Circular Pocket Finishing (Cycle 214) - HEIDENHAIN TNC 426 B User Manual

CIRCULAR POCKET FINISHING (Cycle 214)

1 The TNC automatically moves the tool in the tool axis to set-up
clearance, or — if programmed — to the 2nd set-up clearance,
and subsequently to the center of the pocket.
2 From the pocket center, the tool moves in the working plane to
the starting point for machining. The TNC takes the workpiece
blank diameter and tool radius into account for calculating the
starting point. If you enter a workpiece blank diameter of 0, the
TNC plunge-cuts into the pocket center.
3 If the tool is at the 2nd set-up clearance, it moves in rapid traverse
FMAX to set-up clearance, and from there advances to the first
plunging depth at the feed rate for plunging.
4 The tool then moves tangentially to the contour of the finished
part and, using climb milling, machines one revolution.
5 After this, the tool departs the contour tangentially and returns to
the starting point in the working plane.
6 This process (3 to 5) is repeated until the programmed depth is
reached.
7 At the end of the cycle, the TNC retracts the tool in FMAX to set-
up clearance, or - if programmed - to the 2nd set-up clearance,
and finally to the center of the pocket (end position = starting
position).
Before programming, note the following:
The algebraic sign for the depth parameter determines
the working direction.
If you want to clear and finish the pocket with the same
tool, use a center-cut end mill (ISO 1641) and enter a low
feed rate for plunging.
Set-up clearance Q200 (incremental value): Distance
between tool tip and workpiece surface.
Depth Q201 (incremental value): Distance between
workpiece surface and bottom of pocket
Feed rate for plunging Q206: Traversing speed of the
tool im mm/min when moving to depth. If you are
plunge-cutting into the material, enter a value lower
than that defined in Q207
Plunging depth Q202 (incremental value):
Infeed per cut
Feed rate for milling Q207: Traversing speed of the
tool in mm/min while milling.
HEIDENHAIN TNC 426 B, TNC 430
www.EngineeringBooksPdf.com
Y
Q206
Z
Q200
Q203
Q202
Example NC blocks:
42 Y L DEF 214 IR ULAR PO KET FINISHING
Q200=2 ;SET-UP
Q201=-20 ;DEPTH
Q206=150 ;FEED RATE FOR PLUNGING
Q202=5 ;PLUNGING DEPTH
Q207=500 ;FEED RATE FOR MILLING
Q203=+0 ;SURFA E
Q204=50 ;2. SET-UP
Q216=+50 ; ENTER IN 1ST AXIS
Q217=+50 ; ENTER IN 2ND AXIS
Q222=79 ;WORKPIE E BLANK DIA.
Q223=80 ;FINISHED PART DIA.
X
Q204
Q201
X
LEARAN E
OORDINATE
LEARAN E
175