CNC
8055 ·M·
Error solution
Ref.1705
It is possible that CNC can execute more functions than those described in its
associated documentation; however, Fagor Automation does not guarantee the
validity of those applications. Therefore, except under the express permission
from Fagor Automation, any CNC application that is not described in the
documentation must be considered as "impossible". In any case, Fagor
Automation shall not be held responsible for any personal injuries or physical
All rights reserved. No part of this documentation may be transmitted,
transcribed, stored in a backup device or translated into another language
without Fagor Automation’s consent. Unauthorized copying or distributing of this
software is prohibited.
The information described in this manual may be subject to changes due to
technical modifications. Fagor Automation reserves the right to change the
contents of this manual without prior notice.
All the trade marks appearing in the manual belong to the corresponding owners.
The use of these marks by third parties for their own purpose could violate the
rights of the owners.
This product uses the following source code, subject to the terms of the GPL license. The applications busybox V0.60.2;
dosfstools V2.9; linux-ftpd V0.17; ppp V2.4.0; utelnet V0.1.1. The librarygrx V2.4.4. The linux kernel V2.4.4. The linux boot
ppcboot V1.1.3. If you would like to have a CD copy of this source code sent to you, send 10 Euros to Fagor Automation
for shipping and handling.
damage caused or suffered by the CNC if it is used in any way other than as
explained in the related documentation.
The content of this manual and its validity for the product described here has been
verified. Even so, involuntary errors are possible, hence no absolute match is
guaranteed. However, the contents of this document are regularly checked and
updated implementing the necessary corrections in a later edition. We appreciate
your suggestions for improvement.
The examples described in this manual are for learning purposes. Before using
them in industrial applications, they must be properly adapted making sure that
the safety regulations are fully met.
Error solution
INDEX
PROGRAMMING ERRORS ........................................................................5
BLOCK PREPARATION AND EXECUTION ERRORS ............................37
HARDWARE ERRORS .............................................................................61
PLC ERRORS ...........................................................................................69
SERVO ERRORS ......................................................................................71
CAN ERRORS ...........................................................................................85
TABLE DATA ERRORS ............................................................................91
ERRORS OF THE MC WORK MODE .......................................................95
·M· Model
Ref.1705
·3·
PROGRAMMING ERRORS
0001 ‘Empty line’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When trying to enter into a program or execute an empty block or containing the
label (block number).
2. Within the «Irregular pocket canned cycle with islands (G66)», when parameter
"S" (beginning of the profile) is greater than parameter "E" (end of profile).
SOLUTION The solution for each cause is:
1. The CNC cannot enter into the program or execute an empty line. To enter an
empty line in the program, use the «;» symbol at the beginning of that block. The
CNC will ignore the rest of the block.
2. The value of parameter "S" (block where the profile definition begins) must be
lower than the value of parameter "E" (block where the profile definition ends).
0002 ‘Improper data’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When editing an axis coordinate after the cutting conditions (F, S, T or D) or the
"M" functions.
2. When the marks of the block skip (conditional block /1, /2 or /3) are not at the
beginning of the block.
3. When programming a block number greater than 99999999 while programming
in ISO code.
4. When trying to define the coordinates of the machining starting point in the
finishing operation (G68) of the "Irregular pocket canned cycle".
5. While programming in high-level, the value of the RPT instruction exceeds 9999.
SOLUTION The solution for each cause is:
1. Remember the programming order.
2. Remember the programming order.
• Block skip (conditional block /1, /2 or /3).
• Label (N).
• "G" functions.
• Axis coordinates. (X, Y, Z…).
• Machining conditions (F, S, T, D).
• "M" functions.
3. Correct the syntax of the block. Program the labels between 0 and 99999999.
4. No point can be programmed within the definition of the finishing cycle (G68) for
the "Irregular pocket canned cycle". The CNC selects the point where it will start
machining. The programming format is: G68 B...L...Q...I...R...K...V...
And then the cutting conditions.
5. Correct the syntax of the block. Program a number of repetitions between 0 and
9999
Error solution
0003 ‘Improper data order.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The machining conditions or the tool data have been programmed in the wrong order.
SOLUTION Remember that the programming order is:
… F...S...T...D...…
All the data need not be programmed.
·M· Model
Ref.1705
·5·
Error solution
0004 ‘No more information allowed in the block.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When editing a "G" function after an axis coordinate.
2. When trying to edit some data after a "G" function (or after its associated
parameters) which must go alone in the block (or which only admits its own
associated data).
3. When assigning a numeric value to a parameter that does not need it.
SOLUTION The solution for each cause is:
1. Remember the programming order.
• Block skip (conditional block /1, /2 or /3).
• Label (N).
• "G" functions.
• Axis coordinates. (X, Y, Z…).
• Machining conditions (F, S, T, D).
• "M" functions.
2. There are some "G" functions which carry associated data in the block. Maybe,
this type of functions do not let program other type of information after their
associated parameters. On the other hand, neither machining conditions, (F, S),
tool data (T, D) nor "M" functions may be programmed.
3. There are some "G" functions having certain parameters associated to them
which do not need to be defined with values.
0005 ‘Repeated information’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The same data has been entered twice in a block.
SOLUTION Correct the syntax of the block. The same data cannot be defined twice in a block.
0006 ‘Improper data format’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While defining the parameters of a machining canned cycle, a negative value has
been assigned to a parameter which only admits positive values.
SOLUTION Verify the format of the canned cycle. In some canned cycles, there are parameters
which only accept positive values.
0007 ‘Incompatible G functions.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When programming in the same block two "G" functions which are incompatible
with each other.
2. When trying to define a canned cycle in a block containing a nonlinear movement
(G02, G03, G08, G09, G33).
SOLUTION The solution for each cause is:
1. There are groups of "G" functions which cannot go together in the block because
they involve actions incompatible with each other. For example:
G01/G02: Linear and circular interpolation
G41/G42: Left-hand or right-hand tool radius compensation.
This type of functions must be programmed in different blocks.
2. A canned cycle must be defined in a block containing a linear movement. In other
words, to define a cycle, a "G00" or a "G01" must be active. Nonlinear movements
(G02, G03, G08 and G09) may be defined in the blocks following the profile
definition.
·M· Model
Ref.1705
·6·
0008 ‘Nonexistent G function’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A nonexistent "G" function has been programmed.
SOLUTION Check the syntax of the block and verify that a different "G" function is not being edited
by mistake.
Error solution
0009 ‘No more G functions allowed’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A "G" function has been programmed after the machining conditions or after the tool
data.
SOLUTION Remember that the programming order is:
• Block skip (conditional block /1, /2 or /3).
• Label (N).
• "G" functions.
• Axis coordinates. (X, Y, Z…).
• Machining conditions (F, S, T, D).
• "M" functions.
0010 ‘No more M functions allowed’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE More than 7 "M" functions have been programmed in a block.
SOLUTION The CNC does not let program more than 7 "M" functions in a block. To execute any
other functions, write them in a separate block. The "M" functions may go alone in
a block.
0011 ‘This G or M function must be alone.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The block contains either a "G" or an "M" function that must go alone in the block.
SOLUTION Write it alone in the block.
0012 ‘Program F, S, T, D before the M functions.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A machining condition (F, S) or tool data (T, D) has been programmed after the "M"
functions.
SOLUTION Remember that the programming order is:
… F...S...T...D...M...
Up to 7 "M" functions may be programmed .
