HEIDENHAIN TNC 620 User Manual page 136

5
Fixed cycles: Pocket milling / stud milling / slot milling
5.2 RECTANGULAR POCKET (Cycle 251, DIN/ISO: G251, software
option 19)
Feed rate for plunging Q206: Traversing speed of
the tool while moving to depth in mm/min. Input
range 0 to 99999.999; alternatively FAUTO, FU, FZ
Infeed for finishing Q338 (incremental): Infeed per
cut. Q338=0: Finishing in one infeed. Input range 0
to 99999.9999
Set-up clearance Q200 (incremental): Distance
between tool tip and workpiece surface. Input range
0 to 99999.9999; alternatively PREDEF
Coordinate of workpiece surface Q203 (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
2nd set-up clearance Q204 (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999; alternatively PREDEF
Path overlap factor Q370: Q370 x tool radius
= stepover factor k. Input range: 0.1 to 1.414;
alternatively PREDEF
Plunging strategy Q366: Type of plunging strategy:
0: vertical plunging. The TNC plunges
perpendicularly, regardless of the plunging angle
ANGLE defined in the tool table
1: helical plunging. In the tool table, the plunging
angle ANGLE for the active tool must be defined as
not equal to 0. Otherwise, the TNC generates an
error message
2: reciprocal plunging. In the tool table, the plunging
angle ANGLE for the active tool must be defined as
not equal to 0. Otherwise, the TNC generates an
error message. The reciprocation length depends
on the plunging angle. As a minimum value the TNC
uses twice the tool diameter
PREDEF: The TNC uses the value from the GLOBAL
DEF block
Feed rate for finishing Q385: Traversing speed of
the tool during side and floor finishing in mm/min.
Input range 0 to 99999.999; alternatively FAUTO,
FU, FZ
136
NC blocks
8 CYCL DEF 251 RECTANGULAR
POCKET
Q215=0 ;MACHINING OPERATION
Q218=80 ;FIRST SIDE LENGTH
Q219=60 ;2ND SIDE LENGTH
Q220=5 ;CORNER RADIUS
Q368=0.2 ;ALLOWANCE FOR SIDE
Q224=+0 ;ANGLE OF ROTATION
Q367=0 ;POCKET POSITION
Q207=500 ;FEED RATE FOR
MILLING
Q351=+1 ;CLIMB OR UP-CUT
Q201=-20 ;DEPTH
Q202=5 ;PLUNGING DEPTH
Q369=0.1 ;ALLOWANCE FOR
FLOOR
Q206=150 ;FEED RATE FOR
PLNGNG
Q338=5 ;INFEED FOR FINISHING
Q200=2 ;SET-UP CLEARANCE
Q203=+0 ;SURFACE COORDINATE
Q204=50 ;2ND SET-UP
CLEARANCE
Q370=1 ;TOOL PATH OVERLAP
Q366=1 ;PLUNGE
Q385=500 ;FINISHING FEED RATE
9 L X+50 Y+50 R0 FMAX M3 M99
TNC 620 | User's Manual Cycle Programming | 3/2014