Siemens sinumerik 808d Programming And Operating Manual page 184

Cycles
2.5 Turning cycles
A second version is the distribution of the whole thread depth to constant infeed depths.
When doing so, the cutting cross-section becomes larger from cut to cut, but with smaller
values for the thread depth, this technology can result in better cutting conditions.
The finishing allowance FAL is removed after roughing in one step. Then the idle passes
programmed under parameter NID are executed.
IANG (infeed angle)
By using parameter IANG, the angle is defined under which the infeed is carried out in the
thread. If you wish to infeed at a right angle to the cutting direction in the thread, the value of
this parameter must be set to zero. This means that the parameter can be omitted in the
parameter list, as in this case the value is defaulted automatically with zero. If you wish to
infeed along the flanks, the absolute value of this parameter may amount maximally to the
half of the flank angle of the tool.
The execution of the infeed is defined by the sign of this parameter. With a positive value,
infeed is always carried out at the same flank, and with a negative value, at both flanks
alternating. The infeed type with alternating flanks is only possible for cylindrical threads. If
the value of IANG for tapered threads is nonetheless negative, the cycle will carry out a flank
infeed along a flank.
NSP (starting point offset)
You can use this parameter to program the angle value defining the point of the first cut of
the thread turn at the circumference of the turned part. This involves a starting point offset.
The parameter can assume values between 0.0001 and +359.9999 degrees. If no starting
point offset has been specified or the parameter has been omitted from the parameter list,
the first thread turn automatically starts at the zero-degree mark.
PP1, PP2 and PP3 (thread lead)
These parameters are used to define the value of the thread lead in the three sections of the
thread series. The lead value must be entered as a paraxial value without sign.
VARI (machining type)
By using the VARI parameter, it is defined whether external or internal machining will be
carried out and which technology will be used with regard to the infeed when roughing. The
VARI parameter can assume values between 1 and 4 with the following meaning:
184
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0