Fundamentals for the machining of gear teeth (#157 / #4-05-1)
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
These cycles require the software option Gear Cutting (#157 / #4-05-1). If you would like to use these cycles in turning mode, you also need the software option Turning (#50 / #4-03-1). In milling mode, the tool spindle is the master spindle; in turning mode, it is the workpiece spindle. The other spindle is called slave spindle. Depending on the operating mode, you program the speed or the cutting speed with a TOOL CALL S or FUNCTION TURNDATA SPIN.
To orient the I-CS coordinate system, Cycles 286 and 287 use the precession angle that is also affected by Cycles 800 and 801 in turning mode. At the end of the cycle, the control resets the precession angle to its state at the beginning of the cycle. If one of these cycles is aborted, the precession angle will also be reset.
The axis crossing angle is the angle between workpiece and tool. It results from the angle of inclination of the tool and the angle of inclination of the gear. Based on the required axis crossing angle, Cycles 286 and 287 calculate the required inclination of the rotary axis at the machine. The cycles will always position the first rotary axis starting from the tool.
The cycles control LIFTOFF automatically to enable moving the tool out of the gear safely in case of fault. The cycles define the direction and the path for LIFTOFF. You only need to activate LIFTOFF for your tool. The machine manufacturer can configure the automatic LIFTOFF.
The gear itself will first be described in Cycle 285 DEFINE GEAR. Then, program Cycle 286 GEAR HOBBING or Cycle 287 GEAR SKIVING.
Program the following:
- Call a tool with TOOL CALL
- Select turning mode or milling mode, with FUNCTION MODE TURN or FUNCTION MODE MILL "KINEMATIC_GEAR" kinematics selection
- Spindle direction of rotation (e.g., M3 or M303)
- Perform pre-positioning for the cycle depending on your selection of MILL or TURN
- Define the CYCL DEF 285 DEFINE GEAR cycle
- Define the CYCL DEF 286 GEAR HOBBING or CYCL DEF 287 GEAR SKIVING cycle.
Notes
- Pre-position the tool to a safe position
- Make sure to clamp the workpiece in such a way that it projects far enough from the fixture and no collision can occur between tool and fixture.
- Before calling the cycle, set the preset to the center of rotation of the workpiece spindle.
- Please note that the slave spindle will continue to rotate after the end of the cycle. If you want to stop the spindle before the end of the program, make sure to program a corresponding M function.
- Activate the LiftOff in the tool table. In addition, this function must have been configured by your machine manufacturer.
- Remember that you need to program the speed of the master spindle before calling the cycle, i.e. the tool spindle speed in milling mode and the workpiece spindle speed in turning mode.
Gear formulas
Speed calculation
- nT: Tool spindle speed
- nW: Workpiece spindle speed
- zT: Number of tool teeth
- zW: Number of workpiece teeth
Definition | Tool spindle | Workpiece spindle |
---|---|---|
Hobbing | ||
Skiving |
Straight-cut spur gears
- m: Module (Q540)
- p: Pitch
- h: Tooth height (Q563)
- d: Pitch-circle diameter
- z: Number of teeth (Q541)
- c: Trough-to-tip clearance (Q543)
- da: Diameter of the addendum circle (outside diameter, Q542)
- df: Root circle diameter
Definition | Formula |
---|---|
Module (Q540) | |
Pitch | |
Pitch-circle diameter | |
Tooth height (Q563) | |
Diameter of the addendum circle (outside diameter, Q542) | |
Root circle diameter | |
Root circle diameter if tooth height > 0 | |
Number of teeth (Q541) |
|
Remember to observe the algebraic sign when calculating an inner gear.
Example: Calculating the diameter of the addendum circle (outside diameter)
Outer gear: Q540 * (Q541 + 2) = 1 * (+46 + 2)
Inner gear: Q540 * (Q541 + 2) = 1 * (-46 + 2)