Siemens SINUMERIK 840D Programming Manual page 196

3
Milling Cycles
3.14 Milling circular spigots – CYCLE77 (SW 5.3 and higher)
Depth infeed:
• Infeed to safety distance
• Insertion to machining depth.
The first machining depth is the product of:
• the total depth,
• the final machining allowance and
• the maximum possible depth infeed.
Sequence of motions for finishing (_VARI=2)
Depending on the setting of parameters _FAL and _FALD, a
finishing operation is performed on the spigot surface or
base or both. The approach strategy matches the motions in
the plane executed for roughing operations.
Description of parameters
See Subsection 2.1.2. (Drilling, Centering – CYCLE81)
for a description of parameters RTP, RFP, SDIS, DP,
DPR.
See Section 3.9 for a description of parameters _MID,
_FAL, _FALD, _FFP1, _FFD.
_PRAD (diameter of spigot)
The diameter must be entered without a sign.
_PA, _PO (spigot center point)
With parameters _PA and _PO you define the reference
point of the spigot.
Circular spigots are always measured from the center.
_CDIR (milling direction)
The machining direction of the spigot is defined in this
parameter.
Under parameter _CDIR the mill direction
• direct "2 for G2" and "3 for G3" or
• alternatively "up-cut milling" or "down-cut milling" can
be programmed. Up-cut milling or down-cut milling is
determined within the cycle via the spindle direction
activated prior to the cycle call.
Up-cut
M3 → G3
M4 → G2
_VARI (machining mode)
You can define the type of machining with parameter _VARI.
Possible values are:
• 1=Roughing
• 2=Finishing.
3-196
Down-cut
M3 → G2
M4 → G3
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
04.00
© Siemens AG, 2002. All rights reserved