Cycle Parameters - HEIDENHAIN TNC 620 User Manual

3
Fixed Cycles: Drilling
3.3 DRILLING (Cycle 200)

Cycle parameters

Set-up clearance Q200 (incremental): Distance
between tool tip and workpiece surface. Enter a
positive value. Input range 0 to 99999.9999
Depth Q201 (incremental): Distance between
workpiece surface and bottom of hole. Input range
-99999.9999 to 99999.9999
Feed rate for plunging Q206: Traversing speed of
the tool in mm/min during drilling. Input range 0 to
99999.999, alternatively FAUTO, FU
Plunging depth Q202 (incremental): Infeed per cut.
Input range 0 to 99999.9999. The depth does not
have to be a multiple of the plunging depth. The
TNC will go to depth in one movement if:
Dwell time at top Q210: Time in seconds that the
tool remains at set-up clearance after having been
retracted from the hole for chip removal. Input range
0 to 3600.0000
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
Dwell time at depth Q211: Time in seconds that
the tool remains at the hole bottom. Input range 0 to
3600.0000
Depth reference Q395: Select whether the entered
depth is referenced to the tool tip or the cylindrical
part of the tool. If the TNC is to reference the depth
to the cylindrical part of the tool, the point angle of
the tool must be defined in the T ANGLE column of
the tool table TOOL.T.
0
1
tool
70
the plunging depth is equal to the depth
the plunging depth is greater than the depth
= Depth referenced to the tool tip
= Depth referenced to the cylindrical part of the
NC blocks
11 CYCL DEF 200 DRILLING
Q200=2 ;SET-UP CLEARANCE
Q201=-15 ;DEPTH
Q206=250 ;FEED RATE FOR
PLNGNG
Q202=5 ;PLUNGING DEPTH
Q211=0 ;DWELL TIME AT TOP
Q203=+20 ;SURFACE COORDINATE
Q204=100 ;2ND SET-UP
CLEARANCE
Q211=0.1 ;DWELL TIME AT
BOTTOM
Q395=0 ;DEPTH REFERENCE
12 L X+30 Y+20 FMAX M3
13 CYCL CALL
14 L X+80 Y+50 FMAX M99
TNC 620 | User's Manual Cycle Programming | 3/2014