fagor 8070 User Manual

CNC

8070

Error solving manual

(Ref: 1308)

MACHINE SAFETY

It is up to the machine manufacturer to make sure that the safety of the machine
is enabled in order to prevent personal injury and damage to the CNC or to the
products connected to it. On start-up and while validating CNC parameters, it
checks the status of the following safety elements. If any of them is disabled, the
CNC shows a warning message.

• Feedback alarm for analog axes.

• Software limits for analog and sercos linear axes.

• Following error monitoring for analog and sercos axes (except the spindle)
both at the CNC and at the drives.

• Tendency test on analog axes.

FAGOR AUTOMATION shall not be held responsible for any personal injuries or
physical damage caused or suffered by the CNC resulting from any of the safety
elements being disabled.

HARDWARE EXPANSIONS

FAGOR AUTOMATION shall not be held responsible for any personal injuries or
physical damage caused or suffered by the CNC resulting from any hardware
manipulation by personnel unauthorized by Fagor Automation.

If the CNC hardware is modified by personnel unauthorized by Fagor Automation,
it will no longer be under warranty.

COMPUTER VIRUSES

FAGOR AUTOMATION guarantees that the software installed contains no
computer viruses. It is up to the user to keep the unit virus free in order to
guarantee its proper operation.

Computer viruses at the CNC may cause it to malfunction. An antivirus software
is highly recommended if the CNC is connected directly to another PC, it is part
of a computer network or floppy disks or other computer media is used to transmit
data.

FAGOR AUTOMATION shall not be held responsible for any personal injuries or
physical damage caused or suffered by the CNC due a computer virus in the
system.

If a computer virus is found in the system, the unit will no longer be under warranty.

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 changed due to technical
modifications. Fagor Automation reserves the right to make any changes to 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.

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
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, thus no absolute match is
guaranteed. Anyway, the contents of the manual is periodically checked making
and including the necessary corrections in a future 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 solving manual

INDEX

0000-0999.......................................................................................5

1000-1999.....................................................................................17

2000-2999...................................................................................100

3000-3999...................................................................................106

4000-4999...................................................................................122

5000-5999...................................................................................130

6000-6999...................................................................................133

7000-7999...................................................................................141

8000-8999...................................................................................145

9000-9999...................................................................................173

23000-23999...............................................................................177

Tool and tool magazine table ..................................................178

Profile editor..............................................................................180

CNC 8070

(REF: 1308)

·3·

Error solving manual

0000-0999

0001 'SYSTEM ERROR'

DETECTION During execution.
CAUSE Software or hardware errors that cause corrupt data and/or incoherent results.
SOLUTION This type of errors usually force the CNC output. If the error persists, contact your

supplier.

0002 'SYSTEM WARNING'

DETECTION During execution.
CAUSE Warning of internal situations that could become system errors.
SOLUTION Usually the CNC is restored by closing the warning. If the error persists, contact your

supplier.

0003 'Error when requesting memory. Restart Windows & CNC'

DETECTION During CNC startup.
CAUSE The CNC does not have enough memory or the memory is too fragmented.
SOLUTION Restart the unit and re-initiate the CNC. If the memory is too fragmented, when

starting the unit up and re-initia te the CNC, the error will disappear. If the error persists
after powering up several times, contact your supplier.

0004 'Checksum error in PLC data'

DETECTION During CNC startup.
CAUSE The PLC data related to marks, counters, timers and registers saved into a disk is

not valid. The plcdata.bin file that contains these data does not exist, is not accessible

or is corrupt.
CONSEQUENCE The PLC data related to marks, counters, timers and registers is lost.
SOLUTION If the error persists after powering the CNC up several times, contact your supplier.

0005 'The CNC was not turned off properly, it must be homed'

DETECTION During CNC startup.
CAUSE The CNC data related to coordinates, zero offsets, etc. that are saved into the disk

is not valid. The orgdata.tab file that contains these data does not exist, is not

accessible or is corrupt.
CONSEQUENCE The CNC data related to coordinates, zero offsets, parts counter, kinematics, etc. are

lost.
SOLUTION If the error persists after powering the CNC up several times, contact your supplier.

0006 'Preparation takes longer than half the cycle time.

DETECTION On CNC startup or during execution.
CAUSE Data preparation at the CNC per PLC cycle takes too long.
CONSEQUENCE The PREPFREQ parameter does not have the desired effect.
SOLUTION Decrease the value of the PREPFREQ parameter of the channel.

0007 'To complete the reset, restart the CNC.

DETECTION After a CNC reset.
CAUSE The user has reset the CNC twice in a row and none of them has ended correctly.
SOLUTION Restart the CNC. If the user presses the [RESET] key for the third time, the CNC

application shuts down.

CNC 8070

(REF: 1308)

·5·

Error solving manual

0008 'The key has been rejected.

DETECTION On CNC startup or during execution.
CAUSE The CNC has detected that two incompatible keys have been pressed at the same

time. The [START] key, the spindle start keys and the key for spindle orientation must
always be pressed alone; if they are pressed at the same time, they are both canceled.

SOLUTION If it has been by mistake, ignore the error. If the error persists or it comes up during

start-up, verify that no keys are pressed (stuck) on the keyboard. If the error persists
after powering the CNC up several times, contact your supplier.

0010 'Error when testing the RAM with battery'

DETECTION During CNC startup.
CAUSE The start-up test has detected a checksum error in the data of the NVRAM and,

therefore, a failure in it.

CONSEQUENCE The saved data may not be correct (related to coordinates, zero offsets, parts counter,

kinematics, etc.).

SOLUTION If the error persists after powering the CNC up several times, contact your supplier.

0011 'Checksum error in block search data'

DETECTION During CNC startup.
CAUSE Checksum error in the data required to execute an automatic block search.
CONSEQUENCE An automatic block search cannot be executed.
SOLUTION If the error persists after powering the CNC up several times, contact your supplier.

0020 'Wrong access to a variable'

DETECTION On CNC startup or when changing pages.
CAUSE The CNC is accessing an interface variable that does not exist.
SOLUTION Contact the machine manufacturer or the person who designed the interface screens

to remove or correct the access to the variable.

0022 'Variable that may be modified during setup'

DETECTION When defining variables during setup.
CAUSE A variable has been defined in the setup environment that is not admitted.
SOLUTION Refer to the operating manual for the list of variables that are admitted.

0023 'The program must be stopped before initiating the trace for the first time.

DETECTION When starting a trace at the oscilloscope.
CAUSE It is the first time that the oscilloscope starts a trace and there is a program in

execution. The trace uses drive variables that either are not in the machine
parameters table or are in that table but are asynchronous.

SOLUTION Stop the program in execution.

0024 'Error when initiating the trace'

DETECTION When starting a trace at the oscilloscope.
CAUSE There are no variables defined in the channels of the oscilloscope, there are more

than two Sercos variables of the same drive or the syntax of one of the variables is
wrong.

SOLUTION Check the variables defined in the channels of the oscilloscope. The oscilloscope can

only access two Sercos variables of each drive.

CNC 8070

(REF: 1308)

·6·

0025 'Error when registering PLC defines'

DETECTION When registering the variables associated with the external PDEF symbols defined

in the PLC program.

CAUSE The plc_prg.sym that contains the necessary information to create the variables

associated with the external PDEF symbols is corrupt.

SOLUTION Delete the plc_prg.sym file and compile the PLC program to create this file again. If

the error persists, contact your supplier.

0026 'Variable not allowed in the oscilloscope environment'

DETECTION When defining variables defined in a channel of the oscilloscope.
CAUSE The variable assigned to the channel of the oscilloscope is a simulation,

asynchronous variable or is a string.

SOLUTION Refer to the operating manual for the list of variables that are admitted.

Error solving manual

0040 'M before-before or Before-After with subroutine does not admit movements in the block'

DETECTION During the validation of the machine parameters.
CAUSE In the M functions table, there is a function with associated subroutine and Before-

Before or Before-After synchronization type.
SOLUTION The CNC always executes the subroutine associated with an M function at the end

of the block where the function has been programmed. Define the M function without

synchronization or with After-After synchronization.

0041 'Duplicate M in the table'

DETECTION During the validation of the machine parameters.
CAUSE There is a duplicate function in the M functions table.
SOLUTION Correct the definition of the functions. The table cannot have two M functions with

the same number.

0042 'Wrong machine parameter value'

DETECTION During the validation of the machine parameters.
CAUSE The machine parameter has the wrong value.
SOLUTION Set the machine parameter with a value within the admitted limits. The error window

shows which is the wrong parameter and the maximum and minimum value admitted.

0043 'Restart the CNC to assume the new value'

DETECTION During the validation of the machine parameters.
CAUSE The user has changed a machine parameter and the CNC application must be

restarted in order to assume its new value.
SOLUTION Restart the CNC.

0044 'Wrong axis name or undefined axis name'

DETECTION During the validation of the machine parameters.
CAUSE The machine parameter is not defined or it has the wrong axis name.
SOLUTION Correct the machine parameters. The valid axis names are the ones defined in

parameter AXISNAME.

In parameter AXISNAME, the axis name must be defined by 1 or 2 characters. The

first character must be one of the letters X - Y - Z - U - V - W - A - B - C. The second

character is optional and will be a numerical suffix between 1 and 9. This way, the

name of the spindles may be within the range X, X1…X9,...C, C1…C9.

0045 'Wrong spindle name'

DETECTION During the validation of the machine parameters.
CAUSE The user has defined the machine parameter with the wrong spindle name.
SOLUTION Correct the machine parameters. The valid spindle names are the ones defined in

parameter SPDLNAME.

In parameter SPDLNAME, the spindle name must be defined by 1 or 2 characters.

The first character must be the letter S. The second character is optional and will be

a numerical suffix between 1 and 9. This way, the name of the spindles may be within

the range S, S1 ... S9.

0046 'Nonexistent axis'

DETECTION During the validation of the machine parameters.
CAUSE The user has set a machine parameter that represents the name of an axis with a

name that does not exist in parameter AXISNAME.
SOLUTION Correct the machine parameters. The valid axis names are the ones defined in

parameter AXISNAME.

0047 'A main axis cannot be defined as slave'

DETECTION During the validation of the machine parameters.
CAUSE The slave axis of a gantry axis is the master of another gantry axis.
SOLUTION Correct the gantry axes table. The master axis of a gantry axis cannot be the slave

of another gantry axis.

0048 'An axis cannot be a slave of several masters'

DETECTION During the validation of the machine parameters.
CAUSE The slave axis of a gantry axis is already defined as the slave axis in another gantry

axis.
SOLUTION Correct the gantry axes table. An axis cannot be the slave of several masters.

CNC 8070

(REF: 1308)

·7·

Error solving manual

0049 'A master axis cannot be a slave and vice versa'

DETECTION During the validation of the machine parameters.
CAUSE The master axis of a gantry axis is the slave of another gantry axis or vice versa.
SOLUTION Correct the gantry axes table. The master axis of a gantry axis cannot be the slave

of another gantry axis or vice versa.

0050 'The master and slave axes must be of the same type (AXISTYPE)'

DETECTION During the validation of the machine parameters.
CAUSE Both axes of a gantry pair are not of the same type; linear or rotary.
SOLUTION The axes of a gantry pair must be of the same type, linear or rotary (parameter

AXISTYPE). Check the gantry axes table and/or the AXISTYPE parameter of both
axes.

0051 'The master and slave axes must have certain parameters with the same value'

DETECTION During the validation of the machine parameters.
CAUSE The two axes of a gantry axis do not have the same properties.
SOLUTION Check the gantry axes table and/or the following machine parameters of the axes.

• The linear axes must have parameters AXISMODE, FACEAXIS and LONGAXIS
set the same way.

• The rotary axes must have parameters AXISMODE, SHORTESTWAY and
CAXIS set the same way.

0052 'Module difference too small'

DETECTION During the validation of the machine parameters.
CAUSE The difference between machine parameters MODUPLIM and MODLOWLIM is

lower than the resolution of the axis.

SOLUTION Check the resolution of the axis; if correct, increase MODUPLIM or decrease

MODLOWLIM.

CNC 8070

0053 'Parameter MGPAXIS repeated in several handwheels'

DETECTION During the validation of the machine parameters.
CAUSE There are two or more handwheels assigned to the same axis in the Jog table

parameters.

SOLUTION One axis can only have one handwheel assigned to it.

0054 'The MOVAXIS and COMPAXIS axis must be different'

DETECTION During the validation of the machine parameters.
CAUSE In one of the cross compensation tables, the compensated axis and the axis whose

movement affects the compensated axis are the same.

SOLUTION The two axes of each cross compensation table must be different (parameters

MOVAXIS and COMPAXIS).

0055 'The same axis is causing and suffering the cross compensation error'

DETECTION During the validation of the machine parameters.
CAUSE In the cross compensation tables, checking the different associations of

compensated (affected) axes (parameter COMPAXIS) and those (parameter
MOVAXIS) whose movements affect the other ones, there is an axis whose
movement is affected by itself.

SOLUTION Check the relationship between the defined cross compensations. Check parameters

MOVAXIS and COMPAXIS of the defined cross compensations.

0056 'Compensation table positions not in ascending order'

DETECTION During the validation of the machine parameters.
CAUSE In the compensation tables, the points to be compensated are not ordered correctly

or the value to compensate in all the points have a zero value.

SOLUTION The POSITION parameter within the compensation tables must have ascending

values. The value to compensate cannot be zero in all the points.

(REF: 1308)

·8·

0057 'Compensation table with error slope greater than 1'

DETECTION While validating the machine parameters (leadscrew error compensation table)
CAUSE In the leadscrew compensation tables, the difference between two consecutive errors

is greater than the gap between those points.

SOLUTION The error slope in leadscrew compensation tables cannot be greater than 1. Increase

the gap between points; if this is not possible, the error entered for the leadscrew is
so large that cannot be compensated for.

Error solving manual

0058 'The CNC must be restarted too assume the changes in the HMI table,'

DETECTION During the validation of the machine parameters.
CAUSE The CNC application must be restarted in order to assume the changes made to the

HMI table.

SOLUTION Restart the CNC.

0059 'The CNC must be restarted too assume the changes in the tool magazine table,'

DETECTION During the validation of the machine parameters.
CAUSE The CNC application must be restarted in order to assume the changes made to the

tool magazine table.

SOLUTION Restart the CNC.

0060 'The maximum jogging feedrate exceeds the maximum feedrate set for the axis'

DETECTION During the validation of the machine parameters.
CAUSE Parameter MAXMANFEED is greater than G00FEED.
SOLUTION Decrease the value of parameter MAXMANFEED; it must be lower than G00FEED.

0061 'The manual rapid feedrate exceeds the maximum feedrate set for the axis'

DETECTION During the validation of the machine parameters.
CAUSE Parameter JOGRAPFEED is greater than G00FEED.
SOLUTION Decrease the value of parameter JOGRAPFEED; it must be lower than G00FEED.

0062 'The continuous Jog feedrate exceeds the maximum feedrate set for the axis'

DETECTION During the validation of the machine parameters.
CAUSE Parameter JOGFEED is greater than G00FEED.
SOLUTION Decrease the value of parameter JOGFEED; it must be lower than G00FEED.

0063 'The incremental jog feedrate exceeds the maximum feedrate set for the axis'

DETECTION During the validation of the machine parameters.
CAUSE Parameter INCJOGFEED is greater than G00FEED.
SOLUTION Decrease the value of parameter INCJOGFEED; it must be lower than G00FEED.

0064 'The master and slave axes must have the same I0TYPE'

DETECTION During the validation of the machine parameters.
CAUSE The Io types of both gantry axes are not the same.
SOLUTION Both axes must have the same type of reference mark (parameter I0TYPE).

0065 'A Hirth axis cannot be Gantry"

DETECTION During the validation of the machine parameters.
CAUSE 'A hirth axis cannot be part of the gantry axis'
SOLUTION 'The axis cannot be a hirth axis (parameter HIRTH). Use another type of axis to make

the gantry axis.

0066 'A Gantry axis cannot have REFSHIFT'

DETECTION During the validation of the machine parameters.
CAUSE One of the axes making up the gantry axis has parameter REFSHIFT set to a value

other than zero in some set of parameters.

SOLUTION Set parameter REFSHIFT all the sets to 0.

0067 'A Gantry axis cannot be unidirectional'

DETECTION During the validation of the machine parameters.
CAUSE A unidirectional rotary axis cannot be part of the gantry axis.
SOLUTION The axis cannot be unidirectional (parameter UNIDIR). Use another type of axis to

make the gantry axis.

CNC 8070

0068 'Gantry/Tandem axes: the slave cannot go before the master in AXISNAME'

DETECTION During the validation of the machine parameters.
CAUSE The slave axis is defined before the master axis in the axis name assigning tables

(parameter AXISNAME).

SOLUTION In the table, define the master axis before the slave axis or swap the master and slave

axes in the gantry or tandem pair.

(REF: 1308)

·9·

Error solving manual

0069 'Gantry axes: The slave cannot have DECINPUT (home switch) if the master does not

have one'

DETECTION During the validation of the machine parameters.
CAUSE The slave axis of a gantry axis has a home switch but the master axis doesn't.
SOLUTION In a gantry axis, there may be a home switch on the master axis, on both axes or on

none (parameter DECINPUT).

0070 'Gantry/Tandem axes: LIMIT+ and LIMIT- must be the same for the master and the slave '

DETECTION During the validation of the machine parameters.
CAUSE In a gantry or tandem pair, the software travel limits are different on the two axes.
SOLUTION Set both axes with the same software travel limits (parameters LIMIT+ and LIMIT-).

0071 'Following error monitoring is not active at the CNC'

DETECTION During the validation of the machine parameters.
CAUSE In some set of parameters, following error monitoring is not active. This situation can

only be allowed during setup; once setup is completed, this watch must be enabled.

SOLUTION Activate the following error monitoring in all sets of parameters (parameter

FLWEMONITOR).

0072 'Feedback alarm not activated'

DETECTION During the validation of the machine parameters.
CAUSE In some set of parameters of an analog axis or spindle, the feedback alarm is not

activated. This situation can only be allowed during setup; once setup is completed,
this watch must be enabled.

SOLUTION Activate the feedback alarm in all the sets of the analog axes and spindles (parameter

FBACKAL).

0073 'Software travel limits not activated'

DETECTION During the validation of the machine parameters.
CAUSE The software travel limits of some axis are not activated. Both LIMIT+ and LIMIT-

parameters of the axis are set to 0.

SOLUTION Set the software travel limits of all the axes (parameters LIMIT+ and LIMIT).

0074 'Tendency test not activated'

DETECTION During the validation of the machine parameters.
CAUSE The tendency test of some axis or spindle is not activated. This situation should only

be allowed during setup; once the setup is completed, the tendency test must be
activated.

SOLUTION Activate the tendency test for the axes and spindles (parameter TENDENCY).

0075 'Wrong I/O configuration table'

DETECTION During the validation of the machine parameters.
CAUSE Parameters NDIMOD and NDOMOD must be the same as the number of inputs and

outputs detected by hardware.

SOLUTION Correct parameters NDIMOD and NDOMOD.

0076 'The sum of axes or spindles per channel exceeds the total number of axes or spindles'

DETECTION During the validation of the machine parameters.
CAUSE The value of parameter CHNAXIS is higher than the value of parameter NAXIS or

the value of parameter CHNSPDL is higher than the value of NSPDL.

SOLUTION Correct the machine parameters.

CNC 8070

(REF: 1308)

·10·

0077 'Axis or spindle assigned to more than one channel'

DETECTION During the validation of the machine parameters.
CAUSE There is an axis or spindle assigned to several channels.
SOLUTION Correct machine parameters CHAXISNAME and CHSPDLNAME n all the channels.

An axis or spindle can only belong to a channel or to none of them.

0078 'The master and slave axes must belong to the same channel'

DETECTION During the validation of the machine parameters.
CAUSE Some gantry axis is formed by axes of different channels.
SOLUTION Both axes of a gantry axis must belong to the same channel.

Error solving manual

0079 'A slave gantry axis cannot be parked'

DETECTION On CNC power-up or when validating the machine parameters.
CAUSE The CNC has detected that the slave axis of a gantry pair is parked; the PARKED

signal of the slave axis is active.

SOLUTION Unpark the axis or cancel the gantry axis.

0080 'To validate the axis, you must validate the GENERAL PARAMETERS table'

DETECTION During the validation of the machine parameters.
CAUSE The user has added an axis to the system (parameter NAXIS) and, without validating

the general parameters table, has tried to validate the parameter table of one of the
new axes.

SOLUTION Validate the general parameter table before validating the parameters of the axis.

0081 'The in-position zone cannot be smaller than the resolution of the axis'

DETECTION During the validation of the machine parameters.
CAUSE 'The in-position zone is smaller than the resolution of the axis.
SOLUTION Increase the in-position zone of the axis (parameter INPOSW).

0082 'Impossible leadscrew error or cross compensation table for all the ranges of the axis'

DETECTION During the validation of the machine parameters.
CAUSE In a compensation, the moving axis (parameter MOVAXIS) is rotary and it doesn't

have the same module limits in all the parameter sets.

SOLUTION Assign the same module limits (parameters MODUPLIM and MODLOWLIM) in all the

parameter sets.

0083 'The master and slave axes must be of the same type (DRIVETYPE)'

DETECTION During the validation of the machine parameters.
CAUSE The two axes of a gantry axis have different types of drives; analog or Sercos or

Mechatrolink.

SOLUTION The axes of a gantry pair must have the same type of drive (parameter DRIVETYPE).

0084 'An axis or spindle that cannot be swapped cannot be left unassigned to a channel'

DETECTION During the validation of the machine parameters.
CAUSE There is an axis or spindle without swapping permission that is not assigned to any

channel.

SOLUTION The axes or spindles that cannot be swapped (parameter AXISEXCH) must

necessarily be assigned to one channel.

0085 'There is no digital axis (sercos/Mechatrolink)'

DETECTION During the validation of the machine parameters.
CAUSE The OEM parameters table contains drive variables (DRV) but there are no digital

axes in the system (Sercos or Mechatrolink).

SOLUTION Eliminate the defined drive variables (DRV) or define the right digital axes.

0086 'It is not a digital axis (Sercos/Mechatrolink)'

DETECTION During the validation of the machine parameters.
CAUSE There is a drive variable (DRV) for an axis that is not digital (Sercos/Mechatrolink).
SOLUTION Eliminate the variable of that axis.

0087 'Too many DRV variables'

DETECTION During the validation of the machine parameters.
CAUSE There are too many drive variables (DRV) defined in the OEM parameters table.
SOLUTION The OEM parameters table can have up to 100 drive variables.

0088 'Trace of internal variables activated'

DETECTION During the validation of the machine parameters.
CAUSE The CNC is executing the trace of an internal variable.
SOLUTION Contact Fagor.

CNC 8070

(REF: 1308)

·11·

Error solving manual

0089 'It starts up with a single channel due to errors detected in machine parameters'

DETECTION During the validation of the machine parameters.
CAUSE Errors or warnings have come up while validating machine parameters related to the

axes or spindles of a channel. For example, a channel has an axis associated with
it, but it is not on the list of the system axes.

SOLUTION Being impossible to start up with the user configuration, the CNC starts up with the

default configuration. Correct the machine parameter settings to eliminate the rest
of errors and warnings. This warning is removed without having to change parameter
NCHANNEL (number of channels).

0090 'It starts up with the default axis configuration due to errors in machine parameters'

DETECTION During the validation of the machine parameters.
CAUSE Errors or warnings have come up while validating machine parameters related to the

axes or spindles of a channel. For example, the number of axes in the system is higher
than the number of axes defined in parameter AXISNAME.

SOLUTION Being impossible to start up with the user configuration, the CNC starts up with the

default configuration. Correct the machine parameter settings to eliminate the rest
of errors and warnings.

0091 'DRV variables having the same identifier (ID) cannot have different mnemonic'

DETECTION During the validation of the machine parameters.
CAUSE There are drive variables (DRV) in the OEM machine parameters with the same

Sercos identifier (ID) and different mnemonic.

SOLUTION DRV variables with the same identifier must have the same mnemonic.

0092 'DRV variables having the same identifier (ID) cannot have different MODE or TYPE'

DETECTION During the validation of the machine parameters.
CAUSE There are drive variables (DRV) in the OEM machine parameters with the same

identifier (ID) and different access type (synchronous or asynchronous) or different
access mode (read or write).

SOLUTION DRV variables with the same identifier must have the same type of access (parameter

TYPE) and the same access mode (parameter MODE).

0093 'DRV variables having the same name (MNEMONIC) cannot have different ID, MODE or

TYPE'

DETECTION During the validation of the machine parameters.
CAUSE There are drive variables in the OEM machine parameters with the same mnemonic

and different Sercos identifier (ID), different access type (synchronous or
asynchronous) or different access mode (read or write).

SOLUTION The DRV variables with the same mnemonic must have the same Sercos identifier

(parameter ID), the same type of access (parameter TYPE) and the same access
mode (parameter MODE).

0094 'Some channel must have parameter HIDDENCH = No'

DETECTION During the validation of the machine parameters.
CAUSE All the channels of the system are defined as hidden.
SOLUTION The CNC does not allow all the channels of the system to be hidden; some of them

must be visible (parameter HIDDENCH).

0095 'An axis cannot be MASTERAXIS of several Gantry pairs'

DETECTION During the validation of the machine parameters.
CAUSE There are two gantry axes with the same master axis.
SOLUTION Correct the configuration of the gantry axes.

CNC 8070

(REF: 1308)

·12·

0096 'A tandem axis must be velocity-Sercos'

DETECTION During the validation of the machine parameters.
CAUSE An axis of a tandem axis is not velocity-Sercos.
SOLUTION Both axes of a tandem axis must be velocity-Sercos.

Error solving manual

0097 'Tandem/gantry pair eliminated because they were preceded by an empty pair'

DETECTION During the validation of the machine parameters.
CAUSE The gantry or tandem pairs of axes do not occupy consecutive positions in their

tables; there is an empty space or undefined position in one of them.

SOLUTION Gantry or tandem pairs of axes must occupy consecutive positions in the tables. If

there is an empty space in the table, i.e. an unassigned position, the CNC cancels
the pairs defined behind it.

0098 'The AXISEXCH parameter of the master and slave axes have been set differently'

DETECTION During the validation of the machine parameters.
CAUSE There is a gantry o tandem pair whose master and slave axes have parameter

AXISEXCH set differently.

SOLUTION Assign the same value to parameter AXISEXCH of both axes.

0099 'The value of PROBEFEED is too high to brake applying DECEL and JERK'

DETECTION During the validation of the machine parameters.
CAUSE The maximum probing feedrate (parameter PROBEFEED) is higher than the feedrate

needed to brake within the distance set by PROBERANGE with the acceleration and
jerk values of the axis.

SOLUTION The value of this parameter must be smaller than the feedrate needed to brake within

the distance set by PROBERANGE with the acceleration and jerk values of the axis.
The warning window shows the maximum feedrate that may be reached.

0100 'Too many variables waiting to be reported'

DETECTION During execution.
CAUSE The number of variables modified at the CNC that must be reported to the interface

exceeds the maximum admitted.

SOLUTION If the error persists, contact your supplier.

0104 'Communication time out'

DETECTION During execution.
CAUSE The CNC does not end successfully the reading / writing of an external variable.
SOLUTION If the error persists, contact your supplier.

0105 'Parameters cannot be validated while executing a program'

DETECTION During execution.
CAUSE The user has tried to validate a machine parameter table while a part-program is in

execution or interrupted.

SOLUTION Wait for the program execution to finish or cancel the program execution in all the

channels.

0106 'Parameters cannot be validated Spindle or axis moving'

DETECTION During the validation of the machine parameters.
CAUSE The user has tried to validate a machine parameter table while a spindle or an axis

is moving. An axis may be moving as a result of a command of independent axis.

SOLUTION Stop the axis or spindle movement.

0107 'Error when registering DRV variables'

DETECTION During the validation of the machine parameters.
CAUSE The CNC has generated an error when trying to register the variables defined in the

OEM parameters table.

SOLUTION Contact Fagor.

