Example: Cylinder surface with Cycle 28

 
Tip
  • Cylinder centered on rotary table
  • Machine with B head and C table
  • Preset is at the center of the rotary table
  • Description of the path of the tool center in the contour subprogram

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 4 MM

1 BLK FORM CYLINDER Z R25 L100

2 TOOL CALL 3 Z S2000

; Tool call, tool axis (Z), diameter (7)

3 L Z+250 R0 FMAX M3

; Retract the tool

4 PLANE SPATIAL SPA+0 SPB+90 SPC+0 TURN MB MAX FMAX

; Tilt to position

5 CYCL DEF 14.0 CONTOUR

6 CYCL DEF 14.1 CONTOUR LABEL1

7 CYCL DEF 28 CYLINDRICAL SURFACE SLOT ~

Q1=-7

;MILLING DEPTH ~

Q3=+0

;ALLOWANCE FOR SIDE ~

Q6=+2

;SET-UP CLEARANCE ~

Q10=-4

;PLUNGING DEPTH ~

Q11=+100

;FEED RATE FOR PLNGNG ~

Q12=+250

;FEED RATE F. ROUGHNG ~

Q16=+25

;RADIUS ~

Q17=+1

;TYPE OF DIMENSION ~

Q20=+10

;SLOT WIDTH ~

Q21=+0.02

;TOLERANCE

8 L C+0 R0 FMAX M99

; Pre-position the rotary table, cycle call

9 L Z+250 R0 FMAX

; Retract the tool

10 PLANE RESET TURN MB MAX FMAX

; Tilt back, cancel the PLANE function

11 M30

; End of program run

12 LBL 1

; Contour subprogram, description of the path of the tool center

13 L X+60 Y+0 RL

; Rotary axis data in mm (Q17 = 1)

14 L Y-35

15 L X+40 Y-52.5

16 L X-70

17 LBL 0

18 END PGM 4 MM