Cycle 880 GEAR HOBBING (option 131)

ISO programming

G880

Application

 
Machine

Refer to your machine manual.

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

880_1

With Cycle 880 GEAR HOBBING, you can machine external cylindrical gears or helical gears with any angles. In the cycle you first define the gear and then the tool with which the gear is to be machined. 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 motion of the tool spindle and rotary table. In addition, the gear hob moves along the workpiece in axial direction.

While Cycle 880 GEAR HOBBING is active, the coordinate system might be rotated. It is therefore essential to program Cycle 801 RESET ROTARY COORDINATE SYSTEM and M145 after the end of the cycle.

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; M144 is internally active in the cycle
  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 set-up clearance Q460.
  6. The control now 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+Q460 and the end point in Z Q552+Q460.
  7. When the control reaches the end point, it retracts the tool at the feed rate Q253 and positions it back to the starting point
  8. The control repeats the steps 5 to 7 until the defined gear is completed.
  9. Finally the control positions the tool to the clearance height Q260 at the feed rate FMAX
  10. The machining operation ends in the tilted system.
  11. Now you need to move the tool to a safe height and reset the tilting of the working plane.
  12. It is essential that you now program Cycle 801 RESET ROTARY COORDINATE SYSTEM and M145

Notes

 
Notice
Danger of collision!
If you do not position the tool to a safe position, a collision may occur between the tool and workpiece (fixtures) during tilting.
  1. Pre-position the tool so that it is already on the desired machining side Q550.
  2. Move the tool to a safe position on this machining side
 
Notice
Danger of collision!
If the workpiece is clamped too deeply into the fixture, a collision between tool and fixture might occur during machining. The starting point in Z and the end point in Z are extended by the set-up clearance Q460!
  1. Clamp the workpiece out of the fixtures far enough to prevent a danger of collision between the tool and the fixtures
  2. Clamp the workpiece in such a way that its protrusion from the fixture will not cause any collision when the tool is automatically moved to the starting or end point using a path that is extended by the set-up clearance Q460
 
Notice
Danger of collision!
Depending on whether you use M136 or not, the feed rate values will be interpreted differently by the control. If the programmed feed rate was too high, the workpiece might be damaged.
  1. If you program M136 explicitly before the cycle, the control will interpret the feed rates in the cycle in mm/rev.
  2. If you do not program M136 before the cycle, the control will interpret the feed rates in the cycle in mm/min.
 
Notice
Danger of collision!
If you do not reset the coordinate system after Cycle 880, the precession angle set by the cycle will remain active. There is a danger of collision!
  1. Make sure to program Cycle 801 after Cycle 880 in order to reset the coordinate system.
  2. Make sure to program Cycle 801 after a program abort in order to reset the coordinate system.
  • This cycle can only be executed in the FUNCTION MODE MILL and FUNCTION MODE TURN machining modes.
  • The cycle is CALL-active.
  • Define the tool as a milling cutter in the tool table.
  • Before programming the cycle call, set the datum to the center of rotation.
 
Tip

In order to avoid that the maximum permissible spindle speed of the tool is not exceeded, you can program a limitation. (Specify it in the Nmax column of the "tool.t" tool table.)

Notes on programming

  • The values entered for the module, number of teeth and outside diameter (outside diameter) are monitored. If these values are not coherent, then an error message is displayed. You can fill in 2 of the 3 parameters. Enter 0 for the module, the number of teeth, or the outside diameter (outside diameter). In this case, the control will calculate the missing value.
  • Program FUNCTION TURNDATA SPIN VCONST:OFF.
  • If you program FUNCTION TURNDATA SPIN VCONST:OFF S15, then the spindle speed of the tool is calculated as follows: Q541 x S. With Q541=238 and S=15, this would result in a tool spindle speed of 3570 rpm.
  • Program the direction of rotation of your workpiece (M303/M304) before the start of the cycle.

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

Q540 Module?

Module of the gear

Input: 0...99.999

Q541 Number of teeth?

Describe gear: number of teeth

Input: 0...99999

Cyc880_1

Q542 Outside diameter?

Describe gear: outside diameter of finished part

Input: 0...99999.9999

Q543 Trough-to-tip clearance?

Distance between the addendum circle of the gear to be made and root circle of the mating gear.

Input: 0...9.9999

Q544 Angle of inclination?

Angle at which the teeth of a helical gear are inclined relative to the direction of the axis. For straight-cut gears, this angle is 0°.

Input: –60...+60

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 tool rotation direction?

Describe tool: Direction of spindle rotation of the gear hob

3: Clockwise rotating tool (M3)

4: Counterclockwise rotating tool (M4)

Input: 3, 4

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

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

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

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

Q551 Starting point in Z?

Starting point of the hobbing process in Z

Input: –99999.9999...+99999.9999

Q552 End point in Z?

End point of the hobbing process in Z

Input: –99999.9999...+99999.9999

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

Q460 Set-up clearance?

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

Input: 0...999.999

Q488 Feed rate for plunging

Feed rate of the tool infeed

Input: 0...99999.999 or FAUTO

Q478 Roughing feed rate?

Freed rate during roughing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute.

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. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute.

Input: 0...99999.999 or FAUTO

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 880 GEAR HOBBING ~

Q215=+0

;MACHINING OPERATION ~

Q540=+0

;MODULE ~

Q541=+0

;NUMBER OF TEETH ~

Q542=+0

;OUTSIDE DIAMETER ~

Q543=+0.1666

;TROUGH-TIP CLEARANCE ~

Q544=+0

;ANGLE OF INCLINATION ~

Q545=+0

;TOOL LEAD ANGLE ~

Q546=+3

;CHANGE TOOL DIRECTN. ~

Q547=+0

;ANG. OFFSET, SPINDLE ~

Q550=+1

;MACHINING SIDE ~

Q533=+0

;PREFERRED DIRECTION ~

Q530=+2

;INCLINED MACHINING ~

Q253=+750

;F PRE-POSITIONING ~

Q260=+100

;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=+0.3

;PLUNGING FEED RATE ~

Q478=+0.3

;ROUGHING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q505=+0.2

;FINISHING FEED RATE

Direction of rotation depending on the machining side (Q550)

  1. Determine the direction of rotation of the rotary table:
  2. What tool? (Right-cutting/left-cutting?)
  3. What 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 tables below to find the direction of rotation of your rotary table for the desired machining side X+ (Q550=0) / X- (Q550=1) ab.

cyc880_2

cyc880_3

Tool: Right-cutting M3

  • Machining side
    X+ (Q550=0)

Direction of rotation of the table:
Clockwise (M303)

  • Machining side
    X- (Q550=1)

Direction of rotation of the table:
Counterclockwise (M304)

Tool: Left-cutting M4

  • Machining side
    X+ (Q550=0)

Direction of rotation of the table:
Counterclockwise (M304)

  • Machining side
    X- (Q550=1)

Direction of rotation of the table:
Clockwise (M303)