Reaming (Cycle 201, Din/Iso: G201); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Drilling | REAMING (Cycle 201, DIN/ISO: G201)
3.4

REAMING (Cycle 201, DIN/ISO: G201)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse
FMAX to the entered set-up clearance above the workpiece
surface.
2 The tool reams to the entered depth at the programmed feed
rate F.
3 If programmed, the tool remains at the hole bottom for the
entered dwell time.
4 The tool then retracts to set-up clearance at the feed rate F , and
from there—if programmed—to the 2nd set-up clearance in
FMAX.

Please note while programming:

Program a positioning block for the starting point (hole
center) in the working plane with radius compensation
R0.
The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH=0, the cycle will not be executed.
Danger of collision!
If you enter a positive depth with a cycle, the TNC reverses
calculation of the pre-positioning. This means that the tool
moves at rapid traverse in the tool axis to set-up clearance
below the workpiece surface!
Enter depth as negative
Enter in machine parameter displayDepthErr (No. 201003)
whether the TNC should output an error message (on) or not
(off) if a positive depth is entered
HEIDENHAIN | User's manual for cycle programming | 10/2017
NOTICE
3
83