Operator`s manual

Advanced Haas Mill Programming Techniques Training Manual Page 21
Chamfering using Tool Compensation
Using tool compensation parts may easily be chamfered using the right tools. A chamfering operation may
be easily added to the program example on page 16. To create the chamfer a ¼” 90 degree point carbide
N/C spot drill is selected. Then a tool operation is added using the same tool path found in sub routine
N100, see below. The depth that the tool is set to go is Z-.080. If the tool is uncompensated the part will
end up with an .08 chamfer with a nasty bur at the bottom. See Uncompensated Path illustration below.
If the tool is moved .06 off of the profile as shown in the Compensated Path illustration below, a clean .02”
chamfer results. To do this D4 is set to .06” if the D values are set up as radii or .12” if the D values are set
as diameters.
T4M06 (1/4" 90 DEGREE SPOT DRILL)
(SET D4=.120)
G00 G90 G54 X0. Y1.25 S5000 M03
G43 H04 Z1. M08
G01 Z-0.08 F50.
G01 G41 D04 X-0.5 F50.
M97 P100 (TOOL PATH SUB)
M30
Uncompensated Path Compensated Path