Example: Milling pockets, studs and slots

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 C210 MM

1 BLK FORM 0.1 Z X+0 Y+0 Z-40

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

3 TOOL CALL 6 Z S3500

; Tool call: roughing/finishing

4 L Z+100 R0 FMAX M3

; Retract the tool

5 CYCL DEF 256 RECTANGULAR STUD ~

Q218=+90

;FIRST SIDE LENGTH ~

Q424=+100

;WORKPC. BLANK SIDE 1 ~

Q219=+80

;2ND SIDE LENGTH ~

Q425=+100

;WORKPC. BLANK SIDE 2 ~

Q220=+0

;CORNER RADIUS ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q224=+0

;ANGLE OF ROTATION ~

Q367=+0

;STUD POSITION ~

Q207=+500

;FEED RATE MILLING ~

Q351=+1

;CLIMB OR UP-CUT ~

Q201=-30

;DEPTH ~

Q202=+5

;PLUNGING DEPTH ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+20

;2ND SET-UP CLEARANCE ~

Q370=+1

;TOOL PATH OVERLAP ~

Q437=+0

;APPROACH POSITION ~

Q215=+0

;MACHINING OPERATION ~

Q369=+0.1

;ALLOWANCE FOR FLOOR ~

Q338=+10

;INFEED FOR FINISHING ~

Q385=+500

;FINISHING FEED RATE

6 L X+50 Y+50 R0 FMAX M99

; Cycle call for outside machining

7 CYCL DEF 252 CIRCULAR POCKET ~

Q215=+0

;MACHINING OPERATION ~

Q223=+50

;CIRCLE DIAMETER ~

Q368=+0.2

;ALLOWANCE FOR SIDE ~

Q207=+500

;FEED RATE MILLING ~

Q351=+1

;CLIMB OR UP-CUT ~

Q201=-30

;DEPTH ~

Q202=+5

;PLUNGING DEPTH ~

Q369=+0.1

;ALLOWANCE FOR FLOOR ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q338=+5

;INFEED FOR FINISHING ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q370=+1

;TOOL PATH OVERLAP ~

Q366=+1

;PLUNGE ~

Q385=+750

;FINISHING FEED RATE ~

Q439=+0

;FEED RATE REFERENCE

8 L X+50 Y+50 R0 FMAX M99

; Cycle call for circular pocket

9 TOOL CALL 3 Z S5000

; Tool call: slot milling cutter

10 L Z+100 R0 FMAX M3

11 CYCL DEF 254 CIRCULAR SLOT ~

Q215=+0

;MACHINING OPERATION ~

Q219=+8

;SLOT WIDTH ~

Q368=+0.2

;ALLOWANCE FOR SIDE ~

Q375=+70

;PITCH CIRCLE DIAMETR ~

Q367=+0

;REF. SLOT POSITION ~

Q216=+50

;CENTER IN 1ST AXIS ~

Q217=+50

;CENTER IN 2ND AXIS ~

Q376=+45

;STARTING ANGLE ~

Q248=+90

;ANGULAR LENGTH ~

Q378=+180

;STEPPING ANGLE ~

Q377=+2

;NR OF REPETITIONS ~

Q207=+500

;FEED RATE MILLING ~

Q351=+1

;CLIMB OR UP-CUT ~

Q201=-20

;DEPTH ~

Q202=+5

;PLUNGING DEPTH ~

Q369=+0.1

;ALLOWANCE FOR FLOOR ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q338=+5

;INFEED FOR FINISHING ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q366=+2

;PLUNGE ~

Q385=+500

;FINISHING FEED RATE ~

Q439=+0

;FEED RATE REFERENCE

12 CYCL CALL

; Cycle call for slots

13 L Z+100 R0 FMAX

; Retract the tool

14 M30

; End of program run

15 END PGM C210 MM