The G38.7 command is used to locate the centre of a feature using a probing cycle.

The probing limits are defined by the machine soft limits. If the edges of the probed feature are not detected before a soft limit is reached, the probing cycle will stop and a probing alarm will occur.

During the probing cycle, the feature is probed in the +X, ?X, +Y, and ?Y directions. After all four edges are detected, the probe moves automatically to the calculated centre of the feature and stops.

Work offsets are not automatically updated by this G-code. However, the command can be used in conjunction with G92 or G10 to set or update work offsets as required.

Units are defined as either inches or millimetres, depending on the machine setup or whether G20 or G21 is active.

Syntax & Parameters

The F value defines the feed rate at which the probing movements will occur.

Example Program – Temporary Work Offset Using G92

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, the probing tool is first loaded.

The probe is then moved to a position inside the feature to be measured.

The probe is lowered into the feature, after which the G38.7 command probes the feature at a feed rate of 100. When the probing cycle is complete, the probe moves to the centre of the feature.

A temporary work offset is applied using G92, setting the current X and Y working coordinates to X0 Y0. The X and Y values can be adjusted to compensate for probe offsets if the probe is not aligned with the spindle or cutting head.

Finally, the probe is raised clear of the feature.

Example Program – Updating Work Offset Using G10

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, G55 is selected as the active working coordinate system.

The probing tool is loaded, and the probe is positioned inside the feature before being lowered into it.

The G38.7 command probes the feature at a feed rate of 100 and moves the probe to the centre of the feature at the end of the cycle.

The current work offset, which in this case is G55, is then updated in the F4 Work Offset table using the G10 command. The offset is applied based on the current position and the X and Y values specified. These values can be used to compensate for probe offsets if required.

The probe is then raised above the feature.