ID-range 21000-21249

21000	Thread tapping together with spindle movement not permitted.
	Description	Its not possible to use spindle M-functions (M3, M4, M5, M19, S.POS) while thread tapping is active [PROG - Chapter Tapping (G63)].
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21001 - 21020
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	2
	Solution	Class	8	Restart of NC-control necessary.

21022	Writing of a variable by active kinematic transformation not allowed.
	Description	Its not possible to change the kinematic parameters of the current tool with active kinematic transformation via V.G.WZ_AKT.KIN_PARAM[..].
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Change sequence of processing inside NC program. Change kinematic tool data only after deselection of kinematic transformation.
	Error type	1, Error message from NC-program.

21023	SIZEOF access not permitted for this variable.
	Description	The SIZEOF access on indicated global variables (V.G., e.g. V.G.WZ_AKT.V[i] or V.G.WZ[j].[P[i] is not permitted.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program. The SIZEOF access is only allowed for self-defined variable arrays (V.L., V.P., V.S.).
	Error type	1, Error message from NC-program.

21024	Circle center point and radius are not permitted at the same time.
	Description	Programming a circle is either defined by the centre of the circle or by programming the radius. Example with error: %err_21024.err N10 G00 X0 Y0 Z0 G17 N20 G01 X10 Y100 F10000 N30 X100Y200 N40 X200 N50 G02 X200 I50 J50 R50 N60 G01 X400 Y0 N99 M30 Corrected example: %err_21024.cor N10 G00 X0 Y0 Z0 G17 N20 G01 X10 Y100 F10000 N30 X100Y200 N40 X200 N50 G02 X200 I50 J50 N60 G01 X400 Y0 N99 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21025 / 21026
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21027	3D tool geometry compensation is already active. Renewed call not allowed.
	Description	While active 3D tool geometry compensation in NC program #TGC ON is programmed again. Example: Wrong: N10 #TGC ON : Nxx #TGC ON : Nxx #TGC OFF : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Remove redundant #TGC ON.
	Error type	1, Error message from NC-program.

21028	Tool change is not permitted if 3D tool geometry compensation is active.
	Description	While active 3D tool geometry compensation (TGC) in NC program a tool change is programmed. Example: Wrong: N10 D1 N20 #TGC ON N.. D2 N40 #TGC OFF Correct: N10 D1 N20 #TGC ON : N.. #TGC OFF N.. D2 N.. #TGC ON : N.. #TGC OFF : M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Tool change may only be executed during deselected3D tool geometry compensation(#TGC OFF).
	Error type	1, Error message from NC-program.

21029	Write access to tool data is not allowed while 3D-WGK is active.
	Description	While active 3D tool geometry compensation (TGC) in NC program a write access via V.G.WZ_AKT.* on current tool data (length, radius, axes offsets) is programmed. Example: Wrong: N10 #TGC ON : N.. V.G.WZ_AKT.R = 50 : N.. #TGC OFF : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Write access on current tool data is only permissible during deselected3D tool geometry compensation(#TGC OFF).
	Error type	1, Error message from NC-program.

21035	Unknown NC-command in spindle sequence.
	Description	A programmed command is in combination with spindle specific programming not permitted.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21036	Double programming of the spindle speed.
	Description	Its not possible to assign a spindle a number of revolutions within a block several times.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Modification of NC program.
	Parameter	%1:	Actual value [-]
			Last programmed spindle speed
	Error type	1, Error message from NC-program.

21037	Channel parameters: Invalid log. axes number of the main spindle.
	Description	A spindle axis with the logical axis number of the main spindle is not available in the NC channel. The error message can appear during start-up.
	Reaction	Class		3	NC start-up is continued.
	Solution	Class		6	Check and modify the logical axis number of the main spindle P-CHAN-00051 before next start-up in the channel parameters. During start-up in case of conflict the main spindle the logical axis number of the first spindle P-CHAN-00036 is assigned to and the start-up is continued.
	Parameter	%1:	Incorrect value [-]

		%2:	Corrected value [-]

	Error type	2, Error message by data transfer from parameter list into control device.

21038	Tool request for an unknown spindle.
	Description	In the dynamic data of the requested tool there s a spindle assigned, which is missing in the channel.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Modification of tool data (P-TOOL-00012)
	Parameter	%1:	Actual value [-]
			Logic axis number of the assigned spindle
	Error type	1, Error message from NC-program.

21039	NC-command in this context not permitted.
	Description	In combination with the used NC command a programmed keyword is not allowed.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check ans modify NC command.
	Parameter	%1:	State [-]

	Error type	1, Error message from NC-program.

21040	Double programming in #HSC-command.
	Description	Within the command #HSC keywords are programmed several times or in wrong combinations. Example with error: #HSC ON[CONTERROR 1, OPMODE 2, OPMODE 1] or #HSC ON[CONTERROR 1, OPMODE 2, CONTERROR 0.1]
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of #HSC command in the NC program [PROG].
	Error type	1, Error message from NC-program.

21041	Invalid HSC-mode.
	Description	In the #HSC [] command the keyword OPMODE has an invalid value.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the NC program. Set the operation mode in the #HSC command on a permissible value[PROG].
	Parameter	%1:	Incorrect value [-]
			Invalid HSC-mode
	Error type	1, Error message from NC-program.

21042	Logical axis number exceeds range of data format.
	Description	Within the axis exchange command a logical axis number is programmed, which exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the axis exchange command.
	Parameter	%1:	Incorrect value [-]
			Incorrect logical axis number of the axis in the axis exchange command. P-AXIS-00016, P-CHAN-00035
		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21043
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	8	Restart of NC-control necessary.

21044	DIN-syntax only for main spindle.
	Description	The DIN-syntax ist permitted only for the main spindle. The used spindle is not the main spindle.
	Reaction	Class		1	Abort of the NC program processing.
	Solution	Class		3	Modification of NC program 1.Possibility: change the main spindle with #MAIN SPINDLE 2.Possibility: use spindle specific syntax for the spindle which should be programmed
	Parameter	%1:	Logical axis number [-]
			Logical axes number of the programmed spindle
		%2:	Logical axis number [-]
			Logical axes number of the main spindle
	Error type	1, Error message from NC-program.

21045	Channel parameters: Main spindle name used several times.
	Description	The designation of a spindle P-CHAN-00007 is identical to the name of the main spindle P-CHAN-00053 . This is not permissible. Example with error in channel parameter list: # Spindle data spdl_anzahl 2 # main_spindle_ax_nr 6 main_spindle_name S ... spindel[0].bezeichnung S spindel[0].log_achs_nr 6 ... spindel[1].bezeichnung S2 spindel[1].log_achs_nr 11 Corrected example: # Spindle data spdl_anzahl 2 # main_spindle_ax_nr 6 main_spindle_name ... spindel[0].bezeichnung S1 spindel[0].log_achs_nr 6 ... spindel[1].bezeichnung S2 spindel[1].log_achs_nr 11
	Reaction	Class		3	Start-up of the control is aborted.
	Solution	Class		6	Modification of channel parameter list.
	Parameter	%1:	Actual value [-]
			Designation of main spindle
		%2:	Logical axis number [-]
			Logical axis number of the spindle with the same name
	Error type	2, Error message by data transfer from parameter list into control device.

