Siemens SINUMERIK 840DE Operation & Programming Manual page 85

5
08.02
(alternative)
AS
E
U
V
Q
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/810D Operator's Guide ManualTurn (BAM) – 08.02 Edition
5.2 Turning cycles in CYCLE mode
Parameter α α α α is set to determine the angle of infeed in the thread. If
you require an angle of infeed of 90° to the cutting direction, then this
parameter must be set to zero. If infeed is to take place along the
flanks, then the value of this parameter may not exceed half the flank
angle of the tool.
Infeed along flank
Infeed along alternating flanks
You can infeed along alternate edges instead of just one edge to avoid
loading the same tool cutting edge every time. That increases tool life.
α α α α > 0: Start at rear flank
α α α α < 0: Start at front flank
Number of roughing cuts or first infeed (mm)
When changing between the number of roughing cuts and the first
feed, the associated value is displayed respectively.
Insertion depth (enter without sign)
E is the depth already reached in the previous machining operation,
i.e. the insertion depth only has to be entered if thread finishing is
intended.
Finishing allowance (enter without sign)
The programmed finishing allowance U is subtracted from the
specified thread depth K , the remainder being divided up into the
number of roughing cuts. The cycle automatically calculates the
individual, current infeed depths as a function of the programmed cut
segmentation.
When the thread depth to be machined is divided into infeeds with
constant cut cross-section, all roughing cuts are made with the same
cutting pressure. The tool is then fed in at different infeed depths.
A second possible variant is to divide the total thread depth into
constant infeed depths. In this case, the cut cross-section increases
with every cut, but this technology results in improved cutting
conditions for low thread depth values.
The finishing allowance U is removed in one cut after the roughing
process.
Return distance (enter without sign)
Angular offset for single-turn threads (–360°<Q<360°)
With this parameter you can program the angular value that
determines the point at which the thread starts on the circumference
of the part.
e.g. Q = 30.0
The thread start point is at 30°.
5
Turning with Cycles
5-85