PROGRAMMING ERRORS. Fagor CNC 8055 para otras aplicaciones, CNC 8055 for lathes, CNC 8055 para tornos, CNC 8055 for other applications

   Error solution

PROGRAMMING ERRORS

0001 ‘Empty line’

DETECTION

CAUSE

SOLUTION

While editing at the CNC or while executing a program transmitted via DNC.

The possible causes are:

1. When trying to enter into a program or execute an empty block or containing the label (block number).

2. In the "Pattern repeat canned cycle (G66)", "Roughing canned cycle along the

X axis (G68)" or "Roughing canned cycle along the Z axis (G69)" when parameter

"S" (beginning of profile) is greater than parameter "E" (end of profile).

The solution for each cause is:

1. The CNC cannot enter into the program or execute an empty line. To enter an empty line in the program, use the «;» symbol at the beginning of that block. The

CNC will ignore the rest of the block.

2. The value of parameter "S" (block where the profile definition begins) must be lower than the value of parameter "E" (block where the profile definition ends).

0002 ‘Improper data’

DETECTION

CAUSE

SOLUTION



1. When editing an axis coordinate after the cutting conditions (F, S, T or D) or the

"M" functions.

2. When the marks of the block skip (conditional block /1, /2 or /3) are not at the beginning of the block.

3. When programming a block number greater than 99999999 while programming in ISO code.

4. While programming in high-level, the value of the RPT instruction exceeds 9999.


1. Remember the programming order.

2. Remember the programming order.

• Block skip (conditional block /1, /2 or /3).

• Label (N).

• "G" functions.

• Axis coordinates. (X, Y, Z…).

• Machining conditions (F, S, T, D).

• "M" functions.

3. Correct the syntax of the block. Program the labels between 0 and 99999999.

4. Correct the syntax of the block. Program a number of repetitions between 0 and

9999

0003 ‘Improper data order.’

DETECTION

CAUSE

SOLUTION


The machining conditions or the tool data have been programmed in the wrong order.

Remember that the programming order is:

… F...S...T...D...…

All the data need not be programmed.

·T· Model

Ref.1507

·5·


·T· Model

Ref.1507

0004 ‘No more information allowed in the block.’

DETECTION

CAUSE

SOLUTION



1. When editing a "G" function after an axis coordinate.

2. When trying to edit some data after a "G" function (or after its associated parameters) which must go alone in the block (or which only admits its own associated data).

3. When assigning a numeric value to a parameter that does not need it.


1. Remember that the programming order is:


• Label (N).

• "G" functions.

• Axis coordinates. (X, Y, Z…).


• "M" functions.

2. There are some "G" functions which carry associated data in the block. Maybe, this type of functions do not let program other type of information after their associated parameters. On the other hand, neither machining conditions, (F, S), tool data (T, D) nor "M" functions may be programmed.

3. There are some "G" functions having certain parameters associated to them which do not need to be defined with values.

0005 ‘Repeated information’

DETECTION

CAUSE

SOLUTION


The same data has been entered twice in a block.

Correct the syntax of the block. The same data cannot be defined twice in a block.

0006 ‘Improper data format’

DETECTION

CAUSE

SOLUTION


While defining the parameters of a machining canned cycle, a negative value has been assigned to a parameter which only admits positive values.

Verify the format of the canned cycle. In some canned cycles, there are parameters which only accept positive values.

0007 ‘Incompatible G functions.’

DETECTION

CAUSE

SOLUTION



1. When programming in the same block two "G" functions which are incompatible with each other.

2. When trying to define a canned cycle in a block containing a nonlinear movement

(G02, G03, G08, G09, G33).


1. There are groups of "G" functions which cannot go together in the block because they involve actions incompatible with each other. For example:

G01/G02: Linear and circular interpolation

G41/G42: Left-hand or right-hand tool radius compensation.

This type of functions must be programmed in different blocks.

2. A canned cycle must be defined in a block containing a linear movement. In other words, to define a cycle, a "G00" or a "G01" must be active. Nonlinear movements

(G02, G03, G08 and G09) may be defined in the blocks following the profile definition.

0008 ‘Nonexistent G function’

DETECTION

CAUSE

SOLUTION


A nonexistent "G" function has been programmed.

Check the syntax of the block and verify that a different "G" function is not being edited by mistake.

·6·


0009 ‘No more G functions allowed’

DETECTION

CAUSE

SOLUTION


A "G" function has been programmed after the machining conditions or after the tool data.



• Label (N).

• "G" functions.

• Axis coordinates. (X,Y,Z…).


• "M" functions.

0010 ‘No more M functions allowed’

DETECTION

CAUSE

SOLUTION


More than 7 "M" functions have been programmed in a block.

The CNC does not let program more than 7 "M" functions in a block. To execute any other functions, write them in a separate block. The "M" functions may go alone in a block.

0011 ‘This G or M function must be alone.’

DETECTION

CAUSE

SOLUTION


The block contains either a "G" or an "M" function that must go alone in the block.

Write it alone in the block.

0012 ‘Program F, S, T, D before the M functions.’

DETECTION

CAUSE

SOLUTION


A machining condition (F, S) or tool data (T, D) has been programmed after the "M" functions.


… F...S...T...D...M...

Up to 7 "M" functions may be programmed .

All the data need not be programmed.

0013 ‘Program G30 D +/-359.9999’

No explanation required.

0014 ‘Do not program labels by parameters.’

DETECTION

CAUSE

SOLUTION


A label (block number) has been defined with a parameter.

Programming the block number is optional, but it cannot be defined with a parameter

It can only be defined with a number between 0 and 99999999.

0015 ‘Number of repetitions not possible.’

DETECTION

CAUSE

SOLUTION


A repetition has been programmed wrong or the block does not admit repetitions.

High level instructions do not admit a number of repetitions at the end of the block.

To do a repetition, assign to the block to be repeated a label (block number) and use the RPT instruction.

0016 'Program: G15 or G15 C.’

DETECTION

CAUSE

SOLUTION


An attempt has been made to execute an operation on the "C" axis, but the axis is not active.

In order to operate with the "C" axis, it must be activated first using the "G15" function.

·T· Model

Ref.1507

·7·


·T· Model

0017 'Program: G16 axis-axis.’

DETECTION

CAUSE

SOLUTION


In the function "Main plane selection by two axes (G16)" one of the two parameters for the axes has not been programmed.

Check the syntax of the block. The definition of the "G16" function requires the name of the axes defining the new work plane.

0018 'Program: G22 K(1/2/3/4/5) S(0/1/2).’

DETECTION

CAUSE

SOLUTION


In the function "Enable/Disable work zones (G22)" the type of enable or disable of the work zone has not been defined or it has been assigned the wrong value.

The parameter for enabling or disabling the work zones "S" must always be programmed and it may take the following values.

• S=0: The work zone is disabled.

• S=1: It is enabled as a no-entry zone.

• S=2: It is enabled as a no-exit zone.

0019 ‘Program zone K1, K2, K3, K4 or K5.’