All the data need not be programmed.
0013 ‘Program G30 D +/-359.9999’
No explanation required.
0014 ‘Do not program labels by parameters.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A label (block number) has been defined with a parameter.
SOLUTION Programming the block number is optional, but it cannot be defined with a parameter
It can only be defined with a number between 0 and 99999999.
0015 ‘Number of repetitions not possible.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A repetition has been programmed wrong or the block does not admit repetitions.
SOLUTION High level instructions do not admit a number of repetitions at the end of the block.
To do a repetition, assign to the block to be repeated a label (block number) and use
the RPT instruction.
0016 'Program: G15 axis.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the function "Longitudinal axis selection (G15)" the parameter for the axis has not
been programmed.
SOLUTION Check the syntax of the block. The definition of the "G15" function requires the name
of the new longitudinal axis.
·M· Model
Ref.1705
·7·
Error solution
0017 'Program: G16 axis-axis.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the function "Main plane selection by two axes (G16)" one of the two parameters
for the axes has not been programmed.
SOLUTION Check the syntax of the block. The definition of the "G16" function requires the name
of the axes defining the new work plane.
0018 'Program: G22 K(1/2/3/4/5) S(0/1/2).’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the function "Enable/Disable work zones (G22)" the type of enable or disable of
the work zone has not been defined or it has been assigned the wrong value.
SOLUTION The parameter for enabling or disabling the work zones "S" must always be
programmed and it may take the following values.
• S=0: The work zone is disabled.
• S=1: It is enabled as a no-entry zone.
• S=2: It is enabled as a no-exit zone.
0019 ‘Program zone K1, K2, K3, K4 or K5.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. A "G20", "G21" or "G22" function has been programmed without defining the work
zone K1, K2, K3, K4 or K5
2. The programmed work zone is smaller than 0 or greater than 5.
SOLUTION The solution for each cause is:
1. The programming format for functions "G20", "G21" and "G22" is:
G20 K...X...C±5.5 Definition of lower work zone limits.
G21 K...X...C±5.5 Definition of upper work zone limits.
G22 K...S... Enable/disable work zones.
Where:
K Is the work zone.
X...C Are the axes where the limits are defined.
S Is the type of work zone enable.
2. The "K" work zone may only have the values of K1, K2, K3, K4 or K5.
·M· Model
Ref.1705
0020 ‘Program G36-G39 with R+5.5.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the "G36" or "G39" function, the "R" parameter has not been programmed or it has
been assigned a negative value.
SOLUTION To define "G36" or "G39", parameter "R" must also be defined and with a positive
value).
G36 R= Rounding radius.
G39 R= Distance between the end of the programmed path and the point to
be chamfered.
0021 'Program: G72 S5.5 or axis (axes).’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When programming a general scaling factor (G72) without the scaling factor to
apply.
2. When programming a particular scaling factor (G72) to several axes, but the axes
have been defined in the wrong order.
SOLUTION Remember that the programming format for this function is:
G72 S5.5" When applying a general scaling factor (to all axes).
G72 X…C5.5" When applying a particular scaling factor to one or several
axes.
·8·
Error solution
0022 'Program: G73 Q (angle) I J (center).'
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the "Pattern rotation (G73)" function have been programmed
wrong. The causes may be:
1. The rotation angle has not been defined.
2. Only one of the rotation center coordinates has been defined.
3. The rotation center coordinates have been defined in the wrong order.
SOLUTION The programming format for this function is:
G73 Q (angle) [I J] (center)
The "Q" value must always be programmed.
The "I", "J" values are optional, but if programmed, both must be programmed.
0023 ‘Block incompatible when defining a profile.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the set of blocks defining a pocket profile, there is a block containing a "G" function
that cannot be part of the profile definition.
SOLUTION The "G" functions available in the profile definition of a pocket (2D/3D) are:
G00: Beginning of the profile.
G01: Linear interpolation.
G02/G03: Clockwise/counterclockwise interpolation.
G06: Circle center in absolute coordinates.
G08: Arc tangent to previous path.
G09: Three point arc.
G36: Automatic radius blend.
G39: Chamfer.
G53: Programming with respect to home.
G70/G71: Inch/metric programming.
G90/G91: Programming in absolute/incremental coordinates.
G93: Polar origin preset.
And also, in the 3D pocket profile:
G16: Main plane selection by two axes.
G17: Main plane X-Y and longitudinal Z.
G18: Main plane Z-X and longitudinal Y.
G19: Main plane Y-Z and longitudinal X.
0024 ‘High level blocks not allowed when defining a profile.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE Within the set of blocks defining a pocket profile, a high level block has been
programmed.
SOLUTION The pocket profile must be defined in ISO code. High level instr uctions are not allowed
(GOTO, MSG, RPT ...).
0025 'Program: G77 axes (2 to 6) or G77 S.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the "axis slaving function (G77)" the parameters for the axes are missing or in
"spindle synchronization (G77S) functions the "S" parameter is missing.
SOLUTION In the "axis slaving" function, program at least two axes and in the "spindle
synchronization" function, always program the "S" parameter.
0026 'Program: G93 I J.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the "Polar origin preset (G93)" function, some of the parameters for the new polar
origin have not been programmed.
SOLUTION Remember that the programming format for this function is:
G93 I...J...
The "I", "J" values are optional, but if programmed, both must be programmed and
they indicate the new polar origin.
·M· Model
Ref.1705
·9·
Error solution
0027 ‘G49 T X Y Z S, X Y Z A B C or X Y Z Q R S.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the "Inclined plane definition (G49)" function, a parameter has been programmed
twice.
SOLUTION Check the syntax of the block. The programming formats are:
T X Y Z S X Y Z A B C X Y Z Q R S
0028 ‘G2 or G3 not allowed when programming a canned cycle.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A canned cycle has been attempted to execute while the "G02", "G03" or "G33"
functions were active.
SOLUTION To execute a canned cycle, "G00" or "G01" must be active. A "G02" or "G03" function
may be programmed previously in the program history. Check that these functions
are not active when the canned cycle is defined.
0029 ‘G60: [A] /X I K/(2) [P Q R S T U V].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the "Multiple machining in a straight line (G60)" have been
programmed wrong. These may be the probable causes:
1. Some mandatory parameter is missing.
2. The parameters of the cycle have not been edited in the correct order.
3. Some data might be superfluous.
SOLUTION In this type of machining, two of the following parameters must always be
programmed:
X Path length.
I Step between machining operations.
K Number of machining operations.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message.
·M· Model
Ref.1705
0030 ‘G61-2: [A B] /X I K/(2) Y J D (2)/ [P Q R S T U V].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the "Multiple machining in a parallelogram pattern (G61)" or
"Multiple machining in a grid pattern (G62)" cycle have been programmed wrong.
These may be the probable causes:
1. Some mandatory parameter is missing.
2. The parameters of the cycle have not been edited in the correct order.
3. Some data might be superfluous.
SOLUTION This type of machining requires the programming of two parameters of each group
(X, I, K) and (Y, J, D).
X/Y Path length.
I/J Step between machining operations.
K/D Number of machining operations.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message.
0031 ‘G63: X Y /I K/(1) [C P][P Q R S T U V].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the "Multiple machining in a circle (G63)" cycle have been
programmed wrong. These may be the probable causes:
1. Some mandatory parameter is missing.
2. The parameters of the cycle have not been edited in the correct order.
3. Some data might be superfluous.
SOLUTION This type of machining requires the programming of:
X/Y Distance from the center to the first hole.
