• MMS Youtube
  • MMS Facebook
  • MMS Linkedin
  • MMS Twitter
3/27/2009 | 1 MINUTE READ

What Is The Most Productive End Mill In Titanium?

Facebook Share Icon LinkedIn Share Icon Twitter Share Icon Share by EMail icon Print Icon

Boeing experts recently responded to this question when it was submitted through our Aerospace Machining Zone

Personnel from Boeing's Research & Technology group recently answered readers' questions. One reader asked the following. To see the list of experts taking questions from readers right now, see our Ask An Expert page.


We are machining a 0.423-inch diameter Ti Beta C rod into a 0.375-inch hex. We use a 6-flute carbide end mill at a feed rate of 8.7 ipm and a 0.024-inch depth of cut. No finish pass is needed. We tried an insert cutter that went 3 times as fast, but the interrupted cut tended to tear the material. Can you recommend an end mill we can use for this job that will allow a much faster feed rate than we are now getting?

Response from Boeing’s Research & Technology group

For instances where we are taking very light radial cuts (0.050 inch or less), we use either 1-inch diameter 10-flute tools or 0.75-inch diameter 8-flute solid carbide end mills for finishing titanium parts. The key with these tools is never to touch a corner. We run them at 400 sfm with a 0.003-inch chip load. We go 46 to 48 ipm when cutting with the side of the tool.

If cutting with the bottom of the tool, back off to 300 sfm but maintain the 0.003-inch chip load. When cutting with the bottom of the tool, do not ramp to depth into a part, as there is not enough chip clearance. You should either create a start spot with a different tool, or start off of the part and feed onto it. Limit axial depth of cut to 0.030 inch, but feel free to maximize your step over. Full slots are possible in this situation.

Our primary experience is with titanium 6Al-4V, so your parameters may need to be adjusted for your material. We achieve 90+ minutes of tool life with these parameters as long as our radial engagement is 0.050 inch or less and we never touch a corner. You can buy cutters such as these from Fullerton, Data Flute, Robb Jack and Onsrud, among others. The cutters are a little bit expensive, but they run really fast and in most instances we find that the extra cost is more than worth it, because they are so productive they end up saving a lot of cost in the end.



  • Drill And Bore With A Face Mill

    Cutting holes by interpolating a face milling cutter may be a better process choice for many rough and even finish boring operations. Software improvements and better cutter designs allow expanding use of the versatile face mill for hole making.

  • 10 Tips for Titanium

    Simple process considerations can increase your productivity in milling titanium alloys.

  • Successful Application Of Ceramic Inserts

    Applying ceramic inserts is not a simple substitution of one cutting tool material for another. There are significant process considerations that shops should examine carefully in order to realize performance and tool life expectations from ceramic inserts. Here's a look at some of the ways they are used.