Opening A New Part Program - HEIDENHAIN TNC 620 User Manual

3
Programming: Fundamentals, file management
3.2 Opening programs and entering

Opening a new part program

You always enter a part program in the PROGRAMMING AND
EDITING mode of operation. An example of program initiation:
Select the PROGRAMMING mode of operation
Call the file manager: Press the PGM MGT key
Select the directory in which you wish to store the new program:
FILE NAME = ALT.H
Enter the new program name and confirm your
entry with the ENT key.
Select the unit of measure: Press the MM or INCH
soft key. The TNC switches the screen layout and
initiates the dialog for defining the BLK FORM
(workpiece blank)
WORKING PLANE IN GRAPHIC: XY
Enter 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: Display the BLK form in the NC program
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 TNC 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 by pressing
the DEL key.
The TNC can display the graphics only if the shortest
side is at least 50 µm long and the longest side is no
longer than 99 999.999 mm.
90
Program begin, name, unit of measure
Spindle axis, MIN point coordinates
MAX point coordinates
Program end, name, unit of measure
HEIDENHAIN Conversational Programming | 5/2013
TNC 620 | User's Manual