Collected Thoughts On High-Speed Machining Of Titanium

Edward F. Rossman, PhD
The Boeing Company

Provided Courtesy of:
The Society Of Manufacturing Engineers

This is a sampling of the Technical Papers available to SME Members. Click above to Join SME Now!

High Speed Machining Techniques

Most progress has been made in finish milling cuts, but good progress is also being made in rough cutting.

Finish Milling

High-speed machining of titanium is all about cutter life, and heat is the enemy. So, once again, I tout the use of sharp cutters to keep heat down.

For many years, we left about 0.100 in. of material for the cleanup cuts, and we were limited to about 120 SFM with carbide or carbide-inserted cutters (60 SFM with cobalt cutters). Cobalt cutters are cutters made from good grades of high-speed steel with 8 to 10% cobalt as an ingredient.

In high-speed milling, we leave only about 0.025 in. of material for the finish milling and use solid carbide cutters that are 1 in. in diameter and smaller. We also use titanium-aluminum-nitride as a coating.

We did much testing a few years back and found that coatings usually gave us about 30% greater cutter life at the old feeds and speeds, but the coated cutters cost about 30% more at the time, so it didn't pay to coat. Also, we didn't have to recoat after resharpening.

Today, I do advocate coating of the solid carbide cutters. At high speeds - 400 to 800 SFM - we get nearly double the cutter life as with uncoated tools. We also need to recoat after each resharpening.

In our progress toward higher speeds, it seems that the reason tool life is good (45 minutes to one hour) is because the teeth of the cutter are only engaged a tiny amount of the time. Most of the time the teeth are out of the metal being washed with coolant.

Leaving less material for cleanup got us up to about 400 SFM. To go higher we did two things:

  1. We went to five-axis milling on the roughing cuts that preceded the finish milling
  2. When cutting with the bottom of the cutter, we tilted the cutter about 1% to 1% degree to lift the heel of the cutter that is doing the bottom cutting.
The five-axis roughing meant we were leaving a very consistent amount of metal for finish cuts. Solid carbide cutters do not like inconsistent surfaces. Tilting the cutter gets the heel of the cutter up where coolant can do its cooling. Without tilt, we generated too much heat-the teeth were always in contact with the metal and we could not machine faster than 400 SFM without sacrificing cutter life.

One more step is usually required; we need to re-run the final milling pass because the cutter is not rigid enough to meet our nominal dimensions. In theory, one could build in compensation for cutter deflection and eliminate the extra pass, but this is a tough process to manage. If the operator pauses the machine for any reason, the cutter will tend to walk into the part beyond nominal dimensions, creating scrap. The process is much safer and easier to manage if we use a spring or wash pass.

I don't know of anyone doing the following yet, but it seems to me we could:

  1. Take our bottom cuts to net during roughing and not have to tilt the cutter for these cuts
  2. Write the finish-milling pass to be about 0.001 in. above the pocket floors and eliminate the need to tilt the cutter.
I don't know if anyone has tried the following yet, but another possibility for saving time would be to write a separate program for the final spring pass and run it up in the 1000 to 1200 SFM range. Because we are only removing a couple of thousandths of material, the cutter should handle this speed, and it doesn't matter if the cutter only lasts about 15 minutes at the higher speed.

Copyright (c) 2004 Society of Manufacturing Engineers. All rights reserved.

Home |  About Us |  Back To Technical Library |  Contact Us
Copyright © 1996-2010 All Rights Reserved.
General or Technical Questions? E-mail