And one of the following data:
I Angular step between machining operations.
K Number of machining operations.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message.
·10·
Error solution
0032 ‘G64: X Y B /I K/(1) [C P][P Q R S T U V].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the "multiple machining in an arc (G64)" cycle have been
programmed wrong. These may be the probable causes:
1. Some mandatory parameter is missing.
2. The parameters of the cycle have not been edited in the correct order.
3. Some data might be superfluous.
SOLUTION This type of machining requires the programming of:
X/Y Distance from the center to the first hole.
B Total angular travel.
And one of the following data:
I Angular step between machining operations.
K Number of machining operations.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message.
0033 ‘G65: X Y /A I/(1) [C P].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the "Multiple machining programmed by means of an arc chord
(G65)" cycle have been programmed wrong. These may be the probable causes:
1. Some mandatory parameter is missing.
2. The parameters of the cycle have not been edited in the correct order.
3. Some data might be superfluous.
SOLUTION This type of machining requires the programming of:
X/Y Distance from the center to the first hole.
And one of the following data:
A Angle of the matrix of the chord with the abscissa axis (in degrees).
I Length of the chord.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message.
0034 ‘G66: [D H][R I][C J][F K] S E [Q].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the "Irregular pocket canned cycle with islands (G66)" have been
programmed wrong. These may be the probable causes:
1. A parameter has been programmed which does not match the calling format.
2. Some mandatory parameter is missing.
3. The parameters of the cycle have not been edited in the correct order.
SOLUTION This machining cycle requires the programming of :
S First block of the description of the geometry of the profiles making up
the pocket.
E End block of the description of the geometry of the profiles making up
the pocket.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message. Also, the following parameters cannot be defined:
H if D has not been defined.
I if R has not been defined.
J if C has not been defined.
K if F has not been defined.
The (X...C) position where the machining takes place cannot be programmed either.
·M· Model
Ref.1705
·11·
Error solution
0035 ‘G67: [A] B [C] [I] [R] [K] [V] [Q].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the roughing (2D/3D pocket) or semi-finishing (3D pocket)
operation have been programmed wrong in the "Irregular pocket canned cycle with
islands". These may be the probable causes:
1. A parameter has been programmed which does not match the calling format.
2. Some mandatory parameter is missing.
3. The parameters of the cycle have not been edited in the correct order.
SOLUTION This machining cycle requires the programming of :
Roughing operation (2D or 3D pockets)
B Depth of pass.
I Total pocket depth.
R Coordinate of the reference plane.
Semi-finishing operation (3D pockets)
B Depth of pass.
I Total pocket depth (if no roughing operation has been defined).
R Coordinate of the reference plane (if no roughing operation has been
defined).
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message. The (X...C) position where the machining takes place
cannot be programmed in this cycle.
0036 ‘G68: [B] [L] [Q] [J] [I] [R] [K].’
·M· Model
Ref.1705
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters for the finishing operation (2D/3D pocket) have been programmed
wrong in the "Irregular pocket cycle with islands. These may be the probable causes:
1. A parameter has been programmed which does not match the calling format.
2. Some mandatory parameter is missing.
3. The parameters of the cycle have not been edited in the correct order.
SOLUTION This machining cycle requires the programming of :
2D pockets
B Cutting pass (if no roughing operation has been defined).
I Total pocket depth (if no roughing operation has been defined).
R Coordinate of the reference plane (if no roughing operation has been
defined).
3D pockets
B Depth of pass.
I Total pocket depth (if no roughing or semi-finishing operation has been
defined).
R Coordinate of the reference plane (if no roughing or semi-finishing
operation has been defined).
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message. The (X...C) position where the machining takes place
cannot be programmed in this cycle.
0037 ‘G69: I B [C D H J K L R].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters of the "Deep hole drilling cycle with variable peck (G69)". These may
be the probable causes:
1. Some mandatory parameter is missing.
2. The parameters of the cycle have not been edited in the correct order.
SOLUTION This type of machining requires the programming of:
I Machining depth.
B Drilling peck (step).
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message. The (X...C) position where the machining takes place
can be programmed in this cycle.
·12·
Error solution
0038 ‘G81-84-85-86-89: I [K].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters have been programmed wrong in the following cycles: drilling (G81),
tapping (G84), reaming (G85) or boring (G86/G89). This could be because parameter
"I : Machining depth" is missing in the canned cycle being edited.
SOLUTION This type of machining requires the programming of:
I Machining depth.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message. The (X...C) position where the machining takes place
can be programmed in this cycle.
0039 ‘G82: I K.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters have been programmed wrong in the "Drilling cycle with dwell (G82)".
This could be because some parameter is missing.
SOLUTION Both parameters must be programmed in this cycle:
I Machining depth.
K Dwell at the bottom.
To program a drilling operation without dwell at the bottom, use function G81.
The parameters must be edited in the order indicated by the error message. The
(X...C) position where the machining takes place can be programmed in this cycle.
0040 ‘G83: I J.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters have been programmed wrong in the "Deep hole drilling with
constant peck (G83)". This could be because some parameter is missing.
SOLUTION This type of machining requires the programming of:
I Machining depth.
J Number of pecks.
The parameters must be edited in the order indicated by the error message. The
(X...C) position where the machining takes place can be programmed in this cycle.
0041 ‘G87: I J K B [C] [D] [H] [L] [V].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters have been programmed wrong in the "Rectangular pocket canned
cycle (G87)". These may be the probable causes:
1. Some mandatory parameter is missing.
2. The parameters of the cycle have not been edited in the correct order.
SOLUTION This type of machining requires the programming of:
I Pocket depth.
J Distance from the center to the edge of the pocket along the abscissa
axis.
K Distance from the center to the edge of the pocket along the ordinate
axis.
B Defines the cutting depth according to the longitudinal axis.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message. The (X...C) position where the machining takes place
can be programmed in this cycle.
0042 ‘G88: I J B [C] [D] [H] [L] [V].’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The parameters have been programmed wrong in the "Circular pocket canned cycle
(G88)". These may be the probable causes:
1. Some mandatory parameter is missing.
2. The parameters of the cycle have not been edited in the correct order.
SOLUTION This type of machining requires the programming of:
I Pocket depth.
J Pocket radius.
B Defines the cutting depth according to the longitudinal axis.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message. The (X...C) position where the machining takes place
can be programmed in this cycle.
·M· Model
Ref.1705
·13·
Error solution
0043 ‘Incomplete Coordinates.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. During simulation or execution, when trying to make a movement defined with
only one coordinate of the end point or without defining the arc radius while a
"circular interpolation (G02/G03) is active.
2. During editing, when editing a circular movement (G02/G03) by defining only one
coordinate of the end point or not defining the arc radius.
SOLUTION The solution for each cause is:
1. A "G02" or "G03" function may be programmed previously in the program history.
In this case, to make a move, both coordinates of the end point and the arc radius
must be defined. To make a linear movement, program "G01".
2. To make a circular movement (G02/G03), both coordinates of the end point and
the arc radius must be programmed.
0044 ‘Incorrect Coordinates.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. An attempt has been made to execute a block syntactically incorrect (G1 X20K-
15)
2. The "I" parameter is missing in the definition of a machining canned cycle (G81G89) Machining depth.
SOLUTION The solution for each cause is:
1. Correct the syntax of the block.
2. This type of machining requires the programming of:
I Machining depth.
