WAIT ON INPUT (M66)

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)

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.

EXAMPLE

  • 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.

EXAMPLE

  • 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:

  • M64 P0
  • M64 P2
  • M64 P3

The following is not legal:

  • M64 P023
  • M64 P0 P2 P3

SET CURRENT TOOL NUMBER (M61)

SET CURRENT TOOL NUMBER (M61)

To change the current tool number while in MDI or manual mode, program: M61 Q~

  • Q~ is the tool number

TROUBLESHOOTING

It’s an error if:

  • Q~ is not 0 or greater

SPINDLE SPEED OVERRIDE CONTROL (M51)

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)

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)

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)

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)

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)

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.