0108 'Oscillo: The sampling time cannot be readjusted with the new LOOPTIME'

DETECTION During execution.
CAUSE The user has used the oscilloscope without validating a trace, has modified

parameter LOOPTIME and has validated the machine parameters.

SOLUTION The warning will no longer be displayed when the user executes a trace at the

oscilloscope. Setting the sampling period of a trace of the oscilloscope depends on
parameter LOOPTIME. In order for the CNC to be able to set this, it must have a
validated trace of the oscilloscope; i.e. the trace must have been executed at least
once.

CNC 8070

(REF: 1308)

·13·

Error solving manual

0109 'Parameters cannot be validated: spindle in synchronization'

DETECTION On CNC power-up or when validating the machine parameters or when compiling the

PLC program.

CAUSE The CNC does not admit this type of actions with active synchronized spindles

because they require a system reset.

SOLUTION The parameters must be validated or the PLC program must be compiled before

synchronizing the spindles or the spindles must be momentarily de-synchronized in
order to carry out the desired action.

0110 'The user kinematics could not be loaded'

DETECTION During CNC startup.
CAUSE The CNC does not show the file \windows\system32\drivers\kinematic.sys.
SOLUTION Checks that no errors come up when doing the make of the user kinematics and that

the kinematic.sys driver is generated correctly.

0111 'Error when initializing user kinematics data'

DETECTION During CNC startup.
CAUSE Error in the function for initializing and loading the user kinematics data

(UserTransforDataInit) implemented in the file Kin_iniData.c.

SOLUTION Check and correct the possible reasons why this function generates an error.

0112 'Error when initializing user kinematics'

DETECTION When activating a user kinematics.
CAUSE Error in the function for initializing the kinematics (UserTransforInit) implemented in

the file Kin_impl.c.

SOLUTION Check and correct the possible reasons why this function generates an error.

CNC 8070

0113 'Error when initializing user kinematics parameters'

DETECTION When activating a user kinematics.
CAUSE Error in the function for initializing the kinematics (UserTransforParamInit)

implemented in the file Kin_impl.c.

SOLUTION Check and correct the possible reasons why this function generates an error.

0150 'Too many open files'

DETECTION While executing a part-program with global subroutines.
CAUSE The number of open files (main program plus external subroutines) is greater than 20.
SOLUTION Decrease the number of external subroutines open in the part-program at the same

time.

0151 'Writing access denied'

DETECTION When accessing a file.
CAUSE The CNC has tried to write in a file that does not have a writing permission.
SOLUTION Give the file writing permission.

0152 'The file cannot be opened'

DETECTION When accessing a file.
CAUSE The CNC could not open a file for reading or writing. The file does not have the proper

permissions, is not accessible or is corrupt.

SOLUTION Check that the file exists and that it has the proper permissions for the action to be

carried out (read/write). If the file is corrupt, its data has been lost.

0153 'Reading access denied'

DETECTION When accessing a file.
CAUSE The CNC has tried to read a file that does not have a reading permission.
SOLUTION Give the file reading permission.

(REF: 1308)

·14·

0154 Protected program or routine'

DETECTION When accessing a file.
CAUSE The CNC has tried to read an encrypted file without having permission to read.
SOLUTION Contact the manufacturer of the machine to obtain the file encrypting codes.

Error solving manual

0160 'Axis/Set not available in the system'

DETECTION During execution.
CAUSE The possible causes are:

• The instruction #SET AX or #CALL AX is trying to add to a channel an axis that
does not exist or is in another channel.

• A parameter set that does not exist has been programmed in function G112.

SOLUTION Check the program. If the axis is in another channel, release it with the instruction

#FREE AX.

0165 'RT IT Overflow'

DETECTION During CNC operation.
CAUSE The real time interruptions exceed the allowed amount of time. Some possible causes

may be the installation of some device, driver or application that is incompatible with
the CNC.

SOLUTION If the error comes up often, it may be necessary to adjust the parameter LOOPTIME.

Analyze the cases where the error occurs and contact your supplier.

0166 'Jerk limit overshoot'

DETECTION During the execution of a part-program.
CAUSE The axis is exceeding its jerk limit.
SOLUTION Analyze the cases where it occurs and contact your machine manufacturer.

0167 'No RT IT'

DETECTION During CNC operation.
CAUSE The real time interruption does not kick in.
SOLUTION Restart the CNC. If the error persists, contact your supplier.

0168 'LR Overflow'

DETECTION During CNC operation.
CAUSE The position loop time of the Sercos axes exceeds the time allowed.
SOLUTION Adjust parameter LOOPTIME.

0169 'Safety temperature exceeded'

DETECTION During CNC operation.
CAUSE Unit integrity is at risk The CNC checks every minute the unit temperature; if in three

samples in a row the temperature exceeds 60 ºC (140 ºF), the CNC issues this
warning and activates the OVERTEMP mark. The temperature increase may be due
to a failure in the hardware cooling system or to excessive room temperature. This
warning shows the current temperature.

SOLUTION Respect the dimensions recommended for the enclosure minimum distance

recommended between the enclosure walls and the central unit. If necessary, install
fans for cooling the enclosure. If the error persists, turn the CNC off and contact the
Service Department.

0170 'Low battery voltage'

DETECTION During CNC power-up or after a reset.
CAUSE The CNC checks the battery voltage on start-up and at each reset. The battery is

discharged; its useful life cycle has ended.

SOLUTION Contact the manufacturer to replace the battery. When the CNC is turned off, the

battery keeps the necessary data for the CNC (for example, the position values).

0171 'LOOPTIME overflow'

DETECTION In CNCREADY conditions.
CAUSE The real time interruptions exceed the allowed amount of time.
SOLUTION If the error comes up often, it may be necessary to adjust the parameter LOOPTIME.

Analyze the cases where it occurs and contact your machine manufacturer.

CNC 8070

0172 'CPU fan stopped'

DETECTION During CNC operation.
CAUSE Unit over-temperature risk The CNC has detected that the CPU fan is stopped.

When the CPU has a fan, during regular operation of the CNC, it monitors and verifies
that the fan is running. This test is run every minute, same as the temperature watch.

SOLUTION If the error persists, contact the Service Department.

(REF: 1308)

·15·

Error solving manual

0173 '[Start] not allowed due to safety over-temperature'

DETECTION During CNC operation.
CAUSE Every time [START] is pressed, the CNC checks that the room temperature does not

exceed 65 ºC (149 ºF) and, if it does, inhibits the [START] while the error occurs. This
error shows the current temperature.

SOLUTION If the error persists, turn the CNC off and contact the Service Department.

0200 'Failure when requesting a VxD'

DETECTION When reading the battery status.
CAUSE The CNC cannot be connected with VcompciD.
SOLUTION Contact your supplier.

0201 'Mains failure. PC powered by a battery'

DETECTION When reading the battery status.
CAUSE There has been a CNC power failure and the emergency battery is powering the CNC.
SOLUTION Whether the mains failure is fortuitous or caused by the operator, let the CNC finish

its shut-down sequence. If the mains failure has been fortuitous, check the possible
causes.

CNC 8070

(REF: 1308)

·16·

Error solving manual

1000-1999

1000 'The function of instruction requires programming the axes'

DETECTION During execution.
CAUSE The axes affected by the programmed instruction or G function have not been

programmed.

SOLUTION Check the program.

1004 'Zero spindle speed'

DETECTION During execution.
CAUSE The speed of the spindle used with function G63 is zero.
SOLUTION Program a spindle speed.

1005 'Motion block with zero feed'

DETECTION During execution.
CAUSE No feedrate is active in the channel.
SOLUTION Program the feedrate F.

1006 'G20: spindle not allowed'

DETECTION During execution.
CAUSE Function G20 does not allow programming the spindle.
SOLUTION Check the program.

1007 'The programmed function requires a nonexistent main axis'

DETECTION During execution.
CAUSE The programmed function needs one or two main axes and they are missing in the

channel.

SOLUTION Check the program. Following functions G11, G12, G13 and G14 require one of the

two axes of the main plane. Functions G2, G3, G8, G9, G30, G36, G37, G38, G39,
G73 require both axes of the main plane. Both axes of the main plane are also needed
to activate collision detection (#CD) and for function G20 when collision detection is
active.

1008 'Coordinates out of range'

DETECTION During execution.
CAUSE The possible causes are:

• The coordinate programmed for the axis is too large.

• Function G101 tries to include an offset too large in the axis.

SOLUTION Check the program.

1009 'G4: the dwell has been programmed twice, directly and using K'

DETECTION During execution.
CAUSE The dwell has been programmed twice in the G4 function and in the same block,

directly with a number and with parameter K.

SOLUTION Program the dwell function G4 only once.

1010 'Program G4 K'

DETECTION During execution.
CAUSE The dwell time has not been programmed in function G4.
SOLUTION Program G4 as G4 <time> or G4K<time>, where <time> is the dwell time in seconds.

In both cases, the dwell must be programmed after G4.

1011 'G4: dwell out of range'

DETECTION During execution.
CAUSE The dwell time programmed in function G4 is too long.
SOLUTION The maximum value allowed for the dwell is 2147483646.

CNC 8070

(REF: 1308)

·17·

Error solving manual

1012 'G4: the dwell cannot be programmed using K'

DETECTION During execution.
CAUSE The letter K is associated with the third axis of the channel and in this case there is

no third axis.

SOLUTION If a third axis is not desired in the channel, the dwell may be programmed directly with

a number.

1013 'G4: the dwell cannot be negative'

DETECTION During execution.
CAUSE The dwell time programmed in function G4 is negative.
SOLUTION Program a value equal to or greater than 0.

1014 'It is no t possible to program in diameters with mirror image on the face axis'

DETECTION During execution.
CAUSE The face axis (parameter FACEAXIS) cannot have both the mirror image and

programming in diameters active at the same time.

SOLUTION Check the program.

1015 'Center coordinates out of range'

DETECTION During execution.
CAUSE One of the I, J, K values is too high for the center of the circular interpolation or for

the center of rotation of the coordinate system.

SOLUTION Program a smaller value.

1016 'Negative values cannot be used when programming an axis in diameters'

DETECTION During execution.
CAUSE Negative coordinates cannot be programmed in absolute coordinates (G90) while

programming in diameters is active (parameter DIAMPROG).

SOLUTION Programming in absolute coordinates and diameters does not admit negative

coordinates.

1017 'G198: negative software limit out of range'

DETECTION During execution.
CAUSE The value of the negative software limit is too high.
SOLUTION Check the program.

1018 'G199: positive software limit out of range'

DETECTION During execution.
CAUSE The value of the positive software limit is too high.
SOLUTION Check the program.

1019 'No measurement has been taken on the requested axis (axes)'

DETECTION During execution.
CAUSE Function G101 tries to include a measuring offset in an axis that was not involved in

the measurement or the offset has been canceled (G102).

SOLUTION To include a measuring offset (G101), the axis must have carried out a measurement.

1020 'Negative ramp time'

DETECTION During execution.
CAUSE The ramp time of function G132 is negative.
SOLUTION Program a value equal to or greater than 0.

CNC 8070

(REF: 1308)

·18·

1021 'Ramp time out of range'

DETECTION During execution.
CAUSE The ramp time of function G132 is too long.
SOLUTION Check the program.

1022 'Percentage of Feed-Forward out of range'

DETECTION During execution.
CAUSE The percentage of feed forward (G134) or AC forward (G135) is too high.
SOLUTION The percentage of feed forward or AC forward must be greater than zero and smaller

than 120.

Error solving manual

1023 'Wrong set number

DETECTION During execution.
CAUSE The set number of the axis is wrong.
SOLUTION The set programmed for the axis must be greater than zero and smaller than or equal

to machine parameter NPARSETS of the axis.

1024 'Set number out of range'

DETECTION During execution.
CAUSE The set number of the axis is too high.
.SOLUTION The set programmed for the axis must be greater than zero and smaller than or equal

to machine parameter NPARSETS of the axis.

1025 'Programmed distance equal to zero'

DETECTION During execution.
CAUSE Null movement in the G63 block.
SOLUTION Check the program.

1026 'Wrong circular path with the programmed radius'

DETECTION During execution.
CAUSE The radius for the circular interpolation is too small.
SOLUTION Check the program.

1027 'The starting point and the end point of the circular path are the same (infinite solutions)'

DETECTION During execution.
CAUSE Zero radius for the circular interpolation; there are infinite solutions.
SOLUTION Check the program.

1028 'The difference between the programmed center and the calculated one is too large'

DETECTION During execution.
CAUSE In a circular interpolation with function 265 active, the difference between the initial

radius and the final one exceeds the values of machine parameters CIRINERR and
CIRINFACT.

SOLUTION Check the program.

1029 'Zero radius on circular path'

DETECTION During execution.
CAUSE The possible causes are:

• Zero radius in a circular interpolation.

• Being function G265 active, the CNC calculates a zero radius based on the center
coordinates programmed in the circular interpolation.

• Function G264 being active, both center coordinates are zero.

SOLUTION The radius of a circular interpolation cannot be zero. Both coordinates of the center

of a circular interpolation cannot be zero.

1030 '#AXIS programmed without G200/G201/202'

DETECTION During execution.
CAUSE G200, G201 or G202 are missing in the block of the #AXIS instruction.
SOLUTION Check the program.

1031 '#AXIS expected'

DETECTION During execution.
CAUSE The #AXIS instruction is missing in the block of function G201.
SOLUTION Check the program.

1032 'Spindle position missing for M19'

DETECTION During execution.
CAUSE The spindle position is missing in the block of function M19.
SOLUTION Check the program.

1035 '#SLOPE: parameter out of range'

DETECTION During execution.
CAUSE The value of some parameter of the #SLOPE instruction is too high.
SOLUTION Program smaller values.

CNC 8070

(REF: 1308)

·19·

Error solving manual

1037 'Center coordinates ignored with G0/G1/G100/G63 active'

DETECTION During execution.
CAUSE The CNC has found parameters I, J, K with function G0, G1, G100 or G63 active. The

CNC ignores these parameters.

SOLUTION These functions do not need these parameters.

1038 'Radius compensation cannot be active while measuring'

DETECTION During execution.
CAUSE The CNC tries to execute G100 while tool radius compensation is active (G41/G42).
SOLUTION Check the program.

1039 'There is a previous measurement value for the axis (axes)'

DETECTION During execution.
CAUSE The CNC tries to carry out a measurement (G100) on an axis that has a previous

measuring offset.

SOLUTION Use function G102 to cancel the measuring offset included in the axis.

1040 'Home search not allowed on an axis in G201'

DETECTION During execution.
CAUSE The CNC cannot be home an axis that is in additive manual mode (G201).
SOLUTION Use function G202 to cancel the additive manual mode of the axis in order to home

it. After the home search, activate the additive manual mode (G201) again.

1041 'Corrected circular path center out of range'

DETECTION During execution.
CAUSE In a circular interpolation programmed either with a radius and the coordinates of the

end point or with the coordinates of the middle point, end point and having function
G265 active.

The coordinates of the center of the inter polation calculated by the CNC are too large.
The coordinates programmed for the center, middle point or the radius are too large.

SOLUTION Check the program.

1043 'The third axis of the plane cannot be the same as the first or the second one'

DETECTION During execution.
CAUSE Parameter 5 of function G20 (plane change) is the same as 1 or 2.
SOLUTION If the longitudinal axis of the tool (parameter 3) is the same as the first or second axis

of the plane (parameters 1 and 2), the third axis must be programmed with parameter

5. This parameter must not coincide with the first one or with the second one.

1044 'The first and second axis of the plane cannot be the same'

DETECTION During execution.
CAUSE In function G20 (plane change), the first (parameter 1) and the second (parameter

2) axes of the plane are the same axis.

SOLUTION Check the program.

1045 'The first axis of the plane has been programmed wrong'

DETECTION During execution.
CAUSE In function G20 (plane change) the first axis of the plane (parameter 1) is wrong.
SOLUTION The first axis of the plane must be one of the first three axes of the channel.

CNC 8070

(REF: 1308)

·20·

1046 'The second axis of the plane has been programmed wrong'

DETECTION During execution.
CAUSE Using function G20 (plane change) the second axis of the plane (parameter 2) is

wrong.

SOLUTION The second axis of the plane must be one of the first three axes of the channel.

1047 'A third axis is required for the plane (index 5) '

DETECTION During execution.
CAUSE In function G20 (plane change) the third axis of the plane is missing or is wrong.
SOLUTION If the longitudinal axis of the tool (parameter 3) is the same as the first or second axis

of the plane (parameters 1 and 2), the third axis must be programmed with parameter

5. The parameter must neither coincide with the first or with the second one and must
be one of the first three axes of the channel.

Error solving manual

1048 'Tool length compensation with radius out of range'

DETECTION During execution.
CAUSE The tool dimensions exceed the maximum values.
SOLUTION Modify the tool dimensions.

1049 'Face axis (FACEAXIS) defined twice in the active plane'

DETECTION During execution.
CAUSE It informs that the two axes of the main plane are face axes (parameter FACEAXIS).
SOLUTION There can only be one face axis in the work plane.

1050 'Considering the tool offsets, it exceeds the data range'

DETECTION During execution.
CAUSE The tool dimensions exceed the maximum values.
SOLUTION Modify the tool dimensions.

1051 'The axis does not exist or is not available in the channel'

DETECTION During execution.
CAUSE The possible causes are:

• The CNC has tried to execute an independent movement in a spindle.

• The axis programmed in a variable is not available.

SOLUTION Check the program. In order to be able to interpolate the spindle as independent axis,

it must be active as C axis.

1052 'Values resulting from the measurement out of range'

DETECTION During execution.
CAUSE The CNC has carried out a measurement with function G100 and the coordinate or

offset obtained is too large.

SOLUTION The value obtained in that probing move must be between -2147483647 and

2147483646.

1054 'Nonexistent fixture'

DETECTION During execution.
CAUSE The programmed fixture (clamp) number does not exist.
SOLUTION The fixture (clamp) number must be a value between 0 and 10.

1055 'D and the tool radius cannot be modified in the same block'

DETECTION During execution.
CAUSE The CNC does not allow modifying the tool radius (variable: (V.)G.TOR) or

programming a tool change and/or tool offset in the same block.

SOLUTION Program both instructions in different blocks.

1056 'Too many external variables'

DETECTION During execution.
CAUSE The CNC has reached the maximum number of external variables.
SOLUTION Check the program. The CNC admits up to 500 external variables.

1057 'Variable without reading permission'

DETECTION During execution.
CAUSE The CNC has tried to read, via part-program or MDI, a variable that does not have

reading permission via program.

SOLUTION The variable cannot be read from a part-program or MDI. Refer to the documentation

on permissions of the variable.

1058 'User variable not initialized'

DETECTION During execution.
CAUSE The user variable V.P.name or V.S.name has not been defined.
SOLUTION Check the program. Define the variable properly.

1059 'Variable without writing permission'

DETECTION During execution.
CAUSE The CNC has tried to write, via part-program or MDI, a variable that does not have

writing permission via program.

SOLUTION The variable cannot be written from a part-program or MDI. Refer to the

documentation on permissions of the variable.

CNC 8070

(REF: 1308)

·21·

Error solving manual

1060 'N label value out of range'

DETECTION During execution.
CAUSE Invalid block number "N".
SOLUTION The block number must be a positive value lower than 2147483646.

1061 'Nonexistent G function'

DETECTION During execution.
CAUSE The programmed G function does not exist.
SOLUTION Check the program.

1062 'Incompatible G functions'

DETECTION During execution.
CAUSE Two G functions incompatible with each other have been programmed in the block.
SOLUTION Program the functions in different blocks.

1063 'Incompatible G functions (G108/G109/G193)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1064 'Incompatible G functions (G196/G197)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

CNC 8070

1065 'Incompatible G functions (G17/G18/G19/G20)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1066 'Incompatible G functions (G136/G137)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1067 'Incompatible G functions (G40/G41/G42)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1068 'Incompatible G functions (G151/G152)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1069 'Incompatible G functions (G54-G59/G159)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

(REF: 1308)

·22·

1070 'Incompatible G functions (G5/G7/G50/G60/G61)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

Error solving manual

1071 'Incompatible G functions (G70/G71)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1072 'Incompatible G functions (G80-G88/G160-G166/G281-G286/G287-G297)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1073 'Incompatible G functions (G90/G91)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1074 'Incompatible G functions (G93/G94/G95)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1075 'Incompatible G functions (G96/G97/G192)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1076 'Incompatible G functions (G100/G101/G102)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1077 'Incompatible G functions (G115/G116/G117)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1078 'Incompatible G functions (G134/G135)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1079 'Incompatible G functions (G138/G139)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1080 'Incompatible G functions (G6/G261/G262)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

CNC 8070

(REF: 1308)

·23·

Error solving manual

1081 'Incompatible G functions (G264/G265)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1082 'Incompatible G functions (G200/G201/G202)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1083 'Incompatible G functions (G36/G37/G38/G39)'

DETECTION During execution.
CAUSE Two or more G functions incompatible with each other have been programmed in the

block.

SOLUTION Program the functions in different blocks.

1084 'Plane change not allowed while tool radius compensation is active'

DETECTION During execution.
CAUSE The CNC has tried to change the work plane or the axes that make up the plane, while

tool radius was active.

SOLUTION Cancel the compensation to define the new work plane.

1085 'G41/G42 not allowed if the first or second axis of the active plane is missing'

DETECTION During execution.
CAUSE Tool radius compensation is impossible if one of the two axes of the active plane is

missing in the channel.

SOLUTION Define the work plane. If the channel has yielded its axes to other channels, recover

the missing axis using the instruction #CALL AX or #SET AX.

1087 '"=" expected'

DETECTION During execution.
CAUSE Wrong syntax of the programmed instruction or function.
SOLUTION Check the program.

1088 'Wrong offset number'

DETECTION During execution.
CAUSE In function G159, the programmed zero offset does not exist.
SOLUTION Check the program.

1089 'Incompatible M functions (M3/M4/M5/M19)'

DETECTION During execution.
CAUSE Two or more M functions incompatible with each other have been programmed for

the same spindle in the block.

SOLUTION Program the M functions of the same spindle in different blocks.

1090 'Nonexistent H function'

DETECTION During execution.
CAUSE The H function does not exist.
SOLUTION The function number must be between 1 and 65534.

CNC 8070

(REF: 1308)

·24·

1091 'T function programmed twice'

DETECTION During execution.
CAUSE More than one T function have been programmed in the same block.
SOLUTION Each block can only contain one T function. Program both functions in different

blocks.

1093 'D function programmed twice'

DETECTION During execution.
CAUSE More than one D function have been programmed in the same block.
SOLUTION Each block can only contain one D function. Program both functions in different

blocks.

Error solving manual

1094 'F feedrate programmed twice'

DETECTION During execution.
CAUSE More than one F function have been programmed in the same block.
SOLUTION Each block can only contain one F function. Program both functions in different

blocks.

1095 'Feedrate F cannot be negative or zero'

DETECTION During execution.
CAUSE The feedrate (F) must be positive and other than zero.
SOLUTION Check the program.

1096 'The feedrate cannot be programmed with E'

DETECTION During execution.
CAUSE The feedrate has been programmed with the E function.
SOLUTION Program the feedrate with the F function.

1097 'Unknown spindle name'

DETECTION During execution.
CAUSE The spindle name is not valid, the spindle does not exist in the system or the spindle

does not belong to the channel.

SOLUTION The valid names for the spindle are S, S1, ..., S9. The spindle programmed to in the

block must exist in the system configuration and depending on which instruction it
is, also in the channel configuration. A channel can only control its spindles.

1098 'S speed programmed twice'

DETECTION During execution.
CAUSE There are two or more S functions programmed for the same spindle in the same

block.

SOLUTION There can only be one speed for each spindle in the same block.

1100 'Parameter index out of range'

DETECTION During execution.
CAUSE The arithmetic parameter does not exist; it is not within the range admitted by the

machine parameters.

SOLUTION Check the program. Check the valid arithmetic parameter range in the machine

parameters.

Machine parameters. Valid range.

MINLOCP - MAXLOCP Local arithmetic parameters.

MINGLBP - MAXGLBP Global arithmetic parameters.

MINCOMP - MAXCOMP Common arithmetic parameters.

1101 '#SET IPOPOS instruction programmed wrong'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1102 'The index for R cannot be other than 1'

DETECTION During execution.
CAUSE The radius can only be programmed with R or R1.
SOLUTION Check the program.

1103 'Nonexistent O function'

DETECTION During execution.
CAUSE The O function does not exist.
SOLUTION Check the program.

1104 'The "%" character is not allowed inside the main program'

DETECTION During execution.
CAUSE The "%" character can only be used as first character in the definition of the name

of the main program or of a local subroutine.

SOLUTION Remove this character from the program.

CNC 8070

(REF: 1308)

·25·

Error solving manual

1105 'Assignment operator expected'

DETECTION During execution.
CAUSE No assignment operator has been programmed after the variable or parameter.
SOLUTION The valid assignment operators are "=", "+=", "-=", "*=", "/=".

1106 '"]" expected'

DETECTION During execution.
CAUSE The closing bracket "]" is missing in the programmed expression or instruction.
SOLUTION Check the program.

1107 'The axis does not exist or is not available'

DETECTION During execution.
CAUSE The CNC tries to move an axis that does not exist or is not available in the system

or in the channel. The axis programmed in an instruction or variable does not exist
in the system or in the channel.

SOLUTION Verify that the programmed axis exists in the channel and that it is available (is not

parked).

1108 'Axis programmed twice'

DETECTION During execution.
CAUSE In one of the following functions, an axis has been programmed more than once.

• Axis movement in G0, G1, G2, G3, G8 or G9.

• Threading G33 or G63.

• Instructions #FACE or #CYL.

• Plane selection, G20.

With functions that imply axis movements, programming an axis twice may be
because the axis has been programmed in both Cartesian and Polar coordinates.

SOLUTION Check the program.

CNC 8070

1109 'Wrong axis index'

DETECTION During execution.
CAUSE In functions G20 and G74, the index programmed with the axis name is wrong.
SOLUTION The axis index must be between 1 and the maximum number of axes of the system

or channel.

1110 'Values for I, J, K programmed twice'

DETECTION During execution.
CAUSE One of parameters I, J, K has been programmed more than once in the same block.
SOLUTION Check the program.

1111 'Control instructions $ must be programmed alone in the block'

DETECTION During execution.
CAUSE An instruction has not been programmed alone in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added. The only exception is to program $IF and $GOTO in
the same block.

1112 'The $IF instruction <condition> can only be followed by $GOTO'

DETECTION During execution.
CAUSE The instruction is not programmed alone in the block and the additional information

is not a $GOTO.

SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added. The only exception is to program $IF and $GOTO in
the same block.

(REF: 1308)

·26·

1113 '$ELSE not expected'

DETECTION During execution.
CAUSE The CNC has detected an $ELSE instruction without a previous $IF instruction.
SOLUTION Check the program.

1114 'The $ELSE instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

Error solving manual

1115 '$ELSEIF not expected'

DETECTION During execution.
CAUSE The CNC has detected an $ELSEIF instruction without a previous $IF instruction.
SOLUTION Check the program.

1116 'The $ELSEIF <condition> instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1117 '$ENDIF not expected'

DETECTION During execution.
CAUSE The CNC has detected an $ENDIF instruction without a previous $IF instruction.
SOLUTION Check the program.

1118 'The $ENDIF instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1119 'The $SWITCH <expression> instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1120 '$CASE not expected'

DETECTION During execution.
CAUSE The CNC has detected an $CASE instruction without a previous $SWITCH

instruction.

SOLUTION Check the program.

1121 'The $CASE <expression> instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1122 '$DEFAULT not expected'

DETECTION During execution.
CAUSE The CNC has detected a $DEFAULT instruction without a previous $SWITCH

instruction.

SOLUTION Check the program.

1123 'The $DEFAULT instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1124 '$ENDSWITCH not expected'

DETECTION During execution.
CAUSE The CNC has detected an $ENDSWITCH instruction without a previous $SWITCH

instruction.

SOLUTION Check the program.

1125 'The $ENDSWITCH instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1126 '$FOR: invalid counter variable'

DETECTION During execution.
CAUSE The counter of the $FOR instruction is not valid.
SOLUTION The counter of the $FOR instruction may be a variable or an arithmetic parameter.

