Fanuc OM - Helical Interpolation

[HPT]

Can Fanuc OM be used for helical interpolation? Using a vertical mill and a cutter of dia 1.25", need to produce a hole of dia 4" and 3.8" deep.

[underthetire]

Helical was an option back then. May or may not work.

[glovebox20]

Hello

I've done Helical milling on a Fanuc OM in the past without much troubles. It's just like a regular G2/G3 move except you add a Z move in the same block.

Like this

Mill inside circle

G0 G17 G40 G(work offset #) G90 X0 Y0
Z.05
G01 G41 G91 D(offset#) X2. F(rate)
G2 Z-.1 I-2.
Z-.1 I-2.
Z-.1 I-2.
Z-.1 I-2.
Z-.1 I-2.
I-2.
G1 G40 X-2.
G0 G90 Z1.0

I milled a helix .450" deep taking .1" per rev, 4" in Diameter. (note: D(offset#) equals cutter Radius {.625" with 1 1/4 tool})

Here we go again only in G90

G0 G17 G40 G(work offset #) G90 X0 Y0
Z.05
G01 G41 D(offset#) X2. F(rate)
G2 Z-.05 I-2.
Z-.15 I-2.
Z-.25 I-2.
Z-.35 I-2.
Z-.45 I-2.
I-2.
G1 G40 X0.
G0 Z1.0

This is for the finish past, you will need to rough the inside first. Either by drilling, drilling and Helix milling, drilling/boring and Helix milling or any other suitable process. I hate slugs.

This should work for you. Just make sure your in the X,Y plane (G17). Don't forget the tool change, G43 offset, spindle speed, and Coolant (if needed).

glovebox20

[HPT]

Thank you. This was a good help.

[HPT]

Hello Glovebox,

is there any way that we can modify and use you program for thread milling too? It will be interesting to know if you have tried it before.

[glovebox20]

hello.

Yes, you can do thread milling if you need to. The Z move would be the same as the pitch of the thread. Just make sure you make the right move in "Z" (postive or negitve) or you may end up with left hand threads. Some people take the easy approach and just ram the thread mill straight into the part which may cause excessive tool wear/chatter. It's best the arc in and out of the thread for a smoother entry/exit. If you arc in with a 180* sweep, the Z move should be 1/2 of the pitch amount or the threads may have a nick on them. If doing internal threads, the entry arc should be less than the minor radius (minor diameter divided by two), but more than the Cutter Radius. I always did a couple of passes to ensure little tool deflection.

I can write you a sample program if you need one when I get the time. If you reply back with the thread size/tool type, I just may base the sample off that.

[gbowne1]

I'd like to try this on my 0M-C, never done much heli milling.. but it might work on this part.

I'm normally using my G54 offset and it's my Kurt D675 vise at the center of my table.

The parts: .750" Alcoa 2024T3 QQA250/5 @ 3.500" x 5.000"

There is a 2.21875" bore at X=2.5 Y=1.75 right in the center of the part.

2nd op is to drill 4 ea 0.125" holes with T06 a 14N drill chuck at 4 ea 90° locations around the bore. 0°, 90°, 180° & 270°

3rd op is where I flip the part on both its end edges and drill a #7 drill and tap 1/4-20 in the center of the edges.

Turn on Flood coolant, G17 will work ok for me.

Greg

[HPT]

Advent make solid carbide thread mill. Cutter dia 0.745, Cut length 1.75"
Threads to cut 1.5"-4 ACME, internal RH, 2" long.

[glovebox20]

Originally Posted by HPT Advent make solid carbide thread mill. Cutter dia 0.745, Cut length 1.75" Threads to cut 1.5"-4 ACME, internal RH, 2" long.

Just Thinking about your application. I notice your doing a inside Thread 2" deep and your thread mill is only 1.75" Long. That may be a problem. You will probably have to reach down a good 2.25" or even 2.313" to get the last full thread, unless you can Counter-bore on the bottom side of the part for thread clearance. You can probably do the Full 2" thread depth with that tool if you have enough clearance on the shank of the tool, but rigidity of tool/machine might be a problem. It maybe better if you can find a "single point" tool to do the job, or at least a Thread mill with every other tooth missing.

I never really did thread milling myself before, So maybe I'm wrong and you only do need to reach down 2" get get full thread.

Just a couple of things to think about.

glovebox20