Please Note While Programming - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | GEAR HOBBING (Cycle 880, DIN/ISO: G880)

Please note while programming:

The values entered for module, number of teeth and
outside diameter are monitored. If these values are
not consistent an error message is displayed. With
these parameters you can enter values for 2 of the 3
parameters. Enter the value 0 either for the module or
number of teeth or outside diameter. The TNC then
calculates the missing value.
Program FUNCTION TURNDATA SPIN VCONST:OFF .
If you program FUNCTION TURNDATA SPIN
VCONST:OFF S15, 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.
Define the tool as a milling cutter in the tool table.
To avoid exceeding the maximum permissible spindle
speed of the tool, you can enter a limitation. (Entry in
the "Nmax" column of the tool table "tool.t".)
Before starting the cycle, program the direction of
rotation of the workpiece (M303/M304).
Before cycle call, set the preset to the center of rotation.
Cycle 880 Gear Hobbing is run in turning mode and is
CALL -active.
Software option 50 must be enabled.
Software option 131 must be enabled.
Danger of collision!
If you do not position the tool to a safe position, a collision may
occur between the tool and workpiece (fixtures) during tilting.
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
Danger of collision!
If you clamp the workpiece too tightly to the fixtures, a collision
may occur between the tool and fixtures during execution. The
starting point in Z and the end point in Z are extended by the set-
up clearance Q460!
Clamp the workpiece out of the fixtures far enough to prevent
a danger of collision between the tool and the fixtures
Clamp your component out of the fixtures far enough so that
the extension automatically approached by the cycle of the
starting point and end point by the set-up clearance Q460
does not cause a collision
HEIDENHAIN | User's manual for cycle programming | 10/2017
NOTICE
NOTICE
12
477