The rest of the parameters are optional. The parameters must be edited in the
order indicated by the error message. The (X...C) position where the machining
takes place can be programmed in this cycle.
·M· Model
0045 ‘Polar coordinates not allowed.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE When "Programming with respect to home (G53)", the end point has been defined
in polar or cylindrical coordinates or in Cartesian coordinates with an angle.
SOLUTION When programming with respect to home, only Cartesian coordinates may be
programmed.
Ref.1705
·14·
Error solution
0046 ‘Axis does not exist.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When editing a block whose execution involves the movement of a nonexistent
axis.
2. Sometimes, this error comes up while editing a block that is missing a parameter
of the "G" function. This is because some parameters with an axis name have a
special meaning inside certain "G" functions. For example: G69 I...B....
In this case, parameter "B" has a special meaning after "I". If the "I" parameter
is left out, the CNC assumes "B" as the position where the machining takes place
on that axis. If that axis does not exist, it will issue this error message.
SOLUTION The solution for each cause is:
1. Check that the axis name being edited is correct.
2. Check the block syntax and make sure that all the mandatory parameters have
been programmed.
0047 ‘Program axes.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE No axis has been programmed in a function requiring an axis.
SOLUTION Some instructions require the programming of axes (REPOS, G14, G20, G21...).
0048 ‘Incorrect order of axes.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The axis coordinates have not been programmed in the correct order or an axis has
been programmed twice in the same block.
SOLUTION Remember that the correct programming order for the axes is:
X...Y...Z...U...V...W...A...B...C...
All axes need not be programmed:
0049 ‘Point incompatible with active plane.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When trying to do a circular interpolation, the end point is not in the active plane.
2. When trying to do a tangential exit in a path that is not in the active plane.
SOLUTION The solution for each cause is:
1. Maybe a plane has been defined with "G16", "G17", "G18" or "G19". In this case,
circular interpolations can only be carried out on the main axes defining that plane.
To define a circular interpolation in another plane, it must be defined beforehand.
2. Maybe a plane has been defined with "G16", "G17", "G18" or "G19". In this case,
corner rounding, chamfers and tangential entries/exits can only be carried out on
the main axes defining that plane. To do it in another plane, it must be defined
beforehand.
0050 ‘Program positions on active plane.’
No explanation required.
0051 ‘Perpendicular axis included in active plane.’
No explanation required.
0052 ‘Center of circle programmed incorrectly.’
No explanation required.
0053 ‘Program pitch.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the "Electronic threading cycle (G33)" the parameter for the thread pitch is missing.
SOLUTION Remember that the programming format for this function is:
G33 X...C...L...
Where: "L" is the thread pitch.
·M· Model
Ref.1705
·15·
Error solution
0054 ‘Pitch programmed incorrectly.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A helical interpolation has been programmed with the wrong or negative pitch.
SOLUTION Remember that the programming format is:
G02/G03 X...Y...I...J...Z...K...
Where: "K" is the helical pitch (always positive value).
0055 ‘Positioning axes or Hirth axes not allowed’
No explanation required.
0056 ‘The axis is already slaved.’
No explanation required.
0057 ‘Do not program a slaved axis.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When trying to move an axis alone while being slaved to another one.
2. When trying to slave an axis that is already slaved using the G77 function
"Electronic axis slaving".
SOLUTION The solution for each cause is:
1. A slaved axis cannot be moved separately. To move a slaved axis, its master axis
must be moved. Both axes will move at the same time.
Example: If the Y axis is slaved to the X axis, an X axis move must be programmed
in order to move the Y axis (together with the X axis).
To unslave the axes, program "G78".
2. An axis cannot be slaved to two different axes at the same time. To unslave the
axes, program "G78".
·M· Model
0058 ‘Do not program a GANTRY axis.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When trying to move an axis alone while being slaved to another one as a
GANTRY axis
2. When defining an operation on a GANTRY axis. (Definition of work zone limits,
planes, etc.).
SOLUTION The solution for each cause is:
1. A GANTRY axis cannot be moved separately. To move a GANTRY axis, its
associated axis must be moved. Both axes will move at the same time.
Example: If the Y axis is a GANTRY axis associated with the X axis, an X axis
move must be programmed in order to move the Y axis (together with the X axis).
GANTRY axes are defined by machine parameter.
2. The axes defined as GANTRY cannot be used in the definition of operations or
movements. These operations are defined with the main axis that the GANTRY
axis is associated with.
0059 'Wrong position programmed for the Hirth axis.'
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A rotation of a HIRTH axis has been programmed with a decimal value.
SOLUTION HIRTH axes do not accept decimal angular values. They must be full degrees.
0060 ‘Invalid action.’
No explanation required.
Ref.1705
·16·
Error solution
0061 ‘ELSE not associated with IF.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. While editing in High level language, when editing the "ELSE" instruction without
having previously programmed an "IF".
2. When programming in high level language, an "IF" is programmed without
associating it with any action after the condition.
SOLUTION Remember that the programming formats for this instruction are:
(IF (condition) <action1>)
(IF (condition <action1> ELSE <action2>)
If the condition is true, it executes the <action1>, otherwise, it executes <action2>.
0062 ‘Program label N(0-99999999).’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, a block number out of the 0-99999999
range has been programmed in the "RPT" or "GOTO" instruction.
SOLUTION Remember that the programming format of these instructions is:
(RPT N(block number), N(block number))
(GOTO N(block number))
The block number (label) must be between 0 and 99999999.
0063 ‘Program subroutine number 1 thru 9999.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, a subroutine number out of the 0-9999
range has been programmed in the "SUB" instruction.
SOLUTION Remember that the programming format for this instruction is:
(SUB (integer))
The subroutine number must be between 0 and 9999.
0064 ‘Repeated subroutine.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE There has been an attempt to define a subroutine already existing in another program
of the memory.
SOLUTION In the CNC memory, there could not be more than one subroutine with the same
identifying number even if they are contained in different programs.
0065 ‘The main program cannot have a subroutine.’
DETECTION In execution or while executing programs transmitted via DNC.
CAUSE The possible causes are:
1. An attempt has been made to define a subroutine in the MDI execution mode.
2. A subroutine has been defined in the main program.
SOLUTION The solution for each cause is:
1. Subroutines cannot be defined from the "MDI execution" option of the menu.
2. Subroutines must be defined after the main program or in a separate program.
They cannot be defined before or inside the main program.
0066 ‘Expecting a message.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level, the "MSG" or "ERROR" instruction has been edited
but without the message to be displayed.
SOLUTION Remember that the programming format of these instructions is:
(MSG "message")
(ERROR integer, "error message")
Although it can also be programmed as follows:
(ERROR integer)
(ERROR "error message")
·M· Model
Ref.1705
·17·
Error solution
0067 ‘OPEN is missing.’
DETECTION In execution or while executing programs transmitted via DNC.
CAUSE While programming in high level, a "WRITE" instruction has been edited, but the
OPEN instruction has not been written previously to tell it where that instruction has
to be executed.
SOLUTION The "OPEN" instruction must be edited before the "WRITE" instruction to "tell" the
CNC where (in which program) it must execute the "WRITE" instruction.
0068 ‘Expecting a program number.’
No explanation required.
0069 ‘Program does not exist.’
DETECTION In execution or while executing programs transmitted via DNC.
