HEIDENHAIN CNC PILOT 640 - Circular Pattern on Front Face G745

DIN/ISO programming | Drilling cycles
4
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
385
Circular pattern on front face G745
Cycle G745 is used to machine drilling or milling patterns in which
the individual features are arranged at a regular spacing in a circle
or circular arc on the face.
If the Final point ZE has not been defined, the drilling/milling cycle
of the next NC block is used as a reference
Using this principle, you can combine pattern definitions with:
Drilling cycles (G71, G74, G36)
The milling cycle for a linear slot (G791)
The contour milling cycle with free contour (G793)
Parameters:
XK: Center (Cartesian)
YK: Center (Cartesian)
ZS: Start point of drilling/milling operation
ZE: Final point of drilling/milling operation
X: Diameter – Center (polar)
C: Angle – Center (polar)
K: Diameter – pattern diameter
A: Start angle – position of the first figure (reference: positive X
axis; default: 0°)
W: Final angle – position of the last figure (reference: positive X
axis; default: 360°)
Wi: End angle – Angle increment
Q: Number of holes
V: Rotation dir. (default: 0)
V = 0, without W: Figures are arranged on a full circle
V = 0, with W: Figures are arranged on the longer circular arc
V = 0, with Wi: The algebraic sign of Wi defines the direction
(Wi < 0: clockwise)
V = 1, with W: Clockwise
V = 1, with Wi: Clockwise (algebraic sign of Wi has no effect)
V = 2, with W: Counterclockwise
V = 2, with Wi: Counterclockwise (algebraic sign of Wi has
no effect)
Parameter combinations for defining the center of the pattern and
the pattern positions:
Center point of pattern:
XK, YK
X, C
Pattern positions:
A, W and Q
A, Wi and Q