HEIDENHAIN NC 124 - Manual (Page 72)

6 Programming Workpiece Positions
72 TNC 124
Y
X
1 2
3 4
60 30
20
50
0
0
Programming example: Milling a shoulder
The coordinates are programmed in absolute dimensions.
The datum is the workpiece zero.
Corner
1 : X = 0 mm Y = 20 mm
Corner 2 : X = 30 mm Y = 20 mm
Corner 3 : X = 30 mm Y = 50 mm
Corner 4 : X = 60 mm Y = 50 mm
Summary of all programming steps
➤ In the main menu PROGRAMMING AND EDITING go to
Program Manage.
➤ Key in the number of the program you want to work on, and
press ENT.
➤ Enter the nominal positions.
Running a finished program
When a program is finished it can be run in the PROGRAM RUN
mode (see Chapter 10).
Example of entry:Entering a nominal position into a program
(block 11 in this example)
Entering Workpiece Positions
Select the coordinate axis (X axis).
N o m i n a l p o s i t i o n v a l u e ?
3 0
Confirm the entry. The nominal position is now the current block
(between the dashed lines). ENT
Enter the nominal position value, for example 30 mm
and
select tool radius compensation R –.
Program blocks
0 BEGIN PGM 10 MM
Start of program, program number and unit of measurement
1 F 9999
High feed rate for pre-positioning
2 Z+20
Clearance height
3 X–20 R0
Pre-position the tool in the X axis
4 Y–20 R0
Pre-position the tool in the Y axis
5 Z–10
Move tool to milling depth
6 TOOL CALL 1 Z Call the tool, such as tool 1, tool axis Z
7 S 1000
Spindle speed
8 M 3
Spindle ON, clockwise
9 F 200 Machining feed rate
10 Y+20 R+
Y coordinate, corner 1
11 X+30 R–
X coordinate, corner 2
12 Y+50 R+
Y coordinate, corner 3
13 X+60 R+
X coordinate, corner 4
14 F 9999
High feed rate for retracting
15 Z+20
Clearance height
16 M 2
Stop program run, spindle OFF, coolant OFF
17 END PGM 10 MM
End of program, program number and unit of measurement