I had occasion recently to research this, though I have not (yet) had to
put it into practice myself. FWIW, here are the basics I learned -
please accept it for what it is, paper research not years of hands-on
experience, and worth exactly what you paid for it, but maybe a good
indication of areas to research. There are several suppliers and
institutes that will be able to give more specific detail. However,
Ti has a poor thermal conductivity compared with steel, which means that
higher temperatures are created at the cutting interface. It is also
prone to work hardening, which can create a tough skin. To make matters
worse, although the bulk metal is passivated by an impervious layer of
TiO2, the freshly exposed metal is very reactive, and tends to react
with the tool tip.
All this means that slow feeds but fairly heavy cuts, with high coolant
flow, are desirable, the feeds and coolant to lower temperatures, the
deep-ish cut to ensure penetration of the hardened surface layer. Use a
*very* sharp tool as any trace of bluntness will make all these things
If drilling, using a gun drill with coolant supplied down the drill
shaft is recommended. Also, if the bore is large enough, consider
finishing it by reaming and honing to remove surface cracks.
Water jet cutting is a very effective way of producing shapes from
sheet, and some simpler 3-D shapes too.
Bear in mind also that the elastic modulus is about half that of steel,
so you need to guard against workpiece deflection - which of course
conflicts with the above need for deep cuts! Good support is obviously
the answer. However, if your component is likely to be fatigue-critical,
then you should also try to avoid work-hardening the surface, as this is
likely to increase the risk of surface cracks.
6-4 titanium is significantly tougher to machine than CP (commercially
pure) titanium, as many of the above problems are exacerbated.
Again, if the application is likely to be fatigue-critical, look
carefully at the heat treatment of the alloy; most high-tech uses
require multi-stage treatments to get the desirable crystal structure.
Shot peening is also recommended in such cases, as this can give very
substantial improvements in fatigue performance.
Obviously this is not a high volume aerospace need, or you would not be
asking us bunch of reprobates - there are very detailed protocols for
such work, involving continuous monitoring of tool life, such as by
torque monitoring, etc. etc. If you can give us some idea what the
important needs are we may be able to add further thoughts.
Can't help you with that particular grade, but I have tinkered a
little with some offcuts of anonymous grade bar that I picked up which
seemed to cut reasonably freely.
However, I know that this is material that has to be treated with a
certain degree of caution, as it is possible to ignite the chips if
you cut fast/hard enough without coolant; starting a Titanium fire in
your lathe swarf tray won't be a pleasant experience.
No fear! Never let the tool skate or it work hardens the surface and
is a bugger to get going again. Dead sharp HSS tooling at a reasonable
speed and it turns nicely.
If drilling, again, he who hesitates is lost. If the drill squeeks,
yer buggered! Low(ish) speeds, positive feeds, sharp tools. Esp. the
As I'm sure you will know the grade you have chosen is the "dreaded"
aircraft grade that caused a lot of problems when first introduced. In
reality as others have said it is workable with proper care and
attention. We used to machine a lot of this where I worked and in
general for turning and face milling we would use standard Tungsten
Carbide (C-2) and for drilling tapping and end milling we would use
HSS or a High Cobalt Steel. Tools MUST be sharp and the instant they
start to dull they must be replaced; one of the "tricks" the Ti will
play on tools is to turn them from sharp to scrap in a "squeak". Sorry
had to include that as it was a saying that my apprentice instructor
liked to use constantly.
A couple of other points the material has a relatively low modulus of
elasticity and rod will "push away" from the tool much more than steel
so good support is a necessity. I agree with the advice you have been
given relatively slow speed and high feed rates, do not stop the feed
when the tool is in contact with the work as it will instantly render
the tool useless. Plenty of coolant and here your intended use is
important, if you are going to use it in a fatique critical area then
the type of coolant is critical. Soluable oil (at 15-1) works OK but
for critical aerospace components avoid chlorinated oils.
For engine components we would typically use something like, C2 tools,
150 sfpm speed, 0.200" depth of cut and a feed of 0.010" per rev for
roughing. For finishing it would be C2 tool, 200 sfpm speed, and a
depth of cut never less than 0.010" with a feed never less than 0.006"
per rev. With small diameter bar this is obviously not possible but
you get the general gist. Again tool sharpness is the most critical
factor. Dry machining is possible but as Tony says you might not like
the consequences of getting it wrong.
We would always cold work holes etc as machining will produce
microscopic surface cracking of this grade of Ti so if you are
machining anything that your life depends on you will need to research
the specific alloy as heat treatment might well be required.
You may have found this information but if not it gives a good basic
starting point for our type of equipment, advice for the modern CNC
high volume production areas will differ and be specific for a
Keith - thanks for the detailed information - and for the website, which
I had not happened across. Always better to hear from someone who has
actually done it. I will file it for reference, as I also may need to
machine some Ti at some point - not 6-4, but another very tough alloy.
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.