Official GSK Agents in South Africa
Tel: +27 11 626 2720, [email protected]
Chapter 3 G Commands
123
Ⅰ
Programming
Program: O0006;
G99 G00 X200 Z10 M03 S500; (Specify feedrate per rev and position starting point and
start spindle)
G73 U1.0 W1.0 R3 ; (X tool retraction with 2mm, Z 1mm)
G73 P14 Q19 U0.5 W0.3 F0.3 ; (X roughing with 0.5 allowance and Z 0.3mm)
N14 G00 X80 W-40 ;
G01 W-20 F0.15 S600 ;
X120 W-10 ;
W-20 ; Blocks for finishing
G02 X160 W-20 R20 ;
N19 G01 X180 W-10 ;
G70 P14 Q19 M30; (Finishing)
3.22.4 Finishing Cycle G70
Command format:
G70 P(ns) Q(nf) ;
Command function:
The tool executes the finishing of workpiece from starting point along with
the finishing path defined by ns
～
nf blocks. After executing G71, G72 or
G73 to roughing, execute G70 to finishing and single cutting of finishing
allowance is completed. The tool returns to starting point and execute the
next block following G70 block after G70 cycle is completed.
ns: Block number of the first block of finishing path.
nf: Block number of the last block of finishing path.
G70 path is defined by programmed one of ns
～
nf blocks. Relationships of relative position
of ns, nf block in G70
～
G73 blocks are as follows:
G71/G72/G73 ……
；
N (ns)
．．．．．．
．．．．．．．．
· F
· S Blocks for finishing path
·
·
N (nf)……
．．．
G70 P(ns) Q(nf)
；
Command specifications:
1. ns
～
nf blocks in programming must be followed G70 blocks.
2. F, S, T in ns
～
nf blocks are valid when executing ns
～
nf to command G70 finishing
cycle.
3. G96, G97, G98, G99, G40, G41, G42 are valid in G70;
4. When G70 is executed, the system can stop the automatic run and manual traverse, but
return to the position before manual traversing when G70 is executed again, otherwise,
the following path will be wrong.
5. When the system is executing the feed hold or single block, the program pauses after
the system has executed end point of current path.