CAUSE Inside the "Irregular pocket with islands cycle (G66)", it has been programmed that
the profiles defining the irregular pocket are in another program (parameter "Q"), but
that program does not exist.
SOLUTION Parameter "Q" defines which program contains the definition of the profiles that, in
turn, define the irregular pocket with islands. If this parameter is programmed, that
program number must exist and it must contain the labels defined by parameters "S"
and "E".
0070 ‘Program already exists.’
·M· Model
DETECTION In execution or while executing programs transmitted via DNC.
CAUSE This error comes up during execution when using the "OPEN" instruction (While
programming in high level language) to create an already existing program.
SOLUTION Change the program number or use parameters A/D in the "OPEN" instruction:
(OPEN P.........,A/D,… )
Where:
A: Appends new blocks after the existing ones.
D: Deletes the existing program and it opens it as a new one.
0071 ‘Expecting a parameter’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. When defining the function "Modification of canned cycle parameters (G79)", the
parameter to be modified has not been indicated.
2. While editing the machine parameter table, the wrong parameter number has
been entered (maybe the "P" character is missing) or another action is being
carried out (moving around in the table) before quitting the table editing mode.
SOLUTION The solution for each cause is:
1. To define the "G79" function, the cycle parameter to be modified must be indicated
as well as its new value.
2. Enter the parameter number to be edited or press [ESC] to quit this mode.
0072 ‘Parameter does not exist.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, the "ERROR" instruction has been edited,
but the error number to be displayed has been defined either with a local parameter
greater than 25 or with a global parameter greater than 299.
SOLUTION The parameters used by the CNC are:
Local: 0-25
Global: 100-299
0073 ‘Range of write-protected parameters.
Ref.1705
·18·
No explanation required.
0074 ‘Variable not accessible from CNC.’
No explanation required.
Error solution
0075 ‘Read-only variable.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE An attempt has been made to assign a value to a read-only variable.
SOLUTION Read-only variables cannot be assigned any values through programming. However,
their values can be assigned to a parameter.
0076 ‘Write-only variable.’
No explanation required.
0077 ‘Analog output not available.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE An attempt has been made to write to an analog output currently being used by the
CNC.
SOLUTION The selected analog output may be currently used by an axis or a spindle. Select
another analog output between 1 and 8.
0078 ‘Program channel 0(CNC),1(PLC) or 2(DNC).’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, the "KEYSCR" instruction has been
programmed, but the source of the keys is missing.
SOLUTION When programming the "KEYSCR" instruction, the parameter for the source of the
keys must always be programmed:
(KEYSCR=0) : CNC keyboard
(KEYSCR=1) : PLC
(KEYSCR=2) : DNC
The CNC only lets modifying the contents of this variable if it is "zero"
0079 ‘Program error number 0 thru 9999.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, the "ERROR" instruction has been
programmed, but the error number to be displayed is missing.
SOLUTION Remember that the programming format for this instruction is:
(ERROR integer, "error message")
Although it can also be programmed as follows:
(ERROR integer)
(ERROR "error message")
0080 ‘Operator missing.’
No explanation required.
0081 ‘Incorrect expression.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, an expression has been edited with the
wrong format.
SOLUTION Correct the syntax of the block.
0082 ‘Incorrect operation.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. While programming in high level language, the assignment of a value to a
parameter is incomplete.
2. While programming in high level language, the call to a subroutine is incomplete.
SOLUTION Correct (complete) the format to assign a value to a parameter or a call to a
subroutine.
·M· Model
Ref.1705
·19·
Error solution
0083 ‘Incomplete operation.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The various causes might be:
1. While programming in high level language, the "IF" instruction has been edited
without the condition between brackets.
2. While programming in high level language, the "DIGIT" instruction has been
edited without assigning a value to some parameter.
SOLUTION The solution for each cause is:
1. Remember that the programming formats for this instruction are:
(IF (condition) <action1>)
(IF (condition <action1> ELSE <action2>)
If the condition is true, it executes the <action1>, otherwise, it executes
<action2>.
2. Correct the syntax of the block. All the parameters defined within the "DIGIT"
instruction must have a value assigned to them.
0084 ‘Expecting "=".’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, a symbol or data has been entered that
does not match the syntax of the block.
SOLUTION Enter the "=" symbol in the right place.
0085 ‘Expecting ")".’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, a symbol or data has been entered that
does not match the syntax of the block.
SOLUTION Enter the ")" symbol in the right place.
0086 ‘Expecting "(".’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, a symbol or data has been entered that
does not match the syntax of the block.
SOLUTION Enter the "(" symbol in the right place.
0087 ‘Expecting ",".’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE The possible causes are:
1. While programming in high level language, a symbol or data has been entered
that does not match the syntax of the block.
2. While programming in high level language, an ISO-coded instruction has been
programmed.
3. While programming in high level language, an operation has been assigned either
to a local parameter greater than 25 or to a global parameter greater 299.
SOLUTION The solution for each cause is:
1. Enter the "," symbol in the right place.
2. A block cannot contain high level language instructions and ISO-coded
instructions at the same time.
3. The parameters used by the CNC are:
Local: 0-25.
Global: 100-299.
Other parameters out of this range cannot be used in operations.
·M· Model
Ref.1705
·20·
0088 ‘Operation limit exceeded.’
No explanation required.
0089 ‘Logarithm of zero or negative number.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE An operation has been programmed which involves the calculation of a negative
number or a zero.
SOLUTION Only logarithms of numbers greater than zero can be calculated. When working with
parameters, that parameter may have already acquired a negative value or zero.
Verify that the parameter does not reach the operation with that value (0).
Error solution
0090 ‘Square root of a negative number.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE An operation has been programmed which involves the calculation of the square root
of a negative number.
SOLUTION Only the square root of numbers greater than zero can be calculated. When working
with parameters, that parameter may have already acquired a negative value or zero.
Verify that the parameter does not reach the operation with that value (0).
0091 ‘Division by zero.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE An operation has been programmed whose execution involves dividing by zero.
SOLUTION It is only possible to divide by numbers other than zero. When working with
parameters, that parameter may have already acquired a negative value or zero.
Verify that the parameter does not reach the operation with that value (0).
0092 ‘Base zero with positive exponent.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE An operation has been programmed which involves elevating zero to a negative
exponent (or zero).
SOLUTION Zero can only be elevated to positive exponents greater than zero. When working with
parameters, that parameter may have already acquired a negative value or zero.
Check that the parameter does not reach the operation with that value.
0093 ‘Negative base with decimal exponent.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE An operation has been programmed which involves elevating a negative number to
a decimal exponent.
SOLUTION Negative numbers can only be elevated to integer exponents. When working with
parameters, that parameter may have already acquired a negative value or zero.
Check that the parameter does not reach the operation with that value.
0094 ‘ASIN/ACOS range exceeded.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE An operation has been programmed which involves calculating the arcsine or
arccosine of a number out of the ±1 range.
SOLUTION Only the arc sine (ASIN) or the arc cosine (ACOS) of numbers between ±1 can be
calculated. When working with parameters, that parameter may have already
acquired a value out of the mentioned values. Ver ify that the parameter does not reach
the operation with that value (0).
0095 ‘Program row number.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While editing a customizing program, a window has been programmed with the
"ODW" instruction, but the vertical position of the window on the screen is missing.
SOLUTION The vertical position of the window on the screen is defined by rows (0-25).
0096 ‘Program column number.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While editing a customizing program, a window has been programmed with the
"ODW" instruction, but the horizontal position of the window on the screen is missing.
