HEIDENHAIN TNC 620 E, User Manual

Page: 158 / 840

Fundamentals, File Management | Creating and writing programs
4
158
HEIDENHAIN | TNC 620 | Conversational Programming User's Manual | 10/2017
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
Z
Enter the spindle axis, e.g.
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
Program begin, name, unit of measure
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
Spindle axis, MIN point coordinates
2 BLK FORM 0.2 X+100 Y+100 Z+0
MAX point coordinates
3 END PGM NEW MM
Program end, name, unit of measure
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.