YAMAZAKI MAZAK INTEGREX e Series - Polar Coordinate Interpolation

MACHINING PROGRAM 4
4-31
2. Polar coordinate interpolation
This section explains how to make the program of Polar coordinate interpolation in 3-axis
machining program.
A. Sample program
G109L1
M901
M200
M212
G0G90G94G54G97
G40G49G80G67G69
G91G28X0
G28Z0
G28Y0
T001T00M06
G91G28X0
G28Y0
G28Z0
M108
G90G53B0.
G97S3000M03
G10.9X0
M08
G61.1
M108
G90G53B0.
G90G00C0.
M107
G90G43G00X70.0Y0.Z-15.0H1
G17G90G00X70.0C0.
G12.1
G01G42D51X50.C50.F500.
C-50.
X-50.
C50.
X50.
Z10.0
G40
G13.1
G64
M05
M09
G91G28X0
G28Y0
G28Z0
M30
(3-axis machining_ Polar coordinate interpolation)
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
 G97S3000: Rotation speed 3000 min
-1
 M03: Forward milling spindle rotation
 G10.9X0: Radius data input mode
 M08: Flood coolant ON
End motion for machining
 M05: Stop of milling spindle rotation
 M09: coolants OFF
 Each axis positioning to zero return
 M30: Reset and rewind
Machining motion
 G61.1: Geometry compensation
 Rotational axis positioning
 G17XC: XC-plane selection
 G43H**(P0): Tool length offset
 G12.1: Polar coordinate interpolation ON
 G41D**: Tool radius compensation (left)
 (Machining pattern)
 G40: Tool radius compensation OFF
 G13.1: Polar coordinate interpolation OFF
 G64: Geometry compensation OFF
Machining contour
Serial No. 294060
Copyright (c) 2013 YAMAZAKI MAZAK CORPORATION. All rights reserved.
Serial No. 294060