Technology table for Cycle 287 Gear Skiving (#157 / #4-05-1)

Application

In Cycle 287 GEAR SKIVING, you can use the cycle parameter QS240 NUMBER OF CUTS to call a table containing technology data. The table is a freely definable table and as such is in the *.tab format. The control makes a template Proto_Skiving.TAB available to you. In the table, you define the following data for each individual cut:

  • Feed rate
  • Lateral infeed
  • Lateral offset
  • Angular offset of the workpiece
  • If necessary, a profile program for an individual tooth flank line

Related topics

Requirement

  • Gear Cutting (#157 / #4-05-1) software option

Parameters in the technology table

Parameters in the table

The technology data table provides the following parameters:

Parameter

Function

NR

Number of the cut that also corresponds to the number of the table row

Input: 0...99999

FEED

Feed rate in mm/rev or 1/10 inch/rev for the cut

This parameter replaces the following cycle parameters:

  • Q588 FIRST FEED RATE
  • Q589 LAST FEED RATE
  • Q580 FEED-RATE ADAPTION

Input: 0...9999.999

INFEED

Lateral infeed of the cut. This value has an incremental effect.

This parameter replaces the following cycle parameters:

  • Q586 FIRST INFEED
  • Q587 LAST INFEED

Input: 0...99.99999

dY

Lateral offset between the tool and the workpiece

An offset of dY allows you to machine only one side of the tooth flank. Therefore the surface quality may be improved with dY.

The entered values can lead to a distortion of the tooth flank profile, which might need to be considered in the profile of the cutting edges.

Input: –9.99999...+9.99999

dK

Angular offset of workpiece

Use the dK angular offset to machine only one side of the tooth flank. In this way the surface quality may be improved. The entered values can lead to a distortion of the tooth flank profile, which might need to be considered in the profile of the cutting edges.

Input: –9.99999...+9.99999

PGM

Profile program for an individual tooth flank line

Profile program of tooth flank line

Notes

  • The unit used in the NC program determines whether millimeter or inch units are used.
  • HEIDENHAIN recommends that you program only minimum offset values dY and minimum offsets dK in the individual cuts in order to avoid damage to the contour.
  • The two values dY and dK can be combined with each other.
  • The sum of the lateral infeeds (INFEED) must result in the tooth height.
    • If the tooth height is greater than the total infeed, the control will display a warning.
    • If the tooth height is less than the total infeed, the control will display an error message.
  • Example:

    • TOOTH HEIGHT (Q563) = 2 mm
    • Number of cuts (NR) = 15
    • Lateral infeed (INFEED) = 0.2 mm
    • Total infeed = NR * INFEED = 3 mm
    • In this case, the tooth height is less than the total infeed (2 mm < 3 mm).

    • Reduce the number of cuts to 10.

Profile program of tooth flank line

With a separate NC program you can define an individual tooth flank line 1, such as a minimum crowning of the tooth flank.

Remember the following rules for the profile program:

  • Do not program a feed rate.
  • The cycle automatically calculates and executes pre-positioning and the overrun path.
  • In turning mode, take an active diameter or radius programming into account.
  • The datum for the profile program is at the starting point of the tooth flank.
 
Tip

Use the Q584 NO. OF FIRST CUT parameter to read and evaluate the active cut number in the NC program.

Example application:

The finished gear wheels often transmit large forces when the teeth press against each other. These large forces can cause deformation of the material, for example, and thus lead to uneven load distribution on the tooth flank. The uneven load distribution can cause wear on the gear wheel. To reduce or avoid wear on the gear wheel, you can optimize the tooth flank line; for example, by adding minimum crowning on the tooth flank.

Example of skiving with technology table and profile program