CNC 8070

(REF: 1308)

·27·

Error solving manual

1127 'The $FOR instruction<condition> instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1128 '$FOR: too many characters in the condition'

DETECTION During execution.
CAUSE The block that contains the $FOR instruction has more than 5100 characters.
SOLUTION Write the block that contains the $FOR instruction shorter.

1129 '$ENDFOR not expected'

DETECTION During execution.
CAUSE The CNC has detected an $ENDFOR instruction without a previous $FOR

instruction.

SOLUTION Check the program.

1130 'The $ENDFOR instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1131 'The $WHILE <condition> instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1132 '$WHILE: too many characters in the condition'

DETECTION During execution.
CAUSE The condition of the $WHILE instruction exceeds the maximum number of characters

allowed.

SOLUTION The maximum number of characters allowed is 5000.

1133 '$ENDWHILE not expected'

DETECTION During execution.
CAUSE The CNC has detected an $ENDWHILE instruction without a previous $WHILE

instruction.

SOLUTION Check the program.

1134 'The $ENDWHILE instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1135 'The $DO instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1136 '$ENDDO not expected'

DETECTION During execution.
CAUSE The CNC has detected an $ENDDO instruction without a previous $DO instruction.
SOLUTION Check the program.

CNC 8070

(REF: 1308)

·28·

1137 'The $ENDDO <expression> instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1138 'The $BREAK instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

Error solving manual

1139 '$BREAK not expected'

DETECTION During execution.
CAUSE The CNC has detected a $BREAK instruction, but there is no open control loop; $IF,

$ELSE, $FOR, $WHILE, $DO or $CASE.

SOLUTION Check the program. The CNC uses the $BREAK instruction is used to end a $CASE

or to exit from an $IF, $ELSE, $WHILE, $FOR or $DO loop before it ends.

1140 '$CONTINUE not expected'

DETECTION During execution.
CAUSE The CNC has detected a $CONTINUE instruction, but there is no open control loop;

$FOR, $WHILE or $DO.

SOLUTION Check the program. The CNC uses the $CONTINUE instruction to return to the

starting point of a $FOR, $WHILE or $DO loop.

1141 'The $CONTINUE instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1142 'The #TIME instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1146 'The path before a G37 must be linear'

DETECTION During execution.
CAUSE The motion block before the tangential entry is not linear.
SOLUTION Check the program.

1147 'The path after a G38 must be linear'

DETECTION During execution.
CAUSE The motion block after the tangential exit is not linear.
SOLUTION Check the program.

1149 'The programmed G36/G37/G38/G39 cannot be executed'

DETECTION During execution.
CAUSE The CNC cannot create the blending tool path with the programmed radius.
SOLUTION Check the programmed radius. Check that the joint is actually possible between the

first and the last block.

1150 'Functions G36/G37/G38/G39 must be followed by a motion block'

DETECTION During execution.
CAUSE The CNC does not have a second motion block for generating the joining tool path

(blend).

SOLUTION Do not program any block between the G function that defines the joining path and

the second motion block.

1151 'Functions G8/G36/G37/G38/G39 must be preceded by a motion block'

DETECTION During execution.
CAUSE The CNC does not have a first motion block for generating the joining tool path (blend).
SOLUTION Do not program any block between the G function that defines the joining path and

the first motion block.

1152 'Too many nested subroutines'

DETECTION During execution.
CAUSE The has exceeded the maximum number of nesting levels.
SOLUTION Correct the program decreasing the number of calls to subroutines (local and global)

that imply a new nesting level. The CNC admits up to 20 nesting levels.

1153 'Too many local subroutines defined in the program'

DETECTION During execution.
CAUSE The program has more local subroutines than admitted by the CNC.
SOLUTION Use fewer local subroutines; group several subroutines in one or use global

subroutines. The CNC admits 100 local subroutines per program.

CNC 8070

(REF: 1308)

·29·

Error solving manual

1154 'File name too long'

DETECTION During execution.
CAUSE The file name has too many characters. The name of a program or subroutine may

have a maximum of 63 characters and the path 120. When programming the name
of a program or subroutine with the path, the maximum number of characters will be
the sum of both values.

SOLUTION Decrease the number of characters of the name of the program or subroutine.

Change the location of the program or subroutine to reduce the number of characters
of the path.

1155 'No access to the file'

DETECTION During execution.
CAUSE The CNC cannot access the program or subroutine.
SOLUTION Check that the files are valid and are not corrupted. When calling subroutines, check

that the name and the path are correct. If the path is not defined in the call to the
subroutine, the CNC will apply the default search criterion (see the programming
manual).

1156 'Main program not found'

DETECTION During execution.
CAUSE The CNC cannot find the main program.
SOLUTION In a program with local subroutines, the main program must have a name (%name).

1157 'Global subroutine not found'

DETECTION During execution.
CAUSE The CNC cannot find the global subroutine.
SOLUTION Check that the name and the path of the subroutine are correct. If the path is not

defined in the call to the subroutine, the CNC will apply the default search criterion
(see the programming manual).

CNC 8070

(REF: 1308)

1159 'Name of the local subroutine too long'

DETECTION During execution.
CAUSE The subroutine name has too many characters. The name of a subroutine may have

a maximum of 63 characters.

SOLUTION Check the program.

1160 'Local subroutine not found'

DETECTION During execution.
CAUSE The CNC cannot find the local subroutine.
SOLUTION Check the name of the local subroutine in the calling block is the same as the name

that appears in its definition. The local subroutines must be defined at the beginning
of the program.

1161 '$ control blocks open'

DETECTION During execution.
CAUSE The CNC has found a "$" control block that does not have its corresponding closing

instruction.

SOLUTION Check the program.

1162 'M17/M29/#RET not expected'

DETECTION During execution.
CAUSE The CNC has detected an M17, M29 function or #RET as end of program.
SOLUTION Program M30/M02 as the end of the main program. If the error persists, check that

all the local subroutines end with M17, M29 or #RET.

1163 'M30/M02 not expected'

DETECTION During execution.
CAUSE The CNC has detected an M02 or M30 function as end of program.
SOLUTION Check that all the local and global subroutines end with M17, M29 or #RET.

1164 'Unknown term in mathematical expression'

DETECTION During execution.
CAUSE The mathematical expression is wrong.
SOLUTION Check all the terms of the expression; variables, parameters, operators, etc.

·30·

Error solving manual

1165 'Nonexistent variable'

DETECTION During execution.
CAUSE The possible causes are:

• The requested variable does not exist.

• Syntax error in the name of the variable.

• The variable is an array and the array index has not been indicated.

• A general variable has been requested for a particular axis or the other way
around.

SOLUTION Check the program.

1166 'Square root of a negative number'

DETECTION During execution.
CAUSE The mathematical expression contains a square root (SQRT) of a negative number.
SOLUTION Check the program.

1167 'Logarithm of a negative number or zero'

DETECTION During execution.
CAUSE The mathematical expression contains a logarithm (LOG/LN) of a negative number

or zero.

SOLUTION Check the program.

1168 'Variable index out of range'

DETECTION During execution.
CAUSE One of the indexes defined in the array variable is wrong.
SOLUTION The minimum admissible index for an array variable is 1 and the maximum depends

on which variable it is. There are particular instances where the index 0 is admitted:
G.GS, G.MS, G.LUP1 to G.LUP7, G.LUPACT and MTB.P.

1170 'The #SYNC POS instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1171 '# instructions must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added. The only exception is the #AXIS instruction that must
be programmed in the same block as function G201.

1172 'Instruction not allowed while tool radius compensation is active'

DETECTION During execution.
CAUSE The CNC has tried to execute an instruction that is incompatible with tool radius

compensation.

SOLUTION Cancel tool radius compensation to execute the instruction.

1173 'The #UNLINK instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1174 '#LINK: a new coupling (slaving) cannot be defined if a previous one is active'

DETECTION During execution.
CAUSE The CNC has tried to activate a second axis coupling (slaving ) without deactivating

the first one.

SOLUTION Check the program. Cancel the first coupling (slaving) before activating the second

one. To have both couplings, cancel the first one and activate both with a single #LINK
instruction.

1175 '#LINK: no coupling (slaving) has been defined'

DETECTION During execution.
CAUSE No axis coupling (slaving) has been defined in the #LINK instruction.
SOLUTION Program the master and slave axes in the #LINK instruction.

CNC 8070

(REF: 1308)

·31·

Error solving manual

1176 '#LINK: the master axis does not belong to the current axis configuration'

DETECTION During execution.
CAUSE The possible causes are:

• The master axis of the coupling does not exist or is not available in the channel.

• The CNC has tried to deactivate a coupling whose master axis does not exist or
is not available in the channel.

SOLUTION The master and slave axes must exist in the channel that executes the instruction.

1177 '#LINK: the slave axis does not belong to the current axis configuration'

DETECTION During execution.
CAUSE The possible causes are:

• The slave axis of the coupling does not exist or is not available in the channel.

• The CNC has tried to deactivate a coupling whose slave axis does not exist or
is not available in the channel.

SOLUTION The master and slave axes must exist in the channel that executes the instruction.

1178 '#LINK: the slave axis cannot be an axis of the main plane'

DETECTION During execution.
CAUSE The slave axis of the coupling is one of the main three axes.
SOLUTION Check the program.

1179 '#LINK: The master and slave axes must be of the same type (AXISTYPE)'

DETECTION During execution.
CAUSE The master and slave axes of the coupling are not of the same type, linear or rotary.
SOLUTION Both axes of the coupling must be of the same type (parameter AXISTYPE).

1180 '#LINK: The master and slave axes must have the same mode (AXISMODE)'

DETECTION During execution.
CAUSE The master and slave axes of the coupling are rotary, but they are not of the same

type, linearlike or module.

SOLUTION Both axes of the coupling must be of the same type (parameter AXISMODE).

1181 '#LINK: An axis active in G201 cannot be defined as slave'

DETECTION During execution.
CAUSE The slave axis of the coupling is active in additive manual mode (G201).
SOLUTION Cancel the additive manual mode in order to be able to couple the axis.

1182 '#LINK: too many couplings programmed'

DETECTION During execution.
CAUSE Too many couplings have been defined.
SOLUTION The maximum number of couplings that may be active in a channel is equal to the

number of axes of the channel minus three.

1183 'The #LINK instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1184 '#LINK: The master and slave axes are the same'

DETECTION During execution.
CAUSE The master and slave axes of the coupling are the same axis.
SOLUTION The master and slave axes must be different.

CNC 8070

(REF: 1308)

·32·

1185 '#LINK: An axis cannot be a slave of several masters'

DETECTION During execution.
CAUSE An axis is the slave of several masters.
SOLUTION An axis can only be the slave of one master.

1186 ''#LINK: A master axis cannot be a slave in another coupling and vice versa'

DETECTION During execution.
CAUSE An axis cannot be the slave in a coupling and the master in another.
SOLUTION An axis cannot be the master in a coupling and the slave in another.

Error solving manual

1187 '#AXIS: repeated axis name'

DETECTION During execution.
CAUSE The same axis has been programmed more than once in the instruction.
SOLUTION Check the program.

1188 '"["not expected'

DETECTION During execution.
CAUSE Syntax error in the instruction.
SOLUTION Check the program.

1189 '#MPG: too many parameters'

DETECTION During execution.
CAUSE The instruction has too many parameters.
SOLUTION The #MPG instruction admits a maximum of three parameters. Each one of them

represents the distance moved per handwheel pulse in each position of the switch.

1190 '#MPG: Negative or zero handwheel resolutions are not allowed'

DETECTION During execution.
CAUSE The #MPG instruction tries to define a negative or zero handwheel resolution.
SOLUTION The movement distance per handwheel pulse must be positive and other than zero.

1191 '#INCJOG: Negative or zero incremental jog distances are not allowed'

DETECTION During execution.
CAUSE The #INCJOG instruction tries to define a negative or zero distance.
SOLUTION The value of the incremental movement of the axis in each position of the switch must

be a positive value and other than zero.

1192 '#INCJOG: Negative or zero incremental jog feedrates are not allowed'

DETECTION During execution.
CAUSE The #INCJOG instruction tries to define a negative or zero feedrate.
SOLUTION The feedrate of the axis in each position of the switch must be a positive value and

other than zero.

1193 '#CONTJOG/#INCJOG: programmed feedrate out of range'

DETECTION During execution.
CAUSE The programmed feedrate is too high.
SOLUTION Check the program.

1194 '#INCJOG: too many parameters'

DETECTION During execution.
CAUSE The instruction has too many parameters.
SOLUTION The #INCJOG instruction admits a maximum of five groups of parameters. Each of

them represents the axis feedrate and movement for each position of the switch in
incremental jog.

1195 '#CONTJOG: too many parameters'

DETECTION During execution.
CAUSE The instruction has too many parameters.
SOLUTION The #CONTJOG instruction only admits one parameter that represents the axis

feedrate when the switch is in continuous jog.

1196 '#CONTJOG: Negative or zero continuous jog feedrates are not allowed'

DETECTION During execution.
CAUSE The #CONTJOG instruction tries to define a negative or zero feedrate.
SOLUTION The value of the axis feedrate must be a positive value and other than zero.

CNC 8070

1197 '#SET OFFSET: positive lower offset'

DETECTION During execution.
CAUSE The lower axis travel limit for jogging has a positive value.
SOLUTION The lower axis travel limit for jogging must be negative or zero.

(REF: 1308)

·33·

Error solving manual

1198 '#SET OFFSET: negative limit out of range'

DETECTION During execution.
CAUSE The value of the lower travel limit is too low.
SOLUTION Check the program.

1199 '#SET OFFSET: negative upper offset'

DETECTION During execution.
CAUSE The upper axis travel limit for jogging has a negative value.
SOLUTION The upper axis travel limit for jogging must be positive or zero.

1200 '#SET OFFSET: positive limit out of range'

DETECTION During execution.
CAUSE The value of the upper travel limit is too high.
SOLUTION Check the program.

1201 '#SET OFFSET: zero upper and lower offsets'

DETECTION During execution.
CAUSE The values of the lower axis travel limits for jogging are zero.
SOLUTION Check the program.

1203 'The #SET IPOPOS instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1204 'Nonexistent instruction or programmed wrong'

DETECTION During execution.
CAUSE The instruction does not exist or is programmed wrong.
SOLUTION Check the program.

1205 '#CALL AX/#SET AX: unknown offset type'

DETECTION During execution.
CAUSE The type of offset programmed in the instruction does not exist.
SOLUTION The valid offset types are ALL, LOCOF, FIXOF, TOOLOF, ORGOF, MEASOF,

MANOF.

1206 '"," expected'

DETECTION During execution.
CAUSE "," missing in the instruction or function.
SOLUTION Check the program.

1209 'Axis index out of range'

DETECTION During execution.
CAUSE The possible causes are:

• In instructions #CALL AX/#SET AX the position for some axis is wrong; the
position is taken, the position exceeds the maximum admitted or there is no room
for the axis.

• The axis name has been programmed with the wrong wild character.

SOLUTION The possible solutions are:

• The instruction can place the axes in any unoccupied position between 1 and a
number equal to the total number of axes plus spindles of the system.

• The possible wild characters are @1 to @6 and @SM.

CNC 8070

(REF: 1308)

·34·

1210 '#CALL AX/#SET AX: repeated axis name'

DETECTION During execution.
CAUSE The same axis has been programmed more than once in the instruction.
SOLUTION Check the program.

1211 '#CALL AX/#SET AX: repeated axis index'

DETECTION During execution.
CAUSE Two axes try to occupy the same position in the channel.
SOLUTION Check the program.

Error solving manual

1213 '#CALL AX/#SET AX: not allowed when G63 is active'

DETECTION During execution.
CAUSE #CALL AX cannot be programmed if function G63 is active.
SOLUTION Deactivate the threading G63 before modifying the configuration of the axes.

1214 '#CALL AX/#SET AX: too many axes required'

DETECTION During execution.
CAUSE Too many axes programmed; the number of axes exceeds the number of axes of the

system.

SOLUTION Check the configuration of the axes of a channel The number of axes of a channel

cannot exceed the number of axes of the system.

1215 'The #CALL AX/#SET AX instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1216 '#CALL AX/#CAX: axis name being used'

DETECTION During execution.
CAUSE The name of one of the axes is being used by a C axis.
SOLUTION Check the program.

1217 '#CALL AX: index being used'

DETECTION During execution.
CAUSE One of the positions is occupied by another axis.
SOLUTION Check the configuration of the axes defined for the channel, two axes cannot be in

the same position. An axis can use any free position between 1 and a number equal
to the maximum number of axes plus the maximum number of spindles allowed by
the system.

1218 'The #FREE AX instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1219 '"," or "]" expected'

DETECTION During execution.
CAUSE Syntax error in the instruction.
SOLUTION Check the program.

1220 '#FREE AX: an active axis cannot be eliminated in manual mode'

DETECTION During execution.
CAUSE An axis in additive manual mode G201 cannot be eliminated from the channel.
SOLUTION Use function G202 to cancel the additive manual mode of the axis in order remove

the axis from the channel.

1221 'The #SET AX instruction must be programmed alone in the block'

DETECTION During execution.
CAUSE The instruction has not been programmed alone in the block.
SOLUTION Check the program.

1222 '#COMMENT END not expected'

DETECTION During execution.
CAUSE There is an end-of-comment block (#COMMENT END), but the open-comment block

(#COMMENT BEGIN) is missing.

SOLUTION Check the program.

CNC 8070

1223 'End-of-file character inside the comment block'

DETECTION During execution.
CAUSE The CNC cannot find the end of the program. It may be because there is an open-

comment block (#COMMENT BEGIN), but the end-of-comment block (#COMMENT
END) is missing.

SOLUTION Check the program.

(REF: 1308)

·35·

Error solving manual

1224 'Operator unknown or missing'

DETECTION During execution.
CAUSE No assignment operator has been programmed after the variable or parameter.
SOLUTION The valid assignment operators are "=", "+=", "-=", "*=", "/=".

1225 'Division by zero'

DETECTION During execution.
CAUSE One of the programmed operations is dividing by zero.
SOLUTION Check the program. When working with parameters, in the program history, that

parameter may have taken the value of zero. Verify that the parameter does not reach
the operation with that value (0).

1226 'Face axis (FACEAXIS) missing in the active plane for radius compensation'

DETECTION During execution.
CAUSE None of the axes of the plane has been defined as face axis.
SOLUTION Define one of the axes of the main plane as face axis (parameter FACEAXIS).

1227 'Longitudinal axis (LONGAXIS) missing in the active plane for radius compensation'

DETECTION During execution.
CAUSE None of the axes of the plane has been defined as longitudinal axis.
SOLUTION Define one of the axes of the main plane as longitudinal axis (parameter LONGAXIS).

1233 'The programmed zero offset exceeds the data range'

DETECTION During execution.
CAUSE The defined zero offset exceeds the maximum admitted.
SOLUTION Check the program.

1236 'Macro name too long'

DETECTION During execution.
CAUSE The name of the macro has too many characters.
SOLUTION The maximum number of characters allowed is 30.

1237 ''"\" expected in the text associated with the macro'

DETECTION During execution.
CAUSE In the text for replacing a macro, a macro has been included that does not begin with

the "\" character.

SOLUTION The replacement text of the macro must be between quote marks and may include

other macros which must be delimited by the \" characters; for example
"macro"="\"macro1\" \"macro2\"".

1238 'Replacement text of the macro too long'

DETECTION During execution.
CAUSE The number of characters of the replacement text of the macro exceeds the maximum

allowed.

SOLUTION The maximum number of characters allowed is 140.

1239 'Too many macros'

DETECTION During execution.
CAUSE Too many macros at the CNC.
SOLUTION The maximum is 50 macros. The table of macros may be erased with the instruction

#INIT MACROTAB.

CNC 8070

(REF: 1308)

·36·

1240 'Nonexistent axis'

DETECTION During execution.
CAUSE The macro is not defined in the program.
SOLUTION Define the macro before using it. The macro may be defined in a program.

The CNC stores in a table the macros defined in a program or in MDI/MDA mode so
they are available for all the programs executed afterwards. The CNC initializes the
table of macros on start-up or with the instruction #INIT MACROTAB.

Error solving manual

1241 'The replacement text of the macro is missing'

DETECTION During execution.
CAUSE The replacement text associated with the macro is an empty string of characters.
SOLUTION Associate the proper replacement text with the macro according to the functionality

it should have. The replacement text must be written between quote marks.

1244 'Face axis close to the center: the spindle speed in G96 has been limited'

DETECTION During execution.
CAUSE When working at constant surface speed (G96), the CNC has limited the spindle

speed because the face axis is very close to the center of rotation.

SOLUTION Increase the speed limit (G192) or accept the limitation.

1245 'G96: no face axis (FACEAXIS) has been defined in the active plane'

DETECTION During execution.
CAUSE None of the axes of the plane has been defined as face axis.
SOLUTION Define one of the axes of the main plane as face axis (parameter FACEAXIS).

1246 'Threading is not possible with feedrate in G95'

DETECTION During execution.
CAUSE An attempt has been made to execute a rigid tapping (G63) while function G95 is

active (feed per spindle revolution).

SOLUTION Activate the feedrate as a function of time (G94)

1247 'Threading is not possible while G96 is active'

DETECTION During execution.
CAUSE The CNC has tried to execute a rigid tapping (G63) while function G96 is active

(constant surface speed).

SOLUTION Activate the constant turning speed mode (G97).

1248 'Threading and G192 not allowed in the same block'

DETECTION During execution.
CAUSE The CNC does not admit programming functions G63 (rigid tapping) and G192

(turning speed limitation) in the same block.

SOLUTION Program both instructions in different blocks.

1249 'Gear change is not possible while G96 is active'

DETECTION During execution.
CAUSE The CNC has tried to change the spindle gear (G112) while function G96 was active.
SOLUTION Cancel function G96 to make the spindle gear change.

1251 'Manual mode is not possible while G96 is active'

DETECTION During execution.
CAUSE The CNC has tried to access the jog mode while function G96 was active.
SOLUTION Cancel function G96 to access the jog mode.

1252 '#FREE AX: The face turning axis cannot be eliminated while G96 is active'

DETECTION During execution.
CAUSE The CNC has tried to eliminate the face axis from the configuration of the channel

(#FREE AX) while function G96 was active.

SOLUTION Cancel function G96 to eliminate the face axis from the configuration of the channel.

1254 'G192 and M19 not allowed in the same block'

DETECTION During execution.
CAUSE The CNC does not admit programming functions M19 (spindle orientation) and G192

(turning speed limitation) in the same block.

SOLUTION Program both instructions in different blocks.

1255 'Negative acceleration percentage'

DETECTION During execution.
CAUSE In function G130, the programmed percentage of acceleration is negative.
SOLUTION The percentage of acceleration must be equal to or greater than zero.

CNC 8070

(REF: 1308)

·37·

Error solving manual

1256 'Acceleration percentage out of range'

DETECTION During execution.
CAUSE In function G130, the programmed percentage of acceleration is too high.
SOLUTION Check the program.

1257 'The leadscrew pitch has been programmed twice'

DETECTION During execution.
CAUSE In function G33, the thread pitch has been programmed more than once.
SOLUTION Check the program. Define the thread pitch only once in the block.

1258 'Leadscrew pitch equal to zero'

DETECTION During execution.
CAUSE In function G33, the thread pitch is zero.
SOLUTION Check the program. Program the thread pitch with parameters I J K.

1259 'Leadscrew pitch out of range'

DETECTION During execution.
CAUSE In function G33, the programmed thread pitch is too large.
SOLUTION Check the program.

1261 'Unknown kinematics type'

DETECTION During execution.
CAUSE The CNC has tried to activate function #RTCP or #TLC, or a coordinate

transformation (#CS/ACS) in mode 6 without having a kinematics active.

SOLUTION First activate the kinematics and then the desired function.

CNC 8070

1262 'The group of the axes is not enough for the transformation'

DETECTION During execution.
CAUSE The channel does not have enough axes to activate function RTCP, TLC or the

coordinate transformation. The number of axes required will depend on the
kinematics to be activated.

SOLUTION Correct the configuration of the axes of the channel (instruction: #SET AX) in order

to be able to activate the kinematics.

1263 'Rotary axis (axes) missing for the transformation'

DETECTION During execution.
CAUSE An instruction #TOOL ORI has been programmed, but there is no rotary axis to place

the tool perpendicular to the defined inclined plane.

SOLUTION Either do not program the instruction #TOOL ORI or activate the kinematics that

allows placing the tool perpendicular to the defined inclined plane.

1264 'Programming not allowed while CS/ACS is active'

DETECTION During execution.
CAUSE The CNC does not allow executing the programmed function if coordinate

transformation is active. Some incompatible functions are G74, G198, G199, #LINK,
probing cycles, etc.

SOLUTION Cancel coordinate transformation to execute the rest of the functions.

1265 'Programming not allowed while RTCP/TLC is active'

DETECTION During execution.
CAUSE The CNC does not allow executing the programmed function if function RTCP or TLC

is active. Some incompatible functions are G74, G198, G199, #KIN ID.
LINK.

SOLUTION Cancel the RTCP or TLC function to execute the rest of the functions.

(REF: 1308)

·38·

1266 'The TLC feature is deactivated using the instruction #TLC OFF'

DETECTION During execution.
CAUSE The CNC has tried to modify the TLC function while it was active.
SOLUTION The CNC does not allow modifying the TLC function while it is active. To modify the

TLC function, first deactivate it and then activated again.

Error solving manual

1267 'The RTCP functionality is canceled with the instruction #RTCP OFF'

DETECTION During execution.
CAUSE While RTCP is active, a #RTCP instruction other than #RTCP OFF has been

programmed.

SOLUTION To cancel the RTCP function, program #RTCP OFF. To change the values of the

RTCP, it must be canceled first.

1268 '#CS ON/#ACS ON: syntax error'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong.
SOLUTION Check the program.

1269 '#CS ON/#ACS ON: the programmed angle is not valid'

DETECTION During execution.
CAUSE The programmed angle is wrong.
SOLUTION Program an angle within ±360º.

1270 'The coordinate transformation cannot be calculated'

DETECTION During execution.
CAUSE The CNC has not been able to solve a transformation from part-coordinates to

machine coordinates or vice versa.

SOLUTION Cancel the transformation, change the position of the axes and activate the

transformation again.

1271 'The axes of the active kinematics can neither be excluded nor modified'

DETECTION During execution.
CAUSE The CNC has tried to modify the configuration of the axes of a kinematics while it was

active.

SOLUTION Cancel the kinematics before modifying the configuration of the axes of the channel.

1272 'The axes of the active transformation can neither be excluded nor modified'

DETECTION During execution.
CAUSE The CNC has tried to modify the configuration of the axes of an inclined plane while

it was active.

SOLUTION Cancel the inclined plane transformation to modify the configuration of the axes of

the channel.

1275 'Position calculated by the inverted kinematics transformation out of range'

DETECTION During execution.
CAUSE The CNC has tried to do an unsolved transformation from machine coordinates to

part coordinates.

SOLUTION Cancel the transformation, change the position to be accessed and activate the

transformation again. Check the transformation if it is a user transformation.

1277 'The resulting zero offset exceeds the data range'

DETECTION During execution.
CAUSE The zero offset calculated from the coordinates programmed in function G92 is too

large.

SOLUTION Check the program.

1278 'G131/G133: wrong value'

DETECTION During execution.
CAUSE In function G131 or G133, the programmed percentage of acceleration or jerk is not

valid.

SOLUTION Program a percentage of acceleration or jerk that is positive and less than or equal

to 100.

1279 '" expected'

DETECTION During execution.
CAUSE Quote marks are missing in the programmed expression or instruction.
SOLUTION Check the program.

CNC 8070

(REF: 1308)

·39·

Error solving manual

1281 ''The number of parameters and format indicators do not match'

DETECTION During execution.
CAUSE The number of data identifiers (%D or %d) appearing in the #MSG, #ERROR or

#WARNING instruction does not match the number of parameters to be displayed.

SOLUTION Check the program.

1282 'Message too long'

DETECTION During execution.
CAUSE The text message of the instruction #MSG, #ERROR or #WARNING is too long.
SOLUTION It may have up to 69 characters, including the characters that replace the data

identifiers.

