BLOCK PREPARATION AND EXECUTION ERRORS. Fagor CNC 8055 para otras aplicaciones, CNC 8055 for lathes, CNC 8055 para tornos, CNC 8055 for other applications

BLOCK PREPARATION AND EXECUTION

ERRORS

   Error solution

1000 ‘There is no enough path information.’

DETECTION

CAUSE

SOLUTION

During execution.

The program contains too many blocks without information about the path to apply tool radius compensation, rounding, chamfer or tangential entry or exit.

In order to carry out these operations, the CNC needs to know in advance the path to follow; therefore, there cannot be more than 48 blocks in a row without information about the path to follow.

1001 ‘Plane change in rounding/chamfering.’

DETECTION

CAUSE

SOLUTION

During execution.

A plane change has been programmed on the path following the definition of a

"controlled corner rounding G36" or "chamfer (G39)".

The plane cannot be changed while executing a rounding or a chamfer. The path following the definition of a rounding or chamfer must be in the same plane that the rounding or the chamfer.

1002 ‘Rounding radius too large.’

DETECTION

CAUSE

SOLUTION

During execution.

In the "Controlled corner rounding (G36)" function, the programmed rounding radius is larger than one of the paths where it has been defined.

The rounding radius must be smaller than the paths that define it.

1003 ‘Rounding in last block.’

DETECTION

CAUSE

During execution.

A "Controlled rounding radius (G36) or "Chamfer (G39) has been defined on the last path of the program or when the CNC does not find information about the path following the definition of the rounding or chamfer.

A rounding or chamfer must be defined between two paths.

SOLUTION

1004 ‘Tangential output programmed wrong’

DETECTION

CAUSE

SOLUTION

During execution.

The move following the definition of a tangential output (G38) is a circular path.

The move following the definition of a tangential output must be a straight path.

1005 ‘Chamfer programmed wrong.’

DETECTION

CAUSE

SOLUTION

During execution.

The move following the definition of a "Chamfer (G39)" is a circular path.

The move following the definition of a chamfer must be a straight path.

1006 ‘Chamfer value too large.’

DETECTION

CAUSE

SOLUTION

During execution.

In the "Chamfer (G39)" function, the programmed chamfer value is larger than one of the paths where it has been defined.

The chamfer size must be smaller than the paths that define it.

·T· Model

Ref.1507

·35·


·T· Model

1007 ‘G8 defined wrong.’

DETECTION

CAUSE

SOLUTION

During execution.

The possible causes are:

1. When a full circle has been programmed using the function "Arc tangent to previous path (G08)"

2. When the tangent path ends in a point of the previous path or its extension (in a straight line).

3. In an irregular pocket canned cycle with islands, when programming function

"G08" in the block following the definition of the beginning of the profile (G00).

The solution for each cause is:

1. Function "G08" does not allow programming full circles.

2. Tangent path must not end in a point of the previous path or in its extension (in a straight line).

3. The CNC does not have information about the previous path and cannot execute the tangent arc.

1008 ‘There is no information about the previous path’

DETECTION

CAUSE

SOLUTION

During execution.

An arc tangent to the previous path has been programmed using function "G08", but there is no information about the previous path.

To do a path tangent to the previous one, there must be information about the previous path and it must be within the 48 blocks preceding the tangent path.

1010 ‘Wrong plane for tangent path.’

DETECTION

CAUSE

SOLUTION

During execution.

A plane change has been programmed between the definition of the function "arc tangent to previous path (G08)" and the previous path.

A plane cannot be changed between two paths

1011 ‘No radius has been programmed for G15.’

DETECTION

CAUSE

SOLUTION

During execution.

The Z-C plane has been selected as a new work plane, but the radius of the cylinder to be machined has not been defined.

In order to work in the Z-C plane, first define the radius of the cylinder on which to machine using function "G15 R..."

1015 ‘The tool is not defined in the tool table’

DETECTION

CAUSE

SOLUTION

During execution.

A tool change has been defined, but the new tool is not defined in the tool table.

Define the new tool in the tool table.

1016 ‘The tool is not in the tool magazine’

DETECTION

CAUSE

SOLUTION

During execution.

A tool change has been defined, but the new tool is not defined in position of the tool magazine table.

Define the new tool in the tool magazine table.

1017 ‘There is no empty pocket in the tool magazine’

DETECTION

CAUSE

SOLUTION

During execution.

A tool change has been defined and there is no empty pocket for the tool that is currently in the spindle.

Perhaps, the new tool has been defined as special in the tool table and there are more than one pockets reserved to it in the magazine. In this case, that position is set for that tool and no other tool can occupy it. To avoid this error, an empty pocket (position) should be left in the tool magazine.

Ref.1507

·36·


1018 ‘A tool change has been programmed without M06’

DETECTION

CAUSE

SOLUTION

During execution.

An M06 has not been programmed after having looked for a tool and before searching again.

This error occurs when having a machining center (general machine parameter

TOFFM06(P28)=YES) that has a cyclic tool changer (general machine parameter

CYCATC(P61)=YES). In this case, the tool change must be done with an m06 after searching for a tool and before searching for the next one.

1019 ‘There is no tool of the same family for replacement.’

DETECTION

CAUSE

SOLUTION

During execution.

The real life of the requested tool exceeds its nominal life. The CNC has tried to replace it with another one of the same family, but it has not found any.

