HEIDENHAIN TNC 620 User Manual page 64

1
First Steps with the TNC 620
1.3 Programming the first part
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 TNC saves the entered positioning block
Press the L key to open a program block for a
linear movement
Enter the coordinates of the contour starting point
in X and Y, e.g. 5/5. Confirm with the ENT key
1
Activate radius compensation to the left of the
path: Press the G41 soft key
Feed rate F=? Enter the machining feed rate, e.g.
700 mm/min, save your entry with the END key
Enter 26 to approach the contour: Define
Rounding-off radius? for the circular arc, save
entries with the END key
Machine the contour and move to contour
point 2: You only need to enter the information
that changes. In other words, enter only the Y
coordinate 95 and save your entry with the END
key
Move to contour point 3: Enter the X coordinate 95
and save your entry with the END key
Define chamfer G24 on contour point 3: Chamfer
side length? Enter 10 mm, save with the END key
Move to contour point 4: Enter the Y coordinate 5
and save your entry with the END key
Define chamfer G24 on contour point 4: Chamfer
side length? Enter 20 mm, save with the END key
Move to contour point 1: Enter the X coordinate 5
and save your entry with the END key
Enter 27 to depart from the contour: Define the
Rounding-off radius? of the departing arc
Depart contour: Enter coordinates outside of the
workpiece in X and Y, e.g. -20/-20, confirm with
the ENT key
Activate no radius compensation: Press the G40
soft key
Press the L key to open a program block for a
linear movement
Press the G00 soft key if you want to enter a rapid
traverse motion
Retract tool: Press the orange axis key Z to retract
in the tool axis, 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? Enter M2 to end
the program and confirm with the END key: The
TNC saves the entered positioning block
64
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016