[Jerseycnc]

Not familiar with subroutines and have a part to program with two different pocket sizes plus drilling cycles etc
I attached the part file as jpg-setup twice on vise 1. Would like to duplicate on vise 2 & 3.Vises are 10.0 in apart
Its a Fanuc OMF. The program below is for part 1 vise 1. Do you sub that or post both parts and sub that for
the 2 other vises. I would like to go from vise 1 to 3 then 3 to 1 in maching to save time.
Thanks---JC
%
O126 (PULL BRACKET)
(MACHINE LEADWELL OMF)
(3 VISE MACHINING 2 PARTS PER VISE)
(G54 X0 LEFT EDGE OF BACK JAW VISE 1)
(G54 Y0 BACK EDGE OF MATERIAL VISE 1)
(G54 Z0 TOP OF FIXED JAW VISE 1)
G17 G20 G40 G49 G80 G90
N1 T3
(TOOL_3 .500 DOWEL PIN LOCATOR TLO=H3)
(OPERATION_LOCATE PART )
(VISE 1)
M6
M5 S0
G00 G90 G54 X3.1562 Y-0.741
G43 Z1. H3
M9
G0 X3.1562 Y-0.741
G1 Z0.2812 F35.
M0 (LOAD PARTS OPPOSITE SIDE)
(OF PIN TIGHTEN VISE 1)
G0 Z1.
M9
G00 G28 G91 Z0 M5
N2 T14
(TOOL_14 #7 DRILL .201 TLO=H14)
(OPERATION_DRILL ACCESS HOLE )
(VISE 1)
M6
M3 S1800
G00 G90 G54 X1.1816 Y-0.2626
G43 Z1. H14
M9
G83 X1.1816 Y-0.2626 Z-0.2054 Q0.2 R0.625 F14.
Y-1.2194
X1.6384
Y-0.2626
X1.41 Y-0.741
G80 Z1.
M9
G00 G28 G91 Z0 M5
N3 T5
(TOOL_5 .1875 ENDMILL TLO=H5 TDO=H55)
(OPERATION_MILL POCKET FOR PEDAL)
(VISE 1)
M6
M3 S2500
G00 G90 G54 X1.41 Y-0.741
G43 Z1. H5
M8
G00 Z0.625
G01 Z-0.125 F25.
X1.4067 F8.
G41 X1.3987 H55
G01 Y-1.0022
X1.4212
Y-0.4798
X1.3987
Y-0.741
X1.3238
Y-1.0773
X1.4963
Y-0.4047
X1.3238
Y-0.741
X1.2487
Y-1.1523
X1.5712
Y-0.3298
X1.2487
Y-0.741
G40 X1.2567
G01 X1.2467
G41 X1.2387 H55
G01 Y-1.1623
X1.5812
Y-0.3198
X1.2387
Y-0.741
G40 X1.2467
G00 Z1.
M9
G00 G28 G91 Z0 M5
G28 Y0
M30
%

[Beltdrive]

%
O126 (PULL BRACKET)
(MACHINE LEADWELL OMF)
(3 VISE MACHINING 2 PARTS PER VISE)
(G54 X0 LEFT EDGE OF BACK JAW VISE 1)
(G54 Y0 BACK EDGE OF MATERIAL VISE 1)
(G54 Z0 TOP OF FIXED JAW VISE 1)
G17 G20 G40 G49 G80 G90
N1 T3
(TOOL_3 .500 DOWEL PIN LOCATOR TLO=H3)
(OPERATION_LOCATE PART )
(VISE 1)
M6
M5 S0