Replace the tool or define another one of the same family.

1020 ‘Do not change the active or pending tool using high level language.’

DETECTION

CAUSE

SOLUTION

During execution.

While programming in high level language and using the "TMZT" variable, an attempt has been made to assign the current or next tool to a magazine position.

Use the "T" function to change the active tool or the next one. The "TMZT" variable cannot be used to move the active tool or the next one to the magazine.

1021 ‘No tool offset has been programmed in the canned cycle.’

DETECTION

CAUSE

SOLUTION

During execution.

The "PROBE" canned cycle for tool calibration has been programmed, but no tool offset has been selected.

To execute the "Tool calibration canned cycle (PROBE), a tool offset must be selected where the probing cycle information will be stored.

1022 ‘Tool radius programmed incorrectly’

No explanation required.

1028 ‘Do not switch axes over or back while G15 is active’

DETECTION

CAUSE

During execution.

An attempt has been made to switch over to an axis or back (G28/G29) while function

"G15" was active.

1029 ‘Do not swap axes that are already swapped.’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to swap (G28) an axis that was already swapped with another one.

An axis already swapped with another one cannot be swapped with a third one. It must be switched back first (G29 axis)

1030 ‘The “M” for the automatic gear change does not fit’

DETECTION

CAUSE

SOLUTION

During execution.

Using automatic gear change, 7 "M" functions and the "S" function (involving a gear change) have been programmed. In this case, the CNC cannot include the "M" for automatic gear change in that block.

Program an "M" function or the "S" function in a separate block.

1031 ‘No subroutine is allowed with automatic gear change.’

DETECTION

CAUSE

SOLUTION

During execution.

On machines having an automatic gear change, when programming a spindle speed

"S" that involves a gear change and the "M" function of the automatic gear change has a subroutine associated with it.

When having an automatic gear change, the "M" functions corresponding to the gear change cannot have a subroutine associated with it.

·T· Model

Ref.1507

·37·


·T· Model

Ref.1507

1032 ‘Spindle gear not defined in M19.’

DETECTION

CAUSE

SOLUTION

During execution.

"M19" has been programmed, but none of the gear change functions "M41", "M42",

"M43" or "M44" are active.

On power-up, the CNC does not assume any gear; Therefore, if the gear change function is not generated automatically (spindle parameter AUTOGEAR(P6)=NO), the auxiliary gear change functions ("M41", "M42", "M43" or "M44") must be programmed.

1033 ‘Wrong gear change.’

DETECTION

CAUSE

SOLUTION

During execution.


1. When trying to make a gear change and the machine parameters for gears

(MAXGEAR1, MAXGEAR2, MAXGEAR3, or MAXGEAR4) are set wrong. All the gears have not been used and the unused ones have been set to a maximum speed of zero rpm.

2. When programming a gear change ("M41", "M42", "M43" or "M44") and the PLC has not responded with the relevant active gear signal (GEAR1, GEAR2, GEAR3 or GEAR4).


1. When not using all four gears, the lower ones must be used starting with

"MAXGEAR1" and the unused gears must be assigned the value of the highest one used.

2. Check the PLC program.

1034 ‘"S" has been programmed, but no gear is active.’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to start the spindle, but no gear is selected.

On power-up, the CNC does not assume any gear; Therefore, when programing a spindle speed and the gear change function is not generated automatically (spindle parameter AUTOGEAR(P6)=NO), the auxiliary gear change functions ("M41",

"M42", "M43" or "M44") must be programmed.

1035 ‘Programmed "S" too high’

DETECTION

CAUSE

SOLUTION

During execution.

An "S" has been programmed with a higher value than allowed by the last active gear.

Program a lower spindle speed "S" .

1036 ‘"S" has not been programmed in G95 or in threading’

DETECTION

CAUSE

SOLUTION

During execution.

"mm(inches)/revolution (G95)" or "electronic threading (G33)"has been programmed, but no spindle speed has been selected.

An "S" must be programmed to work in mm/rev (G95) or for an electronic threading

(G33).

1037 ‘No "S" has been programmed for G96.’

DETECTION

CAUSE

SOLUTION

During execution.

The "Constant Surface Speed (G96)" function has been programmed, but no cutting speed has been defined, a previous one does not exist or no spindle gear is selected.

In order to work at constant surface speed (G96), a cutting speed "S" must be already programmed and a spindle gear must be active.

1038 ‘The spindle has not been oriented’

DETECTION

CAUSE

During execution.

An attempt has been made to execute a threading cycle (G86 or G87) as a thread repair without already having oriented the active spindle (main or secondary).

1039 ‘No "F" has been programmed in G94.’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to execute a live tool cycle (G60, G61, G62 and G63) and there is feedrate selected in G94 (mm/min).

First, select the feedrate "F" in mm/min (G94).

·38·


1040 ‘Canned cycle does not exist’

DETECTION

CAUSE

SOLUTION

While executing in MDI mode

When trying to execute a canned cycle (G8x) after interrupting a program during the execution of a canned cycle (G8x) and then changing the plane.

Do not interrupt the program while executing a canned cycle.

1042 ‘Wrong parameter value in canned cycle’

DETECTION

CAUSE

SOLUTION

During execution.

When defining a canned cycle, a parameter has been defined with the wrong value.

Perhaps, a parameter that only takes positive values has been assigned a negative value (or zero).

