[rpdayton]

My company just got a right-angle drilling head with adjustable angle so we can drill holes from the OD to the bore, but pointing toward the bushing at 17 degrees.
The tool has 2 live spindles, one for a center drill and one for the drill.
I do most of the programming at the machine, and would really like to learn how to use this. They want to hire a programming service, but I would like to be able to get it running (makes me look good!)
I'm not sure about a couple things, and hope someone can help me out?
How can I set the machine to do a drill cycle at a 17 degree angle?
How do I set the tool and offset for each spindle?
I haven't done angled drilling before, but I'm thinking there might be a G code to rotate the workplane so I can do a simple YZ cut with a regular drill cycle.
Can anyone please help me with this?

Oh - Fanuc 18i control, no manuals - I think the last guy here took them.

[ghyman]

It has been a few years, so I will have to defer to a few of the experts in this forum.

Angled holes are a simple matter of doing a G68 to rotate the coordinate plane, then just use a standard drill cycle.

[rpdayton]

OK, this is kicking my butt.

The G68 is giving me issues.

The tool holder is in T34 slot, with the drill pointing down, but rotated 17 degrees toward the guide bushing.

G68 X0 Y0 R17. is changing all of the machine moves by what I think is 17 degrees, but it isn't doing anything that I want it to.

The holes I want to drill are located on a .675" OD, at Z1.145.

Moving to X.675 Z1.145 after doing the G68 is not putting the drill anywhere near where it should go.

Could someone please give me just a nudge in the right direction? I can usually figure these things out on my own, but this has me totally stumped.

Thanks.

[asn]

If your machine don't have T35 slot, may be your problem in X-axes limit

[ghyman]

I dug through some of my old programs and came up with this:

G68.1 X Y Z R I J K
where
X = X dimension of the hole
Y = Y dimension of the hole
Z = Z dimension of the hole
R = Degrees to rotate the work plane (CCW is positive, CW is negative)
I/J/K are used to identify the X/Y/Z axis that the workplane is rotated about.

For the part described, it would look something like this:

G68.1 X0.675 Y0.0 Z1.145 R-17.0 I0 J1 K0

Which will do this:
Move the origin to X0.675, Y0.0, Z1.145 (This will put the hole at XYZ0 after the command.)
Rotate the workplane down 17 degrees, using the original Y axis as the pivot axis - I0 J1 K0 identifies the Y axis, as the J is the only word with a value.

Once rotated, all of the standard drilling cycles will work at the 17 degree angle, with the hole at X/Y/Z 0 (which simplifies the program moves considerably.)

When complete, call a G69 to cancel the workplane shift and rotate, and put everything back where it was.

It is also possible to do a G68.1 X0 Y0 Z0 R-17. I0 J1 K0 to *not* shift X/Y/Z, but only to rotate the workplane. The downside is that the desired hole location must be trigged out, and the programmed numbers for the drill cycles are a little less than intuitive.

Lastly, rapid moves are pucker-inducing once the G68 is in effect; I would recommend doing fast feed moves instead.