HEIDENHAIN NC 124 - Manual (Page 93)

7 Drilling, Milling Cycles and Hole Patterns in Programs
TNC 124 93
Cycle 4.0 RECTANGULAR POCKET is executed in the operating mode
PROGRAM RUN
(see Chapter 10).
Program blocks
0 BEGIN PGM 55 MM
Start of program, program number, unit of measurement
1 F 9999
High feed rate for pre-positioning
2 Z+600
Tool-change position
3 X-100
Pre-positioning in the X axis
4 Y-100
Pre-positioning in the Y axis
5 TOOL CALL 7 Z
Call the tool for pocket milling, such as tool 7, tool axis Z
6 S 800
Spindle speed
7 M 3
Spindle ON, clockwise
8 CYCL 4.0 RECTANGULAR
POCKET
Cycle data for Cycle 4.0 RECTANGULAR POCKET follow
9 CYCL 4.1 HEIGHT + 80
Clearance height
10 CYCL 4.2 DIST 2
Setup clearance above the workpiece surface
11 CYCL 4.3 SURF + 0
Absolute coordinate of the workpiece surface
12 CYCL 4.4 DEPTH – 20
Milling depth
13 CYCL 4.5 PECKG 7
Depth per infeed
14 CYCL 4.6 F 80
Pecking feed rate
15 CYCL 4.7 POSX + 50
Pocket center in X
16 CYCL 4.8 POSY + 40
Pocket center in Y
17 CYCL 4.9 LNGTHX 80
Side length X
18 CYCL 4.10 LNGTHY 60
Side length Y
19 CYCL 4.11 F 100
Milling feed rate
20 CYCL 4.12 DIRCTN 0: CLIMB
Climb milling
21 CYCL 4.13 ALLOW 0.5
Finishing allowance
22 M 2
Stop program run, spindle STOP, coolant OFF
23 END PGM 55 MM
End of program, program number, unit of measurement
Rectangular Pockets in Programs