Teach-in | Thread and undercut cycles
5
334
HEIDENHAIN | MANUALplus 620 | User's Manual | 12/2017
Undercut DIN 76
Select Thread cutting
Undercut DIN 76
Select the scope of the cycle:
Off: When the cycle is completed, the tool
remains at the cycle end position
On: The tool returns to the starting point
The cycle machines an Undercut DIN 76, a thread chamfer, then
the cylinder, and finishes with the plane surface. The thread
chamfer is executed when you enter at least one of the parameters
Cylinder 1st cut length or Cut-in radius.
Cycle parameters:
X, Z: Start point
X1, Z1: Start point cylinder
X2, Z2: End point transv.
FP: Thread pitch (default: standard table)
E: Reduced feed for the plunge cut and the thread chamfer
(default: Feed per revolution F)
I: Undercut depth (default: standard table)
K: Undercut length (default: standard table)
W: Undercut angle (default: standard table)
R: Undercut radius on both sides of the undercut (default: value
from standard table)
P1: Undercut oversize
No input: Machining in one cut
P1 > 0: Division into pre-turning and finish-turning. P1 is
longitudinal oversize; the transverse oversize is preset to 0.1
mm
T: Tool number – turret pocket number
G14: Tool change point
Further information: "Tool change point G14", Page 180
ID: ID no.
S: Cutting speed or Constant speed
F: Feed per revolution
B: Cylinder 1st cut length (default: no start chamfer)
WB: Cut-in angle (default: 45°)
RB: Cut-in radius (no input: no element, positive value: first cut
radius, negative value: chamfer)
G47: Safety clearance
Further information: "Safety clearance G47", Page 180 —
evaluated only if "With return" is active
MT: M after T: M function that is executed after the tool call T
MFS: M at beginning: M function that is executed at the
beginning of the machining step
MFE: M at end: M function that is executed at the end of the
machining step
To Next Page
Loading...
Need help?
General
