What's new
What's new

Holding Tight Mill Tolerances in Titanium

jbhagood

Plastic
Joined
May 8, 2018
First time to possibly be machining Ti and hoping to get some tips on maintaining tight toleranced milled features.
The part I'm looking at is TI-10V-2FE-3AL. It has a thru hole with .5" of cutting depth and a milled boss .83" tall. Both the features are around .437 diameter with .0005/.0000 tolerances. Typically i would just run several spring passes with an endmill around these features to maintain that tolerance. Would that plan of attack work with Ti? Would rubbing be an issue on the spring passes? Thanks in advance!
 
I'd consider boring both of those.
But if can normally hold that Tol. in other materials, maybe stick with what you know.

If your worried about rubbing, make slow speed/ high feed finish passes with small step overs, and you should be fine.

never cut that alloy?!?!?
 
First time to possibly be machining Ti and hoping to get some tips on maintaining tight toleranced milled features.
The part I'm looking at is TI-10V-2FE-3AL. It has a thru hole with .5" of cutting depth and a milled boss .83" tall. Both the features are around .437 diameter with .0005/.0000 tolerances. Typically i would just run several spring passes with an endmill around these features to maintain that tolerance. Would that plan of attack work with Ti? Would rubbing be an issue on the spring passes? Thanks in advance!

usually you maintain ipt feed rate depth and width of cut doesnt matter much. true some materials with a boring bar there is a minimum increase you can take with a boring bar. for example increase boring bar .0005" but dont get .0005". some materials you need to take minimum .001" increase in boring size to get .001 increase
.
a lot depends on you cutter length and width and how sharp it is. also sometimes at higher rpm you get chatter. nothing to do with over heating cutting edge. got to do with just going too fast and cutter vibrating.
.
some machinist collect data on cutting parameters and how well they work. that way they know exactly how a tool made up to precise tolerances will perform next time.
 
I'd consider boring both of those.
But if can normally hold that Tol. in other materials, maybe stick with what you know.

If your worried about rubbing, make slow speed/ high feed finish passes with small step overs, and you should be fine.

never cut that alloy?!?!?

By "boring" are you meaning with a boring head?? or helical boring with an endmill??
 
By "boring" are you meaning with a boring head?? or helical boring with an endmill??
.
circular milling rarely is perfectly round. .0005 to .0015" out of roundness is common. boring bar can make rounder hole often to +/-.0001" tolerance with care and experience.
.
also note you can bore a round hole and when vise or fixture unclamped the hole can go out of round. often you rechuck at lighter pressure before final cuts to try to avoid this distortion or warpage
.
a boring head often has a limited length, boring bars are made for deeper longer bore lengths
 
I've never cut that particular TI alloy but for my stuff, the starting point for titanium has been to treat it like aluminum as far as speeds and feeds, and use high pressure coolant whenever possible.

Rubbing might be an issue on multiple spring passes, I've had good luck without spring passes and just milling .001-.005" on the finish pass. With a sharp cutter that should produce a pretty nice finish and hold tolerance well.
 
The .0005/0000 tolerance on the through hole should be easy with a reamer, the diameter on the boss depends on a few things, rigidity and accuracy of the machine and how large a cutter that will machine the boss. If the machine can hold those tolerances on aluminum it most likely will be fine for the Titanium. All bets are off if you have to use a 3/8" end mill 1" length of cut to generate the OD on that boss, 5/8" diameter or larger should work fine. The machine needs to be tight enough to climb mill Titanium. Don't ask me how I know this but some Titanium 6AL4V and 6AL6V will work harden and if you melt a HS cutter down and mix it with the Titanium will turn into mystery metal, a burn is nearly impossible to cut out without a solid carbide cutter! For that reason I'd highly recommend sharp tools, lots of coolant and not letting them load up with chips or dwell in the cuts at all.
Dan
 
By "boring" are you meaning with a boring head?? ?
Yes.
Maybe a reamer for hole, but i've had statistical trouble with serial production. Fancy way of saying a % of holes mysteriously blow oversize.
 
I'd avoid reaming Ti like the plague, surest way I know to work harden the stuff, and mkd says - hole sizes vary for no apparent reason.
 
