YAMAZAKI MAZAK INTEGREX e Series User Manual

MACHINING PROGRAM 4
4-43
2. Tool Radius compensation for 5-axis machining
This section explains how to make the program of 5-axis Machining using Tool Radius
Compensation for 5-axis Machining.
A. Sample program
G109L1
M901
M200
M212
G0G90G94G55G97
G40G49G80G67G69
G91G28X0
G28Z0
G28Y0
T001T00M06
G91G28X0
G28Y0
G28Z0
M108
G90G53B0.0
G97S12000M03
G10.9X0
M51
M825
G61.1
M108
G90G53B0.
G90G00C0.
G43.4G00X76.1704Y118.5904Z350.B0.C0.H1
G41.5 D51
(G05P2)
G01X23.0544Y50.1894Z300.F796.
X21.175Y47.7693
X19.4744Y45.2203
(Machining contour)
X29.6674Y62.4938Z150.9717
X29.6685Y62.4749Z150.9705
X115.2461Y67.3568Z202.4743
(G05P0)
G40
G49
G64
M05
M09
G91G28X0
G28Z0
G28Y0
M108
G90G53B0
M30
Preparation motion for machining
 G109L1: Upper turret selection
 M901: HD1 spindle selection
 M200: C-axis connect/Milling mode select
 M212: C-axis unclamping
 G94: Feed per minute
 G97: Constant surface speed control OFF
 T001M06: Tool change (TNo.01)
 B-axis positioning
 G97S12000: Rotation speed 12000 min
-1
 M03: Forward milling spindle rotation
 G10.9X0: Radius data input mode
 M51: Milling spindle-through coolant ON
 M825: Accuracy level 5
Machining motion
 G61.1: Geometry compensation
 Rotational axis positioning
 G43.4H**: Tool tip point control
 G41.5D**: Tool radius
compensation for 5-axis machining
 (Machining pattern)
 G40: Tool radius compensation
for 5-axis machining OFF
 G49: Tool tip point control OFF
 G64:Geometry compensation OFF
End motion for machining
 M05: Stop of milling spindle rotation
 M09: coolants OFF
 Each axis positioning to zero return
 M30: Reset and rewind
(5-axis Machining _Tool Radius Compensation)
Machining contour
Serial No. 294060
Copyright (c) 2013 YAMAZAKI MAZAK CORPORATION. All rights reserved.
Serial No. 294060

YAMAZAKI MAZAK INTEGREX e Series Specifications

General

Brand	YAMAZAKI MAZAK
Model	INTEGREX e Series
Category	Computer Hardware
Language	English