GSK GSK980TDc, Руководство пользователя

Страница: 319 / 470

Chapter 14 Machining Example
299
Ⅱ
Operation
Tool number Tool shape Explanation
No. 4 Threading tool, tool nose angle 60°
13.1 Programming
Set up the workpiece coordinate system as Fig.13-1 according to the machining process and the
codes introduced in this manual. The programming steps are as follows:
Ｏ０００１；
Name of the part program
Ｎ００００
G0 X150 Z50
； Position to the safety height for tool change
Ｎ０００５
M12
； Clamp the chuck
Ｎ００１０
M3 S800 ； Start the spindle with speed 800
Ｎ００２０
M8
；
Turn on the cooling
Ｎ００３０
T0101
； Change for the No. 1 tool
Ｎ００４０
G0 X136 Z2 ； Approach the part
Ｎ００５０
G71 U0.5 R0.5 F200
；
Cut depth 2mm and retract 1mm
Ｎ００５５
G71 P0060 Q0150 U0.25
W0.5
；
0.25mm pre-reserved in X axis, 0.5mm
machining allowance in Z axis
Ｎ００６０
G0 X16
； Approach to the end face of the part
Ｎ００７０
G1 Z-23 ； Cut the Φ 16 outer circle
Ｎ００８０
X39.98
；
Cut the end face
Ｎ００９０
W-33
； Cut the Φ 39.98 outer circle
Ｎ０１００
X40 ； Cut the end face
Ｎ０１０５
W-30
；
Cut the Φ 40 outer circle
Ｎ０１１０
G3 X80 W-20 R20
； Cut the convex arc
Ｎ０１２０
G2 X120 W-20 R20
； Cut the concave arc
Ｎ０１３０
G1 W-20 ； Cut the Φ 120 outer circle
Ｎ０１４０
G1 X130 W-5
；
Cut the cone
Ｎ０１５０
G1 W-25
； Cut the Φ 130 outer circle
Ｎ０１６０
G0 X150 Z185
；
Rough cut end and back to the tool change
point
Ｎ０１７０
T0202
；
Change for the No.2 tool and execute its
offset
Ｎ０１８０
G70 P0060 Q0150
； Fine cut cycle