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



IMPORTANT! This is a legacy feature. Most modern programming methods don’t use temporary work offsets.

To apply a temporary work offset, program: G92 X~ Y~ Z~ A~

  • X~ is the X-axis coordinate
  • Y~ is the Y-axis coordinate
  • Z~ is the Z-axis coordinate
  • A~ is the A-axis coordinate

G92 reassigns the current controlled point to the coordinates specified by the axis words (X~, Y~, Z~, and/or A~). No motion takes place.

The axis words are optional, except that at least one must be used. If an axis word is not used for a given axis, the coordinate on that axis of the current point is not changed. Incremental distance mode (G91) has no effect on the action of G92.

When G92 is executed, it is applied to the origins of all coordinate systems (G54 through G59.3).

EXAMPLE – If the current controlled point is at X = 4, and there is currently no G92 offset active, and then G92 X7 is programmed, this reassigns the current controlled point to X = 7 — effectively moving the origin of the active coordinate system -3 units in X. The origins of all inactive coordinate systems also move -3 units in X. This -3 is saved in parameter 5211.

G92 offsets may be already be in effect when the G92 is called. If this is the case, the offset is replaced with a new offset that makes the current point become the specified value.

It’s an error if:

  • All axis words are omitted

PathPilot stores the G92 offsets and reuses them on the next run of a program. To prevent this, you can program a G92.1 (to erase them), or program a G92.2 (to stop them being applied – they are still stored).

To reset axis offsets to zero and sets parameters 5211 – 5219 to zero, program: G92.1

To reset axis offsets to zero, program: G92.2

To set the axis offset to the values saved in parameters 5211 to 5219, program: G92.3