Correct the definition of parameters:

• In the "Pattern repeat cycle":

• Parameter "C" only takes positive values greater than zero.

• Parameter "A" only admits values of 0 or 1.

• Parameter "J" only takes positive values greater than zero.

• In the canned cycle for "roughing along the Z axis" or "roughing along the X axis", parameter "C" only takes positive values greater than zero.

• In the " Axial drilling/tapping canned cycle":

• Parameter "I" only admits values other than zero.

• Parameter "B" only takes positive values or zero.

• In the canned cycle for "facing curved sections" or "turning curved sections", parameter "C" only takes positive values greater than zero.

• In the “Face threading canned cycle” or “Longitudinal threading canned cycle”, parameter “I”, “B”, “E” or “C” has been defined with a zero value.

• In the canned cycle for "grooving along the Z axis" or "grooving along the X axis", parameter "C" only takes positive values greater than zero.

• In the canned cycle for "Face drilling/tapping" or "Longitudinal drilling/tapping":

• Parameter "I" only admits values other than zero.

• Parameter "B" only takes positive values or zero.

• Parameter "J" only takes positive values greater than zero.

• In the canned cycle for "slot milling on the face" or "slot milling on the side", the slot dimension cannot be zero and parameters "I" and "J" only take positive values greater than zero.

1043 ‘Wrong tool for programmed profile.’

DETECTION

CAUSE

SOLUTION

During execution.

The selected tool cannot machine anywhere on the profile.

Choose a more appropriate tool to machine the profile.

1044 ‘A profile has been programmed that intersects itself.’

DETECTION

CAUSE

SOLUTION

During execution.

In the set of profiles, there is one that intersects itself.

Check the definition of the profiles. A profile cannot intersect itself.

1045 ‘Wrong cutter geometry angle.’

DETECTION

CAUSE

SOLUTION

During execution.

The cutter’s geometry angles have been assigned a wrong value.

Correct the tool geometry data.

1046 ‘Wrong tool position before the canned cycle’

DETECTION

CAUSE

SOLUTION

During execution.

The canned cycle calling point is defined wrong.

The canned cycle calling point must be off the part and at a distance greater than the one defined as finishing stock on both axes. (Cycles that do not have a finishing stock will use the safety distance).

1047 ‘Wrong location code in canned cycle’

DETECTION

CAUSE

SOLUTION

During execution.

The location code (shape) of the tool is not the right one.

Choose a tool with the right location code (shape).

·T· Model

Ref.1507

·39·


·T· Model

Ref.1507

1048 ‘Wrong cutter width’

DETECTION

CAUSE

SOLUTION

During execution.

A grooving operation has been defined with a cutter of zero width.

Check the definition of the cutter dimensions (NOSEW). The cutter width must be other than zero.

1049 ‘Incompatible tool position and location code in profile cycle.

DETECTION

CAUSE

SOLUTION

During execution.

The canned cycle calling point is defined wrong or the tool location code (shape) is the right one to execute the machining operation.

The canned cycle calling point must be off the part and at a distance greater than the one defined as finishing stock on both axes. Besides, the tool’s location code must allow executing the profile without running into the part.

1050 ‘Wrong value to be assigned to a variable’

DETECTION

CAUSE

SOLUTION

During execution.

Using parameters, the value assigned to a variable is too high.

Check the program history to make sure that this parameter does not have that value when it reaches the block where this assignment is made.

1051 ‘Wrong access to PLC variable.’

DETECTION

CAUSE

During execution.

From the CNC, an attempt has been made to read a PLC variable that is not defined in the PLC program.

1052 ‘Access to a variable with wrong index’

DETECTION

CAUSE

SOLUTION

During editing.

While programming in high level language, an operation has been carried out either with a local parameter greater than 25 or with a global parameter greater 299.

The parameters used by the CNC are:

Local:

Global:

0-25.

100-299.

Other parameters out of these ranges cannot be used in operations.

1053 ‘Local parameters not accessible’

DETECTION

CAUSE

SOLUTION

While executing in the user channel.

An attempt has been made to execute a block with an operation that uses local parameters.

The program that is executed in the user channel does not allow operations with local parameters (P0 to P25).

1054 ‘Limit of local parameters exceeded’

DETECTION

CAUSE

SOLUTION

During execution.

While programming in high level language, more than 6 nesting levels have been used with the "PCALL" instruction. More than 6 calls have been made in the same loop using the "PCALL" instruction.

Only up to 6 nesting levels are allowed for local parameters within the 15 nesting levels of the subroutines. Calling with a "PCALL" instruction generates a new nesting level for local parameters (and a new one for subroutines).

1055 ‘Nesting exceeded’

DETECTION

CAUSE

SOLUTION

During execution.

While programming in high level language, more than 15 nesting levels have been used with the "CALL", "PCALL" or "MCALL" instruction. More than 15 calls have been made in the same loop using the "CALL", "PCALL" or "MCALL" instruction.

Only 15 nesting levels allowed. Calling with the "CALL", "PCALL" and "MCALL" instructions generates a new nesting level.

·40·


1056 ‘RET not associated with subroutine.’

DETECTION

CAUSE

SOLUTION

During execution.

The "RET" instruction has been edited, but the "SUB" instruction has not been edited before.

To using the "RET" instruction (subroutine), the subroutine must begin with the "SUB

(subroutine number)".