21046
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	2
	Solution	Class	8	Restart of NC-control necessary.

21047	Unknown spindle name or close bracket missing..
	Description	While changing the main spindle with the command #MAIN SPINDLE either the identifier of the spindle is unknown or the closing square bracket is missing.
	Reaction	Class	2	Abort of the NC program processing
	Solution	Class	3	Check and modify the NC-command.
	Error type	1, Error message from NC-program.

21050	Changing the main spindle while active turning functions is not allowed.
	Description	While active turning functions a change of the main spindle (#MAIN SPINDLE) is programmed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modify the sequence of NC program, for example deselect the turning function before changing the main spindle.
	Error type	1, Error message from NC-program.

21056	Double programming of signal number.
	Description	Within the commands #SIGNAL or #WAIT the signal-ID is programmed several times.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21057	Too many parameters in signal command programmed.
	Description	The number of maximum permissible parameters when waiting for a signal (#WAIT) or sending a signal (#SIGNAL) was exceeded.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Modification of NC program.
	Parameter	%1:	Limit value [-]
			Maximum permissible number of parameters
	Error type	1, Error message from NC-program.

21058	No signal number was programmed.
	Description	Within the commands #SIGNAL or #WAIT the signal-ID is missing within the square brackets.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21059	Parameter is already used in this command.
	Description	Its not possible to use a parameter several times within the command #SIGNAL. Example with error: #SIGNAL[ID44 P[0]=200 P[0]=944]
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Modification of NC program.
	Parameter	%1:	Actual value [-]

	Error type	1, Error message from NC-program.

21060	No signal parameter available.
	Description	The number of the expected parameters in the #WAIT command does not agree with the number of the sent parameters in #SIGNAL.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of the parameters in the commands #WAIT and #SIGNAL.
	Error type	1, Error message from NC-program.

21061	HSC-parameter exceeds range of data format.
	Description	The value of additional HSC parameters is out of data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Modification of NC program.
	Parameter	%1:	Incorrect value [-]
			Value of the additional HSC-parameter
		%2:	Lower limit value [-]
			Minimal limit of the parameter
		%3:	Upper limit value [-]
			Maximal limit of the parameter
	Error type	1, Error message from NC-program.

21067	Redundant information programmed.
	Description	While using axis-specific programming there are redundant information programmed. Incorrect example; "POS" shows such redundant information: N10 X10 Y11 Z[INDP_SYN POS50POS40 G01 FEED100 G90]
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21068	Syntaxfehler bei Programmierung einer unabhaengigen Achse.
	Description	While programming independent axes a syntax error arose within the brackets when using the G-command. The used G-command does not exist. Incorrect example: N10 X10 Y11 Z[INDP_SYN G03 FEED100 G90] Corrected example: N10 X10 Y11 Z[INDP_SYN G01 FEED100 G90]
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21071	Independent axes during active transformation not allowed.
	Description	While active kinematic or cartesian transformation an independent axis movement is programmed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modify the sequence of NC program, for example deselect the transformation before programming the independent axis. Hint: With multiple ID 1 a kinematic transformation is active. With multiple ID 2 a cartesian transformation is active.
	Error type	1, Error message from NC-program.

21072	No independent movement of circle axes in the circle block.
	Description	The first two main axes needed for a circular block may not be programmed independently.
	Reaction	Class	1	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21076	GANTRY limit out of range.
	Description	The value of a programmed control limit of the gantry mode is out of range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Correction of the control limit. Hint: For first limit multiple ID 1 is indicated. For second limit multiple ID 2 is indicated.
	Parameter	%1:	Incorrect value [-]
			Invalid control limit
		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21077	Scaling factor is 0.
	Description	Within the axes coupling command the numerator <numerator> necessary for the definition of a coupling factor (scaling factor) is set to zero.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Checkaxes coupling command and assign to <numerator> a useful value .
	Parameter	%1:	Actual value [-]
			Invalid value of numerator
	Error type	1, Error message from NC-program.

21078	File for writing the coupling could not be created.
	Description	The log file for the coupling could not be created. The log file existed already and is opened.
	Reaction	Class	1	Abort of the NC program processing.
	Solution	Class	3	Close the opened log file.
	Error type	1, Error message from NC-program.

21079	No synchronous operation active. Deselection has no effect.
	Description	The deselection of axes couplings has no effect, since no active coupling mode is present.
	Reaction	Class	2	Continue NC program processing.
	Solution	Class	1	Remove command #DISABLE AX LINK.
	Error type	1, Error message from NC-program.

21080	No file name for saving defined in channel parameters.
	Description	In the channel parameter list no name for the log file is defined.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Definition of log file name in the channel parameter list.
	Error type	1, Error message from NC-program.

21081	Coupling command is too long for saving in file.
	Description	The number of the used signs within the coupling command is too big for saving into the log file.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Reduce the number of signs.
	Parameter	%1:	Actual value [-]
			Number of used signs of the coupling command
		%2:	Upper limit value [-]
			Limit of signs
	Error type	1, Error message from NC-program.

21083	In current state no independent axes may be programmed.
	Description	Programming indepentent axes is not possible at this time because spline interpolation or a turning function is active.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC program.
	Error type	1, Error message from NC-program.

21085	Clamping axes are not permitted to move independent.
	Description	A positioning axes in motion (e.g. independent axis, oscillation axis) is a so-called "Clampable axis". For positioning axes this characteristic is not permissible.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	The characteristic "Clampable axis - ACHSMODE_CLAMPABLE " has to be removed in the axis parameter P-AXIS-00015 (achs_mode) in the corresponding axis list. After that a new start-up of the control or a reload of the axis parameters is necessary.
	Error type	1, Error message from NC-program.

21086	Maximum number of M- and/or the H-functions per instruction exceeded.
	Description	The limit of M- and H-functions was exceeded when programming axes and/or spindle specific ( e.g. X[.....] , S[.....]).
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Reduce the number of M- and H-functions.
	Parameter	%1:	Upper limit value [-]
			Limit of M- and H-functions
	Error type	1, Error message from NC-program.

21087	Value exceeds range of data format.
	Description	The value of the data is out of range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Correction of the valid value.
	Parameter	%1:	Incorrect value [-]
			Actual value
		%2:	Lower limit value [-]
			Lower limit value
		%3:	Upper limit value [-]
			Upper limit value
	Error type	1, Error message from NC-program.

21088	Number of comma after point exceeds range of data format.
	Description	While programming Sercos parameter the parameter of the number of places after decimal point "DEC" exceeds the limit of the allowed data format. [PROG - Chapter: Non-synchronized reading] , [PROG - Chapter: Non-synchronized writing],
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	The parameter of the number of places after decimal point has to be corrected
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21089	Double programming in #IDENT-command.
	Description	Within the command #IDENT keywords are programmed several times or in wrong combinations. [PROG - Chapter: Non-synchronized reading] ,
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of the #IDENT command in the NC program.
	Error type	1, Error message from NC-program.

