ID-range 20000-20249

20002	Troubleshooting classes
	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.

20003	G-code only sensible with programming of an axis.
	Description	The programmed G-function for syntactical reasons or for the programming of additional information mandatory requires the name of an axis as argument. Warning: Behind the axis name, a value for the co-ordinate is also MANDATORY, otherwise subsequent error message. That value will be interpreted differently according to the programmed G-function. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G160=2 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G160=2 X1 Z1 N1000 M30
	Reaction	Class		1	NC program processing is continued.
	Solution	Class		1	Programming of the additional axis information for the G-function.
	Parameter	%1:	Actual value [-]

	Error type	1, Error message from NC-program.

20007	Spindle speed is 0.
	Description	With NC command G63 the spindle speed must be unequal to zero. Example: Wrong : N10 G63 Z10 F300 S0 Correct : N10 G63 Z10 F300 S17
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Adjusting of spindle speed, feed and used pitch [PROG - Chapter Tapping].
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

20008	Feed rate in motion block is 0.
	Description	At least the first motion command with interpolation (e.g. G01, G02, G03) requires a feed value (F-word). Example: Wrong: N10 G00 X0 Y0 Z0 N20 G01 X10 Correct: N10 G00 X0 Y0 Z0 N20 G01 X10 F1000
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Program a feed value (F word).
	Error type	1, Error message from NC-program.

20010	Programmed function requires at least one axis.
	Description	A previous axis release prevents this G-function from executing. Example circular interpolation: Wrong: N10 #PUT AX[X] N20 G2 R10 Y20 F200 Correct: Solution (do NOT return axis): ... N20 G2 R10 Y20 F200
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Remove unallowed axis release from NC-program code.
	Error type	1, Error message from NC-program.

20011	Coordinate exceeds range of data format.
	Description	The acceptable range for coordinates is exceeded. A movement command with calculated target coordinates outside this acceptable range was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 X94967596 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the coordinates in the NC-program or check data (e.g. offset values) involved in calculation. For information always all possibly invalid values, involved in calculation are monitored.
	Parameter	%1:	Logical axis number [-]

		%2:	Lower limit value [0.1 µm or 0,0001°]
			Limit value for negative coordinates
		%3:	Upper limit value [0.1 µm or 0,0001°]
			Limit value for positive coordinates.
		%4:	Incorrect value [0.1 µm or. 0,0001°]
			Programmed coordinate or calculated value in internal unit
		%5:	Incorrect value [0.1 µm or. 0,0001°]
			Further programmed coordinate or calculated value in internal unit (optional)
	Error type	1, Error message from NC-program.

20012	Radius or bevel is 0 in G301/302.
	Description	For chamfers and rounding of corners an I-value as distance parameter is necessary. Example 1 (Chamfers): Wrong: N10 G00 X0 Y0 Z0 N20 G01 X10 F2000 N30 G301 N40 G01 Y10 N1000 M30 Correct : N10 G00 X0 Y0 Z0 N20 G01 X10 F2000 N30 G301 I5 N40 G01 Y10 N1000 M30 Example 2 (Rounding): Wrong: N10 G00 X0 Y0 Z0 N20 G01 X10 F2000 N30 G302 N40 G01 Y10 N1000 M30 Correct : N10 G00 X0 Y0 Z0 N20 G01 X10 F2000 N30 G302 I5 N40 G01 Y10 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Programming of missing I-value.
	Error type	1, Error message from NC-program.

20013	Dwell time is programmed directly and via coordinate.
	Description	A dwell must be programmed stand-alone within a NC block, without any additional motion commands. It can be defined directly or in conjunction with the name of the first main axis. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G04 10 X2 N1000 M30 Correct: Dwell directly N10 G00 X0 Y0 Z0 N20 G04 10 N1000 M30 Correct: Dwell with name of first main axis N10 G00 X0 Y0 Z0 N20 G04 X2 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify dwell time after G04.
	Error type	1, Error message from NC-program.

20014	Dwell time is not programmed with the coordinate of first axis.
	Description	The dwell was programmed as coordinate of any axis, instead of using the first main axis. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G04 Y2 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G04 X2 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	After G04 programming of the first main axis for the definition of the dwell time.
	Error type	1, Error message from NC-program.

20015	Dwell time exceeds range of data format.
	Description	The dwell time exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check the programmed dwell time and modify it according to the data range.
	Parameter	%1:	Incorrect value [1 µsec]

		%2:	Lower limit value [1 µsec]
			Lower limit value.
		%3:	Upper limit value [1 µsec]
			Upper limit value
	Error type	1, Error message from NC-program.

20016
	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.

20017	Negative dwell time programmed.
	Description	The dwell time exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		1	Check the programmed dwell time and modify it according to the data range.
	Parameter	%1:	Incorrect value [1 µsec]

	Error type	1, Error message from NC-program.

20019	Diameter programming is not allowed to mirror on the primary axis.
	Description	Activated diameter programming assumes parts, which have a rotational symmetry, the programmed co-ordinates are interpreted as distance to the rotational (symmetry) axis. Therefore mirroring and negative co-ordinates are illegal on those axis. Example: Wrong : N10 G90 G01 F1000 N20 G51 X80 N30 G92 X10 N40 X0 N50 G91 X50 N60 G21 X30 N1000 M30 Correct : N10 G90 G01 F1000 N20 G51 X80 N30 G92 X10 N40 X0 N50 G91 X50 N60 X30 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove NC mirroring command.
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

20020	Centre coordinate exceeds range of data format.
	Description	An interpolation parameter (I, J, K) exceeds the permissible data range(e.g. during circular interpolation). Example: Wrong: N10 G00 X0 Y0 Z0 N20 G02 I94967596 F1000 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check the programmed interpolation parameters (I, J, K) and modify it according to the data range.
	Parameter	%1:	Logical axis number [-]

		%2:	Upper limit value [-]

		%3:	Lower limit value [-]

		%4:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20021	Negative diameter programmed.
	Description	Activated diameter programming assumes parts, which have a rotational symmetry, the programmed co-ordinates are interpreted as distance to the rotational (symmetry) axis. Therefore mirroring and negative co-ordinates are illegal on those axis. Example: Wrong: N10 G90 G01 F1000 N20 G51 X80 N30 G92 X10 N40 X0 N50 G91 X50 N60 G90 X-50 N1000 M30 Correct: N10 G90 G01 F1000 N20 G51 X80 N30 G92 X10 N40 X0 N50 G91 X50 N60 G90 X50 N1000 M30
	Reaction	Class		2	Abort of the running NC-program.
	Solution	Class		3	Check and modify NC program. Avoid negative co-ordinates or mirroring.
	Parameter	%1:	Logical axis number [-]

		%2:	Actual value [0.1 µm or 0,0001°]

		%3:	Limit value [0.1 µm or 0,0001°]

	Error type	1, Error message from NC-program.

20022	Negative software limit switch exceeds range of data format.
	Description	The programmed negative software limit switch (G98) exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G98 X-94967596 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Program the neg. software limit switch within the permissible data range.
	Parameter	%1:	Logical axis number [-]

		%2:	Lower limit value [-]
			Lower limit value.
		%3:	Upper limit value [-]
			Upper limit value.
	Error type	1, Error message from NC-program.

20023	Positive software limit switch exceeds range of data format.
	Description	The programmed positive software limit switch (G99) exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G99 X94967596 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Program the pos. software limit switch within the permissible data range.
	Parameter	%1:	Logical axis number [-]

		%2:	Lower limit value [-]
			Lower limit value
		%3:	Upper limit value [-]
			Upper limit value
	Error type	1, Error message from NC-program.

20024	Measured value cannot be considered as it was not requested for.
	Description	If there wasn’t any previous measuring sequence, then there are no measured values available for calculations. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G101 X1 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G100 X10 F100 N30 G101 X1 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Before the access on the measured values firstly execute the measuring sequence.
	Error type	1, Error message from NC-program.

20025	Negative ramp time weighting programmed.
	Description	The ramp time weighting with G132 was programmed with a negative value. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G132 X-10 N1000 M30
	Reaction	Class		1	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Program ramp time weighting with a positive value.
	Parameter	%1:	Logical axis number [-]

		%2:	Incorrect value [0,1%]

		%3:	Limit value [0,1%]
			Lower limit value.
	Error type	1, Error message from NC-program.