SOLUTION The horizontal position of the window on the screen is defined by columns (0-79).
0097 ‘Program another softkey.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While editing a customizing program, the programming format for the "SK" instruction
has not been respected.
SOLUTION Correct the syntax of the block. The programming format is:
(SK1=(text 1), SK2=(text 2)...)
If the "," character is entered after a text, the CNC expects the name of another softkey.
·M· Model
Ref.1705
·21·
Error solution
0098 ‘Program softkeys 1 thru 7.’
DETECTION While executing in the user channel.
CAUSE In the block syntax, a softkey has been programmed out of the 1 to 7 range.
SOLUTION Only softkeys within the 1 to 7 range can be programmed.
0099 ‘Program another window.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While editing a customizing program, the programming format for the "DW"
instruction has not been respected.
SOLUTION Correct the syntax of the block. The programming format is:
(DW1=(assignment), DW2=(assignment)...)
If the "," character is entered after an assignment, the CNC expects the name of
another window.
0100 ‘Program windows 0 thru 25.’
DETECTION While executing in the user channel.
CAUSE In the block syntax, a window has been programmed out of the 0 to 25 range.
SOLUTION Only windows within the 0 to 25 range can be programmed.
0101 ‘Program rows 0 thru 20.’
DETECTION While executing in the user channel.
CAUSE In the block syntax, a row has been programmed out of the 0 to 20 range.
SOLUTION Only rows within the 0 to 20 range can be programmed.
0102 ‘Program columns 0 thru 79.’
DETECTION While executing in the user channel.
CAUSE In the block syntax, a column has been programmed out of the 0 to 79 range.
SOLUTION Only columns within the 0 to 79 range can be programmed.
0103 ‘Program pages 0 thru 255.’
DETECTION While executing in the user channel.
CAUSE In the block syntax, a page has been programmed out of the 0 to 255 range.
SOLUTION Only pages within the 0 to 255 range can be programmed.
0104 ‘Program INPUT.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, an "IB" instruction has been edited without
associating an "INPUT" to it.
SOLUTION Remember that the programming formats for this instruction are:
(IB (expression) = INPUT "text", format)
(IB (expression) = INPUT "text")
0105 ‘Program inputs 0 thru 25.’
DETECTION While executing in the user channel.
CAUSE In the block syntax, an input has been programmed out of the 0 to 25 range.
SOLUTION Only inputs within the 0 to 25 range can be programmed.
·M· Model
Ref.1705
·22·
0106 ‘Program numerical format.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, an "IB" instruction has been edited with
non-numeric format.
SOLUTION Remember that the programming format for this instruction is:
(IB (expression) = INPUT "text", format)
Where "format" must be a signed number with 6 entire digits and 5 decimals at the
most.
If the "," character is entered after the text, the CNC expects the format.
Error solution
0107 ‘Do not program formats greater than 6.5 .’
DETECTION While executing in the user channel.
CAUSE While programming in high level language, an "IB" instruction has been edited in a
format with more than 6 entire digits or more than 5 decimals.
SOLUTION Remember that the programming format for this instruction is:
(IB (expression) = INPUT "text", format)
Where "format" must be a signed number with 6 entire digits and 5 decimals at the
most.
0108 ‘This command can only be executed in the user channel.’
DETECTION During execution.
CAUSE An attempt has been made to execute a block containing information that can only
be executed through the user channel.
SOLUTION There are specific expressions for customizing programs that can only be executed
inside the user program.
0109 ‘C. User: do not program geometric help, compensation or cycles.’
DETECTION While executing in the user channel.
CAUSE An attempt has been made to execute a block containing geometric aide, tool
radius/length compensation or machining canned cycles.
SOLUTION Inside a customizing program the following cannot be programmed:
Neither geometric assistance nor movements.
Neither tool radius nor length compensation.
Canned cycles.
0110 ‘Local parameters not allowed.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE Some functions can only be programmed with global parameters.
SOLUTION Global parameters are the ones included in the 100-299 range.
0111 ‘Block cannot be executed while running another program’
DETECTION While executing in MDI mode
CAUSE An attempt has been made to execute a customizing instruction from MDI mode while
the user channel program is running.
SOLUTION Customizing instructions can only be executed through the user channel.
0112 ‘WBUF can only be executed in user channel while editing’
DETECTION During normal execution or execution through the user channel.
CAUSE An attempt has been made to execute the "WBUF" instruction.
SOLUTION The "WBUF" instruction cannot be executed. It can only be used in the editing stage
through the user input.
0113 ‘Table limits exceeded.’
DETECTION While editing tables.
CAUSE The possible causes are:
1. In the tool offset table, an attempt has been made to define a tool offset with a
greater number than allowed by the manufacturer.
2. In the parameter tables, an attempt has been made to define a nonexistent
parameter.
SOLUTION The tool offset number must be smaller than the one allowed by the manufacturer.
0114 ‘Offset: D3 R L I K.’
DETECTION While editing tables.
CAUSE In the tool offset table, the parameter editing order has not been respected.
SOLUTION Enter the table parameters in the right order.
0115 ‘Tool: T4 D3 F3 N5 R5(.2).’
DETECTION While editing tables.
CAUSE In the tool table, the parameter editing order has not been respected.
SOLUTION Enter the table parameters in the right order.
·M· Model
Ref.1705
·23·
Error solution
0116 ‘Origin: G54-59 G159N(1-20) axes (1-7).’
DETECTION While editing tables.
CAUSE In the Zero offset table, the zero offset to be defined (G54-G59) or G159N(1-20) has
not be selected.
SOLUTION Enter the table parameters in the right order. To fill out the zero offset table, first select
the offset to be defined (G54-G59) or G159N(1-20) and then the zero offset position
for each axis.
0117 ‘M function: M4 S4 bits(8).’
DETECTION While editing tables.
CAUSE In the "M" function table, the parameter editing order has not been respected.
SOLUTION Edit table following the format:
M1234 (associated subroutine) (customizing bits)
0118 ‘G51 [A] E’
DETECTION In execution or while executing programs transmitted via DNC.
CAUSE In the "Look-Ahead (G51)" function, the parameter for the maximum contouring error
is missing.
SOLUTION This type of machining requires the programming of:
E: Maximum contouring error.
The rest of the parameters are optional. The parameters must be edited in the order
indicated by the error message.
0119 ‘Leadscrew: Coordinate-error.’
DETECTION While editing tables.
CAUSE In the leadscrew compensation tables, the parameter editing order has not been
respected.
SOLUTION Enter the table parameters in the right order.
P123 (position of the axis to be compensated) (leadscrew error at that point)
0120 ‘Incorrect axis.’
DETECTION While editing tables.
CAUSE In the leadscrew compensation tables, an attempt has been made to edit a different
axis from the one corresponding to that table.
SOLUTION Each axis has its own table for leadscrew compensation. The table for each axis can
only contain the positions for that axis.
0121 ‘Program P3 = value.’
DETECTION While editing tables.
CAUSE In the machine parameter table, the editing format has not been respected.
SOLUTION Enter the table parameters in the right order.
P123 = (parameter value)
0122 'Tool magazine: P(1-255) = T(1-9999).’
DETECTION While editing tables.
CAUSE In the tool magazine table, the editing format has not been respected or some data
is missing.
SOLUTION Enter the table parameters in the right order.
