Titanium cutting on lathe

[V 45]

I have some titanium bolts 5/8" diamter. How hard would it be to cut these on the mini lathe or bench mill ? Just want to make something out the material, but am curious as to how it will cut. They are aviation grade bolts. Will HSS work or carbide a must ?
Thanx again,
V 45

 

[MachineTom]

I've cut it with both but carbide is much better. If HSS it needs to be fresh sharp, hit Ti with a slightly dull bit an it will harden before the word Oh'xx is spoken. Be careful when drilling for the same reason, sharpen the bit before use, not after it stopped drilling.

It will machine real nice with speed, carbide, lube. a. 1/2" D piece at 2K+ will look as if it was a ground finish. The chips come off bright red hot. DO NOT Pause when cutting, the bit will stick, and it will spot harden.

Mke chips

 

[rake60]

Machining titanium requires low surface speed, high feed rates, flood coolant and very sharp tools.

Never allow the tool to dwell.
Titanium will work harden immediately if you allow a tool to rub on it without cutting.

Be careful with those fine stringer chips.
If the cut is not flooded with coolant, those fine stringer could light up in a metal fire that is very difficult to extinguish.

Rick

 

[V 45]

I tried it on my mill first ... just cut the end with threads...speed was 450 rpm and it cut fairly nice. I did not know that TI would flame !! I know magnesium does easily. Thanx for the advice. I don't have flood but my sprayer puts out a lot of coolant as long as I keep squezing. Just trying to learn something new everytime I go to my little basement shop.
Thanx again... V45

 

[bret4]

I cut ti every day at work. A sharp cutter is needed as mentioned or you will start a fire on thin chips. Heavy chips do not burn easy. I like a tool with a radius on it. A small lathe like yours I'd say .005 to .015 radius. Don't use a sharp pointed tool bit. The heat will dull it quickly. A feed rate of .003 per rev is about right. Hss tools can work but for a lot of turning carbide is best. Just keep them sharp.

When drilling ti I find cobalt drills work good. If you use new hss drills I like to hand grind them so the point is not on center by a little. This lets the drill bit cut over size a little. If you don't do this the drill can burn up and melt. Always use plenty of coolant when drilling.

Tapping ti is harder than most anything you will try to tap. Special taps are made to tap ti. You can tap ti with hss taps by grinding away some of the threads so that there is about 1/4 of the threads left on the diameter of the tap. Then grind the flutes so the the face of the threads are flat. I could post a picture if there is any interest. Its kind of hard to explain.

Bret

 

[Woodster]

I used to make these parts on a CNC lathe using an HSS tool to cut the thread! 4mm pitch, 1mm land, straight sided, 11mm parallel, then increase in diameter on 2 radius's - 136.5mm radius on bottom, 85mm radius on top. Took 3 days to program, on-line, not with CAD/CAM, working out each cuts tool path to keep the tool cutting constantly with 5 lines of G code per cut. Took about 30 mins to cut the thread!!

Woodster

 

[dman]

ti isn't too difficult on a lathe. you get a pretty continuous cut with a lathe, just make sure you're tool is sharp don't really need coolant on the lathe either but it helps. on a mill you have some issues. it work hardens and the Chips are flammable. it is best to cut it aggressively and to take climbing cuts. this may be an issue on a manual mill because the table may jump. the reason is titanium is surprisingly spongy and will compress under the cutting edge and it is difficult to start each chip. climb milling puts the cutting edge into fresh non work hardened material and gives it a steeper angle of attack. it bites into the material better. the more over step or the smaller the end mill (within reason) the better. I try to get 1/3 the cutter diameter in overstep. it can also be difficult to do pocketing. its hard on the corners of an end mill and they easily chip compounding the work hardening problems. you may want to use a small radius on the endmill to strengthen the corners. don't use roughing end mills and it may help to get carbide or high cobalt hss endmills with a higher helix angle for smoother cutting and better cup ejection. the 3flute 60deg cutters work OK for chip clearance and ejection but the corners are weak. I find 5 flute cutters to also work well and maybe some 6 flute as long as it has good chip clearance. it's a balancing act to get the right flute count and chip clearance to cut it well. like someone said earlier don't dwell the cutter. don't be afraid to advance it just go at a steady pace. it's kinda like cutting aluminum in slow motion. same chip thickness but 1/10 the rpm/surface ft/min and therefore 1/10th the in/min feed rate.

 

[Ca-g]

I have been cutting titanium regularly for ten years on a cheap sieg lathe. There is no mystery to it, just follow the rules. The other metal I cut regularly is brass and you can get away with a lot with brass, with titanium I just get a little more fussy. I use HSS inserts. I never let it rub. Too much sharpening work! Yes it can burn but only once has it caught on me and it is hard to imagine how it could become a problem as it needs to be very fine to catch easily and when it is fine the pile is typically too loosely packed to create a draught. I don't use any lubrication. Some lovely tips in this thread.