Machining Titanium

[vivaldi]

I am going to drill a 0.5mm diam. hole (In the vertical machining Centre) on a titanium bar(Ti 6Al 4V ELI). Now I am asking for a advise for machining that titanium( Also I need a help for the selection of the drilling tool material to machine the titanium. If you have a knowledge or any experience on this issue, I will be happy for sharing them.

Kind Regards,

 

Try "guhring" drills. They are some of the best. They will advise you of feeds speeds etc to use on their drills. They are available through all of the catalog dealers such as MSC, J&L, etc.

 

[knobhead]

Similarly, try Sandvik (

http://www.coromant.sandvik.com)

 

[rakes]

We have done upto 0.4mm holes in Ti6Al4V. Remember that Titanium has poor thermal conductivity and is work hardening. Solid carbide drills work best but if L/D ratio is high, then it is better to try HSS-Co with TCN coating (to avoid breakage of drills). In any case, drill run-out should be controlled for maximum yield and always use peck-drilling cycle. Use a good quality soluble oil. Guhring may have the right tool but Sandvik can't help you here.

 

[WIPLASH]

Cobalt with the TCIN coating is the best answer,carbide will catch a chip and break,although carbide will drill the hole much straighter.If I understand correctly your roughly drilling a .020in hole.By calculating feed and speeds you theoreticly should turn your spindle approximatley 9,703RPM and feeding at 1. a minute.I would use a chip breaking peck cycle taking no more than .001 at a time.This is a guesstimate answer figured out at 50 surface feet, I am at home and my machinist hand book is at work,so I can not see the actual surface feetI should use when using cobalt or carbide on titanium.And as far as the pecking cycle it depends on how deep you are going to drill, that will determine the pecking cycle to use(retract/chip clear).

 

[MortenDK]

I am not sure about the coated drill.
Although my only practical experience in machining titanium comes from milling, we found that the coated mills, like TCN or TiAl would wear (probaby abrasive wear from being the same metal) down much faster than the non-coated HSS or carbide types. Morten K. Thillemann

 

[Carthius]

As far as drills, we have many different opinions, all of which I feel are good advice. As far as machining 6-4 Ti,
I would make sure you have a good spot first. I would use a spotter, not a center drill, unless you are sure the face you will drill into is true. I prefer to use a Tin coated HSS drill, (that's just me), and calculate your feeds and speeds as per Machinery's Handbook. Pecking cycle is the way to go. Do not well in the material. Heat and cooling while cutting in 6-4 will give nothing but heartache. As it will shift from alpha to beta while you cut, and your feeds and speeds just went out the window. Good luck.

 

I used to drill Mt. Bike axils (skewer holes) from 6/4 Ti.---I used a cobolt parabolic (high helix), split point,135 deg drill.---Now I was drilling a six inch axil through from both ends with this drill about .200" in dia.--If I tried to run about .003"/ rev at specified speeds the drill would chatter and break imediatly.---but if I fed the firs part at .0005" and a slower (about 1/4 specified speed) for a part or two (six or 12 inched of hole),-and increase the feeds and speeds gradually until I got to .003 (listen for chatter--if you hear chatter, you are rushing the drill break in process, and need to back off a bit for a few inched of hole) and specified speeds (usually took about 10 parts)--the drill would hone itself and I would get over 200 parts (that is 1200" of hole) out of one drill.---it took some time to get to speed, but when I was there there were no problems.

 

[vignash]

Vignash(mechanical)

I have worked with Zirconium which is similar to Titanium.
The best tool would be TiN coated HSS. Continuous feed with lot of coolant will give best results.