20028	Negative precontrol weighting programmed.
	Description	The precontrol weighting with G136 was programmed with a negative value. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G136 X-10 N1000 M30
	Reaction	Class		1	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Program precontrol weighting with a positive value.
	Parameter	%1:	Logical axis number [-]

		%2:	Incorrect value [0,1%]

		%3:	Limit value [0,1%]
			Lower limit value
	Error type	1, Error message from NC-program.

20029	Illegal gear step.
	Description	The number of available gear steps and thus the allowed range of values depends on system configuration. The enumeration of gear steps starts with 1, therefore values smaller than 1 are prohibited. Also values starting from 65536 and above are rejected as well. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G112 X0 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programme a correct value for the gear step.
	Parameter	%1:	Incorrect value [-]

		%2:	Limit value [-]
			Lower limit value
		%3:	Logical axis number [-]

	Error type	1, Error message from NC-program.

20030	Gear step exceeds range of data format.
	Description	The number of available gear steps and thus the allowed range of values depends on system configuration. The enumeration of gear steps start with 1, therefore values smaller than 1 are prohibited. Also values starting from 65536 and above are rejected as well. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G112 X65536 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programme a correct value for the gear step.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

		%4:	Logical axis number [-]

	Error type	1, Error message from NC-program.

20032	Slave axis is programmed, but moving distance is 0.
	Description	The calculated moving distance for a programmed slave axis for tapping is zero, so the tapping can not be executed. Example: Wrong: ( current position : 0) N10 G63 C0 F100 S100 Correct: ( current position : 0) N10 G63 C123 F100 S100
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Program a correct depth for tapping.
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

20033	Circle with programmed radius impossible.
	Description	Circle construction is geometrically impossible with programmed radius. The radius is to small. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G02 X10 R1 F1000 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G02 X10 R7 F1000 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Change the radius. At least this means, increase the radius, until the circle intersects the programmed end point.
	Parameter	%1:	Incorrect value [0.1 µm or 0,0001°]
			Invalid radius.
		%2:	Actual value [0.1 µm or 0,0001°]
			Starting position in 1. main axis
		%3:	Actual value [0.1 µm or 0,0001°]
			Starting position in 2. main axis
		%4:	Actual value [0.1 µm or 0,0001°]
			End position in 1. main axis
		%5:	Actual value [0.1 µm or 0,0001°]
			End position in 2. main axis
	Error type	1, Error message from NC-program.

20034	Circle starting point and circle end point are identical.
	Description	Specifying only the radius does not meet for a full circle, since this specification would allow an indefinite number of circles – the circle center could lay on a full circle with radius R around the start / end point. Therefore, it is necessary to program full circles via the center point instead of using the radius. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G02 X0 Y0 R10 F1000 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G02 I10 F1000 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Always program full circles via the center point definition.
	Error type	1, Error message from NC-program.

20035	Difference between programmed and calculated center point too big.
	Description	During active center point correction (G165) based on the programmed center point coordinates I, J, K a center point is calculated. If this calculated center point differs too much from the programmed center point ( P-CHAN-00059), this error message is indicated. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G02 X10 I7 F1000 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G02 X10 I5 F1000 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Change the center point coordinates. Check the dimension (absolute/ relative) of center point programming (G161/G162). Possibly complete missing center point coordinates.
	Parameter	%1:	Actual value [0.1 µm or 0,0001°]

		%2:	Limit value [0.1 µm or 0,0001°]

	Error type	1, Error message from NC-program.

20036	Radius of circle is 0.
	Description	During inactive center point correction (G164 the center point co-ordinates I, J, K are zero or still not programmed or the programmed co-ordinates of the circle end point are identical to the co-ordinates of the start point. From the calculation of the center point results a circle radius with the value zero and this error message is indicated. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G164 G02 X10 F1000 (Missing center point co-ordin.) N1000 M30 Wrong: N10 G00 X0 Y0 Z0 N20 G164 G02 X0 F1000 (circle end point = start point) N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G164 G02 X10 I5 F1000 N1000 M30
	Reaction	Class	2	Abort of the running NC-Program.
	Solution	Class	3	Correction of the invalid center point co-ordinates I,J,K or circle end points.
	Error type	1, Error message from NC-program.

20037	#ACHSE is programmed without G200/201/202.
	Description	The NC command #ACHSE[] was programmed but can not be evaluated, because in the same NC block G200/G201/G202 is missing. Example: Wrong: N10 G00 X0 Y0 Z0 N20 #ACHSE[X] N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G201 #ACHSE[X] N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Add G200 / G201 / G202.
	Error type	1, Error message from NC-program.

20038	Programming G201 the command #ACHSE is expected.
	Description	The NC command G201 (manual mode with parallel interpolation) requests at least one axis to be selected for activation. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G201 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G201 #ACHSE[X] N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Complete G201 with NC command #ACHSE[..].
	Error type	1, Error message from NC-program.

20041	Motion information is required for MNE_SNS function.
	Description	M-functions of type MNE_SNS trigger on an external event and interrupt the current motion block accordingly. Therefore, they are useless without a programmed motion information at the same time. Example: Wrong: M33 M30 Correct: G01 X150 Y200 M33 F8 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Add a motion information.
	Error type	1, Error message from NC-program.

20042	No face turning axis available for diameter programming.
	Description	When selecting diameter programming, there is exactly one face turning axis required within the working face selected by G17, G18 or G19. Appearance of this error message because of G51 therefore indicates a configuration problem within the axis parameters list.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Change the configuration. Definition of a face turning axis P-AXIS-00015.
	Error type	1, Error message from NC-program.

20044	BACO parameter exceeds range of data format or range of permissible values.
	Description	Within the command #CONTOUR MODE the value of the keyword REMAIN_PART is out of the permissible data range.
	Reaction	Class		2	NC program processing is continued.
	Solution	Class		3	Invalid value is corrected, and NC program processing is continued.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20045	SLOPE parameter exceeds range of data format.
	Description	One of the programmed slope parameters exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 #SET SLOPE PROFIL[2222222222, 0, 0] N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Change the value of the invalid parameter.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20048	Centre point coordinate within linear motion block ignored.
	Description	Centre point co-ordinates (I,J,K) within a linear motion block (G01) are ignored. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G01 I10 X10 F1000 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G01 X10 F1000 N1000 M30
	Reaction	Class	1	NC program processing is continued.
	Solution	Class	1	Check and modify NC program. Remove the Centre point co-ordinates (I,J,K).
	Error type	1, Error message from NC-program.

20049	TRC selected within measuring cycle.
	Description	If the TRC functionality (tool radius compensation) is active, no measuring cycle (G100) can be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 (activates TRC) N20 G41 X100 F1000 (attempts to start measuring cycle) N30 G100 X0 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program sequence. Before selection of measuring cycle deselection of TRC via G40.
	Error type	1, Error message from NC-program.

20050	Old measured value is still considered.
	Description	During a measurement movement, the offset from the last measurement movement is still active. This is an error condition. Please be aware, that before any measurement movement deactivating the existing offset using G102 is as well mandatory as making sure, that the measurement probe is reached during the movement! Example: Wrong: N5 X0 N10 G100 X20 F1000 N20 G101 X1 N30 G100 X10 N40 G101 X1 M30 Correct: N5 X0 N10 G100 X20 F1000 N20 G101 X1 N22 G1 X0.4711 F1000 N25 G102 X1 N30 G100 X10 F1000 N40 G101 X1 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program sequence. Before selection of measuring cycle deselection of old measuring offset via G102.
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

20051	Homing for axes in manual operation mode illegal.
	Description	An axis with activated manual operation mode cannot perform a homing motion. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G201 #ACHSE [X] N30 X100 N40 G74 X1 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G201 #ACHSE [X] N30 X100 N35 G202 N40 G74 X1 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program sequence. Before G74 (homing) programming of G202 ( deselection of manual operation mode).
	Parameter	%1:	Logical axis number [-]
			Axis, which is still in manual operation mode.
	Error type	1, Error message from NC-program.

