Number ContentsMessage
023 ILLEGAL RADIUS COMMAND
(T series)
In circular interpolation by radius designation, negative value was com-
manded for address R. Modify the program.
025 CANNOT COMMAND F0 IN G02/G03
(M series)
F0 (fast feed) was instructed by F1 –digit column feed in circular inter-
polation. Modify the program.
027 NO AXES COMMANDED IN
G43/G44 (M series)
No axis is specified in G43 and G44 blocks for the tool length offset type
C.
Offset is not canceled but another axis is offset for the tool length offset
type C. Modify the program.
028 ILLEGAL PLANE SELECT In the plane selection command, two or more axes in the same direction
are commanded.
Modify the program.
ILLEGAL OFFSET VALUE
(M series)
The offset values specified by H code is too large.
Modify the program.
029
ILLEGAL OFFSET VALUE
(T series)
The offset values specified by T code is too large.
Modify the program.
030
ILLEGAL OFFSET NUMBER
(M series)
The offset number specified by D/H code for tool length offset, cutter
compensation, or three–dimensional tool offset is too large. Alternative-
ly, the number of an additional workpiece coordinate system specified
with the P code is too large. Modify the program.
ILLEGAL OFFSET NUMBER
(T series)
The offset number in T function specified for tool offset is tool large.
Modify the program.
031 ILLEGAL P COMMAND IN G10 In setting an offset amount by G10, the offset number following address
P was excessive or it was not specified.
Modify the program.
032 ILLEGAL OFFSET VALUE IN G10 In setting an offset amount by G10 or in writing an offset amount by sys-
tem variables, the offset amount was excessive.
NO SOLUTION AT CRC
(M series)
A point of intersection cannot be determined for cutter compensation.
Modify the program.
033
NO SOLUTION AT CRC
(T series)
A point of intersection cannot be determined for tool nose radius com-
pensation. Modify the program.
NO CIRC ALLOWED IN ST–UP /EXT
BLK (M series)
The start up or cancel was going to be performed in the G02 or G03
mode in cutter compensation C. Modify the program.
034
NO CIRC ALLOWED IN ST–UP /EXT
BLK (T series)
The start up or cancel was going to be performed in the G02 or G03
mode in tool nose radius compensation. Modify the program.
CAN NOT COMMANDED G39
(M series)
G39 is commanded in cutter compensation B cancel mode or on the
plane other than offset plane. Modify the program.
035
CAN NOT COMMANDED G31
(T series)
Skip cutting (G31) was specified in tool nose radius compensation
mode. Modify the program.
036 CAN NOT COMMANDED G31
(M series)
Skip cutting (G31) was specified in cutter compensation mode.
Modify the program.
037
CAN NOT CHANGE PLANE IN CRC
(M seires)
G40 is commanded on the plane other than offset plane in cutter com-
pensation B. The plane selected by using G17, G18 or G19 is changed
in cutter compensation C mode. Modify the program.
CAN NOT CHANGE PLANE IN NRC
(T seires)
The offset plane is switched in tool nose radius compensation.
Modify the program.
INTERFERENCE IN CIRCULAR
BLOCK (M seires)
Overcutting will occur in cutter compensation C because the arc start
point or end point coincides with the arc center.
Modify the program.
038
INTERFERENCE IN CIRCULAR
BLOCK (T series)
Overcutting will occur in tool nose radius compensation because the arc
start point or end point coincides with the arc center.
Modify the program.
APPENDIX
GFKE-0222-EN
A. ALARM LIST
837