Specifications

I Alarms
Program Errors (P)
I - 60
P38 No spec: Add. Op block skip
Details
"/n" has been issued while the optional block skip addition is not in the specifications.
Remedy
- Check the specifications.
P39 No specifications
Details
- A non-specified G code was commanded.
- The selected operation mode is out of specifications.
Remedy
- Check the specifications.
P45 G-CODE COMB.
Details
The combination of G codes in a block is inappropriate.
A part of unmodal G codes and modal G codes cannot be commanded in a same block.
Remedy
Correct the combination of G codes.
Separate the incompatible G codes into different blocks.
P48 Restart pos return incomplete
Details
A travel command was issued before the execution of the block that had been restart-
searched.
Remedy
- Carry out program restart again.
Travel command cannot be executed before the execution of the block that has been restart-
searched.
P49 Invalid restart search
Details
- Restart search was attempted for the 3-dimensional circular interpolation.
- Restart search was attempted for the mixed control (cross axis control) command (G110).
- Restart search was attempted during the cylindrical interpolation, polar coordinate interpo-
lation, or tool tip center control.
- Restart search was attempted from a block (G68.2) during the inclined surface machining
mode or from the inclined surface machining mode cancel command block (G69).
- Restart search was attempted to the program after direct command mode.
Remedy
- Correct the program.
- Correct the restart search position.
P50 No spec: Inch/Metric change
Details
Inch/Metric changeover (G20/G21) command was issued while the function is out of specifi-
cations.
Remedy
- Check the specifications.
P60 Compensation length over
Details
The commanded movement distance is excessive (over 231).
Remedy
- Correct the command range for the axis address.
P61 No spec: Unidirectional posit.
Details
Unidirectional positioning (G60) was commanded while the function is out of specifications.
Remedy
- Check the specifications.
P62 No F command
Details
- No feed rate command has been issued.
- There is no F command in the cylindrical interpolation or polar coordinate interpolation im-
mediately after the G95 mode is commanded.
Remedy
- The default movement modal command at power ON is G01. This causes the machine to
move without a G01 command if a movement command is issued in the program, and an
alarm results. Use an F command to specify the feed rate.
- Specify F with a thread lead command.
P63 No spec: High-speed machining
Details
High-speed machining cancel (G5P0) was commanded while the high-speed machining is out
of specifications.
Remedy
- Check the specifications.
P65 No spec: High speed mode 3
Details
Remedy
- Check whether the specifications are provided for the high-speed mode III.
P70 Arc end point deviation large
Details
- There is an error in the arc start and end points as well as in the arc center.
- The difference of the involute curve through the start point and the end point is large.
- When arc was commanded, one of the two axes configuring the arc plane was a scaling valid
axis.
Remedy
- Correct the numerical values of the addresses that specify the start and end points, arc cen-
ter as well as the radius in the program.
- Correct the "+" and "-" directions of the address numerical values.
- Check for the scaling valid axis.