Mitsubishi Electric M700V Series Manual page 226

MITSUBISHI CNC
III Functional Specifications
12.1.3.6 Compound Type Fixed Cycle for Turning Machining (Type II)
M720VW
M system ―
L system △
Pocket shapes can be machined in the longitudinal rough cutting cycle (G71) and face rough cutting cycle
(G72).
The cutting method differs according to whether pocket machining is ON or OFF.
Pocket machining OFF ....... Method to pull up the tool in a 45-degree direction from the workpiece
Pocket machining ON ......... Method that traces the shape (After executing the last trace, the tool is
pulled up in the X axis
Pocket machining is designated with the program (H address) or parameter.
Command format (This is a command format when the G71 is commanded. The G72 command is based on
the G71 command.)
G71 Ud Re Hh ; <- (can be omitted when values set in parameters are used)
G71 Aa Pp Qq Uu Ww Ff Ss Tt ;
<H0:Used for finished shapes without pockets>
G71 Ud Re H 0;
. .
G71 Pp Qq ;
q
X
(R)
(f)
e
45°
(f)
Z
(a) Rough cutting start point
: Cut amount (modal) ........................ Reversible parameter
Ud
Increment : μm or 1/10000inch ..... Radius value command
: Retract amount (modal) .................. Reversible parameter
Re
Increment : μm or 1/10000inch .... Radius value command
Hh : Pocket machining (modal) ............. Reversible parameter
0 : Select this only for finished shapes without hollow areas (pockets).
With the beginning of the pockets, the tool is pulled up in the 45-degree direction with each cycle until the
finished shape is finally traced.
1 : This can be selected regardless of whether the finished shape has hollow (pocket) parts or not.
A method that traces the finished shape with each cycle is used for the beginning of the pockets.
Depending on the parameter setting, pocket machining ON/OFF is automatically determined by the number
of axes in the finish shape start block.
Aa : Finish shape program No. (If omitted, the program being executed is designated.)
If the A command is omitted, the program being executed are applied.
If A is omitted, the program following the end of this cycle will be executed at the block after Qq
(finish shape end sequence No.).
A file name can be designated instead of address A by enclosing the file name in brackets <>.
(The file name can have up to 32 characters, including the extension.)
Pp : Finish shape start sequence number (Head of program if omitted.)
Qq : Finish shape end sequence number (To end of program if omitted.)
If M99 precedes the Q command, up to M99.
Uu : Finishing allowance in X axis direction (If omitted, finishing allowance in X axis direction is handled as 0.)
Increment : μm or 1/10000inch ....... Diameter/radius value command follows changeover parameter.
Ww
: Finishing allowance in Z axis direction (If omitted, finishing allowance in Z axis direction is handled as 0.)
Increment : μm or 1/10000inch ......... Radius value command
Ff
: Cutting feed rate (If omitted, cutting feed rate (modal) before G73 is applied.)
Ss, Tt
: Spindle command, tool command
III - 224
M730VW M750VW
― ―
△ △
direction.)
(R)
(R)
(a)
(R/f)
d
(f)
u / 2
p
w
M720VS M730VS M750VS
― ―
△ △
<H1:Mainly used for finished shapes with pockets>
G71 Ud Re H 1;
..
G71 Pp Qq ;
q
(f)
X
(R)
(f)
(b)
e
Z
(a) Rough cutting start point
(b) Hole bottom
―
△
(R)
(R)
(a)
(R/f)
d
u/2
p
w