This tool changer is available in MASSO G3 & MASSO Touch -  v5.06 or higher. 

WARNING: The incorrect use of this Gcode can cause damage to your probing equipment, the item being probed and personal injury. Please understand and exercise care.

This command is used for locating the center of a feature.

• The probing limits are defined by the machine soft limits. If the edge of the probed feature are not located before the soft limit is reached a probing alarm occur.
• The feature will be probed in the + X,-X,+Y and -Y direction before moving to the center of the feature and stopping.
• Work offsets are not updated by this Gcode however it can be used in conjunction with G92 or G10 as required.
• Units are defined as either inches or mm depending on your machines setup or G20 or G21 command in use.

INFORMATION: This Gcode is not available for MASSO G2

Syntax & Parameters

• F Value - The F value defines the feed rate at which the axis will move.

Example program

N10 T100 M06
N20 G0 X20 Y30
N30 G1 Z-2 F500
N40 G38.7 F100
N50 G92 X0 Y0
N60 G0 Z10

In this example

N10 The Probing tool is loaded.

N20 The probe moves to the inside of the feature that needs to be probed

N30 The Probe is lowered into the feature

N40 The feature is probed using G38.7 at the specified feed rate of 100 and at the end of the probing cycle the probe will move to the center of the feature.

N50 The X & Y axis working coordinates to X0 Y0 using temporary work offsets.

The X & Y values can be used to define the offset of the probe if the probe is offset from the spindle or other head.

N60 Probe raised above feature

Example program

N10 G55
N20 T100 M06
N30 G0 X20 Y30
N40 G1 Z-2 F500
N50 G38.7 F100
N60 G10 L2.1 P0 X0 Y0
N70 G0 Z10

In this example

N10 Set G55 as the current working coordinate.

N20 The Probing tool is loaded.

N30 The probe moves to the inside of the feature that needs to be probed

N40 The Probe is lowered into the feature

N50 The feature is probed using G38.7 at the specified feed rate of 100 and at the end of the probing cycle the probe will move to the center of the feature.

N60 The Current work offset (G55) is updated in the F4 work offset table to the current position offset by the amount specifies by the X & Y values.

The X & Y values can be used to define the offset of the probe if the probe is offset from the spindle or other head.

N70 Probe raised above feature

WARNING: G10 does not overwrite G54 - G59 offset values saved to backup memory through the F4 screen, although the F4 screen will display the changed offset values. When restarting a job check the F4 table to ensure the work offsets are correct for your job.