21090	Error in identnumber.
	Description	The indicated ident number of the SERCOS drive is not correct. Examine the ID number. Consult the documentation of the drive manufacurer for a further diagnosis. [PROG - Chapter: Non-synchronized reading] , [PROG - Chapter: Non-synchronized writing],
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Examination of the ident number.
	Error type	1, Error message from NC-program.

21091 - 21093
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21094	Fatal SERCOS-error.
	Description	In the SERCOS drive arose an error which can not be assigned.
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Consult the documentation of the drive manufacturer.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]

	Error type	1, Error message from NC-program.

21095	SERCOS-Parameter: Unknown SERCOS-ID.
	Description	In the command #IDENT or #COMMAND the used SERCOS-ID is unknown. [PROG - Chapter: Non-synchronized reading] , [PROG - Chapter: Non-synchronized writing],
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Examination and correctionof the SERCOS-ID.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			Wrong ident number
	Error type	1, Error message from NC-program.

21096	SERCOS-Parameter: Data size too short.
	Description	The parameter specification of the length of data in the command #IDENT is too small. The indication takes place after the keyword TYP. [PROG - Chapter: Non-synchronized reading] , [PROG - Chapter: Non-synchronized writing],
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Correction of the incorrect parameter.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			SERCOS ident number
	Error type	1, Error message from NC-program.

21097	SERCOS-Parameter: Data size too long.
	Description	The parameter specification of the length of data in the command #IDENT is too big. The indication takes place after the keyword TYP. [PROG - Chapter: Non-synchronized reading] , [PROG - Chapter: Non-synchronized writing],
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Correction of the incorrect parameter.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			SERCOS ident number
	Error type	1, Error message from NC-program.

21098	SERCOS-Parameter: Date cannot be changed.
	Description	The data can not be changed. Possibly the parameter is changeable only in a certain phase during start-up of the SERCOS drive. More detailed informations you can get from the documentation of the drive manufacturer.
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Consult the documentation of the drive manufacturer.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			SERCOS ident number
	Error type	1, Error message from NC-program.

21099	SERCOS-Parameter: Date at this time read only.
	Description	Date is write protected. For changing this date the write protection has to be disabled before. More detailed informations you can get from the documentation of the drive manufacturer.
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Consult the documentation of the drive manufacturer.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			SERCOS ident number
	Error type	1, Error message from NC-program.

21100	SERCOS-Parameter: Date shorter as min. value.
	Description	During the cyclic data communication of the SERCOS drive data blocks are transmitted. These contain names, attribute, unit, maximum and minimum input value and the date. With the occurrence of this error the input value of data is less than the permissible minimal limit of data. More detailed informations you can get from the documentation of the drive manufacturer.
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Consult the documentation of the drive manufacturer.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			SERCOS ident number
	Error type	1, Error message from NC-program.

21101	SERCOS-Parameter: Ddate greater than max. value.
	Description	During the cyclic data communication of the SERCOS drive data blocks are transmitted. These contain names, attribute, unit, maximum and minimum input value and the date. With the occurrence of this error the input value of data is bigger than the permissible maximal limit of data. More detailed informations you can get from the documentation of the drive manufacturer.
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Consult the documentation of the drive manufacturer.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			SERCOS ident number
	Error type	1, Error message from NC-program.

21102	SERCOS-Parameter: Date incorrect.
	Description	With the cyclic data communication of the SERCOS drive data blocks are transmitted. These contain names, attribute, unit, maximum and minimum input value and the date. With the occurrence of this error the input value of data is incorrect. More detailed informations you can get from the documentation of the drive manufacturer.
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Consult the documentation of the drive manufacturer.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			SERCOS ident number
	Error type	1, Error message from NC-program.

21103	Other errors during transfer in service channel.
	Description	Collecting error message for general SERCOS errors.
	Reaction	Class		3	Abort of the NC program processing
	Solution	Class		3	Consult the documentation of the drive manufacturer.
	Parameter	%1:	Actual value [-]
			Error message of the service channel
		%2:	Ident number [-]
			SERCOS ident number
	Error type	1, Error message from NC-program.

21104	NC-command is not complete.
	Description	NC-command is not complete, some important and necessary keywords have not been programmed.
	Reaction	Class		2	Abort of the NC program processing
	Solution	Class		3	Check NC command and supplement the missing keywords.
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

21105	Unknown drive type.
	Description	In the NC command the used drive type is unknown.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	At the moment the NC command may be used only with SERCOS drives. I.e. only the keyword SERC is permissible [PROG].
	Error type	1, Error message from NC-program.

21106	Axis name or NC-command not allowed.
	Description	In the NC command there was used an invalid axis identifier or unknown keyword.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of the NC program.
	Error type	1, Error message from NC-program.

21107	Syntax error while axis programming.
	Description	Within theaxes specific command sequence( e.g. X[..] ) a syntax error has been detected.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the axes specific command sequence. Syntax errors for example are: - Double programming - Excluding keywords - Missing syntax elements; open brackets, close brackets
	Error type	1, Error message from NC-program.

21110	Denominator of the scaling factor is missing.
	Description	Within the axes coupling command the denominator <denominator> necessary for the definition of a coupling factor (scaling factor) is not programmed.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Checkaxes coupling command and supplement the missing <denominator> [PROG].
	Parameter	%1:	Actual value [-]
			Value of assigned numerator.
		%2:	Incorrect value [-]
			Default value of the missing denominator.
	Error type	1, Error message from NC-program.

21111	Invalid scaling factor.
	Description	The coupling factor (scaling factor) defined by <numerator>, <denominator> within the axes coupling commandresults in an illegal value.
	Reaction	Class		2	NC program processing is continued.
	Solution	Class		1	The invalid coupling factor implicitly is set to 1. The coupling is handled like a standard coupling. Factors that result in pure scaling or in scaling with simultaneous mirroring (-1 < factor < 0 or factor > -1) are currently not permitted [PROG]. From <numerator> <denominator> resulting and permissible coupling factors are: -1 Mirror coupling 1 Standard coupling
	Parameter	%1:	Actual value [-]
			Value of numerator
		%2:	Actual value [-]
			Value of denominator
		%3:	Incorrect value [-]
			Invalid coupling factor
	Error type	1, Error message from NC-program.

21120	Double programming of counter parameter.
	Description	Within the command for sending signals #SIGNAL the counter parameter (COUNT) is programmed several times.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check the signal command and remove the redundant COUNT.
	Error type	1, Error message from NC-program.

21121	Syntax error: Programming of this ID range not permitted.
	Description	Within the command for deleting of signals #SIGNAL REMOVE no ID range (IDMIN, IDMAX) may be programmed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check the signal command, remove IDMIN, IDMAX and replace them by a single ID. The ID range is only application-specific available and only useful if also the keyword COUNT in the command #SIGNAL is allowed. Please inform manufacturer of the control.
	Error type	1, Error message from NC-program.

21122	Syntax error: Double programming of ID range.
	Description	Within the command for deleting of signals #SIGNAL REMOVE the upper limit of the ID range (IDMAX) is programmed several times.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check the signal command and remove the redundant IDMAX.
	Error type	1, Error message from NC-program.

