HEIDENHAIN TNC 640 (34059x-05) Cycle programming - Manual (Page 201)

ROUGHING (Cycle 22, DIN/ISO: G122) 7.6
7
TNC 640 | User's Manual Cycle Programming | 1/2015
201
Cycle parameters
Plunging depth Q10 (incremental): Infeed per cut.
Input range -99999.9999 to 99999.9999
Feed rate for plunging Q11: Traversing speed
of the tool in the spindle axis. Input range 0 to
99999.9999, alternatively
FAUTO, FU, FZ
Feed rate for milling Q12: Traversing speed of
the tool in the working plane. Input range 0 to
99999.9999, alternatively
FAUTO, FU, FZ
Coarse roughing tool Q18 or QS18: Number or
name of the tool with which the TNC has already
coarse-roughed the contour. Switch to the name
input: Press the
TOOL NAME soft key. The TNC
automatically inserts the closing quotation mark
when you exit the input field. If there was no coarse
roughing, enter "0"; if you enter a number or a
name, the TNC will only rough-out the portion that
could not be machined with the coarse roughing
tool. If the portion that is to be roughed cannot
be approached from the side, the TNC will mill in
a reciprocating plunge-cut; for this purpose you
must enter the tool length
LCUTS in the tool table
TOOL.T and define the maximum plunging
ANGLE
of the tool. Otherwise, the TNC will display an
error message. Input range 0 to 99999 if a number
is entered; maximum 16 characters if a name is
entered.
Reciprocation feed rate Q19: Traversing speed of
the tool in mm/min during reciprocating plunge cut.
Input range 0 to 99999.9999; alternatively
FAUTO,
FU, FZ
Retraction feed rate Q208: Traversing speed of
the tool in mm/min when retracting after machining.
If you enter Q208 = 0, the TNC retracts the tool at
the feed rate in Q12. Input range 0 to 99999.9999,
alternatively
FMAX,FAUTO
NC blocks
59 CYCL DEF 22 ROUGH-OUT
Q10=+5 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR
PLNGNG
Q12=750 ;FEED RATE FOR
MILLING
Q18=1 ;COARSE ROUGHING
TOOL
Q19=150 ;RECIPROCATION FEED
RATE
Q208=9999 ;RETRACTION FEED
RATE
Q401=80 ;FEED RATE REDUCTION
Q404=0 ;FINE ROUGH
STRATEGY