GREEN
The three common control status indicator lights can be grouped by their actual purpose:
▪Zero return position
▪Cycle end
▪Errors / Alarms / Faults
Additional lights may indicate status that is unique to a particular CNC machine tool.
Zero Return
When one or more machine axis reaches the machine zero reference position (home position), a status indicator light on the Operation Panel will turn on, as a confirmation. Each axis has its own light, so it is easy to check if all axes have reached the machine zero.
These lights are usually green, but can be amber as well - they are assigned to each available axis the machine tool has. On the most common 3-axis CNC vertical machines, there will be three lights identified by the machine axis letters X-Y-Z. If the fourth axis is also present on the machine, the corresponding light can be identified by the digit 4 (as for ‘fourth axis’), as ‘4th’, or it can be the exact name of the fourth axis, such as A or B. Typically it is the A-axis for CNC vertical machining centers and the B-axis for CNC horizontal machining centers.
Most CNC machines have to be zeroed (homed) in ALL axes before running a part program
Cycle End
The end of a cycle can be only temporary (using M00 and M01) or permanent (M02 or M30). Fanuc and similar control systems have at least three confirmation lights that relate to Cycle End modes:
| M00 | Indicator light turns ON, if Program Stop M00 has been detected in the CNC program |
| M01 | Indicator light turns ON, if Optional ProgramStop M01 has been detected in the CNCprogram |
| M02 | Indicator light turn ON, if Program End M02 has been detected in the CNC program (obsolete) |
| M30 | Indicator light turns ON, if Program End M30 has been detected in the CNC program |
Cycle End indicator lights will turn ON only if M00-M01-M02-M30 is detected in the part program
Note that the above illustration does not contain miscellaneous function M02. This function is still supported for backward compatibility but is not used anymore.
As all four indicator lights are directly related to the contents of a part program, it is very important to understand how they affect CNC machine operation.
M00 - Program Stop
Program Stop M00 is typically included in the program if the CNC operator has to perform some task for each individual part of the batch, without exceptions. For example, applying special lubricant for a tapping tool, flipping or repositioning the part, readjusting a clamp, doing a mandatory dimensional check, etc., are all good reasons to include M00 in the part program. Program processing will always be temporarily stopped with M00, without any interference from the CNC operator. The M00 indicator light will only turn ON when the miscellaneous function M00 is detected during program processing.
Typical program application will be at the end of the tool, for example:
...
N31 G00 Z2.0 M09
N32 G28 Z2.0 M05
N33 M00 (PLACE PART IN FIXTURE 2)
It is a good programming practice to include a descriptive comment (message) with the M00 function.
Optional Program Stop M01 is very similar to M00, but the CNC operator does have a choice to use it or not to use it. By turning the Optional Stop switch ON (located on the operation panel), any encounter of M01 in the part program will force the program processing (execution) to stop until the Cycle Start button is pressed.
Both illustrations below show the indicator light status when program processing encounters the M01 function:
Similar to M00, typical program application of M01 will be at the end of the tool, for example:
...
N31 G00 Z2.0 M09
N32 G28 Z2.0 M05
N33 M01
Usually, there is no comment (message) attached to the M01 function.
In either case, when M00 or M01 program function is detected, many machine activities will be stopped:
| ▪All axis motion will stop | |
| ▪Spindle rotation will stop | ... M05 state |
| ▪Coolant will be turned OFF | ... M09 state |
If the program is written correctly, each toolpath that follows M00 or M01 function will include spindle speed and coolant functions, even if no M05 or M09 had been programmed.
Look for missing spindle speed and coolant in the blocks following M00 or M01
Most Fanuc controls support two Program End functions. One of the functions is the old M02, the other is the much more common M30. In the old days of paper tape, M02 was used for a loop tape (that is tape spliced at its ends), because when the end of program had been reached, the tape was physically at its beginning because of the loop. No tape rewind was necessary to use in the program. To accommodate tapes that