20052	This NC-block requires axes being programmed.
	Description	Together with a special NC command in the same NC block at least one axis must be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N30 G100 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N30 G100 X10 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Complete the NC command for the required axes information.
	Error type	1, Error message from NC-program.

20054	Corrected center point exceeds range of data format.
	Description	The values chosen for start / end point and radius imply center co-ordinates, which lay outside the acceptable range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G02 X1 R1000000 F1000 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G02 X1 R0.5 F1000 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Change the value of the radius.
	Parameter	%1:	Logical axis number [-]
			Axis with the exceeded data range
		%2:	Upper limit value [-]

		%3:	Lower limit value [-]

		%4:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20055
	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.

20057	Tool compensation exceeds range of data format.
	Description	During the removing of the tool based corrections the permissible data range is exceeded.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the tool corrections. Possibly for one of the axes a too large tool correction is defined or the tool change is executed at a position, which is too near at the data range limit. In this case move to another position to consider the tool correction.
	Parameter	%1:	Logical axis number [-]

		%2:	Incorrect value [0.1 µm or 0,0001°]

		%3:	Lower limit value [-]

		%4:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20063	Considering the tool radius exceeds range of data format.
	Description	During the calculation of the tool radius the permissible data range is exceeded.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the tool corrections. Change the defined tool radius P-TOOL-00004.
	Parameter	%1:	Logical axis number [-]

		%2:	Actual value [-]

		%3:	Lower limit value [-]

		%4:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20064	Face turning axis is used twice in processing plane.
	Description	Only one axis, the first or the second main axis can be used as face turning axis. But in this case both axes have the same characteristic as face turning axis ( P-AXIS-00015).
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the axes parameter settings. Only one of the main axes may be defined as face turning axis P-AXIS-00015.
	Parameter	%1:	Logical axis number [-]

	Error type	-

20065	Considering the tool offsets exceeds range of data format.
	Description	During the calculation of the tool based corrections the permissible data range is exceeded.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the tool corrections. Change the defined tool offsets P-TOOL-00006.
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

20066	Considering the zero offsets exceeds range of data format.
	Description	During the calculation of the zero shifts the permissible data range is exceeded.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the zero shifts. Change the defined zero shift parameters P-ZERO-00003.
	Parameter	%1:	Logical axis number [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20068 - 20073
	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.

20075	Considering the measured value exceeds range of data format.
	Description	During the calculation of the measurement offset based on the measured value the permissible data range is exceeded. .
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Possibly check the latched measured values in the PLC.
	Parameter	%1:	Logical axis number [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20076	Considering the command value exceeds range of data format.
	Description	During the calculation of the command values the permissible data range is exceeded.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check plausibility of current command values.
	Parameter	%1:	Logical axis number [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20077
	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.

20078	Clamp position index exceeds range of permissible values.
	Description	The clamp position index, entered in the program job sequence, has an invalid value.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		6	Check the program job sequence. Enter a correct clamp position index P-CLMP-00001.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	-

20079	Coordinate initialization exceeds range of data format.
	Description	At program start or RESET during initialization of axes coordinates the permissible data range is exceeded.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		6	Repeat program start or RESET.
	Parameter	%1:	Actual value [-]
			Actual axis position
		%2:	Actual value [-]
			Programmed axis position
		%3:	Logical axis number [-]

		%4:	Lower limit value [-]

		%5:	Upper limit value [-]

	Error type	-

20083	Write access to tool radius is not allowed with D-code in the same block.
	Description	A D word within the block reads miscellaneous parameters like tool length, tool radius etc.. Therefore, it is inhibited to write to the tool radius within the same block. Example: Wrong: N10 G00 X0 Y0 Z0 N20 D1 V.G.WZR=3 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 V.G.WZR=3 N30 D1 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program sequence. Program D word in the following NC block after the write access.
	Error type	1, Error message from NC-program.

20084
	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.

20085	Too many external variables provided.
	Description	There are too many external variables (global and channel specific) declared in the list [EXTV] or the given number of external variables in the parameter „anzahl_belegt“ is wrong. The maximum permissible limit of external variables can be found in [SYSP]. Example: anzahl_belegt 500 # var[0].name VARIABLE_1 var[0].type SGN32 # ... # var[100].name VARIABLE_100 var[100].type UNS32 Possible solutions: Check if the parameter „anzahl_belegt“ contains the correct number of external variables If there are in fact too many variables, you can try to combine variables to variable arrays (same data type) or variable structures (different variable types): Variable-Array: anzahl_belegt 1 # var[0].name VAR_ARRAY_100 var[0].type UNS32 var[0].array_elements 100 Variable-structure: anzahl_belegt 2 # struct[0].name STRUCT_DEF struct[0].element[0].name VARIABLE_1 struct[0].element[0].type SGN32 struct[0].element[1].name VARIABLE_2 struct[0].element[1].type UNS32 # var[0].name VAR_STRUCT var[0].type STRUCT_DEF # var[1].name VAR_STRUCT_ARRAY var[1].type STRUCT_DEF var[1].array_elements 50
	Reaction	Class		2	Not all configured variables are generated.
	Solution	Class		3	Check if the given number in the parameter „anzahl_belegt“ is correct. Combine the external variable declarations in the list [EXTV].
	Parameter	%1:	Incorrect value [-]
			Number of configured external variables
		%2:	Limit value [-]
			Maximum permissible limit
	Error type	-

20087	Maximum number of external variables in one NC-block exceeded.
	Description	In NC program for external variables the read/write access can be executed synchronous to the processing. In this case the maximum permissible number per NC block is limited. If this maximum permissible number is exceeded, this error message is issued. The characteristic "synchronous read/write access" is defined in the list for external variables [EXTV] via the element "var[...].synchronization".
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Distribute the synchronous read/write access on the V.E.-variables on several NC-blocks. Hint: The non-synchronous read/write access on V.E.-variables per NC block is unlimited!
	Parameter	%1:	Limit value [-]
			Maximum number of synchronized V.E.-variables per NC block.
	Error type	1, Error message from NC-program.

20088	External variable is not of format SGN32.
	Description	During start-up it is detected, that the data type of one of the external variables is unknown. The data type is defined in the list for external variables [EXTV] via the element "var[...].type".
	Reaction	Class		2	Start-up of the control is continued. The external variables which were read in after the invalid data type are not stored inside the control, so they are not available after start-up.
	Solution	Class		3	Change the invalid data type in the list of external variables [EXTV] and repeat start-up.
	Parameter	%1:	Actual value [-]
			Index of the external variable with invalid data type
	Error type	-

20092	Variable access on an unknown axis.
	Description	The attempt to access on axis specific variables (V.A.) of in NC channel non-existing axes causes this error message. Occurs especially after returning an axis to axis management. Example: Wrong: N10 G00 X0 Y0 Z0 N20 #PUT AX[X] N30 P1=V.A.PROG.X (Error: No more X-axis in channel) N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=V.A.PROG.X N30 #PUT AX[X] N1000 M30 or N10 G00 X0 Y0 Z0 N20 #PUT AX[X] N25 $IF EXIST[V.A.LOG_AX_NR.X] == TRUE N30 P1=V.A.PROG.X N35 $ENDIF N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program sequence. Programming of variable access before release of axis or check at first with the NC command EXIST[V.A.LOG_AX_NR.xx] [PROG] if the axis is still available in NC channel.
	Error type	1, Error message from NC-program.

20095 / 20096
	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.

20097	Read access to variable denied.
	Description	The attempt to read from CNC an external variable which has only access rights for a write access, causes this error. The write/read access rights are defined in the list for external variables [EXTV] via the element "var[...]. access_rights ".
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Change for the corresponding variable the access rights in the list of external variables [EXTV] and repeat start-up.
	Error type	1, Error message from NC-program.

20098
	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.

