Yx z – HEIDENHAIN TNC 407 (280 580) User Manual User Manual
Page 246
8-39
8
Cycles
TNC 407/TNC 415 B/TNC 425
Fig. 8.41:
Example of an “open contour”
Y
X
Z
CONTOUR TRAIN (Cycle 25)
Process
This cycle – in combination with cycle 14 CONTOUR GEOM. – facilitates
the machining of “open” contours, where the contour does not end at its
starting point.
Cycle 25 CONTOUR TRAIN offers considerable advantages over machin-
ing an open contour using positioning blocks:
• The control monitors the operation to prevent undercuts or surface
blemishes. Please be sure 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 cutting.
The type of milling even remains effective when the contours are
mirrored.
• The tool can be traversed 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.
Cycle 25 CONTOUR TRAIN should not be used for closed contours. With closed contours, the starting point and the
end point of the contour must not be located in a contour corner.
Input data
• MILLING DEPTH Q1:
Distance between workpiece surface and contour floor. The algebraic
sign determines the working direction (a negative value means negative
working direction).
• ALLOWANCE FOR SIDE Q3:
Finishing allowance in the machining plane
• WORKPIECE SURFACE COORDINATES Q5:
Absolute coordinates of the workpiece surface referenced to the
workpiece datum
• CLEARANCE HEIGHT Q7:
Absolute height at which the tool cannot collide with the workpiece
– Position for tool retraction at the end of the cycle
• PECKING DEPTH Q10:
Dimension by which the tool is plunged in each infeed
• FEED RATE FOR PECKING Q11:
Traversing speed of the tool in the tool axis
• FEED RATE FOR MILLING Q12:
Traversing speed of the tool in the machining plane
• CLIMB OR UP-CUT Q15:
Climb milling:
Input value = +1
Conventional up-cut milling: Input value = – 1
To enable up-cut milling and climb milling alternately in several infeeds:
Input value = 0
• If you are using cycle 25 CONTOUR TRAIN, only the first label of cycle 14 CONTOUR GEOM. will be executed.
• Positions that are programmed in incremental dimensions immediately after cycle 25 are referenced to the
position of the tool at the end of the cycle.
• The subprograms can contain up to 128 contour elements each.
• Cycle 20 CONTOUR DATA is not required.