21123	Syntax error: Counter parameter not permitted.
	Description	Within the command for sending signals #SIGNAL the counter parameter (COUNT) may not be used.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check signal command and remove COUNT. The counter parameter COUNT is only application-specific available. Please inform manufacturer of the control.
	Error type	1, Error message from NC-program.

21126	At current axis position kinematic transformation is undefined.
	Description	Some kinematics transformations are not defined for all possible input coordinates. In example forward and backward transformation are not reversible to each other. This will be checked here for need of higher machine safty level (e.g. in case of a medical robot system).
	Reaction	Class	3	Abort of the NC program processing.
	Solution	Class	3	Check input coordinates of kinematics transformation. Increase degree of accuracy.
	Error type	1, Error message from NC-program.

21128	Channel parameters: Channel specific override exceeds limit.
	Description	During start-up the check of the channel parameters detects, that P-CHAN-00056 exceeds the permissible limits.
	Reaction	Class		1	NC start-up is continued.
	Solution	Class		1	During start-up in case of conflict P-CHAN-00056 is set to a limit and the start-up is continued.
	Parameter	%1:	Incorrect value [-]
			Incorrect parameter value
		%2:	Upper limit value [-]
			Permissible limit Hint: With multiple ID 1 the maximum limit is indicated. With multiple ID 2 the minimum limit is indicated.
		%3:	Corrected value [-]
			Automatic corrected parameter value Hint: With multiple ID 1 the parameter is set on the maximum limit. With multiple ID 2 the parameter is set on the minimum limit.
	Error type	2, Error message by data transfer from parameter list into control device.

21129	M02/M30 is missing.
	Description	At the end of the main program no M02 or M30 is programmed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Program M02 or M30 at the end of the main program.
	Error type	1, Error message from NC-program.

21130	M17/M29 is missing.
	Description	At the end of a global sub program no M17 or M29 is programmed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Program M17 or M29 at the end of the global sub program.
	Error type	1, Error message from NC-program.

21131	Axis or spindle for axis specific M/H-function unknown.
	Description	By programming (e.g. X[M20], S[M25]) and/or by channel-specific parametrization assigned axis or spindle (P-CHAN-00039, P-CHAN-00025) of a M/H function is missing in the channel.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify axis specific M/H programming and/or channel-specific default parametrization (P-CHAN-00039, P-CHAN-00025). In the program sequence the assigned axes may not have left the NC channel by an exchange command (e.g. #PUT AX).
	Parameter	%1:	Actual value [-]
			Number of the axis specific M/H-function
	Error type	1, Error message from NC-program.

21132	Double programming of spindle override.
	Description	Error messages is output in use of programming spindle override (G167). Within NC-block the override of a spindle is programmed several times [PROG].
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the spindle programming within NC-block. Remove redundant G167 commands.
	Error type	1, Error message from NC-program.

21134	Syntax error when programming tracking of an axis.
	Description	Within thecommand foraxis tracking (#CAXTRACK) a syntax error (e.g. multiple programming, unknown keyword ..) has been detected.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the command foraxis tracking.
	Error type	1, Error message from NC-program.

21135	Parameter of axis tracking exceeds range of data format.
	Description	Within thecommand foraxis tracking (#CAXTRACK) one of the programmed parameters (ANGLIMIT, OFFSET, ANGPOS) exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the command foraxis tracking.
	Parameter	%1:	Incorrect value [-]

		%2:	Incorrect value [-]

		%3:	Lower limit value [-]

		%4:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21136	Unknown tracking axis.
	Description	With the selection of axis tracking (#CAXTRACK ON) it is detected, that the required tracking axis is not available in the NC-channel.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	In the channel parameter list a tracking axis P-CHAN-00095 has to be defined. Ensure, that the axis is available in the NC-channel during selection of axis tracking.
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

21137	Axes exchange not allowed while axis tracking.
	Description	While active axis tracking (#CAXTRACK ON) in NC program no axis exchange commands may be used.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	In NC program deselection of axis tracking (#CAXTRACK OFF) before the use of axis exchange commands.
	Error type	1, Error message from NC-program.

21138	Missing definition of default C-axis name.
	Description	With the selection of C-axis processing (#CAX) it is detected, that no default C-axis name is configured in the NC-channel.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	In the channel parameter list a default C-axis name P-CHAN-00008 has to be defined
	Error type	1, Error message from NC-program.

21139	Channel parameters: C-axis activity requires a spindle.
	Description	With the selection of C-axis processing (#CAX) it is detected, that the required spindle is not configured in the NC-channel.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	At least one spindle has to be configured in the channel parameter list. P-CHAN-00010, P-CHAN-00082, [CHAN - Chapter definition of a main spindle], P-CHAN-00051
	Parameter	%1:	Limit value [-]
			Invalid number of configured spindles in NC-channel.
	Error type	1, Error message from NC-program.

21141	Invalid NC-command in manual block.
	Description	In manual block NC-commands were used, which are only useful in a NC-program.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Do not use the corresponding commands in manual block. Hint: For #IF / #ELSE / #ENDIF multiple ID 1 is valid. For #COMMENT BEGIN / END multiple 2 is valid.
	Error type	1, Error message from NC-program.

21142	Contour rotation not possible, if 1. or 2. main axis is not available.
	Description	With the selection of the contour rotation it is detected that the first or second main axis is missing in the NC-channel.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the axes configuration of the NC-channel. Error cause can be e.g. an incomplete basic configuration in the channel parameter list or e.g. by the use of axes exchange instructions in the NC-program the first or second main axis from the channel was released.
	Parameter	%1:	Incorrect value [-]
			String as reference, which main axis is missing. FIRST: first main axis SECOND: second main axis
	Error type	1, Error message from NC-program.

21143	Deselection of contour rotation at plane change.
	Description	While active contour rotation #ROTATION ON [...] a plane change (G17, G18, G19, G20) is programmed. Because this causes a new order of the main axes, the contour rotation is implicitly deselected.
	Reaction	Class	2	NC program processing is continued.
	Solution	Class	1	Modify NC program. Deselect contour rotation before plane change with#ROTATION OFF.
	Error type	1, Error message from NC-program.

21144	Loading the V.E.-Variables data to the DECODER failed.
	Description	With the initialization of the external variables [EXTV] a not correctable error was detected.No assumption of the external variables into the control.
	Reaction	Class	3	NC start-up is continued and/or no update of external variables.
	Solution	Class	7	Check the list of external variables and/or preceeding error messages.
	Error type	-

21145
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21146	Syntax error within programming of contour rotation.
	Description	Within the contour rotation command #ROTATION a syntax error has been detected.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the contour rotation command. Syntax errors for example are: - Double programming - Excluding keywords - Missing syntax elements; open brackets, close brackets
	Error type	1, Error message from NC-program.

21147	Programmed rotation centre exceeds range of data format.
	Description	Within the contour rotation command #ROTATION one of the programmed rotation centre coordinates (CENTERxx) exceeds the permissible data range.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the contour rotation command. Hint: For CENTER1 multiple ID 1 is indicated. For CENTER2 multiple ID 2 is indicated.
	Error type	1, Error message from NC-program.