DETECTION

CAUSE

SOLUTION



1. A "G20", "G21" or "G22" function has been programmed without defining the work zone K1, K2, K3, K4 or K5

2. The programmed work zone is smaller than 0 or greater than 5.


1. The programming format for functions "G20", "G21" and "G22" is:

G20 K...X...C±5.5

Definition of lower work zone limits.

G21 K...X...C±5.5

Definition of upper work zone limits.

G22 K...S...

Enable/disable work zones.

Where:

K Is the work zone.

X...C Are the axes where the limits are defined.

S Is the type of work zone enable.

2. The "K" work zone may only have the values of K1, K2, K3, K4 or K5.

0020 ‘Program G36-G39 with R+5.5.’

DETECTION

CAUSE

SOLUTION


In the "G36" or "G39" function, the "R" parameter has not been programmed or it has been assigned a negative value.

To define "G36" or "G39", parameter "R" must also be defined and with a positive value).

G36 R= Rounding radius.

G39 R= Distance between the end of the programmed path and the point to be chamfered.

0021 'Program: G72 S5.5 or axis (axes).’

DETECTION

CAUSE

SOLUTION



1. When programming a general scaling factor (G72) without the scaling factor to apply.

2. When programming a particular scaling factor (G72) to several axes, but the axes have been defined in the wrong order.

Remember that the programming format for this function is:

G72 S5.5” When applying a general scaling factor (to all axes).

G72 X…C5.5” When applying a particular scaling factor to one or several axes.

Ref.1507

·8·


0023 ‘Block incompatible when defining a profile.’

DETECTION

CAUSE

SOLUTION


In the set of blocks defining a profile, there is a block containing a "G" function that cannot be part of the profile definition.

The "G" functions available in the profile definition are:

G00: Beginning of the profile.

G01: Linear interpolation.

G02/G03: Clockwise/counterclockwise interpolation.

G06: Circle center in absolute coordinates.

G08: Arc tangent to previous path.

G09: Three point arc.

G36: Automatic radius blend.

G39: Chamfer.

G53: Programming with respect to home.

G70/G71: Inch/metric programming.

G90/G91: Programming in absolute/incremental coordinates.

G93: Polar origin preset.

0024 ‘High level blocks not allowed when defining a profile.’

DETECTION

CAUSE

SOLUTION


Within the set of blocks defining a profile, a high level block has been programmed.

Profiles must be defined in ISO code. High level instructions are not allowed (GOTO,

MSG, RPT ...).

0025 'Program: G77 axes (2 to 6) or G77 S.’

DETECTION

CAUSE

SOLUTION


In the "axis slaving function (G77)" the parameters for the axes are missing or in

"spindle synchronization (G77S) functions the "S" parameter is missing.

In the "axis slaving" function, program at least two axes and in the "spindle synchronization" function, always program the "S" parameter.

0026 'Program: G93 I J.’

DETECTION

CAUSE

SOLUTION


In the "Polar origin preset (G93)" function, some of the parameters for the new polar origin have not been programmed.


G93 I...J...

The "I", "J" values are optional, but if programmed, both must be programmed and they indicate the new polar origin.

0028 ‘G2 or G3 not allowed when programming a canned cycle.’

DETECTION

CAUSE

SOLUTION


A canned cycle has been attempted to execute while the "G02", "G03" or "G33" functions were active.

To execute a canned cycle, "G00" or "G01" must be active. A "G02" or "G03" function may be programmed previously in the program history. Check that these functions are not active when the canned cycle is defined.

·T· Model

Ref.1507

·9·


·T· Model

Ref.1507

0029 ‘G84-85: X Z Q R C [D L M F H] I K.’

DETECTION

CAUSE

SOLUTION


The parameters of the canned cycle for "Turning of curved sections (G84)" or for

"Facing curved sections (G85)" have been programmed wrong. These may be the probable causes:

1. Some mandatory parameter is missing.

2. The parameters of the cycle have not been edited in the correct order.

3. A parameter has been programmed which does not match the calling format.

The following parameters must be programmed in this cycle:

X-Z Profile starting point

Q-R Profile end point

C Depth of pass.

I-K Distance from the starting point to the arc center.

The rest of the parameters are optional. The parameters must be edited in the order indicated by the error message.

0030 ‘G86-87: X Z Q R I B [D L] C [J A].’

DETECTION

CAUSE

SOLUTION


The parameters of the canned cycle for "longitudinal threadcutting (G86)" or for "face threadcutting (G87)" have been programmed wrong. These may be the probable causes:





I

B

X-Z Starting point of the thread.

Q-R End point of the thread.

Thread depth.

Depth of pass.

C Thread pitch.


0031 ‘G88-G98: X Z Q R [C D K].’

DETECTION

CAUSE

SOLUTION


The parameters of the canned cycle for "grooving along X (G88)" or "grooving along

Z (G89)" have been programmed wrong. These may be the probable causes:





X-Z Starting point of the groove.

Q-R End point of the groove.


0032 ‘G66: X Z I C [A L M H] S E.’

DETECTION

CAUSE

SOLUTION


The parameters of the "Pattern repeat canned cycle with islands (G66)" have been programmed wrong. These may be the probable causes:





S

E


I Remaining stock.

C Depth of pass.

Block where the profile geometry description begins.

Block where the profile geometry description ends.


·10·


0033 ‘G68-G69: X Z C [D L M F H] S E .’

DETECTION

CAUSE

SOLUTION


The parameters of the canned cycle for "roughing along X (G68)" or "roughing along

Z (G69)" have been programmed wrong. These may be the probable causes:





S

E


C Depth of pass.

Block where the profile geometry description begins.

Block where the profile geometry description ends.


0034 ‘G81-G82: X Z Q R C [D L M F H].’

DETECTION

CAUSE

SOLUTION


The parameters of the canned cycle for "Turning of straight sections (G81)" or for

"Facing straight sections (G82)" have been programmed wrong. These may be the probable causes:






Q-R Profile end point

C Depth of pass.


0035 ‘G83: X Z I B [D K H C L R].’

DETECTION

CAUSE

SOLUTION


The parameters have been programmed wrong in the "Axial drilling/tapping cycle

(G83)". These may be the probable causes:





X-Z Machining position.

I

B

Machining depth.

Type of operation.


·T· Model

Ref.1507

·11·


·T· Model

0036 ‘G60-G61: X Z I B Q A J [D K H C] S [L R].’

DETECTION

CAUSE

SOLUTION


The parameters of the canned cycle for "face drilling or tapping (G60)" or for

"longitudinal drilling or tapping (G61)" have been programmed wrong. These may be the probable causes:





A

J

S

X-Z Machining position.

I

B

Machining depth.

Type of operation.

Q Angular position of the first machining operation.

Angular step between machining operations.

Number of machining operations.

Live tool turning speed and direction.


0037 ‘G62-G63: X Z L I Q A J [D] F S.’

DETECTION

CAUSE

SOLUTION


The parameters of the canned cycle for "longitudinal slot milling (G62)" or "face slot milling (G62)" have been programmed wrong. These may be the probable causes:




F

S

A

J

X-Z Slot position.

L Slot length.

I Slot depth.

Q Angular position of the first slot.

Angular step between slots.

Number of slots.

Feedrate.

Live tool turning speed and direction.


0043 ‘Incomplete Coordinates.’

