High-Performance Thread Mills
CNC Programming Instructions
Thread Mill GTM21
Preparation Drilling of thread hole
Process Principle Countersinking, thread milling (conventional milling)
Cycle
Positioning
Countersinking
Raise
Run-in loop for
thread milling
Thread milling
Run-out loop
Returning to
positioning level
Required Specification Values
Example
Size — M10-6H
Thread diameter D .........................................10mm
Pitch .............................................................1,5mm
Core hole diameter D1 ..................................8,5mm
Material — Cast aluminium
Grade — WU12PV
*(measured on the cutting part)
Tool — GTM21
Catalogue number ................................................GTM215004
Number of teeth Z ..................................................................3
Tool diameter d1 ..........................................................8,2mm*
Tool radius compensation k1 ..................................... 0,1mm**
Tool radius to be programmed2 ...................................4mm***
Countersink depth ls ...................................................21,2mm
Cutting speed vc ..................................................... 250 m/min
Feed (countersinking) fs ............................................0,3 mm/U
Feed (milling) fz ................................................ 0,09 mm/tooth
**(0.01 x D)
Vc • 1000
N =
S = 9709
d1 • /
vs = fs • n F = 2913
(countersinking)
vf = fz • Z • n F = 2622
(contour)
vf =
vf contour • (D-d1)
***(1/2 d1 - k)
D
F =
472
(centre point)
Positioning the tool N 10 G 54 G 90
G 00
Advancing tool to full thread depth N 20 G 91 Z-21.200 Countersinking N 30 G 01 Z-2 Raise N 40 G 00 Z 3.450 Moving sideways to the starting point N 50 G 42 G01 X 4.250
X…
Y…
Z 2
T01 2
M03
F 2913 (countersink)
F 1311 (milling, 1/2 contour)
Run-in loop in arc N 60 G 02 X-9.25 Y 0.000 Z-0.750 I-4.625 J 0
Thread milling N 70 G 02 X 0 Y 0 Z-1.500 I 5 J 0.000
Run-out loop in arc N 80 G 02 X 9.25 Y 0.000 Z-0.750 I 4.625 J 0
Exit N 90 G 40 G 01 X-4.25 Retracting tool to positioning level N 100 G 90 G 00 Z 2
Cutting time th
S 9709
[F 236] 3 (milling,1/2 centre point)
F2622
[F 472] 3 (centre point)
1.4 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 feed values in brackets must be used for controllers, which do not calculate the centre point feed themselves.
Y80
widia.com
Program to DIN 66025 (conventional milling, on the contour, incremental)