Example: Open pocket and fine roughing with OCM cycles

The following NC program illustrates the use of OCM cycles. You will program an open pocket that is defined by means of an island and a boundary. Machining includes roughing and finishing of an open pocket.

Program sequence

  • Tool call: Roughing cutter (Ø 20 mm)
  • Program CONTOUR DEF
  • Define Cycle 271
  • Define and call Cycle 272
  • Tool call: Roughing cutter (Ø 8 mm)
  • Define and call Cycle 272
  • Tool call: Finishing cutter (Ø 6 mm)
  • Define and call Cycle 273
  • Define and call Cycle 274

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 OCM_POCKET 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 10 Z S8000 F1500

; Tool call (diameter: 20 mm)

4 L Z+100 R0 FMAX M3

5 CONTOUR DEF P1 = LBL 1 I2 = LBL 2

6 CYCL DEF 271 OCM CONTOUR DATA ~

Q203=+0

;SURFACE COORDINATE ~

Q201=-10

;DEPTH ~

Q368=+0.5

;ALLOWANCE FOR SIDE ~

Q369=+0.5

;ALLOWANCE FOR FLOOR ~

Q260=+100

;CLEARANCE HEIGHT ~

Q578=+0.2

;INSIDE CORNER FACTOR ~

Q569=+1

;OPEN BOUNDARY

7 CYCL DEF 272 OCM ROUGHING ~

Q202=+10

;PLUNGING DEPTH ~

Q370=+0.4

;TOOL PATH OVERLAP ~

Q207=+6500

;FEED RATE MILLING ~

Q568=+0.6

;PLUNGING FACTOR ~

Q253=AUTO

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q438=-0

;ROUGH-OUT TOOL ~

Q577=+0.2

;APPROACH RADIUS FACTOR ~

Q351=+1

;CLIMB OR UP-CUT ~

Q576=+6500

;SPINDLE SPEED ~

Q579=+0.7

;PLUNGING FACTOR S ~

Q575=+0

;INFEED STRATEGY

8 CYCL CALL

; Cycle call

9 TOOL CALL 4 Z S8000 F1500

; Tool call (diameter: 8 mm)

10 L Z+100 R0 FMAX M3

11 CYCL DEF 272 OCM ROUGHING ~

Q202=+10

;PLUNGING DEPTH ~

Q370=+0.4

;TOOL PATH OVERLAP ~

Q207=+6000

;FEED RATE MILLING ~

Q568=+0.6

;PLUNGING FACTOR ~

Q253=AUTO

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q438=+10

;ROUGH-OUT TOOL ~

Q577=+0.2

;APPROACH RADIUS FACTOR ~

Q351=+1

;CLIMB OR UP-CUT ~

Q576=+10000

;SPINDLE SPEED ~

Q579=+0.7

;PLUNGING FACTOR S ~

Q575=+0

;INFEED STRATEGY

12 CYCL CALL

; Cycle call

13 TOOL CALL 23 Z S10000 F2000

; Tool call (diameter: 6 mm)

14 L Z+100 R0 FMAX M3

15 CYCL DEF 273 OCM FINISHING FLOOR ~

Q370=+0.8

;TOOL PATH OVERLAP ~

Q385=AUTO

;FINISHING FEED RATE ~

Q568=+0.3

;PLUNGING FACTOR ~

Q253=+750

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q438=-1

;ROUGH-OUT TOOL ~

Q595=+1

;STRATEGY ~

Q577=+0.2

;APPROACH RADIUS FACTOR

16 CYCL CALL

; Cycle call

17 CYCL DEF 274 OCM FINISHING SIDE ~

Q338=+0

;INFEED FOR FINISHING ~

Q385=AUTO

;FINISHING FEED RATE ~

Q253=+750

;F PRE-POSITIONING ~

Q200=+2

;SET-UP CLEARANCE ~

Q14=+0

;ALLOWANCE FOR SIDE ~

Q438=-1

;ROUGH-OUT TOOL ~

Q351=+1

;CLIMB OR UP-CUT

18 CYCL CALL

; Cycle call

19 M30

; End of program run

20 LBL 1

; Contour subprogram 1

21 L X+0 Y+0

22 L X+100

23 L Y+100

24 L X+0

25 L Y+0

26 LBL 0

27 LBL 2

; Contour subprogram 2

28 L X+0 Y+0

29 L X+100

30 L Y+100

31 L X+70

32 L Y+70

33 RND R5

34 L X+30

35 RND R5

36 L Y+100

37 L X+0

38 L Y+0

39 LBL 0

40 END PGM OCM_POCKET MM