Siemens SINUMERIK 840D Programming Manual page 289

4
03.96
FORM (definition)
Form E and Form F are defined in DIN509 and
determined by this parameter.
If the parameter is assigned a value other than E or
F, the cycle is aborted and alarm
61609 "Form incorrectly defined" is output.
_VARI (undercut position)
The position of the undercut can be either specified
directly or derived from the tool point direction with
parameter _VARI.
VARI=0: According to tool point direction
The cycle automatically determines the tool point
direction from the active tool offset. The cycle can then
only work with tool point directions 1 to 4.
If the cycle recognizes a tool point direction 5 ... 9,
alarm 61608 "Wrong tool point direction programmed"
is output and the cycle is aborted.
_VARI=1...4: Definition of undercut position
The cycle determines the starting point automatically.
This lies 2mm from the final diameter and
10mm from the final dimension in the longitudinal axis.
The position of this starting point in relation to the
programmed coordinate values is determined by the
tool point direction of the active tool.
The cycle monitors the clearance angle of the active
tool if a value has been assigned to the relevant
parameter of the tool offset. If the cycle ascertains that
the undercut form cannot be machined with the
selected tool because the clearance angle is too small,
the message "Altered undercut form" appears on the
control, but machining is continued.
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
4.4 Undercut cycle – CYCLE94
+X
For workpieces with
one machined surface
For workpieces with two
machined surfaces at
right angles to each other
SL 4
SL 1
4
Turning Cycles
FORM E
SL3
+Z
FORM F
SL2
+X
SL 3
+Z
SL 2
4-289