Example of skiving with technology table and profile program

The NC program below uses Cycle 287 GEAR SKIVING with the technology table. The technology table defines an individual tooth flank profile with symmetrical crowning for the last cut.

The profile program checks the defined machining side Q550, and the suitable infeed direction that matches this machining side is used.

Program sequence

  • Tool call of a ring gear milling cutter
  • Start the turning mode
  • Reset the coordinate system with Cycle 801
  • Move to safe position
  • Define Cycle 285
  • Call Cycle 287
  • 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 SKIV MM

1 BLK FORM CYLINDER Z R400 L20 DIST+0 DI300

2 TOOL CALL "SKIVING"

; Call the tool

3 FUNCTION MODE TURN

; Activate turning mode

4 CYCL DEF 801 RESET ROTARY COORDINATE SYSTEM

5 M145

; Cancel a potentially still active M144

6 FUNCTION TURNDATA SPIN VCONST: OFF VC:200 S200

; Constant surface speed OFF

7 L X+0 Y+0 R0 FMAX

; Pre-position the tool at the workpiece center

8 L Z+50 R0 FMAX

; Pre-position the tool in the spindle axis

9 CYCL DEF 285 DEFINE GEAR ~

Q551=+0

;STARTING POINT IN Z ~

Q552=-20

;END POINT IN Z ~

Q540=+4

;MODULE ~

Q541=-76

;NUMBER OF TEETH ~

Q542=+0

;OUTSIDE DIAMETER ~

Q563=+9

;TOOTH HEIGHT ~

Q543=+0

;TROUGH-TIP CLEARANCE ~

Q544=+0

;ANGLE OF INCLINATION

10 CYCL DEF 287 GEAR SKIVING ~

QS240="Skiv.TAB"

;CUTS/TABLE ~

Q584=+1

;NO. OF FIRST CUT ~

Q585=+99

;NO. OF LAST CUT ~

Q200=+2

;SET-UP CLEARANCE ~

Q260=+50

;CLEARANCE HEIGHT ~

Q545=-20

;TOOL LEAD ANGLE ~

Q546=+0

;CHANGE ROTATION DIR. ~

Q547=+0

;ANG. OFFSET, SPINDLE ~

Q550=+1

;MACHINING SIDE ~

Q533=-1

;PREFERRED DIRECTION ~

Q530=+1

;INCLINED MACHINING ~

Q253=+2222

;F PRE-POSITIONING ~

Q586=+1.5

;FIRST INFEED ~

Q587=+0.1

;LAST INFEED ~

Q588=+2

;FIRST FEED RATE ~

Q589=+1

;LAST FEED RATE ~

Q580=+0.2

;FEED-RATE ADAPTION ~

Q466=+0.1

;OVERRUN PATH

11 L X+0 Y+0 R0 FMAX M136

12 CYCL CALL M303

; Call the cycle, spindle ON

13 CYCL DEF 801 RESET ROTARY COORDINATE SYSTEM

14 M305

15 FUNCTION MODE MILL

; Activate milling mode

16 M140 MB MAX

; Retract the tool in the tool axis

17 L A+0 C+0 R0 FMAX

; Reset the rotation

18 M30

; End of program run

19 END PGM SKIV MM

Technology table SKIV.TAB

NR

FEED

INFEED

dY

dK

PGM

0

0.233

1.497

0

0

1

0.251

1.265

0

0

2

0.265

1.117

0

0

3

0.278

1.01

0

0

4

0.288

0.93

0

0.001

5

0.298

0.866

0

-0.001

6

0.307

0.813

0.01

0

7

0.15

0.77

-0.01

0

8

0.1

0.732

0

0

TNC:\Skiving\Prog_contour.h

Profile 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 PROG_CONTOUR MM

1 QL0 = +0

; Z1

2 QL1 = +0.03

; Y1

3 QL2 = -10

; Z2

4 QL3 = +0

; Y2

5 QL4 = -20

; Z3

6 QL5 = +0.03

; Y3

8 FN 9: IF Q550 EQU +0 GOTO LBL "machSideNeg"

; Selection of machining side

9 FN 23: QL10 = CDATA QL0

; Circle data from three points on the circle, QL10 = Circle center Z; QL11 = Circle center X; QL12 = Circle radius

10 L YQL1 ZQL0

11 CR YQL5 ZQL4 RQL12 DR+

12 FN 9: IF +0 EQU +0 GOTO LBL "END"

13 LBL "machSideNeg"

14 QL1 = -QL1

15 QL3 = -QL3

16 QL5 = -QL5

17 FN 23: QL10 = CDATA QL0

; Circle data from three points on the circle

18 L YQL1 ZQL0

19 CR YQL5 ZQL4 RQL12 DR-

20 LBL "END"

21 END PGM PROG_CONTOUR MM