20100	Write access to variable denied.
	Description	The attempt to write to a variable which is marked as ‚READ_ONLY’ for the CNC causes this error messages. The variable might either be a system-defined one or an external variable (V.E.), which might be declared as ‘READ_ONLY’, ‘WRITE_ONLY’ and ‘READ_WRITE’ in the definition list [EXTV]. Example 1: %example1 N10 G00 X0 Y0 Z0 N20 V.A.MENT.X=100 N1000 M30 Example 2: %example2 N10 G00 X0 Y0 Z0 N20 V.A.MODE[4]=0 N1000 M30 Example 3: %example3 N10 G00 X0 Y0 Z0 N20 V.A.MODULO_VALUE[4]=0 N1000 M30 Example 4: (Requires the following variable definition) var[0].name MYREADONLY var[0].index 8 var[0].type SGN32 var[0].scope CHANNEL var[0].synchronization TRUE var[0].access_rights READ_ONLY var[0].array_size 0 var[0].size 4 var[0].create_hmi_interface 0 % example4 N10 G00 X0 Y0 Z0 N20 V.P.DEMO = V.E.MYREADONLY N30 V.E.MYREADONLY = 4711 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Change for the corresponding variable the access rights in the list of external variables [EXTV] and repeat start-up, if this error occurs for an external variable. For all other variable types only, a read access may be programmed.
	Error type	1, Error message from NC-program.

20101	Too many variables programmed in NC-block for report of changes.
	Description	This error-message is switched off.
	Reaction	Class		1	Warning
	Solution	Class		1	For your attention
	Parameter	%1:	Actual value [-]

		%2:	Limit value [-]

	Error type	1, Error message from NC-program.

20103	Too many parameters programmed in NC-block for report of changes.
	Description	This error-message is switched off.
	Reaction	Class		1	Warning
	Solution	Class		1	For your attention.
	Parameter	%1:	Actual value [-]

	Error type	1, Error message from NC-program.

20104
	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.

20105	Double-programmed block number N.
	Description	In the same NC block more than one block number with the N word was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 X10 N30 N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Remove the unnecessary NC block number.
	Error type	1, Error message from NC-program.

20106	NC-block number exceeds range of data format.
	Description	The block number programmed with the N word exceeds the permissible data range.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Program a permissible value for the invalid block number.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20107	G-code number exceeds range of data format.
	Description	The value programmed with the G word exceeds the permissible data range. Note: The current maximum G-function defined in the ISG kernel of cause is within the permissible data range. If an undefined G-function is programmed, then error message 20131: Unknown G-code is issued.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Program a permissible value for the invalid G function number.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20108	Double-programmed block mode.
	Description	In the same NC block, more than one G-function from the group of moving conditions (G00, G01, G02, G03 etc.) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G01 X10 G00 Y20 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20109	Double-programmed prescription of feed rate.
	Description	In the same NC block, more than one G-function from the group of acceleration conditions (G08/G193/G293) was programmed. Example: Wrong: N10 G01 X500 F1000 N20 G193 X900 F400 G293 N30 X1000 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20110	Double-programmed adaptation of the feed rate.
	Description	In the same NC block, more than one G-function from the group of feed adaptations (G10/G11/G92 R) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 G42 N20 G01 G11 X100 G10 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20111	Double-programmed plane.
	Description	In the same NC block, more than one G-function from the group of plane selection (G17/G18/G19) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G18 Y20 Z4 G19 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20112	Double-programmed mirror function.
	Description	In the same NC block, more than one G-function from the group of mirroring (G20/G21/G22/G23/G351) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G20 X10 Y20 G21 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20113	Double-programmed TRC transition block mode.
	Description	In the same NC block, more than one G-function from the group of TRC transition modes (G25/G26) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 G42 N20 G25 G25 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20114	Double-programmed TRC selection.
	Description	In the same NC block, more than one G-function from the group of TRC selection modes (G40/G41/G42/G43/G44) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G41 X10 Y20 G42 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20115	Double-programmed diameter selection.
	Description	In the same NC block, more than one G-function from the group of diameter programming (G51/G52) was programmed. Example: Wrong: N10 G90 G01 F1000 N20 G51 X80 G51 : M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20116	Double-programmed zero-point offsets.
	Description	In the same NC block, more than one G-function from the group of zero-point offsets (G53-G59/G159) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G53 X10 Y10 G54 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20117	Double-programmed block transition.
	Description	In the same NC block, more than one G-function from the group of block transitions (G60/G359/G360/G61/G260/G261) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G360 X100 G60 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20118	Double-programmed unit declarations.
	Description	In the same NC block, more than one G-function from the group of units (G70/G71) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G70 X100 G71 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20119	Double-programmed working cycles.
	Description	Error message is not in use.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20120	Double-programmed dimension declarations.
	Description	In the same NC block, more than one G-function from the group of dimensioning (G90/G91) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G90 X100 G91 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20121	Double-programmed feed rate declarations.
	Description	In the same NC block, more than one G-function from the group of feed definitions (G93/G94/G95) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G93 F500 X100 G94 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20122	Double-programmed spindle speed definitions.
	Description	In the same NC block, more than one G-function from the group of spindle speed definitions (G96/G97/G196) was programmed. Example: Wrong: N10 M03 S1000 G01 F1000 X100 N20 G96 S63 G97 : M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20123	Double-programmed measuring functions.
	Description	In the same NC block, more than one G-function from the group of measuring functions (G100-G108) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G100 X100 G102 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20124	Double-programmed path preparation commands.
	Description	In the same NC block, more than one G-function from the group of path preparation commands (G115/G116/G117) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G115=2 G116 X1 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20125	Double-programmed precontrol function.
	Description	In the same NC block, more than one G-function from the group of precontrol functions (G135/G137) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G135 X100 G137 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20126	Double-programmed TRC selection mode.
	Description	In the same NC block, more than one G-function from the group of TRC selection commands (G138/G139/G237) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G138 G41 G139 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20127	Double-programmed center point selection.
	Description	In the same NC block, more than one G-function from the group of center point selection commands (G161/G162) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G02 G162 I10 X20 G162 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20128	Double-programmed center point correction.
	Description	In the same NC block, more than one G-function from the group of center point correction commands (G164/G165) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G165 G02 I10 X20.05 G164 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20129	Double-programmed manual mode selection/deselection.
	Description	In the same NC block, more than one G-function from the group of manual mode selection commands (G200/G201/G202) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G201 #ACHSE[X] G200 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20130	Double-programmed chamfer/phase selection.
	Description	In the same NC block, more than one G-function from the group of chamfers and rounding commands (G301/G302) was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G01 X20 F1000 N30 G301 I10 G302 N40 Y50 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the inadmissible G function.
	Parameter	%1:	Incorrect value [-]
			Number of the inadmissible programmed G function
	Error type	1, Error message from NC-program.

20131	Unknown G-function.
	Description	A non-existing G function was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G88 X100 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the unknown G function.
	Parameter	%1:	Incorrect value [-]
			Number of the unknown programmed G function
	Error type	1, Error message from NC-program.

20133	Plane selection not allowed while active TRC.
	Description	If the tool radius compensation is active, it is not allowed to program a plane selection via G17, G18 or G19. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G41 N30 G19 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G41 : N25 G40 N30 G19 N35 G41 : N999 G40 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program sequence. Deselect the TRC with G40 before programming of plane selection.
	Parameter	%1:	Incorrect value [-]
			Invalid G function
	Error type	1, Error message from NC-program.

20136	Selection of TRC not possible with gaping main axis.
	Description	The tool radius compensation needs the first 2 main axis of the current plane. TRC is not possible, if one of these main axes is not available in the NC channel. Example: Wrong: N10 G00 X0 Y0 Z0 N20 #PUT AX[X] N30 G41 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Ensure that both main axes of the current plane are available in the NC channel if the TRC is selected.
	Error type	1, Error message from NC-program.

20137	G74 not allowed while active synchronous operation.
	Description	It is not possible to execute homing (G74), while an axis coupling group is active. Also axes not involved in the current couplings may not be referenced. Example: Wrong: N10 G00 X0 Y0 Z0 N30 #SET AX LINK[1, B=Y] N40 #ENABLE AX LINK[1] N50 G74 X1 N1000 M30 Correct:: (temporarily deactivate coupling): N10 G00 X0 Y0 Z0 N30 #SET AX LINK[1, B=Y] N40 #ENABLE AX LINK[1] : N45 #DISABLE AX LINK[1] N50 G74 X1 N55 #ENABLE AX LINK[1] : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program sequence. Deselect all active coupling groups before homing.
	Parameter	%1:	Incorrect value [-]
			Invalid G function
	Error type	1, Error message from NC-program.

