[DryRun]

Some please help me i am having trouble tring to cut a 1.39 hex on the od of my stock using G12.1 on a fanuc 16TT

[CNCRim]

Hope it work for your machine.


O0001
G20

(TOOL - 1 OFFSET - 1)
(FACE CONTOUR UNDEFINED)
(1.39DIM HEX _1/2 ENDMILL)
G0T0101
M23
G0G54X2.3417Z.1
C0.0
G97S1768M54
G98G1Z0.F10.
G98G3G112
G41X.25C1.019R.25
G1X1.64C.6178
G2X1.89C.4013R.25
G1C-.4013
G2X1.64C-.6178R.25
G1X.25C-1.019
G2X0.C-1.0525R.25
X-.25C-1.019R.25
G1X-1.64C-.6178
G2X-1.89C-.4013R.25
G1C.4013
G2X-1.64C.6178R.25
G1X-.25C1.019
G2X0.C1.0525R.25
X.25C1.019R.25
G1X.4232C.969
G113
G0Z.1
G28U0.W0.H0.M55
T0100
M30

[ChattaMan]

Newtexas's prog looks good. But to do other progs, different sizes yourself, I'll try to help.

When the control goes in to G12.1 (G112) it's now in milling mode. Think of coordinates as on the miller, only X is diameter (not radius) and Y is C. Work out your across corner size...

A/F x 1.155....

1.39 x 1.155=1.605

So on the miller you would program the points of the hex as so...

X0.803 Y0
X0.401 Y-0.695
X-0.401 Y-0.695
X-0.803 Y0
X-0.401 Y0.695
X0.401 Y0.695
X0.803 Y0


So on the lathe (double the X, change Y to C) the points of the hex are as so...

X1.605 C0
X0.802 C-0.695
X-0.802 C-0.695
X-1.605 C0
X-0.802 C0.695
X0.802 C0.695
X1.605 C0

A simple prog would look like this....

Tool change..blah, blah
C0X2.2Z0.1
G98G1Z-0.1F..
G112
G1G41X1.605C0
G1X0.802C-0.695
G1X-0.802C-0.695
G1X-1.605C0
G1X-0.802C0.695
G1X0.802C0.695
G1X1.605C0
G1G40X2.2
G113
G0Z.1
Blah, blah
M30

Oooo..hmmm..or macro style

Tool change...blah, blah
#504=0.5 (ENTER CUTTER DIA)
#505=1.39 (ENTER A/F SIZE)


#506=[#505*1.155]
#507=[#505/2]

C0X[#506+#504+0.5]Z0.1
G98G1Z-0.1F...
G112
G1G41X#506C0
X[#506/2]C-#507
X-[#506/2]C-#507
X-#506C0
X-[#506/2]C#507
X[#506/2]C#507
X#506C0
G40X[#506+#504+0.5]
G113
G0Z.1
Blah, blah
M30

Keep this in machine memory and just copy and merge into your prog.

Hope it makes sense??

ChattaMan

[oldjohn]

I have this square and hex generator xls. You guys will find very useful.
You could say thank you.
John

[M-man]

CHange para 6030 to 100.

Call macro as follow M110V___F___

V= WIth of hex F= feed.

Position tool in Z depth of cut and in X-axis, postion a bit above OD. After the macro the tool will end up at the same postion as when it were called.
There are a little bug in the macro, if the toolposition in X-axis are to close to hex when calling the macro it will cut off a bit of the hex while entering toolcomp/starting point. I ve adding some suggestions that might fix it, but i have not tried them myself yet......


%
O9020(MACRO HEX)
M88 ---Clamp anti vib, brake
#29=#9*0.5
#2=0.577
#3=#2*#22*0.5
#5=#5001
#24=#22*0.5
#25=#3*#3
#26=#24*#24
#27=#25+#26
#23=SQRT[#27]
#30=#22+5
G112
#28=#3-1
G1G41X#30C-#28F#9-- (G1G41C-#28F#9--change to this?)
(X#30) --- Add this line?
X#22C-#3
X0C-#23
X-#22C-#3
X-#22C#3
X0C#23
X#22C#3
C-#3
G1G40X#5C0
G113
M90
G0
M99
%

[DryRun]

Thank you for all the help i got g12.1 working but flats do not come out the same i broke down and put a 2" face mill in and just used z to cut flats

and x&c to position machine hex came out off center something is out of wack with machine maybe headstock to turret is my thought programed error out and its running would still like to get it right tho

[cnc-king]

Some please help me i am having trouble tring to cut a 1.39 hex on the od of my stock using G12.1 on a fanuc 16TT

wouldn't it be easier to cut the hex in the -X- axis using the tip of the end mill instead of the side and indexing your spindle in 60 deg increments?

[ChattaMan]

wouldn't it be easier to cut the hex in the -X- axis using the tip of the end mill instead of the side and indexing your spindle in 60 deg increments?

Hmmm...deburring the corners comes to mind.

I wrote the program above as simple as possible so it could be understood. But adding an R to each line would make it possible to put corner rads on, so eliminating any burrs. Also it looks more professional.

Just another way of doing the same thing :-)