21148	Address of the external variable exceeds valid address range.
	Description	During calculation of the address it is detected, that the external variable exceeds the valid address range.
	Reaction	Class		2	NC start-up is continued.
	Solution	Class		7	Check and decrease the element "array_size" for array variables before next start-up in the configuration list [EXTV]. Check and decrease the element "index" for simple external variables before next start-up. During start-up in case of conflict the external variable is skipped and as a result it can not be used.
	Parameter	%1:	Incorrect value [-]
			Incorrect address of the external variable. Hint: Multiple ID 1 is monitored for channel specific variables (CHANNEL). Multiple ID 2 is monitored for global variables (GLOBAL). Multiple ID 3 is monitored, if the address of a variable was not calculated at all.
		%2:	Limit value [-]
			Maximum permissible address of an external variable
		%3:	Actual value [-]
			Index of the incorrect external variable in the configuration list.
		%4:	Actual value [-]

	Error type	-

21149	Offset of external variable array is 0.
	Description	In the configuration list [EXTV] the element "size" for an external array variable has the value 0.
	Reaction	Class		2	NC start-up is continued.
	Solution	Class		3	According to the data type check and modify the element "size" before next start-up in the configuration list. During start-up in case of conflict the value is corrected to 1 and the start-up is continued.
	Parameter	%1:	Incorrect value [-]
			Invalid value of the element "size".
		%2:	Actual value [-]
			Index of the invalid external variable in the configuration list.
	Error type	-

21151	Invalid combination of spindle commands.
	Description	While spindle programming excluding NC-commands are used. For example in the same NC-block M3 and M4 are programmed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify spindle programming.
	Error type	1, Error message from NC-program.

21152	Reset timeout for external tool data management.
	Description	Request for NC-reset of channel was not acknowledged by external tool management in required time limit.
	Reaction	Class		3	Abort of NC-reset
	Solution	Class		6	Repeat NC-reset. Check external tool management.
	Parameter	%1:	Incorrect value [1 µsec]
			Actual exceeded time
		%2:	Limit value [1 µsec]
			Maximum time difference for reset acknowledge after reset request.
	Error type	-

21153 - 21155
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21157	SYN not permitted for this command.
	Description	The keyword SYN is programmed in a not permitted combination with the commands #IDENT and/or #COMMAND.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check the commands #IDENT and/or #COMMAND and remove SYN. A synchronization may be programmed only in combination with #IDENT WR, #COMMAND WR and/or #COMMAND WAIT [PROG].
	Parameter	%1:	Incorrect value [-]
			Invalid keyword
	Error type	1, Error message from NC-program.

21158	Read procedure command not possible (write only).
	Description	The command # COMMAND is to be executed with a read order (RD).But only a write order (WR) is permitted.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC-command. Only a write order (WR) may be programmed.
	Parameter	%1:	Incorrect value [-]
			Invalid keyword
	Error type	1, Error message from NC-program.

21159	Machine date could not be taken over.
	Description	The change of an axis parameter programmed with the command #MACHINE DATA could not be executed.
	Reaction	Class	3	Abort of the NC program processing.
	Solution	Class	3	Move the command #MACHINE DATA within the program sequence. If necessary check and modify the syntax or the value of the parameter. Some parameters may not be changed while active NC-program.
	Error type	1, Error message from NC-program.

21160
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21164	Missing absolute or relative programming.
	Description	Within the command sequence of an independent axis the absolute-/ relative programming (G90/G91) is missing.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check the command sequence of the independent axis and complete the absolute-/ relative programming.
	Error type	1, Error message from NC-program.

21165	Missing feed- or time programming.
	Description	Within the command sequence of an independent axis the programming of feed or the moving time (FEED/TIME) is missing.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check the command sequence of the independent axis and complete the feed or moving time.
	Error type	1, Error message from NC-program.

21167	TIMER-ID exceeds range of permissible values.
	Description	The counter value (ID) programmed in the NC-command #TIMER exceeds the permissible value range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Programming of a permissible counter value (valid values: 0127, see also [PROG - Description of the command #TIMER] ).
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21168	Missing the programming of linear interpolation type.
	Description	Within the command sequence of an independent axis the programming of the interpolation type (G00/G01) is missing.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check the command sequence of the independent axis and complete the type of interpolation.
	Error type	1, Error message from NC-program.

21169	Given path excceeds the max. internal length limit.
	Description	A program path defined in the start-up list exceeds the permissible control internal length of the complete program call.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		7	Modify (shorten) the length of the program paths defined in the start-up list in that way (P-STUP-00018), that the combination with filenames do not exceed the permissible control internal length of the complete program call.
	Parameter	%1:	Limit value [-]
			Actual length of program path
	Error type	5, Error message by access on files.

21170	Given filename exceeds the max. internal length limit.
	Description	The combination of program path and filename exceeds the permissible control internal length of the complete program call.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		7	Shorten the length of the complete program call. There are 2 possibilities: Shorten the length of the filename. Modify (shorten) the program paths defined in the start-up list in that way (P-STUP-00018), that the file names can be maintained.
	Parameter	%1:	Limit value [-]
			Actual length of program path + filename
	Error type	5, Error message by access on files.

21171	ERROR-ID exceeds range of permissible values.
	Description	Within the #ERROR command the programmed error number (ID) exceeds the permissible range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the error number (ID).
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21173	Unknown error class in #ERROR command.
	Description	The error class (RC) programmed in the NC-command #ERROR has an invalid value.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Programming of a permissible error class (valid values are 0, 2 and 7, see also [PROG - Description of the command #ERROR] ).
	Parameter	%1:	Incorrect value [-]
			Invalid value of the error class.
		%2:	[-]

		%3:	[-]

		%4:	[-]

		%5:	[-]

	Error type	1, Error message from NC-program.

21174	The list contains an unknown element.
	Description	During interpretation of the lists an unknown list element is detected.
	Reaction	Class	1	NC start-up is continued.
	Solution	Class	7	Remove or modify the unknown list element in the corresponding list.
	Error type	-

21175	NC-command #CAX only with main spindle allowed.
	Description	The C-axis processing (# CAX [... ]) is to be selected for a spindle, which is currently not main spindle.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Modification of NC-program: There are 2 possibilities: Programming of C-axis processing for the current main spindle. First with #MAIN SPINDLE [...] change to the corresponding main spindle. Then selection of C-axis processing with this new main spindle.
	Error type	1, Error message from NC-program.

21176	Facing during active ACS or CS not allowed.
	Description	Whileactive cartesian transformation (# CS ON and/or #ACS ON) facing (#FACE) is to be selected.
	Reaction	Class	1	Abort of the NC program processing.
	Solution	Class	3	Deselection of the cartesian transformation (# CS OFF and/or # ACS OFF) before facing is selected.
	Error type	1, Error message from NC-program.

21177	Lateral surface processing during active ACS or CS not allowed.
	Description	Whileactive cartesian transformation (# CS ON and/or #ACS ON) a lateral surface processing (#CYL) is to be selected.
	Reaction	Class	1	Abort of the NC program processing.
	Solution	Class	3	Deselection of the cartesian transformation (# CS OFF and/or # ACS OFF) before the lateral surface processing is selected.
	Error type	1, Error message from NC-program.

