume program
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14650
[Channel %1: ] Block %2 SETINT instruction with invalid ASUB input
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Asynchronous subroutines (ASUBs) are subroutines that are executed following a hardware input (interrupt routine started
by a rapid NC input).
The NC input number must lie between 1 and 8. It is assigned a priority from 1 to 128 (1 is the highest priority) in the SETINT
instruction with the keyword PRIO =
Example:
If NCK input 5 changes to "1 signal", the subroutine AB-HEB_ Z should be started with the highest priority.
N100 SETINT (5) PRIO = 1 ABHEB_Z
Restriction for SW PLC2xx: The number of the NCK input must be 1 or 2.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Program the NC input of the SETINT statement with a value of not less than 1 or greater than 8.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14660
[Channel %1: ] Block %2 SETINT instruction with invalid priority
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The NC input number must lie between 1 and 8. It is assigned a priority from 0 to 128 (1 is the highest priority) in the SETINT
instruction with the keyword PRIO =
Example:
If NC input 5 changes to "1-signal" the subroutine ABHEB_ Z should be started with the highest priority.
N100 SETINT (5) PRIO = 1 ABHEB_Z
Restriction for SW PLC2xx: The number of the NC input must be 1 or 2.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Program the priority of the NC input with a value of not less than 1 or greater than 128.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14700
[Channel %1: ] Block %2 timeout during command to interpreter
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A timeout has occurred in control-internal commands such as ANWAHL (part program selection), RESET (channel reset),
REORG (reorganization of the preprocessing buffer) and NEWCONFIG (change in the configuration-specific machine data =
restart).
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
267
NC alarms
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Please inform the authorized personnel/service department.
If the runtime error occurred as the result of a temporary excessive load on the system (e.g. in the HMI area or in OEM
applications) error-free execution is possible on if the program or operator action are repeated.
If you experience such a system error, please contact Technical Support.
Please supply the following information to ensure quick processing:
- Alarm number together with alarm text
- Description of the operation/mode before the alarm message
- Generate log files using the key combination: <Ctrl> + <Alt> + <D>
Programm
Switch control OFF - ON.
continuation:
14701
[Channel %1: ] Block %2 number of available NC blocks reduced by %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Number of non-available blocks
Explanation:
After the reset, it was found that the number of available blocks has decreased compared with the last reset. This is due to
a system error. The part program execution can be resumed after acknowledging the alarm. If the number of blocks no
longer available is less than MD28060 $MC_MM_IPO_BUFFER_SIZE, then the PowerON alarm 14700 is output.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Proceed as in the case of a system error.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14710
[Channel %1: ] Block %2 error in initialization sequence in function %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Identifier of the function which caused the error
Alarms
268
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
Initialization blocks are generated (or not) after control power-up, (program) RESET and (program) START, depending on the
settings in machine data MD20110 $MC_RESET_MODE_MASK and MD20112 $MC_START_MODE_MASK.
Errors can occur because of incorrect machine data settings. The errors are output with the same error messages as would
appear if the function had been incorrectly programmed in the part program.
This alarm is also generated in order to indicate that an error relates to the initialization sequence.
Parameter %3 specifies which function triggers the alarm:
Control power-up and (program) RESET:
Value:
0: Error during synchronization preprocessing/main run
1: Error on selection of tool length compensation
2: Error on selection of transformation
3: Error on selection of work offset
The macro definitions and cycle interfaces are also read in during the power-up procedure. If an error occurs here, this is
indicated by value = 4, or value = 5
6: Error creating 2 1/2 D protection areas during power up.
(Program) START:
Value
100: Error during synchronization preprocessing/main run
101: Error on selection of tool length compensation
102: Error on selection of transformation
103: Error on selection of synchronized spindle
104: Error on selection of work offset
105: Error after WRITE lock on the selected program
Particularly when tool management is active, it is possible that a tool on the spindle or the toolholder is disabled but still
needs to be activated.
