G43, G43.1, G49 (Tool Length Offset)
- To use the tool offset of the tool in the spindle use G43. This assures that always the tool length of the tool in the spindle is compensated.
- To use a tool length offset from the tool table, program G43 H..., where the H number is the desired index in the tool table. ( H = 1-99)
- To use dynamic tool compensation (not from the tool table), use G43.1 I... K... where I... gives the tool X offset (turning) and K... gives the tool Z offset (for turning and milling)
Warning: If you use option 2 or 3, the tool-length compensation will not adapt to the new tool after M6T…
To have no tool length offset compensation, program G49
Variables #5401 to #5499 is the tool length of tool 1-99
Variables #5501 to #5599 is the tool diameter of tool 1-99
Variables #5601 to #5699 is the tool x-offset (width for turning) offset.
The variables can be modified runtime (in the G-Code file) if needed to compensate for tool-wear.