Turn, Longitudinal Plunge Extended (Cycle 814, Din/Iso: G814); Application; Roughing Cycle Run - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | TURN, LONGITUDINAL PLUNGE EXTENDED
(Cycle 814, DIN/ISO: G814)
12.8 TURN, LONGITUDINAL PLUNGE
EXTENDED
(Cycle 814, DIN/ISO: G814)

Application

This cycle enables you to run longitudinal turning of shoulders with
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

The TNC uses the tool position as cycle starting point when a cycle
is called. If the Z coordinate of the starting point is less than Q492
Contour start in Z, the TNC positions the tool in the Z coordinate
to set-up clearance and begins the cycle there.
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 longitudinal direction at the defined feed rate Q478.
3 The TNC returns the tool at the defined feed rate 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.
HEIDENHAIN | User's manual for cycle programming | 10/2017
12
385