Three-D Cont. Train (Cycle 276, Din/Iso: G276); Cycle Run - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Contour Pocket | THREE-D CONT. TRAIN (Cycle 276, DIN/ISO: G276)
7.10 THREE-D CONT. TRAIN (Cycle 276, DIN/
ISO: G276)

Cycle run

This cycle in conjunction with Cycle 14 CONTOUR and Cycle 270
CONTOUR TRAIN DATA enables open and closed contours to
be machined. You can also work with automatic residual material
detection. This way you can subsequently complete e.g. inside
corners with a smaller tool.
Cycle 276 THREE-D CONT. TRAIN also machines coordinates of the
tool axis defined in the contour subprogram, in contrast to Cycle 25
CONTOUR TRAIN. This cycle can thus machine three-dimensional
contours.
You should program Cycle 270 CONTOUR TRAIN DATA before
Cycle 276 THREE-D CONT. TRAIN.
Machining a contour without infeed: Milling depth Q1=0
1 The tool traverses to the starting point for machining. This
starting point results from the first contour point, the selected
climb or up-cut and the parameters from the previously defined
Cycle 270 CONTOUR TRAIN DATA, e.g. the type of approach.
The TNC moves the tool to the first plunging depth
2 The TNC approaches the contour according to the previously
defined Cycle 270 CONTOUR TRAIN DATA and then performs
machining until the end of the contour
3 At the end of the contour the departure movement is performed
as defined in Cycle 270 CONTOUR TRAIN DATA
4 Finally, the TNC retracts the tool to the clearance height.
Machining a contour with infeed: Milling depth Q1 not equal to 0
and plunging depth Q10 are defined
1 The tool traverses to the starting point for machining. This
starting point results from the first contour point, the selected
climb or up-cut and the parameters from the previously defined
Cycle 270 CONTOUR TRAIN DATA, e.g. the type of approach.
The TNC moves the tool to the first plunging depth
2 The TNC approaches the contour according to the previously
defined Cycle 270 CONTOUR TRAIN DATA and then performs
machining until the end of the contour
3 If machining in climb milling and up-cut milling is selected
(Q15=0), the TNC performs a reciprocating movement. It
executes the infeed motion at the end and at the starting point
of the contour. If Q15 is not equal to 0, the TNC moves the
tool to clearance height and returns it to the starting point of
machining. From there it moves the tool to the next plunging
depth
4 The departure movement is performed as defined in Cycle 270
CONTOUR TRAIN DATA
5 This process is repeated until the programmed depth is reached
6 Finally, the TNC retracts the tool to the clearance height
HEIDENHAIN | User's manual for cycle programming | 10/2017
7
241