These tools are automatically activated on RESET. On START, machine data MD22562 $MC_TOOL_CHANGE_ERROR_MODE
can be used to specify whether an alarm is to be generated or an automatic bypass strategy selected.
If the parameter contains 3 values from 200 to 203, this means that an insufficient number of NC blocks is available for NC
block preparation on certain commands (ASUB start, overstore selection, teach-in).
Remedy: Increase machine data MD28070 $MC_MM_NUM_BLOCKS_IN_PREP.
Reaction:
Interpreter stop
Channel not ready.
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
269
NC alarms
Remedy:
Please inform the authorized personnel/service department.
If parameter %3= 0 -3:
If the alarm or alarms occur on RESET:
Check the settings of machine data MD20110 $MC_RESET_MODE_MASK,
MD20120 $MC_TOOL_RESET_VALUE, MD20121 $MC_TOOL_PRESEL_RESET_VALUE,
MD20122 $MC_TOOL_RESET_NAME (only if tool management is active),
MD20130 $MC_CUTTING_EDGE_RESET_VALUE, MD20132 $MC_SUMCORR_RESET_VALUE,
MD20126 $MC_TOOL_CARRIER_RESET_VALUE,
MD20150 $MC_GCODE_RESET_VALUES, MD20154 $MC_EXTERN_GCODE_RESET_VALUES,
MD20140 $MC_TRAFO_RESET_VALUE,
MD21330 $MC_COUPLE_RESET_MODE_1,
MD24002 $MC_CHBFRAME_RESET_MASK
If parameter %3= 100 - 104:
Check the setting of MD20112 $MC_START_MODE_MASK and the machine data specified under '..._RESET_...'. If tool
management is active, if necessary remove the tool stated in the associated alarm from the toolholder/spindle and cancel
the 'disabled' status.
If parameter %3= 4 or 5:
Check macro definitions in _N_DEF_DIR
Check cycle directories _N_CST_DIR and _N_CUS_DIR
If parameter %3= 6:
Alarm 18002 or 18003 was also issued. This alarm contains the number of the incorrectly defined protection area and an
identifier of what is incorrect about the protection area. The system variables must be appropriately corrected.
If Parameter %3= 200 bis 203:
Increase MD28070 $MC_MM_NUM_BLOCKS_IN_PREP.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14711
[Channel %1: ] Transformation selection not possible as axis %2 not available
Parameters:
%1 = Channel number
%2 = Axis name, spindle number
Explanation:
Based on the configuration of machine data MD20110 $MC_RESET_MODE_MASK and MD20140
$MC_TRAFO_RESET_VALUE, a transformation shall be selected by performing a reset or control ramp-up. However, this is
not possible as axis %2 required for this is not available. Possible reason: The axis was occupied by another channel or the
PLC.
Reaction:
Interface signals are set.
Alarm display.
Remedy:
- Use the GET command to get axis %2 in the channel in which the transformation is to be selected.
- Select the transformation by means of the part program command.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14712
[Channel %1: ] Error selecting JOG Retract: error code %4 info %3
Parameters:
%1 = Channel number
%2 = Is not used
%3 = Additional information
%4 = Error code
Alarms
270
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Explanation:
An error occurred on the selection of JOG Retract, which is described in more detail by the error code (parameter%4):
List of error codes:
1: No retract data available
2: Selection is active during taper turning
3: Error preparing the initialization blocks. The additional info (parameter %3) states the initialization step in which the error
occurred. The alarm output immediately before also refers to this initialization step:
100: Error synchronizing the preprocessing/main run
101: Error selecting the tool length compensation
102: Error selecting the transformation
103: Error generating the tool frame
104: Error generating the tapping block
105: Error replacing geometry axes
4: The position of the axis stated in the additional info does not have the status "synchronized" or "restored"
5: The axis stated in the additional info is already assigned in another channel by JOG Retract
6: The geometry axis stated by the selection of JOG Retract does not exist
7: MD 20110 $MC_RESET_MODE_MASK bit 0 is not set
8: Thread cutting is active. The thread direction cannot be explicitly assigned to a JOG axis
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
The following conditions have to be fulfilled in order to select JOG Retract:
- A program execution with active tool offset has been canceled by Reset or PowerOff
- PLC signal DB21-30 DBX377.5 (Retract data available) or OPI variable retractState bit 1 is set
- JOG mode is active
- The channel in which JOG Retract is to be selected is in Reset state
- The function "Taper turning" must not be active when JOG Retract is selected
- Synchronized or restored axis positions must be present for the axes involved in the transformation
If necessary, activate position restoration for incremental encoders (MD34210 $MA_ENC_REFP_STATE[]=3)
- MD 20110 $MC_RESET_MODE_MASK bit 0 must be set (default value)
In the case of an error, the alarm must be acknowledged with Reset. The selection can then be repeated, observing the
above-mentioned conditions.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14720
[Channel %1: ] Block %2 axes for centerless transformation not available
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
In the channel not all of the axes/spindles are available that have been defined in machine data for centerless grinding.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Please inform the authorized personnel/service department.
