How to machine Titanium
After reading this article, you will have no fear about machining Titanium. My intention is not to give a lot of technical data about the different Titanium alloys, but to offer practical information on how the material behaves and the reasons for certain cutting strategies. In order to fully understand this article you will need to be familiar with CNC machines, cutting speeds, feeds, tool entry/exit strategies and material holding techniques.
Why is Titanium so different? To answer that question, I will start with how steel and aluminum behave. Let’s assume that you are machining a piece of steel using a ½” 4 flute carbide endmill. Most likely your cutting surface speed will be 150 spm (1150 rpm) and your feed rate will be 0.002” PT (9.17” pm). If you pick up a chip and measure the thickness, it will be approximately 0.002”. Same as the feed rate value. If we change the material to aluminum the result will be the same, but not for Titanium.
Titanium chips are thinner than the feed rate per tooth value (approximately 50% or less of the FPT value). The cutting process for Titanium is a combination of pure cutting and extruding, the thinner chip also means that the speed between the material and the cutting tool (at the point of contact) is double or more; this friction generates heat, and that’s why you should use low surface speed for cutting Titanium (around 60-80spm) and plenty of coolant.
Clamping the stock material is also critical for machining Titanium. You should hold the material as rigid as possible. The reason is that Titanium is as hard as steel but it is twice as flexible. This means that Titanium will generate forces between the material and tool similar to steel but will flex away from the cutting tool. If you need to hold high tolerances on thin parts, it may be a challenge.
I would recommend designing custom fixtures to strongly hold the part. It is a good practice to leave bosses or clamping features after roughing in preparation for the finishing run.
Separate roughing runs and finishing runs. Roughing runs are the most difficult; if you can get them done right the finishing run will be much easier. I recommend using High Feed Cutters for roughing operations they perform well but try to limit shoulder cuts to a minimum. Also important is to rest the material for 1 or 2 days or send it to stress treatment after rough runs.
If you leave 0.010” to 0.020” allowance for the finish run you are safe. Carbide endmills will finish the part with no problems. Be creative using the CNC compensation values for the high precision features.
As for cutting tools, use the best carbide tool you can find. For roughing operations use high feed index cutters; they are expensive but work well. For tapping use thread milling only (carbide only); never ever use taps. For drilling, use carbide also. It is very important to inspect the tools often and never use a tool for more than 15 min without a visual inspection. A broken tool will generate so much heat that the Titanium will get hard and break any new tool you use next.
Summary:
· Plan your work carefully.
· Separate roughing runs and finishing runs.
· Be creative and design fixtures to strongly hold the material.
· Organize your cutting tools and keep a tool usage logbook.
· Buy plenty of cutting tools and inserts.
· Put a lot of attention to the programming.
· Check that your machine has plenty of coolant.
· Program stops to visually inspect the tools and inserts condition.
· Don’t throw away the chips; you can get good money for them.
· Be patient.
By Carlos Hoefken
Dallas Texas May 2009
www.macroleverinc.com
macrolever©2009