GSK 980TDi, User Manual

Page: 130 / 570

Official GSK Agents in South Africa
Tel: +27 11 626 2720, design@efamatic.com
GSK980TDi Turning CNC System User Manual
114
Ⅰ
Programming
Program: O0004;
G00 X200 Z10 M3 S800; (Spindle clockwise with 800 r/min)
G71 U2 R1 F200; (Cutting depth each time 4mm, tool retraction 2mm [in
diameter])
G71 P80 Q120 U0.5 W0.2; (roughing a---e, machining allowance: X, 1mm;Z, 2mm)
N80 G00 X40 S1200; (Positioning)
G01 Z-30 F100 ;
(a → b)
X60 W-30;
(b → c)
a → b → c → d → e blocks for finishing path
W-20;
(c → d)
N120 X100 W-10;
(d → e)
G70 P80 Q120; (a---e blocks for finishing path)
M30; (End of block)
3.22.2 Radial Roughing Cycle G72
Command format
：
G72 W( Δ d) R(e) F S T
； ⑴
G72 P(ns) Q(nf) U( Δ u) W( Δ w) K0/1 J0/1
； ⑵
N(ns) G00(G01) X(U)_
；
N(ns) G00(G01) X(U)_ Z(W)_
．．．
F
； ．．．
F
；
．．．
S
；
type I
⑶ ．．．
S
；
type II
⑶
．．． ．．．
N(nf) ．．．．．； N(nf) ．．．．．；
Command function: G72 is divided into three parts:
⑴
1st blocks for defining the travels of tool infeed and tool retraction, the cutting speed, the
spindle speed and the tool function in roughing;
⑵
2nd blocks for defining the block interval, finishing allowance;
⑶
3rd blocks for some continuous finishing path, counting the roughing path without being
executed actually when G72 is executed.
According to the finishing path, the finishing allowance, the path of tool infeed and retract tool,
the system automatically counts the path of roughing, the tool cuts the workpiece in paralleling with Z,
and the roughing is completed by multiple executing the cutting cycle tool infeed
→ cutting feed → tool
retraction. The starting point and the end point of G72 are the same one. The command is applied to
the formed roughing of non-formed rod.
Relevant definitions:
Finishing path:
the above-mentioned Part
⑶
of G71 ( ns
～
nf block)defines the finishing path,
and the starting point of finishing path (i.e. starting point of ns block)is the same
these of starting point and end point of G72, called A point; the first block of
finishing path(ns block)is used for Z rapid traversing or cutting feed, and the end
point of finishing path is called to B point; the end point of finishing path(end
point of nf block)is called to C point. The finishing path is A
→ B → C.
Roughing path : The finishing path is the one after offsetting the finishing allowance Δ u, Δ w) and
is the path contour formed by executing G72. A, B, C point of finishing path after
offset corresponds separately to A’, B’, C’ point of roughing path, and the final
continuous cutting path of G72 is B’
→ C’ point.
Δ d: it is Z cutting in roughing, its value: 0.001~99.999 （ IS_B ） /0.0001~99.9999 （ IS_C ） (unit: