Cycle Parameters - HEIDENHAIN TNC 620 User Manual

7
Fixed Cycles: Contour Pocket | THREE-D CONT. TRAIN (Cycle 276, DIN/ISO: G276, software option 19)

Cycle parameters

Q1 Milling depth? (incremental): Distance
between workpiece surface and contour bottom.
Input range -99999.9999 to 99999.9999
Q3 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane. Input
range -99999.9999 to 99999.9999
Q7 Clearance height? (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
Q10 Plunging depth? (incremental): Infeed per
cut. Input range -99999.9999 to 99999.9999
Q11 Feed rate for plunging?: Traversing speed
of the tool in the spindle axis. Input range 0 to
99999.9999, alternatively FAUTO, fu, FZ
Q12 Feed rate for roughing?: Traversing speed
of the tool in the working plane. Input range 0 to
99999.9999, alternatively FAUTO, fu, FZ
Q15 Climb or up-cut? up-cut = -1:
Climb milling: Input value = +1
Up-cut milling: Input value = –1
Climb milling and up-cut milling alternately in
several infeeds: Input value = 0
Q18 Coarse roughing tool? or QS18: Number or
name of the tool with which the TNC has already
coarse-roughed the contour. You are able to apply
the coarse roughing tool via soft key directly
from the tool table. In addition, you can enter
the tool name via the soft key tool name. 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 99999 if a number is entered;
maximum 16 characters if a name is entered.
236
NC blocks
62 CYCL DEF 276 THREE-D CONT. TRAIN
Q1=-20
Q3=+0
Q7=+50
Q10=-5
Q11=150
Q12=500
Q15=+1
Q18=0
Q446=+0.01;RESIDUAL MATERIAL
Q447=+10
Q448=+2
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
;MILLING DEPTH
;ALLOWANCE FOR SIDE
;CLEARANCE HEIGHT
;PLUNGING DEPTH
;FEED RATE FOR PLNGNG
;FEED RATE F. ROUGHNG
;CLIMB OR UP-CUT
;COARSE ROUGHING
TOOL
;CONNECTION DISTANCE
;PATH EXTENSION