1057 ‘Undefined subroutine’

DETECTION

CAUSE

SOLUTION

During execution.

A (CALL, PCALL...) has been made to a subroutine that was not defined in the CNC memory.

Check that the name of the subroutine is correct and that the subroutine exists in the

CNC memory (not necessarily in the same program where the call is).

1058 ‘Undefined probing canned cycle’

DETECTION

CAUSE

SOLUTION

During execution.

Using the "PROBE" instruction, a probing cycle has been defined which is not available.

The available "PROBE" canned cycles are 1 to 4.

1059 ‘Jump to an undefined label’

DETECTION

CAUSE

SOLUTION

During execution.

While programming in high level language, the "GOTO N..." instruction has been programmed, but the programmed block number (N) does not exist.

When programming the "GOTO N..." instruction, the block it refers to must be defined in the same program.

1060 ‘Undefined label’

DETECTION

CAUSE

SOLUTION

During execution.


1. While programming in high level language, the instrucción "RPT N..., N..." instruction has been programmed, but a programmed block number (N) does not exist.

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)" a profile definition has been programmed, but one of the two data defining the beginning

"S" or end "E" of the profiles is missing.


1. When programming the "RPT N..., N..." instruction, the blocks it refers to must be defined in the same program.

2. Check the program. Place the label for parameter "S" at the beginning of the profile definition and the label for parameter "E" at the end of the profile definition.

1061 ‘Label cannot be searched’

DETECTION

CAUSE

SOLUTION

While executing in MDI mode

While programming in high level language, either an "RPT N..., N..." or "GOTO N..." instruction has been defined.

While operating in MDI mode, "RPT" or "GOTO" type instructions cannot be programmed.

1062 ‘Subroutine in an unavailable program.’

DETECTION

CAUSE

SOLUTION

During execution.

A call has been made to a subroutine that it is located in a program being used by the DNC.

Wait for the DNC to finish using the program. If the subroutine is to be used often, it should be stored in a separate program.

1063 ‘The program cannot be opened.’

DETECTION

CAUSE

SOLUTION

During execution.

While executing a program in infinite mode, an attempt has been made to execute another infinite program from the current one using the "EXEC" instruction.

Only one infinite program may be executed at a time.

·T· Model

Ref.1507

·41·


·T· Model

1064 ‘The program cannot be executed’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to execute a program from another with the "EXEC" instruction, but the program does not exist or is protected against execution.

The program to be executed with the "EXEC" instruction must exist in the CNC memory and must be executable.

1065 ‘Beginning of compensation without straight path’

DETECTION

CAUSE

SOLUTION

During execution.

The first movement in work plane after activating tool radius compensation

(G41/G42) is not a linear movement.

The first movement after activating radius compensation (G41/G42) must be linear.

1066 ‘End of compensation without straight path’

DETECTION

CAUSE

SOLUTION

During execution.

The first movement in work plane after deactivating tool radius compensation (G40) is not a linear movement.

The first movement after deactivating radius compensation (G40) must be linear.

1067 ‘Compensation radius too large.’

DETECTION

CAUSE

SOLUTION

During execution.

While working with tool radius compensation (G41/G42), an inside radius has been programmed with a smaller radius than that of the tool.

use a tool with a smaller radius. When working with tool radius compensation, the arc radius must larger than that of the tool. Otherwise, the tool cannot machine the programmed path.

1068 ‘Step on linear path’

DETECTION

CAUSE

SOLUTION

During execution.

When operating with tool compensation (G41/G42), the profile has a straight section that cannot be machined because the tool diameter is too large.

use a tool with a smaller radius.

1069 ‘Circular path defined incorrectly’


1070 ‘Step on circular path’

DETECTION

CAUSE

SOLUTION

During execution.

When operating with tool compensation (G41/G42), the profile has a curved section that cannot be machined because the tool diameter is too large.

use a tool with a smaller radius.

1071 ‘Plane change in tool radius compensation.’

DETECTION

CAUSE

SOLUTION

During execution.

When operating with tool compensation (G41/G42), another work plane has been selected.

To change the work plane, tool radius compensation must be off (G40).

1072 ‘Tool radius compensation not possible with positioning-only rotary axis.

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to move a positioning-only axis with tool radius compensation (G41/G42).

Tool radius compensation not allowed for positioning-only rotary axes. Use "G40" to cancel tool radius compensation.

Ref.1507

·42·


1073 Motion block with zero speed.

DETECTION

CAUSE

SOLUTION

During execution.

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·.

1075 ‘G51 is incompatible helical path.’

DETECTION

CAUSE

SOLUTION

During execution.

A helical path has been executed while function G51 was active.

Cancel G51 before executing the helical path.

1076 ‘Coordinate angle programmed wrong.’

DETECTION

CAUSE

SOLUTION

During execution.

When programming in angle-coordinate format, an axis movement has been programmed with an angle perpendicular to that axis. (For example, the main plane is formed by the XZ axes and the X axis movement is programmed at a 90º angle).

Check and correct the definition of the movement in the program. If using parameters, check that the parameters have the correct values when arriving to the definition of the movement.

1077 ‘Either the arc radius is too small or a full circle has been programmed’

DETECTION

CAUSE

SOLUTION

During execution.


1. When programming a full circle using the "G02/G03 X Z R" format.

2. When programming using the "G02/G03 X Z R" format, the distance to the arc’s end point is greater than the diameter of the programmed circle.