DETECTION

CAUSE

SOLUTION



1. During simulation or execution, when trying to make a movement defined with only one coordinate of the end point or without defining the arc radius while a

"circular interpolation (G02/G03) is active.

2. During editing, when editing a circular movement (G02/G03) by defining only one coordinate of the end point or not defining the arc radius.


1. A "G02" or "G03" function may be programmed previously in the program history.

In this case, to make a move, both coordinates of the end point and the arc radius must be defined. To make a linear movement, program "G01".

2. To make a circular movement (G02/G03), both coordinates of the end point and the arc radius must be programmed.

0044 ‘Incorrect Coordinates.’

DETECTION

CAUSE

SOLUTION

During the execution in programs transmitted via DNC.

An attempt has been made to execute a block syntactically incorrect (G1 X20K-15)

Correct the syntax of the block.

Ref.1507

·12·


0045 ‘Polar coordinates not allowed.’

DETECTION

CAUSE

SOLUTION


When "Programming with respect to home (G53)", the end point has been defined in polar or cylindrical coordinates or in Cartesian coordinates with an angle.

When programming with respect to home, only Cartesian coordinates may be programmed.

0046 ‘Axis does not exist.’

DETECTION

CAUSE

SOLUTION


A block has been edited whose execution involves the movement of a nonexistent axis.

Check that the axis name being edited is correct.

0047 ‘Program axes.’

DETECTION

CAUSE

SOLUTION


No axis has been programmed in a function requiring an axis.

Some instructions require the programming of axes (REPOS, G14, G20, G21...).

0048 ‘Incorrect order of axes.’

DETECTION

CAUSE

SOLUTION


The axis coordinates have not been programmed in the correct order or an axis has been programmed twice in the same block.

Remember that the correct programming order for the axes is:

X...Y...Z...U...V...W...A...B...C...

All axes need not be programmed:

0049 ‘Point incompatible with active plane.’

DETECTION

CAUSE

SOLUTION



1. When trying to do a circular interpolation, the end point is not in the active plane.

2. When trying to do a tangential exit in a path that is not in the active plane.


1. Maybe a plane has been defined with "G16", "G17", "G18" or "G19". In this case, circular interpolations can only be carried out on the main axes defining that plane.

To define a circular interpolation in another plane, it must be defined beforehand.

2. Maybe a plane has been defined with "G16", "G17", "G18" or "G19". In this case, corner rounding, chamfers and tangential entries/exits can only be carried out on the main axes defining that plane. To do it in another plane, it must be defined beforehand.

0050 ‘Program positions on active plane.’


0051 ‘Perpendicular axis included in active plane.’


0052 ‘Center of circle programmed incorrectly.’


0053 ‘Program pitch.’

DETECTION

CAUSE

SOLUTION


In the "Electronic threading cycle (G33)" the parameter for the thread pitch is missing.


G33 X...C...L...

Where: "L" is the thread pitch.

·T· Model

Ref.1507

·13·


0054 ‘Pitch programmed incorrectly.’

DETECTION

CAUSE

SOLUTION


A helical interpolation has been programmed with the wrong or negative pitch.

Remember that the programming format is:

G02/G03 X...Y...I...J...Z...K...

Where: "K" is the helical pitch (always positive value).

0055 ‘Positioning axes or Hirth axes not allowed’


0056 ‘The axis is already slaved.’


0057 ‘Do not program a slaved axis.’

DETECTION

CAUSE

SOLUTION



1. When trying to move an axis alone while being slaved to another one.

2. When trying to slave an axis that is already slaved using the G77 function

"Electronic axis slaving".


1. A slaved axis cannot be moved separately. To move a slaved axis, its master axis must be moved. Both axes will move at the same time.

Example: If the Y axis is slaved to the X axis, an X axis move must be programmed in order to move the Y axis (together with the X axis).

To unslave the axes, program "G78".

2. An axis cannot be slaved to two different axes at the same time. To unslave the axes, program "G78".

0058 ‘Do not program a GANTRY axis.’

DETECTION

CAUSE

SOLUTION



1. When trying to move an axis alone while being slaved to another one as a

GANTRY axis

2. When defining an operation on a GANTRY axis. (Definition of work zone limits, planes, etc.).


1. A GANTRY axis cannot be moved separately. To move a GANTRY axis, its associated axis must be moved. Both axes will move at the same time.

Example: If the Y axis is a GANTRY axis associated with the X axis, an X axis move must be programmed in order to move the Y axis (together with the X axis).

GANTRY axes are defined by machine parameter.

2. The axes defined as GANTRY cannot be used in the definition of operations or movements. These operations are defined with the main axis that the GANTRY axis is associated with.

0059 'Wrong position programmed for the Hirth axis.'

DETECTION

CAUSE

SOLUTION


A rotation of a HIRTH axis has been programmed with a decimal value.

HIRTH axes do not accept decimal angular values. They must be full degrees.

0060 ‘Invalid action.’


·T· Model

Ref.1507

·14·


0061 ‘ELSE not associated with IF.’

DETECTION

CAUSE

SOLUTION



1. While editing in High level language, when editing the "ELSE" instruction without having previously programmed an "IF".

2. When programming in high level language, an "IF" is programmed without associating it with any action after the condition.

Remember that the programming formats for this instruction are:

(IF (condition) <action1>)

(IF (condition <action1> ELSE <action2>)

If the condition is true, it executes the <action1>, otherwise, it executes <action2>.

0062 ‘Program label N(0-99999999).’

DETECTION

CAUSE

SOLUTION


While programming in high level language, a block number out of the 0-99999999 range has been programmed in the "RPT" or "GOTO" instruction.

Remember that the programming format of these instructions is:

(RPT N(block number), N(block number))

(GOTO N(block number))

The block number (label) must be between 0 and 99999999.

0063 ‘Program subroutine number 1 thru 9999.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, a subroutine number out of the 0-9999 range has been programmed in the "SUB" instruction.

Remember that the programming format for this instruction is:

(SUB (integer))

The subroutine number must be between 0 and 9999.

0064 ‘Repeated subroutine.’

DETECTION

CAUSE

SOLUTION


There has been an attempt to define a subroutine already existing in another program of the memory.

In the CNC memory, there could not be more than one subroutine with the same identifying number even if they are contained in different programs.

0065 ‘The main program cannot have a subroutine.’

DETECTION

CAUSE

SOLUTION

In execution or while executing programs transmitted via DNC.


1. An attempt has been made to define a subroutine in the MDI execution mode.

2. A subroutine has been defined in the main program.


1. Subroutines cannot be defined from the "MDI execution" option of the menu.

2. Subroutines must be defined after the main program or in a separate program.

They cannot be defined before or inside the main program.

0066 ‘Expecting a message.’

DETECTION

CAUSE

SOLUTION


While programming in high level, the "MSG" or "ERROR" instruction has been edited but without the message to be displayed.

Remember that the programming format of these instructions is:

(MSG "message")

(ERROR integer, "error message")

Although it can also be programmed as follows:

(ERROR integer)

(ERROR "error message")

·T· Model

Ref.1507

·15·


0067 ‘OPEN is missing.’

