Example: Face milling and fine roughing with OCM cycles

The following NC program illustrates the use of OCM cycles. You will face-mill a surface which will be defined by means of a boundary and an island. In addition, you will mill a pocket that contains an allowance for a smaller roughing tool.

Program sequence

  • Tool call: Roughing cutter (Ø 12 mm)
  • Program CONTOUR DEF
  • Define Cycle 271
  • Define and call Cycle 272
  • Tool call: Roughing cutter (Ø 8 mm)
  • Define Cycle 272 and call it again

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 FACE_MILL MM

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

2 BLK FORM 0.2 X+100 Y+50 Z+2

3 TOOL CALL 6 Z S5000 F3000

; Tool call (diameter: 12 mm)

4 L Z+100 R0 FMAX M3

5 CONTOUR DEF P1 = LBL 1 I2 = LBL 1 DEPTH2 P3 = LBL 2

6 CYCL DEF 271 OCM CONTOUR DATA ~

Q203=+2

;SURFACE COORDINATE ~

Q201=-22

;DEPTH ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q260=+100

;CLEARANCE HEIGHT ~

Q578=+0.2

;INSIDE CORNER FACTOR ~

Q569=+1

;OPEN BOUNDARY

7 CYCL DEF 272 OCM ROUGHING ~

Q202=+24

;PLUNGING DEPTH ~

Q370=+0.4

;TOOL PATH OVERLAP ~

Q207=+8000

;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=+8000

;SPINDLE SPEED ~

Q579=+0.7

;PLUNGING FACTOR S ~

Q575=+1

;INFEED STRATEGY

8 L X+0 Y+0 R0 FMAX M99

; Cycle call

9 TOOL CALL 4 Z S6000 F4000

; Tool call (diameter: 8 mm)

10 L Z+100 R0 FMAX M3

11 CYCL DEF 272 OCM ROUGHING ~

Q202=+25

;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=+6

;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=+1

;INFEED STRATEGY

12 L X+0 Y+0 R0 FMAX M99

; Cycle call

13 M30

; End of program run

14 LBL 1

; Contour subprogram 1

15 L X+0 Y+0

16 L Y+50

17 L X+100

18 L Y+0

19 L X+0

20 LBL 0

21 LBL 2

; Contour subprogram 2

22 L X+10 Y+30

23 L Y+40

24 RND R5

25 L X+60

26 RND R5

27 L Y+20

28 RND R5

29 L X+10

30 RND R5

31 L Y+30

32 LBL 0

33 END PGM FACE_MILL MM