1. This format cannot be used to make full circles. Program the coordinates of the end point different from those of the starting point.

2. The diameter of the circle must be larger than the distance to the arc’s end point.

1078 ‘Negative radius in polar coordinates’

DETECTION

CAUSE

SOLUTION

During execution.

Working with incremental polar coordinates, a block is executed where the end position has a negative radius.

Incremental polar coordinate programming allows negative radius, but the (absolute) end point of the radius must be positive,

G74 ‘There is no subroutine associated with G74’

DETECTION

CAUSE

SOLUTION

While executing a home search.


1. When trying to search home on all the axes manually, but there is no associated subroutine indicating the home searching sequence (order).

2. "G74" has been programmed, but there is no associated subroutine indicating the home searching sequence (order).


1. An associated subroutine is required to execute the "G74" function.

2. If "G74" is to be executed from a program, the home searching order must be defined.

1080 ‘Plane change in tool inspection’

DETECTION

CAUSE

SOLUTION

While executing the "tool inspection" option.

the work plane has been chanted and the original one has not been restored before resuming the execution.

The plane that was active before inspecting the tool must be restored before resuming the execution.

·T· Model

Ref.1507

·43·


·T· Model

Ref.1507

1081 ‘Block not allowed in tool inspection.’

DETECTION

CAUSE

SOLUTION

While executing the "tool inspection" option.

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

This instruction cannot be executed in the "tool inspection" option.

1082 ‘The probe signal has not been received.’

DETECTION

CAUSE

SOLUTION

During execution.


1. When programming a "PROBE" canned cycle, the probe has moved the maximum safety distance of the cycle without the CNC receiving the probe signal.

2. When programming the "G75" function, it has reached the end point and the CNC has not received the signal from the probe. (Only when general machine parameter PROBERR(P119)=YES).


1. Check that the probe is connected properly.

The maximum probing distance (in PROBE cycles) depends on the safety distance "B". To increase this distance, increase the safety distance.

2. If PROBERR(P119)=NO, this error will not be issued when the end point is reached without having received the probe signal (only with "G75").

1083 ‘Range exceeded’

DETECTION

CAUSE

SOLUTION

During execution.

The distance for the axes to travel is very long and the programmed feedrate is too low.

Program a higher speed for that movement.

1084 ‘Arc programmed wrong’

DETECTION

CAUSE

SOLUTION

During execution.


1. When the arc programmed using "G02/G03 X Y I J" cannot go through the defined end point.

2. When programming an arc using "G09 X Y I J" the three points are in line or two of them are the same.

3. When trying to do a rounding tangential entry on a path that is not in the active plane.

4. When programming a tangential exit and the next path is tangent (being on its straight extension) to the path preceding the tangential exit.

If the error comes up in the block calling upon the "Pattern repeat canned cycle

(G66)", "Roughing canned cycle along X (G68)" or "Roughing canned cycle along

Z (G69)" is because in the set of blocks that define the profiles, one of the cases mentioned earlier occurs.


1. Correct the syntax of the block. The coordinates of the end point or of the radius are defined wrong.

2. The three points used to define an arc must be different and cannot be in line.

3. 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.

4. The path after a tangential exit may be tangent, but it cannot be on the extension

(in a straight line) of the previous path.

1085 ‘Helical path programmed wrong’

DETECTION

CAUSE

SOLUTION

During execution.

When programming an arc using "G02/G03 X Y I J Z K", the programmed arc is impossible. The desired height cannot be reached with the programmed helical pitch.

Correct the syntax of the block. The height of the interpolation and the coordinates of the end point in the plane must be related taking the helical pitch into account.

1086 ‘The spindle cannot be homed.’

CAUSE Spindle machine parameter REFEED1(P34) = 0.

·44·


1087 ‘Circle with zero radius’

DETECTION

CAUSE

SOLUTION

During execution.


1. When programming an arc using "G02/G03 X Z I K", an arc has been programmed with a zero radius.

2. When operating with tool radius compensation, an inside arc has been programmed with the same radius as that of the tool.


1. Arcs with zero radius are not allowed. Program a radius other than zero.

2. When working with tool radius compensation, the arc radius must larger than that of the tool. Otherwise, the tool cannot machine the programmed path (because to do so, the tool would have to make an arc of zero radius).

1088 ‘Range exceeded in zero offset.’

DETECTION

CAUSE

SOLUTION

During execution.

A zero offset has been programmed and the value of the end position is too high.

Check that the values assigned to the zero offsets (G54-G59) are correct. If the zero offsets have been assigned values from the program using parameters, check that the parameter values are correct. If an absolute (G54-G57) and an incremental (G58-

G59) zero offset has been programmed, check that the sum of both does not exceed the machine limits.

1089 ‘Range exceeded in zone limit.’

DETECTION

CAUSE

SOLUTION

During execution.

When programming zone limits "G20" or "G21" with parameters, the parameter value is greater than the maximum allowed for that function

Check the program history to make sure that this parameter does not have that value when it reaches the block where the limits have been defined.

1090 ‘Point inside the forbidden zone 1.’

DETECTION

EFFECT

CAUSE

SOLUTION

During execution.

It stops the movement of the axes and the spindle, eliminating all the enable signals and canceling all the analog outputs of the CNC. When detected from the position loop, it opens the position loop and sets the LOPEN mark to ·1·.

