G143 5-Axis Tool Length Compensation + (Group 08)

Next Generation Control Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue

(This G-code is optional; it only applies to machines on which all rotary motion is movement of the cutting tool, such as VR-series mills)

This G code allows the user to correct for variations in the length of cutting tools without the need for a CAD/CAM processor. An H code is required to select the tool length from the existing length compensation tables. A G49 or H00 command will cancel 5-axis compensation. For G143 to work correctly there must be two rotary axes, A and B. G90, absolute positioning mode must be active (G91 cannot be used). Work position 0,0 for the A and B axes must be so the tool is parallel with Z-Axis motion.

The intention behind G143 is to compensate for the difference in tool length between the originally posted tool and a substitute tool. Using G143 allows the program to run without having to repost a new tool length.

G143 tool length compensation works only with rapid (G00) and linear feed (G01) motions; no other feed functions (G02 or G03) or canned cycles (drilling, tapping, etc.) can be used. For a positive tool length, the Z-Axis would move upward (in the + direction). If one of X, Y or Z is not programmed, there will be no motion of that axis, even if the motion of A or B produces a new tool length vector. Thus a typical program would use all 5 axes on one block of data. G143 may effect commanded motion of all axes in order to compensate for the A and B axes.

Inverse feed mode (G93) is recommended, when using G143.

% O61431 (G143 5-AXIS TOOL LENGTH) ; (G54 X0 Y0 is at the top-right) ; (Z0 is on top of the part) ; (BEGIN PREPARATION BLOCKS) ; T1 M06 (Select tool 1) ; G00 G90 G40 G49 G54 (Safe startup) ; G00 G54 X0 Y0 Z0 A0 B0 (Rapid to 1st position) ; S1000 M03 (Spindle on CW) ; G143 H01 X0. Y0. Z0. A-20. B-20. ; (Rapid to position w/ 5 Axis tool length comp) ; M08 (Coolant on) ; (BEGIN CUTTING BLOCKS) ; G01 G93 X.01 Y.01 Z.01 A-19.9 B-19.9 F300. ; (Inverse time feed on , 1st linear motion) ; X0.02 Y0.03 Z0.04 A-19.7 B-19.7 F300. ( 2nd motion) ; X0.02 Y0.055 Z0.064 A-19.5 B-19.6 F300. (3rd motion) ; X2.345 Y.1234 Z-1.234 A-4.127 B-12.32 F200. ; (Last motion) ; (BEGIN COMPLETION BLOCKS) ; G94 F50. (Inverse time feed off) ; G00 G90 Z0.1 M09 (Rapid retract, Coolant off) ; G53 G49 Z0 M05 (Tool length comp off) ; (Z home, Spindle off) ; G53 Y0 (Y home) ; M30 (End program) ; %

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.