HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 321)

TURN, TRANSVERSE PLUNGE EXTENDED
(Cycle 824, DIN/ISO: G824)
13.14
13
TNC 640 | User's Manual Cycle Programming | 5/2013
321
13.14 TURN, TRANSVERSE PLUNGE
EXTENDED
(Cycle 824, DIN/ISO: G824)
Application
This cycle enables you to face turn plunge elements (undercuts).
Expanded scope of function:
You can insert a chamfer or curve at the contour start and
contour end.
In the cycle you can define an angle for the face and a radius for
the contour edge
You can use the cycle either for roughing, finishing or complete
machining. Turning is run paraxially with roughing.
The cycle can be used for inside and outside machining. If the start
diameter
Q491 is larger than the end diameter Q493, the cycle
runs outside machining. If the start diameter
Q491 is less than the
end diameter
Q493, the cycle runs inside machining.
Roughing cycle run
In undercutting the TNC runs the infeed with feed rate Q478. The
return movements are then each at set-up clearance.
1 The TNC runs a paraxial infeed motion at rapid traverse. The
infeed value is calculated by the TNC with
Q463 MAX. CUTTING
DEPTH.
2 The TNC cuts the area between the starting position and the
end point in traverse direction at the defined feed rate.
3 The TNC returns the tool at the defined feed rate
Q478 by one
infeed value.
4 The TNC positions the tool back at rapid traverse to the
beginning of cut.
5 The TNC repeats this process (1 to 4) until the final contour is
completed.
6 The TNC positions the tool back at rapid traverse to the cycle
starting point.