1. Modify part program.
2. Modify machine data:
24110 TRAFO_AXES_IN_n
21522 TRACLG_GRINDSPI_NR
21524 TRACLG_CTRLSPI_NR.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
271
NC alarms
14730
[Channel %1: ] Block %2 conflict at activation of centerless transformation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
- Centerless transformation may not be activated when:
- G96 is active and regulating spindle is also master spindle.
- Regulating spindle is in interdependent grouping.
- Axes of centerless transformation overlap with an active transformation and a tool is active.
- For grinding or for regulating wheel spindle, tools are active that are not centerless tools (T1, T2).
- Constant wheel peripheral speed for the regulating spindle is active.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
- Modify part program.
- Check tool data.
- Check machine data.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14740
[Channel %1: ] Block %2 no tool data available for centerless grinding
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
For centerless grinding, the tool data must be contained in T1, D1 (grinding wheel) or T2,D1 (regulating wheel). An error
has been found here.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
- Modify part program.
- Check tool data.
- Check machine data.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14745
[Channel %1: ] Block %2 centerless grinding not active
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
An attempt has been made to switch off the centerless grinding function even though it was not active.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14750
[Channel %1: ] Block %2 too many auxiliary functions programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
More than 10 auxiliary functions have been programmed in an NC block.
Alarms
272
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Check whether all auxiliary functions are necessary in one block - modal functions need not be repeated. Create separate
auxiliary function block or divide the auxiliary functions over several blocks.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14751
[Channel %1: ] Block %2 resources for motion synchronous actions not sufficient (code: %3)
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Identifier
Explanation:
Processing of motion-synchronous actions requires resources that are configured using MD28060
$MC_MM_IPO_BUFFER_SIZE, MD28070 $MC_MM_NUM_BLOCKS_IN_PREP, MD28251
$MC_MM_NUM_SAFE_SYNC_ELEMENTS, MD28250 $MC_MM_NUM_SYNC_ELEMENTS, and MD28253
$MC_MM_NUM_SYNC_STRINGS. If these resources are insufficient for the execution of the part program, then this alarm
is issued. Parameter %3 shows which resource has run out:
Increase identifier <= 2: MD28060 $MC_MM_IPO_BUFFER_SIZE or
MD28070 $MC_MM_NUM_BLOCKS_IN_PREP.
Increase identifier > 2: MD28250 $MC_MM_NUM_SYNC_ELEMENTS, MD28251 $MC_MM_NUM_SAFE_SYNC_ELEMENTS.
Increase identifier 7: MD28253 $MC_MM_NUM_SYNC_STRINGS.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct part program or increase resources.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14752
[Channel %1: ] Block %2 DELDTG | STOPREOF conflict
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
In a group of motion synchronous actions referring to a motion block, both DELDTG (delete distance-to-go) and STOPREOF
(preprocessing stop) have been programmed.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
The functions DELDTG and STOPREOF exclude each other in a block.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14753
[Channel %1: ] Block %2 motion synchronous action: %3 illegal interpolation type
Parameters:
%1 = Channel number
%2 = Block number, line number
%3 = Synact ID
Explanation:
The active interpolation type (e.g. 5-axis interpolation) is not allowed for the motion synchronous action or for the function
"Several feeds".