20138	G100 is not allowed with actual measuring type.
	Description	The measurement via G100 cannot be executed because the current valid measuring type is not permissible for a G100 movement.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Ensure, that the correct measuring type is entered in the channel parameter list P-CHAN-00057 or in the NC program before programming of G100 switch to the permissible measuring type with the NC command #MEAS MODE[…] [PROG].
	Error type	1, Error message from NC-program.

20147	After this G-function a '=' is expected.
	Description	The called G-function expects an argument, assigned by “=”. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G115 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G115=14 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Complete the missing assignment.
	Parameter	%1:	Actual value [-]
			Number of the G function
	Error type	1, Error message from NC-program.

20149	Value following G159 exceeds range of permissible values.
	Description	The number programmed with G159=<expr> is an index in the table of the zero-point offsets. The size of that table depends on the individual application. Here the programmed index exceeds the maximum permissible index. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G159=500 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G159=7 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programming of an index, which is available in the table of the zero point offsets P-ZERO-00003, [ZERO].
	Parameter	%1:	Incorrect value [-]

		%2:	Limit value [-]

	Error type	1, Error message from NC-program.

20151	Unknown path preparation mode at G115.
	Description	The Look-Ahead mode given via G115=<value> is out of the acceptable range of integers between 0 and 14 [PROG]. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G115=20 N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G115=14 N1000 M30
	Reaction	Class		1	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programming of correct path preparation mode.
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20154	Value following M exceeds range of data format.
	Description	The programmed number of the M function exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 M150000 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed number of M function must be inside the permissible data range. Ensure, that the M function is defined in the channel parameters P-CHAN-00041.
	Parameter	%1:	Incorrect value [-]

		%2:	Limit value [-]

		%3:	Limit value [-]

	Error type	1, Error message from NC-program.

20155	Double-programmed M-function for spindles.
	Description	In the NC block a spindle M function (M3/M4/M5/M19) is programmed several times in spindle specific syntax. Example: Wrong: N10 G00 X0 Y0 Z0 N20 X10 S[M3 S1000 M4] : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify the programming of M functions within the current NC block. Remove surplus spindle specific M function.
	Parameter	%1:	Incorrect value [-]
			Number of the multiple programmed spindle M function
	Error type	1, Error message from NC-program.

20156	Two M-functions with synchronization mode MNE_SNS programmed.
	Description	It is not allowed to program two M-function with the synchronization mode MNE_SNS [CHAN], [FCT-C1]. in the same NC block.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Distribute the M-function on two NC-blocks.
	Parameter	%1:	Actual value [-]
			Number of the second M function with synchronization mode MNE_SNS.
	Error type	1, Error message from NC-program.

20157	Unknown M-function, since not defined in the channel parameters.
	Description	In the NC channel the programmed M-function is unknown, since in the channel parameter list P-CHAN-00041 it is not defined.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Define the M-function in the channel parameter list P-CHAN-00041.
	Parameter	%1:	Incorrect value [-]
			Number of the unknown M function
	Error type	1, Error message from NC-program.

20158	Double-programmed M02/M30 or M17/M29.
	Description	Within the same NC block, the subroutine-terminating M functions M2, M17, M29 or M30 are programmed several times. Note: Dependent on the sequence of programming of M2, M17, M29 M30 in this context, the error message 20376 "Unexpected M17 or M29" might occur. Example: Wrong: %L UP1 N10 X10 Y10 Z10 N20 M17 M30 %MAIN_PRG N10 G00 X0 Y0 Z0 N20 LL UP1 N30 M30 Correct: %L UP1 N10 X10 Y10 Z10 N20 M17 %MAIN_PRG N10 G00 X0 Y0 Z0 N20 LL UP1 N30 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove surplus M function.
	Parameter	%1:	Actual value [-]
			Number of the multiple programmed M function
	Error type	1, Error message from NC-program.

20160	Unknown internal M-function.
	Description	Because of the number the programmed M function exceeds the permissible range of self-defined M functions ( P-CHAN-00041) and so first it is used as an internal M function (like M30). But during the further check it is also not detected as an internal M function and the current error message is output. M-Funktion nicht bekannt ist, wird der vorliegende Fehler ausgegeben. Hint: Internal M functions are M00, M01, M02, M10, M11, M17, M29, M30 Example: Wrong: N10 G00 X0 Y0 Z0 N20 M1001 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Ensure, that the M function is defined in the channel parameters P-CHAN-00041 and that the number of the M function is inside the permissible data range. Now numbers higher than 1000 are not allowed.
	Parameter	%1:	Incorrect value [-]
			Number of the unknown M function
	Error type	-

20161	Value following H exceeds the range of data format.
	Description	The programmed number of the H function exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 H150000 N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed number of H function must be inside the permissible data range. Ensure, that the H function is defined in the channel parameters P-CHAN-00027.
	Parameter	%1:	Incorrect value [-]

		%2:	Limit value [-]

		%3:	Limit value [-]

	Error type	1, Error message from NC-program.

20162	Unknown H-function, since not defined in the channel parameters.
	Description	In the NC channel the programmed H-function is unknown, since in the channel parameter list P-CHAN-00027 it is not defined, or the H number exceeds a permissible maximum limit.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Define the H-function in the channel parameter list P-CHAN-00027.
	Parameter	%1:	Incorrect value [-]
			Number of the unknown H function
	Error type	1, Error message from NC-program.

20163
	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.

20165	Double-programmed T-function.
	Description	In the same NC block, more than one T word was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 T1 T2 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Remove the inadmissible T word.
	Error type	1, Error message from NC-program.

20166	Value following 'T' exceeds range of data format.
	Description	The programmed number of the T function exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 T2147483648 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed number of T function must be inside the permissible data range.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20167	Unknown T-function.
	Description	The programmed T function addresses a tool place, which is not available in the list of tool parameters [TOOL]. Example: Wrong: N10 G00 X0 Y0 Z0 N20 T999 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed number of T function must address a permissible tool place.
	Parameter	%1:	Incorrect value [-]

		%2:	Limit value [-]

	Error type	1, Error message from NC-program.

20168
	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.

20169	Tool change not allowed while active synchronous operation.
	Description	It is not possible to activate a different set of parameters for the tool geometry correction with the D word or #TOOL DATA[…] while an axis coupling group is active. Example: Wrong: N10 G00 X0 Y0 Z0 N30 #SET AX LINK[1, B=C] N40 #ENABLE AX LINK[1] : N100 D2 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N30 #SET AX LINK[1, B=C] N40 #ENABLE AX LINK[1] : N90 #DISABLE AX LINK[1] N100 D2 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program sequence. Deselect synchronous operation with #DISABLE AX LINK before programming of the D word or #TOOL DATA[…].
	Error type	1, Error message from NC-program.

20170	Double-programmed D-function.
	Description	In the same NC block, more than one D word was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 D1 D2 : N1000 M30 When the channel parameter P-CHAN-00014 is active, than the error occur when the following block occur in NC program: N010 T1 D1 A cause for it is that with activated channel parameter P-CHAN-00014, the programming of "T1" corresponds to the programming of "T1 D1".
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Remove the inadmissible D word. When programming T and D word within a NC block check and modify the channel parameter P-CHAN-00014.
	Error type	1, Error message from NC-program.

20171	Value following 'D' exceeds range of data format.
	Description	The programmed number of the D function exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 D232** : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed number of D function must be inside the permissible data range.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20172	Unknown D-function.
	Description	The programmed D function addresses a tool compensation record, which is not available in the list of tool parameters [TOOL]. Example: Wrong: N10 G00 X0 Y0 Z0 N20 D999 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed number of D function must address a permissible tool compensation record .
	Parameter	%1:	Incorrect value [-]

		%2:	Limit value [-]

	Error type	1, Error message from NC-program.

20175	Double-programmed F-word.
	Description	In the same NC block, more than one F word was programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 F100 G01 X100 F200 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Remove the inadmissible F word
	Error type	1, Error message from NC-program.