1283 'Too many format indicators'

DETECTION During execution.
CAUSE There are more than 5 data identifiers (%D ó %d) in the instruction #MSG, #ERROR,

#WARNING.

SOLUTION Reduce the number of data identifiers.

1284 'Arithmetic expression expected'

DETECTION During execution.
CAUSE There are data identifiers (%D ó %d) in the instruction #MSG, #ERROR, #WARNING,

but the parameters to be displayed are missing.

SOLUTION Check the program.

1285 'Tool radius written twice'

DETECTION During execution.
CAUSE The tool radius has been programmed more than once in the same block.
SOLUTION Program the tool radius only once in the block.

1286 'Tool length written twice'

DETECTION During execution.
CAUSE The tool length has been programmed more than once in the same block.
SOLUTION Program the tool length only once in the block.

1287 '"[" expected'

DETECTION During execution.
CAUSE The opening bracket "]" is missing in the programmed expression or instruction.
SOLUTION Check the program.

1288 'Too many parameters programmed in the instruction'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong.
SOLUTION Check the program.

1290 'I, J, K coordinates programmed wrong'

DETECTION During execution.
CAUSE The possible causes are:

• The programmed values for the center of the circular interpolation, Polar origin
or center of rotation of the coordinate system are too high.

• The values programmed for the center of the circular interpolation, being G264
active, are wrong.

SOLUTION Check the program.

CNC 8070

(REF: 1308)

·40·

1291 'No more S functions allowed'

DETECTION During execution.
CAUSE There are too many S functions in the same block.
SOLUTION The maximum number of S functions allowed in the same block is 4.

1292 'M function programmed twice'

DETECTION During execution.
CAUSE The same M function has been programmed more than once in the block.
SOLUTION Program both functions in different blocks.

Error solving manual

1293 'H function programmed twice'

DETECTION During execution.
CAUSE The same H function has been programmed more than once in the block.
SOLUTION Program both functions in different blocks.

1301 'The tool length transformation exceeds the valid numeric format'

DETECTION During execution.
CAUSE The tool length transformation exceeds the valid numeric format.
SOLUTION Modify the values of the length transformation or those of the tool.

1302 'Wrong character in the name'

DETECTION During execution.
CAUSE Wrong character in the name of a label, subroutine or variable.
SOLUTION Check the program.

1303 'Variable name too long'

DETECTION During execution.
CAUSE Too many characters for the name of the variable.
SOLUTION The maximum number of characters allowed is 13.

1304 'Wrong spindle speed'

DETECTION During execution.
CAUSE The programmed speed is too low.
SOLUTION Check the program.

1305 'Programming not allowed while #MCS is active'

DETECTION During execution.
CAUSE The CNC does not allow executing the programmed function if the MCS function is

active. Some incompatible functions are:

• Zero offsets (G54-G59, G159, G92, G158, G53) on/off

• Measuring offset (G101, G102) on/off.

• Fixtures on/off ("V.G.FIX" variable).

• Mirror (G11/G12/G13/G14) image on/off.

• Programming in radius/diameters (G151/G152).

• Activate incremental programming (G91).

• Programming in mm/inches (G70/G71).

• Scaling factor (G72).

• Movement in G0, G1, G2, G3, G8 or G9 in Polar coordinates.

• Threading G63 or G33 in Polar coordinates.

• Polar origin (G30).

• Pattern rotation (G73).

• Instructions #FACE, #CYL and #RTCP.

SOLUTION Check the program.

1306 'The kinematics cannot be changed while tool radius compensation is active'

DETECTION During execution.
CAUSE The CNC has tried to change the kinematics while tool radius compensation was

active.

SOLUTION Cancel the compensation to define the new work plane.

1308 'An axis of the active transformation cannot be a slave'

DETECTION During execution.
CAUSE The slave axis of the coupling is part of the active kinematics.
SOLUTION Cancel the kinematics to be able to couple the axis. The axis involved in the active

kinematics can be master of a coupling.

1309 'File name expected'

DETECTION During execution.
CAUSE No program has been selected for execution.
SOLUTION Select the program to be executed.

CNC 8070

(REF: 1308)

·41·

Error solving manual

1310 'Program line too long'

DETECTION During execution.
CAUSE Too many characters in the #EXBLK instruction.
SOLUTION The maximum number of characters allowed is 128.

1311 'Measurement offset not included in programmed axis (axes)'

DETECTION During execution.
CAUSE The G102 function tries to exclude the measurement offset of an axis that has no

measurement offset included.

SOLUTION The G102 function makes no sense for an axis without measuring offset.

1314 '#CS ON/#ACS ON: wrong identifier'

DETECTION During execution.
CAUSE In these instructions, the number of the coordinate system is not valid.
SOLUTION Program a value between 1 and 5.

1315 '#CS ON/#ACS ON: undefined system'

DETECTION During execution.
CAUSE The instructions do not have parameters and no coordinate system has been stored.

When programming one of these instructions without parameters, the CNC tries to
activate the transformation stored last.

SOLUTION Check the program. Define and save some coordinate system.

1316 '#CS/#ACS DEF: parameters missing'

DETECTION During execution.
CAUSE One or more required parameters have not been programmed.
SOLUTION Check the program. These instructions require programming the coordinate system

number, the definition mode, the components of the translation vector and the rotation
angles.

1318 '#CS ON/#ACS ON: No changes allowed with the active coordinate system'

DETECTION During execution.
CAUSE The CNC has tried to change the parameters of an active coordinate system.
SOLUTION Check the program. The CNC does not allow to change the parameters of an active

coordinate system; it does allow changing the parameters of a coordinate system that
has been already defined, but it is not active.

1319 'Nesting of #CS ON/#ACS ON instructions exceeded'

DETECTION During execution.
CAUSE The The CNC has exceeded the limit of coordinate system combinations.
SOLUTION The allows combining different coordinate systems with each other to build new ones.

The CNC allows combining 10 coordinate systems.

1320 'Too many labels'

DETECTION During execution.
CAUSE The program has too many block labels. The labels to identify a block may be of the

following type

SOLUTION The maximum number of labels for each type is 128. The labels may be represented

by the letter N followed by the block number or by [name] type labels.

CNC 8070

(REF: 1308)

·42·

1321 'Label name too long'

DETECTION During execution.
CAUSE The name of the label has too many characters.
SOLUTION The maximum number of characters allowed is 15.

1322 'Label defined several times'

DETECTION During execution.
CAUSE The block label is repeated (duplicate) in the program.
SOLUTION Eliminate the repeated labels.

Error solving manual

1323 '$GOTO: Wrong label'

DETECTION During execution.
CAUSE A label can only be defined with a string of characters between brackets or with the

"N" character followed by a positive number smaller than 2147483646.

SOLUTION Check the program.

1324 'Undefined label'

DETECTION During execution.
CAUSE The block label defined in the $GOTO or #RPT instruction does not exist in the

program.

SOLUTION Define the jump label in some point of the program.

1325 'Block number defined several times'

DETECTION During execution.
CAUSE The block number "N" is repeated (duplicate) in the program.
SOLUTION Do not repeat the block number.

1326 'Wrong value to be assigned to a variable'

DETECTION During execution.
CAUSE The value of the variable is too high.
SOLUTION Check the program.

1327 'Spindle positioning (orienting) speed programmed twice'

DETECTION During execution.
CAUSE The spindle orientation speed (M19) has been programmed more than once in the

block.

SOLUTION Check the program. Program the positioning speed only once in the block.

1328 '$FOR instruction without $ENDFOR'

DETECTION During execution.
CAUSE A $FOR instruction has been programmed, but its $ENDFOR is missing.
SOLUTION Check the program.

1330 'Mirror image programmed wrong'

DETECTION During execution.
CAUSE Function G14 (mirror image) has been programmed wrong.
SOLUTION Check the program.

1331 '#TANGFEED RMIN: negative radius not allowed'

DETECTION During execution.
CAUSE The programmed radius is less than or equal to zero.
SOLUTION Check the program.

1332 '#TOOL AX: orientation +/- expected after designating the axis'

DETECTION During execution.
CAUSE The tool orientation has not been programmed.
SOLUTION Check the program.

1333 'Change of the first and/or second axis of the plane while tool radius compensation is

active'

DETECTION During execution.
CAUSE Being tool radius compensation active, the CNC has tried to change the axis

configuration of the channel and the change affects the first two axes of the work
plane.

SOLUTION Cancel tool radius compensation in order to make the changes in the axis

configuration of the channel that affect the work plane.

CNC 8070

1334 'G200: does not allow movement in the same block'

DETECTION During execution.
CAUSE An axis movement has been programmed in the same block as function G200.
SOLUTION Check the program.

(REF: 1308)

·43·

Error solving manual

1336 'Wrong configuration: two CAXIS axis'

DETECTION During execution.
CAUSE Both axes programmed in the #FACE/#CYL instruction are C axes.
SOLUTION Only one of the programmed axes may be a C axis (parameter CAXIS).

1337 'No CAXIS has been defined'

DETECTION During execution.
CAUSE None of the axes programmed in the #FACE/#CYL instruction is a C axis.
SOLUTION One of the two programmed axes must be a C axis (parameter CAXIS).

1339 'The selection has no effect'

DETECTION During execution.
CAUSE The programmed instruction has no effect because it is already active, the same

instruction with the same parameters is already programmed in a previous block.

SOLUTION Check the program.

1340 'The deselection has no effect'

DETECTION During execution.
CAUSE The CNC has tried to execute the #CAX OFF instruction, but there is no spindle

working as C axis.

SOLUTION Check the program.

1342 '#CAX OFF not allowed if a transformation is active'

DETECTION During execution.
CAUSE The CNC does not allow canceling the C axis while the RTCP or TLC function is active.
SOLUTION Check the program.

1343 '#FACE OFF not allowed with the type of kinematics active'

DETECTION During execution.
CAUSE The CNC has tried to execute the #FACE OFF instruction, but there is no machining

on the face of the part.

SOLUTION Check the program.

1344 'No plane change allowed while machining the side of the part'

DETECTION During execution.
CAUSE The CNC has tried to change the work plane (G17-G20) while lateral machining is

active.

SOLUTION Check the program.

1345 'G20: Axes programmed wrong'

DETECTION During execution.
CAUSE In function G20 (plane change), the first two axes of the plane (parameters 1 and 2)

are wrong.

SOLUTION The two axes must be different and they must be among the first three axes of the

channel.

1347 '#CYL OFF not allowed with the type of kinematics active'

DETECTION During execution.
CAUSE The CNC has tried to execute the #CYL OFF instruction, but there is no machining

on the side of the part.

SOLUTION Check the program.

CNC 8070

(REF: 1308)

·44·

1348 '#CYL: wrong radius'

DETECTION During execution.
CAUSE The radius programmed in the #CYL instruction is negative or zero. If the radius is

variable, it tries to go through the center of the cylinder generating a zero radius.

SOLUTION Check the program. The radius must be positive and if it is a variable radius, it cannot

go through the center of the cylinder.

Error solving manual

1349 'Negative axis coordinate when activating #FACE'

DETECTION During execution.
CAUSE The linear axis that is part of the face C axis transformation is positioned in the

negative portion with respect to the rotating axis. The CNC does not admit this option
(parameter ALINGC).

SOLUTION Position the axis in the positive portion with respect to the rotation center before

activating the machining operation along the face axis.

1350 'Wrong character between the #VAR/#ENDVAR instructions'

DETECTION During execution.
CAUSE A wrong character has been programmed in some block between these instructions.
SOLUTION Between these instructions, only the declaration of user variables (separated by

commas if there are several in the same line) or the programming of the block number
are allowed.

1351 '#VAR/#ENDVAR/#DELETE: variable type not allowed'

DETECTION During execution.
CAUSE The CNC has tried to define or delete a variable that is not a user variable.
SOLUTION Check the program.

1352 '#VAR/#ENDVAR: the variable defined already exists'

DETECTION During execution.
CAUSE The user variable already exists.
SOLUTION Check the program.

1353 'Too many values to initialize the array'

DETECTION During execution.
CAUSE When initializing an user array variable, the CNC initializes more positions than it has.
SOLUTION Check the program.

1354 'Error when reading the variable'

DETECTION During execution.
CAUSE The CNC cannot read the variable.
SOLUTION Check the program.

1355 'The variable cannot be deleted'

DETECTION During execution.
CAUSE The CNC has tried to delete a variable from the system.
SOLUTION The CNC can only delete user variables (prefixes P and S).

1356 'Variable or parameter expected'

DETECTION During execution.
CAUSE $IF EXIST instruction programmed wrong.
SOLUTION The $IF EXIST instruction only allows arithmetic parameters or variables.

1357 '#DELETE: wrong character'

DETECTION During execution.
CAUSE An invalid character has been detected in the block.
SOLUTION Check the syntax of the block. The instruction must be programmed alone in the block

or next to the block label. This instruction only admits user variables.

1358 '#DELETE: the variable to be deleted does not exist'

DETECTION During execution.
CAUSE The user variable does not exist.
SOLUTION Check the program.

1360 'G33/G63/G95/G96/G97 not allowed while the C axis is active'

DETECTION During execution.
CAUSE The CNC has tried to execute a G33/G63/G95/G96/G97 function while the C axis was

active.

SOLUTION Cancel the C axis in order to be able to execute the function.

CNC 8070

(REF: 1308)

·45·

Error solving manual

1362 'Wrong array dimension.

DETECTION During execution.
CAUSE It is an array variable, but the number of programmed arrays is wrong.
SOLUTION Check the syntax of the variable.

1363 'Wrong declaration of array variables'

DETECTION During execution.
CAUSE User variables that are array variables must be declared between #VAR and

#ENDVAR instructions.

SOLUTION Check the program.

1364 'Too many array variable indexes'

DETECTION During execution.
CAUSE The user variable is a multi-dimensional array with more than 4 dimensions.
SOLUTION Check the program.

1365 'Negative spindle speed not allowed'

DETECTION During execution.
CAUSE Negative spindle speed.
SOLUTION The spindle speed must be positive; a negative value is only allowed when

programming G63 in the same block.

1367 'A gear change and a spindle movements cannot be simultaneous'

DETECTION During execution.
CAUSE An M function for spindle movement and function G112 (parameter set change) have

been programmed in the same block.

SOLUTION Check the program.

CNC 8070

1368 'The circle's center and radius cannot be programmed at the same time'

DETECTION During execution.
CAUSE The circular interpolation is defined with the radius and the center.
SOLUTION In a circular interpolation, one must program the coordinate of the last point and the

radius or the center of the circle.

1369 '#HSC: programming not allowed'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong.
SOLUTION Check the program.

1370 '#HSC: double programming'

DETECTION During execution.
CAUSE The HSC activation and cancellation have been programmed in the same block.
SOLUTION Check the syntax of the instructions in the programming manual.

1371 '#HSC: invalid mode.'

DETECTION During execution.
CAUSE The CNC has tried to activate the HSC mode with an unknown parameter or has tried

to change the work mode without activating it first.

SOLUTION Check the program.

1373 '#HSC: wrong parameter'

DETECTION During execution.
CAUSE The value of parameter FAST or parameter CORNER of the #HSC instruction is

wrong.

SOLUTION Check the program.

(REF: 1308)

·46·

1374 'M02/M30 expected'

DETECTION During execution.
CAUSE M02 or M30 has not been programmed at the end of the main program.
SOLUTION Check the program.

Error solving manual

1375 'M17/M29/#RET expected'

DETECTION During execution.
CAUSE M17, M29 or #RET has not been programmed at the end of the subroutine.
SOLUTION Check the program.

1376 'No default name has been defined for the C axis'

DETECTION During execution.
CAUSE In the #CAX instruction, the name of the C axis is missing and the default name

(parameter CAXIS) is not indicated in the machine parameters.

SOLUTION In the #CAX instruction, indicate the name that will identify the "C" axis.

1377 'Parameter written with wrong index'

DETECTION During execution.
CAUSE The arithmetic parameter does not exist or is write-protected.
SOLUTION Check the program. Check the valid arithmetic parameter range in the machine

parameters.

Machine parameters. Valid range.

MINLOCP - MAXLOCP Local arithmetic parameters.

MINGLBP - MAXGLBP Global arithmetic parameters.

MINCOMP - MAXCOMP Common arithmetic parameters.

The write-protected global parameters are those defined by machine parameters
ROPARMIN - ROPARMAX.

1378 'Parameter read with wrong index'

DETECTION During execution.
CAUSE The arithmetic parameter does not exist; it is not within the range admitted by the

machine parameters.

SOLUTION Check the program. Check the valid arithmetic parameter range in the machine

parameters.

Machine parameters. Valid range.

MINLOCP - MAXLOCP Local arithmetic parameters.

MINGLBP - MAXGLBP Global arithmetic parameters.

MINCOMP - MAXCOMP Common arithmetic parameters.

1380 'Canned cycle programmed wrong'

DETECTION During execution.
CAUSE In the block defining a canned cycle, nothing must be programmed after the cycle

parameters.

SOLUTION Check the program.

1381 'Nonexistent canned cycle'

DETECTION During execution.
CAUSE The programmed canned cycle does not exist.
SOLUTION Check the program.

1382 'Parameter not allowed in canned cycle'

DETECTION During execution.
CAUSE One of the programmed parameters is not allowed for that canned cycle.
SOLUTION Check the programming manual for the parameters required and allowed by each

canned cycle.

CNC 8070

1383 'Mandatory parameter not programmed in canned cycle'

DETECTION During execution.
CAUSE A parameter required in the canned cycle has not been programmed.
SOLUTION Check the programming manual for the parameters required and allowed by each

canned cycle.

(REF: 1308)

·47·

Error solving manual

1384 'M function not allowed with movement'

DETECTION During execution.
CAUSE A movement and an M function with associated subroutine and execution before the

movement have been programmed in the same block. The subroutines are always
executed at the end of the block; therefore, the M function will never be executed
before the programmed movement.

SOLUTION Program the M function in another block or define the M function in the machine

parameters to be executed after the movement.

1385 'D and the tool length cannot be modified in the same block'

DETECTION During execution.
CAUSE The CNC has tried to write the "V.G.TOL" variable in the same block where a tool

change or tool offset change is programmed.

SOLUTION Check the program.

1386 'D and the tool offsets cannot be modified in the same block'

DETECTION During execution.
CAUSE The CNC has tried to write the "V.G.TOFL.xn" variable in the same block where a tool

change or tool offset change is programmed.

SOLUTION Check the program.

1387 'Too many M functions in the same block'

DETECTION During execution.
CAUSE There are too many M functions in the same block.
SOLUTION From version V2.00, the CNC admits up to 14 M functions per block; in earlier

versions, the limit was 7 functions per block.

CNC 8070

1388 'No more H functions allowed'

DETECTION During execution.
CAUSE There are too many H functions in the same block.
SOLUTION The maximum number of H functions allowed in the same block is 7.

1389 'Incompatible G functions (G10/G11/G12/G13/G14)'

DETECTION During execution.
CAUSE Two G functions incompatible with each other have been programmed in the block.
SOLUTION Program the functions in different blocks.

1390 'Incompatible G functions (G98/G99)'

DETECTION During execution.
CAUSE Two G functions incompatible with each other have been programmed in the block.
SOLUTION Program the functions in different blocks.

1392 'Parameter programmed twice'

DETECTION During execution.
CAUSE The same parameter has been programmed more than once in the instruction or

function.

SOLUTION Check the program.

1393 'The current tool and tool offset do not match the ones programmed'

DETECTION During block search.
CAUSE After a tool inspection, the active tool offset D does not match the tool offset D

programmed before interrupting the execution. The CNC has motion blocks prepared
that will be used to machine the part after repositioning with the programmed tool
radius. If the tool that is in the spindle is different and the tool radius is compensated
in the program, the CNC will machine a different part.

SOLUTION Change the tool of the spindle so it matches the one programmed.

(REF: 1308)

·48·

1394 'The subroutine associated with the G function does not exist'

DETECTION During execution.
CAUSE A G180 or G189 function has been programmed, but the associated subroutine does

not exist. A G74 function has been programmed alone in the block, but the associated
subroutine does not exist.

SOLUTION Together with function G74, program the axes to be homed or define the associated

subroutine (parameter REFPSUB). For functions G180 through G189, define the
associated subroutine (parameter OEMSUB).

Error solving manual

1395 'Function G74 with associated subroutine must be programmed alone in the block'

DETECTION During execution.
CAUSE If function G74 has an associated subroutine, it must be programmed alone in the

block or together with the block label.

SOLUTION Check the program.

1396 'Programming not allowed in MDI'

DETECTION During execution.
CAUSE That command cannot be executed in MDI.
SOLUTION Execute that command within the program.

1397 'The position programmed for the Hirth axis is wrong'

DETECTION During execution.
CAUSE The coordinate programmed for the Hirth axis does not correspond to a whole step.
SOLUTION The hirth axis only admits multiples of its pitch.

1398 'An axis with parameter HIRTH = NO cannot be activated as Hirth axis'

DETECTION During execution.
CAUSE The CNC has tried to activate (G171) or deactivate (G170) as a hirth axis one that

is not (parameter HIRTH).

SOLUTION Check the program. 'The axis cannot be activated as a hirth axis.

1399 'The axis cannot be activated as Hirth'

DETECTION During execution.
CAUSE The possible causes are:

• The hir th axis is one of the axes of the plane and tool radius compensation and/or
collision detection is active.

• The hirth axis is part of the active coordinate transformation.

• The hirth axis is par t of the active kinematics and also an #RTCP, #TLC or #TOOL
ORI instruction is active.

SOLUTION Check the program.

1400 'Tool length change is not possible while RTCP is active'

DETECTION During execution.
CAUSE The CNC has tried to make a tool change while function RTCP was active.
SOLUTION Cancel the RTCP function to make the tool change.

1401 '#TLC ON not admitted without unselecting first'

DETECTION During execution.
CAUSE The CNC has tried to activate the TLC function and it is already active.
SOLUTION Check the program.

1402 '#LINK: The master and slave axes must have their HIRTH and HPITCH parameters set

the same way.

DETECTION During execution.
CAUSE The CNC has tried to couple two hirth axes, but one of them is not hirth or they both

have different pitches.

SOLUTION In order to include a hirth axis in a coupling, both axes must be hirth (parameter

HIRTH) and have the same pitch.

1403 '#LINK: a coupling cannot be defined if a Hirth axis is deactivated'

DETECTION During execution.
CAUSE The CNC has tried to couple two hirth axes, but one of them is deactivated.
SOLUTION In order to couple two hirth axes, both of them must be active (G171).

1404 'The gear associated with the programmed M function does not exist'

DETECTION During execution.
CAUSE The CNC has tried to make a spindle gear change using an M41 through M44

function, but the gear does not exist.

SOLUTION The number of gears available at the spindle is determined in the machine parameters

(parameter NPARSETS). The CNC will accept the M41 through M44 functions of the
existing spindle gears.

CNC 8070

(REF: 1308)

·49·

Error solving manual

1405 'The S value exceeds the maximum gear'

DETECTION During execution.
CAUSE The spindle has an automatic gear changer (parameter AUTOGEAR) and a speed

has been programmed that is higher than any of the existing gears for that spindle.

SOLUTION Program a lower spindle speed that may be reached with one of the gears existing

for that spindle. Check that the maximum speed defined in each gear is correct.

1406 '#CALL: does not admit parameter programming'

DETECTION During execution.
CAUSE The #CALL instructiont does not allow to program parameters.
SOLUTION Check the program.

1407 'Error when reading pocket data'

DETECTION During execution.
CAUSE When executing a 2D or 3D pocket, the CNC could not decode some of the data. This

may happen when the pocket data has been edited manually and a numeric value
has been replaced with a variable, the bracket at the end of the instructions
#DATAP2D, #DATAP3D has been eliminated, etc.

SOLUTION Edit the pocket again with the cycle editor.

1408 'It cannot be programmed if the spindle is not controlled in position'

DETECTION During execution.
CAUSE The CNC cannot execute the programmed function or instruction if the spindle is not

controlled in position.

SOLUTION The spindle must have an encoder.

CNC 8070

(REF: 1308)

1409 'Nesting of T functions with subroutine, not allowed'

DETECTION During execution.
CAUSE The CNC has tried to execute a tool change and the subroutine associated with the

T function (parameter TOOLSUB) contains another tool change.

SOLUTION A T function cannot be programmed inside the subroutine associated with the tool

change

1411 '#CD: wrong number of blocks'

DETECTION During execution.
CAUSE The number of blocks programmed in the instruction is wrong.
SOLUTION The maximum number of blocks to analyze is 200.

1412 '#DGWZ: graphics display area defined wrong'

DETECTION During execution.
CAUSE The axis limits have been defined wrong in the instruction.
SOLUTION Both limits may be positive or negative, but the lower limits of an axis must always

be lower than its upper limits.

1413 'The spindle positioning speed cannot be zero'

DETECTION During execution.
CAUSE The programmed positioning speed for function M19 is zero.
SOLUTION Program a positioning speed greater than zero using the command "S.POS".

1414 '#PARK: this instruction only admits one axis'

DETECTION During execution.
CAUSE The #PARK instruction only allows parking one axis.
SOLUTION Program a #PARK block for each axis to be parked.

1417 'File path too long'

DETECTION During execution.
CAUSE The maximum number of characters allowed for the path of a program or subroutine

has been exceeded.

SOLUTION The path of a program or subroutine may have a maximum of 120 characters. Move

the program or subroutine to another directory to reduce the number of characters
of the path.

·50·

Error solving manual

1418 'It is not possible to park axes of the active kinematics or transformation'

DETECTION During execution.
CAUSE The CNC has tried to park an axis that is part the active kinematics or transforms #CS,

#ACS, #ANGAX, #TANGCTRL.

SOLUTION Check the program. To park that axis, cancel the active kinematics or transformation.

1419 'Slaved axes (Gantry or Tandem) cannot be parked.

DETECTION During execution.
CAUSE The CNC has tried to park an axis that is part of a gantry, tandem axis or of an active

coupling (#LINK).

SOLUTION Check the program. To park that axis, cancel the coupling. The axes belonging to a

gantry or tandem pair cannot be parked.

1420 'Open control blocks at the end of the program'

DETECTION During execution.
CAUSE Some $IF, $FOR, etc. does not have its corresponding closing instruction.
SOLUTION Check the program.

1421 'The axes of the active transformation can neither be slaves nor parked'

DETECTION During execution.
CAUSE One of the axes involved in the programmed coordinate transformation is parked, is

a slave of a gantry pair or is a slave of an active coupling.

SOLUTION Unpark, deactivate the active coupling or undo the gantry pair in order to use the axis

in the coordinate transformation.

1422 '#CS ON/#ACS ON: wrong programmed mode'

DETECTION During execution.
CAUSE The programmed MODE parameter is wrong.
SOLUTION The value of the MODE parameter must be between 1 and 6.

1423 '#CS ON/#ACS ON: the parameter of an aligned axis must be 0 or 1'

DETECTION During execution.
CAUSE The value programmed as method for aligning the plane is wrong.
SOLUTION Check the program.

1424 'G function not allowed while MCS is active'

DETECTION During execution.
CAUSE The programmed G function cannot be executed while #MCS is active.
SOLUTION Check the program.

1425 'Block skip is only admitted at the beginning of the line'

DETECTION During execution.
CAUSE The "/" character is only admitted at the beginning of the program line.
SOLUTION Check the program.

1426 'The pocket was resolved with a different tool radius'

DETECTION During execution.
CAUSE The CNC generated the pocket with a tool radius other than the current one.
SOLUTION Generate the pocket again.

1427 'Axis programmed wrong'

DETECTION During execution.
CAUSE Syntax error when programming the instruction or G function; some axis is repeated

in a movement, the home searching order for the axes is missing in the G74 function
or the order of the axes in the system is missing in the G20 function.

SOLUTION Check the program.

1428 'The movement in the main plane must be programmed before the G function of the cycle'

DETECTION During execution.
CAUSE The coordinates of the starting point of the cycle are defined after the G function that

defines the cycle. The cycle considers the coordinates of the starting point as its own
parameters.

SOLUTION Program the coordinates of the axes before the G function of the cycle.

