Siemens SINUMERIK 808D User Manual page 206

The retraction plane (RTP) is approached at rapid traverse rate to then be able to position at this height to the starting point
in the machining plane. The starting point is defined with reference to 0 degrees of the axis of the abscissa.
The tool is fed to the safety clearance (SDIS) at rapid traverse with subsequent traversing to the machining depth at
feedrate. To approach the spigot contour, the tool is approached along a semi-circular path using the programmed blank
spigot.
The milling direction can be determined either as up-cut milling or down-cut milling with reference to the spindle direction.
If the spigot is bypassed once, the contour is left along a semi-circle in the plane, and the tool is fed to the next machining
depth.
The contour is then reapproached along a semi-circle and the spigot traversed once. This process is repeated until the
programmed spigot depth is reached.
Then, the retraction plane (RTP) is approached at rapid traverse rate.
● Depth infeed:
– Feeding to the safety clearance
– Insertion to machining depth
The first machining depth is calculated from the total depth, finishing allowance, and the maximum possible depth infeed.
Se quence of motions when finishing (VARI=2):
According to the set parameters FAL and FALD, either finishing is carried out at the surface contour or at the base or both
together. The approach strategy corresponds to the motions in the plane as with roughing.
Explanation of the parameters
For an explanation of the parameters RTP, RFP, SDIS, DP, and DPR, see Section "Drilling, centering - CYCLE81
(Page 157)".
For an explanation of the parameters MID, FAL, FALD, FFP1, and FFD, see Section "Milling a rectangular pocket -
POCKET3 (Page 221)".
PR AD (diameter o f spigot)
Enter the diameter without sign.
PA, PO (spigot center point)
Use the parameters PA and PO to define the reference point of the spigot.
C D IR (milling direction)
Use this parameter to specify the machining direction for the spigot. Using the parameter CDIR, the milling direction can be
programmed directly with "2 for G2" and "3 for G3", or alternatively with "synchronous milling" or "conventional milling".
Down-cut and up-cut millings are determined internally in the cycle via the direction of rotation of the spindle activated prior
to calling the cycle.
D o wn-cut
M3 → G3
M4 → G2
VAR I (machining type)
Use the parameter VARI to define the machining type. Possible values are:
● 1=roughing
● 2=finishing
AP1 (diameter of blank spigot)
Use this parameter to define the blank dimension of the spigot (without sign). The internally calculated radius of the
approach semi-circle depends on this dimension.
206
U p -cut
M3 → G2
M4 → G3
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017