21178	The NC-command ACS or CS cannot be used during active CAX-transformation.
	Description	While active C-axis processing (# CYL and/or # FACE) a cartesian transformation (# CS ON and/or # ACS ON) is to be selected.
	Reaction	Class	1	Abort of the NC program processing.
	Solution	Class	3	Deselection of the C-axis processing (# CYL OFF and/or # FACE OFF) before a cartesian transformation is selected.
	Error type	1, Error message from NC-program.

21179	Axis of a predefined M-function is also programmed as independent axis in the same NC-block.
	Description	The axis, which is assigned in the channel parameters to a M-function (P-CHAN-00039), is programmed in the same NC-block also as independent axis (see also [PROG - Chapter: Independent axes] ).
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Programming of the M-function and independent axis in separated NC-blocks.
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

21180	Unknown format token within the message string.
	Description	Within the #MSG command an unknown format string (%) is programmed.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the #MSG command. Permissible format strings are:%s , %S , %d , %D , %f , %F
	Parameter	%1:	Actual value [-]
			Incorrect format string.
	Error type	1, Error message from NC-program.

21182	The name of the external variable is too long.
	Description	The name of the external variable consists of too many characters.
	Reaction	Class		2	Start-up of the control is continued.
	Solution	Class		3	Name of the external variable is shortened implicitly on the maximum permissible length. To avoid the error message, adapt the name in the list [EXTV].
	Parameter	%1:	Limit value [-]
			Maximum number of allowed characters inclusive the final character.
		%2:	Incorrect value [-]
			Wrong number of characters.
	Error type	-

21183
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	2
	Solution	Class	8	Restart of NC-control necessary.

21184	CAX-spindle is not in axis mode CAX.
	Description	The spindle axis received by the NC-channel is a CAX-spindle axis, but it has not the correct axis mode.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify axis mode in axis parameter list (P-AXIS-00015).
	Parameter	%1:	Logical axis number [-]
			Logical axis number of CAX-spindle. P-AXIS-00016, P-CHAN-00036, P-CHAN-00051
	Error type	-

21185	Logical axis number exceeds range of data format.
	Description	The logical axis number programmed inside the drive parameter command exceeds thepermissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the drive parameter command.
	Parameter	%1:	Incorrect value [-]
			Incorrect logical axis number of the axis in the command. P-AXIS-00016, P-CHAN-00035
		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21187	Programmed NC-commands before label definition.
	Description	In NC block before a string label definition [STRINGLABEL] already other NC commands are programmed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Programming of the string label definition [STRINGLABEL] at the beginning of the NC block or directly behind the block number. Example: Wrong: N10 X100 [STRINGLABEL] Y200 Correct: N10 [STRINGLABEL] X100 Y200 or [STRINGLABEL] N10 X100 Y200
	Error type	1, Error message from NC-program.

21188	SIGNAL for open WAIT from given channel not expected.
	Description	The received signal comes from a channel, which is not specified in the WAIT.
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		7	Either send the signal from the correct channel or extend the WAIT by the unexpected channel.
	Parameter	%1:	Actual value [-]
			Number of the signal.
		%2:	Incorrect value [-]
			Number of the channel, the signal comes from.
	Error type	1, Error message from NC-program.

21189	Axis not found in command administration data.
	Description	For an axis programmed in the SERCOS command (#COMMAND..) no order could be created.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Axis must be a SERCOS axis.
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

21190	No more space in command administration data.
	Description	For an axis to much SERCOS command (#COMMAND..) are programmed.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Reduce number of SERCOS commands for this axis.
	Parameter	%1:	Logical axis number [-]

		%2:	Ident number [-]

		%3:	Limit value [-]

	Error type	1, Error message from NC-program.

21191
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21192	Channel parameters: Axis specific use of internal M-function not allowed.
	Description	An internal M-function is used in a axis specific contex. Either the M-function is axis specifically predefined in the channel parameters (P-CHAN-00039) or used in the NC program in an axis specific sequence of instructions [PROG]. In the NC-control internal M-functions have a firm meaning and are not freely available. Internal M-functions: M0, M1, M2, M3, M4, M5, M17, M19, M29, M30, M40 - M45 Exception: M0 and M1 may also be used axis specifically. Dependent on P-CHAN-00098 M3, M4, M5 and M19 also can be used axis specifically.
	Reaction	Class		2	Either the start-up of the control is continued and the wrong setting is removed or the NC program is aborted.
	Solution	Class		3	Check and modify the settings of the channel parameters (P-CHAN-00039) or remove the M-functions in the NC program from the axis specific sequence of instructions.
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

21193	ECS: Tool vector has length 0 (KIN ID 0: see wz_kopf_versatz[0],[1],[2]).
	Description	The tool vector, especially necessary during 2.5 D processing for the tool retraction on inclined planes in a ECS system, is not defined in the channel parameter list (kinematic parameters of ID 0).
	Reaction	Class		3	Abort of the NC program processing.
	Solution	Class		3	Check and modify the meant channel parameters. A non-standard tool vector (0,0,1) can be defined by the elements of P-CHAN-00094 under the kinematic-ID 0. Example: Tool vector for a plane, rotated 45° around Y: kinematik[0].param[0] 0.707 kinematik[0].param[1] 0 kinematik[0].param[2] 0.707
	Parameter	%1:	Actual value [-]
			Active kinematic ID
	Error type	-

21195
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21196	No memory (channel / global) for external variable configured.
	Description	In the external variable list an invalid identification is entered for the scope of validity (element scope).
	Reaction	Class		2	Start-up of the control is continued. The incorrect identification is replaced implicitly by the identification VE_CHANNEL. Also the external address of this variable is calculated, but not checked for plausibility.
	Solution	Class		7	In the list correct initialization of external variable [EXTV].
	Parameter	%1:	Incorrect value [-]
			Value of the incorrect identification.
		%2:	Corrected value [-]
			Value of the corrected identification (VE_CHANNEL).
		%3:	Corrected value [-]
			Corrected address of the external variable.
		%4:	Actual value [-]
			Index of the incorrect, but corrected external variable.
	Error type	-

21197	Too many external variables, no more internal memory.
	Description	The memory made available by the control is not sufficient to read in and to store all external variables during start-up.
	Reaction	Class	2	Start-up of the control is continued. The external variables which were read in after memory overflow are not stored inside the control, so they are not available after start-up.
	Solution	Class	7	In the list of external variables [EXTV] too large arrays are defined. Reduce number of array variables or reduce array sizes.
	Error type	-

21198	Feed link factor exceeds range of data format.
	Description	Within the command for the coupling of spindle speed and path feed (F_LINK) a coupling factor (FACT or CORR) exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC command. Program a value within the permissible data range.
	Parameter	%1:	Incorrect value [-]
			Incorrect coupling factor Hint: For FACT multiple ID 1 is valid. For CORR multiple ID 2 is valid.
		%2:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21199	Compare Operator '==' expected.
	Description	Within a $IF control block the result of an EXIST-access for TRUE or FALSE is checked. For this check of the condition the assignment operator "=" is used.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC block. For the check of TRUE or FALSE the comparison operator "==" has to be used.
	Error type	1, Error message from NC-program.