CNC 8070

(REF: 1308)

·51·

Error solving manual

1429 'Too many subroutines in the same block'

DETECTION During execution.
CAUSE The maximum number of subroutines that may be executed in the same block has

been exceeded.

SOLUTION The maximum number of subroutines that may be executed in the same block is 5.

Program the subroutines in different blocks or use subroutine nesting as necessary.

1430 'Numeric format exceeded'

DETECTION During execution.
CAUSE The value assigned to a data, variable or parameter exceeds the established format.
SOLUTION Check the program.

1431 'Wrong spindle position in M19'

DETECTION During execution.
CAUSE The value programmed for the spindle position in M19 is too high.
SOLUTION Program a smaller value.

1432 'A slave axis of a Gantry or coupling cannot be programmed'

DETECTION During execution.
CAUSE In instruction contains the slave axis of an active coupling or of Gantry pair.
SOLUTION In order to operate with the axis in those instructions, deactivate the active coupling

(#UNLINK) or undo the Gantry pair (by machine parameter).

1433 'A parked axis cannot be part of the main plane'

DETECTION During execution.
CAUSE The CNC has tried to include (#CALL / #SET) a parked axis between the first three

axes of the channel.

SOLUTION A parked axis cannot be part of the first of three axes of the channel; unpark the axis

(#UNPARK).

1434 'An associated slave axis could not be included in the configuration'

DETECTION During execution.
CAUSE The CNC has tried to include the master axis of an active coupling or that of a Gantry

pair in the channel configuration (#CALL or #SET). When including the master axis,
the CNC also includes the slave axis which can never occupy one of the main three
positions of the channel. The CNC issues an error because there is no free position
other than the main three axis.

SOLUTION In order to only include the master axis, the active coupling must be deactivated first

(#UNLINK) or undo the Gantry pair. In order to include both the master and the slave
axis, first eliminate another axis from the channel or increase the number of axes of
the channel.

1435 'An associated slave axis could not be assigned a name because it was repeated'

DETECTION During execution.
CAUSE The CNC has tried to include the master axis of an active coupling or that of a Gantry

pair in the channel configuration (#CALL or #SET). When including the master axis,
the CNC also includes the slave axis which can never occupy one of the main three
positions of the channel. The CNC issues an error because the name of the slave
axis is already occupied by another axis of the current configuration of the channel.

SOLUTION Rename either the slave axis to be included or the one that already exists in the

configuration.

CNC 8070

(REF: 1308)

·52·

1436 'The stop block has not been programmed in the block search'

DETECTION During execution.
CAUSE The stop block of the block search is missing.
SOLUTION Once the block search option has been selected, the softkey menu shows the option

to select the stop block. Select the block where the block search will end.

1439 'The axes of the active transformation cannot be Hirth'

DETECTION During execution.
CAUSE The CNC has tried to activate a coordinate transformation (#TLC, #RTCP, #TOOL

ORI, #CS or #ACS), but one of the axes involved in the transformation is a Hirth axis.

SOLUTION A hirth axis must not be part of the coordinate transformation. An axis involved in the

transformation must not be a Hirth axis (G170).

Error solving manual

1440 'Wrong tool or edge'

DETECTION During execution.
CAUSE The tool and/or offset indicated in the variable does not exist.
SOLUTION Check the program. Check the existing tools and tool offsets.

1441 'The kinematics has not been activated'

DETECTION On CNC power-up or when validating the machine parameters.
CAUSE The kinematics that the CNC applies by default (parameter KINID) is unknown or the

axes required for the kinematics are not the right ones.

SOLUTION Check that the type of kinematics is correct and that the axes involved in it are properly

defined and belong to the channel. The axes must always be the first ones of the
channel, they must not be Hirth, they must not be parked and they must not be slaves
of a coupling or a gantry pair.

1442 'The kinematics has been deactivated'

DETECTION After a reset of the CNC or when starting the execution of a part-program.
CAUSE The CNC has canceled a kinematics, either because it is an unknown kinematics or

because the axes required for that kinematics are not the right ones.

SOLUTION Check that the type of kinematics is correct and that the axes involved in it are properly

defined and belong to the channel. The axes must always be the first ones of the
channel, they must not be Hirth, they must not be parked and they must not be slaves
of a coupling or a gantry pair.

1443 '#CS/ACS has been deactivated'

DETECTION After a reset of the CNC, when starting the execution of a part-program or during

home search.

CAUSE The axes used in the inclined plane are not the right ones. The CNC has tried to carry

out a home search while function #CS/ACS was active.

SOLUTION To make an inclined plane, the first three axes of the channel must be defined, linear,

unparked and not slaves of a coupling or a gantry pair. Deactivate the #CS/ACS
functions before searching home.

1444 'The main axes of the transformation must be linear'

DETECTION During execution.
CAUSE One of the main three axes involved in the programmed transformation or kinematics

is neither a linear axis.

SOLUTION The first three axes of the transformation or kinematics must be linear (parameter

AXISTYPE).

1445 'Wrong parameter value'

DETECTION During execution.
CAUSE In a canned cycle, a parameter has the wrong value.
SOLUTION Check the program.

1446 'Starting block not allowed in a local subroutine'

DETECTION During execution.
CAUSE The starting block cannot be a block of a local subroutine.
SOLUTION Select another starting block.

1447 'Software option not allowed'

DETECTION During execution.
CAUSE The CNC does not have the software option required to execute the programmed

command.

SOLUTION In diagnosis mode, it is possible to check the software options offered by the CNC.

1448 'The tool cannot be placed perpendicular to the active plane'

DETECTION During execution.
CAUSE The possible causes are:

• The spindle type does not allow positioning the tool perpendicular to the plane,
as it may be the case of angular spindles.

• Placing the tool perpendicular to the active plane implies exceeding the limits.

SOLUTION Define another plane or position the tool in another point. Use another spindle, if

possible.

CNC 8070

(REF: 1308)

·53·

Error solving manual

1449 '#PATH instruction programmed wrong'

DETECTION During execution.
CAUSE The syntax of the #PATH instruction is wrong.
SOLUTION Check the program.

1450 'Wrong solution for placing spindle perpendicular to the active plane'

DETECTION During execution.
CAUSE The value of the V.G.TOOLORIF1 or V.G.TOOLORIF2 variable is wrong because the

tool cannot be positioned perpendicular to the active plane. The possible causes are:

• The spindle type does not allow positioning the tool perpendicular to the plane,
as it may be the case of angular spindles.

• Placing the tool perpendicular to the active plane implies exceeding the limits.

SOLUTION Define another plane or position the tool in another point. Use another spindle, if

possible.

1451 'Nonexistent variable for the type of axis'

DETECTION During execution.
CAUSE The variable does not exit for the programmed axis type (linear, rotary or spindle).
SOLUTION Check the program.

1452 'Nonexistent variable for the type of drive'

DETECTION During execution.
CAUSE The variable does not exit for the programmed drive type (analog, simulated or

Sercos).

SOLUTION Check the program.

CNC 8070

1453 'Axis name too long'

DETECTION During execution.
CAUSE The axis name has more than two characters.
SOLUTION The axis name is defined by 1 or 2 characters. The first character must be one of the

letters X - Y - Z - U - V - W - A - B - C. The second character is optional and will be
a numerical suffix between 1 and 9. This way, the name of the spindles may be within
the range X, X1…X9,...C, C1…C9.

1455 'PROFILE: Null profile'

DETECTION During execution.
CAUSE The possible causes are:

• In the profile cycle of the cycle editor, the file containing the profile is missing.

• The file indicated in the profile cycle of the cycle editor is empty.

SOLUTION The profile cycle of the cycle editor must indicate the file containing the profile.

1456 '#POLY: Parameters missing'

DETECTION During execution.
CAUSE When programming the #POLY instruction, some required parameter is missing
SOLUTION Check the program.

1457 '#POLY: parameter value'

DETECTION During execution.
CAUSE The possible causes are:

• The interpolation parameters of the polynomial are wrong.

• The curvature radius is less than or equal to zero.

SOLUTION The interpolation parameters of the polynomial must be positive, the starting

parameter of the interpolation (SP) must be smaller than the final parameter (EP) and
the curvature radius must be greater than zero.

(REF: 1308)

·54·

1458 '#POLY: Too many axes have been programmed'

DETECTION During execution.
CAUSE There are more than three axes in the polynomial.
SOLUTION Only three axes can be involved in the polynomial interpolation.

Error solving manual

1459 '#POLY: Wrong starting point'

DETECTION During execution.
CAUSE The starting point of the polynomial is not the same as the current position.
SOLUTION Modify the independent term of the polynomial for each axis making the starting point

of the polynomial the same as the end position of the previous block.

1461 'G9: The arc's intermediate point has been programmed wrong'

DETECTION During execution.
CAUSE One or both coordinates of the arc's intermediate point have not been programmed.
SOLUTION Function G9 requires the programming of both coordinates of the arc's intermediate

point.

1462 'G8: the tangent path cannot be calculated'

DETECTION During execution.
CAUSE An arc tangent to the previous path cannot be done with the programmed radius and

end point.

SOLUTION Check the program.

1463 'G9: Circular path programmed wrong'

DETECTION During execution.
CAUSE No arc can go through those three points.
SOLUTION Define two points in the block with a G9, that define an arc with the end point of the

previous movement. Bear in mind that all three points must be different and cannot
be in line.

1464 'Programmed rotary axis out of the range of the module'

DETECTION During execution.
CAUSE The absolute coordinate (G90) programmed for the MODULE type rotary axis is

wrong.

SOLUTION The coordinate programmed for the axis must be between the limits set by its machine

parameters MODUPLIM and MODLOWLIM.

1465 'Functions RTCP and TLC are incompatible with each other'

DETECTION During execution.
CAUSE The CNC has tried to activate one of the functions while the other one was active.
SOLUTION Both functions cannot be active at the same time.

1466 'G8 cannot be programmed as second motion block for G36/G37/G38/G39'

DETECTION During execution.
CAUSE A G8 block cannot be the second motion block of one of the functions

G36/G37/G38/G39. On one hand, these functions do not have an intermediate block
to make the path joining two blocks and, on the other hand, function G8 does not have
a previous block to be tangent to.

SOLUTION The second motion block of a G36/G37/G38/G39 function must be G0/G1/G2/G3.

1467 'POSLIMIT/NEGLIMIT cannot exceed the value of the machine parameter'

DETECTION During execution.
CAUSE The value to be written in variables V.A.POSLIMIT.xn and V.A.NEGLIMIT.xn cannot

exceed the value of machine parameters POSLIMIT and NEGLIMIT for that axis.

SOLUTION Check the program.

1468 'G30: Polar origin programmed wrong'

DETECTION During execution.
CAUSE One of the two coordinates of the Polar origin is missing in the G30 function.
SOLUTION Check the program. The coordinates of the Polar origin must be programmed in both

main axes.

1469 'Negative or zero radius not allowed'

DETECTION During execution.
CAUSE In a movement in Polar coordinates, the Polar radius is negative or zero.
SOLUTION The Polar radius must always be greater than zero. When programming with

incremental coordinates, the programmed value may be negative or zero, but not the
absolute Polar radius.

CNC 8070

(REF: 1308)

·55·

Error solving manual

1470 'UNIDIR rotary axis programmed wrong in incremental mode'

DETECTION During execution.
CAUSE The incremental coordinate programmed for the unidirectional rotary axis (parameter

UNIDIR) is wrong.

SOLUTION If machine parameter UNIDIR of the rotary axis is POSITIVE, the incremental

coordinate must be programmed with a positive or zero value. If machine parameter
UNIDIR of the rotary axis is NEGATIVE, the incremental coordinate must be
programmed with a negative or zero value.

1471 'G73: Rotation center programmed wrong'

DETECTION During execution.
CAUSE One of the two coordinates of the center of rotation is missing in the G73 function.
SOLUTION Check the program. The coordinates of the rotation center must be programmed in

both main axes.

1472 'G73: The rotation angle has not been programmed'

DETECTION During execution.
CAUSE The rotation angle has not been programmed in function G73.
SOLUTION Check the program. The coordinate system rotation angle must be programmed

together with the coordinates of the rotation center in both main axes.

1473 '#POLY cannot be programmed while pattern rotation is active'

DETECTION During execution.
CAUSE The CNC has tried to execute the #POLY instruction while a coordinate system

rotation (G73) was active.

SOLUTION Check the program.

CNC 8070

(REF: 1308)

1475 'Radius programmed twice'

DETECTION During execution.
CAUSE The radius ("R" or "R1") has been programmed more than one in the same block.
SOLUTION Define only one radius in the block.

1476 'The pocket was resolved with a different tool nose (tip) radius'

DETECTION During execution.
CAUSE The CNC generated the pocket with a tool radius other than the current one.
SOLUTION Generate the pocket again.

1477 'The pocket was resolved with a different tool's cutting length'

DETECTION During execution.
CAUSE The CNC generated the pocket with a tool's cutting length other than the current one.
SOLUTION Generate the pocket again.

1478 'The pocket was resolved with a different tool entry angle'

DETECTION During execution.
CAUSE The CNC generated the pocket with a tool entry angle other than the current one.
SOLUTION Generate the pocket again.

1479 'G74: A subroutine has not been associated'

DETECTION During execution.
CAUSE A G74 function has been programmed alone in the block, but the associated

subroutine does not exist.

SOLUTION Together with function G74, program the axes to be homed or define the associated

subroutine (parameter REFPSUB).

1480 'Program: #EXEC ["path+program",channel]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1481 'Wrong channel number'

DETECTION During execution.
CAUSE Wrong channel number in the instruction #EXEC, #MEET or #WAIT.
SOLUTION The channel number must be between 1 and 4.

·56·

Error solving manual

1483 'Program: #WAIT/#MEET [signal, channel, channel, ...]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1484 'Signal number out of range'

DETECTION During execution.
CAUSE The signal number programmed in the instruction #WAIT, #MEET or #SIGNAL is

wrong.

SOLUTION Check the program.

1485 '#WAIT/#MEET not effective'

DETECTION During execution.
CAUSE The #WAIT or #MEET instruction is not going to generate any wait because the

synchronization mark is programmed for the same channel as the instructions.

SOLUTION Check the program.

1486 'Program: #SIGNAL [signal, signal, signal, ...]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1487 'Program: #CLEAR [signal, signal, signal, ...]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1489 'Axis name repeated in the resulting group'

DETECTION During execution.
CAUSE The #RENAME instruction has tried to rename more than one axis with the same

name.

SOLUTION Rename the axes so there aren't two axes with same name in the channel.

1490 'G63 requires programming M19 before'

DETECTION During execution.
CAUSE The CNC has tried to do a threading G63 with a Sercos spindle without previously

orienting it with M19.

SOLUTION Program M19 before doing the threading.

1491 'Wrong probe number'

DETECTION During execution.
CAUSE The probe number selected with the #SELECT PROBE instruction is wrong.
SOLUTION The selected probe number must be either 1 or 2.

1492 'There is no digital input associated with the probe (PRBDI1/2)'

DETECTION During execution.
CAUSE The CNC has tried to select a probe (#SELECT PROBE) or carry out a probing

movement (G100), but there is no digital probe input associated with the probe.

SOLUTION Associate a digital input with the probe (parameter PRBDI1 or PRBDI2).

1493 '#SPLINE ON, G41/G42 and G136 cannot be programmed at the same time'

DETECTION During execution.
CAUSE The CNC has tried to keep functions #SPLINE ON, G41, G42 and G136 active at the

same time.

SOLUTION Cancel some of these functions.

1494 'Wrong index'

DETECTION During execution.
CAUSE The error number indicated in the #ERROR or #WARNING instruction does not exist.
SOLUTION Check the program.

CNC 8070

(REF: 1308)

·57·

Error solving manual

1495 '#PROBE1: wrong axis for probing cycle'

DETECTION During execution.
CAUSE The PROBE1 cycle issues the error because the main three axes of the current

configuration are not the same as the main three axes of the initial configuration.

SOLUTION Restore the initial configuration of the first three axes of the channel.

1496 '#PROBE1: programming not allowed while #TOOL AX[-] is active'

DETECTION During execution.
CAUSE The CNC has tried to execute the PROBE1 cycle while the tool is oriented in the

negative direction of the axis.

SOLUTION Program #TOOL AX[+] before executing the PROBE1 cycle to orient the tool in the

positive direction of the axis.

1497 'Wrong operator for the type of variable'

DETECTION During execution.
CAUSE The CNC has tried to change a non-numerical variable using the operators "+=", "-

=", "*=" amd "/=".

SOLUTION Check the program.

1499 'Too many nesting levels of #RPT and subroutines'

DETECTION During execution.
CAUSE It is considered nesting when the #RPT instruction is programmed between two labels

that defined the influence area of another #RPT instruction. The CNC issues an error
when exceeding the number of nesting levels of RPT instructions and subroutines,
if any.

SOLUTION The maximum number of nesting levels allowed is 20.

CNC 8070

1500 '#EXEC: the program cannot be executed in the indicated channel'

DETECTION During execution.
CAUSE Using the #EXEC instruction, the CNC has tried to execute a program in a channel

that is in error, is executing another program or is in jog mode and cannot switch into
automatic mode.

SOLUTION Wait for the program to finish in the other channel or reset it.

1501 'Labels repeated in #RPT'

DETECTION During execution.
CAUSE In the #RPT instruction, the starting and finishing labels are the same.
SOLUTION Define different starting and finishing labels.

1502 'The variable requires programming an array index'

DETECTION During execution.
CAUSE It is an array variable and the index has not been indicated.
SOLUTION Check the list of variables in the manuals.

1503 'The variable requires programming an axis'

DETECTION During execution.
CAUSE It is an axis variable and the axis name has not been indicated.
SOLUTION Check the list of variables in the manuals.

1504 'The variable does not allow programming an array index'

DETECTION During execution.
CAUSE The syntax of the variable is wrong.
SOLUTION Check the list of variables in the manuals.

1505 'The variable does not allow programming an axis'

DETECTION During execution.
CAUSE The syntax of the variable is wrong.
SOLUTION Check the list of variables in the manuals.

(REF: 1308)

·58·

Error solving manual

1506 'Undefined label or #RPT command labels swapped'

DETECTION During execution.
CAUSE The possible causes are:

• The second label has not been defined.

• M30 has been programmed between the first and the second labels.

• In the #RPT instruction, the second label has been programmed first and then
the first one.

SOLUTION Check the program.

1507 'The second label of the #RPT must be programmed alone in the block'

DETECTION During execution.
CAUSE In a block repetitions (#RPT), the second label must be programmed alone in the

block without any other type of data.

SOLUTION The last label must be programmed alone in the block. Program the command in the

previous line to execute it with #RPT or in the next line not to execute it with the #RPT.

1508 'G201 and active C axis are not allowed on the axes of the main plane'

DETECTION During execution.
CAUSE The possible causes are:

• One of the axes involved in function G201 is a C axis and is one of the first three
axes of the channel.

• One of the axes programmed in the #FACE instruction is in additive manual mode,
G201.

SOLUTION Cancel the C axis or the additive manual mode.

1509 '#SET AX/#CALL AX: Offset programming has no effect'

DETECTION During execution.
CAUSE All the axes programmed in the instruction already belonged to the current

configuration and, therefore, the instruction only means a change of order
(sequence). In this case, the programmed offset option has no effect.

SOLUTION Check the program.

1510 'The axis does not exist or is not available in the channel'

DETECTION During execution.
CAUSE The possible causes are:

• The CNC has tried to move an axis that does not exist or is not available in the
channel.

• The CNC has tried to execute an instruction that involves an axis that does not
exist or is not available in the channel.

• The CNC has tried to read or write a variable of an axis that does not exist or is
not available in the channel.

SOLUTION Check the program.

1511 'The tool is not in the magazine'

DETECTION During execution.
CAUSE The CNC has tried to use the V.TM.P variable to read the magazine position of a tool

that is not there.

SOLUTION It is only possible to read the position of the tools that are in the magazine.

1512 'Free or nonexistent magazine position'

DETECTION During execution.
CAUSE The CNC has tried to use the V.TM.T variable to read the number of a tool located

in a nonexistent magazine position.

SOLUTION It is only possible to read the tool that is a in valid magazine position.

CNC 8070

(REF: 1308)

·59·

Error solving manual

1513 'Error when writing the variable'

DETECTION During execution.
CAUSE The possible causes are:

• The variable does not exist.

• It is an axis variable, but the axis does not exist.

• It is an axis variable, but it does not exit for the axis type (linear or rotary).

• It is an axis variable, but it does not exist for the type of drive of the axis.

• The combined operator (+= -= *= /=) is not admitted for that variable.

• The value of the variable is not valid.

SOLUTION Check the program.

1514 'A 2D-3D pocket cannot be executed while G72 is active'

DETECTION During execution.
CAUSE The CNC has tried to execute the pocket with an active scaling factor.
SOLUTION Cancel the scaling factor.

1515 'One or several axes of the original configuration are not available'

DETECTION During execution.
CAUSE A channel has released an axis with a temporary change permission (parameter

AXISEXCH) and cannot restore it with a reset or at the beginning of a program
because the channel that took it has not released (freed) it.

SOLUTION The other channel will release the axis with reset or with the beginning of another

program. The axis release can also be programmed with the instruction #FREE AX.

CNC 8070

(REF: 1308)

1516 'Value expected'

DETECTION During execution.
CAUSE The list of subroutine calling parameters (with #PCALL or G180-189) has been

programmed wrong.

SOLUTION Check the program.

1518 'NR requires programming a movement in the block'

DETECTION During execution.
CAUSE A repetition blocks (NR) has been programmed in a block that does not involve a

movement.

SOLUTION Programming block repetition with NR is only valid with blocks that involve a

movement. The repetition of other types of blocks must be programmed using flow
controlling instructions offered by the CNC.

1519 'NR: M/T/D/H cannot be programmed in the same block'

DETECTION During execution.
CAUSE A repetition blocks (NR) has been programmed in a block that contains an M, T, D

or H function.

SOLUTION Programming block repetition with NR is only valid with blocks that involve a

movement. The repetition of other types of blocks must be programmed using flow
controlling instructions offered by the CNC.

1520 'NR: $GOTO cannot be programmed in the same block'

DETECTION During execution.
CAUSE A repetition blocks (NR) has been programmed in a block that contains the $GOTO

instruction.

SOLUTION Programming block repetition with NR is only valid with blocks that involve a

movement. The repetition of other types of blocks must be programmed using flow
controlling instructions offered by the CNC.

1521 'NR: A call to a subroutine cannot be programmed in the same block'

DETECTION During execution.
CAUSE A repetition of blocks (NR) has been programmed in a block that contains a call to

a subroutine (L, LL, #CALL, #PCALL, #MCALL or G180-G189).

SOLUTION Programming block repetition with NR is only valid with blocks that involve a

movement. The repetition of other types of blocks must be programmed using flow
controlling instructions offered by the CNC.

·60·

Error solving manual

1522 'Negative value not allowed'

DETECTION During execution.
CAUSE A negative number of block repetitions (NR) has been programmed.
SOLUTION Check the program.

1523 'POS and T must be programmed in the same block'

DETECTION During execution.
CAUSE The tool T and the position POS has not been programmed in the same block.
SOLUTION The tool T and the position it must be occupied in the magazine must be programmed

in the same block.

1525 'The axis cannot be exchanged'

DETECTION During execution.
CAUSE The CNC has tried to change a channel axis (#CALL, #SET oR #FREE) and the axis

does not have permission to change (parameter AXISEXCH).

SOLUTION In order for the CNC to be able to change the channel axes and spindles, they must

have permission. Parameter AXISEXCH sets whether the axis or the spindle has
permission to change channels and if it does, whether the change is temporary or
permanent; in other words, whether the change is maintained after an M02, M30, a
reset or after restarting the CNC.

1526 '#EXEC: the indicated channel is not a CNC channel'

DETECTION During execution.
CAUSE The CNC has tried to use the #EXEC instruction to execute a program in a channel

that is not a CNC channel, but a PLC channel.

SOLUTION Check the program.

1527 'Wrong identifier after %'

DETECTION During execution.
CAUSE In the instruction #MSG, #ERROR or #WARNING, an invalid identifier has been

programmed.

SOLUTION The valid identifiers are %D or %d to display a number and %% to display the

character "%".

1529 'Expecting list of identifiers or "]" after end-quotes'

DETECTION During execution.
CAUSE In the instruction #MSG, #ERROR or #WARNING , an invalid character has been

programmed after the message to be displayed.

SOLUTION Check the program. After the end-quotes of the message to be displayed, it only

admits the list of variables or parameters to be included in the text.

1530 'G53 cannot be programmed with polar coordinates'

DETECTION During execution.
CAUSE The final point has been defined with Polar or Cylindrical coordinates in function G53.
SOLUTION When programming referred to machine zero (home), the points must be defined only

with Cartesian coordinates.

1531 'Program: #EXBLK [block, channel]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1532 'Program: #MASTER <spindle name>'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1533 'Program: #FREESP [sp1, sp2, ..]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

CNC 8070

(REF: 1308)

·61·

Error solving manual

1534 'Program: #CALLSP [sp1, sp2, ..]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1535 'Program: #SETSP [sp1, sp2, ..]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

1538 'A spindle cannot be restored from the channel'

DETECTION During execution.
CAUSE A channel has released a spindle with a temporary change permission (parameter

AXISEXCH) and cannot restore it with a reset or at the beginning of a program
because the channel that took it has not released (freed) it.

SOLUTION The other channel will release the spindle with reset or with the beginning of another

program. The spindle release can also be programmed with the instruction #FREE
SP.

1539 'Spindle name repeated in the resulting group'

DETECTION During execution.
CAUSE The #RENAME instruction has tried to rename more than one spindle with the same

name.

SOLUTION Rename the spindles so there aren't two with same name in the channel.

CNC 8070

(REF: 1308)

1540 'Programming not allowed without a master spindle in the channel'

DETECTION During execution.
CAUSE The possible causes are:

• The CNC has tried to read or write a variable of the master spindle, but it does
not exist in the channel.

• The G function or instruction cannot be executed if there is no master spindle in
the channel.

SOLUTION Define a master spindle for the channel

1541 'The spindle cannot be eliminated while the C axis is active'

DETECTION During execution.
CAUSE The CNC has tried to eliminate from the channel (#FREE or #SET) a spindle that is

working as C axis.

SOLUTION Deactivate the C axis before eliminating the spindle from the channel.

1542 'The spindle cannot be exchanged'

DETECTION During execution.
CAUSE The CNC has tried to change a channel spindle (#CALL, #SET oR #FREE) and the

spindle does not have permission to change (parameter AXISEXCH).

SOLUTION In order for the CNC to be able to change the channel axes and spindles, they must

have permission. Parameter AXISEXCH sets whether the axis or the spindle has
permission to change channels and if it does, whether the change is temporary or
permanent; in other words, whether the change is maintained after an M02, M30, a
reset or after restarting the CNC.

1544 'G63 and M3/M4/M5/M19/M41-M44 not allowed in the same block'

DETECTION During execution.
CAUSE No M function associated with the spindle may be programmed in the same block that

contains a rigid tapping G63.

SOLUTION It may be programmed either in the previous or next block depending on the result

to be obtained. If programmed in the next block, these M functions cancel the modal
tapping G63 in such way that G63 must be programmed again in the next movement
in order to keep tapping.

·62·

Error solving manual

1545 'Spindle gear change is not possible while G63 or #CAX is active'

DETECTION During execution.
CAUSE The CNC cannot change the spindle gear if tapping G63 is active or the spindle is

working as C axis.

SOLUTION Deactivate the threading and the C axis to change the spindle gear.

1546 'G63 not allowed without prior gear at the spindle'

DETECTION During execution.
CAUSE This situation is only possible if after a system power-up or a reset, the PLC does not

indicate any gear with GEAR1 through GEAR4 for the spindle. Then, the spindle has
no active gear and if it is not used before programming G63, the CNC will not generate
a gear automatically, either.

SOLUTION Before starting a G63 tapping, the spindle must have a gear activated. If the spindle

has an automatic gear changer (parameter AUTOGEAR), the CNC generates the
gear when programming a speed; otherwise, the gear (M41-M44) must be
programmed with the speed.

