Table of Contents
Advertisement
Cycle parameters
U
Nominal diameter Q335: Nominal thread diameter.
Input range 0 to 99999.9999
U
Thread pitch Q239: Pitch of the thread. The algebraic
sign differentiates between right-hand and left-hand
threads:
+= right-hand thread
– = left-hand thread
Input range -99.9999 to 99.9999
U
Thread depth Q201 (incremental): Distance between
workpiece surface and root of thread. Input range -
99999.9999 to 99999.9999
U
Threads per step Q355: Number of thread revolutions
by which the tool is moved:
0 = one 360° helical line to the thread depth
1 = continuous helical path over the entire length of
the thread
>1 = several helical paths with approach and
departure; between them, the TNC offsets the tool by
Q355, multiplied by the pitch. Input range 0 to 99999
U
Feed rate for pre-positioning Q253: Traversing
speed of the tool in mm/min when plunging into the
workpiece, or when retracting from the workpiece.
Input range 0 to 99999.999 alternatively FMAX, FAUTO,
PREDEF.
U
Climb or up-cut Q351: Type of milling operation with
M3
+1 = climb milling
–1 = up-cut milling
Alternatively PREDEF
U
Setup clearance Q200 (incremental): Distance
between tool tip and workpiece surface. Input range
0 to 99999.9999, alternatively PREDEF
U
Workpiece surface coordinate Q203 (absolute):
Coordinate of the workpiece surface. Input range:
-99999.9999 to 99999.9999
U
2nd setup 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
U
Feed rate for milling Q207: Traversing speed of the
tool during milling in mm/min. Input range: 0 to
99999.999, alternatively FAUTO.
HEIDENHAIN iTNC 530
Example: NC blocks
25 CYCL DEF 262 THREAD MILLING
Q335=10
;NOMINAL DIAMETER
Q239=+1.5 ;PITCH
Q201=-20 ;DEPTH OF THREAD
Q355=0
;THREADS PER STEP
Q253=750 ;F PRE-POSITIONING
Q351=+1
;CLIMB OR UP-CUT
Q200=2
;SETUP CLEARANCE
Q203=+30 ;SURFACE COORDINATE
Q204=50
;2ND SETUP CLEARANCE
Q207=500 ;FEED RATE FOR MILLING
119
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