Cycle 287 GEAR SKIVING option 157

ISO programming

G287

Application

 
Machine

Refer to your machine manual.

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

cyc287

With Cycle 287 GEAR SKIVING, you can machine cylindrical gears or helical gears with any angles. Cutting takes place on the one hand by the axial feeding of the tool and on the other hand through the rolling motion.

You can select the machining side in the cycle. The machining process for gear skiving 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.

In the cycle, you can call a table containing technology data. In this table, you can define the feed rate, the lateral infeed, and the lateral offset for each cut.

Technology table for Cycle 287 Gear Skiving

Cycle sequence

  1. The control positions the tool in the tool axis to the clearance height Q260 at the feed rate FMAX. If the value of the current tool position in the tool axis is greater than Q260, the tool will not be moved
  2. Before tilting the working plane, the control positions the tool in X at the feed rate FMAX to a safe coordinate. 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 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. After that, the control positions the tool in the tool axis at the feed rate Q253 to the set-up clearance Q200
  6. The control then traverses the approach length. The control automatically calculates this distance. The approach length is the distance from the initial scratch to the complete plunging depth.
  7. The control rolls the tool over the workpiece to be geared in longitudinal direction at the defined feed rate. During the initial infeed of the cut Q586 the control moves at the initial feed rate Q588. The control then uses intermediate values for the infeed and feed rate of the next cuts. The control calculates these values itself. The intermediate feed rate values, however, depend on the factor for feed-rate adaptation Q580. When the control arrives at the last infeed Q587, it performs the last cut with the feed rate Q589
  8. The area to be machined is limited by the starting point in Z Q551+Q200 and by the end point in Z Q552 (Q551 and Q552 are defined in Cycle 285). The approach length must be added to the starting point. Its purpose is to prevent the tool from plunging into the workpiece all the way to the machining diameter. The control calculates this distance itself.
  9. At the end of machining, the tool moves beyond the defined end point by the overrun path Q580. The overrun path serves to completely machine the gear.
  10. When the control reaches the end point, it retracts the tool at the feed rate Q253 and positions it back to the starting point
  11. Finally the control positions 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 speed ratio between tool and workpiece results from the number of teeth of the gear wheel and the number of cutting edges of the tool.

Notes on programming

  • Make sure to program the direction of rotation of the master spindle (channel spindle) before the cycle start.
  • The larger the factor in Q580 FEED-RATE ADAPTION, the earlier the control will adapt the feed rate to the feed rate for the last cut. The recommended value is 0.2.
  • When defining the tool, make sure to specify the number of cutting edges as indicated in the tool table.
  • If only two cuts have been programmed in Q240, the last infeed from Q587 and the last feed rate from Q589 will be ignored. If only one cut has been programmed, the first infeed from Q586 will also be ignored.

Cycle parameters

Help graphic

Parameter

Q240 Number of cuts?

Number of cuts to the final depth

0: The control automatically determines the minimum number of cuts

1: One cut

2: Two cuts where the control considers only the infeed for the first cut Q586. The control does not consider the infeed for the last cut Q587.

3 to 99: Programmed number of cuts

"...": Path of a table containing technology data see Technology table for Cycle 287 Gear Skiving

Input: 0...99 or text entry of max. 255 characters or QS parameter

Q584 Number of the first cut?

Define which cut number the control will perform first.

Input: 1...999

Q585 Number of the last cut?

Define at which number the control will perform the last cut.

Input: 1...999

cyc287_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 skiving tool. 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

cyc287_1

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

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

Q586 Infeed for first cut?

Infeed for the first cut. This value has an incremental effect.

If the path of a technology table is stored in Q240, this parameter has no effect. see Technology table for Cycle 287 Gear Skiving

Input: 0,001...99.999

Q587 Infeed for last cut?

Infeed for the last cut. This value has an incremental effect.

If the path of a technology table is stored in Q240, this parameter has no effect. see Technology table for Cycle 287 Gear Skiving

Input: 0,001...99.999

Q588 Feed rate for first cut?

Feed rate for the first cut. The control interprets the feed rate in mm per workpiece revolution.

If the path of a technology table is stored in Q240, this parameter has no effect. see Technology table for Cycle 287 Gear Skiving

Input: 0,001...99.999

Q589 Feed rate for last cut?

Feed rate for the last cut. The control interprets the feed rate in mm per workpiece revolution.

If the path of a technology table is stored in Q240, this parameter has no effect. see Technology table for Cycle 287 Gear Skiving

Input: 0,001...99.999

Q580 Factor for feed-rate adaptation?

Using this factor, you can define a feed rate reduction. This is due to the fact that the feed rate must decrease with increasing cutting numbers. The greater the value, the earlier the control will adapt the feed rates to match the last feed rate.

If the path of a technology table is stored in Q240, this parameter has no effect. see Technology table for Cycle 287 Gear Skiving

Input: 0...1

cyc287_6

Q466 Overrun path?

Length of overtravel at the end of the gear teeth. The overtravel path ensures that the control machines the gear teeth up to the desired end point.

If you do not program these optional parameters, then the control uses the safety clearance Q200 as the overtravel path.

Input: 0.1...99.9

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 287 GEAR SKIVING ~

Q240=+0

;NUMBER OF CUTS ~

Q584=+1

;NO. OF FIRST CUT ~

Q585=+999

;NO. OF LAST CUT ~

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 ~

Q586=+1

;FIRST INFEED ~

Q587=+0.1

;LAST INFEED ~

Q588=+0.2

;FIRST FEED RATE ~

Q589=+0.05

;LAST FEED RATE ~

Q580=+0.2

;FEED-RATE ADAPTION ~

Q466=+2

;OVERRUN PATH

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

cyc287_4

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.