High-Performance Thread Mills CNC Programming Instructions
Drill Thread Mill GTM41 • Right Hand
Preparation
None
Process Principle Milling thread and core hole, countersinking( conventional milling) Cycle
Positioning |
Moving sideways to the starting point |
Thread milling( clockwise) |
Exit |
Returning to positioning level |
Required Specification Values
Example
Size— M10-6H Thread diameter D......................................... 10mm Pitch............................................................. 1,5mm Core hole diameter D 1.................................. 8,5mm
Material— Hard steel, 50 HRC Grade— WU16PV
Tool— GTM41 Right Hand Catalogue number................................................ GTM415005 Number of teeth Z.................................................................. 4 Tool diameter d 1........................................................ 7,75mm * Tool radius compensation k 1................................... 0,08mm ** Tool radius to be programmed 2............................ 3,795mm *** Thread depth b.............................................................. 20mm Cutting speed v c..................................................... 100 m / min Feed( milling) f z................................................ 0,04 mm / tooth Number of turns 5................................................................ 17
N =
V c • 1000 d 1 • �
S = 4109
v f = f z • Z • n F = 657( contour)
N = v f contour •( D-d 1) F = 148( centre point)
D
*( measured on the cutting part) **( 0.01 x D; adjust to application) ***( 1 / 2 d 1- k)
Program to DIN 66025( conventional milling, on the contour, incremental)
Positioning the tool |
N 10 |
G 54 |
G 90 |
G 00 |
X … |
Y … |
Z 1.500 |
S 4109 |
T01 2 |
M03 6 |
Incremental programming |
N 20 |
G 91 |
|
|
|
|
|
|
|
|
Moving sideways to the starting point |
N 30 |
G 42 |
G 01 |
X 0 |
Y-5 |
F 657 |
( contour) |
[ F 148 ] 4 |
( centre point) |
|
Thread milling |
N 40 |
G 02 |
|
X 0 |
Y 0 |
Z-1.500 |
I 0 |
J 5.000 |
|
|
Repeat thread milling |
… 5 |
|
|
|
|
|
|
|
|
|
Exit |
N 50 |
G 40 |
G 01 |
X 0 |
Y 5 |
|
|
|
|
|
Retracting tool to positioning level |
N 70 |
G 90 |
G 00 |
Z 2 |
|
|
|
|
|
|
Cutting time t h
widia. com
51.6 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).
Y81
High-Performance Thread Mills KL-TECH s. r. o. | www. klte. cz