Operator`s manual

Advanced Haas Mill Programming Techniques Training Manual Page 17
Tool Length Offset and Cutter Radius Compensation Techniques
Tool Length Offset Compensation
Tool length compensation allows the programmer to not worry about the length of the tool and program to
the top surface of the part. Normally the top surface of the part is set as Z zero.
The following command turns on tool compensation for a particular tool. In this instance Tool #1.
G43 H01 Z.1
The above command (normally given with the machine in the rapid mode, G00) will rapid to .100 inch
above the top face of the part using Tool Length Offset 1. The program would use the value in line 1 and
column labeled H Geometry, 3.5000.
During a set up if T1 was a ½” end mill and a close tolerance .200 +/-.0005” depth of pocket needed to be
held the prudent machinist would add .01” in the WEAR column of T1. The part would be run and the
depth of the pocket measure in the machine. If the value was .192 the cutter needs to go .008 deeper. So
-.008 would be added to the Wear of the tool which would leave it at .002”. The machinist prevents from
possibly scraping out the first piece by adding a small amount to the wear offset.
Another situation may come up where two close tolerance depth features (+/-.0005) are created with the
same tool #1. If both tolerances cannot be held with one length offset then a secondary offset may be
used. Pick an offset that is not being used such as 10 above. Put the same H Geometry value in 10 as in 1.
Also put the same Wear in 10 that was in 1. Then either add or subtract the amount to make the second
feature so it will be at nominal value. The program needs to be edited to reflect using a secondary offset.
In the program after the first feature is completed and the Z is above the top face of part: (G43 H10 Z.1.) is
inserted for the second offset.