Programming instructions

ADT-CNC4620 Programming Manual
- 52 -
3.6.4. Finishing cycle G70
Instruction format:G70 P(ns) Q(nf);
P(ns): the number of the first block of the finishing track;
Q(nf): the number of the last block of the finishing track;
Instruction function: the tool starts finishing from the start position along the workpiece
finishing track specified by ns~nf block. After G71, G72 or G73 roughing,
finish with G70 instruction, and complete the cutting of finishing margin in one
time. After G70 cycle, the tool returns to the start point and executes the next
block after G70.
G70 instruction track depends on the programming track of ns~nf block. The relationship of
ns and nf in G70~g73 block is as follow:
, , , , , , , ,
G71/G72/G73 ……;
N(ns) , , , , , ,
, , , , , , , ,
· F_
· S_
· T_ Finishing path block
·
·
N(nf) … … …
G70 P(ns)
Q(nf)) ;
Note:
● F, S and T instructions in ns~nf block are valid when executing G70;
● While executing G70 instruction, it is possible to stop automatic running and move
manually; however, when G70 cycle is executed again, it is required to return to the
position before manual movement. If not, it will continue the execution and following
running track will be dislocated.
● ns~nf block can’t have the following instructions:
Other group oo G instructions except G04 (pause);
Other group 01 instruction except G00, G01, G02 and G03;
Subroutine calling instruction (e.g. M98/M99).
3.6.5. Axial grooving multi-cycle G74
Instruction format: G74 R (e);
G74 X/U _ Z/W_ P(Δi)
Q(Δk) R(Δd) F_ ;
R(e ): axial (Z axis) tool retreating, unsigned
X/U: groove end coordinates (X is absolute coordinates, and U is the increment from
current coordinates to point coordinates)
Z/W: groove end coordinates (Z is absolute coordinates and W is the increment from
current coordinates to point coordinates)