HEIDENHAIN iTNC 530 (606 42x-01) ISO programming - Manual (Page 317)

HEIDENHAIN iTNC 530 317
1
0
.4 Miscellaneous F
unctions f
o
r Cont
our
ing Beha
vior
Superimposing handwheel positioning during
program run: M118
Standard behavior
In the program run modes, the TNC moves the tool as defined in the
part program.
Behavior with M118
M118 permits manual corrections by handwheel during program run.
Just program M118 and enter an axis-specific value (linear or rotary
axis) in millimeters.
Input
If you enter M118 in a positioning block, the TNC continues the dialog
for this block by asking you the axis-specific values. The coordinates
are entered with the orange axis direction buttons or the ASCII
keyboard.
Effect
Cancel handwheel positioning by programming M118 once again
without coordinate input.
M118 becomes effective at the start of block.
Example NC blocks
You want to be able to use the handwheel during program run to move
the tool in the working plane X/Y by ±1 mm and in the rotary axis B by
±5° from the programmed value:
N250 G01 G41 X+0 Y+38.5 F125 M118 X1 Y1 B5 *
M118 is always effective in the original coordinate system,
even if the working plane is tilted.
In a program with millimeters set as unit of measure, the
TNC interprets M118 values for linear axes in millimeters.
In an inch program it interprets it as inches.
M118 also functions in the Positioning with MDI mode of
operation!
M118 in combination with DCM collision monitoring is
only possible in stopped condition (blinking control-in-
operation symbol). If you try to move an axis during
handwheel superimposition, the TNC will generate an
error message.