Example: Button tool for turning

The following NC program uses Cycle 800 ADJUST XZ SYSTEM and Cycle 815 CONTOUR-PAR. TURNING.

Program sequence

  • Call the tool (e.g., TURN_BUTTON_R5)
  • Activate turning mode
  • Pre-position
  • Cycle 800 ADJUST XZ SYSTEM
  • Select the contours by using SEL CONTOUR
  • Cycle 815 CONTOUR-PAR. TURNING
  • Call the cycle
  • End of program

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 TURNING_BUTTON MM

1 BLK FORM CYLINDER Z D100 L100 DIST+0

2 CALL LBL "RESET"

3 FUNCTION MODE TURN

; Activate turning mode

4 TOOL CALL "TURN_BUTTON_R5"

; Tool call

5 CYCL DEF 800 ADJUST XZ SYSTEM ~

Q497=+0

;PRECESSION ANGLE ~

Q498=+0

;REVERSE TOOL ~

Q530=+2

;INCLINED MACHINING ~

Q531=+30

;ANGLE OF INCIDENCE ~

Q532=MAX

;FEED RATE ~

Q533=-1

;PREFERRED DIRECTION ~

Q535=+3

;ECCENTRIC TURNING ~

Q536=+0

;ECCENTRIC W/O STOP

6 FUNCTION TURNDATA BLANK LBL "BLANK"

7 FUNCTION TURNDATA SPIN VCONST: ON VC:400 SMAX800

; Constant surface speed

8 FUNCTION TURNDATA CORR-WPL:Z/X DZL:+0 DXL:+0

9 L X+102 Y+0 R0 FMAX

10 L Z+2 R0 FMAX M303

11 SEL CONTOUR LBL 1

; Define the contour

12 CYCL DEF 815 CONTOUR-PAR. TURNING ~

Q215=+0

;MACHINING OPERATION ~

Q460=+2

;SAFETY CLEARANCE ~

Q485=+0

;ALLOWANCE ON BLANK ~

Q486=+1

;INTERSECTING LINES ~

Q499=+0

;REVERSE CONTOUR ~

Q463=+3

;MAX. CUTTING DEPTH ~

Q478=+0.3

;ROUGHING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q484=+0.2

;OVERSIZE IN Z ~

Q505=+0.2

;FINISHING FEED RATE

13 CYCL CALL

; Cycle call

14 M305

15 CYCL DEF 801 RESET ROTARY COORDINATE SYSTEM

16 FUNCTION MODE MILL

; Activate milling mode

17 CALL LBL "RESET"

18 ;

19 M30

; End of program run

20 LBL "BLANK"

; Define LBL BLANK

21 L X+0 Z+0

22 L X+100

23 L Z-100

24 L X+0

25 L Z+0

26 LBL 0

27 LBL 1

; Define contour with LBL 1

28 L X+0 Z+0

29 L X+60

30 RND R30

31 L Z-65

32 RND R10

33 L X+95

34 RND R1

35 L Z-70

36 LBL 0

37 LBL "RESET"

; Define LBL RESET

38 FUNCTION RESET TCPM

39 TRANS DATUM RESET

40 PLANE RESET TURN FMAX

41 LBL 0

42 END PGM TURNING_BUTTON MM