High-Performance Thread Mills
CNC Programming Instructions
Drill Thread Mill GTM41 • Left Hand
Preparation None
Process Principle Milling thread and core hole, countersinking (climb milling)
Cycle
Positioning
Moving sideways to
the starting point
Thread milling
(anti-clockwise)
Returning to
positioning level
Exit
Required Specification Values
Example
Size — M10-6H
Thread diameter D .........................................10mm
Pitch .............................................................1,5mm
Core hole diameter D1 ..................................8,5mm
Material — TiAl6V4 titanium
Grade — WU16PV
*(measured on the cutting part)
Tool — GTM41 Left Hand
Catalogue number ................................................GTM415005
Number of teeth Z ..................................................................4
Tool diameter d1 ........................................................7,75mm*
Tool radius compensation k1 ................................... 0,08mm**
Tool radius to be programmed2 ............................3,795mm***
Thread depth b ..............................................................20mm
Cutting speed vc ..................................................... 100 m/min
Feed (milling) fz ................................................ 0,03 mm/tooth
Number of turns5 ................................................................17
**(0.01 x D)
N = Vc • 1000
d1 • / S = 4109
vf = fz • Z • n F=
N =
vf contour • (D-d1)
D
493
(contour)
F = 111
(centre point)
***(1/2 d1 - k)
Positioning the tool N 10 G 54
Incremental programming N 20 G 91
Moving sideways to the starting point N 30 G 42
Thread milling G 02
Repeat thread milling N 40
… 5 Exit N 50 G 40
Retracting tool to positioning level N 70 G 90
Cutting time th
G 90 G 00 X… Y…
G 01 X 0 Y-5 F 493
X 0 Y 0 Z-1.500
G 01 X 0 Y 5 G 00 Z 2
Z 1.500
S 4109
(contour) [F 111] 4
I 0 J 5.000
T01 2
M04
(centre point)
68.8 seconds
NOTES:
1 The cutter radius measured over the tooth crests of the threaded part must be reduced by the amount of the cutter radius compensation. This is necessary to achieve a depth of cut to the middle
of the 6H/ISO2 nut tolerance. Please note, however, that this also depends on the radial deflection of the tool (tensile strength of the material, projecting length of the tool).
2 The cutter radius to be programmed is normally included in the tool memory.
3 The thread depth b must be divisible by the thread pitch P.
4 The feed values in brackets must be used for controllers, which do not calculate the centre point feed themselves.
5 Set N40 must be repeated with the number of threads. Repetitions N = thread depth b/pitch P (rounded up to the nearest integer).
Y82
widia.com
Program to DIN 66025 (climb milling, on the contour, incremental)