20176	Feed rate 'F' is not allowed to be negative or 0.
	Description	The feed rate programmed with the F word is negative or zero. Example: Wrong: N10 G00 X0 Y0 Z0 N20 F[-1000] G01 X100 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 F1000 G01 X100 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Program the feed rate (F word) with a useful value greater than zero.
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20177	Programming of feed rate 'E' not allowed.
	Description	Programming feed rates via E-words is not implemented and therefore generally not allowed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G01 X100 E2000 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G01 X100 F2000 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Replace the E word by the F word.
	Error type	1, Error message from NC-program.

20180	Unknown spindle name or equal sign is missing.
	Description	Either the spindle name programmed in NC block is unknown in NC channel ( P-CHAN-00007, P-CHAN-00053) or at a spindle name with more than one character before the speed value the equal sign is missing. Example (Assumption: Spindle name is „SPINDLE“): Wrong: N10 G00 X0 Y0 Z0 N20 SPDL=1000 M03 : N1000 M30 or N10 G00 X0 Y0 Z0 N20 SPINDLE1000 M03 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 SPINDLE=1000 M03 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Correct the spindle name in accordance with the configured name P-CHAN-00007 . Hint: In NC program for the main spindle only the main spindle name P-CHAN-00053 may be used.
	Error type	1, Error message from NC-program.

20181	Double-programmed spindle.
	Description	In NC block the same spindle was programmed several times in DIN syntax. Example: Wrong: N10 G00 X0 Y0 Z0 N20 S1000 M03 X100 G01 F2000 S1500 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Remove the inadmissible spindle programming.
	Error type	1, Error message from NC-program.

20182	No assignment after name of parameter.
	Description	There was a parameter declaration programmed, but the assignment of a value is missing. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P2 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P2=47.11 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Complete the parameter declaration.
	Error type	1, Error message from NC-program.

20183	Parameter index exceeds range of data format or permissible values.
	Description	The programmed parameter index exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P0=10 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=10 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed parameter index must be inside the permissible data range.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20186	Syntax error within #SET IPO SOLLLPOS[...].
	Description	With the NC command #SET IPO SOLLPOS after the opening square bracket the syntax (commas, equal signs, closing square brackets) is not correct. Syntax example: Wrong: #SET IPO SOLLPOS [P1=X P2=Y] or #SET IPO SOLLPOS [V.L.POS1 X ] or #SET IPO SOLLPOS [P1=X, P2=Y, P3=Z Correct: #SET IPO SOLLPOS [P1=X , P2=Y]or #SET IPO SOLLPOS [V.L.POS1 = X ] or #SET IPO SOLLPOS [P1=X, P2=Y, P3=Z ]
	Reaction	Class	3	Abort of the NC program processing.
	Solution	Class	3	In the NC program check and modify the syntax of #SET IPO SOLLPOS for wrong or missing commas, equal signs and closing square bracket.
	Error type	1, Error message from NC-program.

20187	Radius index exceeds range of data format.
	Description	The value used as index for radius programming is outside the permissible data range. Note: For indexed radius programming, the only allowed index is 1, otherwise error message 20188 “Illegal radius index”. Example: Wrong: N10 G00 X0 Y0 Z0 N20 R-1=10 N50 G02 F1000 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 R1=10 N50 G02 F1000 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed radius index must be inside the permissible data range.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20188	Illegal radius index.
	Description	For indexed radius programming, the only allowed index is 1, all other values cause either this error message 20188 or 20187 “Radius index exceeds range of permissible numbers”. Example: Wrong: N10 G00 X0 Y0 Z0 N20 R2=10 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 R1=10 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Radius index must be programmed with value 1.
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20191	Value following 'O' exceeds range of data format.
	Description	Programming O function is not implemented and therefore generally not allowed.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the O function.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20192	Unknown O-function.
	Description	Programming O function is not implemented and therefore generally not allowed.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the O function.
	Parameter	%1:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20193	Percent sign not allowed within main routine part.
	Description	Within a main routine a percent character (%) is programmed, although the main routine is already in execution. A percent sign is only valid for marking the name of the main program or local sub programs, not inside the main program’s part itself [PROG]. Example: Wrong: %MAIN N10 G00 X0 Y0 Z0 N20 %L SUB1 : N1000 M30 Correct: %L SUB1 : %MAIN N10 G00 X0 Y0 Z0 : N1000 M30 The execution of a main routine is also started, if in the file outside the comments, a character is noticed as the first character that is neither a space character nor a "%". In this case this character is evaluated as the first character of an unnamed program. This also means that in front of the first "%", no block numbers, variable declarations etc. may be programmed.
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program sequence. Remove the invalid percent sign or move the definitions of the local sub programs before the beginning of the main program part. Ensure that no NC block numbers, variable declarations etc. were programmed before the first %-character (e.g. remove block numbers at the beginning of comment lines!).
	Error type	1, Error message from NC-program.

20194	Assignment operation missing or unknown.
	Description	In NC program for a variable (V.A., V.G., V.P., V.L., V.S., V.E.,) an assignment is expected. Either here the programmed assignment operator is unknown or the complete assignment of a value is missing. Example: Wrong: N10 G00 X0 Y0 Z0 N20 V.G.T_AKT : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 V.G.T_AKT =5 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Complete the invalid or missing assignment.
	Error type	1, Error message from NC-program.

20195	Overflow of variable stack.
	Description	The programmed variable operation causes an overflow of an internal system resource, e.g. when using too many indirection operations (nesting levels). Example: Wrong: N10 #VAR N20 V.L.INDEX[10] = [1, 2, 3, 4, 5, 6, 7, 8, 9, 10] N30 V.P.MY_ARRAY[V.L.INDEX[V.L.INDEX[..[..[..[3]]]]]] N40 #ENDVAR N1000 M30 Correct: 10 #VAR N20 V.L.INDEX[10] = [1, 2, 3, 4, 5, 6, 7, 8, 9, 10] N30 V.P.MY_ARRAY[3] N40 #ENDVAR N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Reduce the dimension of the array variable or nesting depth or generally avoid the nesting of array variables.
	Parameter	%1:	Limit value [-]

	Error type	1, Error message from NC-program.

20196	Unknown variable.
	Description	During the linkage of V.G.NP[...].ALL variables on the right side of an assignment an inadmissible operation is programmed. A linkage with axis specific constants or variables is not permitted. Example: Wrong: N10 G00 X0 Y0 Z0 N20 V.G.NP[1].ALL = V.G.NP[2].ALL + 100 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 V.G.NP[1].ALL = V.G.NP[2].ALL N30 V.G.NP[1].V.X += 100 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Use correctly the rules for linkage of .ALL variables [PROG - Chapter Adding/Subtracting offsets].
	Error type	1, Error message from NC-program.

20197	Index of variable exceeds range of data format.
	Description	The programmed index of a variable exceeds the permissible data range. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=V.G.WZ[-1].L : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=V.G.WZ[65].L : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Programmed variable index must be inside the permissible data range.
	Parameter	%1:	Incorrect value [-]

		%2:	Lower limit value [-]

		%3:	Upper limit value [-]

	Error type	1, Error message from NC-program.

20198	Missing ']' after variable.
	Description	Within a variable expression with index, the closing square bracket „]“ is missing. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=V.G.WZ[V.G.WZ[1].L : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=V.G.WZ[V.G.WZ[1].L] : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Complete the variable expression for the missing closing square bracket „]“.
	Error type	1, Error message from NC-program.

20200	NC-command or name of axis expected.
	Description	In NC block an axis is programmed, which is not known in NC channel. The programmed axis name can not be assigned to an axis. This for example applies for: slave axes of gantry or axes links axis, which temporarily are not available in NC channel because of axes exchange commands axes respectively axes names, which are not configured in NC channel axes names, which do not start with the allowed axes letters X, Y, Z, A, B, C, U, V, W or Q. Example: Wrong: N10 G00 X0 Y0 Z0 N20 #SET AX LINK [1, W=X] N30 #ENABLE AX LINK [1] N40 X10 W20 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 #SET AX LINK [1, W=X] N30 #ENABLE AX LINK [1] N40 X10 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Only use axes names, which are available in NC channel.
	Error type	1, Error message from NC-program.

20203	Double-programmed axis.
	Description	In the same NC block, an axis was programmed several times. Example: Wrong: N10 G00 X0 Y0 Z0 N20 X10 Y20 X10 : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Remove the redundant axis programming.
	Parameter	%1:	Logical axis number [-]

	Error type	1, Error message from NC-program.

