Cycle 880 GEAR HOBBING (#50 / #4-03-1) and (#131 / #7-02-1)
ISO programming
G880
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
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.
Related topics
- Cycle 286 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; M144 is internally active in the cycle
- 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 set-up clearance Q460.
- 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.
- When the control reaches the end point, it retracts the tool at the feed rate Q253 and positions it back to the starting point
- The control repeats the steps 5 to 7 until the defined gear is completed.
- Finally the control positions the tool to the clearance height Q260 at the feed rate FMAX
- The machining operation ends in the tilted system.
- Now you need to move the tool to a safe height and reset the tilting of the working plane.
- It is essential that you now program Cycle 801 RESET ROTARY COORDINATE SYSTEM and M145
Notes
- Pre-position the tool so that it is already on the desired machining side Q550.
- Move the tool to a safe position on this machining side
- Clamp the workpiece out of the fixtures far enough to prevent a danger of collision between the tool and the fixtures
- 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
- If you program M136 explicitly before the cycle, the control will interpret the feed rates in the cycle in mm/rev.
- If you do not program M136 before the cycle, the control will interpret the feed rates in the cycle in mm/min.
- Make sure to program Cycle 801 after Cycle 880 in order to reset the coordinate system.
- Make sure to program Cycle 801 after a program abort in order to reset the coordinate system.
- This cycle can be executed only 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.
So as to avoid exceeding the maximum permissible spindle speed of the tool, 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 | |
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 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 | |
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 | |
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? Feed 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.
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 880 GEAR HOBBING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|
Direction of rotation depending on the machining side (Q550)
Determine the direction of rotation of the rotary table:
- What tool? (Right-cutting/left-cutting?)
- What 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 tables below to find the direction of rotation of your rotary table for the desired machining side X+ (Q550=0) / X- (Q550=1) ab.
Tool: Right-cutting M3 | |
Machining side | Direction of rotation of the table: |
Machining side | Direction of rotation of the table: |
Tool: Left-cutting M4 | |
Machining side | Direction of rotation of the table: |
Machining side | Direction of rotation of the table: |