Circular Stud (Cycle 257, Din/Iso: G257, Software Option 19); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 620 User Manual

5
Fixed cycles: Pocket milling / stud milling / slot milling
5.7

CIRCULAR STUD (Cycle 257, DIN/ISO: G257, software option 19)

5.7 CIRCULAR STUD (Cycle 257, DIN/ISO:
G257, software option 19)

Cycle run

Use Cycle 257 to machine a circular stud. If the diameter of the
workpiece blank is greater than the maximum possible stepover,
then the TNC performs multiple stepovers until the finished
diameter has been machined.
1 The tool moves from the cycle starting position (stud center) to
the starting position for stud machining. With the polar angle
you specify the starting position with respect to the stud center
using parameter Q376.
2 If the tool is at the 2nd set-up clearance, it moves at rapid
traverse FMAX to the set-up clearance, and from there advances
to the first plunging depth at the feed rate for plunging.
3 The tool then moves tangentially on a helical path to the stud
contour and machines one revolution.
4 If the finished diameter cannot be machined with one
revolution, the TNC performs helical infeed movements until the
finished diameter is reached. The TNC takes the dimensions of
the workpiece blank diameter, the finished diameter, and the
permitted stepover into account.
5 The TNC retracts the tool on a helical path from the contour.
6 If more than one plunging movement is required, the tool
repeats the plunging movement at the point next to the
departure movement.
7 This process is repeated until the programmed stud depth is
reached.
8 At the end of the cycle, the TNC positions the tool—after the
helical departure movement—in the tool axis to the 2nd set-up
clearance defined in the cycle

Please note while programming:

Pre-position the tool in the machining plane to
the starting position (stud center) with radius
compensation R0.
The TNC automatically pre-positions the tool in the
tool axis. Note the 2nd set-up clearance Q204.
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH=0, the cycle will not be executed.
At the end of the cycle, the TNC returns the tool to
the starting position.
The TNC reduces the infeed depth to the LCUTS tool
length defined in the tool table if the tool length is
shorter than the Q202 infeed depth programmed in
the cycle.
154
TNC 620 | User's Manual Cycle Programming | 3/2014