DETECTION

CAUSE

SOLUTION


While programming in high level, a "WRITE" instruction has been edited, but the

OPEN instruction has not been written previously to tell it where that instruction has to be executed.

The "OPEN" instruction must be edited before the "WRITE" instruction to "tell" the

CNC where (in which program) it must execute the "WRITE" instruction.

0068 ‘Expecting a program number.’


0069 ‘Program does not exist.’

DETECTION

CAUSE

SOLUTION


In the "Pattern repeat canned cycle (G66)", "Roughing canned cycle along the X axis

(G68)" or "Roughing canned cycle along the Z axis (G69)", it has been programmed that the profiles are located in another program (parameter "Q"), but the program does not exist.

Parameter "Q" defines which program contains the profile definitions of the cycles.

If this parameter is programmed, that program number must exist and it must contain the labels defined by parameters "S" and "E".

0070 ‘Program already exists.’

DETECTION

CAUSE

SOLUTION


This error comes up during execution when using the "OPEN" instruction (While programming in high level language) to create an already existing program.

Change the program number or use parameters A/D in the "OPEN" instruction:

(OPEN P.........,A/D,… )

Where:

A: Appends new blocks after the existing ones.

D: Deletes the existing program and it opens it as a new one.

0071 ‘Expecting a parameter’

DETECTION

CAUSE

SOLUTION

While editing tables.

The wrong parameter number has been entered (maybe the "P" character is missing) or another action is being carried out (moving around in the table) before quitting the table editing mode.

Enter the parameter number to be edited or press [ESC] to quit this mode.

0072 ‘Parameter does not exist.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, the "ERROR" instruction has been edited, but the error number to be displayed has been defined either with a local parameter greater than 25 or with a global parameter greater than 299.

The parameters used by the CNC are:

Local:

Global:

0-25

100-299

0073 ‘Range of write-protected parameters.


0074 ‘Variable not accessible from CNC.’


·T· Model

Ref.1507

·16·


0075 ‘Read-only variable.’

DETECTION

CAUSE

SOLUTION


An attempt has been made to assign a value to a read-only variable.

Read-only variables cannot be assigned any values through programming. However, their values can be assigned to a parameter.

0076 ‘Write-only variable.’


0077 ‘Analog output not available.’

DETECTION

CAUSE

SOLUTION


An attempt has been made to write to an analog output currently being used by the

CNC.

The selected analog output may be currently used by an axis or a spindle. Select another analog output between 1 and 8.

0078 ‘Program channel 0(CNC),1(PLC) or 2(DNC).’

DETECTION

CAUSE

SOLUTION


While programming in high level language, the "KEYSCR" instruction has been programmed, but the source of the keys is missing.

When programming the "KEYSCR" instruction, the parameter for the source of the keys must always be programmed:

(KEYSCR=0) : CNC keyboard

(KEYSCR=1) : PLC

(KEYSCR=2) : DNC

The CNC only lets modifying the contents of this variable if it is "zero"

0079 ‘Program error number 0 thru 9999.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, the "ERROR" instruction has been programmed, but the error number to be displayed is missing.


(ERROR integer, "error message")

Although it can also be programmed as follows:

(ERROR integer)

(ERROR "error message")

0080 ‘Operator missing.’


0081 ‘Incorrect expression.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, an expression has been edited with the wrong format.

Correct the syntax of the block.

0082 ‘Incorrect operation.’

DETECTION

CAUSE

SOLUTION



1. While programming in high level language, the assignment of a value to a parameter is incomplete.

2. While programming in high level language, the call to a subroutine is incomplete.

Correct (complete) the format to assign a value to a parameter or a call to a subroutine.

·T· Model

Ref.1507

·17·


·T· Model

0083 ‘Incomplete operation.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, the "IF" instruction has been edited without the condition between brackets.


(IF (condition) <action1>)

(IF (condition <action1> ELSE <action2>)

If the condition is true, it executes the <action1>, otherwise, it executes <action2>.

0084 ‘Expecting "=".’

DETECTION

CAUSE

SOLUTION


While programming in high level language, a symbol or data has been entered that does not match the syntax of the block.

Enter the "=" symbol in the right place.

0085 ‘Expecting ")".’

DETECTION

CAUSE

SOLUTION



Enter the ")" symbol in the right place.

0086 ‘Expecting "(".’

DETECTION

CAUSE

SOLUTION



Enter the "(" symbol in the right place.

0087 ‘Expecting ",".’

DETECTION

CAUSE

SOLUTION



1. While programming in high level language, a symbol or data has been entered that does not match the syntax of the block.

2. While programming in high level language, an ISO-coded instruction has been programmed.

3. While programming in high level language, an operation has been assigned either to a local parameter greater than 25 or to a global parameter greater 299.


1. Enter the "," symbol in the right place.

2. A block cannot contain high level language instructions and ISO-coded instructions at the same time.

3. The parameters used by the CNC are:

Local:

Global:

0-25.

100-299.

Other parameters out of this range cannot be used in operations.

0088 ‘Operation limit exceeded.’


0089 ‘Logarithm of zero or negative number.’

DETECTION

CAUSE

SOLUTION


An operation has been programmed which involves the calculation of a negative number or a zero.

Only logarithms of numbers greater than zero can be calculated. When working with parameters, that parameter may have already acquired a negative value or zero.

Verify that the parameter does not reach the operation with that value (0).

Ref.1507

·18·


0090 ‘Square root of a negative number.’

DETECTION

CAUSE

SOLUTION


An operation has been programmed which involves the calculation of the square root of a negative number.

Only the square root of numbers greater than zero can be calculated. When working with parameters, that parameter may have already acquired a negative value or zero.


0091 ‘Division by zero.’

DETECTION

CAUSE

SOLUTION


An operation has been programmed whose execution involves dividing by zero.

It is only possible to divide by numbers other than zero. When working with parameters, that parameter may have already acquired a negative value or zero.


0092 ‘Base zero with positive exponent.’

DETECTION

CAUSE

SOLUTION


An operation has been programmed which involves elevating zero to a negative exponent (or zero).

Zero can only be elevated to positive exponents greater than zero. When working with parameters, that parameter may have already acquired a negative value or zero.

Check that the parameter does not reach the operation with that value.

0093 ‘Negative base with decimal exponent.’

DETECTION

CAUSE

SOLUTION


An operation has been programmed which involves elevating a negative number to a decimal exponent.

Negative numbers can only be elevated to integer exponents. When working with parameters, that parameter may have already acquired a negative value or zero.

Check that the parameter does not reach the operation with that value.

0094 ‘ASIN/ACOS range exceeded.’

DETECTION

CAUSE

SOLUTION


An operation has been programmed which involves calculating the arcsine or arccosine of a number out of the ±1 range.

Only the arc sine (ASIN) or the arc cosine (ACOS) of numbers between ±1 can be calculated. When working with parameters, that parameter may have already acquired a value out of the mentioned values. Verify that the parameter does not reach the operation with that value (0).

0095 ‘Program row number.’

DETECTION

CAUSE

SOLUTION


While editing a customizing program, a window has been programmed with the

"ODW" instruction, but the vertical position of the window on the screen is missing.

The vertical position of the window on the screen is defined by rows (0-25).

