HEIDENHAIN CNC Pilot 4290 - Manual (Page 145)

HEIDENHAIN CNC PILOT 4290 133
4.7 T
u
rning Cy
cles
– Equidistant around the barrier
– Omission of the first contour element if the start position is
inaccessible
■ Q=1: First X, then Z direction
■ Q=2: First Z, then X direction
■ Q=3: No approach—tool is in the proximity of the starting
point
■ Q=4: Residual finishing
H: Retraction—default: 3
Tool lifts off under 45° in the opposite direction to machining
and moves as follows to the position “I, K“:
■ H=0: Diagonal
■ H=1: First X, then Z direction
■ H=2: First Z, then X direction
■ H=3: Remains at safety clearance
■ H=4: No retraction movement—tool remains at the end
coordinate
Z: Cutting limit (diameter)—default: no cutting limit
Z: Cutting limit—default: no cutting limit
D: Omit element (influences the machining of undercuts, relief
turns, and recessing: see table)—default: 1
I, K: End point that is appropriate at the end of the cycle (I diameter
value)
O: Feed rate reduction—default: 0
■ O=0: No feed rate reduction
■ O=1: Feed rate reduction active
Undercuts/undercut combinations can be omitted as follows:
D G22 G23 G23 G25 G25 G25
= H0 H1 H4 H5/6 H7..9 K
0 • • • • • •
1 • • – • – –
2 • • – • • •
3 • • • • – –
4 • • – • • –
5 • • – • – –
6 • • – • – •
7 – – – – – –
“•”: Skip elements
Other D codes for skipping undercuts/recesses.
Add the codes if you want to skip several
undercuts/recesses:
G call Function D code
G22 Recess for sealing ring 512
G22 Recess for guard ring 1.024
G23 H0 General recess 256
G23 H1 Relief turn 2.048
G23 H4 Undercut type U 32.768
G23 H5 Undercut type E 65.536
G23 H6 Undercut type F 131.072
G23 H7 Undercut type G 262.144
G23 H8 Undercut type H 524.288
G23 H9 Undercut type K 1.048.576
Cutting limitation: The tool position
before the cycle call determines the
effect of a cutting limit. The CNC PILOT
machines the area to the right or to the
left of the cutting limit, depending on
which side the tool has been positioned
before the cycle is called.
G57 oversize: “enlarge” the contour
(also inside contours)
G58 oversize:
■ >0: “enlarges” the contour
■ <0: “reduces” the contour
G57/G58 oversizes are deleted after
cycle end