Example of hob milling

The following NC program uses Cycle 286 GEAR HOBBING. This programming example shows how to machine an involute spline with module = 1 (deviating from DIN 3960).

Program sequence

  • Tool call: Gear hob
  • Start the turning mode
  • Reset the coordinate system with Cycle 801
  • Move to safe position
  • Define Cycle 285
  • Call Cycle 286
  • Reset the coordinate system with Cycle 801

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 7 MM

1 BLK FORM CYLINDER Z D90 L35 DIST+0 DI58

2 TOOL CALL "GEAR_HOB"

; Call the tool

3 FUNCTION MODE TURN

; Activate turning mode

* - ...

; Reset the coordinate system

4 CYCL DEF 801 RESET ROTARY COORDINATE SYSTEM

5 M145

; Cancel a potentially still active M144

6 FUNCTION TURNDATA SPIN VCONST:OFF S50

; Constant surface speed OFF

7 M140 MB MAX

; Retract the tool

8 L A+0 R0 FMAX

; Set the rotary axis to 0

9 L X+0 Y+0 R0 FMAX

; Pre-position the tool at the workpiece center

10 L Z+50 R0 FMAX

; Pre-position the tool in the spindle axis

11 CYCL DEF 285 DEFINE GEAR ~

q551=+0

;STARTING POINT IN Z ~

q552=-11

;END POINT IN Z ~

Q540=+1

;MODULE ~

Q541=+90

;NUMBER OF TEETH ~

Q542=+90

;OUTSIDE DIAMETER ~

q563=+1

;TOOTH HEIGHT ~

Q543=+0.05

;TROUGH-TIP CLEARANCE ~

Q544=-10

;ANGLE OF INCLINATION

12 CYCL DEF 286 GEAR HOBBING ~

Q215=+0

;MACHINING OPERATION ~

Q200=+2

;SET-UP CLEARANCE ~

Q260=+30

;CLEARANCE HEIGHT ~

Q545=+1.6

;TOOL LEAD ANGLE ~

Q546=+0

;CHANGE ROTATION DIR. ~

Q547=+0

;ANG. OFFSET, SPINDLE ~

Q550=+1

;MACHINING SIDE ~

Q533=+1

;PREFERRED DIRECTION ~

Q530=+2

;INCLINED MACHINING ~

Q253=+2222

;F PRE-POSITIONING ~

Q553=+5

;TOOL LENGTH OFFSET ~

Q554=+10

;SYNCHRONOUS SHIFT ~

Q548=+1

;ROUGHING SHIFT ~

Q463=+1

;MAX. CUTTING DEPTH ~

Q488=+0.3

;PLUNGING FEED RATE ~

Q478=+0.3

;PLUNGING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q505=+0.2

;FINISHING FEED RATE ~

Q549=+3

;FINISHING SHIFT

13 CYCL CALL M303

; Call the cycle, spindle ON

14 FUNCTION MODE MILL

; Activate milling mode

15 M140 MB MAX

; Retract the tool in the tool axis

16 L A+0 C+0 R0 FMAX

; Reset the rotation

17 M30

; End of program run

18 END PGM 7 MM