Example

Drilling is carried out with the W axis in the following NC 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 PAR MM

1 BLK FORM 0.1 Z X+0 Y+0 Z-20

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

3 TOOL CALL 5 Z S2222

; Call the tool in the tool axis Z

4 L Z+100 R0 FMAX M3

; Position the main axis

5 CYCL DEF 200 DRILLING

Q200=+2

;SET-UP CLEARANCE

Q201=-20

;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=+0

;DEPTH REFERENCE

6 FUNCTION PARAXCOMP DISPLAY Z

; Activate display compensation

7 FUNCTION PARAXMODE X Y W

; Positive axis selection

8 L X+50 Y+50 R0 FMAX M99

; The parallel axis W executes the infeed

9 FUNCTION PARAXMODE OFF

; Restore the standard configuration

10 L M30

11 END PGM PAR MM