If it is in execution, it interrupts the execution of the part program of the CNC of its channel.

An attempt has been made to move an axis to a point located inside the work area

1 that is defined as "no entry" zone.

In the program history, work zone 1 (defined with G20/G21) has been set as "no entry" zone " (G22 K1 S1). To cancel this work zone, program "G22 K1 S0"


DETECTION

EFFECT

CAUSE

SOLUTION

During execution.






1092 ‘Insufficient acceleration for the speed programmed in threading.’

DETECTION

CAUSE

SOLUTION

During execution.

A thread has been programmed and there isn’t enough room to accelerate and decelerate.

Program a lower speed.

1093 ‘Only one Hirth axis can be moved at a time’


·T· Model

Ref.1507

·45·


·T· Model

Ref.1507

1094 ‘Probe calibrated wrong’


1095 ‘Probing axes out of alignment .’

DETECTION

CAUSE

SOLUTION

During the probe calibration process.

An axis has moved to touch a cube and one of the axis that did not move registers a deflection greater than allowed by machine parameter MINDEFLE(P66). This is because the probing axes are not parallel enough to the axes of the machine.

Correct the parallelism between the probing axes and those of the machine.


DETECTION

EFFECT

CAUSE

SOLUTION

During execution.







DETECTION

EFFECT

CAUSE

SOLUTION

During execution.






1098 ‘Work zone limits defined wrong’

DETECTION

CAUSE

SOLUTION

During execution.

The upper limits (G21) of the defined work zone are the same or smaller than the lower ones (G20) of the same work zone.

Program the upper limits (G21) of the work zone greater than the lower ones (G20).

1099 ‘Do not program a slaved axis.’

DETECTION

CAUSE

SOLUTION

During execution.

When operating in polar coordinates, a movement has been programmed that involves an axis that is slaved to another one.

The movements in polar coordinates are made with the main axes of the work plane; therefore, the axes that define the plane cannot be slaved to each other or to a third one. To unslave the axes, program "G78".

1100 ‘Travel limits of spindle 1 exceeded’

DETECTION

EFFECT

CAUSE

During execution.



An attempt has been made to exceed the physical turning limits of the spindle. As a result, the PLC activates the spindle mark "LIMIT+S" or "LIMIT-S". ("LIMIT+S2" or

"LIMIT-S2" when working with the second spindle).

·46·


1101 ‘Spindle 1 locked’

DETECTION

EFFECT

CAUSE

During execution.



The CNC tries to output the command to the drive when the spindle input SERVOSON is still low. The error may be due to an error in the PLC program where this signal is not properly treated or that the value of the spindle parameter DWELL(P17) is not high enough.

1102 ‘Following error of spindle 1 out of limit’

DETECTION

EFFECT

CAUSE

During execution.



Besides this, it activates the external emergency output.

When the spindle is working in closed loop (M19), its following error is greater than the values indicated by spindle parameter MAXFLWE1(P21) and MAXFLWE2(P22)

The possible causes for this error are:

Servo drive error

Faulty drive.

Enable signals missing.

Power supply missing.

Drive adjusted incorrectly.

The velocity command signal is not received.

Motor error

Faulty motor.

Power cables.

Feedback failure

Defective feedback.

Defective feedback cable.

Mechanical failure

Mechanical stiffness.

Spindle mechanically locked.

CNC error

Defective CNC.

Parameters adjusted incorrectly.

1103 ‘Do not synchronize spindles without homing them first’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to synchronize the spindle without homing them first.

Before activating the synchronization, both spindles must be homed using the "M19" function.

1104 ‘ Do not program G28 or G29 while spindle synchronization is active’

DETECTION

CAUSE

SOLUTION

During execution.

An attempt has been made to swap spindles (G28/G29) while the spindles were synchronized.

First, cancel spindle synchronization (G78S).

1105 ‘Do not change gears while the spindles are synchronized’

DETECTION

CAUSE

SOLUTION

During execution.

While the spindles are synchronized, a gear changing "M" function (M41 to M44) has been executed or the programmed "S" involves a gear change (with automatic gear changer).

First, cancel spindle synchronization (G78S).

·T· Model

Ref.1507

·47·


·T· Model

1106 ‘Travel limits of spindle 2 exceeded’

Same as error 1100, but for the second spindle.

1107 ‘Spindle 2 locked’


1108 ‘Following error of spindle 2 out of limit’


1109 ‘Axis software limit overrun’


1110 ‘Range of the X axis exceeded’

1111 ‘Range of the Y axis exceeded’

1112 ‘Range of the Z axis exceeded’

1113 ‘Range of the U axis exceeded’

1114 ‘Range of the V axis exceeded’

1115 ‘Range of the W axis exceeded’

1116 ‘Range of the A axis exceeded’

1117 ‘Range of the B axis exceeded’

1118 ‘Range of the C axis exceeded’

DETECTION

CAUSE

SOLUTION

During execution.

A movement has been defined with parameters and the parameter value is greater than the maximum travel distance of the axis.

Check the program history to make sure that this parameter does not have that value when it reaches the block where this movement is programmed.