The .0005/0000 tolerance on the through hole should be easy with a reamer, the diameter on the boss depends on a few things, rigidity and accuracy of the machine and how large a cutter that will machine the boss. If the machine can hold those tolerances on aluminum it most likely will be fine for the Titanium. All bets are off if you have to use a 3/8" end mill 1" length of cut to generate the OD on that boss, 5/8" diameter or larger should work fine. The machine needs to be tight enough to climb mill Titanium. Don't ask me how I know this but some Titanium 6AL4V and 6AL6V will work harden and if you melt a HS cutter down and mix it with the Titanium will turn into mystery metal, a burn is nearly impossible to cut out without a solid carbide cutter! For that reason I'd highly recommend sharp tools, lots of coolant and not letting them load up with chips or dwell in the cuts at all.
Dan

Have you had success with reaming Ti? My gut was initially telling me to run away from reaming, and seems like a couple of users agree.
 
reaming on some materials you get lobing or 8 sides holes and curved holes sometimes. often error is in the <.0005" range
.
i have seen holes where you could put 3 brand new confirmed correct size reamers by hand turning in a hole and yet not get a ground pin in hole. make 10 parts and 8 reamed and checked with pin ok but 2 parts pin wouldnt go in and good parts made both before and after the bad parts
.
sometimes you really got to use a spiral flute reamer as straight flute reamer just not working and you really got to have reamers .0002 or .0005 different in size just in case. that is if you want pin to got in part hole by hand
.
with boring bar if pin dont go in hole you can rerun and or adjust bigger. some long boring bars you have trouble with <.001 size increases. sometimes rerun boring bar at higher rpm will cut bigger
 
Ive had good success machine tight tolerances machining titanium. Never have machined that kind though. If you are going to bore that tight tolerance look up a company called DENITOOL, vario system boring bars. They are relatively inexpensive, easy to adjust, and hold tolerances great. Using these boring bars I've held tolerances as close as +-.0001. As far as machining a boss with TI, I don't recommend taking 3 spring passes, just rough it out .01, semi finish .003-.005, and then take ONE slow finish pass at 0 and you should be good as long as you KNOW your machine can hold that tolerance. If your Y ballscrew is no good your boss is going to be no good.

Good luck hope this helps.

Ian
 
I just discovered that Maritool has left-hand spiral right-hand cut carb reamers about every .0004" from .0236" to .5020". Got some on order for a .0850" +/- .0005" hole in 17-4 H900. Got the nominal, one over, and one under for dialing it in.
 
I just discovered that Maritool has left-hand spiral right-hand cut carb reamers about every .0004" from .0236" to .5020". Got some on order for a .0850" +/- .0005" hole in 17-4 H900. Got the nominal, one over, and one under for dialing it in.

Re dialling in, just so you know, IME you only get one bite at the cherry when reaming Ti, if it ain't right, the parts a scrapper.
 
Of all the Tools, in all the shops, on this planet and all the others, a Reamer is the worst one. I would rather use a Woodruff Keyseat Cutter for the job. They never do exactly what they are told to do, it's almost like they are designed to piss me off. A lot of guys say "it has it's place", and I usually agree, but Reamers have been at the very bottom of my choice of Tool for a long time. Give me a Chisel, at least I know what to expect. Give me a clapped out Shaper, I can use shim stock. Reamers errrrr.

R
 
I've never cut that particular TI alloy but for my stuff, the starting point for titanium has been to treat it like aluminum as far as speeds and feeds, and use high pressure coolant whenever possible.

:eek: Don't use this advice! I run 2000 SFM is Aluminum regularly, see how that does in Ti. It isn't about S&F it's about chip load, and Tooling.

R
 
In fairness, we don't know how slowly he runs Aluminum. I had a guy once that believed there was one magic speed and feed for all tools. That was 2501rpm and 10ipm. Didn't matter if it was a 1/16" ball mill in aluminum or a 2" face mill in tool steel.
 
In fairness, we don't know how slowly he runs Aluminum. I had a guy once that believed there was one magic speed and feed for all tools. That was 2501rpm and 10ipm. Didn't matter if it was a 1/16" ball mill in aluminum or a 2" face mill in tool steel.


Ha, Being double wrong doesn't make it right though. Perspective, perspective. Facts (plagiarism) follow;


Use low cutting speeds. Tool tip temperatures are affected more by cutting speed than by any other single variable.
A change from 6 to 46 meters per min (20 to 150 sfm) with carbide tools results in a temperature change from 427ºC to 927ºC (800ºF to 1700ºF).

Maintain high feed rates. Temperature is not affected by feed rate so much as by speed, and the highest feed rates consistent with good machining practice should be used. A change from 0.05 to 0.51 mm (0.002 in. to 0.020 in.) per revolution results in a temperature increase of only 149ºC (300ºF).

So the spindle Speed changes the Tools temperature 900º, and the Feed only changes 150º.
 








 
Back
Top