Siemens SINUMERIK 840D Manual page 65

Key functions for 5-axis machining
CYCLE832 parameters
Machining Finishing (default)
Pre-finishing
Roughing
Deselection
Tolerance_tol. Chord tolerance
(chord tolerance
should be taken from
the CAM system or
weighted with a factor
of 1.0 to 1.5)
Transformation TRAORI
TRAORI(2)
No
(default)
Adaptation Yes
No (default)
Compression COMPOF (default)
COMPCAD
COMPCURV
B SPLINE
Path control G642 (default)
G641
G64
Feedforward FFWOF SOFT
control (default)
FFWON-SOFT
FFWOF-BRISK
© Siemens AG All rights reserved. SINUMERIK, Manual, 5-axis machining
Calling "Deselection" resets the modified
machine/setting data to the value generated by
the machine manufacturer.
Tolerance of linear/rotary axes, default settings:
→ 0.01 mm/ 0.08° (finishing)
→ 0.05 mm/ 0.4° (pre-finishing)
→ 0.1 mm/ 0.8° (roughing)
→ 0.1 mm/ 0.1° (deselection)
→ Activate 5-axis transformation
→ Activate machine-manufacturer-specific 5-
axis transformation (optional)
→ Deactivate transformation. CAM programs
with resolved rotary axis positions are sup-
ported.
→ Subsequent fields can be modified
→ Subsequent fields are not visible.
Activated by machine manufacturer
→ Compressor off
→ Compressor on, constant acceleration rate
for free-form surfaces
→ Jerk-free for circumferential milling
→ Spline interpolation
→ Smoothing with single-axis tolerances
→ Programmable smoothing distance
→ Continuous-path mode
In the case of an NC block compressor with
COMPCAD, G642 is permanently selected.
→ Without feedforward control, with jerk limita-
tion
→ With feedforward control, with jerk limitation
→ Without feedforward control, without jerk lim-
itation
In order for feedforward control (FFWON) and
jerk limitation (SOFT) to be selected, the
machine manufacturer must have optimized the
control or the machining axes.
3.6
65