HEIDENHAIN NC 124 - Manual (Page 87)

7 Drilling, Milling Cycles and Hole Patterns in Programs
TNC 124 87
Hole Patterns in Programs
Program blocks
0 BEGIN PGM 40 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 TOOL CALL 3 Z
Call the tool for drilling, for example tool 3, tool axis Z
4 S 100
Spindle speed
5 M 3
Spindle ON, clockwise
6 CYCL 1.0 PECKING
Cycle data for Cycle 1.0 PECKING follow
7 CYCL 1.1 HEIGHT +50
Clearance height
8 CYCL 1.2 DIST 2
Setup clearance above the workpiece surface
9 CYCL 1.3 SURF + 0
Absolute coordinate of the workpiece surface
10 CYCL 1.4 DEPTH –15
Hole depth
11 CYCL 1.5 PECKG 5
Depth per infeed
12 CYCL 1.6 DWELL 0.5
Dwell time at bottom of hole
13 CYCL 1.7 F 80
Machining feed rate
14 CYCL 5.0 FULL CIRCLE
Cycle data for Cycle 5.0 FULL CIRCLE follow
15 CYCL 5.1 NO. 8
Number of holes
16 CYCL 5.2 CCX +50
X coordinate of the center of the bolt circle
17 CYCL 5.3 CCY +50
Y coordinate of the center of the bolt circle
18 CYCL 5.4 RAD 20
Radius
19 CYCL 5.5 START +30
Starting angle of first hole
20 CYCL 5.6 TYPE 1:PECK
Drill bore holes
21 M 2
Stop program run, spindle STOP, coolant OFF
22 END PGM 40 MM
End of program, program number, unit of measurement
For a circle segment (CYCL 6.0 CIRCLE SEGMENT)
you also enter the angle step (STEP) between the holes
(after the starting angle).
The bolt hole circle is then executed in the operating mode
PROGRAM RUN
(see Chapter 10).