0096 ‘Program column number.’

DETECTION

CAUSE

SOLUTION


While editing a customizing program, a window has been programmed with the

"ODW" instruction, but the horizontal position of the window on the screen is missing.

The horizontal position of the window on the screen is defined by columns (0-79).

·T· Model

Ref.1507

·19·


·T· Model

0097 ‘Program another softkey.’

DETECTION

CAUSE

SOLUTION


While editing a customizing program, the programming format for the "SK" instruction has not been respected.

Correct the syntax of the block. The programming format is:

(SK1=(text 1), SK2=(text 2)...)

If the "," character is entered after a text, the CNC expects the name of another softkey.

0098 ‘Program softkeys 1 thru 7.’

DETECTION

CAUSE

SOLUTION

While executing in the user channel.

In the block syntax, a softkey has been programmed out of the 1 to 7 range.

Only softkeys within the 1 to 7 range can be programmed.

0099 ‘Program another window.’

DETECTION

CAUSE

SOLUTION


While editing a customizing program, the programming format for the "DW" instruction has not been respected.


(DW1=(assignment), DW2=(assignment)...)

If the "," character is entered after an assignment, the CNC expects the name of another window.

0100 ‘Program windows 0 thru 25.’

DETECTION

CAUSE

SOLUTION


In the block syntax, a window has been programmed out of the 0 to 25 range.

Only windows within the 0 to 25 range can be programmed.

0101 ‘Program rows 0 thru 20.’

DETECTION

CAUSE

SOLUTION


In the block syntax, a row has been programmed out of the 0 to 20 range.

Only rows within the 0 to 20 range can be programmed.

0102 ‘Program columns 0 thru 79.’

DETECTION

CAUSE

SOLUTION


In the block syntax, a column has been programmed out of the 0 to 79 range.

Only columns within the 0 to 79 range can be programmed.

0103 ‘Program pages 0 thru 255.’

DETECTION

CAUSE

SOLUTION


In the block syntax, a page has been programmed out of the 0 to 255 range.

Only pages within the 0 to 255 range can be programmed.

0104 ‘Program INPUT.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, an "IB" instruction has been edited without associating an "INPUT" to it.


(IB (expression) = INPUT "text", format)

(IB (expression) = INPUT "text")

0105 ‘Program inputs 0 thru 25.’

DETECTION

CAUSE

SOLUTION


In the block syntax, an input has been programmed out of the 0 to 25 range.

Only inputs within the 0 to 25 range can be programmed.

Ref.1507

·20·


0106 ‘Program numerical format.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, an "IB" instruction has been edited with non-numeric format.



Where "format" must be a signed number with 6 entire digits and 5 decimals at the most.

If the "," character is entered after the text, the CNC expects the format.

0107 ‘Do not program formats greater than 6.5 .’

DETECTION

CAUSE

SOLUTION


While programming in high level language, an "IB" instruction has been edited in a format with more than 6 entire digits or more than 5 decimals.



Where "format" must be a signed number with 6 entire digits and 5 decimals at the most.

0108 ‘This command can only be executed in the user channel.’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to execute a block containing information that can only be executed through the user channel.

There are specific expressions for customizing programs that can only be executed inside the user program.

0109 ‘C. user: do not program geometric help, compensation or cycles.’

DETECTION

CAUSE

SOLUTION


An attempt has been made to execute a block containing geometric aide, tool radius/length compensation or machining canned cycles.

Inside a customizing program the following cannot be programmed:

Neither geometric assistance nor movements.

Neither tool radius nor length compensation.

Canned cycles.

0110 ‘Local parameters not allowed.’

DETECTION

CAUSE

SOLUTION


Some functions can only be programmed with global parameters.

Global parameters are the ones included in the 100-299 range.

0111 ‘Block cannot be executed while running another program’

DETECTION

CAUSE

SOLUTION

While executing in MDI mode

An attempt has been made to execute a customizing instruction from MDI mode while the user channel program is running.

Customizing instructions can only be executed through the user channel.

0112 ‘WBUF can only be executed in user channel while editing’

DETECTION

CAUSE

SOLUTION

During normal execution or execution through the user channel.

An attempt has been made to execute the "WBUF" instruction.

The "WBUF" instruction cannot be executed. It can only be used in the editing stage through the user input.

·T· Model

Ref.1507

·21·


·T· Model

0113 ‘Table limits exceeded.’

DETECTION

CAUSE

SOLUTION



1. In the tool offset table, an attempt has been made to define a tool offset with a greater number than allowed by the manufacturer.

2. In the parameter tables, an attempt has been made to define a nonexistent parameter.

The tool offset number must be smaller than the one allowed by the manufacturer.

0114 ‘Offset: D3 X Z R F I K.’

DETECTION

CAUSE

SOLUTION


In the tool offset table, the parameter editing order has not been respected.

Enter the table parameters in the right order.

0115 ‘Tool: T4 D3 F3 N5 R5(.2).’

DETECTION

CAUSE

SOLUTION


In the tool table, the parameter editing order has not been respected.


0116 ‘Origin: G54-59 G159N(1-20) axes (1-7).’

DETECTION

CAUSE

SOLUTION


In the Zero offset table, the zero offset to be defined (G54-G59) or G159N(1-20) has not be selected.

Enter the table parameters in the right order. To fill out the zero offset table, first select the offset to be defined (G54-G59) or G159N(1-20) and then the zero offset position for each axis.

0117 ‘M function: M4 S4 bits (8).’

DETECTION

CAUSE

SOLUTION


In the "M" function table, the parameter editing order has not been respected.

Edit table following the format:

M1234 (associated subroutine) (customizing bits)

0118 ‘G51 [A] E’

DETECTION

CAUSE

SOLUTION


In the "Look-Ahead (G51)" function, the parameter for the maximum contouring error is missing.

This type of machining requires the programming of:

E : Maximum contouring error.


0119 ‘Leadscrew: Coordinate-error.’

DETECTION

CAUSE

SOLUTION


In the leadscrew compensation tables, the parameter editing order has not been respected.


P123 (position of the axis to be compensated) (leadscrew error at that point)

0120 ‘Incorrect axis.’

DETECTION

CAUSE

SOLUTION


In the leadscrew compensation tables, an attempt has been made to edit a different axis from the one corresponding to that table.

Each axis has its own table for leadscrew compensation. The table for each axis can only contain the positions for that axis.

Ref.1507

·22·


0121 ‘Program P3 = value.’

DETECTION

CAUSE

SOLUTION


In the machine parameter table, the editing format has not been respected.


P123 = (parameter value)

0122 'Tool magazine: Magazine:

DETECTION

CAUSE

SOLUTION


In the tool magazine table, the editing format has not been respected or some data is missing.


0123 ‘Tool T0 does not exist.’

DETECTION

CAUSE

SOLUTION


In the tool table, an attempt has been made to edit a tool as T0.

No tool can be edited as T0. The first tool must be T1.

0124 ‘Offset D0 does not exist.’

DETECTION

CAUSE

SOLUTION


In the tool table, an attempt has been made to edit a tool offset as D0.

No tool offset can be edited as D0. The first tool offset must be D1.

