[msantaji1]

In Oi MC G68 is valid code But in Oi MD It is invalid, What is reason?

[dcoupar]

G68 is an option. It is probably not turned on in the M-D

[msantaji1]

what is procedure to turn on G68 in Oi MD?

[arvindpatel]

To turn on the G68 in Oi MD you need to set parameter bit of 9900 series option parameters..You will get this option from fanuc.
Regards
ARVIND

[ranjankrana]

In Oi MC G68 is valid code But in Oi MD It is invalid, What is reason?

Coordinate system rotation is a standard feature in FS0iMD. Please look into the manual no. B-64304EN-2, page 224, chapter 6.10 for the details.

[fanuc-support.c]

Like on the 0i-C, on the 0i-D there aren't 9900+ options like on other control models. There between 8130 and 8137, and you can simply turn them on, normal parameters.

As this is standard you can't turn it on or off, its just there, ranjankrana is correct, its in the manual where he said.

[rapo]

help! i need to learn simple pocket macro programing on fanuc oi md vertical mill controller.

[sanilpallayi]

G 68 code is applicable in both oi-mc and oi-md. But you should follow specified pattern to in oi-md


Eg:-
G0G69G17G80G15G40G49G90;
G68X0Y0R(angle) ;

and avoid the using of g53, g28, etc. before the closing of g69 by using g 68.

[sanilpallayi]

help! i need to learn simple pocket macro programing on fanuc oi md vertical mill controller.

It is a simple macro program. use able to mill slots on four sides of a round object by using g68.

O0014
G0G69G17G80G15G40G49G90
M06T2H2
G91G28Z0
#20=52(OD)
#21=45(ID)
#22=8(CTR)
#6=0(ST-ANG)
#7=90(angle b/w slotes)
#1=.2(DEPTH OF CUT)
#2=5(TOTAL DEPTH)


#23=[[#20/2]+#22]
#24=[[#21/2]-#22]
G56G90X-#23Y0
G43Z50M03S1000
GOTO4
N1
X-#23Y0
M08
G0Z5F100
G01Z0
#6=[#6+#7]
#3=0
N2
#3=[#3+#1]
IF[#2LT#3]GOTO4
G90Z-#3F200
G01G90X-#24Y0.0
#3=[#3+#1]
IF[#2LT#3]GOTO4
G90Z-#3
G90X-#23Y0
IF[#2LT#3]GOTO4
GOTO2
N4
G0G90Z50
G68X0Y0R#6
IF[#6LT360]GOTO1
G69M09
G91M05G28Z0Y0
M30


if you have any more doubts. explain it briefly.
[email protected]

[sanilpallayi]

Like on the 0i-C, on the 0i-D there aren't 9900+ options like on other control models. There between 8130 and 8137, and you can simply turn them on, normal parameters.

As this is standard you can't turn it on or off, its just there, ranjankrana is correct, its in the manual where he said.

G 68 code is applicable in both oi-mc and oi-md. But you should follow specified pattern to in oi-md


Eg:-
G0G69G17G80G15G40G49G90;
G68X0Y0R(angle) ;

and avoid the using of g53, g28, etc. before the closing of g69 by using g 68.