1547 '#CAX not allowed while G63 is active'

DETECTION During execution.
CAUSE A spindle cannot be activated as C axis if it is being used by function G63.
SOLUTION Cancel G63 before deactivating the C axis or use another spindle of the channel for

the C axis.

1548 'The master spindle cannot be changed while G33/G63/G95/G96 are active'

DETECTION During execution.
CAUSE Function G63 and G96 use the master spindle of the channel. The cannel cannot

eliminate this spindle while the functions are active.

SOLUTION Cancel G63 or G96 before releasing the spindle.

1549 'Null or wrong pocket name'

DETECTION During execution.
CAUSE When a 2D or 3D pocket has been defined with the cycle editor, the pocket name has

not been defined or its name is wrong. The pocket name cannot be #DATAP2D or
#DATAP3D generated by the cycle editor.

SOLUTION Assign a different name to the pocket.

1550 'Two C axes cannot be programmed in the same channel'

DETECTION During execution.
CAUSE The CNC has tried to activate a C axis while another one was active.
SOLUTION Deactivate a C axis before activating another one.

1551 'Too many local parameter nesting levels'

DETECTION During execution.
CAUSE The nesting of subroutine calls with #PCALL or with function G1-G190 increases the

nesting level of the local parameters. The error comes up because the maximum
nesting level (7) of local parameters has been exceeded.

SOLUTION Decrease the nesting of subroutines or use the instructions #CALL, L or LL to call

them; they do not increase the nesting level of local parameters.

1552 'The name of the variable must begin with a "V."

DETECTION During execution.
CAUSE The name of a variable has been written from a part program or MDI without the

starting prefix "V."

SOLUTION Add the prefix "V." to the name of the variable.

1553 'Too many user variables'

DETECTION During execution.
CAUSE The CNC has exceeded the maximum number of user variables (prefixes P and S)

admitted.

SOLUTION The maximum number of user variables admitted is 20.

CNC 8070

(REF: 1308)

·63·

Error solving manual

1554 'The PLC has not recognized the START in a #EXEC instruction'

DETECTION During execution.
CAUSE When giving the order to execute a program in another channel, the PLC must give

the "go ahead" to the program start-up (START) If it doesn't give this go-ahead, it will
issue this error.

SOLUTION Check the PLC program.

1555 'Program #MOVE / #MOVE ABS/ADD/INF[...]'

DETECTION During execution.
CAUSE The syntax of the #MOVE instruction is wrong.
SOLUTION Check the program. Together with the instruction, program one of the commands

ABS/ADD/INF and then the call parameters between square brackets.

1556 'Program type of link: PRESENT, NEXT, NULL, WAITINPOS'

DETECTION During execution.
CAUSE In the #MOVE instruction, the type of transition between movements is wrong.
SOLUTION Check the program.

1557 'Program #CAM ON/OFF/SELECT/DESELECT[...]'

DETECTION During execution.
CAUSE The syntax of the #CAM instruction is wrong.
SOLUTION Check the program. Together with the instruction, program one of the commands ON,

OFF, SELECT or DESELECT and then the call parameters between square brackets.

1558 'Wrong cam number'

DETECTION During execution.
CAUSE In the #CAM instruction, the cam number is wrong.
SOLUTION The cam number must be between 1 and NLEVAS.

1559 'Program type of cam: ONCE or CONT'

DETECTION During execution.
CAUSE In the #CAM instruction, the cam type is wrong; the cam type is defined with the

commands ONCE (non-periodic cam) and CONT (periodic cam).

SOLUTION Check the program.

1560 'Program #FOLLOW ON/OFF[...]'

DETECTION During execution.
CAUSE The syntax of the #FOLLOW instruction is wrong.
SOLUTION Check the program. Together with the instruction, program one of the commands

ON/OFF and then the call parameters between square brackets.

1561 'Invalid master axis'

DETECTION During execution.
CAUSE In the #CAM or #FOLLOW instruction, the master axis is wrong.
SOLUTION The axis must belong to the channel.

1562 'Invalid slave axis'

DETECTION During execution.
CAUSE In the #CAM or #FOLLOW instruction, the slave axis is wrong.
SOLUTION The axis must belong to the channel.

CNC 8070

(REF: 1308)

·64·

1563 'Function G74 must be programmed with axes or alone in the block'

DETECTION During execution.
CAUSE Function G74 has been programmed wrong.
SOLUTION Function G74 may be programmed either with the axes to be homed or alone in the

block. If function G74 is programmed alone in the block, the CNC executes its
associated subroutine (parameter REFPSUB).

1564 'A parked axis cannot be programmed'

DETECTION During execution.
CAUSE The programmed instruction cannot be executed on a parked axis.
SOLUTION Check the program.

Error solving manual

1565 'The spindle cannot work as C axis, CAXIS = No'

DETECTION During execution.
CAUSE The #CAX instruction contains a spindle that does not have permission to work as

C axis (parameter CAXIS).

SOLUTION Check the program.

1566 'Mirror image is not admitted with UNIDIR axes'

DETECTION During execution.
CAUSE Mirror image cannot be programmed on a unidirectional rotary axis (parameter

UNIDIR), because this type of axes cannot rotate in the opposite direction to the one
defined.

SOLUTION Change the type of axis or do not program the mirror image.

1567 'The Polar radius can only be programmed with R'

DETECTION During execution.
CAUSE The radius of a movement in Polar coordinates is programmed with parameter R1

or with function G263.

SOLUTION Program the Polar radius with parameter R.

1568 'Wrong tool magazine number'

DETECTION During execution.
CAUSE Wrong tool magazine number defined in the MZ command.
SOLUTION The tool magazine number must be a value between 1 and 4.

1569 'Execution not admitted, the channel is exclusive to the PLC'

DETECTION During execution.
CAUSE When the channel is a PLC channel only, the CNC does not have permission to

execute in it programs, MDI blocks, jog movements or any other action from the jog
mode.

SOLUTION To execute those actions in that channel, it must be configured as a CNC channel

or as CNC+PLC channel (parameter CHTYPE).

1570 'G74 and simultaneous spindle movement not allowed'

DETECTION During execution.
CAUSE An M function for spindle movement and function G74 (home search) have been

programmed in the same block.

SOLUTION Check the program.

1571 'The "%" character is not allowed inside a global subroutine'

DETECTION During execution.
CAUSE A global subroutine contains the "%" character in a line other than the one defining

the name of the subroutine.

SOLUTION Check the program.

1572 'Variable that can only be accessed by its channel'

DETECTION During execution.
CAUSE The CNC has tried to access a tool preparation variable of another channel (prefix

"G" or "A").

SOLUTION The only tool variables that can be accessed from another channel are the ones

associated with the tool manager (prefix "TM").

1573 'Error when capturing samples of the variable'

DETECTION During execution.
CAUSE An error occurred while the oscilloscope tried to read the value of the variable

assigned to one of its channels.

SOLUTION Reset the CNC and capture the trace again.

1574 'Parameter that cannot be modified from the oscilloscope'

DETECTION During execution.
CAUSE The user has tried to modify from the screen of the oscilloscope a machine parameter

that does not have a writing permission.

SOLUTION This parameter can only be modified from the machine parameters table.

CNC 8070

(REF: 1308)

·65·

Error solving manual

1575 'Instruction only valid in programs with extension FBS'

DETECTION During execution.
CAUSE Programming of instruction #SPLINE or #BSPLINE.
SOLUTION These instructions are only valid in programs with extension fbs'

1576 '"]"not expected'

DETECTION During execution.
CAUSE Syntax error in the instruction.
SOLUTION Check the program.

1577 'Program type of synchronization: VEL or POS'

DETECTION During execution.
CAUSE The parameter that defines the type of synchronization in the #FOLLOW instruction

is wrong.

SOLUTION Check the program. The parameter can take the values VEL (velocity) and POS

(position).

1578 '#LINK: A UNIDIR slave axis must be of the same type as the master (UNIDIR)'

DETECTION During execution.
CAUSE The CNC has tried to activate a coupling (#LINK) with two unidirectional rotary axes

that are not identical.

SOLUTION When the axes are unidirectional, both axes must be set with the same turning

direction (parameter UNIDIR).

1579 'Home search not allowed on a master axis with several slave axes'

DETECTION During execution.
CAUSE The CNC has executed a G74 function on the master axis of a coupling with several

slaves.

SOLUTION Undo the axis coupling (slaving) and home the axes separately.

1580 '#CAX: Requires previously programming M19 in position sercos'

DETECTION During execution.
CAUSE The CNC has tried to activate a Sercos spindle as C axis without previously orienting

it with M19.

SOLUTION Program M19 before activating the spindle as C axis.

1581 'An active C axis cannot be eliminated'

DETECTION During execution.
CAUSE Instructions #SET AX and #FREE AX cannot eliminate the C axis from the

configuration if it is active.

SOLUTION Deactivate the C axis before eliminate it from the configuration.

1582 'NR: The number of repetitions has been programmed twice'

DETECTION During execution.
CAUSE The NR instruction has been programmed more than once in the same block.
SOLUTION Check the program.

1583 '#FOLLOW ON: The master and slave axes cannot be the same ones'

DETECTION During execution.
CAUSE The master and slave axes are the same axis.
SOLUTION Check the program.

CNC 8070

(REF: 1308)

·66·

1584 '#FOLLOW ON: the numerator and denominator must be integers'

DETECTION During execution.
CAUSE The numerator and/or denominator are programmed with decimals.
SOLUTION Program integers in the parameters that define the numerator and denominator of

the gear ratio.

Error solving manual

1585 'The axes of the active transformation cannot be temporarily swapping axes'

DETECTION During execution.
CAUSE The axes of the transformed cannot be temporary-exchange axes because the

defined transform stays active once activated.

SOLUTION If possible, define the axes as maintained exchange; otherwise, use other axes for

the transform. The temporary-exchange axes can only be used in their channel and
when the axes are in their original positions inside the channel.

Temporary-exchange axes may be used in the #FACE and #CYL transforms because
these transforms are canceled with M30 and after a reset.

1586 'The magazine number (MZ) has not been programmed yet'

DETECTION During execution.
CAUSE In a system with several magazines, the tool and the position have been programmed

in the same block, but not the tool magazine where that tool is to be placed.

SOLUTION In a multi-magazine system, the tool, the position and the magazine must be

programmed in the same block.

1587 'This parameter cannot be modified from setup'

DETECTION During execution.
CAUSE The machine parameter has no permission to be written from a setup environment.
SOLUTION The machine parameter can be modified directly at the machine parameters table.

1588 'The slave spindle to be synchronized must belong to the channel'

DETECTION During execution.
CAUSE The master spindle of a synchronization may belong to any channel, but the slave

spindle must belong to the channel where the synchronization is programmed.

SOLUTION Synchronize the slave spindle from its channel, add it to the current channel

configuration or use another spindle of the channel as slave.

1589 'The slave spindle cannot be the same as the master'

DETECTION During execution.
CAUSE In the synchronization, the slave axis is the same as the master axis.
SOLUTION Check the program.

1590 'Program #SYNC[Sm,Ss,Nx,Dx,Ox,CLOOP/OLOOP,CANCEL/NOCANCEL]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program.

1591 'Wrong numerator'

DETECTION During execution.
CAUSE In spindle synchronization, the value of the numerator of a gear ratio is wrong; zero,

for example.

SOLUTION The value may be positive or negative, not necessarily an integer, but must be other

than zero.

1592 'Wrong denominator'

DETECTION During execution.
CAUSE In spindle synchronization, the value of the denominator of a gear ratio is wrong; zero,

for example.

SOLUTION The value may be positive or negative, not necessarily an integer, but must be other

than zero.

1593 'The slave spindle to be desynchronized must belong to the channel'

DETECTION During execution.
CAUSE A channel cannot cancel the synchronization of a slave spindle that belongs to

another channel.

SOLUTION Cancel the synchronization from the channel that the spindle belongs to.

CNC 8070

1594 'The slave spindle is already synchronized with another spindle'

DETECTION During execution.
CAUSE The slave spindle is already synchronized with another spindle.
SOLUTION A spindle can only be the slave of one master. Cancel the previous synchronization

or synchronize another spindle that is available.

(REF: 1308)

·67·

Error solving manual

1595 'A spindle cannot be master and slave of a synchronization at the same time'

DETECTION During execution.
CAUSE The slave spindle of a synchronization is the master spindle of another one.
SOLUTION Check the program.

1596 'The spindle is not synchronized'

DETECTION During execution.
CAUSE The CNC has tried to desynchronize a slave spindle that is not currently

synchronized.

SOLUTION Check the program.

1597 'A slave spindle cannot be synchronized with two masters'

DETECTION During execution.
CAUSE A slave spindle cannot be synchronized with two masters at the same time.
SOLUTION Decide which of the two synchronizations you wish to activate.

1598 'A slave spindle cannot be programmed during synchronization'

DETECTION During execution.
CAUSE An S speed or an M function has been programmed for the slave axis of a

synchronization.

SOLUTION Delete those data from the program or desynchronize the spindle.

1599 'Gear change is not possible on synchronized spindles'

DETECTION During execution.
CAUSE While synchronizing two spindles, the CNC does not allow a gear change in any of

them.

SOLUTION Cancel the synchronization to change the spindle gear.

CNC 8070

1600 'A synchronized spindle cannot work as C axis or in G63'

DETECTION During execution.
CAUSE The CNC has tried to synchronize a spindle that is either working as C axis or has

function G63 active. The CNC has tried to activate the spindle as C axis or function
G63, but the spindle is synchronized.

SOLUTION Cancel the C axis or function G63 to synchronize the spindles. To work with the C

axis or with function G63, cancel the spindle synchronization.

1601 'A synchronized spindle cannot be released (freed)'

DETECTION During execution.
CAUSE Instructions #SET SP and #FREE SP cannot eliminate a spindle if it is synchronized.
SOLUTION Cancel the synchronization to eliminate the spindle from the configuration.

1602 'To park a spindle, it must be stopped (M5)'

DETECTION During execution.
CAUSE The CNC has tried to park a spindle that is not stopped.
SOLUTION Stop the spindle before parking it.

1603 'FOLLOW OFF: Program slave axis'

DETECTION During execution.
CAUSE The programmed axis is not slave in any synchronization.
SOLUTION Check the program.

1604 'G31 requires G02/G03 active'

DETECTION During execution.
CAUSE Function G31 can only be programmed if a circular interpolation is active.
SOLUTION Program G02/G03 in the G31 block.

(REF: 1308)

·68·

1605 'G31 requires programming the polar angle and its interpolation center'

DETECTION During execution.
CAUSE The Polar angle or some coordinate of the center is missing in function G31.
SOLUTION Check the program.

Error solving manual

1606 '#ANGAX: The angular and orthogonal axes must belong to the same channel'

DETECTION During execution.
CAUSE The CNC has tried to activate an angular transformation with two axes that do not

belong to the same channel.

SOLUTION The axes of an angular transformation must belong to the same channel.

1607 'Executing a milling cycle requires three axes in the channel'

DETECTION During execution.
CAUSE A milling cycle has been programmed in a channel with less than three axes or the

longitudinal axis does not exist.

SOLUTION Executing milling cycles requires three axes in the channel.

1608 'The variable cannot be consulted. Assign the value of the variable to Pn and consult Pn'

DETECTION During execution.
CAUSE Particular CNC commands and instructions do not admit reading variables that imply

a synchronization between block preparation and execution.

SOLUTION To avoid this error, assign the value of the variable to a local arithmetic parameter and

read this parameter when necessary.

1609 'Executing a turning cycle requires two axes in the channel'

DETECTION During execution.
CAUSE A lathe cycle has been programmed in a channel with less than two axes or the first

axis is not longitudinal (parameter LONGAXIS) or the second one is not a face axis
(parameter FACEAXIS).

SOLUTION Executing lathe cycles requires two axes in the channel.

1610 'A SERCOS master spindle in POSITION does not admit CLOOP'

DETECTION During execution.
CAUSE A spindle configured as position-Sercos cannot be synchronized in closed loop.
SOLUTION Use another spindle as master.

1611 'On the LATHE XZ model the active plane does not change'

DETECTION During execution.
CAUSE The CNC has tried to change the work plane in a lathe having a plane-type axis

configuration.

SOLUTION On a lathe having a plane-type axis configuration, the active plane is always G18.

To only change the longitudinal axis, use function G20.

1612 'The axes of the active angular transformation, #ANGAX, cannot be excluded'

DETECTION During execution.
CAUSE The CNC has tried to eliminate from the channel the axes that made up the angular

transformation.

SOLUTION Cancel the angular transformation before eliminating the axes of the channel.

1613 'The angular transformation #ANGAX has been canceled'

DETECTION During execution.
CAUSE The CNC has eliminated from the channel the axes that made up the angular

transformation and the latter has been canceled.

SOLUTION The angular transformation is canceled; to activate it, put in the channel again the

axes that make up the angular transformation.

1614 'It cannot be programmed while the angular transformation #ANGAX is active'

DETECTION During execution.
CAUSE The CNC has tried to execute a function incompatible with the angular transformation,

for example a home search (G74), modify the software limits (G198 - G199), #OSC
instruction.

SOLUTION Cancel the active angular transformation to execute the incompatible functions.

1615 'The axis cannot be activated as Hirth, because it is part of the #ANGAX transformation'

DETECTION During execution.
CAUSE The CNC has tried to activate a hirth axis that belongs to the active angular

transformation.

SOLUTION Cancel the angular transformation to activate the hirth axis.

CNC 8070

(REF: 1308)

·69·

Error solving manual

1616 'G31 does not allow programming the polar radius'

DETECTION During execution.
CAUSE A Polar radius has been defined for function G31.
SOLUTION Function G31 does not allow programming the Polar radius. Function G31 only admits

Polar coordinates like G31 Q I J; i.e. programming the angle and one or both center
coordinates.

1617 'Q index not allowed'

DETECTION During execution.
CAUSE The index of parameter Q is wrong; it only admits Q or Q1.
SOLUTION Check the program. When programming in Polar coordinates, use parameter Q. For

function G33, use parameter Q1.

1618 'Q value programmed twice'

DETECTION During execution.
CAUSE The Q parameter has been programmed more than once in the same block.
SOLUTION Check the program.

1619 'Q1 value programmed twice'

DETECTION During execution.
CAUSE The Q1 parameter has been programmed more than once in the same block.
SOLUTION Check the program.

CNC 8070

(REF: 1308)

1620 '#SERVO ON not admitted for POSITION-SERCOS axis or spindle'

DETECTION During execution.
CAUSE Axis or spindle is position Sercos.
SOLUTION This instruction only admits velocity-Sercos axes.

1621 'Q1 not admitted without G33 in the block or G32 active'

DETECTION During execution.
CAUSE A parameter Q1 has been programmed without G33 in the block or without function

G63 being active'

SOLUTION Parameter Q must go in the same block as G33. Parameter Q can only go alone in

the block if function G63 is active.

1622 'A temporary-exchange spindle cannot work as maintained C axis'

DETECTION During execution.
CAUSE The CNC can activate a temporary-exchange spindle as maintained C axis

(parameter PERCAX).

SOLUTION If possible, define the spindle as maintained exchange; otherwise, use another

spindle as C axis.

1623 'Invalid set for synchronization SYNCSET'

DETECTION During execution.
CAUSE Parameter SYNCSET has the wrong value.
SOLUTION Assign a correct value to the parameter.

1624 'Program #TANGCTRL ON/OFF/SUSP [ ]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. Together with the instruction, program one of the commands

ON/SUSP/OFF and then the call parameters between square brackets. It is also
possible to program one of the SUSP/OFF commands without call parameters.

1625 'An axis in active tangential control must be rotary, non-HIRTH and it must not belong to

the active trihedron'

DETECTION During execution.
CAUSE The axes to activate in tangential control must be rotary, not hirth and must not belong

to the active trihedron nor be the longitudinal axis.

SOLUTION Check the program.

·70·

Error solving manual

1626 'Program axis for #TANGCTRL ON/OFF/SUSP/RESUME'

DETECTION During execution.
CAUSE The axis or axes are missing in the instruction.
SOLUTION Check the program.

1627 '#TANGCTRL: program angle values between 0 and ±359.9999'

DETECTION During execution.
CAUSE The angle programmed in the instruction is wrong.
SOLUTION Check the program. The angle value must be between 0 and ±359.9999.

1628 'An axis cannot be eliminated from the configuration while tangential control is active'

DETECTION During execution.
CAUSE The CNC cannot eliminate the tangential axis from the configuration if tangential

control is active.

SOLUTION Cancel the tangential control to eliminate this axis from the configuration.

1629 'Only one axis can be programmed in tangential control'

DETECTION During execution.
CAUSE Tangential control being active, a movement or another operation has been

programmed for the tangential axis.

SOLUTION Tangential control being active, it is not possible to program movements of the

tangential axis; it is up to the CNC to orient this axis. To use this axis, cancel the
tangential control.

1630 'The profile has been programmed wrong with labels'

DETECTION During execution.
CAUSE In the call to the cycle, the parameters that define the beginning and end of the profile

(parameters S and E) have been defined wrong.

SOLUTION Assign the correct values to parameters S and E.

1631 'Profile programming not allowed' [S,E,<Q>] or [P,<Q>]'

DETECTION During execution.
CAUSE In the call to the cycle, the parameters that define the beginning and end of the profile

(parameters S and E), the subroutine that contains the profile (parameter P) or the
file that contains the profile (parameter Q) have been defined wrong.

SOLUTION Check the program.

1632 'An axis in active tangential control must be rotary with 360º module'

DETECTION During execution.
CAUSE The CNC has tried to activate the tangential control on a rotary axis with a module

other than 360º.

SOLUTION Tangential control can only be activated on rotary axes with 360º module. The upper

limit of the module is determined by parameter MODUPLIM and the lower limit by
parameter MODLOWLIM.

1633 'Program: #DGSPSL <spindle name>'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program.

1634 'The #MOVE instruction only admits one axis and it must belong to the channel'

DETECTION During execution.
CAUSE The programmed axis name is wrong, the axis is in another channel or it is an axis

of the system. Spindles cannot be programmed except when they are working as C
axis, in which case, they must be programmed with the name of the C axis.

SOLUTION Check the program.

1635 'There are too many axes in the transformation'

DETECTION During execution.
CAUSE There are more axes defined in parameter NKINAX of the coordinate transformation

than allowed at the CNC.

SOLUTION Correct machine parameter NKINAX.

CNC 8070

(REF: 1308)

·71·

Error solving manual

1636 'The FACE and CYL transforms cannot be active at the same time'

DETECTION During execution.
CAUSE The CNC has tried to activate the #FACE or #CYL instruction while one of them was

active.

SOLUTION Deactivate one of them before activating the other one.

1637 'Spindle turning direction incompatible with the tool'

DETECTION During execution.
CAUSE The pre-established tool rotating direction is incompatible with the current turning

direction of the spindle.

SOLUTION Change the spindle turning direction or correct the turning direction defined for the

tool.

1638 'The axes of the angular transform, #ANGAX, must be linear'

DETECTION During execution.
CAUSE The CNC has tried to activate an angular transformation with a rotary axis.
SOLUTION The axes of the angular transformation must be linear.

1639 'The programmed spindle does not belong to the channel'

DETECTION During execution.
CAUSE The CNC has tried to use a spindle of another channel.
SOLUTION A channel can only control its spindles. Use a spindle that belongs to the channel o

include in the channel configuration the spindle causing the error.

1640 'Parked spindles cannot be programmed'

DETECTION During execution.
CAUSE The CNC has tried to use a parked spindle.
SOLUTION Use a spindle that is not parked or unpark it.

1641 '#CYL: Expecting the programming of the cylinder development radius'

DETECTION During execution.
CAUSE The value of the developing radius is missing in the #CYL instruction.
SOLUTION Check the programming for a variable radius, define a zero value so the CNC

calculates the radius depending on the position of the tool.

1642 'Slaved TANDEM spindles cannot be programmed'

DETECTION During execution.
CAUSE The user has tried to move or home the slave spindle of a tandem pair.
SOLUTION The slave spindle of a tandem pair is controlled by the CNC, it cannot be moved

individually. To move a slave spindle, move the master spindle it is associated with.

1643 'TANDEM spindles cannot be parked'

DETECTION During execution.
CAUSE The CNC has tried to park a spindle that belongs to a tandem pair.
SOLUTION Tandem spindles cannot be parked.

1644 'Spindles cannot be parked in G33/G95'

DETECTION During execution.
CAUSE The CNC has tried to park a spindle while function G33 or G95 was active.
SOLUTION Cancel G33 and G95 before parking a spindle.

CNC 8070

(REF: 1308)

·72·

1645 '#RET/M17/M29 not allowed between the labels of a #RPT'

DETECTION During execution.
CAUSE The CNC has detected an M17, M29 function or #RET between the first and last labels

of a repetition of blocks #RPT.

SOLUTION A subroutine cannot end inside a repetition of blocks.

1646 'Program: #ABORT [label]/#ABORT Nxxxx/#ABORT OFF'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. The instructions must be programmed alone in the block, only

the block label may be added.

Error solving manual

1647 'The gear does not exist in the TANDEM slave'

DETECTION During execution.
CAUSE A gear change has been programmed in a tandem axis or spindle. The gear exists

in the master axis or spindle, but not in the slave.

SOLUTION Define the same gears on the master and slave axes and spindles of the tandem.

1649 'User reverse transformation function not found'

DETECTION During execution.
CAUSE The PcsToMcs coordinates function is missing when trying to do a transformation

from part coordinates to machine coordinates in a user kinematics.

SOLUTION Check the user kinematics integration process.

1650 'User direct transformation function not found'

DETECTION During execution.
CAUSE The McsToPcs coordinates function is missing when trying to do a transformation

from machine coordinates to part coordinates in a user kinematics.

SOLUTION Check the user kinematics integration process.

1651 'Maintained LINK not admitted with temporary axes of another channel'

DETECTION During execution.
CAUSE The CNC cannot couple axes with temporary exchange permission (parameter

AXISEXCH) if they belong to another channel and the couplings of the channel are
defined as maintained (parameter LINKCANCEL).

SOLUTION Couple the axes in their channel.

1653 'An axis of the inclined plane transformation cannot be a slave'

DETECTION During execution.
CAUSE The CNC has tried to define as slave of a coupling an axis that belongs to the inclined

plane.

SOLUTION Cancel the inclined plane to be able to activate the coupling. An axis that belongs to

the inclined plane cannot be the slave axis of a coupling; but the master of a coupling
can.

1654 'Digital bus (Sercos/Mechatrolink)not ready for reading the variable'

DETECTION During execution.
CAUSE With the Sercos bus, the ring is not in phase 4. With the Mechatrolink bus, the bus

has not reached phase 3.
The Sercos ring is not in phase 4.

SOLUTION Condition the writing of the variable to the SERCOSRDY mark in Sercos or to the

MLINKRDY mark in Mechatrolink.

1655 'Digital bus (Sercos/Mechatrolink)not ready for writing the variable'

DETECTION During execution.
CAUSE With the Sercos bus, the ring is not in phase 4. With the Mechatrolink bus, the bus

has not reached phase 3.

SOLUTION Condition the writing of the variable to the SERCOSRDY mark in Sercos or to the

MLINKRDY mark in Mechatrolink.

1656 'Some axis of the plane is set in diameters'

DETECTION When simulating or executing on a lathe a milling canned cycle that contains

movements in the axes of the plane.

CAUSE The coordinate data of the milling canned cycles will be considered in radius. If any

of the axes of the plane is in diameters, the CNC interprets its data as radius and

warns the user in case he was programming them in diameters.
CONSEQUENCE The cycle can execute a different geometry than expected.
SOLUTION Program the data in radius.

CNC 8070

1657 'Wrong variable for spindle that is not a C axis'

DETECTION During execution.
CAUSE The CNC has tried to read an axis variable, but the spindle is activated as C axis.
SOLUTION The variable only exists for axes and spindles working as C axis.

(REF: 1308)

·73·

Error solving manual

1658 'Wrong magazine number'

DETECTION During execution.
CAUSE The magazine number is wrong.
SOLUTION Check the program. The number of magazine is set in parameter NTOOLMZ.

