WARNING: M06 must be preceded by an M05 or unpredictable results may occur.

CAUTION: This command can be used in different combinations and wrong command can result in unexpected loading of tool. See video below

This command is used to change tool immediately and can be used with T value.

Syntax & Parameters

• M06
• M6 - The same as M06
• T Value – specifies the tool number to change, this value can be used before M06 or after M06 but will have a very different process of tool loading.

Tool Numbers

MASSO G2 use tool numbers 0 to 31

MASSO G3 & MASSO Touch use tools 0 to 118

Tool 0 - Dry run laser

Tool 1 - 100 Main spindle tools

Tool 101 - 104 Multi-Head spindles 1 - 4

Tools 111 - Laser

Tool 112 - Plasma

Tool 113 - Oxy Torch

Tool 114 - Waterjet

Tool 115 - Scribe

Tool 116 - 117 Pen

Tool 118 - Camera

WARNING: The T value must precede the M06 or unpredictable results may occur. Please see the video below for additional information

This Video shows the importance of formatting the M6 command correctly with the tool number first.

Example program

N10 M05
N20 T5 M06

In above program the M05 stops the spindle then T5 tells the system that we would like to load tool number 5 and M06 is used to tell the system to load the tool.

Special note for Multi-Head users

When tool changes are done in conjunction with multi-head it is advisable to raise the Z axis to a safe height before performing the tool change.

This ensures that the height difference between the old and new tool will not cause any problems.

One way to do this is with a G53 Z0 or similar to raise the Z axis to the top of the machine travel to give maximum clearance.

Example program

N10 M05
N20 G53 Z0
N30 T5 M06

In above program the M05 stops the spindle.

The Z axis moves to machine coordinate Z0 to ensure clearance between the material surface and the new tool

T5 tells the system that we would like to load tool number 5 and M06 is used to tell the system to load the tool.

Troubleshooting

• If you find that the tool does not change when you issue a the Txx M06 Gcode command it is because the tool number you are requesting is already in the spindle. MASSO remembers the last tool that was in the spindle even after being powered off. Check the tool number currently loaded in the F2 screen.
• If you have to ask for a tool change twice or you find it is loading the previously requested tool it is because you have the tool change command format wrong, Txx M06 is correct and behaves completely differently from M06 Txx. Please watch the video above to understand the difference.
• When using the tool setter if you find the Z0 point of the 2nd tool is incorrect you are using the tool setter / tool changer incorrectly. Please read How the Tool Setter works to understand the correct process.