21200	At block search position no wait for enabling. Processing start is ignored.
	Description	The block search has been assigned with processing start by the user interface, which is not permissible at the current state, because at the block search position no wait for enabling is active.
	Reaction	Class	1	NC program processing is continued.
	Solution	Class	1	Check,why the user interface has assigned the unexpected block search action.
	Error type	-

21201	Double programming of spindle feed forward control.
	Description	Error messages is output in use of programming spindle feed forward control (G135, G136, G137). Either excluding feed forward control commands are programmed (G135,G137) or the commands are programmed several times [PROG].
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC command. Remove redundant or exclusive commands.
	Error type	1, Error message from NC-program.

21202	For a PLC-spindle this command is not available.
	Description	In use of the (spindle-)axis specific programming, for a so-called PLC spindle (P-CHAN-00069) not permissible NC commands are programmed. Only the standard functions M3,M4,M5,M19, REV and POS may be used.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Remove all commands from (spindle-) axis specific programming with exception of the listed above or deselect eventually corresponding pre defined functions (P-CHAN-00039, P-CHAN-00025).
	Parameter	%1:	Incorrect value [-]
			Number of the incorrect M-/H-/G-functions
	Error type	1, Error message from NC-program.

21203	Channel parameters: Synchronization mode MET_SVS needs pre output time greater than or equal to NC-cycle time of control.
	Description	During start-up for M-/H-functions with synchronisation mode MET_SVS the check of the assigned pre output time P-CHAN-00070 / P-CHAN-00107 detects, that these time is smaller than the cycle time.
	Reaction	Class		1	NC start-up is continued.
	Solution	Class		1	Check and modify the pre output time P-CHAN-00070 / P-CHAN-00107 before next start-up for the meant M-/H-functions in the channel parameters. During start-up in case of conflict the pre output time is set to cycle time and the start-up is continued.
	Parameter	%1:	Actual value [-]
			Number of the M-/H-function Hint: For M-functions multiple ID 1 is valid. For H-functions multiple ID 2 is valid.
		%2:	Incorrect value [-]
			Incorrect pre output time.
		%3:	Corrected value [-]
			Automatic corrected pre output time (= cycle time)
	Error type	2, Error message by data transfer from parameter list into control device.

21204	Max. number of Look-ahead M-/H-functions per NC-block exceeded.
	Description	The maximum number of look ahead M-/H-functions with synchronisation modes MET_SVS / MEP_SVS (see P-CHAN-00070) programmed in the NC block is exceeded.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	If possible splitting of the meant M-/H-functions on several NC movement blocks or reduction of the number of M-/H-functions within the NC block.
	Parameter	%1:	Limit value [-]

		%2:	Incorrect value [-]
			Number of the look ahead M-/H-functions programmed in the NC block.
	Error type	1, Error message from NC-program.

21205	Velocitiy limit on the path is negative or zero.
	Description	The velocity limit on the path programmed with #VECTOR LIMIT ...[...] or#VECTORVEL ON is negativ or zero.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the command. Programmed velocity limit must have a positive value larger than zero.
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

21206	Acceleration limit on the path is negative or zero.
	Description	The acceleration limit on the path programmed with #VECTOR LIMIT ... [...] or #VECTORACC ON is negative or zero.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the command. Programmed acceleration limit must have a positive value larger than zero.
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

21207	Change in external tool management, new start of system necessary.
	Description	The modification of P-CHAN-00016 shall be updated while active control by reinterpretation of the channel parameter list.
	Reaction	Class		2	Start-up of the control is aborted.
	Solution	Class		7	For the update of the modification of P-CHAN-00016 a restart of the control is necessary.
	Parameter	%1:	Actual value [-]
			Name of the channel parameter.
		%2:	Corrected value [-]

	Error type	2, Error message by data transfer from parameter list into control device.

21208	Filename not defined.
	Description	Behind the call of a subprogramm in the case of LL the name of a local subprogram and in the case of L the file name of a global subprogram is missing.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Complete behind LL the name of a local subprogram and behind L the file name of a global subprogram [PROG].
	Error type	1, Error message from NC-program.

21209	No feed axes defined. Main axes are set to feed axes.
	Description	If in the channel parameters no axes as feed axes are configured (P-CHAN-00011) and also P-CHAN-00096 is set to 0, in use of programming #FGROUP all main axes implicitly are set to feed axes.
	Reaction	Class	1	NC program processing is continued.
	Solution	Class	1	Define with the command #FGROUP or in the channel parameters (P-CHAN-00011, P-CHAN-00096) axes as feed axis.
	Error type	1, Error message from NC-program.

21210	Too many hardware numbers programmed.
	Description	In the command #SIGNAL the keyword HW is programmed several times.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the NC command. Remove redundant keyword from command #SIGNAL.
	Parameter	%1:	Actual value [-]
			Programmed redundant hardware number.
	Error type	1, Error message from NC-program.

21211	Hardware ID exceeds range of data format.
	Description	The hardware ID programmed in the NC command #SIGNAL exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the NC program. The permissible hardware ID are defined in the start-up list [STUP].
	Parameter	%1:	Incorrect value [-]
			Incorrect hardware-ID.
		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21212	Programmed HW-ID is not known (s. parameter list of NC).
	Description	The value of the hardware ID programmed in the NC command #SIGNAL is unknown.
	Reaction	Class		1	Abort of the NC program processing.
	Solution	Class		1	Check and modify the NC program. If the hardware ID is programmed correctly, then ensure that the hardware ID is entered correctly in the start-up list [STUP].
	Parameter	%1:	Incorrect value [-]
			Incorrect hardware-ID.
	Error type	1, Error message from NC-program.

21213	Double programming of AHEAD.
	Description	In the command #WAIT the keyword AHEAD is programmed several times.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC command.
	Error type	1, Error message from NC-program.

21215	Invalid ESC-parameter configured.
	Description	In use of the #ECS command it is detected, that the necessary channel parameters are wrongly configured.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Correct setting of the ECS parameters in the channel parameter list: kind_of_2nd_ecs_ax[0] (P-CHAN-00031) mach_plane_of_2nd_ecs_ax[0] (P-CHAN-00050) Reinterpret channel parameter list after modification.
	Parameter	%1:	Incorrect value [-]
			Incorrect channel parameters as string.
	Error type	1, Error message from NC-program.

21216	Variable is an array, index not programmed.
	Description	At a array-V.xx-variable the index is missing.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the variables within the NC block.
	Error type	1, Error message from NC-program.

21217	Closing bracket of index is missing.
	Description	At a V.xx-variable with index behind the index "]" is missing.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the variables within the NC block.
	Error type	1, Error message from NC-program.

21218	Type of variable is not available.
	Description	In NC program variables of type V.L. are used. Because of version specific configuration this possibility is not allowed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Replace V.L. variables by V.S. or V.G. variables or P parameters. Or please contact the CNC manufacturer, to enable in this version the use of V.L. variables.
	Error type	1, Error message from NC-program.