·M· Model
Ref.1705
·24·
0123 ‘Tool T0 does not exist.’
DETECTION While editing tables.
CAUSE In the tool table, an attempt has been made to edit a tool as T0.
SOLUTION No tool can be edited as T0. The first tool must be T1.
0124 ‘Offset D0 does not exist.’
DETECTION While editing tables.
CAUSE In the tool table, an attempt has been made to edit a tool offset as D0.
SOLUTION No tool offset can be edited as D0. The first tool offset must be D1.
Error solution
0125 ‘Do not modify the active tool or the next one.’
DETECTION During execution.
CAUSE In the tool magazine table, an attempt has been made to change the active tool or
the next one.
SOLUTION During execution, neither the active tool nor the next one may be changed.
0126 ‘Tool not defined.’
DETECTION While editing tables.
CAUSE In the tool magazine table, an attempt has been made to assign to the magazine
position a tool that is not defined in the tool table.
SOLUTION Define the tool in the tool table.
0127 ‘Magazine is not RANDOM.’
DETECTION While editing tables.
CAUSE There is no RANDOM magazin e and, in the tool magazine table, the to ol number does
not match the tool magazine position.
SOLUTION When the tool magazine is not RANDOM, the tool number must be the same as the
magazine position (pocket number).
0128 ‘The position of a special tool is set.’
DETECTION While editing tables.
CAUSE In the tool magazine table, an attempt has been made to place a tool in a magazine
position reserved for a special tool.
SOLUTION When a special tool occupies more than one position in the magazine, it has a
reserved position in the magazine. No other tool can be placed in this position.
0129 ‘Next tool only possible in machining centers.’
DETECTION During execution.
CAUSE A tool change has been programmed with M06, but the machine is not a machining
center. (it is not expecting the next tool).
SOLUTION When the machining is not a machining center, the tool change is done automatically
when programming the tool number "T".
0130 ‘Write 0/1.’
DETECTION While editing machine parameters
CAUSE An attempt has been made to assign the wrong value to a parameter.
SOLUTION The parameter only admits values of 0 or 1.
0131 ‘Write +/-.’
DETECTION While editing machine parameters
CAUSE An attempt has been made to assign the wrong value to a parameter.
SOLUTION The parameter only admits values of + or -.
0132 ‘Write YES/NO.’
DETECTION While editing machine parameters
CAUSE An attempt has been made to assign the wrong value to a parameter.
SOLUTION The parameter only admits values of YES or NO.
0133 ‘Write ON/OFF.’
DETECTION While editing machine parameters
CAUSE An attempt has been made to assign the wrong value to a parameter.
SOLUTION The parameter only admits values of ON or OFF.
·M· Model
Ref.1705
·25·
Error solution
0134 ‘Values 0 thru 2.’
0135 ‘Values 0 thru 3.’
0136 ‘Values 0 thru 4.’
0137 ‘Values 0 thru 9.’
0138 ‘Values 0 thru 29.’
0139 ‘Values 0 thru 100.’
0140 ‘Values 0 thru 255.’
0141 ‘Values 0 thru 9999.’
0142 ‘Values 0 thru 32767.’
0143 ‘Values within +/-32767.’
0144 ‘Values 0 thru 65535.’
DETECTION While editing machine parameters
CAUSE The possible causes are:
1. An attempt has been made to assign the wrong value to a parameter.
2. During execution, when inside the program a call has been made to a subroutine
(MCALL, PCALL) with a value greater than allowed.
0145 ‘Format +/- 5.5.’
DETECTION While editing machine parameters
CAUSE An attempt has been made to assign the wrong value to a parameter.
SOLUTION The parameter only admits values with the format:
0146 ‘Word does not exist.’
No explanation required.
0147 ‘Numerical format exceeded.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A data or parameter has been assigned a value greater than the established format.
SOLUTION Correct the syntax of the block. Most of the time, the numeric format will be 5.4 (5
integers and 4 decimals).
0148 ‘Text too long.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, the "ERROR" or "MSG" instruction has
been assigned a text with more than 59 characters.
SOLUTION Correct the syntax of the block. The "ERROR" and "MSG" instructions cannot be
assigned texts longer than 59 characters.
0149 ‘Incorrect message.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE While programming in high level language, the text associated with the "ERROR"
or "MSG" instruction has been edited wrong.
SOLUTION Correct the syntax of the block. The programming format is:
(MSG "message")
(ERROR number, "message")
The message must be between " ".
·M· Model
Ref.1705
·26·
0150 ‘Incorrect number of bits.’
DETECTION While editing tables.
CAUSE The possible causes are:
1. In the "M" function table, in the section on customizing bits:
The number does not have 8 bits.
The number does not consist of 0’s and 1’s.
2. In the machine parameter table, an attempt has been made to assign the wrong
value of bit to a parameter.
SOLUTION The solution for each cause is:
1. The customizing bits must consist of 8 digits of 0’s and 1’s.
2. The parameter only admits 8-bit or 16-bit numbers.
Error solution
0151 ‘Negative numbers not allowed.’
No explanation required.
0152 ‘Incorrect parametric programming.’
DETECTION During execution.
CAUSE The parameter has a value that is incompatible with the function it has been assigned
to.
SOLUTION This parameter may have taken the wrong value, in the program history. Correct the
program so this parameter does not reach the function with that value.
0153 ‘Decimal format not allowed.’
No explanation required.
0154 ‘Insufficient memory.’
DETECTION During execution.
CAUSE The CNC does not have enough memory to internally calculate the paths.
SOLUTION Sometimes, this error is taken care of by changing the machining conditions.
0155 ‘Help not available.’
No explanation required.
0156 ‘Don’t program G33 ,G95 or M19 S with no spindle encoder’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A "G33", "G95" or "M19 S" has been programmed without having an encoder on the
spindle.
SOLUTION If the spindle does not have an encoder, functions "M19 S", "G33" or "G95" cannot
be programmed. Spindle machine parameter "NPULSES (P13)" indicates the
number of encoder pulses per turn.
0157 ‘G79 not allowed when there is no active canned cycle.’
DETECTION During execution.
CAUSE An attempt has been made to execute the "Modification of canned cycle parameters
(G79)" function without any canned cycle being active.
SOLUTION The "G79" function modifies the values of a canned cycle; therefore, there must be
an active canned cycle and the "G79" must be programmed in the influence zone of
that canned cycle.
0158 ‘Tool T must be programmed with G67 and G68.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the "Irregular pocket canned cycle with islands (G66)" the tool has not been defined
for roughing "G67" (2D/3D pockets) for semi-finishing "G67" (3D pocket) or finishing
"G68" (2D/3D pocket).
SOLUTION The irregular pocket canned cycle with islands requires the programming of the
roughing tool "G67" (2D/3D pockets), the semi-finishing tool "G67" (3D pocket) and
the finishing tool "G68" (2D/3D pocket).
0159 ‘Inch programming limit exceeded.’
DETECTION During execution.
CAUSE An attempt has been made to execute in inches a program edited in millimeters.
SOLUTION Enter function G70 (inch programming) or G71 (mm programming) at the beginning
of the program.
0160 ‘G79 not allowed when executing the canned cycle.’
No explanation required.
·M· Model
Ref.1705
·27·
Error solution
0161 ‘G66 must be programmed before G67 and G68.’
DETECTION During execution.