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Modify part program.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
273
NC alarms
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14754
[Channel %1: ] Block %2 motion synchronous action: %3 wrong feed type
Parameters:
%1 = Channel number
%2 = Block number, line number
%3 = Synact ID
Explanation:
The active feed type is not allowed for the motion synchronous action or for the function "Several feeds".
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14756
[Channel %1: ] Block %2 motion synchronous action: %3 wrong value
Parameters:
%1 = Channel number
%2 = Block number, line number
%3 = Synact ID
Explanation:
Assignment: Illegal value.
The assignment to a variable or transfer parameter of a procedure or function was found to overshoot or undershoot the
value range.
Reaction:
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Modify part program.
Comply with the value range of the variable or transfer parameter
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14757
[Channel %1: ] Block %2 motion synchronous action and wrong type
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Programmed combination between action and type of motion synchronized action is not allowed.
- RET allowed in technology cycle only
- Function "Several feeds" not allowed in technology cycle
- H and M function outputs not allowed with WHENEVER, FROM and DO
- MEASA / MEAWA / MEAC not allowed with WHENEVER, FROM and DO
- DELDTG and STOPREOF allowed only in block-by-block synchronized action with WHEN and EVERY
- PRESETON / PRESETONS may only be used together with WHEN or EVERY
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
274
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14758
[Channel %1: ] Block %2 programmed value not available
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The synchronous variables $AA_LOAD, $AA_TORQUE, $AA_POWER and $AA_CURR are activated by the MD36730
$MA_DRIVE_SIGNAL_TRACKING. The system variable $VA_IS: Safe actual position is only available if the MD36901
$MA_SAFE_FUNCTION_ENABLE is set and the option $ON_NUM_SAFE_AXES is set to a sufficient size.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify program or machine data.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14760
[Channel %1: ] Block %2 auxiliary function of a group programmed repeatedly
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The M and H functions can be divided up as required over machine data in groups in any variation. Auxiliary functions are
thus put into groups that mutually preclude several individual functions of one group. Within one group only one auxiliary
function is advisable and permissible.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Please inform the authorized personnel/service department. Only program one help function per help function group. (For
the group division, see the machine manufacturer's programming guide).
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14761
[Channel %1: ] Block %2 motion synchronous action: DELDTG function not allowed with active
tool radius compensation
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Rapid delete distance-to-go for synchronous actions is not allowed with DELDTG when tool radius compensation is active.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
You have the following possibilities of eliminating the error:
Select the tool radius compensation before performing rapid delete distance-to-go, and then reselect.
As from SW 4.3: "Delete distance-to-go without preparation".
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14762
[Channel %1: ] Block %2 too many PLC variables programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The number of programmed PLC variables has exceeded the maximum permissible number.
For each write operation, one element is required for the following writing of PLC variables quickly one after the other.
If several write operations that are available as elements are to be executed, the block transport must be guaranteed (under
certain circumstances, initiate preprocessing stop), or if available, increase MD28150 $MC_MM_NUM_VDIVAR_ELEMENTS.
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
275
NC alarms
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Modify the part program or where necessary, the machine data.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14763
[Channel %1: ] Block %2 too many link variables programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The number of NCU link variables programmed exceeds the maximum limit. The number is defined in MD28160
$MC_MM_NUM_LINKVAR_ELEMENTS.
Reaction:
Interpreter stop
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Modify the part program or the machine data.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14764
NCU-Link cannot transfer all non-cyclic link messages of type %2 immediately
Parameters:
%1 = Type of non-cyclic link message (e.g. link variables, machine data, alarms)
Explanation:
This alarm is used by cycle developers for diagnostic purposes.
