ISO programming
G880
G880
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.
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.)
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 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.
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 ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|
Tool: Right-cutting M3 | |
| Direction of rotation of the table: |
| Direction of rotation of the table: |
Tool: Left-cutting M4 | |
| Direction of rotation of the table: |
| Direction of rotation of the table: |