Using live tool to profile hex. Anyone have a sample program.

I have a buddy who needs to mill a 3/8 hex where the corners blend into a .430 diameter with a .016 radius. I was wondering if anyone had a sample of the code on this. I have seen it done in videos but thats about it. The control will be a fanuc 21

Do you have polar interpolation (G12.1 or G112)? If so, that makes it pretty easy. You just program it as if X Y on a mill, but substitute C for Y. Must start at C0 initially. Then, code your polar G code and proceed with the rest of the tool path. Remember to cancel polar with G113 or G13.1, depending upon your control. I think most Fanucs today can use either.

Is your live tool vertical or horizontal?

Horizontal so it will be side cutting with the end mill.

The X's are in Diameter, while the C's are ... not .. I guess...


I have had many issues with C doing rads with tool comp for some reason on the Fanuc's, so I program to tool C/L instead.

(Not done much C on anything other than Fanuc's)


------------------

Think Snow Eh!
Ox

It is going to take some good eyes to tell you didn't do the 1/64" connecting radius. They have to overlap to fit on the corner. Might make your life easier to just do the hex and turn the Ø0.430.



On edit: If you draw a sharp 3/8" hex with 1/64"R at each corner the Ø is 0.428. I was thinking the opposite way. Turn first, under the circumscribed circle of the hex, to knock off the corners.

Ox said:

The X's are in Diameter, while the C's are ... not .. I guess...

Click to expand...

Try putting your machine in C-axis mode and manually rotate the spindle/axis. If you have to move it minus to get the spindle to rotate clockwise, use G42. If C moves positive to get it to spin clockwise, use G41. Just remember to set your tool type as 9 in the geometry page and (at least on ours) the R value is radial.

And you are correct, X values are radial values. C's are not.

At least that's the way it works here.

No warranty expressed or implied.

So there...

Edit: The above is for climb milling.

Using C axis:


( 3/8 FLAT ENDMILL)
M05
M98 P7000
G54

T101

G17 G98
M45(CONNECT C AXIS)
M69(C AXIS BRAKE OFF)
G0 X1.186 Y0. Z.1 C0. M8
G97 S3000 M13
G12.1 (POLAR COORD ON)
G1 X1.186 C0. F60.
Z0.
G41 X.75 F20.
C-.1542
X.702 C-.197
G2 X.6922 C-.2055 R.4025
G1 X.6421 C-.2477
X.1079 C-.4019
X.0099 C-.4025
G2 X0. R.4025
X-.0098 R.4025
G1 X-.1079 C-.4019
X-.6421 C-.2477
X-.6922 C-.2055
G2 X-.702 C-.197 R.4025
G1 X-.75 C-.1542
C.1542
X-.702 C.197
G2 X-.6922 C.2055 R.4025
G1 X-.6421 C.2477
X-.1079 C.4019
X-.0099 C.4025
G2 X0. R.4025
X.0098 R.4025
G1 X.1079 C.4019
X.6421 C.2477
X.6922 C.2055
G2 X.702 C.197 R.4025
G1 X.75 C.1542
C0.
G40 X1.186
Z.1 F500.
G13.1 (POLAR COORD OFF)
M05
M46(DISCONNECT C AXIS)
M9



Or using X, Y:


( 3/8 FLAT ENDMILL)
M05
M98 P7000
G54

T101

G17 G98
M45(CONNECT C AXIS)
M69(C AXIS BRAKE OFF)
G0 X1.186 Y0. Z.1 C0. M8
M68(C AXIS BRAKE ON)
G97 S3000 M13
G1 Z0. F60.
G41 X.75 F20.
Y-.1542
X.702 Y-.197
G2 X.6922 Y-.2055 R.4025
G1 X.6421 Y-.2477
X.1079 Y-.4019
X.0099 Y-.4025
G2 X0. R.4025
X-.0098 R.4025
G1 X-.1079 Y-.4019
X-.6421 Y-.2477
X-.6922 Y-.2055
G2 X-.702 Y-.197 R.4025
G1 X-.75 Y-.1542
Y.1542
X-.702 Y.197
G2 X-.6922 Y.2055 R.4025
G1 X-.6421 Y.2477
X-.1079 Y.4019
X-.0099 Y.4025
G2 X0. R.4025
X.0098 R.4025
G1 X.1079 Y.4019
X.6421 Y.2477
X.6922 Y.2055
G2 X.702 Y.197 R.4025
G1 X.75 Y.1542
Y0.
G40 X1.186
G0 Z.1
M05
M46(DISCONNECT C AXIS)
M69(C AXIS BRAKE OFF)
M9


Anyone questions go ahead and ask

This code is for Mori Seiki machines, some codes might be different for your machine.

These are using a 3/8 endmill, the centerline is programmed.