website logo
Home pageWeb storeDistributors
Software
Hardware
Settings
Troubleshooting
Navigate through spaces
⌘K
EdingCNC Documentation
Getting started with your new controller
G-code
Language standard
Supported G-code
Supported M-codes
Other input codes
Special commands
Special features
Macro programming
Run behavior during loading of job file and simulation
Software installation
Interface
Keyboard shortcuts
Docs powered by archbee 

G43, G43.1, G49 (Tool Length Offset)

2min
  1. 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.
  2. 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)
  3. 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.

PREVIOUS
G40, G41, G41.1, G42, G42.1 (Cutter Radius Compensation)
NEXT
G50, G51 (Scaling)
Docs powered by archbee