Example: Gear hobbing

The following NC program uses Cycle 880 GEAR HOBBING This programming example illustrates the machining of a helical gear, with Module=2.1.

  • Program sequence
  • Tool call: Gear hob
  • Start turning mode
  • Move to safe position
  • Call the cycle
  • Reset the coordinate system with Cycle 801 and M145

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 8 MM

1 BLK FORM CYLINDER Z R42 L150

2 FUNCTION MODE MILL

; Activate milling mode

3 TOOL CALL "GEAD_HOB"

; Call tool

4 FUNCTION MODE TURN

; Activate turning mode

5 CYCL DEF 801 RESET ROTARY COORDINATE SYSTEM

6 M145

; Cancel a potentially still active M144

7 FUNCTION TURNDATA SPIN VCONST:OFF S50

; Constant cutting speed OFF

8 M140 MB MAX

; Retract the tool

9 L A+0 R0 FMAX

; Set turning axis to 0

10 L X+250 Y-250 R0 FMAX M303

; Pre-position the tool in the working plane on the side on which machining will be performed, Spindle ON

11 L Z+20 R0 FMAX

; Pre-position the tool in the spindle axis

12 M136

; Feed rate in mm/rev.

13 CYCL DEF 880 GEAR HOBBING ~

Q215=+0

;MACHINING OPERATION ~

Q540=+2.1

;MODULE ~

Q541=+0

;NUMBER OF TEETH ~

Q542=+69.3

;OUTSIDE DIAMETER ~

Q543=+0.1666

;TROUGH-TIP CLEARANCE ~

Q544=-5

;ANGLE OF INCLINATION ~

Q545=+1.6833

;TOOL LEAD ANGLE ~

Q546=+3

;CHANGE TOOL DIRECTN. ~

Q547=+0

;ANG. OFFSET, SPINDLE ~

Q550=+0

;MACHINING SIDE ~

Q533=+0

;PREFERRED DIRECTION ~

Q530=+2

;INCLINED MACHINING ~

Q253=+800

;F PRE-POSITIONING ~

Q260=+20

;CLEARANCE HEIGHT ~

Q553=+10

;TOOL LENGTH OFFSET ~

Q551=+0

;STARTING POINT IN Z ~

Q552=-10

;END POINT IN Z ~

Q463=+1

;MAX. CUTTING DEPTH ~

Q460=2

;SAFETY CLEARANCE ~

Q488=+1

;PLUNGING FEED RATE ~

Q478=+2

;ROUGHING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q505=+1

;FINISHING FEED RATE

14 CYCL CALL

; Call cycle

15 CYCL DEF 801 RESET ROTARY COORDINATE SYSTEM

16 M145

; Switch off active M144 in the cycle

17 FUNCTION MODE MILL

; Activate milling mode

18 M140 MB MAX

; Retract tool in the tool axis

19 L A+0 C+0 R0 FMAX

; Reset turning

20 M30

; End of program

21 END PGM 8 MM