ID-range 20000-20249

20002

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 informations 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 informations 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 negativ coordinates

%3:

Upper limit value [0.1 µm or 0,0001°]

Limit value for positiv coordinates.

%4:

Incorrect value [0.1 µm bzw. 0,0001°]

Programmed coordinate or calculated value in internal unit

%5:

Incorrect value [0.1 µm bzw. 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. Programme 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. Programme 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 weigthing programmed.

Description

The ramptime weigthing 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. Programme ramp time weigthing 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 weigthing programmed.

Description

The precontrol weigthing 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. Programme precontrol weigthing 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:

( Aktuelle Position : 0)

N10 G63 C0 F100 S100

Correct:

( Aktuelle 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 intersect 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 centre could lay on a full circle with radius R around the start / end point. Therefore it is necessary to program full circles via the centre 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 centre point definition.

Error type

1, Error message from NC-program.

20035

Difference between programmed and calculated centre point too big.

Description

During active centre point correction (G165) based on the programmed centre point coordinates I, J, K a centre point is calculated. If this calculated centre point differs too much from the programmed centre 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 centre point coordinates. Check the dimension (absolut/ relativ) of centre point programming (G161/G162). Possibly complete missing centre 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 centre point correction (G164 the centre 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 centre 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 centre 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 centre 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 paralell 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 as a result 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

As long as 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 has to 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 informations.

Error type

1, Error message from NC-program.

20054

Corrected centre point exceeds range of data format.

Description

The values chosen for start / end point and radius imply centre 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 corretion 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:

1. Check if the parameter „anzahl_belegt“ contains the correct number of external variables

2. 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[...].synchronisation".

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].synchronisation 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 feedrate.

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 chamfer 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

As long as the tool radius compensation is active, it is not allowed to programme 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 this 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 can not 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 preperation 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 synchronisation mode MNE_SNS programmed.

Description

It is not allowed to program two M-function with the synchronisation 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 synchronisation 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: Dependend 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. At the momet 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 adresses 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 adress 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 D2**32

:

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 adresses 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 adress 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

P rogram 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.