20205	Double-programmed center point coordinate.
	Description	In the same NC block, a center point coordinate was programmed several times. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G02 I10 I20 J30 F2000 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Remove the redundant center point coordinate .
	Error type	1, Error message from NC-program.

20206	$-command must be programmed exclusively in NC-block.
	Description	A control block sequence, starting with the dollar character $ , is programmed with other NC commands in the same NC block. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $FOR P10=0, 20, 1 G01 X10 F100 N30 G91 X5 N40 $ENDFOR : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N15 G01 X10 F100 N20 $FOR P10=0, 20, 1 N30 G91 X5 N40 $ENDFOR : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Programming of the control block sequence and the other NC commands in separate NC blocks.
	Error type	1, Error message from NC-program.

20207	#-command must be programmed exclusively in NC-block.
	Description	A string command, starting with the hash character # , is programmed with other NC commands in the same NC block. Example: Wrong: N10 G00 X0 Y0 Z0 N20 G01 X10 F100 #TIME 8.15 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 G01 X10 F100 N30 #TIME 8.15 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Programming of the string command and the other NC commands in separate NC blocks. Hint: Some special string commands also may be programmed in combination with other NC commands in the same NC block [PROG].
	Error type	1, Error message from NC-program.

20208	End of text is reached before M02/M30.
	Description	AT the end of the main program no M02/M30 is programmed. Example: Wrong: N10 G00 X0 Y0 Z0 : N1000 Correct: N10 G00 X0 Y0 Z0 : N1000 M30
	Reaction	Class	-	Abort of the NC program processing.
	Solution	Class	-	Check and modify NC program. Complete the missing M02/M30.
	Error type	-

20209	Unknown NC-command.
	Description	A complete string command or a part of it can not be identified. Example: Wrong: N10 G00 X0 Y0 Z0 N20 #UNKNOWN : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Programming of the string command in correct syntax.
	Error type	1, Error message from NC-program.

20210
	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.

20211	Control block depth not sufficient; Control block nesting too big.
	Description	In NC program too many control block commands are nested. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=1 N30 $IF N40 $IF... Nxx $IF... : etc. Nxx $ENDIF Nxx $ENDIF Nxx $ENDIF : N1000 M30
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Reduce nesting depth of control block structures, possibly modify structure of control block sequences.
	Parameter	%1:	Limit value [-]
			Maximum nesting depth
	Error type	1, Error message from NC-program.

20212	After 'IF' only the condition is permissible.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $IF command only the necessary condition may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 P1=0 N20 $IF P1==1X100 G01 F1000 N30 Y200 N40 $ENDIF : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=0 N20 $IF P1==1 N25 X100 G01 F1000 N30 Y200 N40 $ENDIF : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands to other NC blocks or delete them. Exception: It is allowed to combine a $IF command with a $GOTO in the same NC block. In this case no assigned $ENDIF is necessary [PROG - Chapter the $GOTO statement].
	Error type	1, Error message from NC-program.

20213
	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.

20214	Unexpected 'ELSE'; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $ELSE can only be programmed in combination with $IF/$ENDIF. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $ELSE : N1000 M30 Correct: N01 P1=0 N05 $IF P1==1 N10 G00 X0 Y0 Z0 N20 $ELSE N25 G01 X100 Y0 Z0 F1000 N30 $ENDIF : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $IF/$ENDIF command or remove the $ELSE command.
	Error type	1, Error message from NC-program.

20215	'ELSE' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $ELSE no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 P1=0 N20 $IF P1 N30 G01 X100 F100 N40 $ELSE G01 X200 F500 N50 $ENDIF : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=0 N20 $IF P1 N30 G01 X100 F100 N40 $ELSE N45 G01 X200 F500 N50 $ENDIF : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $ELSE to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20216	Unexpected 'ELSE IF'; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $ELSE can only be programmed in combination with $IF/$ENDIF. Example: False: N10 G00 X0 Y0 Z0 N20 $ELSEIF : N1000 M30 Correct: N01 P1=0 N05 $IF P1==1 N10 G00 X0 Y0 Z0 N20 $ELSEIF P1==2 N30 G00 X100 Y0 Z0 N40 $ENDIF : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $IF/$ENDIF command or remove the $ELSEIF command.
	Error type	1, Error message from NC-program.

20217	After 'ELSEIF' only the condition is permissible.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $ELSEIF command only the necessary condition may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N251 P2=0 N252 $IF P2 : N253 $ELSEIF P2==100 G01 X200 F500 : N254 $ENDIF : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N251 P2=0 N252 $IF P2 : N253 $ELSEIF P2==100 N254 G01 X200 F500 : N254 $ENDIF : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20218	Unexpected 'ENDIF; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $ENDIF can only be programmed in combination with a previous $IF. Example: Wrong : N10 G00 X0 Y0 Z0 P1=0 N20 G01 X100 F10000 N30 $ENDIF : N1000 M30 Correct N10 G00 X0 Y0 Z0 P1=0 N15 $IF P1==0 N20 G01 X100 F10000 N30 $ENDIF : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $IF command or remove the $ENDIF command.
	Error type	1, Error message from NC-program.

20219	'ENDIF' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $ENDIF no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 P1=0 N20 $IF P1 N30 $ENDIF G01 X100 F10000 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=0 N20 $IF P1 N30 $ENDIF N40 G01 X100 F10000 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $ENDIF to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20220	After 'SWITCH' only the condition is permissible.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $SWITCH command only the necessary condition may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=5 N50 $SWITCH P1 G01 X100 F10000 : N65 $ENDSWITCH : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=5 N25 G01 X100 F10000 N50 $SWITCH P1 : N65 $ENDSWITCH : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20221	Unexpected 'CASE'; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $CASE can only be programmed in combination with $SWITCH/$ENDSWITCH. Example: Wrong: N10 G00 X0 Y0 Z0 P1=47 N20 $CASE P1 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=47 N20 $SWITCH P1 N20 $CASE 1 : N30 $ENDSWITCH : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $SWITCH/ $ENDSWITCH command or remove the $CASE command.
	Error type	1, Error message from NC-program.

20222	After 'CASE' only the condition is permissible.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $CASE command only the necessary condition may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=5 N30 $SWITCH P1 N40 $CASE 5 G01 X100 F100 N50 $BREAK : N90 $ENDSWITCH : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=5 N30 $SWITCH P1 N40 $CASE 5 N45 G01 X100 F100 N50 $BREAK : N90 $ENDSWITCH : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20223	Unexpected 'DEFAULT'; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $DEFAULT can only be programmed in combination with $SWITCH/$ENDSWITCH. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $DEFAULT : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=0 N15 $SWITCH P1 : N20 $CASE : N30 $DEFAULT : N40 $ENDSWITCH : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $SWITCH/ $ENDSWITCH command or remove the $DEFAULT command.
	Error type	1, Error message from NC-program.

20224	'DEFAULT' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $DEFAULT no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=5 N50 $SWITCH P1 : N62 $DEFAULTG01 X100 F10000 : N65 $ENDSWITCH : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=5 N50 $SWITCH P1 : N62 $DEFAULT N63 G01 X100 F10000 : N65 $ENDSWITCH : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $DEFAULT to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20225	Unexpected 'ENDSWITCH'; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $ENDSWITCH can only be programmed in combination with a previous $SWITCH. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=5 N30 $ENDSWITCH : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=5 N30 $SWITCH P1 : N40 $ENDSWITCH : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $SWITCH command or remove the $ENDSWITCH command.
	Error type	1, Error message from NC-program.

20226	'ENDSWITCH' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $ENDSWITCH no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=5 N50 $SWITCH P1 : N62 $DEFAULT : N65 $ENDSWITCH G01 X100 F10000 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=5 N50 $SWITCH P1 : N62 $DEFAULT : N65 $ENDSWITCH N66 G01 X100 F10000 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $ENDSWITCH to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20227	Wrong counting variable after 'FOR'; name has to be P, V or R.
	Description	The counting variable in a FOR loop was programmed in an invalid syntax. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $FOR COUNT=1,10,1 N30 $ENDFOR : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 $FOR V.P.COUNT=1,10,1 N30 $ENDFOR : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. The counting variable in a FOR loop needs a permissible variable name: · Any parameter: starts with character ‘P’ (or ‘R’, if allowed) · Any user defined variable: starts with ‘V.P’, ‘V.L’, ‘V.S’ · Pre-defined or system-defined variables: start with ‘V.A’, ‘V.G’, ‘V.E’ (Caution: not all variables allow write access!!!)
	Error type	1, Error message from NC-program.

