Axial Recessing (Cycle 850, Din/Iso: G850); Application; Roughing Cycle Run - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | AXIAL RECESSING
(Cycle 850, DIN/ISO: G850)
12.21 AXIAL RECESSING
(Cycle 850, DIN/ISO: G850)

Application

This cycle enables you to recess right-angled slots of any form in
longitudinal direction. With recess turning, a recessing traverse
to plunging depth and then a roughing traverse is alternatively
machined.
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
starting point of the contour is larger than the end point of the
contour, the cycle runs outside machining. If the contour starting
point is less than the end point, 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
the contour starting point, the TNC positions the tool in the Z
coordinate to the contour starting point and begins the cycle there.
1 The TNC positions the tool at rapid traverse in the X coordinate
(first cut-in position).
2 The TNC recesses until the first plunging depth.
3 The TNC cuts the area between the starting position and the
end point in traverse direction at the defined feed rate Q478.
4 If the input parameter
elements are machined at the programmed feed rate for
plunging.
5 If only one machining direction Q507=1 was specified in
the cycle, the TNC retracts the tool by the set-up clearance,
positions the tool back at rapid traverse and approaches the
contour again with the defined feed rate. With machining
direction Q507=0, infeed is on both sides.
6 The tool recesses to the next plunging depth.
7 The TNC repeats this process (2 to 4) until the slot depth is
reached.
8 The TNC returns the tool to set-up clearance and machines a
recessing traverse on both side walls.
9 The TNC positions the tool back at rapid traverse to the cycle
starting point.
HEIDENHAIN | User's manual for cycle programming | 10/2017
Q488 is defined in the cycle, plunging
12
433