The activation of these alarms can be configured with MD11416 $MN_LINK_DYNMSG_ALARM_MASK. The specified type
corresponds to the relevant bit in MD11416 (see bit description there).
A value assignment to a link variable (e.g. $a_dld[16]=19) is performed in the main run, and transferred via NCU link to all
NCUs in the link network. The bandwidth of this connection restricts the number of value assignments which can be
transferred in one interpolation cycle.
All value assignments are combined in the next main run block and performed immediately this block is executed. A main
run block is the block at which you would stop in single block mode SLB1.
Examples:
Blocks with real traversing motion (G0 X100), Stopre, G4, WAITM, WAITE,...
The alarm occurs if the number of link variables set in any interpolation cycle exceeds the number that can be transferred.
The link variables are first transferred in one of the next interpolation cycles. The assignment is not lost!
Reaction:
Alarm display.
Warning display.
Remedy:
Insert main run blocks between the assignments if the program sequence allows. See also $A_LINK_TRANS_RATE.
Programm
Clear alarm with the Delete key or NC START.
continuation:
Alarms
276
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14765
NCU link cannot transfer all link variables
Explanation:
A value assignment to a link variable (e.g. $a_dld[16]=19) is performed in the main run and transferred via NCU link to all
NCUs in the link network. The bandwidth of this connection restricts the number of value assignments which can be
transferred in one interpolation cycle. Assignment operations which are not transferred are stored in a buffer memory. This
buffer is full!
All value assignments are combined in the next main run block and performed immediately this block is executed.
A main run block is the block at which you would stop in single block mode SLB1.
Examples:
Blocks with real traversing motion (G0 X100), Stopre, G4, WAITM, WAITE,...
Link variable scanning operations are not affected (e.g.: R100= $a_dld[16])
Reaction:
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Between the assignments, insert main run blocks that require a sufficient number of interpolation cycles for execution, e.g.
G4 F10. A block with an additional preprocessor stop does not improve the situation! See also $A_LINK_TRANS_RATE, for a
variable which you can test before an assignment.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14766
NCU link is heavily loaded, impending memory shortage
Explanation:
Informational alarm for part program developers.
The bandwidth of the NCU link is not currently large enough to transfer all the data. This non-cyclic data includes link variable
assignments, machine data write operations, values for the container switch and setting data write operations.
These data are buffered and are not lost. This buffer memory is now 70% full.
Reaction:
Alarm display.
Warning display.
Remedy:
Stagger non-cyclic data in the part program to improve data distribution.
Programm
Clear alarm with the Delete key or NC START.
continuation:
14767
Machine data matching via NCU link not complete
Explanation:
A non-released option has been used in the block.
Reaction:
NC not ready.
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Change fewer setting or machine data at the same time.
Programm
Switch control OFF - ON.
continuation:
14768
Axial auxiliary function for the NCU link cannot be output
Explanation:
Informational alarm for the part program developer.
An axial auxiliary function transmitted via an NCU link cannot be output as the transmission buffer for the
PLC is filled up to 100%.
Reaction:
Alarm display.
Warning display.
Remedy:
In the part program, cyclic data - in this case the output of auxiliary functions for link axes on the
interpolating NCU - should be separated with regard to the time.
Programm
Clear alarm with the Delete key or NC START.
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
277
NC alarms
14769
[Channel %1: ] Block %2 Spindle %3 Implicit auxiliary function %4 Buffer full
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Spindle number
%4 = Auxiliary function number
Explanation:
A maximum of 5 auxiliary functions of type "M" may be entered in an NC block. The upper limit is the total of programmed
and implicitely generated M auxiliary functions. Implicit auxiliary functions M19 and M70 are generated, if in MD35035
$MA_SPIND_FUNCTION_MASK, bit 19 has been set for M19 and/or bit 20 for M70. M19 is generated with SPOS and SPOSA
depending on the configuration. The same applies to M70 and transition into axis operation. The address extension
corresponds to the spindle number like it is output to the PLC.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
- Distribute the M auxiliary functions and spindle functions that implicitely generate M19 and M70 to several blocks.
