HEIDENHAIN CNC PILOT 640 - Defining the Tool Change Pointg140; Tool Change Point G14

DIN/ISO programming | Tool positioning
4
292
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
Tool change point G14
G14 moves the slide at rapid traverse to the Tool change point.
In setup mode, define permanent coordinates for the tool change
position.
Parameters:
Q: Order (default: 0)
0: Simultaneously
1: First X, then Z
2: First Y, then Z, then X
3: Only X
4: Only Z
5: Only Y (machine-dependent)
6: Simultaneous w/ Y (machine-dependent)
D: Number: of the tool change position to be approached 0-2
(default: 0 = tool change position from parameters)
Example: G14
. . .
N1 G14 Q0
Move to the tool change position
N2 T3 G95 F0.25 G96 S200 M3
N3 G0 X0 Z2
. . .
Defining the Tool change pointG140
G140 defines the position of the Tool change point defined in D.
This position can be approached with G14.
Parameters:
D: Number: of the tool change point 1-2
X: Diameter – position of the tool change point
Z: Target point – position of the tool change point
If X or Z parameters are missing, the values from the
tool change point parameter are entered.
Example: G140
. . .
N1 G14 Q0
Tool change position from parameter
N2 T3 G95 F0.25 G96 S200 M3
N3 G0 X40 Z10
N5 G140 D1 X100 Z100
Set tool change pos.1
N6 G14 Q0 D1
Move to tool change pos. 1
N7 G140 D2 X150
Set tool change pos. 2, use Z from parameters
N8 G14 Q0 D2
Move to tool change pos. 2
. . .