WAIT ON INPUT (M66)
NOTE: This command is only useful when the mill is equipped with the USB M-Code I/O Interface Kit.
There are four digital inputs available on the USB I/O module.
M66 P- | E-
- P- is the digital input number from 0 to 3.
- L- is the wait mode type:
- Mode 0: IMMEDIATE – no waiting, returns immediately. The value of the input at that time is stored in parameter #5399.
- Mode 1: RISE – waits for the selected input to perform a rise event.
- Mode 2: FALL – waits for the selected input to perform a fall event.
- Mode 3: HIGH – waits for the selected input to go to the HIGH state.
- Mode 4: LOW – waits for the selected input to go to the LOW state.
- Q- is the timeout in seconds for waiting
The Q value is ignored if the L word is zero (IMMEDIATE). A Q value of zero is an error if the L word is non-zero.
SET OUTPUT STATE (M64 AND M65)
NOTE: These commands are only useful when the mill is equipped with the USB M-Code I/O Interface Kit.
There are four output relays available on the USB I/O module.
To activate output relays (contact close), program: M64
To deactivate output relays (contact open), program: M65
There are four contacts, numbered from 0 to 3. The contact is specified by the P word.
- Activating the first relay: M64 P0
- Activating the second relay: M64 P1
The outputs are deactivated using M65 with the P word specifying the relay.
- Deactivating the second relay: M65 P1
- Deactivating the fourth relay: M65 P3
There is only one P word and one relay per line. Each relay command must be done on an individual line.
The following is legal:
The following is not legal:
SET CURRENT TOOL NUMBER (M61)
To change the current tool number while in MDI or manual mode, program: M61 Q~
It’s an error if:
SPINDLE SPEED OVERRIDE CONTROL (M51)
To enable the spindle speed override control, program: M51 P1
The P1 is optional.
To disable the spindle speed override control, program: M51 P0
When spindle speed override control is disabled, the spindle speed override slider has no influence, and the spindle speed is equal to the value of the S word.
FEED OVERRIDE CONTROL (M50)
To enable the feed rate override control, program: M50 P1
The P1 is optional.
To disable the feed rate control, program: M50 P0
When feed rate override control is disabled, the feed rate override slider has no influence, and all motion is executed at programmed feed rate (unless there is an adaptive feed rate override active).
OVERRIDE CONTROL (M48 AND M49)
To enable the speed and feed override, program: M48
To disable both overrides, program: M49
It’s okay to enable or disable the switches when they are already enabled or disabled.
COOLANT CONTROL (M07, M08, AND M09)
To turn coolant on, program: M07
To turn flood coolant on, program: M08
To turn all coolant off, program: M09
It’s always okay to use any of these commands, regardless of what coolant is on or off.
TOOL CHANGE (M06)
To execute a tool change sequence, program: M06
M06 behaves differently depending on whether or not a mill is equipped with an Automatic Tool Changer (ATC):
- If you have an ATC:
- If the requested tool (T number) is assigned to the carousel, M06 initiates an automatic tool change.
- If the tool is not assigned to the carousel, you’re prompted to manually change the tool and select Cycle Start to confirm the tool change. This resumes the program.
- If you don’t have an ATC:
- M06 commands the mill, stops the spindle, pauses program execution, and prompts operator to change tools by flashing Tool Change LED.
- The program resumes after you select Cycle Start to confirm that the tool has been changed.
We recommend putting the T~, the M06, and the G43 H~ on one line (block) of code.
EXAMPLE – N191 M06 T3 G43 H3
SPINDLE CONTROL (M03, M04, AND M05)
To start the spindle turning clockwise (forward) at the currently programmed speed, program: M03
To start the spindle turning counterclockwise at the currently programmed speed, program: M04
The speed is programmed by the S word.
To stop the spindle from turning, program: M05
It’s okay to use M03 or M04 if the spindle speed is set to 0; if this is done, the spindle won’t start turning. If later the spindle speed is set above 0, the spindle starts turning. It is permitted to use M03 or M04 when the spindle is already turning, or to use M05 when the spindle is already stopped.