G00 G90 G54 X3.1562 Y-0.741
M97P1

G00 G90 G55 X3.1562 Y-0.741
M97P1

G00 G90 G56 X3.1562 Y-0.741
M97P1

M9
G00 G28 G91 Z0 M5
N2 T14
(TOOL_14 #7 DRILL .201 TLO=H14)
(OPERATION_DRILL ACCESS HOLE )
(VISE 1)
M6
M3 S1800

G00 G90 G56 X1.1816 Y-0.2626
M97P2

G00 G90 G55 X1.1816 Y-0.2626
M97P2

G00 G90 G54 X1.1816 Y-0.2626
M97P2


M9
G00 G28 G91 Z0 M5
N3 T5
(TOOL_5 .1875 ENDMILL TLO=H5 TDO=H55)
(OPERATION_MILL POCKET FOR PEDAL)
(VISE 1)
M6
M3 S2500
G00 G90 G54 X1.41 Y-0.741
M97P3

G00 G90 G55 X1.41 Y-0.741
M97P3

G00 G90 G56 X1.41 Y-0.741
M97P3

M9
G00 G28 G91 Z0 M5
G28 Y0
M30


N1
G00 G90 X3.1562 Y-0.741
G43 Z1. H3
M9
G0 X3.1562 Y-0.741
G1 Z0.2812 F35.
M0 (LOAD PARTS OPPOSITE SIDE)
(OF PIN TIGHTEN VISE )
G0 Z1.
M99

N2
G00 G90 X1.1816 Y-0.2626
G43 Z1. H14
M9
G83 X1.1816 Y-0.2626 Z-0.2054 Q0.2 R0.625 F14.
Y-1.2194
X1.6384
Y-0.2626
X1.41 Y-0.741
G80 Z1.
M99

N3
G00 G90 X1.41 Y-0.741
G43 Z1. H5
M8
G00 Z0.625
G01 Z-0.125 F25.
X1.4067 F8.
G41 X1.3987 H55
G01 Y-1.0022
X1.4212
Y-0.4798
X1.3987
Y-0.741
X1.3238
Y-1.0773
X1.4963
Y-0.4047
X1.3238
Y-0.741
X1.2487
Y-1.1523
X1.5712
Y-0.3298
X1.2487
Y-0.741
G40 X1.2567
G01 X1.2467
G41 X1.2387 H55
G01 Y-1.1623
X1.5812
Y-0.3198
X1.2387
Y-0.741
G40 X1.2467
G00 Z1.
M99
%


This would work on my hitachi seiki

[Jerseycnc]

Beltdrive,

Im not sure about the M97 which I understand is calling a sub program with in a main
but will definitely try. I can see thats keeping the program short. This is and old Fanuc
early 80's.I maybe stuck with the M98 where it has to be outside the main as a subroutine.
Thanks
JC

[angelw]

Beltdrive,

Im not sure about the M97 which I understand is calling a sub program with in a main
but will definitely try. I can see thats keeping the program short. This is and old Fanuc
early 80's.I maybe stuck with the M98 where it has to be outside the main as a subroutine.
Thanks
JC

Hi JC,
M97 won't work with a Fanuc control. However, from FS16i onwards, you can set SQC bit to enable calling a subprogram with its sequence number. The parameter bit is 6005.0 This allows the Sub Programs to be included in the Main Program, after the M30, as shown following:

Main Program
O1000
-------------
-------------
-------------
M98 Q100
-------------
-------------
-------------
M98 Q200
-------------
-------------
-------------
M98 Q300
-------------
-------------
-------------
M30
(SUB PROGRAMS START HERE)
N100 --------
-------------
-------------
-------------
-------------
M99
N200 --------
-------------
-------------
-------------
-------------
M99
N300 --------
-------------
-------------
-------------
-------------
M99
%

In the above program, Sub Programs commencing with the sequence numbers N100, N200, and N300 are called by the M98 call combined with a "Q" address relating to the sequence number of the required Sub Program.

The following format can be used to start at a particular Sequence Number within an External Sub Program.

M98 P2000 Q50 (Calls External Sub Program O2000 and starts control at Sequence Number 50)

M98 P3000 Q20 (Calls External Sub Program O3000 and starts control at Sequence Number 20)

Regards,

Bill

[Jerseycnc]

Bill,
Thanks Funny how you keep fine tuning till it works. I appreciate all in puts. Sad part is not having
a manual causes these questions. Will look into the parameter bit is 6005.0.
Thanks
JC