Creating A New Nc Program - HEIDENHAIN TNC 620 User Manual

4

Creating a new NC program

You always enter an NC program in Programming mode. An
example of program initiation:
Operating mode: Press the Programming key
Press the PGM MGT key
The control opens the file manager.
Select the directory in which you wish to store the new NC
program:
FILE NAME = NEW.H
Enter the new program name
Press the ENT key
Select the unit of measure: Press the MM or
INCH soft key
The control switches the screen layout and
initiates the dialog for defining the BLK FORM
(workpiece blank).
Select a rectangular workpiece blank: Press the
soft key for a rectangular blank form
Working plane in graphic: XY
Enter the spindle axis, e.g. Z
Z
Workpiece blank def.: Minimum
Enter in sequence the X, Y and Z coordinates of
the MIN point and confirm each of your entries
with the ENT key
Workpiece blank def.: Maximum
Enter in sequence the X, Y and Z coordinates of
the MAX point and confirm each of your entries
with the ENT key
Example
0 BEGIN PGM NEW MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 END PGM NEW MM
The control automatically generates the block numbers as well as
the BEGIN and END blocks.
If you do not wish to define a blank form, cancel the
dialog at Working plane in graphic: XY using the DEL
key.
158
Fundamentals, File Management | Creating and writing programs
Program begin, name, unit of measure
Spindle axis, MIN point coordinates
MAX point coordinates
Program end, name, unit of measure
HEIDENHAIN | TNC 620 | Conversational Programming User's Manual | 10/2017