Siemens SINUMERIK 840D Programming Manual page 210

3
Milling Cycles
3.15 Pocket milling with islands – CYCLE73, CYCLE74, CYCLE75
Description of parameters
_VARI (machining mode)
You can define the type of machining with parameter
_VARI. Possible values are:
Units digit:
• 1=Rough cut (solid machine) from solid material
• 2=Rough cut residual material
• 3=Finish edge
• 4=Finish base
• 5=Rough drill.
When "Rough cut from solid material" is set, the
machining program solid machines the pocket
completely down to the final machining allowance.
If it is not possible to machine areas of the edge
surfaces with the selected mill diameter, then setting "2"
can be selected to machine them afterwards with a
smaller milling tool. To do this, cycle CYCLE73 must be
called again.
Tens digit:
• 1=Vertical with G1
• 2=Along a helical path
• 3=Oscillation.
Selection of insertion strategies:
• Insert vertically (_VARI=XX1X)
means that the current infeed depth calculated
internally is executed in one block.
• Insert along helical path (_VARI=XX2X)
means that the mill center point traverses along
the helical path determined by radius _RAD and
depth per revolution _DP1. The feedrate is
always programmed through _FFD. The sense of
rotation of this helical path corresponds to the
direction to be used for machining the pocket.
The depth programmed under _DP1 on insertion
is calculated as the maximum depth and is
always calculated as a whole number of
revolutions of the helical path.
3-210
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
08.99
© Siemens AG, 2002. All rights reserved