Cycle 286 GEAR HOBBING (option 157)

ISO programming

G286

Application

 
Machine

Refer to your machine manual.

This function must be enabled and adapted by the machine manufacturer.

880_1

With Cycle 286 GEAR HOBBING, you can machine external cylindrical gears or helical gears with any angles. You can select the machining strategy and the machining side in the cycle. The machining process for gear hobbing is performed with a synchronized rotary movement of the tool spindle and workpiece spindle. In addition, the cutter moves along the workpiece in axial direction. Both for roughing and for finishing, the cutting operation may be offset by x edges relative to a height defined at the tool (e.g., 10 cutting edges for a height of 10 mm). This means that all cutting edges will be used in order to increase the tool life of the tool.

Cycle sequence

  1. The control positions the tool in the tool axis to clearance height Q260 at the feed rate FMAX. If the tool is already at a location in the tool axis higher than Q260, the tool will not be moved.
  2. Before tilting the working plane, the control positions the tool in X to a safe coordinate at the FMAX feed rate. If the tool is already located at a coordinate in the working plane that is greater than the calculated coordinate, the tool is not moved.
  3. The control then tilts the working plane at the feed rate Q253
  4. The control positions the tool at the feed rate FMAX to the starting point in the working plane
  5. The control then moves the tool in the tool axis at the feed rate Q253 to the set-up clearance Q200.
  6. The control moves the tool at the defined feed rate Q478 (for roughing) or Q505 (for finishing) to hob the workpiece in longitudinal direction. The area to be machined is limited by the starting point in Z Q551+Q200 and by the end point in Z Q552+Q200 (Q551 and Q552 are defined in Cycle 285).
  7. Cycle 285 DEFINE GEAR (option 157)

  8. When the tool reaches the end point, it is retracted at the feed rate Q253 and returns to the starting point.
  9. The control repeats the steps 5 to 7 until the defined gear is completed.
  10. Finally, the control retracts the tool to the clearance height Q260 at the feed rate FMAX.

Notes

 
Notice
Danger of collision!
When programming helical gears, the rotary axes will remain tilted, even after the end of the program. There is a danger of collision!
  1. Make sure to retract the tool before changing the position of the tilting axis
  • This cycle can only be executed in the FUNCTION MODE MILL and FUNCTION MODE TURN machining modes.
  • The cycle is CALL-active.
  • The maximum speed of the rotary table cannot be exceeded. If you have specified a higher value under NMAX in the tool table, the control will decrease the value to the maximum speed.
 
Tip

Avoid master spindle speeds of less than 6 rpm. Otherwise, it is not possible to reliably use a feed rate in mm/rev.

Notes on programming

  • In order to ensure constant engagement of the cutting edge of a tool, you need to define a very small path in cycle parameter Q554 SYNCHRONOUS SHIFT.
  • Make sure to program the direction of rotation of the master spindle (channel spindle) before the cycle start.
  • If you program FUNCTION TURNDATA SPIN VCONST:OFF S15, the spindle speed of the tool is calculated as Q541 x S. With Q541 = 238 and S = 15, this would result in a tool spindle speed of 3570 rpm.

Cycle parameters

Help graphic

Parameter

Q215 Machining operation (0/1/2/3)?

Define extent of machining:

0: Roughing and finishing

1: Only roughing

2: Only finishing to final dimension

3: Only finishing to oversize

Input: 0, 1, 2, 3

cyc286_1

cyc286_2

Q200 Set-up clearance?

Distance for retraction and prepositioning. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q260 Clearance height?

Coordinate in the tool axis in which no collision with the workpiece can occur (for intermediary positioning and retraction at the end of the cycle). This value has an absolute effect.

Input: –99999.9999...+99999.9999 or PREDEF

Q545 Tool lead angle?

Angle of the edges of the gear hob. Enter this value in decimal notation.

Example: 0°47'=0.7833

Input: –60...+60

Q546 Reverse spindle rotation dir.?

Direction of rotation of the slave spindle:

0: No change in the direction of rotation

1: Change in the direction of rotation

Input: 0, 1

Verifying and changing directions of rotation of the spindles

Q547 Angle offset of tool spindle?

Angle at which the control turns the workpiece at the beginning of the cycle.

Input: -180...+180

Q550 Machining side (0=pos./1=neg.)?

Define at which side machining is to take place.

0: Positive machining side of the main axis in the I-CS

1: Negative machining side of the main axis in the I-CS

Input: 0, 1

Q533 Preferred dir. of incid. angle?

Selection of alternate possibilities of inclination. The angle of incidence you define is used by the control to calculate the appropriate positioning of the tilting axes present on your machine. In general, there are always two possible solutions. Via parameter Q533, you configure which solution option the control is to use:

0: Solution that is the shortest distance from the current position

-1: Solution that is in the range between 0° and -179.9999°

+1: Solution that is in the range between 0° and +180°

-2: Solution that is in the range between -90° and -179.9999°

+2: Solution that is between +90° and +180°

Input: –2, –1, 0, +1, +2

Q530 Inclined machining?

Position the tilting axes for inclined machining:

1: Automatically position the tilting axis, and orient the tool tip (MOVE). The relative position between the workpiece and tool remains unchanged. The control performs a compensating movement with the linear axes

2: Automatically position the tilting axis without orienting the tool tip (TURN)

Input: 1, 2

cyc286_4

cyc286_3

Q253 Feed rate for pre-positioning?