20228	FOR loop: After counting variable an equal sign '=' is expected.
	Description	During the initialization of the FOR loop the starting value of the counting variable has to be assigned directly. Example: Wrong: N10 G00 X0 Y0 Z0 N20 V.P.EIGENDEF = 0 N30 $FOR V.P.EIGENDEF,100,10 : N150 $ENDFOR : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N30 $FOR V.P.EIGENDEF = 0,100,10 : N150 $ENDFOR : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Correct initialization of t he counting variable in the FOR loop.
	Error type	1, Error message from NC-program.

20229	FOR loop: During initialization of counting variable a comma ',' is expected.
	Description	Start value, increment and end value of a $FOR loop need to be separated by ”,“. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $FOR P1 = 1 10,1 : N150 $ENDFOR : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 $FOR P1 = 1, 10,1 : N150 $ENDFOR : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Complete the missing comma in the initialization of t he FOR loop.
	Error type	1, Error message from NC-program.

20230	After 'FOR' only the condition is permissible.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $FOR command only the necessary loop condition may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $FOR P2=1,10,1 G01 X100 F1000 : N30 $ENDFOR : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 $FOR P2=1,10,1 N25 G01 X100 F1000 : N30 $ENDFOR : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20231	Cache overflow, 'FOR' condition consists of too many characters.
	Description	The string length of the loop condition exceeds the permissible limit.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Reduce the string length of the loop condition.
	Parameter	%1:	Limit value [-]

		%2:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20232	Unexpected 'ENDFOR'; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $ENDFOR can only be programmed in combination with a previous $FOR. Example: Wrong: N10 G00 X0 Y0 Z0 P1=1 N20 $ENDFOR : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=1 N15 $FOR P1=100, 200, 300 : N20 $ENDFOR : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $FOR command or remove the $ENDFOR command.
	Error type	1, Error message from NC-program.

20233	'ENDFOR' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $ENDFOR no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $FOR P1=1, 10, 2 : N30 $ENDFOR G01 X100 F10000 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 $FOR P1=1, 10, 2 : N30 $ENDFOR N40 G01 X100 F10000 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $ENDFOR to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20234	Continuation of parameter syntax is wrong.
	Description	The counting variable in a FOR loop was programmed in an invalid syntax. Only P,V or R are allowed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $FOR COUNT=1,10,1 N30 $ENDFOR : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 $FOR V.P.COUNT=1,10,1 N30 $ENDFOR : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. The counting variable in a FOR loop needs a permissible variable name: · Any parameter: starts with character ‘P’ (or ‘R’, if allowed) · Any user defined variable: starts with ‘V.P’, ‘V.L’, ‘V.S’ · Pre-defined or system-defined variables: start with ‘V.A’, ‘V.G’, ‘V.E’ (Caution: not all variables allow write access!!!)
	Error type	1, Error message from NC-program.

20235	After 'WHILE' only the condition is permissible.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $WHILE command only the necessary condition may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=1 N30 $WHILE P1>0G01 X100 F1000 : N40 $ENDWHILE : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=1 N30 $WHILE P1>0 N35 G01 X100 F1000 N40 $ENDWHILE : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20236	Cache overflow, 'WHILE' condition consists of too many characters.
	Description	The string length of the loop condition exceeds the permissible limit.
	Reaction	Class		2	Abort of the NC program processing.
	Solution	Class		3	Check and modify NC program. Reduce the string length of the loop condition.
	Parameter	%1:	Limit value [-]

		%2:	Incorrect value [-]

	Error type	1, Error message from NC-program.

20237	Unexpected 'ENDWHILE'; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $ENDWHILE can only be programmed in combination with a previous $WHILE. Example: Wrong: N10 G00 X0 Y0 Z0 P1=1 N20 $ENDWHILE : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=1 N15 $WHILE P1>0 : N20 $ENDWHILE : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $WHILE command or remove the $ENDWHILE command.
	Error type	1, Error message from NC-program.

20238	'ENDWHILE' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $ENDWHILE no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=1 N30 $WHILE P1 : N40 $ENDWHILE G01 X200 F500 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=1 N30 $WHILE P1 : N40 $ENDWHILE N50 G01 X200 F500 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $ENDWHILE to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20239	'DO' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $DO no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 P1=0 N20 $DO P1=P1+1 : N50 $ENDDO P1<2 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=0 N20 $DO N30 P1 =P1+1 : N50 $ENDDO P1<2 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $DO to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20240	Unexpected 'ENDDO'; it does not match the actual control block.
	Description	A control block statement was programmed in incomplete syntax. A $ENDDO can only be programmed in combination with a previous $DO. Example: Wrong: N10 G00 X0 Y0 Z0 P1=1 N20 $ENDDO P1<2 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=1 N15 $DO : N20 $ENDDO P1<2 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a $DO command or remove the $ENDDO command.
	Error type	1, Error message from NC-program.

20241	After 'ENDDO' only the condition is permissible.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $ENDDO command only the necessary condition may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P2=10 N30 $DO : N40 $ENDDO P2 >= 10G01 X100 F1000 : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P2=10 N30 $DO : N40 $ENDDO P2 >= 10 N45 G01 X100 F1000 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20242	'BREAK' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $BREAK no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 P1=5 N30 $SWITCH P1 N60 $CASE 5 N70 G01 X100 F10000 N80 $BREAK G01 Y200 F10000 N90 $DEFAULT N100 P1=0 N110 $BREAK N120 $ENDSWITCH : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 P1=5 N30 $SWITCH P1 N60 $CASE 5 N70 G01 X100 F10000 N75 G01 Y200 F10000 N80 $BREAK N90 $DEFAULT N100 P1=0 N110 $BREAK N120 $ENDSWITCH : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $BREAK to other NC blocks or delete them.
	Error type	1, Error message from NC-program.

20243	Unexpected 'BREAK'; no valid/open control blocks.
	Description	A control block statement was programmed in incomplete syntax. A $BREAK can only be programmed inside any loop or $SWITCH construct. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $BREAK : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=1 N20 $SWITCH P1 N30 $CASE 2 N35 G01 X100 F10000 N40 $BREAK : N100 $ENDSWITCH : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a loop or $SWITCH construct or remove the $BREAK command.
	Error type	1, Error message from NC-program.

20244	Unexpected 'CONTINUE'; no valid/open control blocks.
	Description	A control block statement was programmed in incomplete syntax. A $CONTINUE can only be programmed inside any loop or $SWITCH construct. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $CONTINUE : N1000 M30 Correct: N10 G00 X0 Y0 Z0 P1=1 N20 $DO N30 P1=P1+1 N40 $IF P1 == 2 N50 $CONTINUE N60 $ENDIF : N100 $ENDDO P1 < 10 : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify the NC program sequence. Insert a loop or $SWITCH construct or remove the $CONTINUE command.
	Error type	1, Error message from NC-program.

20245	'CONTINUE' must be programmed exclusively in NC-block.
	Description	In the same NC block a control block command was programmed together with other NC commands. After a $CONTINUE no further NC commands may be programmed. Example: Wrong: N10 G00 X0 Y0 Z0 N20 $FOR P1=1, 10, 2 N30 $IF P1 == 8 N40 $CONTINUE G01 X100 F10000 N50 $ENDIF : N100 $ENDFOR : N1000 M30 Correct: N10 G00 X0 Y0 Z0 N20 $FOR P1=1, 10, 2 N30 $IF P1 == 8 N35 G01 X100 F10000 N40 $CONTINUE N50 $ENDIF : N100 $ENDFOR : N1000 M30
	Reaction	Class	2	Abort of the NC program processing.
	Solution	Class	3	Check and modify NC program. Move the not permissible NC commands after $CONTINUE to other NC blocks or delete them.
	Error type	1, Error message from NC-program.