[ChrisPhoenix]

I'm making an ultrasonic welding horn, and I need to drill (and then tap) a hole for the stud. It's a 1/2"-20 thread (thus, 15/32" hole) and the hole needs to be about 3/4" deep with a flat bottom.

The only machine I have available that could do the job is a Tormach CNC mill (there's also a lathe with 4-jaw chuck (the horn is rectangular) but I've never used it). I've done this horn in aluminum, but I'm told I really need titanium for the amplitudes I'm using.

I've read that Ti chips work-harden a lot. So I suspect that a deep-pocketing operation would be problematic as chips would get worked and re-worked. (There's no through-tool coolant option on the Tormach.)

I only need to make one of these, so I can take extra time - for example, drill or pocket 1/20", clear the hole manually, drill or pocket another 1/20" - if that's what it takes. Also, I can buy whatever tool I need for the job - it'll still be far cheaper than the $2000 price to get the horn made elsewhere.

I've read what I can find on machining Ti. Mainly it boils down to:
1) Keep the surface speed low, and the chip size large (depending what your tool will tolerate - I've been using GWizard)
2) Never dwell a running tool.
3) Use lots of coolant, and carbide tools, either uncoated or modern TiAlN coated.

So... what's the best recipe, and what do I need to know?

- HSS drill? (Harvey Tool doesn't seem to have any carbide drills.)
- Carbide end-mill for pocketing?

I'm inclined toward using maybe a 1/4" end-mill and pocketing bit-by-bit all the way down, because that'll leave at least a little space for chips, and if it breaks I've got a chance to get it out of the hole and save the part. But I don't know if a 1" stickout on a 1/4" tool will be stiff enough for Ti.

If you can't tell by now, I'm kind of self-taught on machining. I've made aluminum injection molds for 0.040" wall thickness parts that worked the first time, and my aluminum horn worked the first time. So I am capable of learning... but on titanium, I don't even know what questions to ask, and I don't really know what options are available or how to select the best one. Feel free to point me at a web page (or even a book! :-) that will help.

Thanks!

[Superman]

Ti.....don't let the stories scare you

It is easy to cut, but tough
- do not allow it to heat up.....drill with NO pecks
HSS Co drills work OK, any carbide should be uncoated,
sharp corners on tips or endmills are OK for finishing, but, (for roughing) if the corners break down, then the cutter needs the corners to be touched up
- longer cutter life if you have small radius or chamfer on the corners ( ie 0.020"-0.060" ), I have used sharp corner then extended it's life by adding chamfer to remove the wear

threading, you might be able to tap, but I suggest threadmilling, use a lathe thread bar with the correct tip, start the cut at the bottom moving up in CCW direction for a RH thread ( chips are kept below the cutting edge )

[ChrisPhoenix]

Thanks, Superman - a couple of questions:

1) Did you mean I should put the lathe thread bar in the Tormach? Or that I should use the lathe - in which case I don't understand "start the cut at the bottom."
2) I found these single form thread cutting tools - could/should I use these instead of the thread bar? Harvey Tool - Carbide Thread Milling Cutters - Single Form
3) If I drill with no pecks, won't that produce insane chips (whipping around at 2000 RPM - doesn't even sound safe! Plus I'd worry about them pumping all the coolant out of the hole.) I understand that I don't want to chip-break by pausing the downward motion, because that will heat things up. But if I alternate between feed-up and feed-down with no pause, won't that break the chips and avoid the heating problem?
4) If I use a drill (as opposed to a plunging endmill) how can I finish the bottom of the hole to be flat, with enough chip removal to avoid re-cutting my chips?

Thanks!

[bhurts]

You won't be drilling at 2000 rpm. More like 750 for that size hole. Feed at 3.5-4ipm. For .75 deep you shouldn't need to peck. If you do use a peck depth of .4 inch or so and flood coolant. Those threadmills will work fine.

Ben

[Superman]

1) Did you mean I should put the lathe thread bar in the Tormach? Or that I should use the lathe - in which case I don't understand "start the cut at the bottom."
------- threadmills can be expensive, using a threading bar from a lathe is a "single pointed threadmill" for those on a low budget
2) I found these single form thread cutting tools - could/should I use these instead of the thread bar? Harvey Tool - Carbide Thread Milling Cutters - Single Form
------ a threadmill is a better choice by far, but easier to replace a turning tip than a whole threadmill. Either method is still your choice.
3) If I drill with no pecks, won't that produce insane chips (whipping around at 2000 RPM - doesn't even sound safe! Plus I'd worry about them pumping all the coolant out of the hole.) I understand that I don't want to chip-break by pausing the downward motion, because that will heat things up. But if I alternate between feed-up and feed-down with no pause, won't that break the chips and avoid the heating problem?
4) If I use a drill (as opposed to a plunging endmill) how can I finish the bottom of the hole to be flat, with enough chip removal to avoid re-cutting my chips?
----- Ti is tough, use a 5/16" HSS Co drill to depth, correct Speed/Feed should chipbreak, then interpolate the hole with 1/4" endmill to get the correct core diameter & to get the flat bottom, chamfer the top, then mill the thread ( coolant into the hole to flush chips out while cutting )

[daniellyall]

have a look at NYCCNC on youtube he does a lot of drilling and threading on a tormach no Ti that I have seen but the way it is done is very simaller just different feed and speed

[ChrisPhoenix]

bhurts, thanks! You're right about rpm, of course - I was remembering the rpm for a 1/4" carbide endmill on a shallow slot.

Superman, again thanks! I understand the threadbar/threadmill options now; I think I'll go with the "better choice by far." :-)

I can keep the hole full of coolant, but I'm pretty sure I can't spray it in with enough pressure to flush the chips out while I flatten the bottom. I'd expect the 1/4" endmill to just stir things around and keep re-grinding the same chips. This has me pretty worried. I'm actually thinking of using it in plunge mode to remove most of the material - a single plunge, then pull it out and blast the pocket clear with air, then plunge in a different spot, do that in six or eight spots around the edge, then one quick sweep to clean up the rest material. Am I worrying too much?

Chris

[bhurts]

Way to much worrying. It will be fine without all the plunge cuts. The drill bit if drilled to depth will leave very little actual material to remove. Depending on how thick the material is you may not need to use the endmill at all. If you have enough just drill a little deeper enough to account for the tip angle of the drill and a slight bit extra. Having a flat bottom for a threaded hole won't make the part any better since once you put a bolt in it will never be seen or affect the part. If I rigid tap a 1/2 inch thread 1 inch deep I just drill 1 1/4-1 1/2 deep if possible. Doesn't hurt a thing. Also drilling is much quicker then milling so time saved.

Ben

[ChrisPhoenix]

The bolt that will go in this hole has a knurled/pointed end that grips the bottom of the pocket. The flat bottom matters very much for this particular part.

[AARONT]

a 1/2-20 tap drill is a 29/64" NOT a 15/32". your minor diameter will be out of spec.

Just drill it with a 135deg stub drill. and interpolate the .100" of drill point out.

[ChrisPhoenix]

Aaront, this chart: Thread - Drill & Tap Chart says for "Alum, Brass, & Plasitcs" I should use 75% thread and 29/64, but for "Stainless Steel, Steels & Iron" I should use 50% thread and 15/32. That's where I got the 15/32, thinking Ti was closer to ferric than to aluminum/brass.

Chris