Definition of the traversing speed of the tool during tilting and during pre-positioning. And during positioning of the tool axis between the individual infeeds. Feed rate is in mm/min.

Input: 0...99999.9999 or FMAX, FAUTO, PREDEF

Q553 TOOL:L offset, machining start?

Define the minimum length offset (L OFFSET) that the tool should have when in use. The control offsets the tool in the longitudinal direction by this amount. This value has an incremental effect.

Input: 0...999.999

Q554 Path for synchronous shift?

Define by which distance the gear hob will be offset in its axial direction during machining. This way, tool wear can be distributed over this area of the cutting edges. For helical gears, it is thus possible to limit the cutting edges used for machining.

Entering 0 deactivates the synchronous shift function.

Input: –99...+99.9999

Q548 Tool shift for roughing?

Specify the number of cutting edges by which the control will shift the roughing tool in its axial direction. The shift will be performed incrementally relative to parameter Q553. Entering 0 deactivates the shift function.

Input: –99...+99

Q463 Maximum cutting depth?

Maximum infeed (radius value) in the radial direction. The infeed is distributed evenly to avoid abrasive cuts.

Input: 0,001...999.999

Q488 Feed rate for plunging

Feed rate for tool infeed. The control interprets the feed rate in mm per workpiece revolution.

Input: 0...99999.999 or FAUTO

Q478 Roughing feed rate?

Feed rate during roughing. The control interprets the feed rate in mm per workpiece revolution.

Input: 0...99999.999 or FAUTO

Q483 Oversize for diameter?

Diameter oversize on the defined contour. This value has an incremental effect.

Input: 0...99.999

Q505 Finishing feed rate?

Feed rate during finishing. The control interprets the feed rate in mm per workpiece revolution.

Input: 0...99999.999 or FAUTO

Q549 Tool shift for finishing?

Specify the number of cutting edges by which the control will shift the finishing tool in its longitudinal direction. The shift will be performed incrementally relative to parameter Q553. Entering 0 deactivates the shift function.

Input: –99...+99

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.

Example

11 CYCL DEF 286 GEAR HOBBING ~

Q215=+0

;MACHINING OPERATION ~

Q200=+2

;SET-UP CLEARANCE ~

Q260=+100

;CLEARANCE HEIGHT ~

Q545=+0

;TOOL LEAD ANGLE ~

Q546=+0

;CHANGE ROTATION DIR. ~

Q547=+0

;ANG. OFFSET, SPINDLE ~

Q550=+1

;MACHINING SIDE ~

Q533=+0

;PREFERRED DIRECTION ~

Q530=+2

;INCLINED MACHINING ~

Q253=+750

;F PRE-POSITIONING ~

Q553=+10

;TOOL LENGTH OFFSET ~

Q554=+0

;SYNCHRONOUS SHIFT ~

Q548=+0

;ROUGHING SHIFT ~

Q463=+1

;MAX. CUTTING DEPTH ~

Q488=+0.3

;PLUNGING FEED RATE ~

Q478=+0.3

;ROUGHING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q505=+0.2

;FINISHING FEED RATE ~

Q549=+0

;FINISHING SHIFT

Verifying and changing directions of rotation of the spindles

Before performing a machining operation, make sure that the direction of rotation has been set correctly for both spindles.

  1. Determine the direction of rotation of the rotary table:
  2. What tool? (Right-cutting/left-cutting?)
  3. Which machining side? X+ (Q550=0) / X- (Q550=1)
  4. Look up the direction of rotation of the rotary table in one of the two tables below! To do so, select the appropriate table for the direction of rotation of your tool (right-cutting/left-cutting). Please refer to the appropriate table below to find the direction of rotation of your rotary table for the desired machining side X+ (Q550=0) / X- (Q550=1).
Tool: Right-cutting M3

Machining side

Direction of rotation of the rotary table

X+ (Q550=0)

Clockwise (e.g., M303)

X- (Q550=1)

Counterclockwise (e.g., M304)

Tool: Left-cutting M4

Machining side

Direction of rotation of the rotary table

X+ (Q550=0)

Counterclockwise (e.g., M304)

X- (Q550=1)

Clockwise (e.g., M303)

 
Tip

Keep in mind that in special cases, the directions of rotation might deviate from the ones indicated in these tables.

Changing the direction of rotation

cyc286_6

Milling:

  • Master spindle 1: Use M3 or M4 to define the tool spindle as the master spindle. This defines the direction of rotation (changing the direction of rotation of the master spindle does not affect the direction of rotation of the slave spindle)
  • Slave spindle 2: To change the direction of rotation of the slave spindle, adjust the value of input parameter Q546.

Turning:

  • Master spindle 1: Use an M function to define the tool spindle as the master spindle. This M function is machine manufacturer-specific (M303, M304,...). This defines the direction of rotation (changing the direction of rotation of the master spindle does not affect the direction of rotation of the slave spindle)
  • Slave spindle 2: To change the direction of rotation of the slave spindle, adjust the value of input parameter Q546.
 
Tip

Before performing a machining operation, make sure that the direction of rotation has been set correctly for both spindles.

If required, define a low spindle speed to make sure that the direction of rotation is correct.