0125 ‘Do not modify the active tool or the next one.’

DETECTION

CAUSE

SOLUTION

During execution.

In the tool magazine table, an attempt has been made to change the active tool or the next one.

During execution, neither the active tool nor the next one may be changed.

0126 ‘Tool not defined.’

DETECTION

CAUSE

SOLUTION


In the tool magazine table, an attempt has been made to assign to the magazine position a tool that is not defined in the tool table.

Define the tool in the tool table.

0127 ‘Magazine is not RANDOM.’

DETECTION

CAUSE

SOLUTION


There is no RANDOM magazine and, in the tool magazine table, the tool number does not match the tool magazine position.

When the tool magazine is not RANDOM, the tool number must be the same as the magazine position (pocket number).

0128 ‘The position of a special tool is set.’

DETECTION

CAUSE

SOLUTION


In the tool magazine table, an attempt has been made to place a tool in a magazine position reserved for a special tool.

When a special tool occupies more than one position in the magazine, it has a reserved position in the magazine. No other tool can be placed in this position.

0129 ‘Next tool only possible in machining centers.’

DETECTION

CAUSE

SOLUTION

During execution.

A tool change has been programmed with M06, but the machine is not a machining center. (it is not expecting the next tool).

When the machining is not a machining center, the tool change is done automatically when programming the tool number "T".

·T· Model

Ref.1507

·23·


0130 ‘Write 0/1.’

DETECTION

CAUSE

SOLUTION

0131 ‘Write +/-.’

DETECTION

CAUSE

SOLUTION

While editing machine parameters

An attempt has been made to assign the wrong value to a parameter.

The parameter only admits values of 0 or 1.



The parameter only admits values of + or -.

0132 ‘Write YES/NO.’

DETECTION

CAUSE

SOLUTION



The parameter only admits values of YES or NO.

0133 ‘Write ON/OFF.’

DETECTION

CAUSE

SOLUTION



The parameter only admits values of ON or OFF.

0134 ‘Values 0 thru 2.’

0135 ‘Values 0 thru 3.’

0136 ‘Values 0 thru 4.’

0137 ‘Values 0 thru 9.’

0138 ‘Values 0 thru 29.’

0139 ‘Values 0 thru 100.’

0140 ‘Values 0 thru 255.’

0141 ‘Values 0 thru 9999.’

0142 ‘Values 0 thru 32767.’

0143 ‘Values within +/-32767.’

0144 ‘Values 0 thru 65535.’

DETECTION

CAUSE



1. An attempt has been made to assign the wrong value to a parameter.

2. During execution, when inside the program a call has been made to a subroutine

(MCALL, PCALL) with a value greater than allowed.

0145 ‘Format +/- 5.5.’

DETECTION

CAUSE

SOLUTION



The parameter only admits values with the format:

0146 ‘Word does not exist.’


0147 ‘Numerical format exceeded.’

DETECTION

CAUSE

SOLUTION


A data or parameter has been assigned a value greater than the established format.

Correct the syntax of the block. Most of the time, the numeric format will be 5.4 (5 integers and 4 decimals).

·T· Model

Ref.1507

·24·


0148 ‘Text too long.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, the "ERROR" or "MSG" instruction has been assigned a text with more than 59 characters.

Correct the syntax of the block. The "ERROR" and "MSG" instructions cannot be assigned texts longer than 59 characters.

0149 ‘Incorrect message.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, the text associated with the "ERROR" or "MSG" instruction has been edited wrong.


(MSG "message")

(ERROR number, "message")

The message must be between " ".

0150 ‘Incorrect number of bits.’

DETECTION

CAUSE

SOLUTION



1. In the "M" function table, in the section on customizing bits:

The number does not have 8 bits.

The number does not consist of 0’s and 1’s.

2. In the machine parameter table, an attempt has been made to assign the wrong value of bit to a parameter.


1. The customizing bits must consist of 8 digits of 0’s and 1’s.

2. The parameter only admits 8-bit or 16-bit numbers.

0151 ‘Negative numbers not allowed.’


0152 ‘Incorrect parametric programming.’

DETECTION

CAUSE

SOLUTION

During execution.

The parameter has a value that is incompatible with the function it has been assigned to.

This parameter may have taken the wrong value, in the program history. Correct the program so this parameter does not reach the function with that value.

0153 ‘Decimal format not allowed.’


0154 ‘Insufficient memory.’

DETECTION

CAUSE

SOLUTION

During execution.

The CNC does not have enough memory to internally calculate the paths.

Sometimes, this error is taken care of by changing the machining conditions.

0155 ‘Help not available.’


0156 ‘Don’t program G33 ,G95 or M19 S with no spindle encoder’

DETECTION

CAUSE

SOLUTION


A "G33", "G95" or "M19 S" has been programmed without having an encoder on the spindle.

If the spindle does not have an encoder, functions "M19 S", "G33" or "G95" cannot be programmed. Spindle machine parameter "NPULSES (P13)" indicates the number of encoder pulses per turn.

·T· Model

Ref.1507

·25·


0159 ‘Inch programming limit exceeded.’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to execute in inches a program edited in millimeters.

Enter function G70 (inch programming) or G71 (mm programming) at the beginning of the program.

0162 ‘No negative radius allowed with absolute coordinates’

DETECTION

CAUSE

SOLUTION

During execution.

While operating with absolute polar coordinates, a movement with a negative radius has been programmed.

Negative radius cannot be programmed when using absolute polar coordinates.

0164 ‘Wrong password.’

DETECTION

CAUSE

SOLUTION

While assigning protections.

[ENTER] has been pressed before selecting the type of code to be assigned a password.

Use the softkeys to select the type of code to which a password is to be assigned.

0165 ‘Password: use uppercase/lowercase letters or digits.’

DETECTION

CAUSE

SOLUTION

While assigning protections.

A bad character has been entered in the password.

The password can only consist of letters (upper and lower case) or digits.

0166 ‘Only one HIRTH axis per block is allowed.’

DETECTION

CAUSE

SOLUTION


A movement has been programmed which involves the movement of two HIRTH axes simultaneously.

The CNC does not admit movements involving more than one HIRTH axis at a time.

HIRTH axes must move one at a time.

0167 ‘Rot. axis position.: absolute values (G90) between 0-359.9999.’

DETECTION

CAUSE

SOLUTION

During execution.

A movement of a positioning-only rotary axis has been programmed. The movement has been programmed in absolute coordinates (G90) and the target coordinate of the movement is not within the 0 to 359.9999 range.

Positioning-only rotary axes: In absolute coordinates, only movements within the 0 to 359.9999 range are possible.

= 0168 'Rotary axis: absolute values (G90) within ±359.9999.’

DETECTION

CAUSE

SOLUTION

During execution.

A movement of a rotary axis has been programmed. The movement has been programmed in absolute coordinates (G90) and the target coordinate of the movement is not within the 0 to 359.9999 range.

Rotary axes: In absolute coordinates, only movements within the 0 to 359.9999 range are possible.

0169 ‘Modal subroutines cannot be programmed.’

DETECTION

CAUSE

SOLUTION

While executing in MDI mode

An attempt has been made to call upon a modal subroutine (MCALL).

