Haas Mill, Operator'S Manual

Page: 123 / 217

1 1 6 G Codes 96-8000 rev R June 2007
Corner Rounding and Chamfering example:
G00 X1. Y1.
G01 X5. F10. ,C0.75
Y2.5 ,R0.4
G03 X8. Y5. R3. ,R0.8
G01 X5. ,C0.8
Y7. ,R1.
X1. ,R1.
Y1.
G00 X0 Y0
M30
Thread Milling
Thread milling uses a standard G02 or G03 move to create the circular move in X-Y and then adds a Z move on the
same block to create the thread pitch. This will generate one turn of the thread; the multiple teeth of the cutter will
generate the rest. A typical line of code follows:
N100 G02 I-1.0 Z-.05 F5. (generates a 1-inch radius for 20-pitch thread)
Thread Milling notes: Internal holes smaller than 3/8 inch may not be possible or practical. Always climb cut the
cutter.
Use a G03 to cut I.D. threads or a G02 to cut O.D. threads. An I.D. right hand thread will move up in the Z-axis by
the amount of one thread pitch. An O.D. right hand thread will move down in the Z-axis by the amount of one
thread pitch. PITCH = 1/Threads per inch (Example - 1.0 divided by 8 TPI = .125)
Thread Milling Example:
This program will I.D. thread mill a 1.5 x 8 TPI hole using a .750 diameter x 1.0 thread hob.
To start, take the hole diameter (1.500). Subtract the cutter diameter .750 and then divide by 2.
(1.500 - .75) / 2 = .375
The result (.375) is the distance the cutter starts from the I.D. of the part.
After the initial positioning, the next step of the program is to turn on cutter compensation and move to the I.D. of
the circle.
The next step is to program a complete circle (G02 or G03) with a Z-axis command of the amount of one full pitch
of the thread (this is called "helical interpolation")
The last step is to move away from the I.D. of the circle and turn off cutter compensation
Cutter compensation cannot be turned off or on during an arc movement. A linear move must be made, either in the
X or Y axis to move the tool to and from the diameter to cut. This move will be the maximum compensation amount
that can be adjusted.