1119 ‘The X axis cannot be synchronized’

1120 ‘The Y axis cannot be synchronized’

1121 ‘The Z axis cannot be synchronized’

1122 ‘The U axis cannot be synchronized’

1123 ‘The V axis cannot be synchronized’

1124 ‘The W axis cannot be synchronized’

1125 ‘The A axis cannot be synchronized’

1126 ‘The B axis cannot be synchronized’

1127 ‘The C axis cannot be synchronized’

DETECTION

CAUSE

During execution.


1. When trying to synchronize two axes from the PLC and one axis is already slaved to another one using the "G77" function.

2. When programming or trying to move an axis that is slaved to another one.

1128 ‘Maximum feedrate of the X axis exceeded’

1129 ‘Maximum feedrate of the Y axis exceeded’

1130 ‘Maximum feedrate of the Z axis exceeded’

1131 ‘Maximum feedrate of the U axis exceeded’

1132 ‘Maximum feedrate of the V axis exceeded’

1133 ‘Maximum feedrate of the W axis exceeded’

1134 ‘Maximum feedrate of the A axis exceeded’

1135 ‘Maximum feedrate of the B axis exceeded’

1136 ‘Maximum feedrate of the C axis exceeded’

DETECTION

CAUSE

During execution.

The resulting feedrate of one of the axes after applying an individual scaling factor exceeds the maximum value indicated by axis machine parameter MAXFEED (P42).

Ref.1507

·48·


1137 ‘Wrong feedrate parameter of the X axis’

1138 ‘Wrong feedrate parameter of the Y axis’

1139 ‘Wrong feedrate parameter of the Z axis’

1140 ‘Wrong feedrate parameter of the U axis’

1141 ‘Wrong feedrate parameter of the V axis’

1142 ‘Wrong feedrate parameter of the W axis’

1143 ‘Wrong feedrate parameter of the A axis’

1144 ‘Wrong feedrate parameter of the B axis’

1145 ‘Wrong feedrate parameter of the C axis’

DETECTION

CAUSE

During execution.

"G00" programmed with parameter G00FEED(P38)=0 or "G1 F00" with axis parameter MAXFEED(P42) = 0.

1146 'X axis locked up'

1147 'Y axis locked up'

1148 'Z axis locked up'

1149 'U axis locked up'

1150 'V axis locked up'

1151 'W axis locked up'

1152 'A axis locked up'

1153 'B axis locked up'

1154 'C axis locked up'

DETECTION

EFFECT

CAUSE

During execution.



The CNC tries to output the command to the drive when the spindle input

SERVO(n)ON is still low. The error may be due to an error in the PLC program where this signal is not properly treated or that the value of the axis parameter DWELL(P17) is not high enough.

1155 ‘Maximum X axis software exceeded’

1156 ‘Maximum Y axis software exceeded’

1157 ‘Maximum Z axis software exceeded’

1158 ‘Maximum U axis software exceeded’

1159 ‘Maximum V axis software exceeded’

1160 ‘Maximum W axis software exceeded’

1161 ‘Maximum A axis software exceeded’

1162 ‘Maximum B axis software exceeded’

1163 ‘Maximum C axis software exceeded’

DETECTION

EFFECT

CAUSE

During execution.



A coordinate has been programmed that is out of the limits defined by axis parameters

LIMIT+(P5) and LIMIT-(P6).

·T· Model

Ref.1507

·49·

·T· Model

Ref.1507

·50·


1164 ‘Work zone 1 of the X axis exceeded’

1165 ‘Work zone 1 of the Y axis exceeded’

1166 ‘Work zone 1 of the Z axis exceeded’

1167 ‘Work zone 1 of the U axis exceeded’

1168 ‘Work zone 1 of the V axis exceeded’

1169 ‘Work zone 1 of the W axis exceeded’

1170 ‘Work zone 1 of the A axis exceeded’

1171 ‘Work zone 1 of the B axis exceeded’

1172 ‘Work zone 1 of the C axis exceeded’

DETECTION

EFFECT

CAUSE

SOLUTION

During execution.



An attempt has been made to move an axis to a point located out of the work area

1 that is defined as "no exit" zone.

In the program history, work zone 1 (defined with G20/G21) has been set as "no exit" zone " (G22 K1 S2). To cancel this work zone, program "G22 K1 S0"










DETECTION

EFFECT

CAUSE

SOLUTION

During execution.







1182 'X axis following error beyond limits'

1183 'Y axis following error beyond limits'

1184 'Z axis following error beyond limits'

1185 'U axis following error beyond limits'

1186 'V axis following error beyond limits'

1187 'W axis following error beyond limits'

1188 'A axis following error beyond limits'

1189 'B axis following error beyond limits'

1190 'C axis following error beyond limits'

DETECTION

EFFECT

CAUSE

During execution.




The following error of the axis is greater than the values indicated by axis parameter

MAXFLWE1(P21) or maxflwe2(P22). The possible causes for this error are:

Servo drive error

Faulty drive.

Enable signals missing.

Power supply missing.

Drive adjusted incorrectly.

The velocity command signal is not received.

Motor error

Faulty motor.

Power cables.

Feedback failure

Defective feedback.

Defective feedback cable.

Mechanical failure

Mechanical stiffness.

Spindle mechanically locked.

CNC error

Defective CNC.

Parameters adjusted incorrectly.