1659 'Macro previously defined with #DEF FIX'

DETECTION During execution.
CAUSE The macro already exists; it was defined with the command #DEF FIX. Remember

that the macros table is not initialized with the beginning and end of program, only
with the instruction #INIT MACROTAB.

SOLUTION Define the macro with a different name. The macros defined using the command

#DEF FIX are not deleted after a reset. Use the command #INIT MACROTAB to reset
the whole table of macros; it erases the macros that have been defined with #DEF
and with #DEF FIX.

1660 'Wrong array index'

DETECTION During execution.
CAUSE Some array index programmed in the variable is out of range.
SOLUTION Check the program. Check the variable and its range of values.

1661 'The "." is missing after [ChannelNumber]'

DETECTION During execution.
CAUSE The channel number must be between square brackets and followed by a ".".
SOLUTION Check the program. Check the syntax of the variable.

CNC 8070

(REF: 1308)

1662 'Unknown variable type'

DETECTION During execution.
CAUSE The programmed variable type does not exist.
SOLUTION Check the program. Check the syntax of the variable.

1663 '#DELETE: the variable(s) to be deleted is (are) missing'

DETECTION During execution.
CAUSE The variable(s) to be deleted is (are) missing in the #DELETE instruction.
SOLUTION Indicate in the #DELETE instruction the variables to be deleted.

1665 'Function G174 only admits one axis or spindle'

DETECTION During execution.
CAUSE More than one axis or spindle have been programmed in function G174.
SOLUTION Program one G174 per axis or spindle.

1666 'G174: slaved axes (GANTRY or TANDEM) are not admitted'

DETECTION During execution.
CAUSE The CNC has tried to initialize the machine coordinates (G174) of an axis that is part

of a pair of gantry or tandem axes or of an active coupling (#LINK).

SOLUTION Cancel the coupling to initialize the machine coordinates for that axis. The machine

coordinates of gantry or tandem axes cannot be initialized.

1667 'G174: Axes of the active kinematics or transforms are not admitted'

DETECTION During execution.
CAUSE The CNC has tried to initialize the machine coordinates (G174) of an axis that is part

the active kinematics or transforms #CS, #ACS, #ANGAX, #TANGCTRL.

SOLUTION Cancel the active kinematics or transformation to initialize the machine coordinates

for that axis.

1668 'Multi-axis group out of range'

DETECTION While reading (V.)MPA.MULAXISNAMEn[grupo] variables.
CAUSE The (group) index does not correspond to any multi-axis group defined in the machine

parameters.

SOLUTION Check the program. Program the multi-axis group number properly.

·74·

Error solving manual

1669 'Program #ROTATEMZ1-4 Pn/+n/-n'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program. Program the position to be selected on the turret or the number

of positions to rotate.

1670 'The indicated magazine must be a TURRET type'

DETECTION During execution.
CAUSE The instruction #ROTATEMZ is only valid for a turret type magazine.
SOLUTION Check the program. Verify that the magazine is a turret type.

1672 'G74-G174 not admitted for synchronized spindles'

DETECTION During execution.
CAUSE Once the spindles have been synchronized, the CNC does not allow programming

a home search or force a coordinate on any of them.
SOLUTION The CNC homes the spindles before synchronizing them. To do a home search or

force the coordinate, cancel the synchronization.

1673 'Variable that cannot be accessed by program or MDI'

DETECTION During execution.
CAUSE The programmed variable, although exists, has no permission to be accessed from

the program.
SOLUTION Check the access permissions of the variables.

1674 'Program #SELECT PROBE [probe number, POS/NEG]'

DETECTION During execution.
CAUSE The syntax of the instruction is wrong or there is more data in the block.
SOLUTION Check the program.

1676 'The active inclined plane has been recovered'

DETECTION During execution.
CAUSE After power-up, the CNC has recovered the inclined plane that was active when

turning the CNC off.
SOLUTION The inclined plane may be deactivated with the #CS OFF instruction.

1677 '#RTCP/TLC has been deactivated'

DETECTION During execution.
CAUSE The CNC has tried to carry out a home search while function #RTCP or #TLC was

active.
SOLUTION Deactivate the #RTCP/TLC functions before searching home.

1678 'Variable only exists for external analog feedback'

DETECTION During execution.
CAUSE The programmed variable only exists for axes with external analog feedback and the

indicated axis does not meet this condition.
SOLUTION Check the program. Check the variables that may be accessed depending on the type

of axes in the manuals.

1679 '#CAM SELECT not allowed when a cam is being executed or being loaded'

DETECTION During execution.
CAUSE The CNC has requested to load a cam that is in execution or already being loaded.
SOLUTION Wait for the cam to finish execution or be loaded.

1680 'Wrong part number'

DETECTION During execution.
CAUSE A wrong part number has been programmed in the #DGWZ instruction.
SOLUTION Program the part number within the P1-P4 range.

1681 'Too many channels programmed in the instruction'

DETECTION During execution.
CAUSE More than one channel number have been programmed in the #DGWZ instruction.
SOLUTION Program a single channel number C1-C4.

CNC 8070

(REF: 1308)

·75·

Error solving manual

1682 'Only one part number may be programmed'

DETECTION During execution.
CAUSE More than one part number have been programmed in the #DGWZ instruction.
SOLUTION Program a single part number P1-P4.

1683 'The #REPOS instruction is only allowed in interruption subroutines'

DETECTION During execution.
CAUSE The #REPOS instruction is not programmed in an interruption subroutine.
SOLUTION The #REPOS instruction can only be programmed in interruption subroutines.

Remove that instruction from any other subroutine or program.

1684 'Local subroutine and M, T, or G with subroutine in the same block'

DETECTION During execution.
CAUSE The same program block is executing a call to a local subroutine and an M, T or G

function that have an associated subroutine.

SOLUTION Program the call to the local subroutine in another program block.

1685 '$GOTO: Jump to blocks nested inside a $IF, $FOR, $WHILE, etc. instruction not allowed'

DETECTION During execution.
CAUSE The instruction $GOTO is not inside a loop, but it is jumping to a label defined inside

an $IF, $FOR, etc. loop.

SOLUTION Check the program. There could be no jumps into a loop.

1687 'Program: #REPOS <INT/INI> <sequence of axes/spindles>'

DETECTION During execution.
CAUSE The #REPOS instruction has been programmed wrong.
SOLUTION The #REPOS instruction can include an optional parameter INT or INI, followed by

a sequence of axes and/or spindles fo the channel without a particular order.

1688 'No #REPOS instructions of any other type are allowed'

DETECTION During execution.
CAUSE There are different types (INT/INI) of #REPOS instructions programmed in the same

interruption subroutines.

SOLUTION All #REPOS instructions must be of the same type.

1689 'No blocks are allowed after #REPOS'

DETECTION During execution.
CAUSE A block has been programmed between the #REPOS instructions and the end-of-

subroutine block in an interruption subroutine.

SOLUTION The #REPOS instruction must be the last blocks of the interruption subroutine, except

the end-of-subroutine block.

1690 'Multiple axis programmed twice'

DETECTION During execution.
CAUSE 'There cannot be more than one axis of the same multi-axis group programmed in

the same block'

SOLUTION Check the program. Only program the active axis of the multi-axis group.

CNC 8070

(REF: 1308)

·76·

1691 'Nested G subroutine'

DETECTION During execution.
CAUSE In a subroutine associated with a G function, it is not possible to program the G

function that is calling this subroutine.

SOLUTION Check the program. Do not program the G function inside the subroutine. In the case

of the G74, the function may be programmed inside the subroutine as long as it is
followed by the axes to be homed.

1692 'Program #VOLCOMP ON/OFF [n]'

DETECTION During execution.
CAUSE The instruction and/or some of its parameters are programmed wrong.
SOLUTION Check the program.

Error solving manual

1693 #RTCP cannot be programmed with the current kinematics. Program #FACE or #CYL'

DETECTION During execution.
CAUSE The instruction is not allowed with the current active kinematics.
SOLUTION Program the #FACE or #CYL instruction to activate that transformation.

1949 'The cutter cannot machine the whole profile'

DETECTION While executing a roughing canned cycle, pattern repeat on a lathe.
CAUSE The tool geometry makes it impossible for the tool to machine the whole programmed

profile.
CONSEQUENCE The cycle cannot machine the whole programmed profile.
SOLUTION Change the profile or the tool so it can machine the whole profile.

1700 'CENTER PUNCHING: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter F is 0. No feedrate has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1701 'CENTER PUNCHING: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter S is 0. No speed has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1702 'CENTER PUNCHING: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T is 0. No tool has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1703 'CENTER PUNCHING: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1704 'CENTER PUNCHING: ALPHA = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter alpha is 0. No angle has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1705 'CENTER PUNCHING: DIAMETER = 0'

DETECTION During the execution of the cycle.
CAUSE The value of the parameter to define the diameter is 0.
SOLUTION Assign a value greater than 0 to the parameter.

1706 'DRILLING 1: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter F is 0. No feedrate has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1707 'DRILLING 1: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter S is 0. No speed has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1708 'DRILLING 1: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T is 0. No tool has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1709 'DRILLING 1: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

CNC 8070

(REF: 1308)

·77·

Error solving manual

1710 'DRILLING 2: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter F is 0. No feedrate has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1711 'DRILLING 2: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter S is 0. No speed has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1712 'DRILLING 2: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T is 0. No tool has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1713 'DRILLING 2: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1714 'DRILLING 2: B = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter B is 0. No drilling peck has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1715 'THREADING: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter F is 0. No feedrate has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1716 'THREADING: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter S is 0. No speed has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1717 'THREADING: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T is 0. No tool has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1718 'THREADING: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1719 'REAMING: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter F is 0. No feedrate has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

CNC 8070

(REF: 1308)

·78·

1720 'REAMING: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter S is 0. No speed has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1721 'REAMING: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T is 0. No tool has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

Error solving manual

1722 'REAMING: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1723 'BORING 1: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter F is 0. No feedrate has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1724 'BORING 1: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter S is 0. No speed has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1725 'BORING 1: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T is 0. No tool has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1726 'BORING 1: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1727 'DRILLING 3: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter F is 0. No feedrate has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1728 'DRILLING 3: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter S is 0. No speed has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1729 'DRILLING 3: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T is 0. No tool has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1730 'DRILLING 3: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1731 'BORING 2: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter F is 0. No feedrate has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1732 'BORING 2: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter S is 0. No speed has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1733 'BORING 2: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T is 0. No tool has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

CNC 8070

(REF: 1308)

·79·

Error solving manual

1734 'BORING 2: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1735 'RECTANGULAR POCKET: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.
The value of some F parameter is 0. No feedrate has been programmed.

SOLUTION Assign a value greater than 0 to the parameter.

1736 'RECTANGULAR POCKET: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1737 'RECTANGULAR POCKET: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.

SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

1738 'RECTANGULAR POCKET: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1739 'RECTANGULAR POCKET: tool diameter smaller than DELTA'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is sma ller than the milling pass

(parameter Δ).

SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1740 'RECTANGULAR POCKET: tool diameter greater than the pocket'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is greater than the pocket

dimensions (parameter L or H).

SOLUTION Choose a tool with a smaller diameter.

1741 'RECTANGULAR POCKET: Finishing tool diameter smaller than delta'

DETECTION During the execution of the cycle.
CAUSE The diameter of the finishing tool is smaller than the residual stock on the side walls

(parameter δ).

SOLUTION Choose a tool of a greater diameter for the finishing pass.

1742 'PRE-EMPTIED POCKET: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.

SOLUTION Assign a value greater than 0 to the parameter.

CNC 8070

(REF: 1308)

·80·

1743 'PRE-EMPTIED POCKET: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1744 'PRE-EMPTIED POCKET: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.

SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

Error solving manual

1745 'PRE-EMPTIED POCKET: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1746 'PRE-EMPTIED POCKET: tool diameter smaller than DELTA'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is smaller than the milling pass

(parameter Δ).
SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1747 'PRE-EMPTIED POCKET: tool diameter greater than the pocket'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is greater than the pocket

dimensions (parameter L or H).
SOLUTION Choose a tool with a smaller diameter.

1748 'PRE-EMPTIED POCKET: Finishing tool diameter smaller than delta'

DETECTION During the execution of the cycle.
CAUSE The diameter of the finishing tool is smaller than the residual stock on the side walls

(parameter δ).
SOLUTION Choose a tool of a greater diameter for the finishing pass.

1749 'PRE-EMPTIED POCKET: R <r'

DETECTION During the execution of the cycle.
CAUSE The pocket radius (parameter R) is smaller than the pre-emptying radius (parameter

r).
SOLUTION The pocket radius (outside radius must be larger than the pre-emptying radius (inside

radius).

1750 'RECTANGULAR BOSS: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1751 'RECTANGULAR BOSS: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1752 'RECTANGULAR BOSS: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.
SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

1753 'RECTANGULAR BOSS: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1754 'RECTANGULAR BOSS: tool diameter smaller than DELTA'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is smaller than the milling pass

(parameter Δ).
SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1755 'RECTANGULAR BOSS: Finishing tool diameter smaller than delta'

DETECTION During the execution of the cycle.
CAUSE The diameter of the finishing tool is smaller than the residual stock on the side walls

(parameter δ).
SOLUTION Choose a tool of a greater diameter for the finishing pass.

CNC 8070

(REF: 1308)

·81·

Error solving manual

1756 'CIRCULAR BOSS: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.

SOLUTION Assign a value greater than 0 to the parameter.

1757 'CIRCULAR BOSS: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1758 'CIRCULAR BOSS: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.

SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

1759 'CIRCULAR BOSS: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1760 'CIRCULAR BOSS: R = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter R is 0. No radius has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1761 'CIRCULAR BOSS: tool diameter smaller than DELTA'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is sma ller than the milling pass

(parameter Δ).

SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1762 'CIRCULAR BOSS: Finishing tool diameter smaller than delta'

DETECTION During the execution of the cycle.
CAUSE The diameter of the finishing tool is smaller than the residual stock on the side walls

(parameter δ).

SOLUTION Choose a tool of a greater diameter for the finishing pass.

1763 'SURFACE MILLING: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.

SOLUTION Assign a value greater than 0 to the parameter.

1764 'SURFACE MILLING: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

CNC 8070

(REF: 1308)

·82·

1765 'SURFACE MILLING: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.

SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

1766 'SURFACE MILLING: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

Error solving manual

1767 'SURFACE MILLING: L = 0 and H = 0'

DETECTION During the execution of the cycle.
CAUSE The length (parameter L) and/or the width of the surface milling (parameter H) are 0.
SOLUTION Define both dimensions of the surface milling with a value other than zero.

1768 'POINT-TO-POINT PROFILE: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1769 'POINT-TO-POINT PROFILE: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1770 'POINT-TO-POINT PROFILE: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.
SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

1771 'POINT-TO-POINT PROFILE: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1772 'POINT-TO-POINT PROFILE: Null profile'

DETECTION During the execution of the cycle.
CAUSE The first two points of the profile (P1 and P2) are the same; the cycle considers that

no profile has been defined.
SOLUTION Define the points of the profile correctly. Two identical points indicate the end of the

profile.

1773 'POINT-TO-POINT PROFILE: Tool radius equal to or greater than the tangential entry/exit

radius'

DETECTION During the execution of the cycle.
CAUSE The radius of one of the tools used in the cycle is equal to or greater than the tangential

entry radius (radius of point P1) or of the tangential exit (radius of P12).
SOLUTION Increase the radius of the tangential entry/exit or execute the cycle with a tool of

smaller radius.

1774 'PROFILE: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1775 'PROFILE: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1776 'PROFILE: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.
SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

CNC 8070

(REF: 1308)

·83·

Error solving manual

1777 'PROFILE: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1778 'PROFILE: (FINISHING): Tool's cutting length < P'

DETECTION During the execution of the cycle.
CAUSE The cutting length of the finishing tool is smaller than the profile depth (parameter P).
SOLUTION Choose as the finishing tool, a tool with greater cutting length.

1779 'SLOT MILLING: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.

SOLUTION Assign a value greater than 0 to the parameter.

1780 'SLOT MILLING: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1781 'GROOVING: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.

SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

CNC 8070

1782 'GROOVING: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1783 'SLOT MILLING: L = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter L is 0. The slot (groove) has no length.
SOLUTION Assign a value greater than 0 to the parameter.

1784 'SLOT MILLING: tool diameter smaller than DELTA'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is sma ller than the milling pass

(parameter Δ).

SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1785 'GROOVING: tool diameter greater than the pocket'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is greater than the groove

dimensions (parameter L or H).

SOLUTION Choose a tool with a smaller diameter.

1786 'GROOVING: FINISHING tool diameter smaller than delta'

DETECTION During the execution of the cycle.
CAUSE The diameter of the finishing tool is smaller than the residual stock on the side walls

(parameter δ).

SOLUTION Choose a tool of a greater diameter for the finishing pass.

(REF: 1308)

·84·

1787 'CIRCULAR POCKET: F = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some F parameter is 0; the feedrate for roughing, finishing or Z-axis

penetration is missing.

SOLUTION Assign a value greater than 0 to the parameter.

Error solving manual

1788 'CIRCULAR POCKET: S = 0'

DETECTION During the execution of the cycle.
CAUSE The value of some S parameter is 0; the speed for roughing or finishing is missing.
SOLUTION Assign a value greater than 0 to the parameter.

1789 'CIRCULAR POCKET: T = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter T of roughing and finishing operations is 0. No tool has been

programmed.
SOLUTION Program a tool for roughing or finishing operations. If an operation does not have a

tool, the cycle will not executed it; at least one operation must have a tool.

1790 'CIRCULAR POCKET: P = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P is 0. No depth has been programmed.
SOLUTION Assign a value greater than 0 to the parameter.

1791 'CIRCULAR POCKET: tool diameter smaller than DELTA'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool diameter is smaller than the milling pass

(parameter Δ).
SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1792 'CIRCULAR POCKET: tool diameter greater than the pocket'

DETECTION During the execution of the cycle.
CAUSE In the roughing or finishing operation, the tool radius is greater than the pocket radius

(parameter R).
SOLUTION Choose a tool with a smaller diameter.

1793 'CIRCULAR POCKET: Finishing tool diameter smaller than delta'

DETECTION During the execution of the cycle.
CAUSE The diameter of the finishing tool is smaller than the residual stock on the side walls

(parameter δ).
SOLUTION Choose a tool of a greater diameter for the finishing pass.

1794 'RECTANGULAR POCKET: Tool diameter = 0'

DETECTION During the execution of a cycle.
CAUSE The radius of the roughing or finishing tool is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1795 'CIRCULAR POCKET: Tool diameter = 0'

DETECTION During the execution of a cycle.
CAUSE The radius of the roughing or finishing tool is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1796 'PRE-EMPTIED POCKET: Tool diameter = 0'

DETECTION During the execution of a cycle.
CAUSE The radius of the roughing or finishing tool is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1797 'RECTANGULAR BOSS: Tool diameter = 0'

DETECTION During the execution of a cycle.
CAUSE The radius of the roughing or finishing tool is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1798 'CIRCULAR BOSS: Tool diameter = 0'

DETECTION During the execution of a cycle.
CAUSE The radius of the roughing or finishing tool is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1799 'SURFACE MILLING: Tool diameter = 0'

DETECTION During the execution of a cycle.
CAUSE The radius of the roughing or finishing tool is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

CNC 8070

(REF: 1308)

·85·

Error solving manual

1800 'SLOT MILLING: Tool diameter = 0'

DETECTION During the execution of a cycle.
CAUSE The radius of the roughing or finishing tool is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1801 'RECTANGULAR POCKET: Beta or theta < 0 or Beta or theta > 90'

DETECTION During the execution of a pocket.
CAUSE In the pocket cycle, the lateral penetration angle for roughing (parameter β) or for

finishing (parameter θ) is not between 0º and 90º.

SOLUTION Correct the lateral penetration angle; program a value between 0º and 90º.

1802 'CIRCULAR POCKET: Beta or theta < 0 or Beta or theta > 90'

DETECTION During the execution of a pocket.
CAUSE In the pocket cycle, the lateral penetration angle for roughing (parameter β) or for

finishing (parameter θ) is not between 0º and 90º.

SOLUTION Correct the lateral penetration angle; program a value between 0º and 90º.

1803 'PRE-EMPTIED POCKET: Beta or theta < 0 or Beta or theta > 90'

DETECTION During the execution of a pocket.
CAUSE In the pocket cycle, the lateral penetration angle for roughing (parameter β) or for

finishing (parameter θ) is not between 0º and 90º.

SOLUTION Correct the lateral penetration angle; program a value between 0º and 90º.

1804 'G87: Depth = 0'

DETECTION During the execution of the cycle.
CAUSE The resulting depth of the pocket is zero. The programmed depth (parameter I) is the

same as the sum of parameters Z and D; if parameter Z has not been programmed,
the programmed depth (parameter I) is the same as parameter D.

SOLUTION Correct the programming of parameters I Z D.

1805 'G87: tool diameter greater than the pocket'

DETECTION During the execution of the cycle.
CAUSE The tool radius is greater than the dimensions of the pocket (parameters J and/or K).
SOLUTION Select a tool with a smaller diameter.

1806 'G87: tool diameter smaller than L'

DETECTION During the execution of the cycle.
CAUSE The tool diameter is smaller than the finishing stock (parameter L).
SOLUTION Select a tool with a larger diameter.

1807 'G87: Tool diameter = 0'

DETECTION During the execution of the cycle.
CAUSE The tool diameter is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1808 'G87: Tool missing'

DETECTION During the execution of the cycle.
CAUSE Tool missing at the spindle.
SOLUTION Program a tool before the cycle or load a tool at the spindle.

CNC 8070

(REF: 1308)

·86·

1809 'G87: tool diameter smaller than C'

DETECTION During the execution of the cycle.
CAUSE The tool diameter is smaller than the milling pass (parameter C).
SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1810 'G88: Depth = 0'

DETECTION During the execution of the cycle.
CAUSE The resulting depth of the pocket is zero. The programmed depth (parameter I) is the

same as the sum of parameters Z and D; if parameter Z has not been programmed,
the programmed depth (parameter I) is the same as parameter D.

SOLUTION Correct the programming of parameters I Z D.

Error solving manual

1811 'G88: tool diameter greater than the pocket'

DETECTION During the execution of the cycle.
CAUSE The tool radius is greater than the dimensions of the pocket (parameter J).
SOLUTION Select a tool with a smaller diameter.

1812 'G88: tool diameter smaller than L'

DETECTION During the execution of the cycle.
CAUSE The tool diameter is smaller than the finishing stock (parameter L).
SOLUTION Select a tool with a larger diameter.

1813 'G88: Tool diameter = 0'

DETECTION During the execution of the cycle.
CAUSE The tool diameter is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1814 'G88: Tool missing'

DETECTION During the execution of the cycle.
CAUSE Tool missing at the spindle.
SOLUTION Program a tool before the cycle or load a tool at the spindle.

1815 'G88: tool diameter smaller than C'

DETECTION During the execution of the cycle.
CAUSE The tool diameter is smaller than the milling pass (parameter C).
SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1816 'The X parameter must be multiple of the I parameter'

DETECTION During the execution of a multiple machining cycle.
CAUSE The length of the machining operation (parameter X) must be multiple of the step

between machining operations (parameter I).
SOLUTION Assign a correct value to the parameters.

1817 'One of parameters I and K must be programmed'

DETECTION During the execution of a multiple machining cycle.
CAUSE The step between machining operations (parameter I) or the number of machining

operations (parameter K) has not been programmed.
SOLUTION Assign a correct value to the parameter.

1818 'J = 0'

DETECTION During the execution of a multiple machining cycle.
CAUSE In a multiple machining operation, parameter J (machining step along the ordinate

axis) is 0.
SOLUTION Assign a correct value to the parameter.

1819 'K = 0'

DETECTION During the execution of a multiple machining cycle.
CAUSE In a multiple machining operation, parameter K (number of machining operations) is

0.

SOLUTION Assign a correct value to the parameter.

1820 'Two of parameters X, I and K must be programmed'

DETECTION During the execution of a multiple machining cycle.
CAUSE Two of these parameters have not been programmed: X (machining length), I (step

between machining operations), K (number of machining operations).
SOLUTION Assign a correct value to the parameters.

CNC 8070

1821 'B must be multiple of I'

DETECTION During the execution of a multiple machining cycle.
CAUSE The angular length of the machining operation (parameter B) must be multiple of the

angular step between machining operations (parameter I).
SOLUTION Assign a correct value to the parameters.

(REF: 1308)

·87·

Error solving manual

1822 'The Y parameter must be multiple of the J parameter'

DETECTION During the execution of a multiple machining cycle.
CAUSE The length of the machining operation (parameter Y) must be multiple of the step

between machining operations (parameter J).

SOLUTION Assign a correct value to the parameters.

1823 'Two of parameters Y, J and D must be programmed'

DETECTION During the execution of a multiple machining cycle.
CAUSE Two of these parameters have not been programmed: Y (machining length), J (step

between machining operations), D (number of machining operations).

SOLUTION Assign a correct value to the parameters.

1824 'One of parameters I and K must be programmed'

DETECTION During the execution of a multiple machining cycle.
CAUSE One of these parameters has not been programmed: I (step between machining

operations), K (number of machining operations).

SOLUTION Assign a correct value to the parameters.

1825 'One of parameters I and A must be programmed'

DETECTION During the execution of a multiple machining cycle.
CAUSE Two of these parameters have not been programmed: I (angular step between

machining operations), A (number of machining operations).

SOLUTION Assign a correct value to the parameter.

1826 'Parameter I multiplied by K must be equal to 360'

DETECTION During the execution of a multiple machining cycle.
CAUSE The angular step between machining operations (parameter I) multiplied by the

number of machining operations (parameter K) must be 360º.

SOLUTION Assign a correct value to the parameter.

1827 'Parameters X and Y are equal to 0'

DETECTION During the execution of a multiple machining cycle.
CAUSE Parameters X Y (center of the machining arc) are 0.
SOLUTION Assign a correct value to the parameter.

1828 '360 must be multiple of parameter I'

DETECTION During the execution of a multiple machining cycle.
CAUSE The angular step (parameter I) must be sub-multiple of 360º.
SOLUTION Assign a correct value to the parameter.

1829 'I = 0'

DETECTION During the execution of a multiple machining cycle.
CAUSE In a multiple machining operation, parameter I (machining step) is 0.
SOLUTION Assign a value other than 0 to the parameter.

1830 'Tool diameter = 0'

DETECTION During the execution of a cycle.
CAUSE The tool diameter is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

CNC 8070

(REF: 1308)

·88·

1831 'G82: C = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter C (approach coordinate) is 0.
SOLUTION Assign a value other than 0 to the parameter.

1832 'ROUGHING: I = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter I (maximum penetration step) is 0.
SOLUTION Assign to the parameter a value other than zero and smaller than the cutting length

of the tool.

Error solving manual

1833 'FINISHING: N = 0 and undefined tool's cutting length.

DETECTION During the execution of the cycle.
CAUSE The value of parameter N (number of penetration passes) is 0 and the cutting length

of the finishing tool has not been defined.
SOLUTION Program the number of penetrating passes (parameter N) or define the cutting length

in the tool table.

1834 'FINISHING: Z delta greater than the tool's cutting length'

DETECTION During the execution of the cycle.
CAUSE Parameter δz (finishing stock at the bottom) exceeds the cutting length of the finishing

tool.
SOLUTION Program a smaller finishing stock (parameter δz) or use another tool.

1835 'Pocket with islands: Wrong safety Z'

DETECTION During the execution of the cycle.
CAUSE The safety plane (parameter Zs) is located inside the part.
SOLUTION Assign a correct value to the parameter.

1836 'Pocket with islands: Wrong Z profile'

DETECTION During the execution of the cycle.
CAUSE Some depth profile is closed or the cycle cannot machine some depth profile with the

programmed tool.
SOLUTION Check that the depth profiles are correct.

1837 'Pocket with islands: Profile in XY intersects itself'

DETECTION During the execution of the cycle.
CAUSE Some surface profile forms more than one closed profile.
SOLUTION Check that the surface profiles do not intersect each others and that only their starting

point is the same.