- Deactivate any implicit auxiliary functions that are not required in MD35035 $MA_SPIND_FUNCTION_MASK, bit 19 and/or
bit 20.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14770
[Channel %1: ] Block %2 auxiliary function programmed incorrectly
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The permissible number of programmed auxiliary functions per NC block has been exceeded or more than one auxiliary
function of the same auxiliary function group has been programmed (M and S function).
In the user-defined auxiliary functions, the maximum number of auxiliary functions per group in the NCK system settings
has been defined for all auxiliary functions by means of the MD11100 $MN_AUXFU_MAXNUM_GROUP_ASSIGN (default: 1)
For each user-defined auxiliary function to be assigned to a group, the assignment is effected through 4 channel-specific
machine data.
Return jump from asynchronous subprogram with M02/M17/M30, whereby the M code is not alone in the block. This is
impermissible if the asynchronous subprogram interrupts a block with WAITE, WAITM or WAITMC. Remedy: Program M02/
M17/M30 alone in the block or replace via RET.
22010 AUXFU_ASSIGN_TYPE: type of auxiliary function, e.g. M
22000 AUXFU_ASSIGN_GROUP: required group
22020 AUXFU_ASSIGN_EXTENSION: any required extension
22030 AUXFU_ASSIGN_VALUE: function value
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct the part program - max. 16 auxiliary functions, max. 5 M functions per NC block, max. 1 auxiliary function per group.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14780
[Channel %1: ] Block %2 option '%3<OPTNX>' is not set.
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Brief description of option
Explanation:
A non-released option has been used in the block.
The stated or an equivalent option is required to execute the action.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Alarms
278
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Remedy:
Modify part program, retrofit option.
In this context, please compare the available option data and/or (if available) the license image of your controller.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14781
[Channel %1: ] Block %2 motion synchronized action: %3 Option '%4<OPTNX>' is not set
Parameters:
%1 = Channel number
%2 = Block number, line number
%3 = Synact ID
%4 = Brief description of option
Explanation:
Motion synchronized action: a non-enabled option was used.
The specified or an equivalent option is required to execute the action.
Reaction:
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Change motion synchronized action, retrofit option.
In this context, please compare the available option data and/or (if available) the license image of your control
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14782
[Channel %1: ] Block %2 non-active function used (identification %3)
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Fine ID
Explanation:
A non-active function is used in the block
Code Short description
1 Transformation
2 Tool H numbers
3 3D protection areas
4 Tool management, multitools
5 COMPSURF and MD28071 $MC_MM_NUM_SURF_LEVELS=0
6 TOFF (see OD19320 $ON_TECHNO_FUNCTION_MASK)
In a handling channel, the following functions are not active either:
10 Synchronous actions
11 COMPCAD with MD20482 $MC_COMPRESSOR_MODE > 99 (Advanced Surface)
12 COMPSURF (Top Surface)
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
- Modify part program.
- Activate function.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14783
[Channel %1: ] Block %2 coordinate system-specific working area limitation is not active
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
An attempt is made in the block to activate a group of the coordinate system-specific working area limitation.
However, this group is not set up (see MD28600 $MC_MM_NUM_WORKAREA_CS_GROUPS).
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
279
NC alarms
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
The NC program is stopped. The G code of the group WALCS01 - WALCS10 can be changed.
Remedy:
- Modify part programm.
- Activate more coordinate system-specific working area limitations.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14784
[Channel %1: ] Block %2 motion synchronous action: %3 function not possible
Parameters:
%1 = Channel number
%2 = Block number, line number
%3 = Synact ID
Explanation:
It is not possible to execute the function:
Reaction:
NC Start disable in this channel.
Interface signals are set.
Alarm display.
NC Stop on alarm.
Remedy:
Modify part program.
Programm
Clear alarm with the RESET key. Restart part program
continuation:
14790
[Channel %1: ] Block %2 axis %3 programmed by PLC
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis
Explanation:
In the NC block, an axis has been programmed that is already being traversed by the PLC.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
- Modify part program, do not use this axis.