21219	Double programming in #MACHINE DATA-command.
	Description	In the command #MACHINE DATA syntax elements are programmed several times.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC command.
	Error type	1, Error message from NC-program.

21220	Unknown or incomplete token in NC-command.
	Description	Within a NC command a token is programmed, which can not be decoded by the control. The cause can be a write error or a not permissible or incompletely keyword in connection with the command itself.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC command.
	Error type	1, Error message from NC-program.

21226 / 21227
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21230	Excursion of oscillation is 0.
	Description	Within the oscillating axis command the excursion (EXCUR) is too small or zero.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the oscillating axis command.
	Parameter	%1:	Incorrect value [-]
			Incorrect excursion.
	Error type	1, Error message from NC-program.

21231	Missing zero position programming.
	Description	Within the oscillating axis command at specifying of the oscillation travel distance via excursion no zero position is defined.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the oscillating axis command.
	Error type	1, Error message from NC-program.

21232	Unknown format string.
	Description	Within the #MSG command an unknown format string (%) is programmed.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the #MSG command. Permissible format strings are:%s , %S , %d , %D , %f , %F
	Parameter	%1:	Actual value [-]
			Incorrect format string.
	Error type	1, Error message from NC-program.

21233
	Description	This error message informs about internal states, error solutions and the place of error in the source.Please give the complete error message data to the CNC manufacturer.
	Reaction	Class	3
	Solution	Class	8	Restart of NC-control necessary.

21234	Number of permissible (A)CS definitions exceeded.
	Description	The number of defined (A)CS coordinate systems within the NC program exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Reduce the number of (A)CS definitions or modify the NC program in the way, that no more required (A)CS definitions in the further program processing can be used for new definitions.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21235	Double programming in #WCS/MCS-command.
	Description	In the NC commands#WCS TO MCS [...] or #MCS TO WCS [...] syntax elements are programmed several times.
	Reaction	Class	2	Abort of the running NC-program.
	Solution	Class	3	Check and modify the NC program. Remove redundant or exclusive syntax elements from the NC commands.
	Error type	1, Error message from NC-program.

21236	NC-command during active transformation not allowed.
	Description	The commands #WCS TO MCS or #MCS TO WCS may not be programmed during active cartesian ((#(A)CS ON) or kinematic transformation (#TRAFO ON / #RTCP ON).
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Before use of the commands #WCS TO MCS or #MCS TO WCS deselection of all active transformations (#TRAFO OFF / RTCP OFF, #(A)CS OFF).
	Error type	1, Error message from NC-program.

21237	Number of oscillations exceeds range of data format.
	Description	Within the oscillating axis command the programmed number of oscillations (NBR_OSC) exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the oscillating axis command.
	Parameter	%1:	Incorrect value [-]
			Incorrect number of oscillations.
		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21238	Path axis configured in channel parameters may not be a SAI-axis or spindle.
	Description	A path axis configured in the channel parameter list is a single axis (SAI, PLCOpen) resp. a spindle axis.
	Reaction	Class		3	Start-up of the control is aborted.
	Solution	Class		7	Either in the channel parameter list the axis may not be configured as path axis (P-CHAN-00035), or in the axis parameter list the SAI-property must be deselected (P-AXIS-00250).
	Parameter	%1:	Logical axis number [-]

		%2:	Actual value [-]
			Index of the axis within the axis group [CHAN-chapter Axis structure]
	Error type	-

21239	Spindle command is disabled.
	Description	Wrong setting for a synchronisation mode of a spindle function.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the synchronisation modes of the spindle functions in the channel parameter list: REV (P-CHAN-00081) M3 (P-CHAN-00045) M4 (P-CHAN-00047) M5 (P-CHAN-00049) M19 (P-CHAN-00043) Reinterpret channel parameter list after modification.
	Parameter	%1:	Incorrect value [-]
			Incorrect spindle function
		%2:	Logical axis number [-]
			Logical axis number of the meant spindle axis P-CHAN-00036
	Error type	-

21240	G-command has no effect, because precontrol is disabled in one axis.
	Description	Precontrol can not be selected in one axis, because this axis is blocked by P-AXIS-00256.
	Reaction	Class		1	NC program processing is continued.
	Solution	Class		1	Set in the meant axis P-AXIS-00256 to 0.
	Parameter	%1:	Actual value [-]
			Number of the G command
		%2:	Logical axis number [-]

		%3:	Incorrect value [-]
			Value of P-AXIS-00256
	Error type	1, Error message from NC-program.

21241	Value exceeds definition range of trigonometric function.
	Description	The value programmed with the trigonometric function exceeds the definition range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify trigonometric function.
	Parameter	%1:	Incorrect value [-]

		%2:	Actual value [-]
			Incorrect trigonometric function.
	Error type	1, Error message from NC-program.

21242	Value prog. with D exceeds range of data format.
	Description	The value programmed with the D word exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify D word. Program a value within the permissible data range.
	Parameter	%1:	Incorrect value [-]
			Incorrect value behind D.
		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

21243	In spindle specific syntax the D-command for main spindle is not allowed.
	Description	The D word is programmed inside the spindle specific command sequence of the main spindle. Example: Wrong: N10 S[REV1000 M3 D5] Correct: N10 D5S[REV1000 M3]
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Program D word outside the spindle specific command sequence of the main spindle.
	Error type	1, Error message from NC-program.

21244	Channel parameters: T with implicit FLUSH without active "t_info_to_wzv" is not useful.
	Description	Setting P-CHAN-00106 to 1 is only useful, if P-CHAN-00087 is also set to 1.
	Reaction	Class		1	Start-up of the control is continued.
	Solution	Class		1	Parameter is set implicitly to default value 0.
	Parameter	%1:	Incorrect value [-]
			Incorrect channel parameter P-CHAN-00106
		%2:	Corrected value [-]

	Error type	2, Error message by data transfer from parameter list into control device.

21247	Active transformations on program end.
	Description	At program end (M02, M30) coordinate systems (transformations) selected by the command #CS ON / #ACS ON are still active.
	Reaction	Class	1	NC program processing is continued.
	Solution	Class	1	Edit NC program. Enter CS OFF / #ACS OFF resp. #CS OFF ALL / #ACS OFF ALL before program end.
	Error type	1, Error message from NC-program.

21248	Deselection of axis tracking has no effect.
	Description	Axis tracking is deselected by #CAXTRACK OFF, although no axis tracking is active.
	Reaction	Class	2	NC program processing is continued.
	Solution	Class	1	Delete #CAXTRACK OFF from NC program.
	Error type	1, Error message from NC-program.

21249	Axis tracking during active (A)CS only for rotation around Z-axis allowed.
	Description	It is tried to select axis tracking in a coordinate system defined by #CS or #ACS, which is turned in several axes. Axis tracking in a coordinate system defined by #CS or #ACS is only permissible, if the new coordinate system is shifted parallel in X/Y plane and turned only around Z.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Define a suitable coordinate system with #CS or #ACS or reclamp the workpiece in a position which allows the definition of a suitable coordinate system for axis tracking.
	Error type	1, Error message from NC-program.

See also

Troubleshooting classes