Example: Simultaneous turning

The following NC program uses Cycle 882 SIMULTANEOUS ROUGHING FOR TURNING and Cycle 883 TURNING SIMULTANEOUS FINISHING.

Program sequence

  • Call the tool (e.g., TURN_ROUGH)
  • Activate turning mode
  • Pre-position
  • Select the contours by using SEL CONTOUR
  • Cycle 882 SIMULTANEOUS ROUGHING FOR TURNING
  • Call the cycle
  • Call the tool (e.g., TURN_FINISH)
  • Activate turning mode
  • Cycle 883 TURNING SIMULTANEOUS FINISHING
  • 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 1341941_1 MM

1 BLK FORM ROTATION Z DIM_D FILE "1341941_blank.H"

2 FUNCTION MODE TURN

; Activate turning mode

3 TOOL CALL "TURN_ROUGH"

; Tool call

4 CYCL DEF 800 ADJUST XZ SYSTEM ~

Q497=+0

;PRECESSION ANGLE ~

Q498=+0

;REVERSE TOOL ~

Q530=+2

;INCLINED MACHINING ~

Q531=+1

;ANGLE OF INCIDENCE ~

Q532=MAX

;FEED RATE ~

Q533=-1

;PREFERRED DIRECTION ~

Q535=+3

;ECCENTRIC TURNING ~

Q536=+0

;ECCENTRIC W/O STOP ~

Q599=+0

;RETRACT

5 FUNCTION TURNDATA SPIN VCONST: ON VC:400 SMAX800

; Constant surface speed

6 M145

; Reset the tool offset

7 FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS REFPNT TIP-CENTER

; Activate TCPM

8 L X+120 Y+0 R0 FMAX

; Pre-position

9 L Z+20 R0 FMAX M303

10 FUNCTION TURNDATA BLANK "1341941_blank.H"

; Workpiece blank update

11 SEL CONTOUR "1341941_finish.h"

; Define the contour

12 CYCL DEF 882 SIMULTANEOUS ROUGHING FOR TURNING ~

Q460=+2

;SAFETY CLEARANCE ~

Q499=+0

;REVERSE CONTOUR ~

Q558=-90

;EXT:ANGLE CONT.START ~

Q559=+90

;CONTOUR END EXT ANGL ~

Q478=+0.3

;ROUGHING FEED RATE ~

Q488=+0.3

;PLUNGING FEED RATE ~

Q556=-80

;MIN. INCLINAT. ANGLE ~

Q557=+90

;MAX. INCLINAT. ANGLE ~

Q567=+0.4

;FINISH. ALLOW. CONT. ~

Q519=+2

;INFEED ~

Q463=+2.5

;MAX. CUTTING DEPTH ~

Q590=+1

;MACHINING MODE ~

Q591=+0

;MACHINING SEQUENCE ~

Q389=+0

;UNI.- BIDIRECTIONAL

13 CYCL CALL

; Cycle call

14 M305

15 TOOL CALL "TURN_FINISH"

; Tool call

16 CYCL DEF 800 ADJUST XZ SYSTEM ~

Q497=+0

;PRECESSION ANGLE ~

Q498=+0

;REVERSE TOOL ~

Q530=+2

;INCLINED MACHINING ~

Q531=+1

;ANGLE OF INCIDENCE ~

Q532=MAX

;FEED RATE ~

Q533=+1

;PREFERRED DIRECTION ~

Q535=+3

;ECCENTRIC TURNING ~

Q536=+0

;ECCENTRIC W/O STOP ~

Q599=+0

;RETRACT

17 FUNCTION TURNDATA SPIN VCONST: ON VC:400 SMAX800

; Constant surface speed

18 M145

; Reset the tool offset

19 FUNCTION TCPM F TCP AXIS POS PATHCTRL AXIS REFPNT TIP-CENTER

; Activate TCPM

20 L X+120 Y+0 R0 FMAX

21 L Z+20 R0 FMAX M303

22 CYCL DEF 883 TURNING SIMULTANEOUS FINISHING ~

Q460=+2

;SAFETY CLEARANCE ~

Q499=+0

;REVERSE CONTOUR ~

Q558=-90

;EXT:ANGLE CONT.START ~

Q559=+90

;CONTOUR END EXT ANGL ~

Q505=+0.2

;FINISHING FEED RATE ~

Q556=-80

;MIN. INCLINAT. ANGLE ~

Q557=+90

;MAX. INCLINAT. ANGLE ~

Q555=+1

;STEPPING ANGLE ~

Q537=+0

;INCID. ANGLE ACTIVE ~

Q538=+0

;INCLIN. ANGLE START ~

Q539=+0

;INCLINATN. ANGLE END ~

Q565=+0

;FINISHING ALLOW. D. ~

Q566=+0

;FINISHING ALLOW. Z ~

Q567=+0

;FINISH. ALLOW. CONT.

23 CYCL CALL

; Cycle call

24 M305

25 FUNCTION TURNDATA BLANK OFF

; Deactivate workpiece blank update

26 CYCL DEF 801 RESET ROTARY COORDINATE SYSTEM

27 FUNCTION MODE MILL

; Activate milling mode

28 TOOL CALL 0 Z

29 PLANE RESET TURN FMAX

30 M30

; End of program run

31 END PGM 1341941_1 MM

NC program 1341941_blank.h

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 1341941_BLANK MM

1 L X+0 Z+0.4

2 L X+80

3 L Z-139.6

4 L X+0

5 L Z+0.4

6 END PGM 1341941_BLANK MM

NC program 1341941_finish.h

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 1341941_FINISH MM

1 L X+0 Z+0 RR

2 CR Z-65.136 X+15 R+33 DR+

3 RND R2

4 L Z-86

5 RND R10

6 L X+78 Z-95

7 RND R5

8 L Z-100

9 END PGM 1341941_FINISH MM