- Stop traversing motion of the axis by the PLC, modify part program (insert WAITP).
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14800
[Channel %1: ] Block %2 programmed path velocity less or equal to zero
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
Zero or a negative F or FZ value has been programmed in conjunction with the G functions G93, G94, G95 or G96. The path
velocity may be programmed in the range of 0.001 to 999 999.999 [mm/min, mm/rev, mm/tooth, deg/min, deg/rev] for the
metric input system and 0.000 1 to 39 999.999 [inch/min, inch/rev, inch/tooth] for the inch input system.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Program the path velocity (geometric sum of the velocity components of the geometry axes involved) within the limits given
above.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
280
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
14810
[Channel %1: ] Block %2 negative axis speed programmed for positioning axis %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis
Explanation:
A negative feed (FA value) has been programmed for the displayed axis presently operating as a positioning axis. The
positioning velocity may be programmed in the range 0.001 to 999 999.999 [mm/min, deg/min] for the metric input system
and 0.000 1 to 39 999.999 9 [inch/min, inch/rev] for the inch input system.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Program the positioning velocity within the limits given above.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14811
[Channel %1: ] Block %2 Incorrect value range for programmed dynamic value of axis/spindle
%3, error no. %4
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Axis, spindle
%4 = Error no.
Explanation:
A value outside the permissible input range of a programmable dynamic value was used. The following causes of error are
possible:
1: The value programmed for the axis velocity with VELOLIM or VELOLIMA lies outside the permissible range. The permissible
range for VELOLIM is from 1 to 100 percent and for VELOLIMA from 1 to 200 percent.
2: The value programmed for the axis acceleration with ACC or ACCLIMA lies outside the permissible range from 1 to 200
percent.
3: The value programmed for the axis jerk with JERKLIM or JERKLIMA lies outside the permissible range from 1 to 200
percent.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Adjust the value range in accordance with the Programming Guide.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14812
[Channel %1: ] Block %2 Incorrect value range for the programmed dynamic path response,
error no. %3
Parameters:
%1 = Channel number
%2 = Block number, label
%3 = Error no.
Explanation:
The permissible input range for a programmable dynamic path response value was not observed. The causes of the error
are as follows:
1: The value programmed for path acceleration with PACCLIM lies outside the permitted range. The permitted range for
PACCLIM is from 1.0e-6 to 1.0e+38 m/ss.
2: The value programmed for path speed with FLIM lies outside the permitted range of 1.0e-6 to 1.0e+38.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Adjust the value range in accordance with the Programming Guide.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
281
NC alarms
14815
[Channel %1: ] Block %2 negative thread pitch change programmed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
A negative thread pitch change has been programmed.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Correct the value assignment. Ensure that the programmed F value is greater than zero. Zero is allowed, but has no effect.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14820
[Channel %1: ] Block %2 negative value for maximum spindle speed programmed with
constant cutting speed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
For the function "Constant cutting speed G96" a maximum spindle speed can be programmed with the keyword LIMS=
The values are in the range 0.1 - 999 999.9 [rev/min].
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Program the maximum spindle speed for the constant cutting speed within the limits given above. The keyword LIMS is
modal and can either be placed in front of or within the block that selects the constant cutting speed.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14821
[Channel %1: ] Block %2 error in selection or deselection of GWPS
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
On selecting GWPS programming (constant grinding wheel peripheral speed) with GWPSON, one of the following errors
occurred:
- An attempt has been made to select the GWPS programming for a spindle that has already been assigned to another tool
by TMON, GWPSON, CLGON or activation of the tool length compensation.
- An attempt has been made to select a tool which has not been defined.
- An attempt has been made to select an edge (implicitely) which has not been defined (implicit selection: D1 of a tool, if
no tool has been specified.)
- Selection does not refer to a grinding-specific tool (400-499).
- An attempt has been made to select GWPS for the active tool, although the TLC is not switched on.
- Selection refers to an invalid spindle number.
