HEIDENHAIN TNC 320 - CONTOUR TRAIN (Cycle 25, DIN;ISO: G125); Cycle Run; Please Note While Programming

CONTOUR TRAIN (Cycle 25, DIN/ISO: G125) 7.9
7
HEIDENHAIN | TNC 320 | User’s manual for cycle programming | 9/2016
205
7.9 CONTOUR TRAIN (Cycle 25, DIN/ISO:
G125)
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.
Danger of collision!
To avoid collisions,
Do not program positions in incremental
dimensions immediately after Cycle 25 since they
are referenced to the position of the tool at the
end of the cycle.
Move the tool to defined (absolute) positions in
all main axes, since the position of the tool at the
end of the cycle is not identical to the position of
the tool at the start of the cycle.