Multi cut threading macro program example using G76
Custom Macro – Using variables for the Programming :
Ideal application for the use of Variable programming (i.e. Custom Macro Programming) on a CNC Lathe :
As such the usage is covering very vast application area. You name it and it can be coded using macros. But, by and large following are the core application areas :
1) Threading applications like variable lead threading, Multi start threading,
Square and Trapezoidal threading, circular form non-standard type
threading ;
2) Multi-start worm cutting ;
3) Face and radial grooving of non-standard type;
4) Design one’ s own cycle of any type.
Example : Carrying out 4 start threading of the size – M16 x 2.0 mm pitch. Write a custom Macro “A” Program for the same. Use Multi-cut threading cycle – G76. Use following data :
Data :
i) O. D. = 15.8 mm
ii) δ1 = 30.0 mm
iii) δ2 = 5.0 mm
iv) 1st cut depth = 0.3 mm
v) Lead = Pitch x no. of starts = 2 x 4 = 8 mm
vi) Chamfer amount = 1.0 times the lead.
vi) Root diameter = 13.3 mm
vii) Thd. Height = 1.25 mm
viii) Length of threads = 50 mm
ix) No. of finishing passes = 3 nos.
x) Limiting depth of cut per pass = 0.075 mm
xi) Depth of cut for finishing pass = 0.050 mm.
xii) Angle of Approach = 60 degrees.
(A) Custom Macro – A for FANUC OT-D/C systems
O0001 (4 START THREADING);
N1;
T0000;
G28 U0 W0;
T0101;
G50 S800;
G97 S800 M03;
G65 H01 P#100 Q30000;
M08;
N10;
G0 X17.0 Z#100;
G65 H83 P20 Q#100 R36000;
G76 P031060 Q75 R50;
G76 X13.3 Z-55.0 P1250 Q300 F8.0;
G65 H02 P#100 Q#100 R2000;
G65 H80 P10;
N20;
M09;
G97 M05;
G28 U0 W0;
M30;
%
(B) Custom Macro “B” for FANUC Oi Mate – TB/TC system :
O0001 (4 START THREADING);
N1;
T0000;
G28 U0 W0;
T0101;
G50 S800;
G97 S800 M03;
#100 = 30.0;
M08;
N10;
G0 X17.0 Z#100;
IF [#100 GT 36.0] GOTO 20;
G76 P031060 Q75 R50;
G76 X13.3 Z-55.0 P1250 Q300 F8.0;
#100 = #100 + 2.0;
GOTO 10;
N20;
M09;
G97 M05;
G28 U0 W0;
M30;
%
source http://www.machinetoolhelp.com
cnc macro programing,cnc fanuc programing,fanuc macro proghraming