- A grinding wheel radius equal to zero has been specified.
On deselecting GWPS programming with GWPSOFF, one of the following errors occurred:
- Deselection does not refer to a grinding-specific tool (400-499).
- An attempt has been made to deselect GWPS for the active tool, although the tool length compensation has not been
activated.
- Deselection refers to an invalid spindle number.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
- Check GWPSON and GWPSOF command.
- Check tool compensation data:
$TC_DP1 : 400 - 499;
$TC_TGP1: Spindle number.
Alarms
282
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
NC alarms
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14822
[Channel %1: ] Block %2 incorrect programming of GWPS
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
When selecting GWPS (constant grinding wheel peripheral speed) with GWPSON or programming the GWPS with "S[spindle
number] = value" one of the following errors has occurred:
Invalid spindle number.
Invalid parameter number for radius calculation in $TC_TPG9.
The following values are valid:
3 for $TC_DP3 (length 1)
4 for $TC_DP4 (length 2)
5 for $TC_DP5 (length 3)
6 for $TC_DP6 (radius)
Invalid angle in $TC_TPG8.
The following values are valid: -90 <= $TC_TPG8 < +90.
A grinding wheel radius equal to zero was specified.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Check tool compensation data.
- $TC_DP1 : 400 - 499.
- $TC_TPG1: Spindle number.
- $TC_TPG8: Inclination angle for slope grinding wheel.
- $TC_TPG9: Compensation parameters for radius computation, e.g. 3 for $TC_GP3.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14823
[Channel %1: ] Block %2 error on selection or deselection of tool monitoring
Parameters:
%1 = Channel number
%2 = Block number, label
Alarms
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
283
NC alarms
Explanation:
When selecting tool monitoring with TMON, one of the following errors occurred:
- Selection does not refer to a grinding-specific tool (tool types 400-499).
- Selection refers to an invalid spindle number.
- An attempt has been made to select tool monitoring for a spindle that is already assigned to another tool by TMON,
GWPSON, CLGON or activation of tool length compensation.
- An attempt has been made to select a tool that has not been defined.
- An attempt has been made to select an edge (implicitly) that has not been defined. (Implicit selection: D1 of a tool, if no
edge has been specified.)
- An attempt has been made to select tool monitoring for the active tool, although no tool length compensation has been
activated.
- Invalid parameter number for radius calculation in $TC_TPG9.
The following values are valid:
3 for $TC_DP3 (length 1)
4 for $TC_DP4 (length 2)
5 for $TC_DP5 (length 3)
6 for $TC_DP6 (radius)
A grinding wheel radius equal to zero has been specified.
On deselecting tool monitoring with TMOF, one of the following errors occurred:
- Deselection does not refer to a grinding-specific tool (400-499).
- An attempt has been made to deselect tool monitoring for the active tool, although tool length compensation is not active.
- Deselection refers to an invalid spindle number.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Check TMON and TMOF command.
Check tool compensation data.
- $TC_DP1 : 400 - 499.
- $TC_TPG1: Spindle number.
- $TC_TPG8: Inclination angle for slope grinding wheel.
- $TC_TPG9: Parameter number for radius computation, e.g. 3 for $TC_GP3.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14824
[Channel %1: ] Block %2 conflict with GWPS
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The functions of constant grinding wheel peripheral speed GWPS and constant cutting speed G96 S... have been activated
at the same time for a spindle.
Reaction:
Correction block is reorganized.
Interface signals are set.
Alarm display.
Remedy:
Modify part program.
Programm
Clear alarm with NC START or RESET key and continue the program.
continuation:
14840
[Channel %1: ] Block %2 incorrect value range for constant cutting speed
Parameters:
%1 = Channel number
%2 = Block number, label
Explanation:
The programmed cutting speed is not within the input range
Input range metric: 0.01 to 9 999.99 [m/min]
Input range inch: 0.1 to 99 999.99 [inch/min]
Alarms
284
Diagnostics Manual, 10/2020, 6FC5398-6BP40-6BA4
|