×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Hi speed milling 6Al-4V titanium?

Hi speed milling 6Al-4V titanium?

Hi speed milling 6Al-4V titanium?

(OP)
I have an application to mill 2mm square "windows" thru 1mm thick 6Al-4V titanium. The "windows" require .5mm corner radii, so I plan to use 1mm dia carbide end mills. Quantities are 3,000 parts with 250 "windows" per part. I have CNC spindle speeds available to 30,000 rpm. Does anyone have any suggestions as to how this might be handled? Any thoughts about speeds, feeds, depths of cut, expected tool life etc...

Thanks,
Dave

RE: Hi speed milling 6Al-4V titanium?

There may be some specifics about your project that get in the way, but I think I'd look for some other method, perhaps a punch press.  The milling approach would, in my opinion, be extremely slow and unreliable.

But:

If you must use an end mill, you'll likely have to pre-drill a start hole in each window.  Even if your end mill claims to be center-cutting, I think you'll find it unsatisfactory for that purpose, in terms of tool life.  Drills are MUCH better at making holes from the solid than are end mills.

My data suggests a starting speed for the end mill around 100 SFM, which would translate to 9700 RPM for a 1mm tool.  Feed of not more than .0001 IPT (and possibly much less) - a two-flute end mill would thus feed at 1.94 IPM.

I think you'd be unlikely to finish even one complete part without catastrophic tool failure.

RE: Hi speed milling 6Al-4V titanium?

I would be careful with high speed machining of Ti alloys.  They do have a tendency to catch fire.

RE: Hi speed milling 6Al-4V titanium?

You might try reviewing some of the links that were provided in the following thread:

Thread281-48509

RE: Hi speed milling 6Al-4V titanium?

I'd be talking to the designer about a round hole.....

Can Ti be cut with a water jet?

Keep the wheels on the ground
Bob
showshine@aol.com

RE: Hi speed milling 6Al-4V titanium?

I would be using cobalt instead carbide EM, much more forgiving, have milled ti for years and never seen a carbide end mill being used (except to cut out broken cobalt end mills (using high rpm)).



RE: Hi speed milling 6Al-4V titanium?

(OP)
   I thought I'd share the results of this project, started 18 months ago. I was fortunate enough to have many chances to try various combinations of speeds, feeds, tools and methods. By far the most reliable was to first pilot drill through with a #2 carbide center drill. Tool life was easily 10,000 "windows" at 100 SFM at .0007/rev feed. Then rough mill with 1/16 4fl carbide em at 100 SFM at .0007/rev feed, then finish mill with 1mm 4fl carbide em at 100 SFM and .001/rev feed. Seemed a bit time consuming, but customer required milled surfaces and the reliability was very predictable as well as the cycle time remaining within the quoted restraints. Rough end mills consistently lasted 600 "windows" and finish end mills lasted 1200 "windows. The reliability allowed us to very effectively keep all equipment running virtually non stop for the entire length of the project.
I did find exceeding 100SFM was nearly impossible.

Dave

RE: Hi speed milling 6Al-4V titanium?

ncassist,

Thanks for the update on your project.  Which company's inserts did you use for this?  Coating type?  Coolant?  It would be nice to have all of this together with your speeds, tool life, etc.

RE: Hi speed milling 6Al-4V titanium?

(OP)
Actually nothing special as far as tooling. I found the cheapest generic tools worked as well as good quality in this application. I tried various coatings (Tin, TiAiN, etc) with no improvement.

Dave

RE: Hi speed milling 6Al-4V titanium?

Yeah, I usually use 150 SFM for Ti, if you want better cutter life reduce it to 80 to 70%.

RE: Hi speed milling 6Al-4V titanium?

Are you still making these?

Is EDM an acceptable alternative for these parts?

We used to just machine the electrodes out of graphite and burn a dozen or so screens at a time.
The graphite machines quickly and a whole lot easier than Ti. On our parts the windows .187" x .187" were about .020 apart and grids of 6" x 6" at about 25 degrees.
You might have to do a thinner stack with the smaller windows
Talk to your local EDM job shop. Should be a no-brainer for for them.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources