Общий каталог Widia 2017 - страница 1784

Предыдущая страница Следующая страница

Навигация

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 Run-out loop Returning to thread milling positioning level Required Specification Values Example Size — M10-6H Tool — GTM21Thread diameter D.........................................10mmCatalogue number ................................................GTM215004 N =Pitch ............................................................. 1,5mmNumber of teeth Z..................................................................3Vc • 1000d1 • /S= 9709 Core hole diameter D1 ..................................8,5mmMaterial — Cast aluminiumGrade — WU12PVTool Tool draiadmiuestceor md1p.e..n.s..a..t.i.o..n...k..1.............................................................................0.8,1,2mmmm***Tool radius to be programmed2 ...................................4mm***vs = fs • nF= 2913 (countersinking) Countersink depth ls...................................................21,2mmCutting speed vc..................................................... 250 m/minvf = fz • Z • n F = 2622 (contour) Feed (countersinking) fs............................................0,3 mm/U Feed (milling) fz ................................................ 0,09 mm/tooth vf contour • (D-d1)vf =DF= 472 (centre point) *(measured on the cutting part) **(0.01 x D) ***(1/2 d1 - k) Program to DIN 66025 (conventional milling, on the contour, incremental) Positioning the tool N 10 G 54 G 90 G 00 X… Y… Z2 S 9709 T01 2 M03 Advancing tool to full thread depth N 20 G 91 Z-21.200 Countersinking N 30 G 01 Z-2 F 2913 (countersink) Raise N 40 G 00 Z 3.450 Moving sideways to the starting point N 50 G 42 G01 X 4.250 F 1311 (milling, 1/2 contour) [F 236] 3 (milling,1/2 centre point) Run-in loop in arc N 60 G 02 X-9.25 Y 0.000 Z-0.750 I-4.625 J0 Thread milling N 70 G 02 X0 Y0 Z-1.500 I5 J 0.000 F2622 [F 472] 3 (centre point) Run-out loop in arc N 80 G 02 X 9.25 Y 0.000 Z-0.750 I 4.625 J0 Exit N 90 G 40 G 01 X-4.25 Retracting tool to positioning level N 100 G 90 G 00 Z2 Cutting time th 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 High-Performance Thread Mills