Programming A Simple Contour - HEIDENHAIN TNC 320 User Manual

Programming a simple contour

The contour shown to the right is to be milled once to a depth of
5 mm You have already defined the workpiece blank. After you
have initiated a dialog through a function key, enter all the data
requested by the TNC in the screen header.
Call the tool: Enter the tool data. Confirm the entry
in each case with the ENT key, and do not forget
the Z tool axis
Retracting tool: Press the orange axis key Z and
enter the value for the position to be approached,
e.g. 250. Press the ENT key
Tool radius comp: RL/RR/no comp? confirm with
the ENT key: Do not activate radius compensation
Vorschub F=? confirm with the ENT key: Rapid
traverse (FMAX)
Enter Miscellaneous function M? and confirm with
the END key: The TNC saves the input positioning
block
Preposition the tool in the working plane: Press
the orange X axis key and enter the value for the
position to be approached, e.g. -20
Press the orange axis key Y and enter the value for
the position to be approached, e.g. -20. Press the
ENT key
Tool radius comp: RL/RR/no comp? confirm with
the ENT key: Do not activate radius compensation
Vorschub F=? confirm with the ENT key: Rapid
traverse (FMAX)
Confirm Miscellaneous function M? with the END
key: The TNC saves the input positioning block
Move tool to working depth: Press the orange axis
key Z and enter the value for the position to be
approached, e.g. -5. Press the ENT key
Tool radius comp: RL/RR/no comp? confirm with
the ENT key: Do not activate radius compensation
Feed rate F=? Enter the positioning feed rate, e.g.
3000 mm/min, confirm with the ENT key
Miscellaneous function M? Switch on the spindle
and coolant, e.g. M13, confirm with the END key:
The TNC saves the entered positioning block
Move to the contour: Press the APPR/DEP key:
The TNC shows a soft-key row with approach and
departure functions
HEIDENHAIN | TNC 320 | Conversational Programming User's Manual | 9/2016
Programming the first part
1
1.3
59