Contour Train (Cycle 25, Din/Iso: G125, Software Option 19); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 620 User Manual

7
Fixed Cycles: Contour Pocket
7.9 CONTOUR TRAIN (Cycle 25, DIN/ISO: G125)
7.9 CONTOUR TRAIN (Cycle 25, DIN/ISO:
G125, software option 19)

Cycle run

In conjunction with Cycle 14 CONTOUR GEOMETRY, this cycle
facilitates the machining of open and closed contours.
Cycle 25 CONTOUR TRAIN offers considerable advantages over
machining a contour using positioning blocks:
The TNC monitors the operation to prevent undercuts and
surface blemishes. It is recommended that you run a graphic
simulation of the contour before execution.
If the radius of the selected tool is too large, the corners of the
contour may have to be reworked.
The contour can be machined throughout by up-cut or by climb
milling. The type of milling even remains effective when the
contours are mirrored.
The tool can traverse back and forth for milling in several
infeeds: This results in faster machining.
Allowance values can be entered in order to perform repeated
rough-milling and finish-milling operations.

Please note while programming:

The algebraic sign for the cycle parameter DEPTH
determines the working direction. If you program
DEPTH=0, the cycle will not be executed.
The TNC takes only the first label of Cycle 14
CONTOUR GEOMETRY into account.
The sub program allows no APPR- or DEP motions.
When you use local QL Q parameters in a contour
subprogram you must also assign or calculate these
in the contour subprogram.
The memory capacity for programming an SL cycle
is limited. You can program up to 16384 contour
elements in one SL cycle.
Cycle 20 CONTOUR DATA is not required.
If M110 is activated during operation, the feed rate
of compensated circular arcs within will be reduced
accordingly.
208
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 9/2015