G38.7 - Center Probing Cycle
G38.7 finds the centre of a feature. It probes in +X, −X, +Y and −Y, then moves the probe to the calculated centre and stops. It doesn't update work offsets itself; use it with G92 or G10 to do that.
Syntax
G38.7 F100
Probing limits
Machine soft limits
Not available on
MASSO G2
WARNING
Incorrect use of G38.7 can damage the probe and the item being probed, and can cause injury. Make sure you fully understand the probing process and take extreme care with this command.1. Parameters
If an edge isn't found before a soft limit is reached, the cycle stops and a probing alarm is raised. Units are inches or millimetres, depending on the machine setup and whether G20 or G21 is active.
2. Example – temporary offset with G92
N10 T100 M06 N20 G0 X20 Y30 N30 G1 Z-2 F500 N40 G38.7 F100 N50 G92 X0 Y0 N60 G0 Z10
3. Example – update a work offset with 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
WARNING
G10 does not overwrite the G54 to G59 values saved to backup memory from the F4 screen, even though the F4 screen shows the new values. When restarting a job, always check the F4 Work Offset table to make sure the offsets are correct.