MCALL modal subroutines cannot be executed from the menu option "MDI execution".

·T· Model

Ref.1507

·26·


0170 ‘Program symbols 0 thru 255 in positions 0-639, 0-335. ‘


0171 ‘The window must be previously defined.’

DETECTION

CAUSE

SOLUTION

During normal execution or execution through the user channel.

An attempt has been made to write in a window (DW) that has not been previously defined (ODW).

It is not possible to write in a window that has not been previously defined. Check that the window to write in (DW) has been previously defined.

0172 ‘The program is not accessible’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to execute a program that cannot be executed.

The program may be protected against execution. To know whether a program may be executed, check for the "X" character on the attributes column. If this character is missing, the program cannot be executed.

0173 ‘It is not possible to program angle + angle.’


0174 ‘Circular (helical) interpolation not possible.’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to execute a helical interpolation while the "LOOK-

AHEAD (G51)" function was active.

Helical interpolations are not possible while the "LOOK-AHEAD (G51)" function is active.

0175 'Analog inputs: ANAI(1-8) = +/-5 Volts.’

DETECTION

CAUSE

SOLUTION

During execution.

An analog input has taken a value out of the ±5V range.

Analog inputs may only take values within the ±5V range.

0176 'Analog outputs: ANAO(1-8) = +/-10 Volts.’

DETECTION

CAUSE

SOLUTION

During execution.

An analog output has been assigned a value out of the ±10V range.

Analog outputs may only take values within the ±10V range.

0177 ‘A gantry axis cannot be part of the active plane.’


0178 ‘G96 only possible with analog spindle.’

DETECTION

CAUSE

SOLUTION

During execution.

The "G96" function has been programmed but either the spindle speed is not controlled or the spindle does not have an encoder.

To operate with the "G96" function, the spindle speed must be controlled

(SPDLTYPE(P0)=0) and the spindle must have an encoder (NPULSES(P13) other than zero).

0179 ‘Do not program more than 4 axes simultaneously.’


·T· Model

Ref.1507

·27·


·T· Model

Ref.1507

0180 ‘Program DNC1/2/E, HD or CARD A (optional).’

DETECTION

CAUSE

SOLUTION

While editing or executing.

While programming in high level language, in the "OPEN" and "EXEC" instructions, an attempt has been made to program a parameter other than DNC1/2E, HD or CARD

A, or the DNC parameter has been assigned a value other than 1, 2 or E.

Check the syntax of the block.

0181 ‘Program A (append) or D (delete).’

DETECTION

CAUSE

SOLUTION


In the "OPEN" instruction the A/D parameter is missing.

Check the syntax of the block. The programming format is:

(OPEN P.........,A/D,… )

Where:

A

D

Appends new blocks after the existing ones.

Deletes the existing program and it opens it as a new one.

0182 ‘Option not available.’

DETECTION

CAUSE


A "G" function has been defined which is not a software option.

0184 ‘T with subroutine: program only T and D.’


0185 ‘Tool offset does not exist’

DETECTION

CAUSE

SOLUTION


Within the block syntax, a tool offset has been called upon which is greater than the ones allowed by the manufacturer.

Program a new smaller tool offset.

0186 ‘The "C" axis does not exist.’

DETECTION

CAUSE


An attempt has been made to activate the "C" axis, but the machine does not have this feature.

0187 ‘G66, G68, G69 are not allowed when machining with the "C" axis.’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to execute a "G66", "G68" or "G69" canned cycle while the "C" axis is active.

Cancel the "C" axis to work with these canned cycles.

0188 ‘Function not possible from PLC.’

DETECTION

CAUSE

SOLUTION

During execution.

From the PLC channel and using the "CNCEX" instruction, an attempt has been made to execute a function that is incompatible with the PLC channel execution.

The installation manual (chapter 11.1.2) offers a list of the functions and instructions that may be executed through the PLC channel.

0189 ‘The live tool does not exist.’

DETECTION

CAUSE


An attempt has been made to start the live tool "M45 S...", but the machine does not have this feature.

0194 ‘Repositioning not allowed.’

DETECTION

CAUSE

SOLUTION

During execution.

The axes cannot be repositioned using the "REPOS" instruction because the subroutine has not been activated with one of the interruption inputs.

Before executing the "REPOS" instruction, one of the interruption inputs must be activated.

·28·


0195 ‘Axes X, or Z slaved or synchronized.’

DETECTION

CAUSE

SOLUTION

During execution.

While programming in high level language, an attempt has been made to execute a probing cycle using the "PROBE" instruction, but one of the X or Z axis is slaved or synchronized.

To execute the "PROBE"¨ instruction, the X-Z axes must not be slaved or synchronized. To unslave the axes, program "G78".

0196 ‘Axes X and Z must exist.’

DETECTION

CAUSE

SOLUTION


While programming in high level language, an attempt has been made to edit the

"PROBE" instruction, but one of the X or Z axis is missing.

To operate with the "PROBE" instruction, the X, Z axes must be defined.

0197 ‘G15 must be programmed before the "C" axis.’

DETECTION

CAUSE

SOLUTION


An attempt has been made to execute an operation on the "C" axis, but the axis is not active.

In order to operate with the "C" axis, it must be activated first using the "G15" function.

0199 ‘Presetting rotary axes: values between 0 and -359.9999.'

DETECTION

CAUSE

SOLUTION

While presetting coordinates.

An attempt has been made preset the coordinates of a rotary axis with a value out of the 0 to 359.9999 range.

The preset value of rotary axes must be within the 0 to 359.9999 range.

0200 'Program: G52 axis +/-5.5’

DETECTION

CAUSE

SOLUTION


When programming the "Movement against a hard stop (G52)", either the axis to be moved has not been programmed or several axes have been programmed.

When programming "G52", the axis to be moved must be indicated. Only one axis may be programmed at a time.

0201 ‘Program only one positioning axis in G01.’


0206 ‘Values 0 thru 6.’

DETECTION

CAUSE

SOLUTION



The parameter only admits values between 0 and 6.

0207 ‘Complete Table.’

DETECTION

CAUSE

SOLUTION


In the tables for "M" functions or tool offsets, an attempt has been made to define more data than those allowed by the manufacturer by means of machine parameters. When loading a table via DNC, the CNC does not delete the previous table, it replaces the existing values and it copies the new data in the free positions of the table.

The maximum number of data that can be defined is limited by the machine parameters:

Maximum number of "M" functions

Maximum number of

Maximum number of tool offset

Maximum number of magazine positions

NMISCFUN(P29).

NTOOL(P23).

NTOFFSET(P27).

NPOCKET(P25).

To load a new table via DNC, the previous table should be deleted.

·T· Model

Ref.1507

·29·


0208 ‘Program A from 0 to 255’

DETECTION

CAUSE

SOLUTION

During execution.

In the "LOOK-AHEAD (G51)" function, parameter "A" (% of acceleration to be applied) has been programmed with a value greater than 255.

Parameter "A" is optional, but when programmed, it must have a value between 0 and

255.

0209 ‘Program nesting not allowed.’

DETECTION

CAUSE

SOLUTION

During execution.

