[Superiorforge]

Hi guys I am very rusty when it comes to manual programming(I always used work NC to generate my programs) I am on a Giddings and Lewis post mill using a GE Fanuc 160I control.I am trying to program a rectangular box key 4" long by 4" wide with a depth of 2 inches could someone write a program example using those dimensions.That would help me get started as I have alot of different box keys to do.My company is to cheap to buy mastercam or any other conversion software.Thanks Shawn.

[Get lucky]

Dose the machine have macro b or not mill inside for a pocket or out side out side for a box are you mill all the way around a print would realy help

[Superiorforge]

Dose the machine have macro b or not mill inside for a pocket or out side out side for a box are you mill all the way around a print would realy help

No macro b and its an inside pocket 4" wide 4" long by 2" deep.

[Get lucky]

well this is how I would long hand wright the program for a 2" cutter. xy zero center of the pocket z zero top of pocet

O0000
(customer)
(part #)
(part description)
G0G90G40G17
G91G28Z0(SAFE START)
G28X0Y0
N100M01
T1M6
(2" INSERT CUTTER)
(BODY #)
(INSERT #)
G0G90G54X.5Y0S0000M3(POSITION TOOL OVER STAT POINT TURN SPINDAL ON AND CALL WORK OFFSET 54)
G43H1Z.1M8(BRING TOOL TO .1 ABOVE POCKET)
G1Z-.2F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-.4F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-.6F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-.8F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-.9F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-1.F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-1.2F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-1.4F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-1.6F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-1.8F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G1Z-2.F5.(z FEED)
M98P100(RUN SUB PROGRAM)
G0G28Z1.M9(SEND Z HOME)
G91G28Y0(SEND Y HOME)
T1M6
M99P100(LOOP TO N100 TO SKIP SAFE START)
%


(SUB PROGRAM)
O100
G41D1X1.F?
Y1.
X-1.
Y-1.
X1.
Y0
G40X.5

I hope this helps you if if not sorry
Kyle

[Superiorforge]

Thanks alot man this will help me alot to get started thank a bunch.

[Get lucky]

Sorry but I for got my M99 at the end of my sub program

[cnc-king]

another way of doing this is
i modified get lucky's prog a bit
Did not look at the math just the program format

O0000
(customer)
(part #)
(part description)
G0G90G40G17
N100M01
T1M6
(2" INSERT CUTTER)
(BODY #)
(INSERT #)
G0G90G54X.5Y0S0000M3(POSITION TOOL OVER STAT POINT TURN SPINDAL ON AND CALL WORK OFFSET 54)
G43H1Z.1M8(BRING TOOL TO .1 ABOVE POCKET)
Z.01
M98P100 L10(RUN SUB PROGRAM 10 TIMES )
OR
( FOR OLDER FANUC CONTROLS)
M98P00100100(RUN SUB PROGRAM 10 TIMES )
G0Z.1
MOVE TO NEXT LOCATION
Z.01
M98P100 L10
G0Z1.M9
G91G28Z0(SEND Z HOME)
G91G28Y0(SEND Y HOME)
M30
%


(SUB PROGRAM)
O100
G91
G1Z-.201F***
G90
G1G41D1X1.F?
Y1.
X-1.
Y-1.
X1.
Y0
G40X.5
M99