HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 292)

Cycles: Turning
13.6 TURN SHOULDER LONGITUDINAL EXTENDED
(Cycle 812, DIN/ISO: G812)
13
292
TNC 640 | User's Manual Cycle Programming | 5/2013
13.6 TURN SHOULDER LONGITUDINAL
EXTENDED
(Cycle 812, DIN/ISO: G812)
Application
This cycle enables you to run longitudinal turning of shoulders.
Expanded scope of function:
You can insert a chamfer or curve at the contour start and
contour end.
In the cycle you can define angles for the face and
circumferential surfaces
You can insert a radius in 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 starting point is within the area to be machined,
the TNC positions the tool in the X coordinate and then in the Z
coordinate to set-up clearance and begins the cycle there.
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.