Creating A Cycle Program - HEIDENHAIN TNC 640 User Manual

1

Creating a cycle program

The holes (depth of 20 mm) shown in the figure at right are to be
drilled with a standard drilling cycle. You have already defined the
workpiece blank.
Call the tool: Enter the tool data. Confirm the
entry in each case with the ENT key, do not
forget the tool axis
Press the L key to open an NC block for a linear
movement
Press the left arrow key to switch to the input
range for G codes
Press the G00 soft key if you want to enter a
rapid traverse motion
Press the G90 soft key for absolute values
Retract tool: Press the orange axis key Z and
enter the value for the position to be approached,
e.g. 250. Press the ENT key
Activate no radius compensation: Press the G40
soft key
Miscellaneous function M? Switch on the
spindle and coolant, e.g. M13. Confirm with the
END key
The control stores the entered positioning block.
Call the cycle menu: Press the CYCL DEF key
Display the drilling cycles
Select standard drilling cycle 200
The control starts the dialog for cycle definition.
Enter all parameters requested by the control
step by step and conclude each entry with the
ENT key
In the screen to the right, the control also
displays a graphic showing the respective cycle
parameter
Enter 0 to approach the first drilling position:
Enter the coordinates of the drilling position, call
the cycle with M99
Enter 0 to move to further drilling positions:
Enter the coordinates of the specific drilling
positions, and call the cycle with M99
Enter 0 to retract the tool: Press the orange axis
key Z and enter the value for the position to be
approached, e.g. 250. Press the ENT key
Miscellaneous function M? Enter M2 to end the
program, then confirm with the END key
The control stores the entered positioning block.
76
First Steps with the TNC 640 | Programming the first part
HEIDENHAIN | TNC 640 | ISO Programming User's Manual | 10/2017