Cycle 286 GEAR HOBBING (#157 / #4-05-1)
ISO programming
G286
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
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.
Related topics
- Cycle 880 GEAR HOBBING
Cycle run
- 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.
- 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.
- The control then tilts the working plane at the feed rate Q253
- The control positions the tool at the feed rate FMAX to the starting point in the working plane
- The control then moves the tool in the tool axis at the feed rate Q253 to the set-up clearance Q200.
- 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).
- When the tool reaches the end point, it is retracted at the feed rate Q253 and returns to the starting point.
- The control repeats the steps 5 to 7 until the defined gear is completed.
- Finally, the control retracts the tool to the clearance height Q260 at the feed rate FMAX.
Notes
- Make sure to retract the tool before changing the position of the rotary axis
- This cycle can be executed only 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.
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 | |
Q200 Set-up clearance? Distance for retraction and prepositioning. This value has an incremental effect. Input: 0...99999.9999 or PREDEF | |
Q260 Clearance height? Position in the tool axis at which no collision can occur with the workpiece. The control approaches this position for intermediate positions and when retracting 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 inclination angle you define is used by the control to calculate the appropriate positioning of the rotary axis present on the machine. In general, there are two possible solutions. Via parameter Q533, you configure which solution option the control will 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 in the range between +90° and +180° Input: –2, –1, 0, +1, +2 | |
Q530 Inclined machining? Position the rotary axes for inclined machining: 1: Automatically position the rotary axis, and orient the tool tip accordingly (MOVE). The relative position between the workpiece and the tool remains unchanged. The control performs a compensation movement with the linear axes. 2: Automatically position the rotary axis without orienting the tool tip accordingly (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 | |
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.
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.
11 CYCL DEF 286 GEAR HOBBING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|
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.
Determine the direction of rotation of the rotary table:
- What tool? (Right-cutting/left-cutting?)
- Which machining side? X+ (Q550=0) / X- (Q550=1)
- 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).
Machining side | Direction of rotation of the rotary table |
---|---|
X+ (Q550=0) | Clockwise (e.g., M303) |
X- (Q550=1) | Counterclockwise (e.g., M304) |
Machining side | Direction of rotation of the rotary table |
---|---|
X+ (Q550=0) | Counterclockwise (e.g., M304) |
X- (Q550=1) | Clockwise (e.g., M303) |
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
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.
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.