From a running program, an attempt has been made to execute another program with the "EXEC" instruction which in turn also has an "EXEC" instruction.

Another program cannot be called upon from a program being executed using the

"EXEC" instruction.

0210 ‘No compensation is permitted.’

DETECTION

CAUSE

SOLUTION


An attempt has been made to activate or cancel tool radius compensation (G41, G42,

G40) in a block containing a nonlinear movement.

Tool radius compensation must be activated/deactivated in linear movements (G00,

G01).

0213 ‘A second spindle is required for G28, G29, G77 or G78.’

DETECTION

CAUSE

SOLUTION


An attempt has been made to select the work spindle with "G28/G29" or synchronize spindles with "G77/G78", but the machine only has one work spindle.

If the machine only has one work spindle, the "G28, G29, G77 and G78" functions cannot be programmed.

0214 ‘Invalid G function when selecting a profile’

DETECTION

CAUSE

SOLUTION

While restoring a profile.

Within the group of blocks selected to restore the profile, there is a block containing a "G" code that does not belong in the profile definition.


G00

G36

G01

G37

G02

G38

G03

G39

G06

G90

G08

G91

G09

G93

0215 ‘Invalid G function after first point of profile’

DETECTION

CAUSE

SOLUTION


Within the selected blocks for restoring the profile, and after the starting point of a profile, there is a block containing a "G" function that does not belong in the profile definition.


G00

G36

G01

G37

G02

G38

G03

G39

G06

G90

G08

G91

G09

G93

0216 ‘Nonparametric assignment after first point of profile’

DETECTION

CAUSE

SOLUTION


Within the selected blocks for restoring the profile, and after the starting point of a profile, a nonparametric assignment has been programmed in high level language

(a local or global parameter).

The only high level instructions that can be edited are assignments to local parameters (P0 thru P25) and global parameters (P100 thru P299).

·T· Model

Ref.1507

·30·


0217 ‘Invalid programming after first point of profile’

DETECTION

CAUSE

SOLUTION


Within the selected blocks for restoring the profile, and after the starting point of a profile, there is a high level block that is not an assignment.

The only high level instructions that can be edited are assignments to local parameters (P0 thru P25) and global parameters (P100 thru P299).

0218 ‘The axis cannot be programmed after first point of profile’

DETECTION

CAUSE

SOLUTION


Within the selected blocks for restoring the profile, and after the starting point of a profile, a position has been defined on an axis that does not belong to the active plane.

A surface coordinate may have been defined after the starting point of the profile.

The surface coordinate of the profiles is only defined in the starting block of the first profile, the one corresponding to the starting point of the outside profile.

0219 ‘First point programmed wrong when selecting profile’

DETECTION

CAUSE

SOLUTION

While selecting a profile.

The starting point of the profile has been programmed wrong. One of the two coordinates defining its position is missing.

The starting point of a profile must be defined on the two axes forming the active plane.

0220 ‘Invalid axes’

DETECTION

CAUSE

SOLUTION


The defined axes are not valid for G46.

Check the following:

• g.m.p. ANGAXNA (P171) and g.m.p. ORTAXNA (P172) are other than 0.

• The defined axes exist and are linear.

0227 ‘Program Q between +/-359.9999.’

DETECTION

CAUSE

SOLUTION


In the "Electronic threading (G33)" function, the entry angle "Q" has been programmed with a value out of the ±359.9999 range.

Program an entry angle within the ±359.9999 range.

0228 ‘Do not program "Q" with parameter M19TYPE=0.’

DETECTION

CAUSE

SOLUTION


In the "Electronic threading (G33)" function, an entry angle “Q” has been programmed, but the type of spindle orientation available does not allow this operation.

In order to define an entry angle, spindle machine parameter M19TYPE(P43) must be set to "1".

·T· Model

Ref.1507

·31·


·T· Model

Ref.1507

0229 ‘Program maximum Z’

0230 ‘Program inside R’

0231 ‘Program outside R’

DETECTION

CAUSE

SOLUTION


While programming in high level language, in the "DGWZ" instruction, the indicated limit is missing or it has been defined with a non-numerical value.

Check the syntax of the block.

0234 ‘Wrong graphic limits’

DETECTION

CAUSE

SOLUTION

During execution.

One of the lower limits defined with the "DGWZ" instruction is greater than its corresponding upper limit.

Program the upper limit of the graphics display area greater than the lower ones.

0235 ‘Do not program the axis in tangential control’


0236 ‘Do not program the longitudinal axis or the axis of the active plane’


0237 ‘Program values between +/-359.9999.’

DETECTION

CAUSE

SOLUTION

During execution.

A G30 offset has been programmed greater than the maximum allowed. For example

G30 D380

The offset must be within ±359.9999.

0238 ‘Do not program G30 without synchronizing the spindles in speed’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to synchronize the spindles in "G30" offset without having them synchronized in speed.

First, synchronize the spindle in speed using G77S.

0239 ‘Do not synchronize the spindles while the "C" axis is active’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to synchronize the spindle, but the "C" axis is not active.

Activate the "C" axis first.

0240 ‘Do not activate the "C" axis while the spindles are synchronized’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to activate the "C" axis while the spindles were synchronized.

First, cancel the spindle synchronization (G78 S).

0241 ‘Don’t program G77 S, G78 S with no spindle encoder.’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to synchronize the spindles (G77 S or G78 S) and one of them does not have an encoder or Sercos feedback.

Both spindles must have an encoder or Sercos feedback.

0242 ‘Do not synchronize spindles with M19TYPE=0’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to synchronize the spindles (G77 S or G78 S) and one of them has parameter M19TYPE=0.

Both spindles must have parameter M19TYPE=1

0243 ‘Values 0 thru 15.’

0244 ‘Values between 0.00% - 100.00%.’

0245 ‘Values between -100.00% - 100.00%.’


·32·


0246 'The feedrate cannot be negative or zero.'

DETECTION

CAUSE

SOLUTION


If g.m.p. FEEDTYPE (P170) has a value other than ·0·, F0 cannot be programmed.

The possible solutions are:

• Set g.m.p. FEEDTYPE (P170) to ·0·.

In this case, the motion blocks are executed at the maximum feedrate allowed.

• Program F other than ·0·.

0247 ‘Values 0 thru 8.’


·T· Model

Ref.1507

·33·


·T· Model

Ref.1507

·34·

PROGRAMMING ERRORS. Fagor CNC 8055 para otras aplicaciones, CNC 8055 for lathes, CNC 8055 para tornos, CNC 8055 for other applications

PROGRAMMING ERRORS

Related manuals

Table of contents

PROGRAMMING ERRORS. Fagor CNC 8055 para otras aplicaciones, CNC 8055 for lathes, CNC 8055 para tornos, CNC 8055 for other applications

PROGRAMMING ERRORS

Related manuals

Fagor

CNC 8055

Fagor

CNC 8055

Fagor

CNC 8040M

Fagor

CNC 8040T

Fagor

CNC 8035T

Fagor

CNC 8037

Fagor

CNC 8037

Fagor

CNC 8055 for other applications

Fagor

CNC 8040T

Fagor

CNC 8035M

Fagor

CNC 8055

Fagor

CNC 8055

Table of contents