Example: void areas with OCM cycles

The following NC program shows how to define void areas by using OCM cycles. Two circles from the previous machining operation are used to define void areas in CONTOUR DEF. The tool plunges perpendicularly within the void area.

Program sequence

  • Tool call: drill (diameter: 20 mm)
  • Define Cycle 200
  • Tool call: roughing cutter (diameter: 14 mm)
  • Define CONTOUR DEF with void areas
  • Define Cycle 271
  • Define and call Cycle 272

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

0 BEGIN PGM VOID_1 MM

1 BLK FORM 0.1 Z X+0 Y+0 Z-30

2 BLK FORM 0.2 X+100 Y+100 Z+0

3 TOOL CALL 206 Z S8000 F900

; Tool call (diameter: 20 mm)

4 L Z+100 R0 FMAX M3

5 CYCL DEF 200 DRILLING ~

Q200=+2

;SET-UP CLEARANCE ~

Q201=-30

;DEPTH ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q202=+5

;PLUNGING DEPTH ~

Q210=+0

;DWELL TIME AT TOP ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q211=+0

;DWELL TIME AT DEPTH ~

Q395=+1

;DEPTH REFERENCE

6 L X+30 Y+30 R0 FMAX M99

7 L X+60 Y+60 R0 FMAX M99

8 TOOL CALL 7 Z S7000 F2000

; Tool call (diameter: 14 mm)

9 L Z+100 R0 FMAX M3

10 CONTOUR DEF P1 = LBL 1 V1 = LBL 2 V2 = LBL 3

; Definition of contour and void area

11 CYCL DEF 271 OCM CONTOUR DATA ~

Q203=+0

;SURFACE COORDINATE ~

Q201=-20

;DEPTH ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q260=+100

;CLEARANCE HEIGHT ~

Q578=+0.2

;INSIDE CORNER FACTOR ~

Q569=+0

;OPEN BOUNDARY

12 CYCL DEF 272 OCM ROUGHING ~

Q202=+20

;PLUNGING DEPTH ~

Q370=+0.441

;TOOL PATH OVERLAP ~

Q207=+6000

;FEED RATE MILLING ~

Q568=+0.6

;PLUNGING FACTOR ~

Q253=+750

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q438=-1

;ROUGH-OUT TOOL ~

Q577=+0.2

;APPROACH RADIUS FACTOR ~

Q351=+1

;CLIMB OR UP-CUT ~

Q576=+13626

;SPINDLE SPEED ~

Q579=+1

;PLUNGING FACTOR S ~

Q575=+2

;INFEED STRATEGY

13 CYCL CALL

14 M30

; End of program run

15 LBL 1

; Contour subprogram 1

16 L X+90 Y+50

17 L Y+10

18 RND R10

19 L X+10 Y+15

20 RND R10

21 L Y+75

22 RND R10

23 L X+90 Y+90

24 RND R10

25 L Y+50

26 LBL 0

27 LBL 2

; Void area 1

28 CC X+30 Y+30

29 L X+40 Y+30

30 C X+40 Y+30 DR-

31 LBL 0

32 LBL 3

; Void area 2

33 CC X+60 Y+60

34 L X+70 Y+60

35 C X+70 Y+60 DR-

36 LBL 0

37 END PGM VOID_1 MM