CAUSE A roughing operation "G67" (2D/3D pockets), a semi-finishing operation "G67" (3D
pocket) or a finishing operation "G68" (2D/3D pocket) has been programmed without
having previous programmed the call to an "Irregular pocket canned cycle with islands
(G66)".
SOLUTION When working with irregular pockets, before programming the aforementioned
cycles, the call to the "Irregular canned cycle with islands (G66)" must be
programmed.
0162 ‘No negative radius allowed with absolute coordinates’
DETECTION During execution.
CAUSE While operating with absolute polar coordinates, a movement with a negative radius
has been programmed.
SOLUTION Negative radius cannot be programmed when using absolute polar coordinates.
0163 ‘The programmed axis is not longitudinal.’
DETECTION During execution.
CAUSE An attempt has been made to modify the coordinates of the point where the canned
cycle is to be executed using the "Modification of the canned cycle parameters
(G79)"function.
SOLUTION With "G79", the parameters defining a canned cycle may be modified, except the
coordinates of the point where it will be executed. To change those coordinates,
program only the new coordinates.
0164 ‘Wrong password.’
DETECTION While assigning protections.
CAUSE [ENTER] has been pressed before selecting the type of code to be assigned a
password.
SOLUTION Use the softkeys to select the type of code to which a password is to be assigned.
0165 ‘Password: utilizar letras (mayúsculas o minúsculas) o dígitos.’
DETECTION While assigning protections.
CAUSE A bad character has been entered in the password.
SOLUTION The password can only consist of letters (upper and lower case) or digits.
0166 ‘Only one HIRTH axis per block is allowed.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A movement has been programmed which involves the movement of two HIRTH axes
simultaneously.
SOLUTION The CNC does not admit movements involving more than one HIRTH axis at a time.
HIRTH axes must move one at a time.
0167 ‘Rot. axis position.: absolute values (G90) within 0-359.9999.’
DETECTION During execution.
CAUSE A movement of a positioning-only rotary axis has been programmed. The movement
has been programmed in absolute coordinates (G90) and the target coordinate of the
movement is not within the 0 to 359.9999 range.
SOLUTION Positioning-only rotary axes: In absolute coordinates, only movements within the 0
to 359.9999 range are possible.
·M· Model
Ref.1705
·28·
0168 'Rotary axis: absolute values (G90) within +/-359.9999.'
DETECTION During execution.
CAUSE A movement of a rotary axis has been programmed. The movement has been
programmed in absolute coordinates (G90) and the target coordinate of the
movement is not within the 0 to 359.9999 range.
SOLUTION Rotary axes: In absolute coordinates, only movements within the 0 to 359.9999 range
are possible.
Error solution
0169 ‘Modal subroutines cannot be programmed.’
DETECTION While executing in MDI mode
CAUSE An attempt has been made to call upon a modal subroutine (MCALL).
SOLUTION MCALL modal subroutines cannot be executed from the menu option "MDI
execution".
0170 ‘Program symbols 0 thru 255 in positions 0-639, 0-335. ‘
No explanation required.
0171 ‘The window must be previously defined.’
DETECTION During normal execution or execution through the user channel.
CAUSE An attempt has been made to write in a window (DW) that has not been previously
defined (ODW).
SOLUTION It is not possible to write in a window that has not been previously defined. Check that
the window to write in (DW) has been previously defined.
0172 ‘The program is not accessible’
DETECTION During execution.
CAUSE An attempt has been made to execute a program that cannot be executed.
SOLUTION The program may be protected against execution. To know whether a program may
be executed, check for the "X" character on the attributes column. If this character
is missing, the program cannot be executed.
0173 ‘It is not possible to program angle + angle.’
No explanation required.
0174 ‘Circular (helical) interpolation not possible.’
DETECTION During execution.
CAUSE An attempt has been made to execute a helical interpolation while the "LOOK-
AHEAD (G51)" function was active.
SOLUTION Helical interpolations are not possible while the "LOOK-AHEAD (G51)" function is
active.
0175 'Analog inputs: ANAI(1-8) = +/-5 Volts.’
DETECTION During execution.
CAUSE An analog input has taken a value out of the ±5V range.
SOLUTION Analog inputs may only take values within the ±5V range.
0176 'Analog outputs: ANAO(1-8) = +/-10 Volts.’
DETECTION During execution.
CAUSE An analog output has been assigned a value out of the ±10V range.
SOLUTION Analog outputs may only take values within the ±10V range.
0177 ‘A gantry axis cannot be part of the active plane.’
No explanation required.
0178 ‘G96 only possible with analog spindle.’
DETECTION During execution.
CAUSE The "G96" function has been programmed but either the spindle speed is not
controlled or the spindle does not have an encoder.
SOLUTION To operate with the "G96" function, the spindle speed must be controlled
(SPDLTYPE(P0)=0) and the spindle must have an encoder (NPULSES(P13) other
than zero).
0179 ‘Do not program more than 4 axes simultaneously.’
No explanation required.
·M· Model
Ref.1705
·29·
Error solution
0180 ‘Program DNC1/2/E, HD or CARD A (optional).’
DETECTION While editing or executing.
CAUSE While programming in high level language, in the "OPEN" and "EXEC" instructions,
an attempt has been made to program a parameter other than DNC1/2E, HD or CARD
A, or the DNC parameter has been assigned a value other than 1, 2 or E.
SOLUTION Check the syntax of the block.
0181 ‘Program A (append) or D (delete).’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the "OPEN" instruction the A/D parameter is missing.
SOLUTION Check the syntax of the block. The programming format is:
(OPEN P.........,A/D,… )
Where:
A Appends new blocks after the existing ones.
D Deletes the existing program and it opens it as a new one.
0182 ‘Option not available.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE A "G" function has been defined which is not a software option.
0183 ‘Cycle does not exist.’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE In the "DIGIT" instruction, a digitizing cycle has been defined which is not available.
SOLUTION The "DIGIT" instruction only admits two types of digitizing:
(DIGIT 1,…) : Grid pattern digitizing cycle.
(DIGIT 2,…) : Arc pattern digitizing cycle.
·M· Model
0184 ‘T with subroutine: program only T and D.’
No explanation required.
0185 ‘Tool offset does not exist’
DETECTION While editing at the CNC or while executing a program transmitted via DNC.
CAUSE Within the block syntax, a tool offset has been called upon which is greater than the
ones allowed by the manufacturer.
SOLUTION Program a new smaller tool offset.
0188 ‘Function not possible from PLC.’
DETECTION During execution.
CAUSE From the PLC channel and using the "CNCEX" instruction, an attempt has been made
to execute a function that is incompatible with the PLC channel execution.
SOLUTION The installation manual (chapter 11.1.2) offers a list of the functions and instructions
that may be executed through the PLC channel.
0189 ‘The live tool does not exist.’
No explanation required.
0190 ‘Programming not allowed while in tracing mode.’
DETECTION During execution.
CAUSE Among the blocks defining the "Tracing and digitizing canned cycles (TRACE)", there
is block that contains a "G" function which does not belong in the profile definition.
SOLUTION The "G" functions available in the profile definition are:
G00 G01 G02 G03 G06 G08 G09 G36
G39 G53 G70 G71 G90 G91 G93
Ref.1705
·30·
0191 ‘Do not program tracing axes.’
DETECTION During execution.
CAUSE An attempt has been made to move an axis that has been defined as a tracing axis
using the "G23" function.
SOLUTION The tracing axes are controlled by the CNC. To deactivate the tracing axes, use the
"G25" function..
Loading...