1191 ‘Difference of following errors of the slaved X axis * tool large’

1192 ‘Difference of following errors of the slaved Y axis * tool large’

1193 ‘Difference of following errors of the slaved Z axis * tool large’

1194 ‘Difference of following errors of the slaved U axis * tool large’

1195 ‘Difference of following errors of the slaved V axis * tool large’

1196 ‘Difference of following errors of the slaved W axis * tool large’

1197 ‘Difference of following errors of the slaved A axis * tool large’

1198 ‘Difference of following errors of the slaved B axis * tool large’

1199 ‘Difference of following errors of the slaved C axis * tool large’

EFFECT

CAUSE




The "n" axis is electronically coupled to another one or is a slaved Gantry axis and the difference between the following errors of the "n" axis and the one it is coupled to is greater than the value set by the machine parameter for the "n" axis

MAXCOUPE(P45).

·T· Model

Ref.1507

·51·


·T· Model

1200 ‘X axis travel limits exceeded’

1201 ‘Y axis travel limits exceeded’

1202 ‘Z axis travel limits exceeded’

1203 ‘U axis travel limits exceeded’

1204 ‘V axis travel limits exceeded’

1205 ‘W axis travel limits exceeded’

1206 ‘A axis travel limits exceeded’

1207 ‘B axis travel limits exceeded’

1208 ‘C axis travel limits exceeded’

DETECTION

EFFECT

CAUSE

During execution.



An attempt has been made to exceed the physical travel limits. As a result, the PLC activates the axis mark "LIMIT+1" or "LIMIT-1".

1209 ‘X axis servo error’

1210 ‘Y axis servo error’

1211 ‘Z axis servo error’

1212 ‘U axis servo error’

1213 ‘V axis servo error’

1214 ‘W axis servo error’

1215 ‘A axis servo error’

1216 ‘B axis servo error’

1217 ‘C axis servo error’

EFFECT

CAUSE




The real feedrate of the axis, after the time indicated by axis parameter

FBALTIME(P12), is below 50% or over 200% of the one programmed.










DETECTION

EFFECT

CAUSE

SOLUTION

During execution.






Ref.1507

·52·











DETECTION

EFFECT

CAUSE

SOLUTION

During execution.






1237 ‘Do not change the entry angle inside a thread’

DETECTION

CAUSE

SOLUTION

During execution.

A thread joint has been defined and an entry angle "Q" has been programmed between two threads.

When joining threads, only the first one may have an entry angle "Q".

1238 ‘Range of write-protected parameters. P297, P298’

DETECTION

CAUSE

During execution.

Parameters P297 and P298 are write-protected by means of machine parameters

ROPARMIN(P51) and ROPARMAX(P52).


DETECTION

EFFECT

CAUSE

SOLUTION

During execution.






·T· Model

Ref.1507

·53·


·T· Model

Ref.1507










DETECTION

EFFECT

CAUSE

SOLUTION

During execution.






1249 ‘Variable pitch thread programmed wrong’

DETECTION

CAUSE

During execution.

We are trying to make a variable-pitch thread with the following conditions:

• The "K" increment is positive and equal to or greater than 2L.

• The "K" increment is positive and with one of the calculated pitches, it exceeds the maximum feedrate (parameter MAXFEED) of one of the threading axis.

• The "K" increment is negative and one of the calculated pitches 0 or negative.

1250 ‘The K value is too large in G34’

DETECTION

EFFECT

CAUSE

During execution.



The ratio between the initial and final pitches of the variable-pitch thread (G34) to be executed is greater than 32767.

1251 ‘Two variable-pitch threads cannot be joined in round corner’

DETECTION

EFFECT

CAUSE

During motionless simulation, except when graphics are active.



To variable-pitch threads cannot be joined in round corner unless the second one is of the type: G34 ... L0 K0.

1252 ‘G5 G34 without a pitch is only allowed after a variable-pitch thread’

DETECTION

EFFECT

CAUSE

During motionless simulation, except when graphics are active.



G34...L0 K0 (blending a variable pitch thread with another one with a fixed pitch) can only be programmed after a G34 with a K value other than ·0· and round corner (G05).

·54·


1253 ‘Retrace function unavailable’

EFFECT




1254 ‘Parameter restricted to OEM programs’

DETECTION

EFFECT

CAUSE

During execution.



An attempt has been made to use an OEM parameter P2000-P2255 in a program that has no OEM permission.

Use a non-OEM parameter.

SOLUTION

1255 ‘Subroutine restricted to an OEM program’

DETECTION

EFFECT

CAUSE

During execution.



An attempt has been made to use an OEM subroutine SUB10000-SUB20000 in a program that has no OEM permission.

Use a general subroutine P0000-P9999.

SOLUTION

1256 ‘M transfer interrupted’

DETECTION

EFFECT

CAUSE

While executing a gear change, when pressing STOP and entering in tool inspection or in MDI.



The operator has interrupted a gear change and has accessed tool inspection or MDI.

·T· Model

Ref.1507

·55·


·T· Model

Ref.1507

·56·

BLOCK PREPARATION AND EXECUTION ERRORS. Fagor CNC 8055 para otras aplicaciones, CNC 8055 for lathes, CNC 8055 para tornos, CNC 8055 for other applications

BLOCK PREPARATION AND EXECUTION

ERRORS

Related manuals

Table of contents

BLOCK PREPARATION AND EXECUTION ERRORS. Fagor CNC 8055 para otras aplicaciones, CNC 8055 for lathes, CNC 8055 para tornos, CNC 8055 for other applications

BLOCK PREPARATION AND EXECUTION

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