HEIDENHAIN TNC 410 User Manual

Page 159

8 Programming: Cycles

146

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 (4 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 in mm/min when moving to depth. If you are
plunge-cutting into the material, enter a lower value
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.

Workpiece surface coordinate Q203 (absolute value):
Coordinate of the workpiece surface

8.4 Cy

cles f

or Milling P

ets,

uds and Slots

Q200

Q201

Q206

Q202

Q203

Q204

Example NC blocks:

42 CYCL DEF 214 CIRCULAR POCKET FINISHING

Q200=2

;SET-UP CLEARANCE

Q201=-20

;DEPTH

Q206=150

;FEED RATE FOR PLUNGING

Q202=5

;PLUNGING DEPTH

Q207=500

;FEED RATE FOR MILLING

Q203=+0

;SURFACE COORDINATE

Q204=50

;2. SET-UP CLEARANCE

Q216=+50

;CENTER IN 1ST AXIS

Q217=+50

;CENTER IN 2ND AXIS

Q222=79

;WORKPIECE BLANK DIA.

Q223=80

;FINISHED PART DIA.