Cycle Parameters - HEIDENHAIN TNC 640 User Manual
Hide thumbs
Also See for TNC 640:
- User manual (948 pages) ,
- User manual (903 pages) ,
- Operating instructions manual (64 pages)
Table of Contents
Advertisement
4
Cycle parameters
Q335 Nominal diameter?: Thread nominal
diameter. Input range 0 to 99999.9999
Q239 Pitch?: Pitch of the thread. The algebraic
sign differentiates between right-hand and left-
hand threads:
+
–= left-hand thread
Input range -99.9999 to 99.9999
Q201 Depth of thread? (incremental): Distance
between workpiece surface and root of thread.
Input range -99999.9999 to 99999.9999
Q355 Number of threads per step?: Number of
thread grooves by which the tool is shifted:
0
1
length
>1
departure; between these the TNC shifts the tool
by Q355 multiplied by the pitch. Input range 0 to
99999
Q253 Feed rate for pre-positioning?: Traversing
speed of the tool in mm/min when plunging
into the workpiece, or when retracting from
the workpiece. Input range 0 to 99999.9999
alternatively fmax, FAUTO
Q351 Direction? Climb=+1, Up-cut=-1: Type of
milling operation with M3
+1
–1
performed)
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Input
range 0 to 99999.9999
Q203 Workpiece surface coordinate? (absolute):
Coordinate of the workpiece surface. Input range
-99999.9999 to 99999.9999
Q204 2nd set-up clearance? (incremental):
Coordinate in the spindle axis at which no collision
between tool and workpiece (fixtures) can occur.
Input range 0 to 99999.9999
Q207 Feed rate for milling?: Traversing speed of
the tool in mm/min while milling. Input range 0 to
99999.999 alternatively FAUTO
Q512 Feed rate for approaching?: Traversing
speed of the tool in mm/min while approaching.
For smaller thread diameters you can decrease
the approaching feed rate in order to reduce
the danger of tool breakage. Input range 0 to
99999.999 alternatively FAUTO
138
Fixed Cycles: Tapping / Thread Milling | THREAD MILLING (Cycle 262, DIN/ISO: G262)
= right-hand thread
= one helix on the thread depth
= continuous helix on the complete thread
= several helical paths with approach and
= Climb milling
= Up-cut milling (if you enter 0, climb milling is
NC blocks
25 CYCL DEF 262 THREAD MILLING
Q335=10
;NOMINAL DIAMETER
Q239=+1.5
;THREAD PITCH
Q201=-20
;DEPTH OF THREAD
Q355=0
;THREADS PER STEP
Q253=750
;F PRE-POSITIONING
Q351=+1
;CLIMB OR UP-CUT
Q200=2
;SET-UP CLEARANCE
Q203=+30
;SURFACE COORDINATE
Q204=50
;2ND SET-UP CLEARANCE
Q207=500
;FEED RATE FOR MILLNG
Q512=0
;FEED FOR APPROACH
HEIDENHAIN | User's manual for cycle programming | 10/2017
Advertisement
Table of Contents
