4.36 G Codes From Previous Controls; Fundamentals; Undercut G25 - Contour Definitions In The Machining Section - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | G codes from previous controls

4.36 G codes from previous controls

Fundamentals

The commands described in the following are supported to enable
you to use NC programs from previous controls. HEIDENHAIN
recommends no longer using these commands with new NC
programs.
Undercut G25 – contour definitions in the machining
section
G25 generates an undercut form element (DIN 509 E, DIN 509 F,
DIN 76) that can then be integrated in roughing or finishing cycles.
The help graphic illustrates the undercut parameters.
Parameters:
H: Cut type (default: 0)
0 or 5: DIN 509 E
6: DIN 509 F
7: DIN 76
I: Undercut depth (default: standard table)
K: Undercut width (default: standard table)
R: Undercut radius (default: standard table)
P: Trav.dpth (default: value from standard table)
W: Undercut angle (default: standard table)
A: Face angle (default: standard table)
FP: Thread pitch (no input: FP is calculated from the thread
diameter)
U: Grind. overs. (default: 0)
E: Reduc. Feed for machining the undercut (default: active feed
rate)
If the parameters are not defined, the control determines the
following values from the diameter or the thread pitch in the
standard table:
DIN 509 E: I, K, W, R
DIN 509 F: I, K, W, R, P, A
DIN 76: I, K, W, R (determined from the Thread pitch)
All parameters that you enter will be accounted for—
even if the standard table prescribes other values.
If you are programming an internal thread, it is
advisable to preset the Thread pitch FP since the
diameter of the longitudinal element is not the
thread diameter. If you have the control calculate the
Thread pitch automatically, slight deviations may
occur.
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
497