O/T Fun fun fun in Titanium

[bhyde]

Good Morning!

 

Ok, so I have a rather extensive Titanium job that I have to have complete in about 3 months. Problem, the amount of titanium that I have run I can count on one hand and it generally has been a simple lathe job such as a bushing of some sort. The job that I now have to do is about 100k worth of titanium material alone! Mostly mill work, the lathe work is screws that will be made on a screw machine outside our shop due to the fact that NC Lathes are not available where I work. The information that I am after is feeds/speeds, special cutters be it mill, drills, and taps. Most of the work if flat work with some fairly tight tolerances between holes/bosses. But unfortunately, the part starts out as plate stock .375 thick and finishes at .265 to the bosses and the body is .187 thick after the 4 bosses are cleared off. (one part and informed the engineer that the bosses would have been cheaper to make as separate parts and pressed in as opposed to making from one solid piece of titanium). So, I am thinking after all this milling, I am going to have a nice titanium taco which will blow the tolerance between the bosses +.0006 minus .0000. NIIIIIICE....Any suggestions would be greatly appreciated!!!!

 

Thanks!

Bill

[Greg Williams]

Bill,

 

I have played with my fair share of Ti and I use the following as a start. Values are in metric

 

Surface Speed = 40mmin

Chip load = 0.1mm

Depth of cut = 10% of Ø

And no cutter dwelling

 

As for the tolerance

 

Rough machine +1mm

Stress Relieve

Semi finish +0.5mm

Stress Relieve

Finish machine min 0.1 depth of cut

 

Good Luck

[bhyde]

Thanks Greg!

 

These values are a good starting point to an already stressfull situation! Arrrg, I can see many nights spent in my second home due to this job!

 

Thanks again!

 

Bill

[Harryman]

Not too many replies on this one.

 

Sharp tools are good. Carbide is good. Coatings are good. Grade 2 (pure) can be form tapped with OSG Electrolube coated taps and Tap Heavy. Emuge is supposed to make good taps for cutting threads. TICN on Union Butterfield taps has worked. 55 sfpm for HSS drills. Peck short when drilling, chips tend to accordion fold in the flutes.

 

Surface Solutions in the Twin Cities has a Zirconium Nitride coating that would be fun to try. I haven't yet, but it's on my mind to try on Ti simply because it's not Ti*.

 

You'll have to get your tacos at Casa Lupita's, Ti doesn't boing as much as you fear.

[Greg Williams]

Bill,

 

Almost forgot, Cutters

 

I use Sumitomo SSUP which are specifically for Ti

[bhyde]

 

Im going to have to go somewhere else for me tacos? This is a little more encouraging than all the info that I have read on this nasty stuff. But at least its not as bad as one of my other favorite materials! KOVAR....Love that stuff!

Thanks alot Greg and Harry! Oh...Gotta love the fact that I am slowly but surely getting my post count up Maybe one of these days I can have an avatar too!

 

Bill

[Philcott]

Hi Bill,

 

I too, have know the troubles of Kovar and have had a few too many crappy days running that stuff. Luckily the work was on the lathe but I have never been the same with tapping since.

 

Phil

[Harryman]

Ti is really not so nasty. Tapping can be a pain when the stuff wants to adhere to the tap on reverse. Consider milling threads, not for speed, but because thread milling is less likely to destroy a valuable part than tapping. In milling, its pretty honest stuff. It just cannot be frightened. By that I mean, if one is accustomed to brutalizing steels with blunt tooling at high speed and you try that on Ti, you'll discover a whole rainbow of colors from glowing red, during the "cut" to some very cool blues after everything cools down.

[Chris Rizzo]

I like how you put it Harryman! When your tools lose the edge, forget about it....don't even try to run just "one more part (or cut)". Sharp tools are an absolute must.

[Davidgil]

Hello Bill,

We cut a fair bit of plate Titanium, and I would agree with what has been said. Keep your tools sharp and the contact point cool as possible. Never feed hold in the middle of a cut. I have had good luck using Robbjack tools, who I believe just came out with a new series that is supposed to work really well in Ti.

Dave

[Trevor Bailey]

I have cut a few Ti putters, 2d & 3d. Sharpe tooling and no pausing with constant coolant. I have used standard grade carbide and plain highspeed endmills and, knock on wood, never broke or scrapped a part. My feeds/speeds were based on SS. I did not know what I was getting into, but everything worked with tool life and made some nice chips. Oh yeah, and putters.