Table of Contents
Advertisement
Cycle parameters
U
Milling depth Q1 (incremental): Distance between
workpiece surface and bottom of pocket. Input range
-99999.9999 to 99999.9999
U
Path overlap factor Q2: Q2 x tool radius = stepover
factor k. Input range -0.0001 to 1.9999.
U
Finishing allowance for side Q3 (incremental):
Finishing allowance in the working plane. Input range:
-99999.9999 to 99999.9999
U
Finishing allowance for floor Q4
(incremental): Finishing allowance in the tool axis.
Input range -99999.9999 to 99999.9999
U
Workpiece surface coordinate Q5 (absolute):
Absolute coordinate of the workpiece surface. Input
range -99999.9999 to 99999.9999
U
Setup clearance Q6 (incremental): Distance between
tool tip and workpiece surface. Input range 0 to
99999.9999, alternatively PREDEF
U
Clearance height Q7 (absolute): Absolute height at
which the tool cannot collide with the workpiece (for
intermediate positioning and retraction at the end of
the cycle). Input range -99999.9999 to 99999.9999,
alternatively PREDEF
U
Inside corner radius Q8: Inside "corner" rounding
radius; entered value is referenced to the path of the
tool center. Q8 is not a radius that is inserted as a
separate contour element between programmed
elements! Input range 0 to 99999.9999
U
Direction of rotation? Q9: Machining direction for
pockets.
Q9 = –1 up-cut milling for pocket and island
Q9 = +1 climb milling for pocket and island
Alternative: PREDEF
You can check the machining parameters during a program
interruption and overwrite them if required.
HEIDENHAIN iTNC 530
Example: NC blocks
57 CYCL DEF 20 CONTOUR DATA
Q1=-20
;MILLING DEPTH
Q2=1
;TOOL PATH OVERLAP
Q3=+0.2
;ALLOWANCE FOR SIDE
Q4=+0.1
;ALLOWANCE FOR FLOOR
Q5=+30
;SURFACE COORDINATE
Q6=2
;SETUP CLEARANCE
Q7=+80
;CLEARANCE HEIGHT
Q8=0.5
;ROUNDING RADIUS
Q9=+1
;DIRECTION
191
Hide quick links:
Advertisement
Table of Contents
Need help?
Do you have a question about the ITNC 530 - CYCLE PROGRAMMING and is the answer not in the manual?
Questions and answers
Can I change the approach direction when cycle def a stud to avoid obstruction to the right
The provided context does not explicitly mention changing the approach direction to avoid obstruction. However, it describes selecting different axis configurations using the MOD function in the Programming and Editing mode. If modifying the axis configuration allows for adjusting the approach direction, it may be possible. Otherwise, specific cycle parameters should be checked in the programming manual.
This answer is automatically generated