HEIDENHAIN TNC 640 User Manual page 76

1
First Steps with the TNC 640 | Programming the first part
Press the approach function soft key APPR CT:
Enter the coordinates of the contour starting
in X and Y, e.g. 5/5, confirm with the ENT
point 1
key
Center angle? Enter the approach angle, e.g.
90°, confirm with the ENT key
Circle radius? Enter the circular radius, e.g.
8 mm, confirm with the ENT key
Confirm Tool radius comp: RL/RR/no comp?
with the RL soft key: Activate the radius
compensation to the left of the programmed
contour
Feed rate F=? Enter the machining feed rate,
e.g. 700 mm/min, save your entry 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 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 the chamfer at contour point 3: Enter the
chamfer width 10 mm and save with the END key
Move to contour point 4: Enter the Y coordinate
5 and save your entry with the END key
Define the chamfer at contour point 4: Enter the
chamfer width 20 mm and save with the END
key
Move to contour point 1: Enter the X coordinate
5 and save your entry with the END key
Depart contour: Press the APPR DEP key
Departure function: Press the DEP CT soft key
Center angle? Enter the departure angle, e.g.
90°, confirm with the ENT key
Circle radius? Enter the departure radius, e.g.
8 mm, confirm with the ENT key
Feed rate F=? Enter the positioning feed rate,
e.g. 3000 mm/min, confirm with the ENT key
Miscellaneous function M? Switch off the
coolant, e.g. M9, and confirm with the END key
The control stores the entered positioning block.
76
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017