1838 'Pocket with islands: The XY profile is not closed'

DETECTION During the execution of the cycle.
CAUSE Some surface profile is not a closed profile; its initial and final points are not the same.
SOLUTION Check that all the surface profiles are closed.

1839 'Pocket with islands: Wrong intersection of XY profiles'

DETECTION During the execution of the cycle.
CAUSE Two surface profiles have some straight or arc section in common.
SOLUTION Check that the surface profiles do not have sections in common, the profiles must

intersect in points.

1840 'Pocket with islands: Not enough memory to resolve it'

DETECTION During the execution of the cycle.
CAUSE The system has not enough memory to continue resolving the pocket.
SOLUTION Contact FAGOR.

1841 'Wrong tool position before the canned cycle'

DETECTION During the execution of the cycle.
CAUSE When executing the canned cycle, the tool tip is located between the reference plane

and the surface of the part.
SOLUTION To execute the cycle, position the tool above the reference plane.

1842 'Tool diameter smaller than DELTA'

DETECTION During the execution of the cycle.
CAUSE The finishing tool diameter is smaller than the milling pass (parameter Δ).
SOLUTION Reduce the milling pass or use a tool with a larger diameter.

1843 'Pocket with islands: Wrong roughing tool radius'

DETECTION During the execution of the cycle.
CAUSE The roughing tool radius is 0 or the tool is too large for the geometry of the pocket

considering the lateral stock (parameter δ).
SOLUTION Correct the value of the tool radius in the tool table or select another tool. Check the

value of the lateral residual stock.

CNC 8070

(REF: 1308)

·89·

Error solving manual

1844 'Pocket with islands: Wrong finishing tool radius'

DETECTION During the execution of the cycle.
CAUSE The finishing tool radius is 0 or the tool is too large for the geometry of the pocket.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1845 'G165: Chord length (I) greater than the diameter'

DETECTION During the execution of a multiple machining cycle.
CAUSE The length of the chord (parameter I) is greater than the diameter of the circle.
SOLUTION Assign a correct value to the parameter.

1846 'Zero arc radius'

DETECTION During the execution of a multiple machining cycle.
CAUSE The possible causes are:

• There is an arc with zero radius in the profile.

• In a multiple machining operation in an arc or a circle, both center coordinates
are the same as the those of the starting point.

SOLUTION Check the program.

1847 'RECTANGULAR BOSS: Q = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter Q (stock to be removed) is 0.
SOLUTION Assign a value other than 0 to the parameter.

1848 'CIRCULAR BOSS: Q = 0'

DETECTION During the execution of the cycle.
CAUSE The value of parameter Q (stock to be removed) is 0.
SOLUTION Assign a value other than 0 to the parameter.

1849 'RECTANGULAR POCKET: Finishing stock DELTA greater than the pocket'

DETECTION During the execution of the cycle.
CAUSE The size of the pocket minus the tool diameter is smaller than the lateral residual stock

(twice parameter δ).

SOLUTION Assign a correct value to the parameter.

1850 'Lx must be multiple of Ix'

DETECTION During the execution of a multiple machining cycle.
CAUSE The length of the machining operation (parameter Lx) must be multiple of the step

between machining operations (parameter Ix).

SOLUTION Assign a correct value to the parameters.

1851 'Ly must be multiple of Iy'

DETECTION During the execution of a multiple machining cycle.
CAUSE The length of the machining operation (parameter Ly) must be multiple of the step

between machining operations (parameter Iy).

SOLUTION Assign a correct value to the parameters.

1852 'No tool has been programmed'

DETECTION During the execution of a #PROBE probing cycle.
CAUSE There is no probe at the spindle so the cycle can be executed.
SOLUTION Execute the cycle with a tool at the spindle or with a probe, depending on the cycle.

CNC 8070

(REF: 1308)

·90·

1853 'The probe signal has not been received'

DETECTION During the execution of a #PROBE probing cycle.
CAUSE The probe has not touched the part during the probing movement.
SOLUTION Correct the definition of the canned cycle.

1854 'The diameter J must be greater than zero'

DETECTION During the execution of a #PROBE 2 or #PROBE 9 probing cycle.
CAUSE Parameter J (theoretical hole diameter) has the wrong value.
SOLUTION Assign a positive value to the parameter.

Error solving manual

1855 'Tool diameter greater than that of the hole'

DETECTION During the execution of a #PROBE 2 or #PROBE 9 probing cycle.
CAUSE The probe diameter is greater than the diameter of the hole to be measured or greater

than the hole used to calibrate the probe.

SOLUTION Correct the definition of the canned cycle.

1856 'Wrong withdraw distance E'

DETECTION During the execution of a #PROBE 2 or #PROBE 9 probing cycle.
CAUSE Parameter E (withdrawal distance) has the wrong value.
SOLUTION Assign to the parameter a value between 0 and the diameter of the hole.

1857 'There is no tool offset selected'

DETECTION During the execution of a #PROBE 1 or #PROBE 2 probing cycle.
CAUSE There is no active tool offset for the tool calibration cycle.
SOLUTION Program the tool offset (function D) before the cycle.

1858 'Program I = 0/1'

DETECTION During the execution of a #PROBE probing cycle.
CAUSE Parameter I (type of calibration) has the wrong value.
SOLUTION Parameter I only admits values of 0 (single calibration) or 1 (double calibration).

1859 'The active plane for calibrating the probe must be G17, G18 or G19'

DETECTION During the execution of a #PROBE 2 probing cycle.
CAUSE When executing the cycle, there is an active work plane defined with G20.
SOLUTION Activate a main plane G17, G18 or G19 to execute the cycle.

1860 'Program K = 0/1/2'

DETECTION During the execution of a #PROBE 3 probing cycle.
CAUSE Parameter K (probing axis) has the wrong value.
SOLUTION Parameter K only admits values of 0 (abscissa axis), 1 (ordinate axis) or 2

(longitudinal axis).

1861 'The safety distance B must be greater than zero'

DETECTION During the execution of a #PROBE probing cycle.
CAUSE The value of parameter B is negative.
SOLUTION Assign a positive value to the parameter.

1862 '#PROBE 1: not allowed when G20 is active'

DETECTION During the execution of a #PROBE 1 probing cycle.
CAUSE When executing the cycle, there is an active work plane defined with G20.
SOLUTION Activate a main plane G17, G18 or G19 to execute the cycle.

1863 'Tool worn out'

DETECTION During the execution of a #PROBE 1 probing cycle.
CAUSE The cycle has detected a tool that is worn out. The measured wear is greater than

the allowed tolerance (parameter L or M).

SOLUTION Change the tool and execute the cycle again.

1864 '#PROBE 1: Parameters U, V, W must be greater than X, Y, Z'

DETECTION During the execution of a #PROBE 1 probing cycle.
CAUSE The tabletop probe position has been defined wrong in the cycle. One of parameters

X, Y, Z is greater than its corresponding parameter U, V, W. Parameters X Y Z refer
to the minimum coordinates of the probe and parameters U V W refer to the maximum
coordinates.

SOLUTION Define the probe position so U > X, V > Y, W > Z.

CNC 8070

1865 'Pocket with islands: Roughing T missing'

DETECTION During the execution of the cycle.
CAUSE The programmed tool does not exist in the tool table.
SOLUTION Correct the tool in the table or select another tool.

(REF: 1308)

·91·

1866 'Pocket with islands: Wrong roughing F'

DETECTION During the execution of the cycle.
CAUSE The roughing feedrate is 0.
SOLUTION Define a feedrate higher than 0.

1867 'Pocket with islands: Wrong roughing S'

DETECTION During the execution of the cycle.
CAUSE The spindle speed for the roughing operation is 0.
SOLUTION Define a speed higher than 0.

1868 'Pocket with islands: Finishing T missing'

DETECTION During the execution of the cycle.
CAUSE The programmed tool does not exist in the tool table.
SOLUTION Correct the tool in the table or select another tool.

1869 'Pocket with islands: Wrong finishing F'

DETECTION During the execution of the cycle.
CAUSE The finishing feedrate is 0.
SOLUTION Define a feedrate higher than 0.

1870 'Pocket with islands: Wrong finishing S'

DETECTION During the execution of the cycle.
CAUSE The spindle speed for the finishing operation is 0.
SOLUTION Define a speed higher than 0.

Error solving manual

1871 'Pocket with islands: Wrong roughing pass'

DETECTION During the execution of the cycle.
CAUSE The roughing pass (parameter Δ) is greater than tool diameter.
SOLUTION Correct the location code (tool shape) or select another tool.

1872 'Pocket with islands: Wrong finishing pass'

DETECTION During the execution of the cycle.
CAUSE In a 2D pocket, the finishing pass (parameter Δ) is greater than tool diameter. In a

3D pocket, the finishing pass (parameter ε) is 0.

SOLUTION Correct the machining pass.

1873 'Pocket with islands: Wrong side stock (excess material)'

DETECTION During the execution of the cycle.
CAUSE The lateral finishing stock (parameter δ) is greater than tool diameter.
SOLUTION Correct the lateral finishing stock or select another tool.

1874 'Pocket with islands: Wrong depth'

DETECTION During the execution of the cycle.
CAUSE The value of parameter P (pocket depth) is 0.
SOLUTION Assign a correct value to the parameter.

1875 'Pocket with islands: XY profile does not exist'

DETECTION During the execution of the cycle.
CAUSE The programmed surface profile does not exist.
SOLUTION Select an existing profile or generate the programmed profile.

CNC 8070

(REF: 1308)

·92·

1876 'Pocket with islands: Wrong XY profile'

DETECTION During the execution of the cycle.
CAUSE Geometry of the surface profile programmed wrong.
SOLUTION Correct the geometry of the profile from the profile editor.

1877 'Pocket with islands: Z profile does not exist'

DETECTION During the execution of the cycle.
CAUSE The programmed depth profile does not exist.
SOLUTION Select an existing profile or generate the programmed profile.

Error solving manual

1878 'Pocket with islands: Wrong finishing tool tip (nose) radius'

DETECTION During the execution of the cycle.
CAUSE The tip radius (Rp) of the finishing tool is greater than its radius ( R ).
SOLUTION Correct the tool tip (nose) radius.

1879 'Pocket with islands: Wrong semi-finishing tool radius'

DETECTION During the execution of the cycle.
CAUSE The semi-finishing tool radius 0 or it is too large for the geometry of the pocket.
SOLUTION Correct the tool in the table or select another tool.

1880 'Pocket with islands: Semi-finishing T missing'

DETECTION During the execution of the cycle.
CAUSE The programmed tool does not exist in the tool table.
SOLUTION Correct the tool in the table or select another tool.

1881 'Pocket with islands: Wrong semi-finishing F'

DETECTION During the execution of the cycle.
CAUSE The semi-finishing feedrate is 0.
SOLUTION Define a feedrate higher than 0.

1882 'Pocket with islands: Wrong semi-finishing S'

DETECTION During the execution of the cycle.
CAUSE The spindle speed for the semi-finishing operation is 0.
SOLUTION Define a speed higher than 0.

1883 'Pocket with islands: Pocket already in execution'

DETECTION During the execution of the cycle.
CAUSE The CNC cannot simulate or execute the pocket because it is already in execution

or simulation.

SOLUTION Wait for the CNC to finish the simulation or execution.

1884 'Pocket with islands: Arc programmed wrong in the profile'

DETECTION During the execution of the cycle.
CAUSE In some profile of the pocket, there is an arc that has been defined wrong or the profile

has been modified with a program other than the profile editor.

SOLUTION Correct the geometry of the profile from the profile editor.

1885 'Pocket with islands: Wrong pocket geometry'

DETECTION During the execution of the cycle.
CAUSE In some profile of the pocket, there is a section that has been defined wrong (rounding,

chamfer, etc.).

SOLUTION Correct the geometry of the profile from the profile editor.

1886 'Pocket with islands: Wrong roughing tool's penetration angle'

DETECTION During the execution of the cycle.
CAUSE The roughing penetration angle (parameter β) is not between 0º and 90º.
SOLUTION Correct the penetration angle; program a value between 0º and 90º.

1887 'Pocket with islands: Wrong penetration angle of the semi-finishing tool'

DETECTION During the execution of the cycle.
CAUSE The finishing penetration angle (parameter θ) is not between 0º and 90º.
SOLUTION Correct the penetration angle; program a value between 0º and 90º.

1888 'Pocket with islands: Wrong type of finishing'

DETECTION During the execution of the cycle.
CAUSE The type of finishing (parameter Q) is wrong.
SOLUTION Assign a correct value to the parameters.

1889 'Back-and-forth movement: Distance traveled too short'

DETECTION Execution of the back-and-forth movement for adjusting the inertia.
CAUSE The distance programmed in the back-and-forth movement is not long enough.
SOLUTION Program a longer distance.

CNC 8070

(REF: 1308)

·93·

Error solving manual

1890 'Back-and-forth movement: Distance traveled too long'

DETECTION Execution of the back-and-forth movement for adjusting the inertia.
CAUSE The distance programmed in the back-and-forth movement is too long.
SOLUTION Program a shorter distance.

1900 'Required data not programmed

DETECTION During the execution of the cycle.
CAUSE One or more required parameters have not been programmed. The wrong parameter

will be indicated in the error message.

SOLUTION Program all the mandatory parameters of the cycle.

1901 'Wrong character'

DETECTION During the execution of the cycle.
CAUSE Some cycle parameter has the wrong value. The wrong parameter will be indicated

in the error message.

SOLUTION Correct the program.

1902 'Incompatible starting position and location code (shape) of the tool

DETECTION During the execution of the cycle.
CAUSE The initial position of the tool is not compatible with the location code (tool shape)

and the geometry of the tool.

SOLUTION Position the tool properly or change the tool.

1903 'Arc programmed wrong'

DETECTION During the execution of the cycle.
CAUSE Arc defined wrong in the geometry of the canned cycle.
SOLUTION Correct the program.

1904 'No tool has been programmed'

DETECTION During the execution of the cycle.
CAUSE No tool has been programmed.
SOLUTION Program a tool before the cycle or load a tool at the spindle.

1905 'SLOT MILLING: Zero cutter width'

DETECTION During the execution of the cycle.
CAUSE The tool width is 0.
SOLUTION Correct the tool width or select another tool.

1906 'Wrong tool location code (shape)

DETECTION During the execution of the cycle.
CAUSE The location code (tool shape) is not valid for the programmed cycle.
SOLUTION Correct the location code (tool shape) or select another tool.

1907 'Zero feedrate F before the cycle

DETECTION During the execution of the cycle.
CAUSE The machining feedrate is 0.
SOLUTION Define a feedrate higher than 0.

CNC 8070

(REF: 1308)

·94·

1908 'No residual stock has been programmed'

DETECTION During the execution of the cycle.
CAUSE The finishing stock is 0.
SOLUTION Define a finishing stock greater than 0.

1909 'Zero roughing pass'

DETECTION During the execution of the cycle.
CAUSE The value of the machining pass is 0.
SOLUTION Define a machining pass greater than 0.

1910 'Roughing pass greater than cutter width'

DETECTION During the execution of the cycle.
CAUSE The roughing pass is greater than cutter width.
SOLUTION Program a roughing pass smaller or equal to the cutter width.

Error solving manual

1911 'Wrong location code (shape code) in profile roughing cycle'

DETECTION During the execution of the cycle.
CAUSE The location code (tool shape) is not valid for the programmed cycle.
SOLUTION Correct the location code (tool shape) or select another tool.

1912 'Wrong cutter angle'

DETECTION During the execution of the cycle.
CAUSE The cutter angle is not valid for the programmed cycle.
SOLUTION Correct the cutter angle or select another tool.

1913 'Wrong cutting angle of the cutter'

DETECTION During the execution of the cycle.
CAUSE The cutting angle is not valid for the programmed cycle.
SOLUTION Correct the cutting angle or select another tool.

1914 'Wrong roughing F'

DETECTION During the execution of the cycle.
CAUSE The roughing feedrate is 0.
SOLUTION Define a feedrate higher than 0.

1915 'Wrong finishing F'

DETECTION During the execution of the cycle.
CAUSE The finishing feedrate is 0.
SOLUTION Define a feedrate higher than 0.

1916 'Wrong roughing S'

DETECTION During the execution of the cycle.
CAUSE The spindle speed for the roughing operation is 0.
SOLUTION Define a speed higher than 0.

1917 'Wrong finishing S'

DETECTION During the execution of the cycle.
CAUSE The spindle speed for the finishing operation is 0.
SOLUTION Define a speed higher than 0.

1918 'The programmed profile is closed'

DETECTION During the execution of the cycle.
CAUSE The profile defined in the canned cycle is not valid because it is a closed profile.
SOLUTION Program a profile that is not closed.

1919 'The programmed profile intersects itself'

DETECTION During the execution of the cycle.
CAUSE The profile defined in the canned cycle is not valid because it intersects itself.
SOLUTION Program a profile that does not intersect itself.

1920 'No profile has been programmed'

DETECTION During the execution of the cycle.
CAUSE The profile that defines the geometry of the canned cycle has not been programmed.
SOLUTION Define the profile that defines the geometry of the cycle.

1921 'The programmed geometry is not an outside geometry'

DETECTION During the execution of the cycle.
CAUSE The geometry programmed in the canned cycle does not correspond to an external

geometry, as indicated in the cycle.

SOLUTION Change the geometry or define it as internal geometry in the cycle.

1922 'The programmed geometry is not an inside geometry'

DETECTION During the execution of the cycle.
CAUSE The geometry programmed in the canned cycle does not correspond to an internal

geometry, as indicated in the cycle.

SOLUTION Change the geometry or define it as external geometry in the cycle.

CNC 8070

(REF: 1308)

·95·

Error solving manual

1923 'Wrong geometry'

DETECTION During the execution of the cycle.
CAUSE The geometry of the canned cycle is wrong.
SOLUTION Correct the program.

1924 ‘Insufficient memory’

DETECTION During the execution of the cycle.
CAUSE The system has not enough memory to continue resolving the pocket.
SOLUTION Contact FAGOR.

1925 'Neither roughing nor finishing has been programmed'

DETECTION During the execution of the cycle.
CAUSE No operation has been defined in the canned cycle.
SOLUTION The canned cycle must have the definition of the roughing or finishing operation. If

an operation does not have a tool, the cycle will not executed it; at least one operation
must have a tool.

1926 'Vertex programmed wrong'

DETECTION During the execution of the cycle.
CAUSE The geometry of the canned cycle is wrong.
SOLUTION Correct the program.

1927 'Wrong cutter for programmed profile'

DETECTION During the execution of the cycle.
CAUSE The tool is not valid for the geometry of the programmed cycle.
SOLUTION Select another tool.

1928 'Grooving pass greater than cutter width'

DETECTION During the execution of the cycle.
CAUSE The slot milling (grooving) pass is greater than cutter width.
SOLUTION Program a grooving (slot milling) pass smaller or equal to the cutter width.

1929 'No spindle speed has been programmed'

DETECTION During the execution of the cycle.
CAUSE The spindle speed is 0.
SOLUTION Define a feedrate higher than 0.

1930 'A zero drilling peck has been programmed'

DETECTION During the execution of the cycle.
CAUSE The value of the drilling peck is 0.
SOLUTION Define a drilling peck other than 0.

1931 'No depth has been programmed'

DETECTION During the execution of the cycle.
CAUSE The machining depth is 0.
SOLUTION Define a machining depth other than 0.

1932 'Spindle missing to execute the cycle'

DETECTION During the execution of the cycle.
CAUSE The channel that executes the cycle does not a spindle.
SOLUTION Yield a spindle to the channel or execute the cycle in a channel with spindle.

CNC 8070

(REF: 1308)

·96·

1933 'Live tool missing to execute the cycle'

DETECTION During the execution of the cycle.
CAUSE The channel that executes the cycle does not a spindle for the live tool.
SOLUTION Yield a live tool to the channel or execute the cycle in a channel with live tool.

1934 'Wrong cutter width'

DETECTION During the execution of the cycle.
CAUSE The cutter width is larger than the slot (groove) or the cycle cannot leave the

programmed residual stock.

SOLUTION Check that the selected tool can machine the programmed slot (groove), leaving the

programmed finishing stock.

Error solving manual

1935 'No axis has been defined as LONGAXIS in C axis cycle'

DETECTION During the execution of the cycle.
CAUSE No longitudinal axis has been defined in the channel.
SOLUTION Set machine parameter LONGAXIS = TRUE for the longitudinal axis.

1936 'No axis has been defined as FACEAXIS in C axis cycle'

DETECTION During the execution of the cycle.
CAUSE No face axis has been defined in the channel.
SOLUTION Set machine parameter FACEAXIS = TRUE for the face axis.

1950 'The Z coordinate of the part surface has not been programmed'

DETECTION During the execution of the cycle.
CAUSE 'The coordinate of the part surface has not been programmed (parameter Z).
SOLUTION Correct the program.

1951 'The safety Z coordinate has not been programmed'

DETECTION During the execution of the cycle.
CAUSE The safety plane has not been programmed (parameter Zs).
SOLUTION Correct the program.

1952 'The part depth has not been programmed'

DETECTION During the execution of the cycle.
CAUSE The part depth has not been programmed (parameter P).
SOLUTION Correct the program.

1953 'The penetration step has not been programmed'

DETECTION During the execution of the cycle.
CAUSE The penetration step (parameter I) has not been programmed.
SOLUTION Correct the program.

1954 'The roughing pass has not been programmed'

DETECTION During the execution of the cycle.
CAUSE The roughing pass (parameter D) has not been programmed.
SOLUTION Correct the program.

1955 'Zero roughing tool radius'

DETECTION During the execution of the cycle.
CAUSE The roughing tool radius is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1956 'Zero finishing tool radius'

DETECTION During the execution of the cycle.
CAUSE The finishing tool radius is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1957 'Zero semi-finishing tool radius'

DETECTION During the execution of the cycle.
CAUSE The semi-finishing tool radius is 0.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1958 'Roughing tool radius too large'

DETECTION During the execution of the cycle.
CAUSE The roughing tool radius is too large for the geometry of the pocket.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1959 'Finishing tool radius too large'

DETECTION During the execution of the cycle.
CAUSE The finishing tool radius is too large for the geometry of the pocket.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

CNC 8070

(REF: 1308)

·97·

Error solving manual

1960 'Semi-finishing tool radius too large'

DETECTION During the execution of the cycle.
CAUSE The semi-finishing tool radius is too large for the geometry of the pocket.
SOLUTION Correct the value of the tool radius in the tool table or select another tool.

1961 'Wrong finishing tool tip radius'

DETECTION During the execution of the cycle.
CAUSE The tip radius (Rp) of the finishing tool is greater than its radius ( R ).
SOLUTION Correct the tool tip (nose) radius.

1962 'Wrong roughing penetration angle'

DETECTION During the execution of the cycle.
CAUSE The roughing penetration angle is not between 0º and 90º.
SOLUTION Correct the penetration angle; program a value between 0º and 90º.

1963 'Wrong semi-finishing penetration angle'

DETECTION During the execution of the cycle.
CAUSE The semi-finishing penetration angle is not between 0º and 90º.
SOLUTION Correct the penetration angle; program a value between 0º and 90º.

1964 'A roughing pass has been programmed greater than tool diameter'

DETECTION During the execution of the cycle.
CAUSE The roughing pass is greater than tool diameter.
SOLUTION Correct the location code (tool shape) or select another tool.

1965 'A finishing pass has been programmed greater than tool diameter'

DETECTION During the execution of the cycle.
CAUSE The finishing pass is greater than tool diameter.
SOLUTION Correct the location code (tool shape) or select another tool.

1966 'Wrong type of finishing'

DETECTION During the execution of the cycle.
CAUSE The type of finishing is wrong.
SOLUTION Assign a correct value to the parameters.

1967 'Wrong Z coordinate of the starting plane'

DETECTION During the execution of the cycle.
CAUSE The Z coordinate of the beginning of the cycle is located inside the part.
SOLUTION The Z coordinate of the beginning of the cycle must be above the reference plane.

1968 'Wrong safety Z coordinate

DETECTION During the execution of the cycle.
CAUSE The safety plane is located inside the part.
SOLUTION Assign a correct value to the parameter.

1969 'The programmed XY profile does not exist'

DETECTION During the execution of the cycle.
CAUSE The surface profile does not exist.
SOLUTION Edit the profile. The CNC saves the profiles in the folder ..\Users\Profile.

CNC 8070

(REF: 1308)

·98·

1970 'The programmed Z profile does not exist'

DETECTION During the execution of the cycle.
CAUSE The depth profile does not exist.
SOLUTION Edit the profile. The CNC saves the profiles in the folder ..\Users\Profile.

1971 'An open XY profile has been programmed'

DETECTION During the execution of the cycle.
CAUSE Some surface profile is not a closed profile; its initial and final points are not the same.
SOLUTION Check that all the surface profiles are closed.

Error solving manual

1972 'Wrong XY profile'

DETECTION During the execution of the cycle.
CAUSE The surface profile does not exist.
SOLUTION Edit the profile. The CNC saves the profiles in the folder ..\Users\Profile.

1973 'Wrong Z profile'

DETECTION During the execution of the cycle.
CAUSE Some depth profile is closed or the cycle cannot machine some depth profile with the

programmed tool.

SOLUTION Check that the depth profiles are correct.

1974 'Wrong profile intersection'

DETECTION During the execution of the cycle.
CAUSE Two surface profiles generate an invalid intersection.
SOLUTION Check that the surface profiles do not have sections in common, the profiles must

intersect in points.

1975 'Probing has not taken place'

DETECTION During the execution of a probing cycle.
CAUSE The probe has not touched the part during the probing movement.
SOLUTION Correct the definition of the canned cycle.

CNC 8070

(REF: 1308)

·99·

Error solving manual

2000-2999

2000 'Tool radius greater than the arc radius'

DETECTION During execution.
CAUSE The tool radius is greater than the radius of the arc to be machined.
SOLUTION Use a tool with a smaller radius.

2001 'Profile damaged by tool radius compensation'

DETECTION During execution.
CAUSE The tool radius is too large for the programmed profile; the tool will damage the profile.
SOLUTION Use a tool with a smaller radius.

2002 'The first block of the linear compensation must be linear'

DETECTION During execution.
CAUSE After activating tool radius compensation (G41 or G42), the next motion block is a

circular block. Tool radius compensation cannot begin in a circular block.

SOLUTION Tool radius compensation must begin in a linear block. Therefore, the motion block

that goes after G41-G42 must be a linear motion block.

2003 'Tool radius too large in consecutive arcs'

DETECTION During execution.
CAUSE When machining two consecutive arcs that form a loop (the two arcs intersect each

other), the tool radius is too large for machining the inside of the loop.

SOLUTION Use a tool with a smaller radius.

2004 'Too many motionless blocks between blocks that have tool radius compensation'

DETECTION During execution.
CAUSE While tool radius compensation is active, there are too many motionless blocks

(parameter assignments P, variables, etc.) between two motion blocks.

SOLUTION Reduce the number of motionless blocks programmed; for example, group several

of these blocks into a single block.

2005 'The last block of the linear compensation must be linear'

DETECTION During execution.
CAUSE After canceling tool radius compensation (G40), the next motion block is a circular

block. Tool radius compensation cannot end in a circular block.

SOLUTION Tool radius compensation must end in a linear block. Therefore, the motion block that

goes after G40 must be a linear motion block.

2006 'Tool radius compensation (G41/G42) must be changed on a linear path'

DETECTION During execution.
CAUSE The program has changed the type of tool radius compensation (from G41 to G42

or vice versa) and the next motion block is a circular block.

SOLUTION The tool radius compensation cannot be changed if the next motion block is an arc.

Change the type of radius compensation on a linear tool path.

CNC 8070

(REF: 1308)

·100·

2007 'While G138 is active, G40 is not allowed after the first compensation block'

DETECTION During execution.
CAUSE After activating tool radius compensation with the direct method (G138), a

compensation cancellation has been programmed before the first motion block.

SOLUTION To activate tool radius compensation with the direct method (G138), the CNC needs

an additional block in the plane besides the activation block. The CNC allows
canceling tool radius compensation after this movement. If this block cannot be
programmed, use the indirect method (G139) to activate tool radius compensation.