Introducing the new 1500MX CNC Mill. In stock and ready to ship in the continental US. Learn more



G38.2 probes toward the workpiece, stops on contact, and signals error if failure

G38.3 probes toward the workpiece and stops on contact

G38.4 probes away from the workpiece, stops on loss of contact, and signals error if failure

G38.5 probes away from the workpiece and stops on loss of contact

G38.6 moves away from the workpiece and ignores probe input

To perform a straight probe operation program: G31 X~ Y~ Z~ A~

Conventionally, the probe is tool #99. The rotational axis words are allowed, but it’s better to omit them. If rotational axis words are used, the numbers must be the same as the current position numbers so that the rotational axes do not move. The tool in the spindle must be a probe.

In response to this command, the mill moves the controlled point (which should be at the end of the probe tip) in a straight line at the current feed rate toward the programmed point; if the probe trips, then the probe decelerates.

After successful probing, parameters 5061 to 5064 will be set to the coordinates of the location of the controlled point at the time the probe tripped (not where it stopped), or if it does not trip to the coordinates at the end of the move and a triplet giving X, Y, and Z at the trip is written to the triplet file.


It’s an error if:

  • The current point is less than 0.01 in. (0.254 mm) from the programmed point
  • G38 is used in inverse time feed rate mode
  • Any rotational axis is commanded to move
  • No X-, Y- or Z-axis word is used – The linear axis words are optional, except that at least one of them must be used.
  • Feed rate is zero
  • The probe is already tripped