Programming example
This example describes the milling of a hexagonal polygon with a side length of 40mm from a cylinder blank of radius 50mm. The polygon has a chamfer 1mm wide at the corner points. The spigot is 10mm deep. The blank also runs parallel to the X axis. The centre of the spigot is at the current position when the cycle is called.
The aim is to execute finishing and roughing in one pass. The finishing allowance at the base and edge is 1mm in each case. The maximum feed in the XY direction is to be half the tool diameter (10mm), resulting in a value of 5mm. In the Z direction, the tool is to be lowered by a maximum of 3mm per pass. The spigot is milled in the clockwise direction.
The Z value of the spigot surface is 0. On approach a safety clearance of 10mm is to be observed. The tool can be moved at this height at rapid traverse. The retraction plane is at height 40. The safety clearance to the blank in XY direction is 10mm.
The milling velocity in the XY plane is 200mm/min and feed in Z direction is 500mm/min.
Programing Example
Multi-edge milling
The following parameter settings are conceivable for the successful execution of the cycle.
- Hexagonal spigot:
@P6 = 6 - Side length 40mm:
@P7 = 40 - Blank of radius 50mm:
@P9 = 50 - Underside parallel to X axis
@P13 = 0 - Spigot is 10mm deep:
@P5 = 10 - Finishing allowance at base and edge is 1mm in each case:
@P18=1 @P19=1 - Finishing and roughing in one pass:
@21 = 3 - Maximum infeed in XY direction is 5mm:
@P16 = 5 - Maximum feed in Z direction is 3mm:
@P14 = 3 - Spigot is milled in clockwise direction:
@P20 = 2 - Z value of spigot surface is 0:
@P1 = 0 - Retraction plane is at height 40:
@P2 = 40 - Safety clearance in Z of 10mm:
@P3 = 10 - Safety clearance in XY of 10mm:
@P4 = 10 - Feedrate for milling in XY plane is 200mm/min:
@P17 = 200 - Feed rate for feeding in Z is 500mm/min:
@P15 = 500 - Chamfer 1mm wide:
@P22 = 1 - The spigot centre is at current position when cycle is called: No definition of @P10 and @P11
This results in the following cycle call:
T9 D9 ( Tool data / length compensation )
M6 ( Tool change )
G00 G90 M03 S6000 ( Machining values )
G00 Z600 ( Approach starting position in Z )
G00 X-50 Y0 ( Approach spigot centre point )
; Polynomial smoothing for smooth movements
#CONTOUR MODE [DEV, PATH_DEV = V.G.WZ_AKT.R / 100]
G261
L CYCLE [NAME=SysMillMultiEdge.ecy, @P6 = 6, @P7 = 40, @P9 = 50, @P21 = 3, \
@P5 = 10, @P20 = 2 @P18 = 1, @P19 = 1, @P15 = 500,\
@P16 = 5, @P14 = 3, @P13 = 0, @P1 = 0, @P2 = 40, \
@P3 = 10, @P4 = 10, @P17 = 200, @P22 = 1 ]
G260
M30