HEIDENHAIN TNC 320 User Manual page 184

Cycle parameters
U
Plunging depth Q10 (incremental): Infeed per cut.
Input range -99999.9999 to 99999.9999
U Feed rate for plunging Q11: Plunging feed rate in
mm/min. Input range 0 to 99999.9999; alternatively
FAUTO, FU, FZ
U
Feed rate for roughing Q12: Milling feed rate in
mm/min. Input range 0 to 99999.9999; alternatively
FAUTO, FU, FZ
U Coarse roughing tool Q18 or QS18: Number or
name of the tool with which the TNC has already
coarse-roughed the contour. Press the TOOL NAME
soft key to switch to name input. 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. The TNC will
otherwise generate an error message. Input range 0
to 32767.9 if a number is entered; maximum 16
characters if a name is entered.
U 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
U
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
184
Example: NC blocks
59 CYCL DEF 22 ROUGH-OUT
Q10=+5 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR PLNGNG
Q12=750 ;FEED RATE FOR ROUGHING
Q18=1 ;COARSE ROUGHING TOOL
Q19=150 ;RECIPROCATION FEED RATE
Q208=99999 ;RETRACTION FEED RATE
Fixed Cycles: Contour Pocket